Docstoc

wb sim

Document Sample
wb sim Powered By Docstoc
					              Mechanical (formerly Simulation)




ANSYS, Inc.                           Release 12.0
Southpointe                           April 2009
275 Technology Drive                  ANSYS, Inc. is
Canonsburg, PA 15317                  certified to ISO
ansysinfo@ansys.com                   9001:2008.
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
Copyright and Trademark Information
© 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.

ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any and
all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks
of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names
or trademarks are the property of their respective owners.

Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL
AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and document-
ation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains pro-
visions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties,
disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may
be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. is certified to ISO 9001:2008.

U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use, du-
plication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software
license agreement and FAR 12.212 (for non-DOD licenses).

Third-Party Software
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software and
third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.

Published in the U.S.A.
Table of Contents
The Mechanical Application Approach ...................................................................................................... 1
   Overall Steps to Using the Mechanical Application .................................................................................. 1
      Create Analysis System ..................................................................................................................... 1
      Define Engineering Data ................................................................................................................... 2
      Attach Geometry .............................................................................................................................. 2
      Define Part Behavior ......................................................................................................................... 4
      Define Connections .......................................................................................................................... 7
      Apply Mesh Controls and Preview Mesh ............................................................................................ 8
      Establish Analysis Settings ................................................................................................................ 8
      Define Initial Conditions ................................................................................................................. 13
      Apply Loads and Supports .............................................................................................................. 14
      Solve .............................................................................................................................................. 15
      Review Results ................................................................................................................................ 16
      Create Report (optional) ................................................................................................................. 17
   Analysis Types ...................................................................................................................................... 17
      Electric Analysis .............................................................................................................................. 17
      Explicit Dynamics Analysis .............................................................................................................. 20
      Harmonic Response Analysis ........................................................................................................... 31
      Linear Buckling Analysis .................................................................................................................. 39
      Magnetostatic Analysis ................................................................................................................... 44
      Modal Analysis ............................................................................................................................... 48
      Random Vibration Analysis ............................................................................................................. 52
      Response Spectrum Analysis ........................................................................................................... 56
      Shape Optimization Analysis ........................................................................................................... 60
      Static Structural Analysis ................................................................................................................. 64
      Steady-State Thermal Analysis ......................................................................................................... 69
      Thermal-Electric Analysis ................................................................................................................ 72
      Transient Structural Analyses .......................................................................................................... 76
           Transient Structural (ANSYS) Analysis ........................................................................................ 76
           Transient Structural (MBD) Analysis ........................................................................................... 84
      Transient Thermal Analysis .............................................................................................................. 91
   Special Analysis Topics .......................................................................................................................... 95
      2-D Analyses ................................................................................................................................... 95
      Using Generalized Plane Strain ........................................................................................................ 97
      Using Symmetry ............................................................................................................................. 98
           Introduction ............................................................................................................................. 98
           Types of Symmetry ................................................................................................................... 99
               Structural Symmetry ........................................................................................................... 99
               Structural Anti-Symmetry ................................................................................................... 99
               Electromagnetic Symmetry ............................................................................................... 100
               Electromagnetic Anti-Symmetry ....................................................................................... 100
               Electromagnetic Periodicity .............................................................................................. 101
               Electromagnetic Anti-Periodicity ....................................................................................... 101
           Working With Symmetry Defined in DesignModeler ................................................................ 101
           Defining Symmetry in the Mechanical Application .................................................................. 102
           Periodicity Example ................................................................................................................ 104
           Symmetry in Explicit Dynamics ............................................................................................... 106
               General Symmetry ............................................................................................................ 106
               Global Symmetry Planes ................................................................................................... 106
      Static Analysis From Transient Structural (MBD) Analysis ................................................................ 107

                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                            iii
Mechanical (formerly Simulation)

       Fluid-Structure Interaction (FSI) ..................................................................................................... 108
           Fluid-Structure Interaction (FSI) - One Way Transfer .................................................................. 108
                Face Forces at Fluid-Structure Interface ............................................................................. 109
                Face Temperatures and Convections at Fluid-Structure Interface ........................................ 109
                CFD Results Mapping ........................................................................................................ 110
           Fluid-Structure Interaction (FSI) - Two Way Transfer .................................................................. 110
   Wizards .............................................................................................................................................. 111
       The Mechanical Wizard ................................................................................................................. 112
The Mechanical Application Basics ......................................................................................................... 115
   The Mechanical Application Interface .................................................................................................. 115
       The Mechanical Application Window ............................................................................................. 115
       Tree Outline Conventions .............................................................................................................. 117
       Tree Outline .................................................................................................................................. 118
       Environment Filtering ................................................................................................................... 118
       Interface Behavior Based on License Levels .................................................................................... 119
       Suppress and Unsuppress Items .................................................................................................... 119
       Tabs ............................................................................................................................................. 120
       Geometry ..................................................................................................................................... 120
       Legend Functionality .................................................................................................................... 120
           Discrete Legends in the Mechanical Application ...................................................................... 120
       Graphical Selection ....................................................................................................................... 121
       Named Selections ......................................................................................................................... 129
           Creating Named Selections ..................................................................................................... 129
           Managing Named Selections .................................................................................................. 130
           Scoping to Named Selections .................................................................................................. 131
           Inspecting Large Meshes Using Named Selections ................................................................... 132
           Importing Named Selections ................................................................................................... 134
           Converting Named Selection Groups to Mechanical APDL Application Components ................ 134
       Details View .................................................................................................................................. 134
       Worksheet Tab .............................................................................................................................. 140
       Graph and Tabular Data Windows ................................................................................................. 142
       Parameters ................................................................................................................................... 144
       Toolbars ....................................................................................................................................... 144
           Main Menu ............................................................................................................................. 144
           Standard Toolbar .................................................................................................................... 147
           Graphics Toolbar ..................................................................................................................... 148
           Context Toolbar ...................................................................................................................... 151
           Unit Conversion Toolbar .......................................................................................................... 161
           Named Selection Toolbar ........................................................................................................ 161
       Messages Window ........................................................................................................................ 161
       Workbench Windows Manager ..................................................................................................... 162
           Restore Original Window Layout ............................................................................................. 163
           Window Manager Features ..................................................................................................... 163
       Print Preview ................................................................................................................................ 163
       Triad and Rotation Cursors ............................................................................................................ 163
   Customizing the Mechanical Application ............................................................................................. 164
       The Mechanical Application Options ............................................................................................. 164
       Variables ....................................................................................................................................... 171
       Macros ......................................................................................................................................... 172
Using the Mechanical Application Features ........................................................................................... 173
   Geometry in the Mechanical Application ............................................................................................. 173
       Assemblies, Parts, and Bodies ........................................................................................................ 173


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
iv                                                         of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Mechanical (formerly Simulation)

   Solid Bodies .................................................................................................................................. 176
   Surface Bodies .............................................................................................................................. 176
   Rigid Bodies ................................................................................................................................. 177
   Path ............................................................................................................................................. 178
   Remote Point ................................................................................................................................ 180
        Remote Point Overview .......................................................................................................... 180
        Connection Lines .................................................................................................................... 182
        Promote Remote Point ............................................................................................................ 183
        Remote Point Commands Objects ........................................................................................... 183
   Point Mass .................................................................................................................................... 183
   Contact ........................................................................................................................................ 184
   Spot Welds ................................................................................................................................... 184
   Joints ........................................................................................................................................... 185
        Joint Characteristics ................................................................................................................ 185
        Types of Joints ........................................................................................................................ 187
        Joint Properties and Application ............................................................................................. 193
        Example: Assembling Joints .................................................................................................... 199
        Example: Configuring Joints .................................................................................................... 210
        Automatic Joint Creation ........................................................................................................ 215
        Joint Stops and Locks .............................................................................................................. 216
        Ease of Use Features ............................................................................................................... 218
        Detecting Overconstrained Conditions .................................................................................... 220
   Springs ......................................................................................................................................... 221
   Beam ............................................................................................................................................ 224
   Virtual Topology ........................................................................................................................... 225
Coordinate Systems Overview ............................................................................................................. 225
   Creating Coordinate Systems ........................................................................................................ 225
        Initial Creation and Definition ................................................................................................. 225
        Establishing Origin for Associative and Non-Associative Coordinate Systems ............................ 226
        Setting Principal Axis and Orientation ..................................................................................... 227
        Using Transformations ............................................................................................................ 227
   Importing Coordinate Systems ...................................................................................................... 228
   Applying Coordinate Systems as Reference Locations .................................................................... 228
   Using Coordinate Systems to Specify Joint Locations ..................................................................... 229
   Transferring Coordinate Systems to the Mechanical APDL Application ........................................... 229
Graphics ............................................................................................................................................. 229
   Annotations ................................................................................................................................. 229
   Lighting Controls .......................................................................................................................... 234
   New Section Plane ........................................................................................................................ 234
   Comments, Images, Figures ........................................................................................................... 237
Analysis Settings ................................................................................................................................. 238
   Analysis Settings for Most Analysis Types ....................................................................................... 238
   Analysis Settings for Explicit Dynamics Analyses ............................................................................ 247
   Steps and Step Controls for Static and Transient Analyses .............................................................. 262
        Role of Time in Tracking .......................................................................................................... 262
        Steps, Substeps, and Equilibrium Iterations .............................................................................. 263
        Automatic Time Stepping ....................................................................................................... 264
        Guidelines for Integration Step Size ......................................................................................... 264
        Step Controls .......................................................................................................................... 266
   Nonlinear Controls ........................................................................................................................ 269
   Output Controls ............................................................................................................................ 270
   Solver Controls ............................................................................................................................. 271


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                               v
Mechanical (formerly Simulation)

        Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Ana-
        lyses ............................................................................................................................................. 273
        Damping Controls ........................................................................................................................ 276
        Visibility ....................................................................................................................................... 277
        Analysis Data Management ........................................................................................................... 277
     Applying Loads ................................................................................................................................... 278
        Types of Loads and Conditions ...................................................................................................... 279
            Acceleration ........................................................................................................................... 280
            Standard Earth Gravity ............................................................................................................ 282
            Rotational Velocity .................................................................................................................. 283
            Pressure ................................................................................................................................. 284
            Hydrostatic Pressure ............................................................................................................... 285
            Force ...................................................................................................................................... 285
            Remote Force ......................................................................................................................... 287
            Bearing Load .......................................................................................................................... 288
            Bolt Pretension ....................................................................................................................... 290
            Moment ................................................................................................................................. 291
            Generalized Plane Strain ......................................................................................................... 292
            Line Pressure .......................................................................................................................... 293
            PSD Base Excitation ................................................................................................................ 293
            RS Base Excitation ................................................................................................................... 294
            Joint Load ............................................................................................................................... 295
            Imported Body Temperature ................................................................................................... 297
            Thermal Condition .................................................................................................................. 297
            Temperature ........................................................................................................................... 298
            Convection ............................................................................................................................. 298
            Radiation ................................................................................................................................ 300
            Heat Flow ............................................................................................................................... 300
            Perfectly Insulated .................................................................................................................. 302
            Heat Flux ................................................................................................................................ 302
            Internal Heat Generation ......................................................................................................... 303
            Imported Heat Generation ...................................................................................................... 303
            Voltage ................................................................................................................................... 303
            Current ................................................................................................................................... 304
            Electromagnetic Boundary Conditions and Excitations ............................................................ 305
                  Magnetic Flux Boundary Conditions .................................................................................. 305
                  Conductor ........................................................................................................................ 307
                        Solid Source Conductor Body ...................................................................................... 307
                        Voltage Excitation for Solid Source Conductors ............................................................ 309
                        Current Excitation for Solid Source Conductors ............................................................ 310
                        Stranded Source Conductor Body ............................................................................... 311
                        Current Excitation for Stranded Source Conductors ..................................................... 312
            CFD Imported Pressure ........................................................................................................... 314
            CFD Imported Temperature ..................................................................................................... 314
            CFD Imported Convection ....................................................................................................... 314
            Motion Load ........................................................................................................................... 315
            Fluid Solid Interface ................................................................................................................ 317
        How to Apply Loads ...................................................................................................................... 317
        Remote Boundary Conditions ....................................................................................................... 319
        Harmonic Loads ............................................................................................................................ 321
        Spatial Varying Loads and Displacements ...................................................................................... 322
        Tabular and Function Loads .......................................................................................................... 324


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
vi                                                         of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  Mechanical (formerly Simulation)

   Imported Loads ............................................................................................................................ 325
   Resolving Thermal Boundary Condition Conflicts ........................................................................... 326
   Direction ...................................................................................................................................... 326
   Scope ........................................................................................................................................... 328
   Types of Supports ......................................................................................................................... 328
        Fixed Face ............................................................................................................................... 329
        Fixed Edge .............................................................................................................................. 329
        Fixed Vertex ............................................................................................................................ 330
        Displacement for Faces ........................................................................................................... 330
        Displacement for Edges .......................................................................................................... 331
        Displacement for Vertices ........................................................................................................ 332
        Remote Displacement ............................................................................................................. 333
        Velocity .................................................................................................................................. 334
        Frictionless Face ...................................................................................................................... 334
        Compression Only Support ..................................................................................................... 335
        Cylindrical Support ................................................................................................................. 336
        Simply Supported Edge .......................................................................................................... 336
        Simply Supported Vertex ........................................................................................................ 336
        Fixed Rotation ........................................................................................................................ 337
        Elastic Support ....................................................................................................................... 338
        Coupling ................................................................................................................................ 338
        Impedance Boundary ............................................................................................................. 339
Results in the Mechanical Application ................................................................................................. 340
   Structural Results .......................................................................................................................... 340
        Deformation ........................................................................................................................... 341
        Stress and Strain ..................................................................................................................... 342
             Equivalent (von Mises) ...................................................................................................... 343
             Maximum, Middle, and Minimum Principal ........................................................................ 344
             Maximum Shear ............................................................................................................... 344
             Intensity ........................................................................................................................... 345
             Strain Energy .................................................................................................................... 346
             Vector Principals ............................................................................................................... 346
             Error (Structural) ............................................................................................................... 346
             Thermal Strain .................................................................................................................. 347
             Equivalent Plastic Strain .................................................................................................... 348
        Calculating Linearized Stresses ................................................................................................ 349
        Contact Results ....................................................................................................................... 349
        Reactions ............................................................................................................................... 352
        Energy .................................................................................................................................... 353
        Frequency .............................................................................................................................. 354
        Stress Tools ............................................................................................................................. 354
             Maximum Equivalent Stress Safety Tool ............................................................................ 354
             Maximum Shear Stress Safety Tool .................................................................................... 356
             Mohr-Coulomb Stress Safety Tool ...................................................................................... 357
             Maximum Tensile Stress Safety Tool ................................................................................... 359
        Fatigue (Fatigue Tool) .............................................................................................................. 361
        Contact Tool ........................................................................................................................... 361
             Contact Tool Initial Information ......................................................................................... 365
        Beam Tool ............................................................................................................................... 365
        Structural Probes .................................................................................................................... 366
             Joint Probes ...................................................................................................................... 370
             Spring Probes ................................................................................................................... 372


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                            vii
Mechanical (formerly Simulation)

                Beam Probes .................................................................................................................... 372
       Thermal Results ............................................................................................................................ 372
           Temperature ........................................................................................................................... 372
           Heat Flux ................................................................................................................................ 373
           Heat Reaction ......................................................................................................................... 373
           Error (Thermal) ....................................................................................................................... 374
           Thermal Probes ....................................................................................................................... 374
       Magnetostatic Results ................................................................................................................... 374
           Electric Potential ..................................................................................................................... 375
           Total Magnetic Flux Density .................................................................................................... 375
           Directional Magnetic Flux Density ........................................................................................... 375
           Total Magnetic Field Intensity .................................................................................................. 375
           Directional Magnetic Field Intensity ........................................................................................ 375
           Total Force .............................................................................................................................. 375
           Directional Force .................................................................................................................... 375
           Current Density ...................................................................................................................... 376
           Inductance ............................................................................................................................. 376
           Flux Linkage ........................................................................................................................... 376
           Error (Magnetic) ...................................................................................................................... 377
           Magnetostatic Probes ............................................................................................................. 377
       Electric Results .............................................................................................................................. 379
           Electric Probes ........................................................................................................................ 379
       Results Related Topics ................................................................................................................... 380
           Adaptive Convergence ............................................................................................................ 381
           Animation .............................................................................................................................. 381
           Averaged vs. Unaveraged Contour Results ............................................................................... 383
           Capped Isosurfaces ................................................................................................................. 383
           Chart and Table ...................................................................................................................... 383
           Cleaning Results Data ............................................................................................................. 386
           Composite Result Over Time ................................................................................................... 386
           Contour Results ...................................................................................................................... 386
           Dynamic Legend .................................................................................................................... 386
           Eroded Nodes in Explicit Dynamics Analyses ........................................................................... 388
           Exporting Data ....................................................................................................................... 389
           Generating Reports ................................................................................................................ 390
           Results Legend ....................................................................................................................... 390
                Named Legends ............................................................................................................... 391
                Date and Time .................................................................................................................. 392
                Max, Min on Color Bar ....................................................................................................... 392
                Logarithmic Scale ............................................................................................................. 392
                All Scientific Notation ....................................................................................................... 392
                Digits ............................................................................................................................... 392
                Independent Bands .......................................................................................................... 392
                Color Scheme ................................................................................................................... 392
           Path Results ............................................................................................................................ 392
           Probes .................................................................................................................................... 393
                Overview and Probe Types ................................................................................................ 394
                Probe Details View ........................................................................................................... 395
           Renaming Results Based on Definition .................................................................................... 397
           Result Limitations ................................................................................................................... 397
           Results Averaging ................................................................................................................... 397
           Results Based on Geometry ..................................................................................................... 398


                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
viii                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Mechanical (formerly Simulation)

         Results Toolbar ....................................................................................................................... 400
         Scoping Results ...................................................................................................................... 400
         Solution Combinations ........................................................................................................... 400
         Solution Coordinate System .................................................................................................... 402
         Unconverged Results .............................................................................................................. 404
         User Defined Results ............................................................................................................... 404
             Overview .......................................................................................................................... 404
             Characteristics .................................................................................................................. 405
             Application ....................................................................................................................... 405
             User Defined Result Expressions ........................................................................................ 407
             User Defined Result Identifier ............................................................................................ 410
             Unit Description ............................................................................................................... 411
             User Defined Results for Explicit Dynamics Analyses .......................................................... 412
         Vector Plots ............................................................................................................................ 415
Solving Overview ................................................................................................................................ 415
    Solve Process Capabilities ............................................................................................................. 416
    Solving Workflow .......................................................................................................................... 416
    Using Solve Process Settings ......................................................................................................... 416
    The Solving Process ...................................................................................................................... 419
    Solving Scenarios .......................................................................................................................... 421
    Solution Information ..................................................................................................................... 424
    Postprocessing During Solve ......................................................................................................... 426
    Result Tracker Objects ................................................................................................................... 426
    Adaptive Convergence .................................................................................................................. 432
    File Management in the Mechanical Application ............................................................................ 435
    Solving Units ................................................................................................................................ 436
    Saving your Results in the Mechanical Application ......................................................................... 486
    Writing and Reading the Mechanical APDL Application Files .......................................................... 486
    Converting Boundary Conditions to Nodal DOF Constraints (ANSYS Solver) ................................... 488
    Resume Capability for Explicit Dynamics (ANSYS) Analyses ............................................................ 488
Commands Objects ............................................................................................................................ 489
Report Preview ................................................................................................................................... 494
    Tables ........................................................................................................................................... 494
    Figures and Images ....................................................................................................................... 494
    Publishing .................................................................................................................................... 495
    Sending ........................................................................................................................................ 495
    Comparing Databases ................................................................................................................... 495
Customize Report Content .................................................................................................................. 495
Meshing in the Mechanical Application ............................................................................................... 496
Parameters ......................................................................................................................................... 496
    Specifying Parameters .................................................................................................................. 497
    CAD Parameters ............................................................................................................................ 498
Fatigue Overview ................................................................................................................................ 499
    Fatigue Material Properties ........................................................................................................... 500
    Fatigue Analysis and Loading Options ........................................................................................... 501
    Reviewing Fatigue Results ............................................................................................................. 504
Contact .............................................................................................................................................. 507
    Global Contact Settings ................................................................................................................ 508
    Contact Region Settings ............................................................................................................... 510
         Scope Settings ........................................................................................................................ 510
         Definition Settings .................................................................................................................. 511
         Advanced Settings .................................................................................................................. 512


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                              ix
Mechanical (formerly Simulation)

       Supported Contact Types and Formulations .................................................................................. 517
       Setting Contact Conditions Manually ............................................................................................ 518
       Contact Ease of Use Features ......................................................................................................... 518
             Controlling Transparency for Contact Regions ......................................................................... 519
             Hiding Bodies Not Scoped to a Contact Region ........................................................................ 519
             Renaming Contact Regions Based on Geometry Names ........................................................... 519
             Identifying Contact Regions for a Body .................................................................................... 520
             Flipping Contact and Target Scope Settings ............................................................................. 520
             Merging Contact Regions That Share Geometry ....................................................................... 521
             Saving or Loading Contact Region Settings ............................................................................. 521
             Resetting Contact Regions to Default Settings ......................................................................... 522
             Locating Bodies Without Contact ............................................................................................ 522
   Body Interactions in Explicit Dynamics Analyses .................................................................................. 523
       Properties for Body Interactions Folder .......................................................................................... 524
             Contact Detection .................................................................................................................. 524
             Formulation ............................................................................................................................ 526
             Shell Thickness Factor ............................................................................................................. 527
             Body Self Contact ................................................................................................................... 527
             Element Self Contact ............................................................................................................... 527
             Tolerance ................................................................................................................................ 528
             Pinball Factor .......................................................................................................................... 528
             Time Step Safety Factor ........................................................................................................... 528
             Limiting Time Step Velocity ..................................................................................................... 528
             Edge on Edge Contact ............................................................................................................ 528
       Interaction Type Properties for Body Interaction Object ................................................................. 529
             Frictionless Type ..................................................................................................................... 529
             Frictional Type ........................................................................................................................ 529
             Bonded Type .......................................................................................................................... 530
             Reinforcement Type ................................................................................................................ 532
   Virtual Topology in the Mechanical Application ................................................................................... 532
Mechanical Objects Reference ................................................................................................................ 533
   Alert ................................................................................................................................................... 535
   Analysis Settings ................................................................................................................................. 535
   Angular Velocity ................................................................................................................................. 536
   Beam .................................................................................................................................................. 537
   Body .................................................................................................................................................. 539
   Body Interactions ................................................................................................................................ 541
   Body Interaction ................................................................................................................................. 542
   Chart .................................................................................................................................................. 543
   Commands ......................................................................................................................................... 544
   Comment ........................................................................................................................................... 546
   Connections ....................................................................................................................................... 546
   Construction Geometry ...................................................................................................................... 548
   Contact Region ................................................................................................................................... 549
       Object Properties - Most Structural Analyses ................................................................................. 550
       Object Properties - Explicit Dynamics Analyses .............................................................................. 550
       Object Properties - Thermal and Electromagnetic Analyses ............................................................ 551
   Contact Tool (Group) ........................................................................................................................... 551
   Convergence ...................................................................................................................................... 553
   Coordinate System ............................................................................................................................. 554
   Coordinate Systems ............................................................................................................................ 554
   Environment (Group) .......................................................................................................................... 555


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
x                                                          of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Mechanical (formerly Simulation)

   Fatigue Tool (Group) ........................................................................................................................... 556
   Figure ................................................................................................................................................. 559
   Geometry ........................................................................................................................................... 560
   Global Coordinate System ................................................................................................................... 563
   Image ................................................................................................................................................. 564
   Imported Load (Group) ....................................................................................................................... 564
   Initial Conditions ................................................................................................................................ 565
   Initial Temperature .............................................................................................................................. 566
   Joint ................................................................................................................................................... 566
   Loads and Supports (Group) ............................................................................................................... 567
   Mesh .................................................................................................................................................. 568
   Mesh Control Tools (Group) ................................................................................................................. 571
   Modal ................................................................................................................................................. 572
   Model ................................................................................................................................................. 573
   Named Selections ............................................................................................................................... 574
   Part .................................................................................................................................................... 576
   Path ................................................................................................................................................... 577
   Periodic Region .................................................................................................................................. 578
   Point Mass .......................................................................................................................................... 579
   Pre Stress ............................................................................................................................................ 581
   Probe ................................................................................................................................................. 581
   Project ................................................................................................................................................ 582
   Remote Point ...................................................................................................................................... 583
   Remote Points .................................................................................................................................... 584
   Result Tracker ..................................................................................................................................... 585
   Results and Result Tools (Group) .......................................................................................................... 587
   Solution ............................................................................................................................................. 589
   Solution Combination ......................................................................................................................... 590
   Solution Information ........................................................................................................................... 590
   Spot Weld ........................................................................................................................................... 591
   Spring ................................................................................................................................................ 593
   Stress Tool (Group) .............................................................................................................................. 594
   Symmetry ........................................................................................................................................... 596
   Symmetry Region ............................................................................................................................... 597
   Velocity .............................................................................................................................................. 598
   Virtual Cell .......................................................................................................................................... 599
   Virtual Topology ................................................................................................................................. 600
CAD Systems ........................................................................................................................................... 603
   Geometry Interface Support for Windows ........................................................................................... 603
   Geometry Preferences ........................................................................................................................ 604
   General Information ............................................................................................................................ 612
   CAD System Support .......................................................................................................................... 612
        ACIS ............................................................................................................................................. 613
        Autodesk Inventor ........................................................................................................................ 613
        Autodesk Mechanical Desktop ...................................................................................................... 614
        CATIA V4 ....................................................................................................................................... 615
        CATIA V5 (standard) ...................................................................................................................... 615
        CATIA V5 (optional) (CADNexus/CAPRI Gateway) ........................................................................... 616
        DesignModeler ............................................................................................................................. 617
        IGES ............................................................................................................................................. 618
        CoCreate Modeling ....................................................................................................................... 619
        Parasolid ...................................................................................................................................... 619


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                               xi
Mechanical (formerly Simulation)

         Pro/ENGINEER ............................................................................................................................... 620
         Solid Edge .................................................................................................................................... 622
         SolidWorks ................................................................................................................................... 623
         STEP ............................................................................................................................................. 624
         NX ................................................................................................................................................ 625
Troubleshooting ..................................................................................................................................... 629
    Problem Situations ............................................................................................................................. 629
         A Load Transfer Error Has Occurred. ............................................................................................... 630
         Although the Solution Failed to Solve Completely at all Time Points. .............................................. 630
         An Error Occurred Inside the SOLVER Module: Invalid Material Properties ....................................... 630
         An Error Occurred While Solving Due To Insufficient Disk Space ..................................................... 631
         An Error Occurred While Starting the ANSYS Solver Module ........................................................... 631
         An Internal Solution Magnitude Limit Was Exceeded. ..................................................................... 632
         An Iterative Solver Was Used for this Analysis ................................................................................. 632
         At Least One Body Has Been Found to Have Only 1 Element ........................................................... 632
         Animation Does not Export Correctly ............................................................................................ 633
         Assemblies Missing Parts .............................................................................................................. 633
         CATIA V5 and IGES Surface Bodies ................................................................................................. 633
         Error Inertia tensor is too large ...................................................................................................... 633
         Illogical Reaction Results ............................................................................................................... 634
         Large Deformation Effects are Active ............................................................................................. 634
         One or More Contact Regions May Not Be In Initial Contact ........................................................... 634
         One or more MPC contact regions or remote boundary conditions may have conflicts ................... 635
         One or More Parts May Be Underconstrained ................................................................................. 635
         One or More Remote Boundary Conditions is Scoped to a Large Number of Elements .................... 636
         Problems Unique to Background (Asynchronous) Solutions ........................................................... 636
         Problems Using Solution ............................................................................................................... 637
         Running Norton AntiVirusTM Causes the Mechanical Application to Crash ...................................... 638
         The Correctly Licensed Product Will Not Run ................................................................................. 638
         The Deformation is Large Compared to the Model Bounding Box .................................................. 639
         The Initial Time Increment May Be Too Large for This Problem ........................................................ 639
         The Joint Probe cannot Evaluate Results ........................................................................................ 639
         The License Manager Server Is Down ............................................................................................. 640
         The Solution Combination Folder .................................................................................................. 640
         The Solver Engine was Unable to Converge ................................................................................... 640
         The Solver Has Found Conflicting DOF Constraints ........................................................................ 641
         Unable to Find Requested Modes .................................................................................................. 641
         You Must Specify Joint Conditions to all Three Rotational DOFs ...................................................... 642
    CAD Related Troubleshooting ............................................................................................................. 642
    Recommendations ............................................................................................................................. 645
I. Appendices ........................................................................................................................................... 647
    A. Glossary of General Terms ................................................................................................................ 649
    B. LS-DYNA Keywords Used in an Explicit Dynamics Analysis ................................................................ 651
         Supported LS-DYNA Keywords ...................................................................................................... 651
         LS-DYNA General Descriptions ...................................................................................................... 676
    C. Workbench Mechanical Wizard Advanced Programming Topics ........................................................ 679
         Overview ...................................................................................................................................... 679
         URI Address and Path Considerations ............................................................................................ 680
         Using Strings and Languages ........................................................................................................ 681
         Guidelines for Editing XML Files .................................................................................................... 682
         About the TaskML Merge Process .................................................................................................. 682
         Using the Integrated Wizard Development Kit (WDK) ..................................................................... 683


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
xii                                                        of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                             Mechanical (formerly Simulation)

Using IFRAME Elements ................................................................................................................ 683
TaskML Reference ......................................................................................................................... 684
    Overview Map of TaskML ........................................................................................................ 684
    Document Element ................................................................................................................. 685
        simulation-wizard ............................................................................................................. 685
    External References ................................................................................................................ 685
        Merge .............................................................................................................................. 685
        Script ............................................................................................................................... 686
    Object Grouping ..................................................................................................................... 686
        object-group .................................................................................................................... 686
        object-groups ................................................................................................................... 687
        object-type ....................................................................................................................... 687
    Status Definitions ................................................................................................................... 688
        status ............................................................................................................................... 688
        statuses ............................................................................................................................ 688
    Language and Text ................................................................................................................. 689
        data .................................................................................................................................. 689
        language .......................................................................................................................... 689
        string ............................................................................................................................... 690
        strings .............................................................................................................................. 690
    Tasks and Events ..................................................................................................................... 690
        activate-event ................................................................................................................... 690
        task .................................................................................................................................. 691
        tasks ................................................................................................................................. 692
        update-event .................................................................................................................... 692
    Wizard Content ....................................................................................................................... 692
        body ................................................................................................................................ 692
        group ............................................................................................................................... 693
        iframe ............................................................................................................................... 694
        taskref .............................................................................................................................. 694
    Rules ...................................................................................................................................... 695
        Statements ....................................................................................................................... 695
             and ............................................................................................................................ 695
             debug ........................................................................................................................ 695
             if then else stop .......................................................................................................... 695
             not ............................................................................................................................. 696
             or ............................................................................................................................... 697
             update ....................................................................................................................... 697
        Conditions ........................................................................................................................ 697
             assembly-geometry .................................................................................................... 697
             changeable-length-unit ............................................................................................. 698
             geometry-includes-sheets .......................................................................................... 698
             level ........................................................................................................................... 698
             object ......................................................................................................................... 699
             zero-thickness-sheet ................................................................................................... 700
             valid-emag-geometry ................................................................................................. 700
             enclosure-exists .......................................................................................................... 700
        Actions ............................................................................................................................. 700
             click-button ................................................................................................................ 701
             display-details-callout ................................................................................................. 701
             display-help-topic ....................................................................................................... 702
             display-outline-callout ................................................................................................ 702


                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                            xiii
Mechanical (formerly Simulation)

                         display-status-callout .................................................................................................. 703
                         display-tab-callout ...................................................................................................... 703
                         display-task-callout ..................................................................................................... 704
                         display-toolbar-callout ................................................................................................ 704
                         open-url ..................................................................................................................... 705
                         select-all-objects ........................................................................................................ 705
                         select-field .................................................................................................................. 706
                         select-first-object ........................................................................................................ 707
                         select-first-parameter-field .......................................................................................... 708
                         select-first-undefined-field .......................................................................................... 708
                         select-zero-thickness-sheets ....................................................................................... 709
                         select-enclosures ........................................................................................................ 709
                         send-mail ................................................................................................................... 709
                         set-caption ................................................................................................................. 710
                         set-icon ...................................................................................................................... 710
                         set-status .................................................................................................................... 711
              Scripting ................................................................................................................................. 711
                   eval .................................................................................................................................. 711
          Standard Object Groups Reference ................................................................................................ 713
          Tutorials ....................................................................................................................................... 715
              Tutorial: Adding a Link ............................................................................................................ 716
              Tutorial: Creating a Custom Task .............................................................................................. 717
              Tutorial: Creating a Custom Wizard .......................................................................................... 718
              Tutorial: Adding a Web Search IFRAME ..................................................................................... 719
              Completed TaskML Files .......................................................................................................... 721
                   Links.xml .......................................................................................................................... 721
                   Insert100psi.xml ............................................................................................................... 721
                   CustomWizard.xml ............................................................................................................ 722
                   Search.htm ....................................................................................................................... 723
                   CustomWizardSearch.xml ................................................................................................. 724
          Wizard Development Kit (WDK) Groups ......................................................................................... 725
              WDK: Tools Group ................................................................................................................... 725
              WDK: Commands Group .......................................................................................................... 726
              WDK Tests: Actions .................................................................................................................. 727
              WDK Tests: Flags (Conditions) .................................................................................................. 727
      D. Material Models Used in Explicit Dynamics Analysis ......................................................................... 729
          Introduction ................................................................................................................................. 729
          Explicit Material Library ................................................................................................................. 731
          Density ......................................................................................................................................... 737
          Linear Elastic ................................................................................................................................ 737
              Isotropic Elasticity ................................................................................................................... 737
              Orthotropic Elasticity .............................................................................................................. 737
              Viscoelastic ............................................................................................................................. 738
          Test Data ...................................................................................................................................... 739
          Hyperelasticity .............................................................................................................................. 739
          Plasticity ....................................................................................................................................... 744
              Bilinear Isotropic Hardening .................................................................................................... 745
              Multilinear Isotropic Hardening ............................................................................................... 745
              Bilinear Kinematic Hardening .................................................................................................. 746
              Multilinear Kinematic Hardening ............................................................................................. 746
              Johnson-Cook Strength .......................................................................................................... 746
              Cowper-Symonds Strength ..................................................................................................... 748


                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
xiv                                                         of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                         Mechanical (formerly Simulation)

               Steinberg-Guinan Strength ..................................................................................................... 749
               Zerilli-Armstrong Strength ...................................................................................................... 750
         Brittle/Granular ............................................................................................................................. 752
               Drucker-Prager Strength Linear ............................................................................................... 752
               Drucker-Prager Strength Stassi ................................................................................................ 753
               Drucker-Prager Strength Piecewise ......................................................................................... 754
               Johnson-Holmquist Strength Continuous ................................................................................ 755
               Johnson-Holmquist Strength Segmented ................................................................................ 757
               RHT Concrete Strength ........................................................................................................... 759
               MO Granular ........................................................................................................................... 765
         Equations of State ......................................................................................................................... 766
               Background ............................................................................................................................ 766
               Bulk Modulus .......................................................................................................................... 767
               Shear Modulus ....................................................................................................................... 767
               Polynomial EOS ...................................................................................................................... 767
               Shock EOS Linear .................................................................................................................... 769
               Shock EOS Bilinear .................................................................................................................. 770
         Porosity ........................................................................................................................................ 772
               Porosity-Crushable Foam ........................................................................................................ 772
               Compaction EOS Linear .......................................................................................................... 774
               Compaction EOS Non-Linear ................................................................................................... 775
               P-alpha EOS ............................................................................................................................ 777
         Failure .......................................................................................................................................... 780
               Plastic Strain Failure ................................................................................................................ 781
               Principal Stress Failure ............................................................................................................ 781
               Principal Strain Failure ............................................................................................................. 782
               Stochastic Failure .................................................................................................................... 783
               Tensile Pressure Failure ........................................................................................................... 785
               Crack Softening Failure ........................................................................................................... 785
               Johnson-Cook Failure ............................................................................................................. 787
               Grady Spall Failure .................................................................................................................. 788
         Thermal Specific Heat ................................................................................................................... 789
         Rigid Materials .............................................................................................................................. 789
Index ........................................................................................................................................................ 791




                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                            of ANSYS, Inc. and its subsidiaries and affiliates.                                               xv
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
xvi                               of ANSYS, Inc. and its subsidiaries and affiliates.
The Mechanical Application Approach
Use the Mechanical application to perform various types of structural, thermal, and electromagnetic analyses.
Within the Mechanical application, you define your model's environmental loading conditions, solve the
analysis, and review results in various formats depending on the analysis type. The following topics are
covered in this section.
 Overall Steps to Using the Mechanical Application
 Analysis Types
 Special Analysis Topics
 Wizards

Overall Steps to Using the Mechanical Application
This section describes the overall workflow involved when performing any analysis in the Mechanical applic-
ation. The following workflow steps are described:
 Create Analysis System
 Define Engineering Data
 Attach Geometry
 Define Part Behavior
 Define Connections
 Apply Mesh Controls and Preview Mesh
 Establish Analysis Settings
 Define Initial Conditions
 Apply Loads and Supports
 Solve
 Review Results
 Create Report (optional)

Create Analysis System
There are several types of analyses you can perform in the Mechanical application. For example, if natural
frequencies and mode shapes are to be calculated, you would choose a modal analysis.

Each analysis type is represented by an analysis system that includes the individual components of the ana-
lysis such as the associated geometry and model properties. Most analyses are represented by one independ-
ent analysis system. However, an analysis with data transfer can exist where results of one analysis are used
as the basis for another analysis. In this case, an analysis system is defined for each analysis type, where
components of each system can share data. An example of an analysis with data transfer is a response
spectrum analysis, where a modal analysis is a prerequisite.

 •   To create an analysis system, expand the Standard Analyses folder in the Toolbox and drag an analysis
     type object “template” onto the Project Schematic. The analysis system is displayed as a vertical array
     of cells (schematic) where each cell represents a component of the analysis system. Address each cell
     by right-clicking on the cell and choosing an editing option.
 •   To create an analysis system with data transfer to be added to an existing system, drag the object
     template representing the upstream analysis directly onto the existing system schematic such that red


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               1
The Mechanical Application Approach

     boxes enclose cells that will share data between the systems. After you upclick, the two schematics are
     displayed, including an interconnecting link and a numerical designation as to which cells share data.

See Building an Analysis System for more information.

Unit System Behavior
When you start the Mechanical application, the unit system defaults to the same system used in the previous
session. You can change this unit system, but subsequent Mechanical editors that you start while the first
one is open, will default to the unit system from the initial session. In the event that you change a unit system,
numerical values are converted accordingly but there is no change in physical quantity.

Define Engineering Data
A part’s response is determined by the material properties assigned to the part.

 •   Depending on the application, material properties can be linear or nonlinear, as well as temperature-
     dependent.
 •   Linear material properties can be constant or temperature-dependent, and isotropic or orthotropic.
 •   Nonlinear material properties are usually tabular data, such as plasticity data (stress-strain curves for
     different hardening laws), hyperelastic material data.
 •   To define temperature-dependent material properties, you must input data to define a property-versus-
     temperature graph.
 •   Although you can define material properties separately for each analysis, you have the option of adding
     your materials to a material library by using the Engineering Data workspace. This allows quick access
     to and re-use of material data in multiple analyses.
 •   For all orthotropic material properties, by default, the Global Coordinate System is used when you apply
     properties to a part in the Mechanical application. If desired, you can also apply a local coordinate system
     to the part.

To manage materials, right-click on the Engineering Data cell in the analysis system schematic and choose
Edit ....

See "Basics of Engineering Data" for more information.

Attach Geometry
There are no geometry creation tools in the Mechanical application so geometry must be attached to the
Mechanical application. You can create the geometry from either of the following sources:

 •   From within Workbench using DesignModeler. See the DesignModeler Help for details on the use of
     the various creation tools available.
 •   From a CAD system supported by Workbench. See the CAD Systems section for a complete list of the
     supported systems.

Before attaching the geometry from either of these sources, you can specify several options that determine
the characteristics of the geometry you choose to import. These options are: solid bodies, surface bodies,
line bodies, parameters, attributes, named selections, material properties; Analysis Type (2-D or 3–D), allowing
CAD associativity, importing coordinate systems (Import Work Points are only available in the DesignModeler
application), saving updated CAD file in reader mode, “smart” refreshing of models with unmodified com-
ponents, and allowing parts of mixed dimension to be imported as assembly components that have parts

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
2                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Related Procedures

of different dimensions. The availability of these options varies across the supported CAD systems. See the
Geometry Preferences section for details.

Related Procedures
 Procedure                Condition                                                             Procedural Steps
Specifying       Optional task that can be                  1.      In an analysis system schematic, perform either of the
geometry         done before attaching                              following:
options          geometry.                                          •     Right-click on the Geometry cell and choose Proper-
                                                                          ties

                                                                          OR
                                                                    •     Select the Geometry cell in the schematic for a
                                                                          standard analysis, the from the Workspace toolbar
                                                                          drop down menu, choose any option that includes
                                                                          Properties or Components.
                                                            2.      Check boxes to specify Default Geometry Options and
                                                                    Advanced Geometry Defaults.

Attaching        DesignModeler is running                   Double-click on the Model cell in the same analysis system
DesignModel-     in an analysis system.                     schematic. The Mechanical application opens and displays
er geometry                                                 the geometry.
to the Mech-     DesignModeler is not run-                  1.      Select the Geometry cell in an analysis system schematic.
anical applic-   ning. Geometry is stored
ation                                                       2.      Browse to the agdb file from the following access points:
                 in an agdb file.
                                                                    •     Right-click on the Geometry cell in the Project
                                                                          Schematic, Import Geometry and choose Browse.
                                                            3.      Double-click on the Model cell in the schematic. The
                                                                    Mechanical application opens and displays the geometry.

Attaching        CAD system is running.                     1.      Select the Geometry cell in an analysis system schematic.
CAD geo-                                                    2.      Right-click on the Geometry cell listed there.
metry to the
Mechanical                                                  3.      Double-click on the Model cell in the same analysis sys-
application                                                         tem schematic. The Mechanical application opens and
                                                                    displays the geometry.
                                                            4.      If required, set geometry options in the Mechanical ap-
                                                                    plication by highlighting the Geometry object and
                                                                    choosing settings under Preferences in the Details view.

                 CAD system is not running.                 1.      Select the Geometry cell in an analysis system schematic.
                 Geometry is stored in a                    2.      Browse to the CAD file from the following access points:
                 native CAD system file, or
                 in a CAD “neutral” file such                       •     Right-click on the Geometry cell in the Project
                 as Parasolid or IGES.                                    Schematic and choose Import Geometry.
                                                            3.      Double-click on the Model cell in the Project Schematic.
                                                                    The Mechanical application opens and displays the geo-
                                                                    metry.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                               3
The Mechanical Application Approach

CAD Interface Terminology
The CAD interfaces can be run in either plug-in mode or in reader mode.

 •   Attaching geometry in plug-in mode: requires that the CAD system be running.
 •   Attaching geometry in reader mode: does not require that the CAD system be running.

Updating Geometry from Within the Mechanical Application
You can selectively update individual parts by right-clicking on an individual part (or after multiple parts are
selected) and choosing Update Selected Parts:

 •   Update: Use Geometry Parameter Values synchronizes the Mechanical application model to the CAD
     model. This will read the latest geometry and process other data (parameters, attributes, etc.) based on
     the current user preferences for that model.

          Note

          If you change either the number of turns or the thickness properties associated with a body,
          these changes are not updated to the CAD model when you choose Update: Use Geometry
          Parameter Values.


The selective update feature is applied to selected part(s) only and it does not import new parts added in
the CAD system following the original import or last complete update. Parameter values for the assembly
are always updated.

In addition, this feature is not a tool for removing parts from the Mechanical application tree, however; it
will remove parts which have been selected for update in WB, but that no longer exist in the CAD model if
an update is successful (if at least one valid part is updated).

The selective update feature is supported only for the following CAD Plug-Ins and Associative Readers:
DesignModeler, Autodesk Inventor, Mechanical Desktop, OneSpace Modeling, Pro/ENGINEER, Solid Edge,
NX, CATIAv5 (Optional plug-in CAPRI), SolidWorks.

Executing the Selective Update for ACIS, CATIAv5 (Standard reader — Spatial), CATIAv4, Parasolid, XML, IGES,
or STEP will complete a full update of the model.

Define Part Behavior
After attaching geometry, you can access settings related to part behavior by right-clicking on the Model
cell in the analysis system schematic and choosing Edit .... The Mechanical application opens with the envir-
onment representing the analysis system displayed under the Model object in the tree.

An Analysis Settings object is added to the tree. See the Establish Analysis Settings (p. 8) overall step for
details.

An Initial Condition object may also be added. See the Define Initial Conditions (p. 13) overall step for details.

The Mechanical application uses the specific analysis system as a basis for filtering or making available only
components such as loads, supports and results that are compatible with the analysis. For example, a Static
Structural analysis type will allow only structural loads and results to be available.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
4                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Reference Temperature

Presented below are various options provided in the Details view for parts and bodies following import.

Stiffness Behavior
In addition to making changes to the material properties of a part, you may designate a part's Stiffness
Behavior as being flexible or rigid.

 •   Setting a part’s behavior as rigid essentially reduces the representation of the part to a single point
     mass thus significantly reducing the solution time.
 •   A rigid part will need only data about the density of the material to calculate mass characteristics. Note
     that if density is temperature dependent, density will be evaluated at the reference temperature. For
     contact conditions, specify Young’s modulus.
 •   This is applicable only for static structural, transient structural (ANSYS), transient structural (MBD) , and
     modal analyses.

Flexible is the default Stiffness Behavior. To change, simply select Rigid from the Stiffness Behavior drop-
down menu. Also see the Rigid Bodies (p. 177) section.

     Note

     Rigid behavior is not available for the SAMCEF solver.

Coordinate Systems
The Coordinate Systems object and its child object, Global Coordinate System, is automatically placed in
the tree with a default location of 0, 0, 0, when a model is imported.

For solid parts and bodies: by default, a part and any associated bodies use the Global Coordinate System.
If desired, you can apply a apply a local coordinate system to the part or body. When a local coordinate
system is assigned to a Part, by default, the bodies also assume this coordinate system but you may modify
the system on the bodies individually as desired.

For surface bodies, solid shell bodies, and line bodies: by default, these types of geometries generate co-
ordinates systems on a per element type basis. It is necessary for you to create a local coordinate system
and associated it with the parts and/or bodies using the Coordinate System setting in the Details view for
the part/body if you wish to orient those elements in a specific direction.

Reference Temperature
The default reference temperature is taken from the environment (By Environment), which occurs when
solving. This necessarily means that the reference temperature can change for different solutions. The reference
temperature can also be specified for a body and will be constant for each solution (By Body). Selecting By
Body will cause the Reference Temperature Value field to specify the reference temperature for the body.
It is important to recognize that any value set By Body will only set the reference temperature of the body
and not actually cause the body to exist at that temperature (unlike the Environment Temperature entry
on an environment object, which does set the body's temperature).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                             5
The Mechanical Application Approach


     Note

     Selecting By Environment can cause the body to exist at that temperature during the analysis
     but selecting By Body will only ever effect reference temperature. So if the environment temper-
     ature and the body have a different specification, thermal expansion effects can occur even if no
     other thermal loads are applied.


     Note

     If the material density is temperature dependent, the mass that is displayed in the Details view
     will either be computed at the body temperature, or at 22°C. Therefore, the mass computed
     during solution can be different from the value shown, if the Reference Temperature is the En-
     vironment.


     Note

     When nonlinear material effects are turned off, values for thermal conductivity, specific heat, and
     thermal expansion are retrieved at the reference temperature of the body when creating the
     ANSYS solver input.

Material Property Assignment
Once you have attached your geometry, you can choose a material for the simulation. When you select a
part in the tree outline, the Assignment entry under Material in the Details view lists a default material for
the part. You can edit material properties in the Engineering Data workspace.

Nonlinear Material Effects
You can also choose to ignore any nonlinear effects from the material properties.

 •   By default the program will use all applicable material properties including nonlinear properties such
     as stress-strain curve data.
 •   Setting Nonlinear Effects to No will ignore any nonlinear properties only for that part.
 •   This option will allow you to assign the same material to two different parts but treat one of the parts
     as linear.
 •   This option is applicable only for static structural, transient structural (ANSYS), steady state thermal and
     transient thermal analyses.

Thermal Strain Effects
For structural analyses, you can choose to have Workbench calculate a Thermal Strain result by setting
Thermal Strain Effects to Yes. Choosing this option enables the coefficient of thermal expansion to be sent
to the solver.

Beam Section
When a line body is imported into the Mechanical application, the Details view displays the Beam Section
field. This read-only field displays the name assigned to the geometry in DesignModeler or the supported



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
6                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Define Connections

CAD system, if one was defined. In addition, the field has the following beam offset options that allow you
modify geometry characteristics:

 •   Offset Mode: A drop down menu with the following options:
     –   Refresh on Update (default): Details view values update when the CAD system updates.
     –   Manual: Details view values override CAD system updates.
 •   Offset Type: Displays the selected type of offset.
     –   Centroid
     –   Shear Center
     –   Origin
     –   User Defined - if selected, the following inputs become available:
         ¡ Offset X
         ¡ Offset Y

Model Dimensions
When you attach your geometry or model, the model dimensions display in the Details View (p. 134) in the
Bounding Box sections of the Geometry or Part objects. Dimensions have the following characteristics:

 •   Units are created in your CAD system.
 •   ACIS, CATIA, and Autodesk Mechanical Desktop model units may be set.
 •   Other geometry units are automatically detected and set.
 •   Assemblies must have all parts dimensioned in the same units.

Define Connections
Connections include contact regions, joints, springs, or beams. Explicit analysis connections include body
interactions.

Contact conditions are formed where bodies meet. When an assembly is imported from a CAD system,
contact between various parts is automatically detected. In addition you can also set up contact regions
manually. You can transfer structural loads and heat flows across the contact boundaries and "connect" the
various bodies. Depending on the type of contact, the analysis can be linear or nonlinear. Please refer to
the Contact (p. 507) section for more details.

Once contact regions are established, you can examine the initial contact conditions of the assembly before
loading and adjust a variety of settings that globally affect all contact regions, as well as settings1 that
control the characteristics of individual contact regions. After solving, you can again examine results such
as contact pressure and gap values.

A joint is an idealized kinematic linkage that controls the relative movement between two bodies. Joint
types are characterized by their rotational and translational degrees of freedom as being fixed or free. Sev-
eral different types of joints are available1 such as revolute, spherical and universal joints. Rigid parts can
be connected to the rest of the structure only through joints. An automatic joint creation capability is
available to facilitate creation of joints in complex assemblies. Please refer to the Joints (p. 185) section for
more details.

You can define a spring to connect two bodies together or to connect a body to ground. Please refer to the
Springs (p. 221) section for more details.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                               7
The Mechanical Application Approach

1 - Availability depends on license level.

Apply Mesh Controls and Preview Mesh
Meshing is the process in which your geometry is spatially discretized into elements and nodes. This mesh
along with material properties is used to mathematically represent the stiffness and mass distribution of
your structure.

Your model is automatically meshed at solve time. The default element size is determined based on a
number of factors including the overall model size, the proximity of other topologies, body curvature, and
the complexity of the feature. If necessary, the fineness of the mesh is adjusted up to four times (eight times
for an assembly) to achieve a successful mesh.

If desired, you can preview the mesh before solving. Mesh controls are available to assist you in fine tuning
the mesh to your analysis. Please refer to the Meshing Help for further details.

To preview the mesh in the Mechanical Application:
See the Previewing Surface Mesh section.

To apply global mesh settings in the Mechanical Application:
See the Global Mesh Controls section.

To apply mesh control tools on specific geometry in the Mechanical Application:
See the Local Mesh Controls section.

Establish Analysis Settings
Each analysis type includes a group of analysis settings that allow you to define various solution options
customized to the specific analysis type, such as large deflection for a stress analysis. Refer to the specific
                                                                                               .
analysis types section for the customized options presented under “Preparing the Analysis” Default values
are included for all settings. You can accept these default values or change them as applicable.

Some procedures below include animated presentations. Please view online if you are reading the PDF version
of the help. Interface names and other components shown in the demos may differ from those in the released
product.

 To verify/change analysis settings in the Mechanical application:
 1.   Highlight the Analysis Settings object in the tree. This object was inserted automatically when you
      established a new analysis in the Create Analysis System (p. 1) overall step.
 2.   Verify or change settings in the Details view of the Analysis Settings object. These settings include
      default values that are specific to the analysis type. You can accept or change these defaults. If your
      analysis involves the use of steps, refer to the procedures presented below.

 To create multiple steps (applies to structural static, transient structural (ANSYS), transient
 structural (MBD), steady-state thermal, transient thermal, magnetostatic, and electric analyses):

 You can create multiple steps using any one of the following methods:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
8                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Establish Analysis Settings

1.   Highlight the Analysis Settings object in the tree. Modify the Number of Steps field in the Details
     view. Each additional Step has a default Step End Time that is one second more than the previous
     step. These step end times can be modified as needed in the Details view. You can also add more
     steps simply by adding additional step End Time values in the Tabular Data window.

     The following demonstration illustrates adding steps by modifying the Number of Steps field in the
     Details view.




     Or
2.   Highlight the Analysis Settings object in the tree. Begin adding each step's end time values for the
     various steps to the Tabular Data window. You can enter the data in any order but the step end time
     points will be sorted into ascending order. The time span between the consecutive step end times
     will form a step. You can also select a row(s) corresponding to a step end time, click the right mouse
     button and choose Delete Rows from the context menu to delete the corresponding steps.

     The following demonstration illustrates adding steps directly in the Tabular Data window.




     Or
3.   Highlight the Analysis Settings object in the tree. Choose a time point in the Graph window. This
     will make the corresponding step active. Click the right mouse button and choose Insert Step from
     the context menu to split the existing step into two steps, or choose Delete Step to delete the step.

     The following demonstration illustrates inserting a step in the Graph window, changing the End Time
     in the Tabular Data window, deleting a step in the Graph window, and deleting a step in the Tabular
     Data window.




Specifying Analysis Settings for Multiple Steps
1.   Create multiple steps following the procedure ”To create multiple steps” above.
2.   Most Step Controls, Nonlinear Controls, and Output Controls fields in the Details view of Analysis
     Settings are “step aware” that is, these settings can be different for each step. Refer to the table in
                               ,
     Analysis Settings for Most Analysis Types (p. 238) to determine which specific controls are step aware
     (designated as footnote 2 in the table). Activate a particular step by selecting a time value in the Graph



                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                              9
The Mechanical Application Approach

     window or the Step bar displayed below the chart in the Graph window. The Step Controls grouping
     in the Details view indicates the active Step ID and corresponding Step End Time.

     The following demonstration illustrates turning on the legend in the Graph window, entering analysis
     settings for a step, and entering different analysis settings for another step.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
10                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                           Establish Analysis Settings


Note




       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                             11
The Mechanical Application Approach


          If you want to specify the same analysis setting(s) to several steps, you can select all the
          steps of interest as follows and change the analysis settings details.

          •   To change analysis settings for a subset of all of the steps:
              –    From the Tabular Data window:
                   1.    Highlight the Analysis Settings object.
                   2.    Highlight steps in the Tabular Data window using either of the following
                         standard windowing techniques:
                         ¡ Ctrl key to highlight individual steps.
                         ¡ Shift key to highlight a continuous group of steps.
                   3.    Click the right mouse button in the window and choose Select All Highlighted
                         Steps from the context menu.
                   4.    Specify the analysis settings as needed. These settings will apply to all selected
                         steps.
              –    From the Graph window:
                   1.    Highlight the Analysis Settings object.
                   2.    Highlight steps in the Graph window using either of the following standard
                         windowing techniques:
                         ¡ Ctrl key to highlight individual steps.
                         ¡ Shift key to highlight a continuous group of steps.
                   3.    Specify the analysis settings as needed. These settings will apply to all selected
                         steps.
          •   To specify analysis settings for all the steps:
              1.    Click the right mouse button in either window and choose Select All Steps.
              2.    Specify the analysis settings as needed. These settings will apply to all selected
                    steps.

          The following demonstration illustrates multiple step selection using the bar in the Graph
          window, entering analysis settings for all selected steps, selecting only highlighted steps in
          the Tabular Data window, and selecting all steps.




          The Worksheet tab for the Analysis Settings object provides a single display of pertinent
          settings in the Details view for all steps.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
12                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                             Define Initial Conditions




Details of various analysis settings are discussed in Analysis Settings (p. 238).

Define Initial Conditions
This step is based upon the selected type analysis. Workbench provides you with the ability to begin your
analysis with an initial condition, a link to an existing solved or associated environment, or an initial temper-
ature.

For the following analysis types, a tree object is automatically generated allowing you to define specifications.
For additional information, please see the individual analysis types section.

Analysis         Tree Object            Description
Type
Transient        Initial Condi-         A transient structural (ANSYS) analysis is at rest, by default.The Initial
Structural       tions                  Conditions object allows you to specify Velocity.
(ANSYS)
Explicit Dy-     Initial Condi-         An explicit dynamics analysis is at rest, by default.The Initial Conditions
namics           tions                  object allows you to specify Velocity and/or Angular Velocity.
Modal            Pre-Stress             A modal analysis can use the stress results from a static structural analysis
                                        to account for stress-stiffening effect.
Linear Buck-     Pre-Stress             A linear buckling analysis must use the stress-stiffening effects of a static
ling                                    structural analysis.
Random Vibra-    Modal                  A random vibration or response spectrum analysis must use the mode shapes
tion or Re-                             derived in a modal analysis.
sponse Spec-
trum
Steady-State     Initial Temper-        For a steady-state thermal analysis, you have the ability to specify an initial
Thermal          ature                  temperature.
Transient        Initial Temper-        For a transient thermal analysis, the initial temperature distribution should
Thermal          ature                  be specified.


     Note

     Temperatures from a steady-state thermal or transient thermal analysis can be applied to a static
     structural or transient structural (ANSYS) analysis as a Thermal Condition load.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              13
The Mechanical Application Approach

Depending upon the analysis type an object is automatically added to the tree. To define an initial condition
in the Mechanical application:

 •   For a Transient Structural (ANSYS), use the Initial Conditions object to insert Velocity. For an Explicit
     Dynamics analysis, use the Initial Conditions object to insert Velocity and/or Angular Velocity.

     These values can be scoped to specific parts of the geometry. For a Transient Structural (ANSYS)
     analysis, you can also set an initial condition using step controls.
 •   For a Modal or a Linear Buckling analysis, use the Details view of the Pre-Stress object to define the
     associated Pre-Stress Environment.
 •   For a Random Vibration or Response Spectrum analysis, you must point to a modal analysis using
     the drop-down list of the Modal Environment field in the Details view.
 •   For the Steady-State and Transient Thermal analyses, use the Details of the Initial Temperature object
     to scope the initial temperature value. For a Transient Thermal analysis that has a non-uniform temper-
     ature, you need to define an associated Initial Temperature Environment.

Apply Loads and Supports
You apply loads and support types based on the type of analysis. For example, a stress analysis may involve
pressures and forces for loads, and displacements for supports, while a thermal analysis may involve convec-
tions and temperatures.

Loads applied to static structural, transient structural (ANSYS), transient structural (MBD), steady-state thermal,
transient thermal, magnetostatic, electric, and thermal-electric analyses default to either step-applied or
ramped. That is, the values applied at the first substep stay constant for the rest of the analysis or they increase
gradually at each substep.

Load                                                                    Load
                                                                                                      Substep


                      Full value applied
                                                                                                      Load step
                      at first substep

                                     1                                                                     1
                                                                 Final

                                                                 load

                                                                 value




                                                        2                                                                  2



                                                        Time                                                                        Time

         (a) Stepped loads                                                                 (b) Ramped loads



You can edit the table of load vs. time and modify this behavior as needed.

By default you have one step. However you may introduce multiple steps at time points where you want
to change the analysis settings such as the time step size or when you want to activate or deactivate a load.
An example is to delete a specified displacement at a point along the time history.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
14                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Solve

You do not need multiple steps simply to define a variation of load with respect to time. You can use tables
or functions to define such variation within a single step. You need steps only if you want to guide the
analysis settings or boundary conditions at specific time points.

When you add loads or supports in a static or transient analysis, the Tabular Data and Graph windows
appear. You can enter the load history, that is, Time vs Load tabular data in the tabular data grid. Another
option is to apply loads as functions of time. In this case you will enter the equation of how the load varies
with respect to time. The procedure “To apply a tabular or function load” is outlined under the How to Apply
Loads (p. 317) section.

     Note
      •   You can also import or export load histories from or to any pre-existing libraries.
      •   If you have multiple steps in your analysis, the end times of each of these steps will always
          appear in the load history table. However you need not necessarily enter data for these time
          points. These time points are always displayed so that you can activate or deactivate the
          load over each of the steps. Similarly the value at time = 0 is also always displayed.
      •   If you did not enter data at a time point then the value will be either a) a linearly interpolated
          value if the load is a tabular load or b) an exact value determined from the function that
          defines the load. An “=” sign is appended to such interpolated data so you can differentiate
          between the data that you entered and the data calculated by the program as shown in the
          example below. Here the user entered data at Time = 0 and Time = 5. The value at Time =
          1e-3, the end time of step 1, is interpolated.




To apply loads or supports in the Mechanical Application:
See the How to Apply Loads (p. 317) section.

Solve
This step initiates the solution process. The solution could be carried out on your local machine or on a remote
machine such as a powerful server you might have access to.

Since nonlinear or transient solutions can take significant time to complete, a status bar is provided that
indicates the overall progress of solution. More detailed information on solution status can be obtained from
the Solution Information object which is automatically inserted under the Solution folder for all analyses.

You can use the Remote Solve Manager (RSM) to perform solutions on a remote machine. Once the solution
is completed the results will be brought back to the local machine for postprocessing. Refer to the Solve
Process Capabilities (p. 416) section for more details.

The overall solution progress is indicated by a status bar. In addition you can use the Solution Information
object which is inserted automatically under the Solution folder. This object allows you to i) view the actual
output from the solver, ii) graphically monitor items such as convergence criteria for nonlinear problems
and iii) diagnose possible reasons for convergence difficulties by plotting Newton-Raphson residuals. Addi-


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 15
The Mechanical Application Approach

tionally you can also monitor some result items such as displacement or temperature at a vertex or contact
region’s behavior as the solution progresses.

Solve References for the Mechanical Application
See the Solving Overview (p. 415) section for details on the above and other topics related to solving.

Review Results
The analysis type determines the results available for you to examine after solution. For example, in a
structural analysis, you may be interested in equivalent stress results or maximum shear results, while in a
thermal analysis, you may be interested in temperature or total heat flux. The Results in the Mechanical Ap-
plication (p. 340) section lists various results available to you for postprocessing.

 To add result objects in the Mechanical application:
 1.   Highlight a Solution object in the tree.
 2.   Select the appropriate result from the Solution context toolbar or use the right-mouse click option.

 To review results in the Mechanical application:
 1.   Click on a result object in the tree.
 2.   After the solution has been calculated, you can review and interpret the results in the following ways:

      •   Contour results - Displays a contour plot of a result such as stress over geometry.
      •   Vector Plots - Displays certain results in the form of vectors (arrows).
      •   Probes - Displays a result at a single time point, or as a variation over time, using a graph and a
          table.
      •   Charts - Displays different results over time, or displays one result against another result, for example,
          force vs. displacement.
      •   Animation - Animates the variation of results over geometry including the deformation of the
          structure.
      •   Stress Tool - to evaluate a design using various failure theories.
      •   Fatigue Tool - to perform advanced life prediction calculations.
      •   Contact Tool - to review contact region behavior in complex assemblies.
      •   Beam Tool - to evaluate stresses in line body representations.

           Note

           Displacements of rigid bodies are shown correctly in transient structural (ANSYS) and tran-
           sient structural (MBD) analyses. If rigid bodies are used in other analyses such as static
           structural or modal analyses, the results are correct, but the graphics will not show the de-
           formed configuration of the rigid bodies in either the result plots or animation.


See the Results in the Mechanical Application (p. 340) section for more references on results.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
16                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Introduction

Create Report (optional)
Workbench includes a provision for automatically creating a report based on your entire analysis. The docu-
ments generated by the report are in HTML. The report generates documents containing content and
structure and uses an external Cascading Style Sheet (CSS) to provide virtually all of the formatting inform-
ation.

Report References for the Mechanical Application
See the Report Preview (p. 494) section.

Analysis Types
You can perform several types of analyses in the Mechanical application using pre-configured analysis systems
(see Create Analysis System (p. 1)). For doing more advanced analysis you can use Commands objects in
the Mechanical interface. This will allow you to enter the Mechanical APDL application commands in the
Mechanical application to perform the analysis. If you are familiar with the Mechanical APDL application
commands, you will have the capability of performing analyses and techniques that are beyond those
available using the analysis systems in Workbench.

This section describes the following analysis types that you can perform in the Mechanical interface. Available
features can differ from one solver to another. Each analysis section assumes that you are familiar with the
nature and background of the analysis type as well as the information presented in the Overall Steps to Using
the Mechanical Application (p. 1) section.
 Electric Analysis
 Explicit Dynamics Analysis
 Harmonic Response Analysis
 Linear Buckling Analysis
 Magnetostatic Analysis
 Modal Analysis
 Random Vibration Analysis
 Response Spectrum Analysis
 Shape Optimization Analysis
 Static Structural Analysis
 Steady-State Thermal Analysis
 Thermal-Electric Analysis
 Transient Structural Analyses
 Transient Thermal Analysis

Electric Analysis
Introduction
An electric analysis supports Steady-State Electric Conduction. Primarily, this analysis type is used to determine
the electric potential in a conducting body created by the external application of voltage or current loads.
From the solution, other results items are computed such as conduction currents, electric field, and joule
heating.

An Electric Analysis supports single and multibody parts. Contact conditions are automatically established
between parts. In addition, an analysis can be scoped as a single step or in multiple steps.

An Electric analysis computes Joule Heating from the electric resistance and current in the conductor. This
joule heating may be passed as a load to a Thermal analysis simulation using an Imported Load if the Electric

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        17
The Mechanical Application Approach

analysis Solution data is to be transferred to Thermal analysis. Similarly, an electric analysis can accept a
Thermal Condition from a thermal analysis to specify temperatures in the body for material property evaluation
of temperature-dependent materials.

Points to Remember
A steady-state electric analysis may be either linear (constant material properties) or nonlinear (temperature
dependent material properties). Additional details for scoping nonlinearities are described in the Nonlinear
Controls section.

Once an Electric Analysis is created, Voltage and Current loads can be applied to any conducting body. For
material properties that are temperature dependent, a temperature distribution can be imported using the
Thermal Condition option.

In addition, equipotential surfaces can be created using the Coupling Condition load option.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

From the Toolbox, drag the Electric template to the Project Schematic.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

       When an Emag license is being used only the following material properties are allowed: Iso-
       tropic Resistivity, Orthotropic Resistivity, Relative Permeability, Relative Permeability (Ortho-
       tropic), Coercive Force & Residual Induction, B-H Curve, B-H Curve (Orthotropic), Demagnet-
       ization B-H Curve. You may have to turn the filter off in the Engineering Data workspace to
       suppress or delete those material properties/models which are not supported for this license.

Attach Geometry

          Basic general information about this topic

           ... for this analysis type:

       3-D shell bodies and line bodies are not supported in an electric analysis.

Define Part Behavior

          Basic general information about this topic

           ... for this analysis type:



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
18                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis

       There are no specific considerations for an electric analysis.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       In an electric analysis, only bonded, face-face contact is valid. Any joints or springs are ignored.
       For perfect conduction across parts, use the MPC formulation. To model contact resistance,
       use Augmented Lagrange or Pure Penalty with a defined Electric Conductance.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       Only higher order elements are allowed for an electric analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For an electric analysis, the basic controls are:

       Step Controls (p. 266): used to specify the end time of a step in a single or multiple step ana-
       lysis.

       Multiple steps are needed if you want to change load values, the solution settings, or the
       solution output frequency over specific steps. Typically you do not need to change the default
       values.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. A multi-step analysis involves calculating solutions at several
       time points in the load history. However you may not be interested in all of the possible
       results items and writing all the results can make the result file size unwieldy. You can restrict
       the amount of output by requesting results only at certain time points or limit the results
       that go onto the results file at each time point.

       Analysis Data Management (p. 277) settings.

Define Initial Conditions

         Basic general information about this topic

          ... for this analysis type:

       There is no initial condition specification for an Electric analysis.

Apply Loads and Supports

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              19
The Mechanical Application Approach


             Basic general information about this topic

              ... for this analysis type:

        The following loads are supported in a Steady-State Electric analysis:

         •     Voltage
         •     Current
         •     Coupling Condition (Electric)
         •     Thermal Condition

Solve

             Basic general information about this topic

              ... for this analysis type:

        The Solution Information object provides some tools to monitor solution progress.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the model during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

Review Results

             Basic general information about this topic

              ... for this analysis type:

        Applicable results are all electric result types.

        Once a solution is available, you can contour the results or animate the results to review the
        responses of the model.

        For the results of a multi-step analysis that has a solution at several time points, you can use
        probes to display variations of a result item over the steps.

        You may also wish to use the Charts feature to plot multiple result quantities against time
        (steps). For example, you could compare current and joule heating. Charts can also be useful
        when comparing the results between two analysis branches of the same model.

Explicit Dynamics Analysis
Introduction
You can perform a transient explicit dynamics analysis in the Mechanical application using an Explicit Dy-
namics (ANSYS) system. Additionally, the Explicit Dynamics (LS-DYNA Export) system is available to export
the model in LS-DYNA .k file format for subsequent analysis with the LS-DYNA solver. Unless specifically
mentioned otherwise, this section addresses both the ANSYS AUTODYN and LS-DYNA solvers. Special condi-
tions for the LS-DYNA solver are noted where pertinent.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
20                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Points to Remember

An explicit dynamics analysis is used to determine the dynamic response of a structure due to stress wave
propagation, impact or rapidly changing time-dependent loads. Momentum exchange between moving
bodies and inertial effects are usually important aspects of the type of analysis being conducted. This type
of analysis can also be used to model mechanical phenomena that are highly nonlinear. Nonlinearities may
stem from the materials, (for example, hyperelasticity, plastic flows, failure), from contact (for example, high
speed collisions and impact) and from the geometric deformation (for example, buckling and collapse).
Events with time scales of less than 1 second (usually of order 1 millisecond) are efficiently simulated with
this type of analysis. For longer time duration events, consider using a Transient Structural (ANSYS) Analys-
is (p. 76) system.

Points to Remember
An explicit dynamics analysis typically includes many different types of nonlinearities including large deform-
ations, large strains, plasticity, hyperelasticity, material failure etc.

The time step used in an explicit dynamics analysis is constrained to maintain stability and consistency via
the CFL condition, that is, the time increment is proportional to the smallest element dimension in the
model and inversely proportional to the sound speed in the materials used. Time increments are usually on
the order of 1 microsecond and therefore thousands of time steps (computational cycles) are usually required
to obtain the solution.

 •   Explicit dynamics analyses only support the mm, mg, ms solver unit system . This will be extended to
     support more unit systems in a future release.
 •   2-D analyses are not supported in Explicit Dynamics, but are available as a beta feature for preprocessing
     in the Mechanical application. Analyses set-up this way may then be imported into ANSYS AUTODYN,
     where they can be solved and postprocessed.
 •   Consideration should be given to the number of elements in the model and the quality of the mesh to
     give larger resulting time steps and therefore more efficient simulations.
 •   A coarse mesh can often be used to gain insight into the basic dynamics of a system while a finer mesh
     is required to investigate nonlinear material effects and failure.
 •   The quality of the solution can be monitored by reviewing momentum and energy conservation graphs
     in the solution output. Low energy errors (<10% of initial energy) are indicative of good quality solutions.
 •   The Explicit Dynamics (LS-DYNA Export) system allows for an LS-DYNA input file (otherwise known as
     a “keyword” file or a “.k” file) to be exported. This keyword file contains all the necessary information
     available in the Mechanical application environment to carry out the analysis with the LS-DYNA solver.

     The exported keyword file follows the same format as the one exported by the respective Mechanical
     APDL application. All the LS-DYNA keywords are implemented according to the “LS_DYNA Keyword
     Users Manual” version 971.

     All the LS-DYNA keywords that can currently be exported are described in detail in Supported LS-DYNA
     Keywords (p. 651). Any parameters that are not shown for a card are not used and their default values
     will be assigned for them by the LS-DYNA solver. Some descriptions of Workbench features that do not
     relate directly to keywords are given under ”General Descriptions” located at the end of this appendix.
 •   When using Commands objects with the Explicit Dynamics (LS-DYNA ) solver, be aware of the following:
     –   Keyword cards read from Commands object content (renamed to "Keyword" snippets for the LS-
         DYNA system) should not have any trailing empty lines if they are not intentional. This is due to the
         fact that some keywords have more than one mandatory card that can be entered as blank lines,
         in which case the default values for the card will be used. Hence trailing blank lines can be significant
         only if required, otherwise they may cause solver execution errors.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              21
The Mechanical Application Approach

     –   The first entry in the Commands object content must be a command name which is preceded by
         the * symbol.
     –   Refer to LS-DYNA General Descriptions (p. 676) regarding ID numbers entered in Commands object
         content.

An explicit dynamics analysis can contain both rigid and flexible bodies. For rigid/flexible body dynamic
simulations involving mechanisms and joints you may wish to consider using either the Transient Structural
(ANSYS) Analysis (p. 76) or Transient Structural (MBD) Analysis (p. 84) options.

     Note

     The intent of this document is to provide an overview of an explicit dynamics analysis. Consult
     our technical support department to obtain a more thorough treatment of this topic.

Preparing the Analysis
Create Analysis System

              Basic general information about this topic

               ... for this analysis type:

         From the Toolbox drag an Explicit Dynamics (ANSYS) or an Explicit Dynamics (LS-DYNA
         Export) template to the Project Schematic.

Define Engineering Data

              Basic general information about this topic

               ... for this analysis type:

         Material properties can be linear elastic or orthotropic. Many different forms of material
         nonlinearity can be represented including hyperelasticity, rate and temperature dependant
         plasticity, pressure dependant plasticity, porosity, material strength degradation (damage),
         material fracture/failure/fragmentation. For a detailed discussion on material models used in
         Explicit Dynamics, please refer to Appendix D (p. 729).

         Density must always be specified for materials used in an explicit dynamics analysis.

         Data for a range of materials is available in the Explicit material library.

         For Explicit Dynamics (LS-DYNA Export) systems, only the following material models are
         supported (also see *MAT_ keywords in Supported LS-DYNA Keywords (p. 651)). Any models
         that are not mentioned in this list can be entered through the "Keyword Snippet" facility (see
         the LS-DYNA General Descriptions section):

          •     Strength models
                –   Linear Elastic
                    ¡ Isotropic
                    ¡ Orthotropic


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
22                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Preparing the Analysis

             –   Plasticity
                 ¡ Bilinear Isotropic Hardening
                 ¡ Multilinear Isotropic Hardening
                 ¡ Bilinear Kinematic Hardening
                 ¡ Johnson Cook
             –   Hyperelastic:
                 ¡ Mooney-Rivlin
                 ¡ Polynomial
                 ¡ Yeoh
                 ¡ Ogden
             –   Rigid (there is no entry for this in the Engineering Data workspace of Workbench.
                 See *MAT_RIGID in Supported LS-DYNA Keywords (p. 651) for more details).
       •     Equation of state (EOS) models
             –   Linear (there is no entry for this in the Engineering Data workspace of Workbench.
                 See *EOS_LINEAR_POLYNOMIAL in Supported LS-DYNA Keywords (p. 651) for more
                 details).
             –   Shock
       •     Failure models
             –   Plastic Strain
             –   Johnson Cook

             Note

             For line bodies, the LS-DYNA solver only supports the following three material
             properties from the above list: Isotropic Linear Elastic, Bilinear Kinematic Hardening
             Plasticity and Rigid bodies. Additional material models that are supported by the
             LS-DYNA solver for line bodies can be added through the "Keyword Snippet" facility.

Attach Geometry

           Basic general information about this topic

            ... for this analysis type:

      Solid, plane and line bodies can be present in an explicit dynamics analysis. Springs and
      dampers are not available.

      Only symmetric cross sections are supported for line bodies in explicit dynamics analyses,
      except for the Explicit Dynamics (LS-DYNA Export) systems. The following cross sections are
      not supported: T-Sections, L-Sections, Z-Sections, Hat sections, Channel Sections. For I-Sections,
      the two flanges must have the same thickness. For rectangular tubes, opposite sides of the
      rectangle must be of the same thickness. For LS-DYNA Export systems all available cross
      sections in DesignModeler will be exported for analysis with the LS-DYNA solver. However
      there are some limitations in the number of dimensions that the LS-DYNA solver supports


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                              23
The Mechanical Application Approach

       for the Z, Hat and Channel cross sections. For more information consult the LS-DYNA Keywords
       manual.

       To prevent the generation of unnecessarily small elements (and long run times) try using
       DesignModeler to remove unwanted “small” features or holes from your geometry.

       Note that the 2-D Analysis Type is currently only available as a beta option (not supported)
       but may be used to setup 2-D simulations to be transferred to ANSYS AUTODYN to perform
       a solve, if a license is available.

       Symmetry is not supported when exporting to the LS-DYNA .k file.

Define Part Behavior

            Basic general information about this topic

             ... for this analysis type:

       Nonlinear effects are always accounted for in explicit dynamics analysis.

       Parts may be defined as rigid or flexible. In the solver, rigid parts are represented by a single
       point that carries the inertial properties together with a discretized exterior surface that
       represents the geometry. Rigid bodies should be meshed using similar Method mesh controls
       as those used for flexible bodies. The inertial properties used in the solver will be derived
       from the discretized representation of the body and the material density and hence may
       differ slightly from the values presented in the properties of the body in the Mechanical ap-
       plication GUI.

       At least one flexible body must be specified when using the ANSYS AUTODYN solver. The
       solver requires this in order to calculate the time-step increments. In the absence of a flexible
       body, the time-step becomes underdefined. The boundary conditions allowed for the rigid
       bodies with explicit dynamics are:

        •     Connections
              –   Contact Regions - Frictionless, Frictional and Bonded.
              –   Body Interactions: Frictionless, Frictional and Bonded. Bonded body interactions are
                  not supported for LS-DYNA Export.
              –   For ANSYS AUTODYN, rigid bodies may not be bonded to other rigid bodies.
        •     Initial Conditions: Velocity, Angular Velocity
        •     Supports: Displacement, Fixed Support and Velocity.
        •     Loads: Pressure and Force. Force is not supported for ANSYS AUTODYN.

       For an Explicit Dynamics (ANSYS) analysis, the following postprocessing features are available
       for rigid bodies:

        •     Results and Probes: Deformation only - that is, Displacement, Velocity.
        •     Result Trackers: Body average data only.

       If a multibody part consists only of rigid bodies, all of which share the same material assign-
       ment, the part will act as a single rigid body, even if the individual bodies are not physically
       connected.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
24                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Preparing the Analysis

Define Connections

           Basic general information about this topic

            ... for this analysis type:

      Line body to line body contact is possible if:

       •     Contact Detection should be set to Proximity Based in the Body Interactions Details
             view.
       •     Edge on Edge is set to Yes in the Body Interactions Details view.
       •     The Interaction Type is defined as Frictional or Frictionless – bonded interactions and
             connections are not supported for line bodies.

      Reinforcement body interaction should be supported in the case when only line bodies are
      scoped to a Body Interaction of Type = Reinforcement. The line bodies will then be tied
      to any solid body that they intersect.

      Body Interactions, Contact and Spot Welds are all valid in explicit dynamics analyses. Frictional,
      Frictionless and Bonded body interactions and contact options are available. Conditionally
      bonded contact can be simulated using the breakable property of each bonded region. Spot
      Welds can also be made to fail using the breakable property.

      Joints, Springs and Beam connections are not supported for explicit dynamics analyses. The
      Contact Tool is also not applicable to explicit dynamics analyses.

      By default, a Body Interaction object will be automatically inserted in the Mechanical applic-
      ation tree and will be scoped to all bodies in the model. This object activates frictionless
      contact behavior between all bodies that come into proximity during the analysis.

      For Explicit Dynamics (LS-DYNA Export) systems, bonded body interactions are not supported.
      Also, Contact Region objects with Auto Asymmetric Behavior or just Asymmetric Behavior
      are treated the same. Symmetric Behavior will create a _SURFACE_TO_SURFACE keyword
      for the contact and an Asymmetric Behavior will create a _NODES_TO_SURFACE keyword.

Apply Mesh Controls/Preview Mesh

           Basic general information about this topic

            ... for this analysis type:

      A smooth uniform mesh should be sought in the regions of interest for the analysis. Elsewhere,
      coarsening of the mesh may help to reduce the overall size of the problem to be solved. Use
      the Explicit meshing preference (set by default) to auto-assign the default mesh controls
      that will provide a mesh well suited for explicit dynamics analyses. This preference automat-
      ically sets the Rigid Body Behavior mesh control to Full Mesh. The Full Mesh setting is
      only applicable to explicit dynamics analyses.

      Swept/multi-zone meshes are preferred in explicit dynamics analyses so geometry slicing,
      combined with multibody part options in DesignModeler are recommended to facilitate
      hexahedral meshing. Alternatively use the patch independent tetrahedral meshing method
      to obtain more uniform element sizing and take advantage of automatic defeaturing.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                              25
The Mechanical Application Approach

       Define the element size manually to produce more uniform element size distributions espe-
       cially on surface bodies.

       Midside nodes should be dropped from the mesh for all elements types (solids, surface and
       line bodies). Error/warning messages are provided if unsupported (higher order) elements
       are present in the mesh.

       Pyramid elements are not supported in Explicit Dynamics analyses. Any elements of this type
       are converted into two tetrahedral elements, and will warrant a warning in the message
       window of the Mechanical application.

       For Explicit Dynamics (LS-DYNA Export) systems, only the element types listed below are
       supported (partly due to LS-DYNA limitations). Any parts with a mesh containing unsupported
       elements will be excluded from the exported mesh. A warning is displayed specifying excluded
       parts.

        •     Shells
              –   1st Order: triangles, quadrilaterals
              –   2nd Order: none
        •     Solids
              –   1st Order: tetrahedrons, pyramids, wedges, hexahedrons, beams
              –   2nd Order: tetrahedrons

              Note

              Pyramids are not recommended for LS-DYNA, a warning is issued if such elements
              are present in the mesh.

Establish Analysis Settings

            Basic general information about this topic

             ... for this analysis type:

       The basic analysis settings for explicit dynamics analyses are:

        •     Step Controls - The required input for step control is the termination time for the ana-
              lysis. This should be set to your best estimate of the solution time required to simulate
              the event being modeled. You should normally allow the solver to determine its own
              time step size based on the smallest CFL condition in the model. The efficiency of the
              solution can be increased with the help of mass scaling options. Use this feature with
              caution. Too much mass scaling can give rise to non-physical results.

              An explicit dynamic solution may be started, interrupted and resumed at any point in
              time. For example, an existing solution that has reached its End Time may be extended
              to continue to review the progression of the mechanical phenomena simulated. The
              Resume From Cycle option allows you to select which Restart file you would like the
              Solve to resume the analysis from. See Resume Capability for Explicit Dynamics (ANSYS)
              Analyses (p. 488) for more information. Explicit dynamics analyses are always solved in a
              single analysis step.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
26                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                       Preparing the Analysis

    Step Control options
    –   Resume from cycle (option not available in LS-DYNA)
    –   Maximum Number of Cycles in ANSYS AUTODYN is replaced by Maximum time
        steps in LS-DYNA
    –   Reference energy cycle (option not available in LS-DYNA)
    –   The Maximum Element Scaling and Update frequency (options not available in
        LS-DYNA)
•   Solver Controls – These advanced controls allow you to control a range of solver features
    including element formulations and solution velocity limits. The defaults are applicable
    to wide range of applications.
    –   Shell thickness update, shell inertia update, density update, minimum velocity, max-
        imum velocity and radius cutoff options can only be set in ANSYS AUTODYN.
    –   Full shell integration is available only in LS-DYNA.
•   Damping Controls – Damping is used to control oscillations behind shock waves and
    reduce hourglass modes in reduced integration elements. These options allow you to
    adapt the levels of damping, and formulation used for the analysis being conducted.
    Elastic oscillations in the solution can also be automatically damped to provide a quasi-
    static solution after a dynamic event.

    For Hourglass Damping, only one of either the Viscous Coefficient or Stiffness Coef-
    ficient, is used for the Flanagan Belytschko option - when running an explicit dynamics
    analysis using the LS-DYNA solver, LS-DYNA does not allow for two coefficients to be
    entered in *CONTROL_HOURGLASS. Thus the non-zero coefficient determines the
    damping format to be either “Flanagan-Belytschko viscous” or “Flanagan-Belytschko
    stiffness” accordingly. if both are non-zero, the Stiffness Coefficient will be used
              ,
    –   Linear viscosity in expansion options should be available only for ANSYS AUTODYN.
    –   Hourglass damping in LS-DYNA is standard by default, in ANSYS AUTODYN the same
        control is AUTODYN Standard.
•   Erosion Controls – Erosion is used to automatically remove highly distorted elements
    from an analysis and is required for applications such as cutting and impact penetration.
    In an explicit dynamics analysis, erosion is a numerical tool to help maintain large time
    steps, and thus obtain solutions in appropriate time scales. Several options are available
    to initiate erosion. The default settings will erode elements which experience geometric
    strains in excess of 100%. The default value should be increased when modeling hyper-
    elastic materials. Geometric strain limit and material failure criteria are not present in
    LS-DYNA.
•   Output Controls – Solution output is provided in several ways:
    –   Results files which are used to provide nodal and element data for contour and probe
        results such as deformation, velocity, stress and strain. Note that probe results will
        provide a filtered time history of the result data due to the relatively infrequent
        saving of results files.
    –   Restart files should be stored less frequently than results files and can be used to
        resume an analysis.
    –   Tracker data is usually stored much more frequently than results or restart data and
        thus is used to produce full transient data for specific quantities.



             Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                         of ANSYS, Inc. and its subsidiaries and affiliates.                                              27
The Mechanical Application Approach

              –   Output controls to save result tracker and solution output are not available for LS-
                  DYNA.

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

        •     Initial conditions are defined by either applying a translational or rotational velocity to
              a single body or to multiple bodies.
        •     In an explicit dynamics analysis, by default, all bodies are assumed to be at rest with no
              external constraint or load applied. It is not a requirement to apply an initial condition
              to a body.
        •     An Explicit Dynamics solve can be performed if the model contains at least one Initial
              Condition (Translational or Rotational velocity), or a non-zero constraint (displacement
              or velocity), or a valid load.

Apply Loads and Supports

            Basic general information about this topic

             ... for this analysis type:

        •     You can apply the following loads and supports in an explicit dynamics analysis:
              – Acceleration (p. 280)
              –   Standard Earth Gravity (p. 282)
              –   Pressure (p. 284)
              –   Force (p. 285)
              –   Line Pressure (p. 293)
              –   Fixed Face (p. 329)
              –   Fixed Edge (p. 329)
              –   Fixed Vertex (p. 330)
              –   Displacement for Faces (p. 330)
              –   Displacement for Edges (p. 331)
              –   Displacement for Vertices (p. 332)
              –   Velocity (p. 334)
              –   Impedance Boundary (p. 339)
              –   Simply Supported Edge (p. 336)
              –   Simply Supported Vertex (p. 336)
              –   Fixed Rotation (p. 337)
        •     Explicit Dynamics does not support cylindrical coordinate systems to specify the directions
              of components for loads and constraints.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
28                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

        •     Step or time varying tabular loads can be applied in an explicit dynamics analysis.
              However, Explicit Dynamics does not support tabular data to specify the magnitude or
              components of Accelerations or Line Pressures. Functionally defined loads are not
              available.
        •     A step displacement condition will be applied as a linearly varying displacement over
              the solution time, that is, the specified displacement will only be reached when the
              analysis reaches the specified End Time.
        •     Loads must be applied in a single step.
        •     For Explicit Dynamics (ANSYS), if multiple constraints (for example, displacements) are
              applied to a node then they must use the same coordinate system. This restriction is
              especially applicable at nodes on a shared topology such as an edge, where two adjacent
              faces, each with different constraints, may come together. These constraints must use
              the same coordinate system in their specification.
        •     In LS-DYNA, a Velocity or Displacement boundary condition (implemented with the
              *BOUNDARY_PRESCRIBED_MOTION keyword) will override a Fixed Support or a Simple
              Support or a Fixed Rotation boundary condition (implemented with the *BOUNDARY_SPC
              keyword). Hence if a body has a Velocity constraint and a Fixed Support applied to it,
              the whole body will move in the direction of the applied velocity.
        •     The default unconstrained body is valid. It is not a requirement to constrain any DOF of
              a body In Explicit Dynamics systems.
        •     • An Explicit Dynamics solve can be performed if the model contains at least one Initial
              Condition (Translational or Rotational velocity) or a non-zero constraint (displacement
              or velocity) or a valid load.

Solve

            Basic general information about this topic

             ... for this analysis type:

        •     Solution output
              –   The Solution Information object provides a summary of the solution time increments
                  and progress is continuously updated in the solution output. Histograms of time
                  step, energy and momentum are also available for real time monitoring of solution
                  progress.
              –   Choose Tools> Solve Process Settings to solve in the background either locally or
                  remotely. Retrieve results while the analysis is running to get immediate feedback
                  on progress and accuracy of the solution.

                       Note

                       If you choose the My Computer, Background setting, it is necessary that
                       you also click the Advanced... button and check Use Shared License, if
                       possible, to obtain a successful solution.


        •     Result Tracker




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              29
The Mechanical Application Approach

              –   Full transient time history data can be viewed after the insertion of Result Tracker
                  objects. Body averaged data such as momentum and energy can be selected for
                  display. Data at a specific location (position, velocity, stress etc) can also be displayed.
              –   The frequency at which Result Tracker information is provided is defined in the
                  Save Result Tracker Data On option of the analysis settings.
        •     Solve an Explicit Dynamics (LS-DYNA Export) system to produce the LS-DYNA keyword
              file. This can be used to directly solve with the LS-DYNA solver, outside of the Workbench
              environment.

Review Results

            Basic general information about this topic

             ... for this analysis type:

        •     The following structural result types are available as results of an explicit dynamic ana-
              lysis:
              – Deformation (p. 341)
              –   Stress and Strain (p. 342)
              –   Energy (p. 353)
              –   Stress Tools (p. 354)
              –   Structural Probes (p. 366) - Limited to: Deformation, Strain, Stress, Position, Velocity,
                  Acceleration.
        •     Once a solution is available you can display contour results or animate them to review
              the response of the structure through time.

                   Note

                   For an explicit dynamics analysis, there is no results interpolation between
                   the results sets. Specifying a time in the GUI will display results for the closest
                   results set.


        •     Eroded nodes can be toggled on or off in the graphics display.
        •     Probes can be used to display the variation in specific results over the saved time points
              in the analysis. The frequency at which data is available is defined in the Save Results
              On option of the analysis settings. This data should be specified prior to a solve.
        •     You can use a Solution Information object to track, monitor, or diagnose problems
              that arise during a solution.
        •     Additional results specific to an explicit dynamics analysis are available via User Defined
              Results for Explicit Dynamics Analyses (p. 412).
        •     The Explicit Dynamics (LS-DYNA Export) system does not support the ability to review
              the results of a simulation using the LS-DYNA solver. Nevertheless results can be viewed
              with the lsprepost.exe application available at the ANSYS installation folder under
              ANSYS Inc\v120\ansys\bin\.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
30                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

Harmonic Response Analysis
Introduction
In a structural system, any sustained cyclic load will produce a sustained cyclic or harmonic response. Har-
monic analysis results are used to determine the steady-state response of a linear structure to loads that
vary sinusoidally (harmonically) with time, thus enabling you to verify whether or not your designs will
successfully overcome resonance, fatigue, and other harmful effects of forced vibrations.

This analysis technique calculates only the steady-state, forced vibrations of a structure. The transient vibra-
tions, which occur at the beginning of the excitation, are not accounted for in a harmonic response analysis.

In this analysis all loads as well as the structure’s response vary sinusoidally at the same frequency. A typical
harmonic analysis will calculate the response of the structure to cyclic loads over a frequency range (a sine
sweep) and obtain a graph of some response quantity (usually displacements) versus frequency. “Peak” re-
sponses are then identified from graphs of response vs. frequency and stresses are then reviewed at those
peak frequencies.

Points to Remember
Harmonic response analysis is a linear analysis. Some nonlinearities, such as plasticity will be ignored, even
if they are defined.

All loads and displacements vary sinusoidally at the same known frequency (although not necessarily in
phase).

If the reference temperature is set by body and that temperature doesn't match the environment temperature,
a thermally induced harmonic load will result (from the thermal strain assuming a non-zero thermal expansion
coefficient).

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

       From the Toolbox, drag the Harmonic Response template to the Project Schematic.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

       Both Young’s modulus (or stiffness in some form) and density (or mass in some form) must
       be defined. Material properties must be linear but can be isotropic or orthotropic, and constant
       or temperature-dependent. Nonlinear properties, if any, are ignored.

Attach Geometry

          Basic general information about this topic

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              31
The Mechanical Application Approach


             ... for this analysis type:

       There are no specific considerations for a harmonic response analysis.

Define Part Behavior

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a harmonic response analysis.

Define Connections

            Basic general information about this topic

             ... for this analysis type:

       Any nonlinear contact such as Frictional contact retains the initial status throughout the
       harmonic response analysis. The stiffness contribution from the contact is based on the initial
       status and never changes.

       Joints are not allowed in a harmonic response analysis.

       The stiffness as well as damping of springs is taken into account in a Full method of harmonic
       response analysis. In a Mode Superposition harmonic response analysis, the damping from
       springs is ignored.

Apply Mesh Controls/Preview Mesh

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for harmonic response analysis.

Establish Analysis Settings

            Basic general information about this topic

             ... for this analysis type:

       For a harmonic response analysis the basic controls are:

        •     Options - Here you specify the frequency range and the number of solution points at
              which the harmonic analysis will be carried out as well as the solution method to use
              and the relevant controls.

              Two solution methods are available to perform harmonic response analysis: the Mode
              Superposition method and the Direct Integration (full) method.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
32                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Preparing the Analysis

–   Mode Superposition method: In this method a modal analysis is first performed to
    compute the natural frequencies and mode shapes. Then the mode superposition
    solution is carried out where these mode shapes are combined to arrive at a solution.

    This is the default method, and generally provides results faster than the Full method.
    The Mode Superposition method cannot be used if you need to apply imposed
    (nonzero) displacements. This method also allows solutions to be clustered about
    the structure's natural frequencies. This results in a smoother, more accurate tracing
    of the response curve. The default method of equally spaced frequency points can
    result in missing the peak values.

    Without Cluster Option:




    With Cluster Option:




    A Store Results At All Frequencies option is also available to request that only
    minimal data be retained to supply just the harmonic results requested at the time
    of solution.


         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              33
The Mechanical Application Approach


                       Note

                       With this option set to No, the addition of new frequency responses to a
                       solved environment requires a new solution. The addition of new contour
                       results or phase responses does not share this requirement; data from the
                       closest available frequency is displayed (the reported frequency is noted
                       on each result). However, data at an even closer frequency may be ob-
                       tained with a new solution as needed.


              –   Full method: Calculates all displacements and stresses in a single pass. Its chief dis-
                  advantages are:
                  ¡ It is more “expensive” in CPU time than the Mode Superposition method.
                  ¡ It does not allow clustered results, but rather requires the results to be evenly
                    spaced within the specified frequency range.
        •     Damping Controls allow you to specify damping for the structure in the harmonic re-
              sponse analysis. Alpha and Beta damping as well as constant damping ratio are available
              for a harmonic response analysis. In addition material dependent damping can also be
              applied using the Engineering Data workspace.
              –   Constant Damping Ratio: The simplest way of specifying damping in the structure,
                  this value is a constant damping ratio.
              –   Beta Damping: Defines a stiffness matrix multiplier for damping. Beta Damping is
                  the option for Direct Input or Damping versus Frequency. For Direct Input, enter
                  a Beta Damping value. For Damping versus Frequency, you can enter both a Fre-
                  quency value and a Beta Damping value.
              –   Material Damping: Two types of material-based damping, Material Dependent
                  Damping and Constant Material Damping Coefficient are available for use with
                  harmonic analyses. These are defined as material properties in Engineering Data. The
                  Constant Material Damping Coefficient is used only in a Full method harmonic
                  analysis.
              –   Element Damping: You can also apply damping through spring-damper elements.
                  The damping from these elements is used only in a Full method harmonic analysis.

                   Note

                   If multiple damping specifications are made the effect is cumulative.


        •     Analysis Data Management settings enable you to save solution files from the harmonic
              response analysis. The default behavior is to only keep the files required for postpro-
              cessing. You can use these controls to keep all files created during solution or to create
              and save the Mechanical APDL application database (db file).

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
34                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Preparing the Analysis

      Initial condition is not applicable for Harmonic Response analyses.

Apply Loads and Supports

           Basic general information about this topic

            ... for this analysis type:

      The following loads are allowed in a harmonic response analysis:

       •     Acceleration (p. 280)
       •     Pressure (p. 284)
       •     Force (p. 285) (applied to a face, edge, or vertex)
       •     Bearing Load (p. 288)
       •     Moment (p. 291)
       •     Given (Specified) Displacement
       •     Remote Force
       •     Remote Displacement (p. 333)
       •     Line Pressure (p. 293)

      In a harmonic response analysis the loads have the following restrictions:

       •     All loads must be sinusoidally time-varying.
       •     All loads must have the same frequency.
       •     Loads can be out of phase with each other. You can specify a phase shift using the
             Phase Angle Details view entry for each load. You can specify the preferred unit for
             phase angle (in fact all angular inputs) to be degrees or radians using the Units toolbar.
       •     Thermal Condition is not supported.
       •     Any type of linear Support can be used in harmonic response analyses. The Compression
             Only support is nonlinear but will behave linearly in harmonic response analyses similar
             to a Frictionless Support, so it should not be utilized in order to avoid confusion.
       •     Pressure loads and Force loads can be applied, with magnitude and phase angle input.
             Line Pressure loads allow magnitude input but no phase angle input.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                              35
The Mechanical Application Approach




               Remote Force, Moment, and Acceleration loads may be defined, although these loads
               are assumed to act at a phase angle of zero.
         •     The Bearing Load, as shown below, acts on one side of the cylinder.




               In harmonic response analyses, you may expect that the other side of the cylinder is
               loaded in reverse, but the applied load simply reverses sign (goes in tension). Therefore
               the use of Bearing Loads is not recommended.

Solve

             Basic general information about this topic

              ... for this analysis type:

        Solution Information continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis.

Review Results

             Basic general information about this topic

              ... for this analysis type:

        Two type of results can be requested for harmonic response analyses: Contour plots of results
        at a particular frequency and phase angle or graphs.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
36                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Preparing the Analysis

Contour plots include stress, elastic strain, and deformation, and are basically the same as
those for other analyses. For these results, you must specify a frequency and phase angle.

The following demo is presented as an animated GIF. Please view online if you are reading the
PDF version of the help. Interface names and other components shown in the demo may differ
from those in the released product.




Graphs can be either Frequency Response graphs that display how the response varies with
frequency or Phase Response plots that show how much a response lags behind the applied
loads. Results displayed on a graph can be scoped to specific geometric entity (vertex, face,
or edge) and can be viewed as a value graphed along a specified frequency range. These
include the frequency or phase results for stress, elastic strain, deformation, or acceleration
(frequency only) plotted as a graph. The plot will include all the frequency points at which
a solution was obtained. When you generate frequency response results, the default plot
(Bode) shows the amplitude. For phase response results, there is only one graph shown and
there are no display options for them. The following figure shows a reduced version of the
Bode plot.




Optionally, you can plot the following results values for graphs: real, imaginary, amplitude,
and phase angle. You can select any of these from a drop-down list in the Details view for
the results. For edges, faces, surface bodies, and multiple vertex selections (which contain
multiple nodes), the results can be scoped as minimum, maximum, or average. This is also
available for frequency and phase response results scoped on a single vertex.

The Use Minimum and Use Maximum settings are based on the amplitude and thus are
reported from the location with either the largest or smallest amplitude. The Use Average
setting calculates the average by calculating the real and imaginary components separately.



              Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                          of ANSYS, Inc. and its subsidiaries and affiliates.                                              37
The Mechanical Application Approach


            Note

            You cannot use the Mechanical application convergence capabilities for any results
            item under a harmonic response analysis. Instead, you can first do a convergence
            study on a modal analysis and reuse the mesh from that analysis.

       The Reported Frequency in the Information category is the frequency at which contour
       results were found and plotted. This frequency can be potentially different from the frequency
       you requested.

       General approach to harmonic analysis postprocessing

       Generally speaking, you would look at Frequency Response plots at critical regions to ascer-
       tain what the frequency of interest may be. In conjunction with Phase Response plots, the
       phase of interest is also determined. Then, you can request Stress, Strain, or Deformation
       contour plots to evaluate the response of the entire structure at that frequency and phase
       of interest.

       Presented below is an example of a Frequency Response plot:




       The average, minimum, or maximum value can be chosen for selected entities. Stress, Strain,
       Deformation, and Acceleration components vary sinusoidally, so these are the only result
       types that can be reviewed in this manner. (Note that items such as Principal Stress or
       Equivalent Stress do not behave in a sinusoidal manner since these are derived quantities.)

       Similarly, Phase Response plots show the minimum, average, or maximum Stress, Strain,
       or Deformation for selected entities. Presented below is an example of a Phase Response
       plot.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
38                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Introduction




       However, unlike Frequency Response plots that show a response amplitude over a frequency
       range, Phase Response plots show a response over a range of phase angles, so you can
       determine how much a response lags behind the applied load.

       For contour results, you must specify the frequency and phase angle of interest, as noted
       above. All types of Stress, Strain, and Deformation are available, including derived quantities
       such as Total Deformation or Equivalent (von-Mises) Stress. You can then see the total
       response of the structure at a given point in time, as shown below.




       Since each node may have different phase angles from one another, the complex response
       can also be animated to see the time-dependent motion.

Linear Buckling Analysis
Introduction
Linear buckling (also called as Eigenvalue buckling) analysis predicts the theoretical buckling strength of an
ideal elastic structure. This method corresponds to the textbook approach to elastic buckling analysis: for
instance, an eigenvalue buckling analysis of a column will match the classical Euler solution. However, im-
perfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic
buckling strength. Thus, linear buckling analysis often yields quick but non-conservative results.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                        39
The Mechanical Application Approach

F                                                                        F
              Snap-through

              buckling
                                                                                                         Bifurcation point



                                                                                                        Limit load (from

                                                                                                        nonlinear buckling)




                                                        u                                                                              u

                   (a)                                                                                 (b)



(a) Nonlinear load-deflection curve, (b) Linear (Eigenvalue) buckling curve

A more accurate approach to predicting instability is to perform a nonlinear buckling analysis. This involves
a static structural analysis with large deflection effects turned on. A gradually increasing load is applied in
this analysis to seek the load level at which your structure becomes unstable. Using the nonlinear technique,
your model can include features such as initial imperfections, plastic behavior, gaps, and large-deflection
response. In addition, using deflection-controlled loading, you can even track the post-buckled performance
of your structure (which can be useful in cases where the structure buckles into a stable configuration, such
as "snap-through" buckling of a shallow dome).

Points to Remember
 •   Linear buckling analysis must be preceded by a static structural analysis.
 •   The results calculated by the linear buckling analysis are buckling load factors that scale the loads applied
     in the static structural analysis. Thus for example if you applied a 10 N compressive load on a structure
     in the static analysis and if the linear buckling analysis calculates a load factor of 1500, then the predicted
     buckling load is 1500x10 = 15000 N. Because of this it is typical to apply unit loads in the static analysis
     that precedes the buckling analysis.
 •   The buckling load factor is to be applied to all the loads used in the static analysis.
 •   A structure can have infinitely many buckling load factors. Each load factor is associated with a different
     instability pattern. Typically the lowest load factor is of interest.
 •   Only linear behavior is valid. If your model includes contact connections, for example, their effects are
     calculated based on their status at the beginning of the static analysis.
 •   Note that the load factors represent scaling factors for all loads. If certain loads are constant (for example,
     self-weight gravity loads) while other loads are variable (for example, externally applied loads), you
     need to take special steps to ensure accurate results.

     One strategy that you can use to achieve this end is to iterate on the linear buckling solution, adjusting
     the variable loads until the load factor becomes 1.0 (or nearly 1.0, within some convergence tolerance).

     Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To
     determine the limiting value of A in a linear buckling analysis, you could solve repetitively, using different
     values of A, until by iteration you find a load factor acceptably close to 1.0.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
40                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis




•   You can apply a nonzero constraint in the static analysis. The load factors calculated in the buckling
    analysis should also be applied to these nonzero constraint values. However, the buckling mode shape
    associated with this load will show the constraint to have zero value.
•   Buckling mode shape displays are helpful in understanding how a part or an assembly deforms when
    buckling, but do not represent actual displacements.

Preparing the Analysis
Create Analysis System

            Basic general information about this topic

             ... for this analysis type:

       From the Toolbox, drag the Linear Buckling template to the Project Schematic.

Define Engineering Data

            Basic general information about this topic

             ... for this analysis type:

        •     Young's modulus (or stiffness in some form) must be defined.
        •     Material properties can be linear, isotropic or orthotropic, and constant or temperature-
              dependent.
        •     Nonlinear properties, if any, are ignored.

Attach Geometry

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a linear buckling analysis.

Define Part Behavior

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a linear buckling analysis.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              41
The Mechanical Application Approach

Define Connections

            Basic general information about this topic

             ... for this analysis type:

       Remember that a linear buckling analysis uses the model and connections from a linear
       static analysis. Only linear behavior is valid in a linear buckling analysis. If your model includes
       contact regions, for example, the effect of these contact regions are calculated based on
       their status at the end of the static analysis.

       Joints and springs are taken into account if they are present in the static analysis.

Apply Mesh Controls/Preview Mesh

            Basic general information about this topic

             ... for this analysis type:

       There are no considerations specifically for a linear buckling analysis.

Establish Analysis Settings

            Basic general information about this topic

             ... for this analysis type:

       For linear buckling analysis the basic controls are:

       Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Ana-
       lyses (p. 273): Number of Modes: You need to specify the number of buckling load factors
       and corresponding buckling mode shapes of interest. Typically the first (lowest) buckling
       load factor is of interest.

       Output Controls (p. 270): By default only buckling load factors and corresponding buckling
       mode shapes are calculated. You can request Stress and Strain results to be calculated but
       note that “stress” results only show the relative distribution of stress in the structure and are
       not real stress values.

       In Analysis Data Management (p. 277), users can set the save the Mechanical APDL application
       database and delete unneeded file settings.

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

       You must point to a static structural analysis of the same model in the initial condition envir-
       onment.

        •     Linear buckling analysis must be preceded by a static structural analysis.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
42                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Preparing the Analysis

         •     If the static structural analysis has multiple result sets, the values from the last solve
               point are used as the basis for the linear buckling analysis.
         •     The results calculated by the linear buckling analysis are buckling load factors that scale
               the loads applied in the static structural analysis. Thus for example if you applied a 10
               N compressive load on a structure in the static analysis and if the linear buckling analysis
               calculates a load factor of 1500, then the predicted buckling load is 1500x10 = 15000
               N. Because of this it is typical to apply unit loads in the static analysis that precedes the
               buckling analysis.
         •     The buckling load factor is to be applied to all the loads used in the static analysis.

Apply Loads and Supports

             Basic general information about this topic

              ... for this analysis type:

        No loads are allowed in the linear buckling analysis. The supports as well as the stress state
        from the static structural analysis are used in the linear buckling analysis.

               Note

               If the static analysis has a pressure load applied “normal to” faces (3-D) or edges
               (2-D), this could result in an additional stiffness contribution called the “pressure
               load stiffness” effect. This effect plays a significant role in linear buckling analyses.
               This additional effect is computed during a buckling analysis using the pressure
               value in the static analysis at time = 0. Because of this if the static analysis is to
               be used for a subsequent buckling analysis you should step apply any pressure
               loads in the static analysis.

               Different buckling loads may be predicted from seemingly equivalent pressure
               and force loads in a buckling analysis because in the Mechanical application a
               force and a pressure are not treated the same. As with any numerical analysis, we
               recommend that you use the type of loading which best models the in-service
               component. For more information, see the Theory Reference for the Mechanical
               application, under Structures with Geometric Nonlinearities> Stress Stiffening> Pressure
               Load Stiffness.

Solve

             Basic general information about this topic

              ... for this analysis type:

        Solution Information continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis.

Review Results

             Basic general information about this topic

              ... for this analysis type:

                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              43
The Mechanical Application Approach

        You can view the buckling mode shape associated with a particular load factor by displaying
        a contour plot or by animating the deformed mode shape. The contours represent relative
        displacement of the part.

        Buckling mode shape displays are helpful in understanding how a part or an assembly deforms
        when buckling, but do not represent actual displacements.

        “Stresses” from a modal analysis do not represent actual stresses in the structure, but give
        you an idea of the relative stress distributions for each mode. Stress and Strain results are
        available only if requested before solution using Output Controls (p. 270).

Magnetostatic Analysis
Introduction
Magnetic fields may exist as a result of a current or a permanent magnet. In the Mechanical application you
can perform 3-D static magnetic field analysis. You can model various physical regions including iron, air,
permanent magnets, and conductors.

Typical uses for a magnetostatic analysis are as follows:

 •   Electric machines
 •   Transformers
 •   Induction heating
 •   Solenoid actuators
 •   High-field magnets
 •   Nondestructive testing
 •   Magnetic stirring
 •   Electrolyzing cells
 •   Particle accelerators
 •   Medical and geophysical instruments.

Points to Remember
 •   This analysis is applicable only to 3-D geometry.
 •   The geometry must consist of a single solid multibody part.
 •   A magnetic field simulation requires that air surrounding the physical geometry be modeled as part of
     the overall geometry. The air domain can be easily modeled in DesignModeler using the Enclosure
     feature. Ensure that the resulting model is a single multibody part which includes the physical geometry
     and the air.
 •   In many cases, only a symmetric portion of a magnetic device is required for simulation. The geometry
     can either be modeled in full symmetry in the CAD system, or in partial symmetry. DesignModeler has
     a Symmetry feature that can slice a full symmetry model, or identify planes of symmetry for a partial
     symmetry model. This information is passed to the Mechanical application for convenient application
     of symmetry plane boundary conditions.
 •   A Magnetostatic analysis supports a mulit-step solution.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
44                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

Preparing the Analysis
Create Analysis System

            Basic general information about this topic

             ... for this analysis type:

From the Toolbox, drag the Magnetostatic template to the Project Schematic.

Define Engineering Data

            Basic general information about this topic

             ... for this analysis type:

        •     Magnetic field simulation support 4 categories of material properties:
              1.   Linear “soft” magnetic materials - typically used in low saturation cases. A Relative
                   Permeability is required. This may be constant, or orthotropic with respect to the
                   coordinate system of the body (See Details view). Orthotropic properties are often
                   used to simulate laminate materials.
              2.   Linear “hard” magnetic materials - used to model permanent magnets. The demag-
                   netization curve of the magnet is assumed to be linear. Residual Induction and
                   Coercive Force are required.
              3.   Nonlinear “soft” magnetic material - used to model devices which undergo magnetic
                   saturation. A B-H curve is required. For orthotropic materials, you can assign the B-
                   H curve in any of the orthotropic directions, while specifying a constant Relative
                   Permeability in the other directions. (Specifying a value of “0” for Relative Per-
                   meability will make use of the B-H curve in that direction.)
              4.   Nonlinear “hard” magnetic material - used to model nonlinear permanent magnets.
                   A B-H curve modeling the material demagnetization curve is required.
        •     When an Emag license is being used only the following material properties are allowed:
              Isotropic Resistivity, Orthotropic Resistivity, Relative Permeability, Relative Permeability
              (Orthotropic), Coercive Force & Residual Induction, B-H Curve, B-H Curve (Orthotropic),
              Demagnetization B-H Curve. You may have to turn the filter off in the Engineering Data
              workspace to suppress or delete those material properties/models which are not suppor-
              ted for this license.
        •     Conductor bodies require a Resistivity material property. Solid source conductor bodies
              can be constant or orthotropic with respect to the coordinate system of the body.
              Stranded source conductor bodies can only be modeled as isotropic materials.
        •     For convenience, a library of common B-H curves for soft magnetic material is supplied
              with the product. Use the Import tool in Engineering Data to review and retrieve curves
              for use.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              45
The Mechanical Application Approach


              Note

              In a magnetostatic analysis, you can orient a polarization axis for a Linear or
              Nonlinear Hard material in either the positive or negative x direction with respect
              to a local or global coordinate system. Use the Material Polarization setting in
              the Details view for each body to establish this direction. The Material Polarization
              setting appears only if a hard material property is defined for the body. For a cyl-
              indrical coordinate system, a positive x polarization is in the positive radial direction,
              and a negative x polarization is in the negative radial direction.

Attach Geometry

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a magnetostatic analysis.

Define Part Behavior

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a magnetostatic analysis.

Define Connections

            Basic general information about this topic

             ... for this analysis type:

       Connections are not supported in a magnetostatic analysis.

Apply Mesh Controls/Preview Mesh

            Basic general information about this topic

             ... for this analysis type:

        •     Although your body is automatically meshed at solve time, it is recommended that you
              select the Electromagnetic Physics Preference in the Details view of the Mesh object
              folder.
        •     Solution accuracy is dependent on mesh density. Accurate force or torque calculations
              require a fine mesh in the air regions surrounding the bodies of interest.
        •     The use of pyramid elements in critical regions should be minimized. Pyramid elements
              are used to transition from hexagonal to tetrahedral elements. You can eliminate pyramid
              elements from the model by specifying Tetrahedrons using a Method mesh control
              tool.

Establish Analysis Settings

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
46                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis


            Basic general information about this topic

             ... for this analysis type:

       The basic controls are:

       Step Controls (p. 266): used to specify the end time of a step in a single or multiple step ana-
       lysis.

       Multiple steps are needed if you want to change load values, the solution settings, or the
       solution output frequency over specific steps. Typically you do not need to change the default
       values.

       Solver Controls (p. 271) allow you to select either a direct or iterative solver. By default the
       program will use the direct solver. Convergence is guaranteed with the direct solver. Use the
       Iterative solver only in cases where machine memory is an issue. The solution is not guaranteed
       to converge for the iterative solver.

       Nonlinear Controls (p. 269) allow you to modify convergence criteria and other specialized
       solution controls. These controls are used when your solution is nonlinear such as with the
       use of nonlinear material properties (B-H curve). Typically you will not need to change the
       default values for this control. CSG convergence is the criteria used to converge the magnetic
       field. CSG represents magnetic flux. AMPS convergence is only used for temperature-dependent
       electric current conduction for solid conductor bodies. AMPS represents current.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. A multi-step analysis involves calculating solutions at several
       time points in the load history. However you may not be interested in all of the possible
       results items and writing all the results can make the result file size unwieldy. You can restrict
       the amount of output by requesting results only at certain time points or limit the results
       that go onto the results file at each time point.

       Analysis Data Management (p. 277) settings enable you to save solution files from the mag-
       netostatic analysis. The default behavior is to only keep the files required for postprocessing.
       You can use these controls to keep all files created during solution or to create and save the
       Mechanical APDL application database (db file).

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

       There is no initial condition specification for a magnetostatic analysis.

Apply Loads and Supports

            Basic general information about this topic

             ... for this analysis type:

        •     You can apply electromagnetic boundary conditions and excitations in the Mechanical
              application. See Electromagnetic Boundary Conditions and Excitations (p. 305) for details.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              47
The Mechanical Application Approach

         •     Boundary conditions may also be applied on symmetry planes via a Symmetry folder.
               A Symmetry folder allows support for symmetry, anti-symmetry, and periodic conditions.

Solve

             Basic general information about this topic

              ... for this analysis type:

        The Solution Information object provides some tools to monitor solution progress in the
        case of a nonlinear magnetostatic analysis.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

        Adaptive mesh refinement is available for magnetostatic analyses.

Review Results

             Basic general information about this topic

              ... for this analysis type:

        A magnetostatic analysis offers several results for viewing. Results may be scoped to bodies
        and, by default, all bodies will compute results for display. For Inductance or Flux Linkage,
        define these objects prior to solution. If you define these after a solution, you will need to
        re-solve.

Modal Analysis
Introduction
A modal analysis determines the vibration characteristics (natural frequencies and mode shapes) of a structure
or a machine component. It can also serve as a starting point for another, more detailed, dynamic analysis,
such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis. The natural fre-
quencies and mode shapes are important parameters in the design of a structure for dynamic loading con-
ditions. You can also perform a modal analysis on a prestressed structure, such as a spinning turbine blade.

A modal analysis can be performed using the ANSYS or SAMCEF solver. Any differences are noted in the
sections below.

Points to Remember
 •   Damping is ignored in a modal analysis.
 •   Any applied loads are ignored.
 •   Prestressed modal analysis requires performing a static structural analysis first. In the modal analysis
     you can use the Initial Condition object to point to the Static Structural analysis to include prestress
     effects.
 •   If the analysis is a pre-stress modal analysis and your model includes contact connections, their effects
     are calculated based on their status at the beginning of the static analysis. Commands objects can be

                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
48                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis

    added if a different behavior is required. See Prestressed Modal Analysis in the Structural Analysis Guide
    for more information.

Preparing the Analysis
Create Analysis System

         Basic general information about this topic

          ... for this analysis type:

       From the Toolbox, drag a Modal (ANSYS) or a Modal (SAMCEF) template to the Project
       Schematic.

Define Engineering Data

         Basic general information about this topic

          ... for this analysis type:

       Due to the nature of modal analyses any nonlinearities in material behavior are ignored.
       Optionally, orthotropic and temperature-dependent material properties may be used. The
       critical requirement is to define stiffness as well as mass in some form. Stiffness may be
       specified using isotropic and orthotropic elastic material models (for example, Young's
       modulus and Poisson's ratio), using hyperelastic material models (they are linearized to an
       equivalent combination of initial bulk and shear moduli), or using spring constants, for ex-
       ample. Mass may derive from material density or from remote masses.

Attach Geometry

         Basic general information about this topic

          ... for this analysis type:

       When 2D geometry is used, only the 2D axisymmetric behavior is available for SAMCEF
       solvers.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for a modal analysis.

Define Connections

         Basic general information about this topic

          ... for this analysis type:



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              49
The Mechanical Application Approach

        •     Any nonlinear contact such as Frictional contact retains the initial status throughout
              the modal analysis. The stiffness contribution from the contact is based on the initial
              status and never changes.
        •     Joints are allowed in a modal analysis. They restrain degrees of freedom as defined by
              the joint definition.
        •     The stiffness of any spring is taken into account, however any damping specified is ig-
              nored.
        •     For the SAMCEF solver, only contacts, springs, and beams are supported. Joints are not
              supported.

Apply Mesh Controls/Preview Mesh

            Basic general information about this topic

             ... for this analysis type:

       There are no special considerations for this analysis type.

Establish Analysis Settings

            Basic general information about this topic

             ... for this analysis type:

       Number of Modes: You need to specify the number of frequencies of interest. The default is
       to extract the first 6 natural frequencies. The number of frequencies can be specified in two
       ways:

        1.     The first N frequencies (N > 0), or
        2.     The first N frequencies in a selected range of frequencies.

       Solver Type (p. 271)(applicable to Modal (ANSYS) systems only): Typically you should let the
       program choose the type of solver appropriate for your model.

       Output Controls (p. 270): By default only mode shapes are calculated. You can request Stress
       and Strain results to be calculated but note that “stress” results only show the relative distri-
       bution of stress in the structure and are not real stress values.

       Analysis Data Management (p. 277) (applicable to Modal (ANSYS) systems only) settings enable
       you to save specific solution files from the Modal analysis for use in other analyses. You can
       set the Future Analysis field to PSD/RS Analyses if you intend to use the modal results in
       a subsequent Modal, Random Vibration (PSD), or Response Spectrum (RS) analysis. When
       a PSD or RS analysis is linked to a modal analysis, additional solver files must be saved to
       achieve the PSD or RS solution. If the files were not saved, then the modal analysis has to
       be solved again and the files saved.

              Note

              Solver Type, Scratch Solver Files..., Save ANSYS db, Solver Units, and Solver
              Unit System are applicable to Modal (ANSYS) systems only.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
50                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

Define Initial Conditions

          Basic general information about this topic

           ... for this analysis type:

        You can point to a Static Structural analysis in the Initial Condition environment field if
        you want to include prestress effects. A typical example is the large tensile stress induced in
        a turbine blade under centrifugal load that can be captured by a static structural analysis.
        This causes significant stiffening of the blade. Including this prestress effect will result in
        much higher, realistic natural frequencies in a modal analysis.

             Note

             When you perform a prestressed modal analysis, the support conditions from the
             static analysis are used in the modal analysis. You cannot apply any new supports
             in the modal analysis portion of a prestressed modal analysis.

Apply Loads and Supports

          Basic general information about this topic

           ... for this analysis type:

        No loads are allowed in the modal analysis. All structural supports can be applied except the
        Non-zero Displacement and the Velocity boundary condition. Due to their nonlinear nature,
        compression only supports are not recommended in a modal analysis. Use of compression
        only supports may result in extraneous or missed natural frequencies.

        For the SAMCEF solver, the following supports are not available: Compression Only Support,
        Elastic Support.

             Note

             Pre-stressed Modal Analysis: In a pre-stressed modal analysis any structural
             supports used in the static analysis persist. Therefore, you are not allowed to add
             new supports in the pre-stressed modal analysis.

Solve

          Basic general information about this topic

           ... for this analysis type:

        Solution Information continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis.

Review Results

          Basic general information about this topic


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              51
The Mechanical Application Approach


           ... for this analysis type:

        Highlight the Solution object in the tree to view a bar chart of the frequencies obtained in
        the modal analysis. A tabular data grid is also displayed that shows the list of frequencies.

        You can choose to review the mode shapes corresponding to any of these natural frequencies
        by selecting the frequency from the bar chart or tabular data and using the context sensitive
        menu (right mouse click) to choose Create Mode Shape Results. You can also view a range
        of mode shapes.

        You can view the mode shape associated with a particular frequency as a contour plot. You
        can also animate the deformed shape. The contours represent relative displacement of the
        part as it vibrates.

        Mode shape pictures are helpful in understanding how a part or an assembly vibrates, but
        do not represent actual displacements. If there are structural loads present in the environment,
        then the frequencies and mode shapes will depend on the loads and their magnitudes.

Random Vibration Analysis
Introduction
This analysis enables you to determine the response of structures to vibration loads that are random in
nature. An example would be the response of a sensitive electronic component mounted in a car subjected
to the vibration from the engine, pavement roughness, and acoustic pressure.

Loads such as the acceleration caused by the pavement roughness are not deterministic, that is, the time
history of the load is unique every time the car runs over the same stretch of road. Hence it is not possible
to predict precisely the value of the load at a point in its time history. Such load histories, however, can be
characterized statistically (mean, root mean square, standard deviation). Also random loads are non-periodic
and contain a multitude of frequencies. The frequency content of the time history (spectrum) is captured
along with the statistics and used as the load in the random vibration analysis. This spectrum, for historical
reasons, is called Power Spectral Density or PSD.

In a random vibration analysis since the input excitations are statistical in nature, so are the output responses
such as displacements, stresses, and so on.

Typical applications include aerospace and electronic packaging components subject to engine vibration,
turbulence and acoustic pressures, tall buildings under wind load, structures subject to earthquakes, and
ocean wave loading on offshore structures.

Points to Remember
 •   The excitation is applied in the form of Power Spectral Density (PSD). The PSD is a table of spectral
     values vs. frequency that captures the frequency content. The PSD captures the frequency and mean
     square amplitude content of the load’s time history.
 •   The square root of the area under a PSD curve represents the root mean square (rms) value of the ex-
     citation. The unit of the spectral value of acceleration, for example, is G2/Hertz.
 •   The input excitation is expected to be stationary (the average mean square value does not change with
     time) with a zero mean.
 •   This analysis is based on the mode superposition method. Hence a modal analysis that extracts the
     natural frequencies and mode shapes is a prerequisite.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
52                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

•   This feature covers one type of PSD excitation only- base excitation.
•   The base excitation could be an acceleration PSD (either in acceleration2 units or in G2 units), velocity
    PSD or displacement PSD.
•   The base excitation is applied in the specified direction to all entities that have a Fixed Support
    boundary condition. Other support points in a structure such as Frictionless Surface are not excited
    by the PSD.
•   Multiple uncorrelated PSDs can be applied. This is useful if different, simultaneous excitations occur in
    different directions.
•   If stress/strain results are of interest from the random vibration analysis then you will need to request
    stress/strain calculations in the modal analysis itself. Only displacement results are available by default.
•   Postprocessing:
    –   The results output by the solver are one sigma or one standard deviation values (with zero mean
        value). These results follow a Gaussian distribution. The interpretation is that 68.3% of the time the
        response will be less than the standard deviation value.
    –   You can scale the result by 2 times to get the 2 sigma values. The response will be less than the 2
        sigma values 95.91% of the time and 3 sigma values 99.737% of the time.
    –   The Coordinate System setting for result objects is, by default, set to Solution Coordinate System
        and cannot be changed because the results only have meaning when viewed in the solution coordin-
        ate system.
    –   Since the directional results from the solver are statistical in nature they cannot be combined in the
        usual way. For example the X, Y, and Z displacements cannot be combined to get the magnitude
        of the total displacement. The same holds true for other derived quantities such as principal stresses.
    –   A special algorithm by Segalman-Fulcher is used to compute a meaningful value for equivalent
        stress.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

        Because a random vibration analysis is based on modal responses, a modal analysis is a re-
        quired prerequisite. The requirement then is for two analysis systems, a modal analysis system
        and a random vibration analysis system that share resources, geometry, and model data.

        From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Random
        Vibration template directly onto the Modal template.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              53
The Mechanical Application Approach

       Both Young’s modulus (or stiffness in some form) and density (or mass in some form) must
       be defined in the modal analysis. Material properties must be linear but can be isotropic or
       orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.

Attach Geometry

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for a random vibration analysis.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for a random vibration analysis.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       Only linear behavior is valid in a random vibration analysis. Nonlinear elements, if any, are
       treated as linear. If you include contact elements, for example, their stiffnesses are calculated
       based on their initial status and are never changed.

       Joints are not allowed in a random vibration analysis.

       Only the stiffness of springs are taken into account in a random vibration analysis.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for a random vibration analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For a random vibration analysis the basic controls are:

       Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Ana-
       lyses (p. 273). You can specify the number of modes to use from the modal analysis. A conser-
       vative rule of thumb is to include modes that cover 1.5 times the maximum frequency in the

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
54                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

       PSD excitation table. You can also exclude insignificant modes by setting a mode significance
       level between 0 (all modes selected) and 1 (no modes selected).

       Damping Controls (p. 276) allow you to specify damping for the structure in the random vibra-
       tion analysis. Alpha and Beta damping as well as constant damping ratio are available for a
       random vibration analysis. In addition material dependent damping can also be applied using
       the Engineering Data workspace.

       Analysis Data Management (p. 277) settings enable you to save solution files from the Random
       Vibration analysis. The default behavior is to only keep the files required for postprocessing.
       You can use these controls to keep all files created during solution or to create and save a
       the Mechanical APDL application database (db file).

              Note

              The Inertia Relief option (under Analysis Settings) for an upstream static struc-
              tural analysis is not supported in a random vibration analysis.

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

       You must point to a modal analysis in the Initial Condition environment field. The modal
       analysis must extract enough modes to cover the PSD frequency range. A conservative rule
       of thumb is to extract enough modes to cover 1.5 times the maximum frequency in the PSD
       excitation. When a PSD analysis is linked to a modal analysis, additional solver files must be
       saved to achieve the PSD solution. (See Analysis Data Management (p. 277).) If the files were
       not saved, then the modal analysis has to be solved again and the files saved.

Apply Loads and Supports

            Basic general information about this topic

             ... for this analysis type:

        •     Any support boundary condition must be defined in the modal analysis itself. You cannot
              add any new support boundary conditions in the random vibration analysis.
        •     The only applicable load is a PSD Base Excitation of spectral value vs. frequency.
        •     Remote displacement cannot coexist with other boundary condition types (for example,
              fixed support or displacement) on the same location for excitation. The remote displace-
              ment will be ignored due to conflict with other boundary conditions.
        •     Four types of base excitation are supported: PSD Acceleration, PSD G Acceleration,
              PSD Velocity, and PSD Displacement.
        •     Each PSD base excitation should be given a direction in the nodal coordinate of the ex-
              citation points.
        •     Multiple PSD excitations (uncorrelated) can be applied. Typical usage is to apply 3 different
              PSDs in the X, Y, and Z directions. Correlation between PSD excitations is not supported.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              55
The Mechanical Application Approach

Solve

             Basic general information about this topic

              ... for this analysis type:

        Solution Information continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis. In addition to
        solution progress you will also find the participation factors for each PSD excitation. The
        solver output also has a list of the relative importance of each mode in the modal covariance
        matrix listing.

Review Results

             Basic general information about this topic

              ... for this analysis type:

         •     If stress/strain results are of interest from the random vibration analysis then you will
               need to request stress/strain calculations in the modal analysis itself. You can use the
               Output Controls under Analysis Settings in the modal analysis for this purpose. Only
               displacement results are available by default.
         •     Applicable results are Directional (X/Y/Z) Displacement/Velocity/Acceleration, normal
               and shear stresses/strains and equivalent stress. These results can be displayed as contour
               plots.
         •     The displacement results are relative to the base of the structure (the fixed supports).
         •     The velocity and acceleration results include base motion effects (absolute).
         •     Since the directional results from the solver are statistical in nature they cannot be
               combined in the usual way. For example the X, Y, and Z displacements cannot be com-
               bined to get the magnitude of the total displacement. The same holds true for other
               derived quantities such as principal stresses.
         •     For directional acceleration results, an option is provided to displayed acceleration in G
               (gravity) by selecting Yes in the Acceleration in G field.
         •     By default the 1 σ results are displayed. You can apply a scale factor to review any mul-
               tiples of σ such as 2 σ or 3 σ. The Details view as well as the legend for contour results
               also reflects the percentage (using Gaussian distribution) of time the response is expected
               to be below the displayed values.
         •     Meaningful equivalent stress is computed using a special algorithm by Segalman-Fulcher.
               Note that the probability distribution for this equivalent stress is neither Gaussian nor
               is the mean value zero. However, the “3 σ” rule (multiplying the RMS value by 3) yields
               a conservative estimate on the upper bound of the equivalent stress.

Response Spectrum Analysis
Introduction
Response spectrum analyses are widely used in civil structure designs, for example, high-rise buildings under
wind loads. Another prime application is for nuclear power plant designs under seismic loads.



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
56                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

A response spectrum analysis has similarities to a random vibration analysis. However, unlike a random vi-
bration analysis, responses from a response spectrum analysis are deterministic maxima. For a given excitation,
the maximum response is calculated based upon the input response spectrum and the method used to
combine the modal responses. The combination methods available are: the Square Root of the Sum of the
Squares (SRSS), the Complete Quadratic Combination (CQC) and the Rosenblueth’s Double Sum Combination
(ROSE). See Response Spectrum - Options Control Settings (p. 276) for further details.

Points to Remember
 •   The excitation is applied in the form of a response spectrum. The response spectrum can have displace-
     ment, velocity or acceleration units. For each spectrum value, there is one corresponding frequency.
 •   The excitation must be applied at fixed degrees of freedom.
 •   The response spectrum is calculated based on modal responses. A modal analysis is therefore a pre-
     requisite.
 •   If response strain/stress is of interest, then the modal strain and the modal stress need to be determined
     in the modal analysis.
 •   Because a new solve is required for each requested output, for example, displacement, velocity and
     acceleration, the content of Commands objects inserted in a response spectrum analysis is limited to
     SOLUTION commands.
 •   The results from the ANSYS solver are displayed as the model’s contour plot. The results are in terms
     of the maximum response.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

        Because a response spectrum analysis is based on modal responses, a modal analysis is a
        required prerequisite. The modal analysis system and the response spectrum analysis system
        must share resources, geometry, and model data.

        From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Response
        Spectrum template directly onto the Modal template.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

        Material properties must be defined in a modal analysis. Nonlinear material properties are
        not allowed.

Attach Geometry

          Basic general information about this topic



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              57
The Mechanical Application Approach


             ... for this analysis type:

       There are no specific considerations for a response spectrum analysis.

Define Part Behavior

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a response spectrum analysis.

Define Connections

            Basic general information about this topic

             ... for this analysis type:

       Nonlinear element types are not supported. They will be treated as linear. For example, the
       contact stiffness is calculated using the initial status without convergence check.

Apply Mesh Controls/Preview Mesh

            Basic general information about this topic

             ... for this analysis type:

       There are no specific considerations for a response spectrum analysis.

Establish Analysis Settings

            Basic general information about this topic

             ... for this analysis type:

       Options for Response Spectrum Analyses:

        •     Specify the Number of Modes To Use for the response spectrum calculation. It is recom-
              mended to include the modes whose frequencies span 1.5 times the maximum frequency
              defined in the input response spectrum.
        •     Specify the Spectrum Type to be used for response spectrum calculation as either Single
              Point or Multiple Points. If the input response spectrum is applied to all fixed degrees
              of freedom, use Single Point, otherwise use Multiple Points.
        •     Specify the Modes Combination Type to be used for response spectrum calculation.
              In general, the SRSS method is more conservative than the CQC and the ROSE methods.

              Note

              The Inertia Relief option (under Analysis Settings) for an upstream static struc-
              tural analysis is not supported in a response spectrum analysis.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
58                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

       Output Controls (p. 270). By default, only displacement responses are calculated. To include
       velocity and/or acceleration responses, set their respective Output Controls to Yes.

       Damping Controls (p. 276) allow you to specify damping for the structure in the response
       spectrum analysis. For the CQC mode combination type, a non-zero constant damping ratio
       is required.

       Analysis Data Management (p. 277) settings enable you to save solution files from the response
       spectrum analysis. An option to save an the Mechanical APDL application database (db file)
       from the analysis is provided.

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

       A specific Modal Environment must be set as an initial condition/environment for response
       spectrum analysis to be solved.

Apply Loads and Supports

            Basic general information about this topic

             ... for this analysis type:

        •     Supported boundary condition types include fixed support, displacement, remote dis-
              placement and body-to-ground spring. If one or more fixed supports are defined in the
              model, the input excitation response can be applied to all fixed supports.
        •     Remote displacement cannot coexist with other boundary condition types (for example,
              fixed support or displacement) on the same location for excitation. The remote displace-
              ment will be ignored due to conflict with other boundary conditions.
        •     Note that the All boundary condition types for Single Point Response Spectrum only
              includes those fixed degree of freedoms defined using Fixed Support, Displacement,
              Remote Displacement and Body-to-Ground Spring. To apply an RS load to All boundary
              condition types for Single Point Response Spectrum, at least one allowed boundary
              condition must be defined.
        •     For a Single Point spectrum type, input excitation spectrums are applied to all boundary
              condition types defined in the model. For Multiple Points however, each input excitation
              spectrum is associated to only one boundary condition type.
        •     Three types of input excitation spectrum are supported: displacement input excitation
              (RS Displacement), velocity input excitation (RS Velocity) and acceleration input excit-
              ation (RS Acceleration). See RS Base Excitation (p. 294) for further details.
        •     The input excitation spectrum direction is defined in the global coordinate system for
              Single Point spectrum analysis. For Multiple Points spectrum analysis, however, the input
              excitation is defined in the nodal coordinate systems (if any) attached to the constrained
              nodes.
        •     More than one input excitation, with any different combination of spectrum types, are
              allowed for the response spectrum analysis.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              59
The Mechanical Application Approach

         •     Specify option to include or not include contribution of high frequency modes in the
               total response calculation by setting Missing Mass Effect to Yes or No. The option for
               including the modes is normally required for nuclear power plant design.
         •     Specify option to include or not include rigid responses to the total response calculation
               by setting Rigid Response Effect to Yes or No. The rigid responses normally occur in
               the frequency range that is lower than that of missing mass responses, but is higher
               than that of periodic responses.
         •     Missing Mass Effect and Rigid Response Effect are only applicable to RS Acceleration
               excitation.
         •     For a Single Point spectrum type, the entire table of input excitation spectrum can be
               scaled using the Scale Factor setting. The factor must be greater than 0.0. The default
               is 1.0.

Solve

             Basic general information about this topic

              ... for this analysis type:

        It is recommended that you review the Solution Information page for any warnings or errors
        that might occur during the ANSYS solve. Some warning messages will still enable the solve.

Review Results

             Basic general information about this topic

              ... for this analysis type:

         •     To view strain/stress results, a selection must be made in Output Controls of the modal
               analysis. By default, only displacement results are available.
         •     Applicable results are directional (X/Y/Z) displacement, velocity and acceleration. If
               strain/stress are requested, applicable results are normal strain and stress, and shear
               strain and stress.
         •     Results are displayed as a contour plot on the model.
         •     In addition to standard files generated by the Mechanical APDL application after the
               solve, the file Displacement.mcom is also made available. If the Output Controls are
               set to Yes for Calculate Velocity and/or Calculate Acceleration, the corresponding
               Velocity.mcom and/or Acceleration.mcom are also made available. These files
               contain the combination instructions including mode coefficients.

Shape Optimization Analysis
Introduction
The purpose of a shape optimization analysis is to find the best use of material for a body. Typically this in-
volves optimizing the distribution of material so that a structure will have the maximum stiffness for a set
of loads. The output of this analysis is a contour plot that shows the portions of the geometry that least
contributes to the stiffness of the structure for a given load. An optimization example showing a 60 percent
volume reduction is shown below.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
60                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Preparing the Analysis




Points to Remember
The following limitations apply to a shape optimization analysis:

 •   Only applicable to 3-D solids and 2-D plane stress geometries.
 •   Only linear static analysis is supported.
 •   A model containing any shell elements cannot be used in a shape optimization analysis.
 •   Only structural loads are allowed including thermal condition.
 •   The input you provide is a target percent reduction in material volume.
 •   The output is a contour plot that shows where material can possibly be removed with least impact on
     overall stiffness.

Preparing the Analysis
Create Analysis System

           Basic general information about this topic

            ... for this analysis type:

From the Toolbox, drag the Shape Optimization template to the Project Schematic.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                              61
The Mechanical Application Approach

Define Engineering Data

         Basic general information about this topic

          ... for this analysis type:

       Only linear, isotropic material properties are supported, that is, Young’s modulus and Poisson’s
       ratio. Temperature dependent material properties are also supported.

Attach Geometry

         Basic general information about this topic

          ... for this analysis type:

       The geometry must be 3-D or 2-D plane stress for shape optimization.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for shape optimization analysis.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       Contact and springs are allowed in a shape optimization analysis, but joints are not allowed.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for shape optimization analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       Shape optimization does not require any analysis settings.

Define Initial Conditions

         Basic general information about this topic

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
62                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Preparing the Analysis


              ... for this analysis type:

        There is no initial condition specification for a shape optimization analysis.

Apply Loads and Supports

             Basic general information about this topic

              ... for this analysis type:

        For a shape optimization analysis applicable loads/supports are are all inertial and structural
        loads, including Thermal Condition, and all structural supports. You can include the effect
        of any thermal expansion via a Thermal Condition load.

        The shape optimization analysis must contain at least one of the following loads:

         •     Structural Loads (p. 279)
         •     Structural inertial load (acceleration or rotation)

        Since all calculations assume static equilibrium, you must attach at least one structural support.
        Use at least one fixed-type support, or a combination of supports that prevent all possible
        rigid body motion of the body in space.

Solve

             Basic general information about this topic

              ... for this analysis type:

        Before solving you must insert a Shape Finder tool under the Solution branch and specify
        a Target Reduction percentage value in the Details view of the Shape Finder tool. A sub-
        sequent solve will aim towards pointing out areas of the structure where material could be
        removed while meeting the target reduction value.

        You can use scoping in the Shape Finder tool and focus material removal to a part, selected
        parts, or an entire assembly. This will eliminate material only on the scoped part(s).

        Solution Information continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis.

Review Results

             Basic general information about this topic

              ... for this analysis type:

        The only allowable result is the Shape Finder tool itself. Shape displays results as contour
        plots of the original part or assembly, with regions of material to remove specially colored.
        Shape optimization pictures provide insight into the optimal layout of material to carry a
        given load. Use this information as a guide in determining parametric or feature changes to
        improve the design of a part or the assembly.



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              63
The Mechanical Application Approach


               Note

               A Shape Finder animation is not supported when the Geometry drop down list
               in the Result toolbar is set to Slice Planes. Any animation produced in this mode
               will not function correctly.

        The Details view of the Shape Finder shows the following information:

         •     Target Reduction percentage.
         •     Original Mass of the part or assembly.
         •     Optimized Mass of the part or assembly
         •     Marginal Mass of material.

               Note

               If Density is temperature dependent, then the mass values reported use a density
               value calculated at the reference temperature of the body.

        The estimation of optimized weight includes all "marginal" material.

Static Structural Analysis
Introduction
A static structural analysis determines the displacements, stresses, strains, and forces in structures or com-
ponents caused by loads that do not induce significant inertia and damping effects. Steady loading and re-
sponse conditions are assumed; that is, the loads and the structure's response are assumed to vary slowly
with respect to time. A static structural load can be performed using the ANSYS or SAMCEF solver. The types
of loading that can be applied in a static analysis include:

 •   Externally applied forces and pressures
 •   Steady-state inertial forces (such as gravity or rotational velocity)
 •   Imposed (nonzero) displacements
 •   Temperatures (for thermal strain)

Point to Remember
A static structural analysis can be either linear or nonlinear. All types of nonlinearities are allowed - large
deformations, plasticity, stress stiffening, contact (gap) elements, hyperelasticity and so on. This chapter focuses
on linear static analyses, with brief references to nonlinearities. Details of how to handle nonlinearities are
described in Nonlinear Controls (p. 269).

Note that available nonlinearities can differ from one solver to another.

Preparing the Analysis
Create Analysis System

             Basic general information about this topic


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
64                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis


          ... for this analysis type:

      From the Toolbox, drag a Static Structural (ANSYS) or Static Structural (Samcef) template
      to the Project Schematic.

Define Engineering Data

         Basic general information about this topic

          ... for this analysis type:

      Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or tem-
      perature-dependent. You must define stiffness in some form (for example, Young's modulus,
      hyperelastic coefficients, and so on). For inertial loads (such as Standard Earth Gravity), you
      must define the data required for mass calculations, such as density.

Attach Geometry

         Basic general information about this topic

          ... for this analysis type:

      When 2D geometry is used, only the 2D axisymmetric behavior is available for the SAMCEF
      solver.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

      A “rigid” part is essentially a point mass connected to the rest of the structure via joints.
      Hence in a static structural analysis the only applicable loads on a rigid part are acceleration
      and rotational velocity loads. You can also apply loads to a rigid part via joint loads. The
      output from a rigid part is the overall motion of the part plus any force transferred via that
      part to the rest of the structure. Rigid behavior cannot be used with SAMCEF.

      If your model includes nonlinearities such as large deflection or hyperelasticity, the solution
      time can be significant due to the iterative solution procedure. Hence you may want to
      simplify your model if possible. For example you may be able to represent your 3-D structure
      as a 2-D plane stress, plane strain, or axisymmetric model or you may be able to reduce your
      model size through the use of symmetry or antisymmetry surfaces. Similarly if you can omit
      nonlinear behavior in one or more parts of your assembly without affecting results in critical
      regions it will be advantageous to do so.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

      Contact, joints springs, and beams are all valid in a static structural analysis.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              65
The Mechanical Application Approach

       For the SAMCEF solver, only contacts, springs, and beams are supported. Joints are not sup-
       ported.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       Provide an adequate mesh density on contact surfaces to allow contact stresses to be distrib-
       uted in a smooth fashion. Likewise, provide a mesh density adequate for resolving stresses;
       areas where stresses or strains are of interest require a relatively fine mesh compared to that
       needed for displacement or nonlinearity resolution. If you want to include nonlinearities, the
       mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires
       a reasonable integration point density (and therefore a fine element mesh) in areas with high
       plastic deformation gradients.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For simple linear static analyses you typically do not need to change these settings. For more
       complex analyses the basic controls are:

       Large Deflection (p. 272) is typically needed for slender structures. A rule of thumb is that you
       can use large deflection if the transverse displacements in a slender structure are more than
       10% of the thickness.

       Small deflection and small strain analyses assume that displacements are small enough that
       the resulting stiffness changes are insignificant. Setting Large Deflection to On will take into
       account stiffness changes resulting from changes in element shape and orientation due to
       large deflection, large rotation, and large strain. Therefore the results will be more accurate.
       However this effect requires an iterative solution. In addition it may also need the load to
       be applied in small increments. Therefore, the solution may take longer to solve.

       You also need to turn on large deflection if you suspect instability (buckling) in the system.
       Use of hyperelastic materials also requires large deflection to be turned on.

       Step Controls (p. 266) are used to i) control the time step size and other solution controls and
       ii) create multiple steps when needed. Typically analyses that include nonlinearities such as
       large deflection or plasticity require control over time step sizes as outlined in the Automatic
       Time Stepping (p. 264) section. Multiple steps are required for activation/deactivation of dis-
       placement loads or pretension bolt loads. This group can be modified on a per step basis.

            Note

            Time Stepping is available for any solver.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. In a nonlinear analysis it may be necessary to perform many


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
66                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis

       solutions at intermediate load values. However i) you may not be interested in all the inter-
       mediate results and ii) writing all the results can make the results file size unwieldy. This
       group can be modified on a per step basis except for Calculate Stress and Calculate Strain.

       Nonlinear Controls (p. 269)(applicable to Static Structural (ANSYS) or Static Structural
       (SAMCEF) systems only) allow you to modify convergence criteria and other specialized
       solution controls. Typically you will not need to change the default values for this control.
       This group can be modified on a per step basis.

       Analysis Data Management (p. 277) settings enable you to save specific solution files from the
       Static Structural analysis for use in other analyses. You can set the Future Analysis field to
       Pre-Stressed Analysis if you intend to use the static structural results in a subsequent
       Modal or Linear Buckling (Linear Buckling is applicable to Static Structural (ANSYS) systems
       only) analysis. A typical example is the large tensile stress induced in a turbine blade under
       centrifugal load. This causes significant stiffening of the blade resulting in much higher,
       realistic natural frequencies in a modal analysis. More details are available in the section
       Define Initial Conditions (p. 13).

            Note

            Scratch Solver Files, Save ANSYS db, Solver Units, and Solver Unit System are
            applicable to Static Structural (ANSYS) systems only.

Define Initial Conditions

         Basic general information about this topic

          ... for this analysis type:

       Initial condition is not applicable for Static Structural analyses.

Apply Loads and Supports

         Basic general information about this topic

          ... for this analysis type:

       For a static structural analysis applicable loads/supports are all inertial and structural loads,
       and all structural supports.

       For the SAMCEF solver, the following loads and supports are not available: Hydrostatic Pressure,
       Bearing Load, Bolt Pretension, Joint Load, Fluid Solid Interface, Motion Loads, Compression
       Only Support, Elastic Support.

       Loads and supports vary as a function of time even in a static analysis as explained in the
       Role of Time in Tracking (p. 262). In a static analysis, the load’s magnitude could be a constant
       value or could vary with time as defined in a table or via a function. Details of how to apply
       a tabular or function load are described in Applying Tabular and Function Loads. In addition,
       see the Apply Loads and Supports section for more information about time stepping and
       ramped loads.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              67
The Mechanical Application Approach


             Note

             A static analysis can be followed by a “pre-stressed” analysis such as modal or
             linear (eigenvalue) buckling analysis. In this subsequent analysis the effect of stress
             on stiffness of the structure (stress-stiffness effect) is taken into account. If the
             static analysis has a pressure or force load applied on faces (3-D) or edges (2-D)
             this could result in an additional stiffness contribution called “pressure load stiff-
             ness” effect. This effect plays a significant role in linear (eigenvalue) buckling
             analysis. This additional effect is computed during the buckling analysis using the
             pressure or force value in the static analysis at time = 0. Because of this if the
             static analysis is to be used for a subsequent buckling analysis you should step
             apply any pressure loads.

Solve

          Basic general information about this topic

           ... for this analysis type:

        When performing a nonlinear analysis you may encounter convergence difficulties due to a
        number of reasons. Some examples may be initially open contact surfaces causing rigid body
        motion, large load increments causing non-convergence, material instabilities, or large de-
        formations causing mesh distortion that result in element shape errors. To identify possible
        problem areas some tools are available under Solution Information object Details view.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

        You can display contour plots of Newton-Raphson Residuals in a nonlinear static analysis.
        Such a capability can be useful when you experience convergence difficulties in the middle
        of a step, where the model has a large number of contact surfaces and other nonlinearities.
        When the solution diverges identifying regions of high Newton-Raphson residual forces can
        provide insight into possible problems.

        Result Tracker (applicable to Static Structural (ANSYS) systems only) is another useful tool
        that allows you to monitor displacement and energy results as the solution progresses. This
        is especially useful in case of structures that possibly go through convergence difficulties
        due to buckling instability.

Review Results

          Basic general information about this topic

           ... for this analysis type:

        All structural result types except frequencies are available as a result of a static structural
        analysis. You can use a Solution Information object to track, monitor, or diagnose problems
        that arise during a solution.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
68                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

       Once a solution is available you can contour the results or animate the results to review the
       response of the structure.

       As a result of a nonlinear static analysis you may have a solution at several time points. You
       can use probes to display the variation of a result item as the load increases. An example
       might be large deformation analyses that result in buckling of the structure. In these cases
       it is also of interest to plot one result quantity (for example, displacement at a vertex) against
       another results item (for example, applied load). You can use the Charts feature to develop
       such charts.

Steady-State Thermal Analysis
Introduction
You can use a steady-state thermal analysis to determine temperatures, thermal gradients, heat flow rates,
and heat fluxes in an object that are caused by thermal loads that do not vary over time. A steady-state
thermal analysis calculates the effects of steady thermal loads on a system or component. Engineers often
perform a steady-state analysis before performing a transient thermal analysis, to help establish initial con-
ditions. A steady-state analysis also can be the last step of a transient thermal analysis, performed after all
transient effects have diminished.

Point to Remember
A steady-state thermal analysis may be either linear, with constant material properties; or nonlinear, with
material properties that depend on temperature. The thermal properties of most material do vary with
temperature, so the analysis usually is nonlinear. Including radiation effects or temperature dependent
convection coefficient also makes the analysis nonlinear.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

From the Toolbox, drag a Steady-State Thermal template to the Project Schematic.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

       Thermal Conductivity must be defined for a steady-state thermal analysis. Thermal Conduct-
       ivity can be isotropic or orthotropic, and constant or temperature-dependent.

Attach Geometry

          Basic general information about this topic

           ... for this analysis type:

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              69
The Mechanical Application Approach

       There are no specific considerations for a steady-state thermal analysis.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for a steady-state thermal analysis.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       In a thermal analysis only contact is valid. Any joints or springs are ignored.

       With contact the initial status is maintained throughout the thermal analysis, that is, any
       closed contact faces will remain closed and any open contact faces will remain open for the
       duration of the thermal analysis. Heat conduction across a closed contact face is set to a
       sufficiently high enough value (based on the thermal conductivities and the model size) to
       model perfect contact with minimal thermal resistance. If needed, you can model imperfect
       contact by manually inputting a Thermal Conductance value.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for steady-state thermal analysis itself. However if the
       temperatures from this analysis are to be used in a subsequent structural analysis the mesh
       must be identical. Therefore in this case you may want to make sure the mesh is fine enough
       for structural analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For a steady-state thermal analyses you typically do not need to change these settings. The
       basic controls are:

       Step Controls (p. 266) allow you to control the rate of loading which could be important in a
       steady-state thermal analysis if the material properties vary rapidly with temperature. When
       such nonlinearities are present it may be necessary to apply the loads in small increments
       and perform solutions at these intermediate loads to achieve convergence. You may wish to
       use multiple steps if you a) want to analyze several different loading scenarios within the
       same analysis or b) if you want to change the analysis settings such as the time step size or
       the solution output frequency over specific time ranges.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
70                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Preparing the Analysis

        Output Controls (p. 270) allow you to specify the time points at which results should be
        available for postprocessing. In a nonlinear analysis it may be necessary to perform many
        solutions at intermediate load values. However i) you may not be interested in all the inter-
        mediate results and ii) writing all the results can make the results file size unwieldy. In this
        case you can restrict the amount of output by requesting results only at certain time points.

        Nonlinear Controls (p. 269) allow you to modify convergence criteria and other specialized
        solution controls. Typically you will not need to change the default values for this control.

        Analysis Data Management (p. 277) settings enable you to save specific solution files from the
        steady-state thermal analysis for use in other analyses.

Define Initial Conditions

             Basic general information about this topic

              ... for this analysis type:

        For a steady-state thermal analysis you can specify an initial temperature value. This uniform
        temperature is used during the first iteration of a solution as follows:

         •     To evaluate temperature-dependent material properties.
         •     As the starting temperature value for constant temperature loads.

Apply Loads and Supports

             Basic general information about this topic

              ... for this analysis type:

        The following loads are supported in a steady-state thermal analysis:

         •     Temperature (p. 298)
         •     Convection (p. 298)
         •     Radiation (p. 300)
         •     Heat Flow (p. 300)
         •     Perfectly Insulated (p. 302)
         •     Heat Flux (p. 302)
         •     Internal Heat Generation (p. 303)
         •     CFD Imported Temperature (p. 314)
         •     CFD Imported Convection (p. 314)

        Loads and supports vary as a function of time even in a static analysis as explained in the
        Role of Time in Role of Time in Tracking (p. 262). In a static analysis, the load’s magnitude could
        be a constant value or could vary with time as defined in a table or via a function. Details of
        how to apply a tabular or function load are described in Applying Tabular and Function
        Loads. In addition, see the Apply Loads and Supports section for more information about
        time stepping and ramped loads.

Solve

                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              71
The Mechanical Application Approach


          Basic general information about this topic

           ... for this analysis type:

        The Solution Information object provides some tools to monitor solution progress.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

        You can also insert a Result Tracker object under Solution Information. This tool allows
        you to monitor temperature at a vertex as the solution progresses.

Review Results

          Basic general information about this topic

           ... for this analysis type:

        Applicable results are all thermal result types.

        Once a solution is available you can contour the results or animate the results to review the
        response of the structure.

        As a result of a nonlinear analysis you may have a solution at several time points. You can
        use probes to display the variation of a result item over the load history. Also of interest is
        the ability to plot one result quantity (for example, average temperature on a face) against
        another results item (for example, applied heat generation rate). You can use the Charts
        feature to develop such charts.

        Note that Charts are also useful to compare results between two analyses of the same model.

Thermal-Electric Analysis
Introduction
A Steady-State Thermal-Electric Conduction analysis allows for a simultaneous solution of thermal and
electric fields. This coupled-field capability models joule heating for resistive materials and contact electric
conductance as well as Seebeck, Peltier, and Thomson effects for thermoelectricity, as described below.

 •   Joule heating - Heating occurs in a resistive conductor carrying an electric current. Joule heating is
     proportional to the square of the current, and is independent of the current direction. Joule heating is
     also present and accounted for at the contact interface between bodies in inverse proportion to the
     contact electric conductance properties. (Note however that the Joule Heat results object will not display
     contact joule heating values. Only solid body joule heating is represented).
 •   Seebeck effect - A voltage (Seebeck EMF) is produced in a thermoelectric material by a temperature
     difference. The induced voltage is proportional to the temperature difference. The proportionality
     coefficient is know as the Seebeck Coefficient (α).
 •   Peltier effect - Cooling or heating occurs at a junction of two dissimilar thermoelectric materials when
     an electric current flows through that junction. Peltier heat is proportional to the current, and changes
     sign if the current direction is reversed.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
72                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis

 •   Thomson effect - Heat is absorbed or released in a non-uniformly heated thermoelectric material when
     electric current flows through it. Thomson heat is proportional to the current, and changes sign if the
     current direction is reversed.

Points to Remember
Electric loads may be applied to parts with electric properties and thermal loads may be applied to bodies
with thermal properties. Parts with both physics properties can support both thermal and electric loads. See
the Steady-state Thermal Analysis section and the Electric Analysis section of the help for more information
about applicable loads, boundary conditions, and results types.

In addition to calculating the effects of steady thermal and electric loads on a system or component, a
Steady-State Thermal-Electric analysis supports a multi-step solution.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

From the Toolbox, drag the Thermal-Electric template to the Project Schematic.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

        To have Thermal and/or Electrical effects properly applied to the parts of your model, you
        need to define the appropriate material properties. For a steady-state analysis, the electrical
        property Resistivity is required for Joule Heating effects and Thermal Conductivity for
        thermal conduction effects. Seebeck/Peltier/Thomson effects require you to define the Seebeck
        Coefficient material property.

Attach Geometry

          Basic general information about this topic

           ... for this analysis type:

        There are no specific considerations for an thermal-electric analysis.

Define Part Behavior

          Basic general information about this topic

           ... for this analysis type:

        There are no specific considerations for a thermal-electric analysis.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              73
The Mechanical Application Approach

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       Contact across parts during a thermal-electric analysis consider thermal and/or electric effects
       based on the material properties of adjacent parts. That is, if both parts have thermal prop-
       erties, thermal contact is applied and if both parts have electric properties, electric contact
       is applied.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations regarding meshing for a thermal-electric analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For an thermal-electric analysis, the basic controls are:

       Step Controls (p. 266): used to specify the end time of a step in a single or multiple step ana-
       lysis. Multiple steps are needed if you want to change load values, the solution settings, or
       the solution output frequency over specific steps. Typically you do not need to change the
       default values.

       Typical thermal-electric problems contain temperature dependent material properties and
       are therefore nonlinear. Nonlinear Controls for both thermal and electrical effects are available
       and include Heat and Temperature convergence for thermal effects and Voltage and Current
       convergence for electric effects. The Program Controlled option for Nonlinear Formulation
       defaults to the Quasi option, but the Full option is used in cases when a Radiation load is
       present or when a distributed solver is used during the solution.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. A multi-step analysis involves calculating solutions at several
       time points in the load history. However you may not be interested in all of the possible
       results items and writing all the results can make the result file size unwieldy. You can restrict
       the amount of output by requesting results only at certain time points or limit the results
       that go onto the results file at each time point.

       Analysis Data Management (p. 277) settings.

       The default Solver Controls setting for thermal-electric analysis is the Direct (Sparse) solver.
       The Iterative (PCG) solver may be selected as an alternative solver. If Seebeck effects are in-
       cluded, the solver is automatically set to Direct.

Define Initial Conditions

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
74                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Preparing the Analysis


             Basic general information about this topic

              ... for this analysis type:

        There is no initial condition specification for an thermal-electric analysis.

Apply Loads and Supports

             Basic general information about this topic

              ... for this analysis type:

        The following loads are supported in a Thermal-Electric analysis:

         •     Voltage
         •     Current
         •     Coupling Condition
         •     Temperature
         •     Convection
         •     Radiation
         •     Heat Flow
         •     Perfectly Insulated
         •     Heat Flux
         •     Internal Heat Generation

Solve

             Basic general information about this topic

              ... for this analysis type:

        The Solution Information object provides some tools to monitor solution progress.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the model during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

Review Results

             Basic general information about this topic

              ... for this analysis type:

        Applicable results include all thermal and electric results.

        Once a solution is available, you can contour the results or animate the results to review the
        responses of the model.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              75
The Mechanical Application Approach

        For the results of a multi-step analysis that has a solution at several time points, you can use
        probes to display variations of a result item over the steps.

        You may also wish to use the Charts feature to plot multiple result quantities against time
        (steps). For example, you could compare current and joule heating. Charts can also be useful
        when comparing the results between two analysis branches of the same model.

Transient Structural Analyses
A transient analysis, by definition, involves loads that are a function of time. In the Mechanical application,
you can perform a transient structural analysis, on either a flexible structure or a rigid assembly. For a flexible
structure, the Mechanical application uses the ANSYS Mechanical solver, and for a rigid assembly, the
Mechanical application uses the ANSYS Rigid Dynamics solver. Please see the following subsections based
on your need.
 Transient Structural (ANSYS) Analysis
 Transient Structural (MBD) Analysis

Transient Structural (ANSYS) Analysis
Introduction
You can perform a transient structural (ANSYS) analysis (also called time-history analysis) in the Mechanical
application using the transient structural analysis that specifically uses the ANSYS Mechanical solver. This
type of analysis is used to determine the dynamic response of a structure under the action of any general
time-dependent loads. You can use it to determine the time-varying displacements, strains, stresses, and
forces in a structure as it responds to any transient loads. The time scale of the loading is such that the in-
ertia or damping effects are considered to be important. If the inertia and damping effects are not important,
you might be able to use a static analysis instead.

Points to Remember
A transient structural (ANSYS) analysis can be either linear or nonlinear. All types of nonlinearities are allowed
- large deformations, plasticity, contact, hyperelasticity and so on.

A transient dynamic analysis is more involved than a static analysis because it generally requires more
computer resources and more of your resources, in terms of the “engineering” time involved. You can save
a significant amount of these resources by doing some preliminary work to understand the physics of the
problem. For example, you can:

 1.   Try to understand how nonlinearities (if you are including them) affect the structure's response by
      doing a static analysis first. In some cases, nonlinearities need not be included in the dynamic analysis.
      Including nonlinear effects can be expensive in terms of solution time.
 2.   Understand the dynamics of the problem. By doing a modal analysis, which calculates the natural
      frequencies and mode shapes, you can learn how the structure responds when those modes are excited.
      The natural frequencies are also useful for calculating the correct integration time step.
 3.   Analyze a simpler model first. A model of beams, masses, springs, and dampers can provide good insight
      into the problem at minimal cost. This simpler model may be all you need to determine the dynamic
      response of the structure.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
76                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Preparing the Analysis


    Note

    Refer to the following sections of the Mechanical APDL application documentation for a more
    thorough treatment of dynamic analysis capabilities:

     •     The Transient Dynamic Analysis chapter of the Structural Analysis Guide - for a technical
           overview of nonlinear transient dynamics.
     •     The Multibody Analysis Guide - for a reference that is particular to multibody motion problems.
           In this context, “multibody” refers to multiple rigid or flexible parts interacting in a dynamic
           fashion.

    Although not all dynamic analysis features discussed in these manuals are directly applicable to
    Workbench features, the manuals provide an excellent background on general theoretical topics.

Preparing the Analysis
Create Analysis System

           Basic general information about this topic

            ... for this analysis type:

         From the Toolbox, drag a Transient Structural (ANSYS) template to the Project Schematic.

Define Engineering Data

           Basic general information about this topic

            ... for this analysis type:

         Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or tem-
         perature-dependent. Both Young’s modulus (and stiffness in some form) and density (or mass
         in some form) must be defined.

Attach Geometry

           Basic general information about this topic

            ... for this analysis type:

         There are no specific considerations for a transient structural (ANSYS) analysis.

Define Part Behavior

           Basic general information about this topic

            ... for this analysis type:

         In a transient structural (ANSYS) analysis, rigid parts are often used to model mechanisms
         that have gross motion and transfer loads between parts, but detailed stress distribution is
         not of interest. The output from a rigid part is the overall motion of the part plus any force


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                              77
The Mechanical Application Approach

       transferred via that part to the rest of the structure. A “rigid” part is essentially a point mass
       connected to the rest of the structure via joints. Hence in a transient structural (ANSYS)
       analysis the only applicable loads on a rigid part are acceleration and rotational velocity
       loads. You can also apply loads to a rigid part via joint loads.

       If your model includes nonlinearities such as large deflection or hyperelasticity, the solution
       time can be significant due to the iterative solution procedure. Hence, you may want to
       simplify your model if possible. For example, you may be able to represent your 3-D structure
       as a 2-D plane stress, plane strain, or axisymmetric model, or you may be able to reduce your
       model size through the use of symmetry or antisymmetry surfaces. Similarly, if you can omit
       nonlinear behavior in one or more parts of your assembly without affecting results in critical
       regions, it will be advantageous to do so.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       Contact, joints and springs are all valid in a transient structural (ANSYS) analysis. In a transient
       structural (ANSYS) analysis, you can specify a damping coefficient property in longitudinal
       springs that will generate a damping force proportional to velocity.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       Provide an adequate mesh density on contact surfaces to allow contact stresses to be distrib-
       uted in a smooth fashion. Likewise, provide a mesh density adequate for resolving stresses;
       areas where stresses or strains are of interest require a relatively fine mesh compared to that
       needed for displacement or nonlinearity resolution. If you want to include nonlinearities, the
       mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires
       a reasonable integration point density (and therefore a fine element mesh) in areas with high
       plastic deformation gradients.

       In a dynamic analysis, the mesh should be fine enough to be able to represent the highest
       mode shape of interest.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For transient structural (ANSYS) analysis the basic controls are:

       Large Deflection (p. 272) is typically needed for slender structures. A rule of thumb is that you
       can use large deflection if the transverse displacements in a slender structure are more than
       10% of the thickness.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
78                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

       Small deflection and small strain analyses assume that displacements are small enough that
       the resulting stiffness changes are insignificant. Setting Large Deflection to On will take into
       account stiffness changes resulting from change in element shape and orientation due to
       large deflection, large rotation, and large strain. Therefore the results will be more accurate.
       However this effect requires an iterative solution. In addition it may also need the load to
       be applied in small increments. Therefore the solution may take longer to solve.

       You also need to turn on large deflection if you suspect instability (buckling) in the system.
       Use of hyperelastic materials also requires large deflection to be turned on.

       Step Controls (p. 266) allow you to control the time step size in a transient analysis. Refer to
       the Guidelines for Integration Step Size (p. 264) section for further information. In addition this
       control also allows you create multiple steps. Multiple steps are useful if new loads are intro-
       duced or removed at different times in the load history, or if you want to change the analysis
       settings such as the time step size at some points in the time history. When the applied load
       has high frequency content or if nonlinearities are present, it may be necessary to use a small
       time step size (that is, small load increments) and perform solutions at these intermediate
       time points to arrive at good quality results. This group can be modified on a per step basis.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. In a transient nonlinear analysis it may be necessary to perform
       many solutions at intermediate time values. However, i) you may not be interested in all the
       intermediate results, and ii) writing all the results can make the results file size unwieldy. This
       group can be modified on a per step basis except for Calculate Stress and Calculate Strain.

       Nonlinear Controls (p. 269) allow you to modify convergence criteria and other specialized
       solution controls. Typically you will not need to change the default values for this control.
       This group can be modified on a per step basis.

       Damping Controls (p. 276) allow you to specify damping for the structure in a transient analysis.
       The following forms of damping are available for a transient analysis: Beta damping and
       Numerical damping. In addition, element based damping from spring elements as well as
       material based damping factors are also available for the transient structural (ANSYS) analysis.

       Analysis Data Management (p. 277) settings enable you to save specific solution files from the
       transient structural (ANSYS) analysis for use in other analyses. The default behavior is to only
       keep the files required for postprocessing. You can use these controls to keep all files created
       during solution or to create and save the Mechanical APDL application database (db file).

Define Initial Conditions

         Basic general information about this topic

             ... for this analysis type:

        1.     A transient analysis involves loads that are functions of time. The first step in applying
               transient loads is to establish initial conditions (that is, the condition at Time = 0).
        2.     The default initial condition for a transient structural (ANSYS) analysis is that the structure
                          ,
               is “at rest” that is, both initial displacement and initial velocity are zero. A transient
               structural (ANSYS) analysis is at rest, by default. The Initial Conditions object allows
               you to specify Velocity.
        3.     In many analyses one or more parts will have an initial known velocity such as in a
               drop test, metal forming analysis or kinematic analysis. In these analyses, you can specify

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              79
The Mechanical Application Approach

             a constant Velocity initial condition if needed. The constant velocity could be scoped
             to one or more parts of the structure. The remaining parts of the structure which are
             not part of the scoping will retain the “at rest” initial condition.
        4.   Initial Condition using Steps: You can also specify initial conditions using step controls,
             that is, by specifying multiple steps in a transient analysis and controlling the time in-
             tegration effects along with activation/deactivation of loads. This comes in handy when,
             for example, you have different parts of your model that have different initial velocities
             or more complex initial conditions. The following are approaches to some commonly
             encountered initial condition scenarios:
             a.   Initial Displacement = 0, Initial Velocity ≠ 0 for some parts: The nonzero velocity
                  is established by applying small displacements over a small time interval on the
                  part of the structure where velocity is to be specified.
                  i.       Specify 2 steps in your analysis. The first step will be used to establish initial
                           velocity on one or more parts.
                  ii.      Choose a small end time (compared to the total span of the transient analysis)
                           for the first step. The second step will cover the total time span.
                  iii.     Specify displacement(s) on one or more faces of the part(s) that will give you
                           the required initial velocity. This requires that you do not have any other
                           boundary condition on the part that will interfere with rigid body motion of
                           that part. Make sure that these displacements are ramped from a value of 0.
                  iv.      Deactivate or release the specified displacement load in the second step so
                           that the part is free to move with the specified initial velocity.

                           For example, if you want to specify an initial Y velocity on a part of 0.005
                           inch/sec and your first step end time is 0.001 second, then specify the following
                           loads. Make sure that the load is ramped from a value of 0 at time = 0 so that
                           you will get the required velocity.




                           In this case the end time of the actual transient analysis is 30 seconds. Note
                           that the Y displacement in the second step is deactivated.
                  v.       In the Analysis Settings Details view, set the following for first step:




                  vi.      You can choose appropriate time step sizes for the second step (the actual
                           transient). Make sure that time integration effects are turned on for the second
                           step.



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
80                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                      Preparing the Analysis

     In the first step, inertia effects will not be included but velocity will be computed
     based on the displacement applied. In the second step, this displacement is released
     by deactivation and the time integration effects are turned on.
b.   Initial Displacement ≠ 0, Initial Velocity ≠ 0: This is similar to case a. above
     except that the imposed displacements are the actual values instead of “small”
     values. For example if the initial displacement is 1 inch and the initial velocity is
     2.5 inch/sec then you would apply a displacement of 1 inch over 0.4 seconds.
     i.       Specify 2 steps in your analysis. The first step will be used to establish initial
              displacement and velocity on one or more parts.
     ii.      Choose a small end time (compared to the total span of the transient analysis)
              for the first step. The second step will cover the total time span.
     iii.     Specify the initial displacement(s) on one or more faces of the part(s) as
              needed. This requires that you do not have any other boundary condition on
              the part that will interfere with rigid body motion of that part. Make sure that
              these displacements are ramped from a value of 0.
     iv.      Deactivate or release the specified displacement load in the second step so
              that the part is free to move with the specified initial velocity.

              For example if you want to specify an initial Z velocity on a part of 0.5 inch/sec
              and an have an initial displacement of 0.1 inch, then your first step end time
              = (0.1/0.5) = 0.2 second. Make sure that the displacement is ramped from a
              value of 0 at time = 0 so that you will get the required velocity.




              In this case the end time of the actual transient analysis is 5 seconds. Note
              that the Z displacement in the second step is deactivated.
     v.       In the Analysis Settings Details view, set the following for first step:




     vi.      You can choose appropriate time step sizes for the second step (the actual
              transient). Make sure that time integration effects are turned on for the second
              step.

     In the first step, inertia effects will not be included but velocity will be computed
     based on the displacement applied. In the second step, this displacement is released
     by deactivation and the time integration effects are turned on.
c.   Initial Displacement ≠ 0, Initial Velocity = 0: This requires the use of two steps
     also. The main difference between b. above and this scenario is that the displace-
     ment load in the first step is not ramped from zero. Instead it is step applied as

            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                        of ANSYS, Inc. and its subsidiaries and affiliates.                                              81
The Mechanical Application Approach

                 shown below with 2 or more substeps to ensure that the velocity is zero at the
                 end of step 1.
                 i.       Specify 2 steps in your analysis. The first step will be used to establish initial
                          displacement on one or more parts.
                 ii.      Choose an end time for the first step that together with the initial displacement
                          values will create the necessary initial velocity.
                 iii.     Specify the initial displacement(s) on one or more faces of the part(s) as
                          needed. This requires that you do not have any other boundary condition on
                          the part that will interfere with rigid body motion of that part. Make sure that
                          this load is step applied, that is, apply the full value of displacements at time
                          = 0 itself and maintain it throughout the first step.
                 iv.      Deactivate or release the specified displacement load in the second step so
                          that the part is free to move with the initial displacement values.

                          For example if you want to specify an initial Z displacement of 0.1 inch and
                          the end time for the first step is 0.001 seconds, then the load history displays
                          as shown below. Note the step application of the displacement.




                          In this case the end time of the actual transient analysis is 5 seconds. Note
                          that the Z displacement in the second step is deactivated.
                 v.       In the Analysis Settings Details view, set the following for first step. Note
                          that the number of substeps must be at least 2 to set the initial velocity to
                          zero.




                 vi.      You can choose appropriate time step sizes for the second step (the actual
                          transient). Make sure that time integration effects are turned on for the second
                          step.

                 In the first step, inertia effects will not be included but velocity will be computed
                 based on the displacement applied. But since the displacement value is held con-
                 stant, the velocity will evaluate to zero after the first substep. In the second step,
                 this displacement is released by deactivation and the time integration effects are
                 turned on.

Apply Loads and Supports

         Basic general information about this topic


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
82                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Preparing the Analysis


           ... for this analysis type:

        For a transient structural (ANSYS) analysis applicable loads/supports are are all inertial and
        structural loads, and all structural supports. Joint Loads are used to kinematically drive joints.
        See the Joint Load (p. 295) section for details.

        In this analysis, the load’s magnitude could be a constant value or could vary with time as
        defined in a table or via a function. Details of how to apply a tabular or function load are
        described in Applying Tabular and Function Loads. In addition, see the Apply Loads and
        Supports section for more information about time stepping and ramped loads.

        For the transient structural (ANSYS) solver to converge, it is recommended that you ramp
        joint load angles and positions from zero to the real initial condition over one step.

Solve

          Basic general information about this topic

           ... for this analysis type:

        When performing a nonlinear analysis, you may encounter convergence difficulties due to a
        number of reasons. Some examples may be initially open contact surfaces causing rigid body
        motion, large load increments causing non-convergence, material instabilities, or large de-
        formations causing mesh distortion that result in element shape errors. To identify possible
        problem areas some tools are available under Solution Information object Details view.

        Solution Output continuously updates any listing output from the solver and provides
        valuable information on the behavior of the structure during the analysis. Any convergence
        data output in this printout can be graphically displayed as explained in the Solution Inform-
        ation section.

        You can display contour plots of Newton-Raphson Residuals in a nonlinear static analysis.
        Such a capability can be useful when you experience convergence difficulties in the middle
        of a step, where the model has a large number of contact surfaces and other nonlinearities.
        When the solution diverges, identifying regions of high Newton-Raphson residual forces can
        provide insight into possible problems.

        Result Tracker is another useful tool that allows you to monitor displacement and energy
        results as the solution progresses. This is especially useful in case of structures that possibly
        go through convergence difficulties due to buckling instability.

Review Results

          Basic general information about this topic

           ... for this analysis type:

        All structural result types except frequencies are available as a result of a transient structural
        (ANSYS) analysis. You can use a Solution Information object to track, monitor, or diagnose
        problems that arise during a solution.

        Once a solution is available you can contour the results or animate the results to review the
        response of the structure.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              83
The Mechanical Application Approach

        As a result of a nonlinear static analysis, you may have a solution at several time points. You
        can use probes to display the variation of a result item as the load increases.

             Note

             Fixed body-to-body joints between two rigid bodies will not produce a joint force
             or moment in a transient structural (ANSYS) analysis.

        Also of interest is the ability to plot one result quantity (for example, displacement at a vertex)
        against another result item (for example, applied load). You can use the Charts feature to
        develop such charts. Charts are also useful to compare results between two analyses of the
        same model. For example, you can compare the displacement response at a vertex from two
        transient structural (ANSYS) analyses with different damping characteristics.

Transient Structural (MBD) Analysis
Introduction
You can perform a transient structural multibody dynamics (MBD) analysis in the Mechanical application
using the ANSYS Rigid Dynamics solver. This type of analysis is used to determine the dynamic response of
an assembly of rigid bodies linked by joints and springs. You can use this type of analysis to study the kin-
ematics of a robot arm or a crankshaft system for example.

Points to Remember
 •   Joint rotations are not cumulative with each additional step.
 •   Inputs and outputs are forces, moments, displacements, velocities and accelerations.
 •   All parts are rigid such that there are no stresses and strain results produced, only forces, moments,
     displacements, velocities and accelerations.
 •   The solver is tuned to automatically adjust the time step. Doing it manually is often inefficient and
     results in longer run times.
 •   Viscous damping can be taken into account through springs.

     Note

     Refer to the Multibody Analysis Guide for a reference that is particular to multibody motion prob-
     lems. In this context, “multibody” refers to multiple rigid parts interacting in a dynamic fashion.

     Although not all dynamic analysis features discussed in this manual are directly applicable to
     Workbench features, it provides an excellent background on general theoretical topics.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

            ... for this analysis type:

        From the Toolbox, drag a Transient Structural (MBD) template to the Project Schematic.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
84                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis

Define Engineering Data

         Basic general information about this topic

          ... for this analysis type:

       Density is the only material property utilized in a rigid dynamics analysis.

Attach Geometry

         Basic general information about this topic

          ... for this analysis type:

       Sheet, solid, and plane bodies are supported by the ANSYS Rigid Dynamics solver. Line
       bodies cannot be used.

Define Part Behavior

         Basic general information about this topic

          ... for this analysis type:

       Part stiffness behavior is not required for the ANSYS Rigid Dynamics solver in ANSYS Work-
       bench.

Define Connections

         Basic general information about this topic

          ... for this analysis type:

       Applicable connections are joints and springs.

       When an assembly is imported from a CAD system, joints or constraints are not imported,
       but joints may be created automatically after the model is imported. You can also choose to
       create the joints manually.

       Each joint is defined by its coordinate system of reference. The orientation of this coordinate
       system is essential as the free and fixed degrees of freedom are defined in this coordinate
       system.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       Mesh controls are not applicable for the ANSYS Rigid Dynamics solver.

Establish Analysis Settings



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              85
The Mechanical Application Approach


            Basic general information about this topic

             ... for this analysis type:

       For transient structural (MBD) analysis the basic controls are:

       Step Controls (p. 266) allow you to create multiple steps. Multiple steps are useful if new loads
       are introduced or removed at different times in the load history.

       Transient structural (MBD) analyses use an explicit time integration scheme. Unlike the implicit
       time integration, there are no iterations to converge in an explicit time integration scheme.
       The solution at the end of the time step is a function of the derivatives during the time step.
       As a consequence, the time step required to get accurate results is usually smaller than is
       necessary for an implicit time integration scheme. Another consequence is that the time step
       is governed by the highest frequency of the system. A very smooth and slow model that has
       a very stiff spring will require the time step needed for the stiff spring itself, which generates
       the high frequencies that will govern the required time step.

       Because it is not easy to determine the frequency content of the system, an automatic time
       stepping algorithm is available, and should be used for the vast majority of models. This
       automatic time stepping algorithm is governed by Initial Time Step, Minimum Time Step,
       and Maximum Time Step under Step Controls; and Energy Accuracy Tolerance under
       Nonlinear Controls.

        •     Initial Time Step: If the initial time step chosen is vastly too large, the solution will
              typically fail, and produce an error message that the accelerations are too high. If the
              initial time step is a only slightly too large, the solver will realize that the first time steps
              are inaccurate, automatically decrement the time step and start the transient solution
              over. Conversely, if the chosen initial time step is excessively small, and the simulation
              can be accurately performed with higher time steps, the automatic time stepping al-
              gorithm will, after a few gradual increases, find the appropriate time step value. Choosing
              a good initial time step is a way to reduce the cost of having the solver figure out what
              time step size is optimal to minimize run time. While important, choosing the correct
              initial time step typically does not have a large influence on the total solution time due
              to the efficiency of the automatic time stepping algorithm.
        •     Minimum Time Step: During the automatic adjustment of the time step, if the time
              step that is required for stability and accuracy is smaller than the specified minimum
              time step, the solution will not proceed. This value does not influence solution time or
              its accuracy, but it is there to prevent Workbench from running forever with an extremely
              small time step. When the solution is aborting due to hitting this lower time step
              threshold, that usually means that the system is over constrained, or in a lock position.
              Check your model, and if you believe that the model and the loads are valid, you can
              decrease this value by one or two orders of magnitude and run again. That can, however
              generate a very large number of total time steps, and it is recommended that you use
              the Output Controls settings to store only some of the generated results.
        •     Maximum Time Step: Sometimes the time step that the automatic time stepping settles
              on produces too few results outputs for precise post processing needs. To avoid these
              postprocessing resolution issues, you can force the solution to use time steps that are
              no bigger than this parameter value.

       Solver Controls: for this analysis type, allows you to select a time integration algorithm
       (Runge-Kutta order 4 or 5) and select whether to use constraint stabilization. The default

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
86                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Preparing the Analysis

       time integration option, Runge-Kutta 4, provides the appropriate accuracy for most applica-
       tions. When constraint stabilization is employed, Stabilization Parameters are an automatic
       option. The default, Program Controlled is valid for most applications, however; you may
       wish to set this option to User Defined and manually enter customized settings for weak
       spring and damping effects. The default is Off.

       Nonlinear Controls (p. 269) allow you to modify convergence criteria and other specialized
       solution controls. Typically you will not need to change the default values for this control.

        •     Energy Accuracy Tolerance: This is the main driver to the automatic time stepping. The
              automatic time stepping algorithm measures the portion of potential and kinetic energy
              that is contained in the highest order terms of the time integration scheme, and computes
              the ratio of the energy to the energy variations over the previous time steps. Comparing
              the ratio to the Energy Accuracy Tolerance, Workbench will decide to increase or de-
              crease the time step.

                   Note

                   For systems that have very heavy slow moving parts, and also have small fast
                   moving parts, the portion of the energy contained in the small parts is not
                   dominant and therefore will not control the time step. It is recommended
                   that you use a smaller value of integration accuracy for the motion of the
                   small parts.

                   Spherical, slot and general joints with three rotation degrees of freedom
                   usually require a small time step, as the energy is varying in a very nonlinear
                   manner with the rotation degrees of freedom.


       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. In a transient nonlinear analysis it may be necessary to perform
       many solutions at intermediate time values. However i) you may not be interested in reviewing
       all of the intermediate results and ii) writing all the results can make the results file size un-
       wieldy. This group can be modified on a per step basis.

Define Initial Conditions

            Basic general information about this topic

             ... for this analysis type:

       Before solving, you can configure the joints and/or set a joint load to define initial conditions.

        1.     Define a Joint Load to set initial conditions on the free degrees of freedom of a joint.

               For the ANSYS Mechanical solver to converge, it is recommended that you ramp the
               angles and positions from zero to the real initial condition over one step. The ANSYS
               Rigid Dynamics solver does not need these to be ramped. For example, you can directly
               create a joint load for a revolute joint of 30 degrees, over a short step to define the
               initial conditions of the simulation. If you decide to ramp it, you have to keep in mind
               that ramping the angle over 1 second, for example, means that you will have a non-
               zero angular velocity at the end of this step. If you want to ramp the angle and start
               at rest, use an extra step maintaining this angle constant for a reasonable period of

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                              87
The Mechanical Application Approach

               time or, preferably, having the angular velocity set to zero. Another way to specify the
               initial conditions in terms of positions and angles is to use the Configure tool, which
               eliminates the time steps needed to apply the initial conditions.

               To fully define the initial conditions, you must define position and velocities. Unless
               specified by joint loads, if your system is initially assembled, the initial configuration
               will be unchanged. If the system is not initially assembled, the initial configuration will
               be the “closest” configuration to the unassembled configuration that satisfies the as-
               sembly tolerance and the joint loads.

               Unless specified otherwise, relative joint velocity is, if possible, set to zero. For example,
               if you define a double pendulum and specify the angular velocity of the grounded re-
               volute joint, by default the second pendulum will not be at rest, but will move rigidly
               with the first one.
        2.     Configure a joint to graphically put the joint in its initial position.

       See Joint Initial Conditions (p. 185) for further details.

Apply Loads and Supports

         Basic general information about this topic

             ... for this analysis type:

       For a transient structural (MBD) analysis there are no surface supports and loads except Inertial
       loads such as Acceleration and Standard Earth Gravity. Both Acceleration and Standard
       Earth Gravity must be constant throughout a transient structural (MBD) analysis and cannot
       be deactivated.

       All other loads are applied through Joint Loads. The joint condition’s magnitude could be
       a constant value or could vary with time as defined in a table or via a function. Details of
       how to apply a tabular or function load are described in Applying Tabular and Function
       Loads. Details on Joint Loads are included below.

       In addition, see the Apply Loads and Supports section for more information about time
       stepping and ramped loads.

Joint Load Interpolation/Derivation
       For joint loads applied through tabular data values, because the number of points input will
       very likely be less than the number of time steps required to solve the system, a cubic spline
       interpolation is performed, as shown on the following graph:




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
88                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                   Joint Load Interpolation/Derivation




Sometimes, the difference between the interpolated curve and the linear interpolation is
high, and the solution cannot proceed. In these cases, If your intent is to use the linear inter-
polation, you can simply use multiple time steps, as the interpolation is done only within a
time step.

When defining a joint load for a position and an angle, the corresponding velocities and ac-
celerations will be computed internally. When defining a joint load for a translational and
angular velocity, corresponding accelerations are also computed internally. By activating and
deactivating joint loads, you can generate some forces/accelerations/velocities, and position
discontinuities. Always consider what the implications of these discontinuities are for velocities
and accelerations. Force and acceleration discontinuities are perfectly valid physical situations.
No special attention is required to define these velocity discontinuities, that can, for example
be obtained by changing the slope of a relative displacement joint load on a translational
joint as shown on the following graph, using two time steps:




              Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                          of ANSYS, Inc. and its subsidiaries and affiliates.                                      89
The Mechanical Application Approach

       The corresponding velocity profile is shown here.




       This discontinuity of velocity is physically equivalent to a shock, and implies infinite acceler-
       ation if the change of slope is over a zero time duration. The ANSYS Rigid Dynamics solver
       will handle these discontinuities, and redistribute velocities after the discontinuity according
       to all active joint loads. This process of redistribution of velocities usually provides accurate
       results, however no shock solution is performed, and this process is not guaranteed to produce
       proper energy balance. A closer look at the total energy probe will tell you if the solution is
       valid. In case the redistribution is not done properly, use one step instead of two to use an
       interpolated, smooth position variation with respect to time.

       Discontinuities of positions and angles are not a physically acceptable situation. Results ob-
       tained in this case are very likely to make no physical sense. Workbench cannot detect this
       situation up front. If you proceed with position discontinuities, the solution either may abort,
       or, if it does solve completely, false results may be produced.

Joint Load Rotations
       For fixed axis rotations, it is possible to count a number of turns. For 3-D general rotations,
       it is not possible to count turns. In a single axis case, although it is possible to prescribe
       angles higher than 2π, it is not recommended because Workbench can lose count of the
       number of turns based on the way you ramp the angle. It is highly recommended that you
       use an angular velocity joint load instead of an angle value to ramp a rotation, whenever
       possible.

       For example, replace a rotation joint load designed to create a joint rotation from an angle
       from 0 to 720 degrees over 2 seconds by an angular velocity of 360 degrees/second. The
       second solution will always provide the right result, while the behavior of the first case can
       sometimes lead to the problems mentioned above.

       For 3-D rotations on a general joint for example, no angle over 2π can be handled. Use an
       angular velocity joint load instead.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
90                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Introduction

Multiple Joint Loads On The Same Joint
        When prescribing a position or an angle on a joint, velocities and acceleration are also pre-
        scribed. The use of multiple joint loads on the same joint motion can cause for joint loads
        to be determined inaccurately.

Solve

          Basic general information about this topic

           ... for this analysis type:

        Only synchronous solves are supported for transient structural (MBD) analyses.

Review Results

          Basic general information about this topic

           ... for this analysis type:

        Use a Solution Information object to track, monitor, or diagnose problems that arise during
        solution.

        Applicable results are Deformation and Probe results.

             Note

             If you highlight Deformation results in the tree that are scoped to rigid bodies,
             the corresponding rigid bodies in the Geometry window are not highlighted.

        To plot different results against time on the same graph or plot one result quantity against
        a load or another results item, use the Chart and Table (p. 383) feature.

        If you duplicate a transient structural (MBD) analysis, the results of the duplicated branch are
        also cleaned.

Transient Thermal Analysis
Introduction
Transient thermal analyses determine temperatures and other thermal quantities that vary over time. The
variation of temperature distribution over time is of interest in many applications such as with cooling of
electronic packages or a quenching analysis for heat treatment. Also of interest are the temperature distri-
bution results in thermal stresses that can cause failure. In such cases the temperatures from a transient
thermal analysis are used as inputs to a structural analysis for thermal stress evaluations.

Many heat transfer applications such as heat treatment problems, electronic package design, nozzles, engine
blocks, pressure vessels, fluid-structure interaction problems, and so on involve transient thermal analyses.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        91
The Mechanical Application Approach

Point to Remember
A transient thermal analysis can be either linear or nonlinear. Temperature dependent material properties
(thermal conductivity, specific heat or density), or temperature dependent convection coefficients or radiation
effects can result in nonlinear analyses that require an iterative procedure to achieve accurate solutions. The
thermal properties of most materials do vary with temperature, so the analysis usually is nonlinear.

Preparing the Analysis
Create Analysis System

          Basic general information about this topic

           ... for this analysis type:

From the Toolbox, drag the Transient Thermal template to the Project Schematic.

Define Engineering Data

          Basic general information about this topic

           ... for this analysis type:

       Thermal Conductivity, Density, and Specific Heat must be defined for a transient thermal
       analysis. Thermal Conductivity can be isotropic or orthotropic. All properties can be constant
       or temperature-dependent.

Attach Geometry

          Basic general information about this topic

           ... for this analysis type:

       There are no specific considerations for a transient thermal analysis.

Define Part Behavior

          Basic general information about this topic

           ... for this analysis type:

       There are no specific considerations for a transient thermal analysis.

Define Connections

          Basic general information about this topic

           ... for this analysis type:

       In a thermal analysis only contact is valid. Any joints or springs are ignored.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
92                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Preparing the Analysis

       With contact the initial status is maintained throughout the thermal analysis, that is, any
       closed contact faces will remain closed and any open contact faces will remain open for the
       duration of the thermal analysis. Heat conduction across a closed contact face is set to a
       sufficiently high enough value (based on the thermal conductivities and the model size) to
       model perfect contact with minimal thermal resistance. If needed, you can model imperfect
       contact by manually inputting a Thermal Conductance value.

Apply Mesh Controls/Preview Mesh

         Basic general information about this topic

          ... for this analysis type:

       There are no specific considerations for transient thermal analysis itself. However if the tem-
       peratures from this analysis are to be used in a subsequent structural analysis the mesh must
       be identical. Therefore in this case you may want to make sure the mesh is fine enough for
       a structural analysis.

Establish Analysis Settings

         Basic general information about this topic

          ... for this analysis type:

       For a transient thermal analysis the basic controls are:

       Step Controls (p. 266), used to: i) specify the end time of the transient analysis ii) control the
       time step size and iii) create multiple steps when needed.

       The rate of loading could be important in a transient thermal analysis if the material properties
       vary rapidly with temperature. When such nonlinearities are present it may be necessary to
       apply the loads in small increments and perform solutions at these intermediate loads to
       achieve convergence. Multiple steps are needed if you want to change the solution settings,
       for example, the time step size or the solution output frequency over specific time spans in
       the transient analysis.

       Output Controls (p. 270) allow you to specify the time points at which results should be
       available for postprocessing. A transient analysis involves calculating solutions at several time
       points in the load history. However: i) you may not be interested in all the intermediate results
       and ii) writing all the results can make the results file size unwieldy. In this case you can restrict
       the amount of output by requesting results only at certain time points.

       Nonlinear Controls (p. 269) allow you to modify convergence criteria and other specialized
       solution controls. Typically you will not need to change the default values for this control.

       Analysis Data Management (p. 277) settings enable you to save specific solution files from the
       transient thermal analysis for use in other analyses.

Define Initial Conditions

         Basic general information about this topic

          ... for this analysis type:

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              93
The Mechanical Application Approach

        A transient thermal analysis involves loads that are functions of time. The first step in applying
        transient thermal loads is to establish initial temperature distribution at Time = 0.

        The default initial condition for a transient thermal analysis is a uniform temperature of 22
        o
         C or 71.6 oF. You can change this to an appropriate value for your analysis. An example
        might be modeling the cooling of an object taken out of a furnace and plunged into water.

        You can also use the temperature results from a steady-state analysis of the same model for
        the initial temperature distribution. A casting solidification study might start with different
        initial temperatures for the mold and the metal. In this case a steady-state analysis of the
        hot molten metal inside the mold can serve as the starting point for the solidification analysis.

        In the first iteration of a transient thermal analysis, this initial temperature is used as the
        starting temperature value for the model except where temperatures are explicitly specified.
        In addition this temperature is also used to evaluate temperature-dependent material property
        values for the first iteration.

        If the Initial Temperature field is set to Non-Uniform Temperature, a Time field is displayed
        where you can specify a time at which the temperature result of the steady-state thermal
        analysis (selected in Initial Condition Environment field) will be used as the initial temper-
        ature in the transient analysis. A zero value will be translated as the end time (of the steady-
        state thermal analysis) and this value can not be greater than the end time.

Apply Loads and Supports

                Basic general information about this topic

                 ... for this analysis type:

        The following loads are supported in a transient thermal analysis:

            •     Temperature (p. 298)
            •     Convection (p. 298)
            •     Radiation (p. 300)
            •     Heat Flow (p. 300)
            •     Perfectly Insulated (p. 302)
            •     Heat Flux (p. 302)
            •     Internal Heat Generation (p. 303)
            •     CFD Imported Temperature (p. 314)
            •     CFD Imported Convection (p. 314)

        In this analysis, the load’s magnitude could be a constant value or could vary with time as
        defined in a table or via a function. Details of how to apply a tabular or function load are
        described in Applying Tabular and Function Loads. In addition, see the Apply Loads and
        Supports section for more information about time stepping and ramped loads.

Solve

                Basic general information about this topic



                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
94                                                      of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    2-D Analyses


           ... for this analysis type:

       The Solution Information object provides some tools to monitor solution progress.

       Solution Output continuously updates any listing output from the solver and provides
       valuable information on the behavior of the structure during the analysis. Any convergence
       data output in this printout can be graphically displayed as explained in the Solution Inform-
       ation section.

       You can also insert a Result Tracker object under Solution Information. This tool allows
       you to monitor temperature at a vertex as the solution progresses.

Review Results

          Basic general information about this topic

           ... for this analysis type:

       Applicable results are all thermal result types.

       Once a solution is available you can contour the results or animate the results to review the
       response of the structure.

       As a result of a nonlinear analysis you may have a solution at several time points. You can
       use probes to display the variation of a result item over the load history. Also of interest is
       the ability to plot one result quantity (for example, average temperature on a face) against
       another results item (for example, applied heat generation rate). You can use the Charts
       feature to develop such charts.

       Note that Charts are also useful to compare results between two analyses of the same model.

Special Analysis Topics
This section includes special topics available the Mechanical application for particular applications. The fol-
lowing topics are included:
 2-D Analyses
 Using Generalized Plane Strain
 Using Symmetry
 Static Analysis From Transient Structural (MBD) Analysis
 Fluid-Structure Interaction (FSI)

2-D Analyses
The Mechanical application has a provision that allows you to run structural and thermal problems that are
strictly two-dimensional (2-D). For models and environments that involve negligible effects from a third di-
mension, running a 2-D simulation can save processing time and conserve machine resources.

You can configure Workbench for a 2-D analysis by first creating or opening a surface body model in
DesignModeler, or in any supported CAD system that has provisions for surface bodies (Autodesk Mechan-
ical Desktop does not support surface bodies). The model must be in the x-y plane. 2-D planar bodies are
supported, 2-D wire bodies are not. Then, with the Geometry cell selected in the Project Schematic, expose
the Properties Details of Geometry window using the toolbar Workspace drop-down menu, and choose
2-D in the Analysis Type drop-down menu (located under Advanced Geometry Defaults). Attach the

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        95
The Mechanical Application Approach

model into the Mechanical application by double-clicking on the Model cell. You can specify a 2-D analysis
only when you attach the model. After attaching, you cannot change from a 2-D analysis to a 3-D analysis
or vice versa.

A 2-D analysis has the following characteristics:

 •   For Geometry items in the tree, you have the following choices located in the 2D Behavior field
     within the Details view:
     –   Plane Stress (default): Assumes zero stress and non-zero strain in the z direction. Use this option
         for structures where the z dimension is smaller than the x and y dimensions. Example uses are flat
         plates subjected to in-plane loading, or thin disks under pressure or centrifugal loading. A Thickness
         field is also available if you want to enter the thickness of the model.
     –   Axisymmetric: Assumes that a 3-D model and its loading can be generated by revolving a 2-D
         section 360o about the y-axis. The axis of symmetry must coincide with the global y-axis. The geometry
         has to lie on the positive x-axis of the x-y plane. The y direction is axial, the x direction is radial, and
         the z direction is in the circumferential (hoop) direction. The hoop displacement is zero. Hoop strains
         and stresses are usually very significant. Example uses are pressure vessels, straight pipes, and shafts.
         Axisymmetric behavior cannot be used in a shape optimization analysis.
     –   Plane Strain: Assumes zero strain in the z direction. Use this option for structures where the z di-
         mension is much larger than the x and y dimensions. The stress in the z direction is non-zero. Example
         uses are long, constant, cross-sectional structures such as structural line bodies. Plane Strain beha-
         vior cannot be used in a thermal analysis (steady-state or transient) or a shape optimization analysis.

              Note

              Since thickness is infinite in plane strain calculations, different results (displace-
              ments/stresses) will be calculated for extensive loads (that is, forces/heats) if the solution
              is performed in different unit systems (MKS vs. NMM). Intensive loads (pressure, heat flux)
              will not give different results. In either case, equilibrium is maintained and thus reactions
              will not change. This is an expected consequence of applying extensive loads in a plane
              strain analysis. In such a condition, if you change the Mechanical application unit system
              after a solve, you should clean the result and solve again.


     –   Generalized Plane Strain: Assumes a finite deformation domain length in the z direction, as opposed
         to the infinite value assumed for the standard Plane Strain option. Generalized Plane Strain
         provides more practical results for deformation problems where a z direction dimension exists, but
         is not considerable. See Using Generalized Plane Strain (p. 97) for more information.

         Generalized Plane Strain needs the following three types of data:
         ¡ Fiber Length: Sets the length of the extrusion.
         ¡ End Plane Rotation About X: Sets the rotation of the extrusion end plane about the x-axis.
         ¡ End Plane Rotation About Y: Sets the rotation of the extrusion end plane about the y-axis.
     –   By Body: Allows you to set the Plane Stress (with Thickness option), Plane Strain, or Axisymmetric
         options for individual bodies that appear under Geometry in the tree. If you choose By Body, then
         click on an individual body, these 2-D options are displayed for the individual body.
 •   For a 2-D analysis, use the same procedure for applying loads and supports as you would use in a 3-D
     analysis. The loads and results are in the x-y plane and there is no z component.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
96                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                         Using Generalized Plane Strain

 •     You can apply all loads and supports in a 2-D analysis except for the following: Bolt Pretension Load,
       Line Pressure, Simply Supported, and Fixed Rotation.
 •     A Pressure load can only be applied to an edge.
 •     A Bearing Load and a Cylindrical Support can only be applied to a circular edge.
 •     For analyses involving axisymmetric behavior, a Rotational Velocity load can only be applied about the
       y-axis.
 •     For loads applied to a circular edge, the direction flipping in the z axis will be ignored.

Using Generalized Plane Strain
The generalized plane strain feature can be used in structural, modal, and linear buckling analyses. Stepped
analyses and Shape optimizations are not supported. The feature assumes a finite deformation domain
length in the z direction, as opposed to the infinite value assumed for standard plane strain. It provides a
more efficient way to simulate certain 3-D deformations using 2-D options.

The deformation domain or structure is formed by extruding a plane area along a curve with a constant
curvature, as shown below.
                 Y




                       Starting Plane




                                                      Starting Point



Ending Plane




                                                                X


                                    Fiber Direction




                 Ending Point


          Z




The extruding begins at the starting (or reference) plane and stops at the ending plane. The curve direction
along the extrusion path is called the fiber direction. The starting and ending planes must be perpendicular
to this fiber direction at the beginning and ending intersections. If the boundary conditions and loads in
the fiber direction do not change over the course of the curve, and if the starting plane and ending plane
remain perpendicular to the fiber direction during deformation, then the amount of deformation of all cross
sections will be identical throughout the curve, and will not vary at any curve position in the fiber direction.
Therefore, any deformation can be represented by the deformation on the starting plane, and the 3-D de-
formation can be simulated by solving the deformation problem on the starting plane. The Plane Strain
and Axisymmetric options are particular cases of the Generalized Plane Strain option.

All inputs and outputs are in the global Cartesian coordinate system. The starting plane must be the x-y
plane, and must be meshed. The applied nodal force on the starting plane is the total force along the fiber
length. The geometry in the fiber direction is specified by the rotation about the x-axis and y-axis of the
ending plane, and the fiber length passing through a user-specified point on the starting plane called the
starting or reference point. The starting point creates an ending point on the ending plane through the ex-
trusion process. The boundary conditions and loads in the fiber direction are specified by applying displace-
ments or forces at the ending point.

The fiber length change is positive when the fiber length increases. The sign of the rotation angle or angle
change is determined by how the fiber length changes when the coordinates of the ending point change.
If the fiber length decreases when the x coordinate of the ending point increases, the rotation angle about
y is positive. If the fiber length increases when the y coordinate of the ending point increases, the rotation
angle about x is positive.

                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                        of ANSYS, Inc. and its subsidiaries and affiliates.                                         97
The Mechanical Application Approach

For linear buckling and modal analyses, the Generalized Plane Strain option usually reports fewer Eigen-
values and Eigenvectors than you would obtain in a 3-D analysis. Because it reports only homogenous de-
formation in the fiber direction, generalized plane strain employs only three DOFs to account for these de-
formations. The same 3-D analysis would incorporate many more DOFs in the fiber direction.

Because the mass matrix terms relating to DOFs in the fiber direction are approximated for modal and
transient analyses, you cannot use the lumped mass matrix for these types of simulations, and the solution
may be slightly different from regular 3-D simulations when any of the three designated DOFs is not restrained.

 Overall steps to using Generalized Plane Strain
 1.   Attach a 2-D model in the Mechanical application.
 2.   Click on Geometry in the tree.
 3.   In the Details view, set 2D Behavior to Generalized Plane Strain.
 4.   Define extrusion geometry by providing input values for Fiber Length, End Plane Rotation About
      X, and End Plane Rotation About Y.
 5.   Add a Generalized Plane Strain load under the analysis type object in the tree.

           Note

           The Generalized Plane Strain load is applied to all bodies. There can be only one Gener-
           alized Plane Strain load per analysis type so this load will not be available in any of the
           load drop-down menu lists if it has already been applied.


 6.   In the Details view, input the x and y coordinates of the reference point , and set the boundary condi-
      tions along the fiber direction and rotation about the x and y-axis.
 7.   Add any other loads or boundary conditions that are applicable to a 2-D model.
 8.   Solve. Reactions are reported in the Details view of the Generalized Plane Strain load.
 9.   Review results.

Using Symmetry
You can use the inherent geometric symmetry of a body to model only a portion of the body for simulation.
Using symmetry provides the benefits of faster solution times and less use of system resources. For example,
a rectangular shell under a uniform normal pressure can be simplified by modeling only ¼ of the geometry
by taking advantage of two symmetry planes. This section addresses the following topics on using symmetry:
 Introduction
 Types of Symmetry
 Working With Symmetry Defined in DesignModeler
 Defining Symmetry in the Mechanical Application
 Periodicity Example
 Symmetry in Explicit Dynamics

Introduction
Making use of the Symmetry feature requires an understanding of the geometry symmetry and the symmetry
of loading and boundary conditions. If geometric symmetry exists, and the loading and boundary conditions
are suitable, then the model can be simplified to just the symmetry sector of the model.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
98                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Using Symmetry

DesignModeler can be used to simplify a full model into a symmetric model. This is done by identifying
symmetry planes in the body. DesignModeler will then slice the full model and retain only the symmetry
portion of the model. (See Symmetry in the DesignModeler help).

When the Mechanical application attaches to a symmetry model from DesignModeler, a Symmetry folder
is placed in the tree and each Symmetry Plane from DesignModeler is given a Symmetry Region object
in the tree. In addition, Named Selection objects are created for each symmetry edge or face. (See Working
With Symmetry Defined in DesignModeler (p. 101).)

The Symmetry folder supports Symmetry Region objects and Periodic Region objects. Symmetry regions
are supported for structural and magnetostatic analyses. Periodic regions are supported for magnetostatic
analyses only.

For models generated originally as symmetry models, you may create a Symmetry folder and manually
identify Symmetry Region objects or Periodic Region objects. (See Defining Symmetry in the Mechanical
Application (p. 102).)

Types of Symmetry
The following types of symmetry are addressed in this section:
 Structural Symmetry
 Structural Anti-Symmetry
 Electromagnetic Symmetry
 Electromagnetic Anti-Symmetry
 Electromagnetic Periodicity
 Electromagnetic Anti-Periodicity

Structural Symmetry
A symmetric structural boundary condition means that out-of-plane displacements and in-plane rotations
are set to zero. The following figure illustrates a symmetric boundary condition. Structural symmetry is ap-
plicable to solid and surface bodies.




Structural Anti-Symmetry
An anti-symmetric boundary condition means that the rotation normal to the anti-symmetric face is con-
strained. The following figure illustrates an anti-symmetric boundary condition. Structural anti-symmetry is
applicable to solid and surface bodies.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                          99
The Mechanical Application Approach




      Note

      The Anti-Symmetric option does not prevent motion normal to the symmetry face. This is appro-
      priate if all loads on the structure are in-plane with the symmetry plane. If applied loads, or loads
      resulting from large deflection introduce force components normal to the face, an additional load
      constraint on the normal displacement may be required.

Electromagnetic Symmetry
Symmetry conditions exist for electromagnetic current sources and permanent magnets when the sources
on both sides of the symmetry plane are of the same magnitude and in the same direction as shown in the
following example.




Electromagnetic symmetric conditions imply Flux Normal boundary conditions, which are naturally satisfied.

Electromagnetic Anti-Symmetry
Anti-Symmetry conditions exist for electromagnetic current sources and permanent magnets when the
sources on both sides of the symmetry plane are of the same magnitude but in the opposite direction as
shown in the following example.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
100                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Using Symmetry




Electromagnetic anti-symmetric conditions imply Flux Parallel boundary conditions, which you must apply
to selected faces.

Electromagnetic Periodicity
A model exhibits angular periodicity when its geometry and sources occur in a periodic pattern around
some point in the geometry, and the repeating portion that you are modeling represents all of the sources,
as shown below.




Electromagnetic Anti-Periodicity
A model exhibits angular anti-periodicity when its geometry and sources occur in a periodic pattern around
some point in the geometry and the repeating portion that you are modeling represents a subset of all of
the sources, as shown below.




Working With Symmetry Defined in DesignModeler
 1.   While in DesignModeler, from the Tools menu, apply the Symmetry feature to the model or define
      an Enclosure.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         101
The Mechanical Application Approach

 2.   Enter the Mechanical application by double-clicking on the Model cell in the Project Schematic. The
      Mechanical application screen appears and includes the following objects in the tree:
      •    A Symmetry object.
      •    Symmetry Region objects displayed under the Symmetry folder. The number of Symmetry Region
           objects corresponds to the number of symmetry planes you defined in DesignModeler.
      •    A Named Selections folder object. Each child object displayed under this folder replicates the
           enclosure named selections that were automatically created when you started the Mechanical ap-
           plication.
 3.   In the Details view of each Symmetry Region object, under Definition, specify the type of symmetry
      by first clicking on the Type field, then choosing the type from the drop down list. Boundary conditions
      will be applied to the symmetry planes based on both the simulation type and what you specify in
      the symmetry Type field. The Scope Mode read-only indication is Automatic when you follow this
      procedure of defining symmetry in DesignModeler. The Coordinate System and Symmetry Normal
      fields include data that was “inherited” from DesignModeler. You can change this data if you wish.
      The Symmetry Normal entry must correspond to the Coordinate System entry.

Defining Symmetry in the Mechanical Application
 1.   Insert a Symmetry object in the tree.
 2.   Insert a Symmetry Region object or a Periodic Region object (applicable only to electromagnetic
      analyses) to represent each symmetry plane you want to define. Refer to Types of Symmetry (p. 99) to
      determine which object to insert.
 3.   For each Symmetry Region object or Periodic Region object, complete the following in the Details
      view:
      a.    Scoping Method - Perform one of the following:
            •   Choose Geometry Selection if you want to define a symmetry plane by picking in the Geo-
                metry window. Pick the geometry, then click on the entry field for Geometry Selection (labeled
                No Selection) and click the Apply button. For a Periodic Region object, perform the same
                procedure for the Periodic Low and Periodic High entries, where Periodic Low and Periodic
                High represent the two opposite face selections or edge selections on the different sides of
                the periodic sector of the model.

                     Note

                     A Symmetry Region object can only be scoped to a flexible body.


            •   Choose Named Selection if you want to define a symmetry plane using geometry that was
                pre-defined in a named selection. Click on the entry field for Named Selection and, from the
                drop down list, choose the particular named selection to represent the symmetry plane. For
                a Periodic Region object, you perform the same procedure, where Named Selection corres-
                ponds to the Periodic Low component and Other Selection corresponds to the Periodic
                High component.
      b.    Type - Click on the entry field, and, from the drop down list, choose the symmetry type. Boundary
            conditions will be applied to the symmetry planes based on both the simulation type and the
            value you specify in the symmetry Type field. The Scope Mode read-only indication is Manual
            when you follow this procedure of defining symmetry directly in the Mechanical application.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
102                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Using Symmetry


               Note

               When using a Periodic Region with Periodic and Anti-Periodic types, the mesher will
               automatically set up match face meshing on the opposite periodic faces.


     c.   Coordinate System - Select an appropriate coordinate system from the drop down list. You must
          use a Cartesian coordinate system for a Symmetry Region and a cylindrical coordinate system
          for a Periodic Region. See the Coordinate Systems section, Initial Creation and Definition, for the
          steps to create a local coordinate system.
     d.   Symmetry Normal - For a Symmetry Region object only, specify the normal axis from the drop
          down list that corresponds to the coordinate system that you chose.

The following example shows a body whose Symmetry Region was defined in the Mechanical application.




    Note

    You can select multiple faces to work with a symmetry region. For non-periodic symmetry regions,
    all faces selected (or chosen through Named Selection folder) must have only one normal. For
    periodic types, you should additionally choose the proper cylindrical coordinate system with the
    z-axis showing the rotation direction, similar to the Matched Face Mesh meshing option.

The following example shows a body whose Periodic Region was defined in the Mechanical application.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         103
The Mechanical Application Approach




      Warning

      For a magnetic field simulation with periodic regions, you must be careful when applying flux
      parallel boundary conditions to adjoining faces. With a periodic region, the net flux across the
      periodic faces must not be zero. If all adjacent faces to the periodic region are set to flux parallel,
      a net zero flux will be forced, leading to a non-physical solution. The figure below shows the
      adjacent faces to a periodic region. The simulation is properly posed if at least one of these faces
      does not have a flux parallel boundary condition.




Periodicity Example
Periodicity is illustrated in the following example. A coil, arrangement consists of 4 coils. A ½ symmetry
model of surrounding air is created. The model is conveniently broken into 8 octants for easy sub-division
into periodic sectors and for comparison of results.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
104                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Using Symmetry

Below is a display of the Magnetic Field Intensity for the ½ symmetry model at the mid-plane. The arrows
clearly indicate an opportunity to model the domain for both Periodic or Anti-periodic sectors. Periodic
planes are shown to exist at 180 degree intervals. Anti-perioidc planes are shown to exist at 90 degree inter-
vals.




The model can be cut in half to model Periodic planes. Applying periodic symmetry planes at 90 degrees
and 270 degrees leads to the following results.




The model can be cut in half again to model Anti-Periodic planes. Applying anti-periodic symmetry planes
at 0 degrees and 90 degrees leads to the following results.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         105
The Mechanical Application Approach

Symmetry in Explicit Dynamics
Symmetry regions can be defined in explicit dynamics analyses. Symmetry objects should be scoped to faces
of flexible bodies defined in the model. All nodes lying on the plane, defined by the selected face will be
constrained to give a symmetrical response of the structure.

      Note
       •   Anti-symmetry, periodicity and anti-periodicity symmetry regions are not supported in Explicit
           Dynamics (ANSYS) systems.
       •   Symmetry cannot be applied to rigid bodies.


Symmetry conditions can be interpreted by the solver in two ways:
 General Symmetry
 Global Symmetry Planes

General Symmetry
In general, a symmetry condition will result in degree of freedom constraints being applied to the nodes on
the symmetry plane. For volume elements, the translational degree of freedom normal to the symmetry
plane will be constrained. For shell and beam elements, the rotational degrees of freedom in the plane of
symmetry will be additionally constrained.

For nodes which have multiple symmetry regions assigned to them (for example, along the edge between
two adjacent faces), the combined constraints associated with the two symmetry planes will be enforced.

      Note
       •   Symmetry regions defined with different local coordinate systems may not be combined,
           unless they are orthogonal with the global coordinate system.
       •   General symmetry does not constrain eroded nodes. Thus, if after a group of elements erodes,
           a “free” eroded node remains, the eroded node will not be constrained by the symmetry
           condition. This can be resolved in certain situations via the special case of Global symmetry,
           described in the next section.


Global Symmetry Planes
If a symmetry object is aligned with the Cartesian planes at x=0, y=0 or z=0, and all nodes in the model are
on the positive side of x=0, y=0, or z=0, the symmetry condition is interpreted as a special case termed
Global symmetry plane. In addition to general symmetry constraints:

 •    If a symmetry plane is coincident with the YZ plane of the global coordinate system (Z=0), and no parts
      of the geometry lie on the negative side of the plane, then a symmetry plane is activated at X=0. This
      will prevent any nodes (including eroded nodes) from moving through the plane X=0 during the ana-
      lysis.
 •    If a symmetry plane is coincident with the ZX plane of the global coordinate system (Y=0), and no parts
      of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Y=0. This
      will prevent any nodes (including eroded nodes) from moving through the plane Y=0 during the ana-
      lysis.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
106                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Point to Remember

 •    If a symmetry plane is coincident with the XY plane of the global coordinate system (Z=0), and no parts
      of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Z=0. This
      will prevent any nodes (including eroded nodes) from moving through the plane Z=0 during the ana-
      lysis.

Static Analysis From Transient Structural (MBD) Analysis
You can perform a Transient Structural (MBD) Analysis (p. 84) and then change it to a Transient Structural
(ANSYS) Analysis (p. 76) for the purpose of determining deformation, stresses, and strains - which are not
available in the MBD analysis.

Creating an Analysis System
 1.    From the toolbox, drag and drop a transient structural (MBD) template onto the project schematic.
       Follow the procedure for creating a transient structural (MBD) analysis. Apply forces and/or drivers,
       and insert any valid solution result object(s).
 2.    Specify the time of interest in the tabular data table or in the Graph window.
 3.    Select a solution result object and click the right mouse to display the popup menu. Select Export
       Motion Loads and specify a load file name.
 4.    In the project schematic, duplicate the transient structural (MBD) analysis system. Replace the duplicated
       analysis system with a static structural (ANSYS) analysis system.

            Note

            If you do not need to keep the original MBD analysis, you can replace it with the static
            structural (ANSYS) analysis system.



 5.    Edit the static structural (ANSYS) analysis (using Model, Edit) by suppressing all parts except the desired
       part for the static structural analysis.
 6.    Change the stiffness behavior of the part to be analyzed from Rigid to Flexible.
 7.    Change mesh solver preference to be ANSYS Mechanical instead of ANSYS Rigid Dynamics.
 8.    Delete or suppress all loads used in the transient structural (MBD) analysis.
 9.    Import the motion loads that were exported from the transient structural (MBD) analysis. Highlight
       the static structural branch and then right mouse click, Insert> Motion Loads....

            Note

            Moments and forces created for the static structural analysis can be in an invalid state if all
            three components of the force/moment are almost equal to zero.


 10. Delete the result objects and add new ones.
 11. Solve the single part model with the static structural analysis and evaluate the results.

Point to Remember
It is important that you create the static structural (ANSYS) analysis after the transient structural (MBD) ana-
lysis is finished and the export load is done.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            107
The Mechanical Application Approach

Fluid-Structure Interaction (FSI)
Fluid-Structure Interaction (FSI) analysis is an example of a multiphysics problem where the interaction
between two different analyses is taken into account. The FSI analysis in the Mechanical application involves
performing a structural or thermal analysis in the Mechanical application taking into account the interaction
with the corresponding fluid or previous CFD analysis. The interaction between the two analyses typically
takes place at the boundary of the Mechanical application model - the fluid-structure interface, where the
results of one analysis is passed to the other analysis as a load.

The Mechanical application supports two types of Fluid-Structure Interaction:

One way FSI: The result (forces or temperature or convection load) from a CFD analysis at the fluid-structure
interface is applied as a load to the Mechanical application analysis. The boundary displacement from the
Mechanical application is not passed back to the CFD analysis, that is, the result from the Mechanical applic-
ation is not considered to have significant impact on the fluid analysis to calculate thermal stress, but the
resulting mesh displacements are too small to be significant enough to consider.

Two way FSI: In this analysis the results of structural analysis in the Mechanical application is transferred to
the ANSYS CFX analysis as a load. Similarly the results of the ANSYS CFX analysis are passed back to the
Mechanical application analysis as a load. For example, the fluid pressure at the boundary can be applied
as a load on the structural analysis in the Mechanical application and the resulting displacement, velocity
or acceleration obtained in the Mechanical application could be passed on as a load to the ANSYS CFX fluid
analysis. The analyses will continue until overall equilibrium is reached between the Mechanical application
solution and ANSYS CFX solution. Two way FSI is only supported between ANSYS and CFX solvers.

Typical applications of FSI include:

 •    Biomedical applications, such as drug delivery pumps, intravenous catheters, elastic artery modeling
      for stent design.
 •    Aerospace applications, such as airfoil flutter and turbine engines.
 •    Automotive applications, such as under hood cooling, HVAC heating/cooling, and heat exchangers.
 •    Fluid handling applications, such as valves, fuel injection components, and pressure regulators.
 •    Civil engineering applications, such as wind and fluid loading of structures.
 •    Electronics cooling.

Fluid-Structure Interaction (FSI) - One Way Transfer
This feature enables you to import fluid forces, temperatures, and convections from a steady-state or transient
CFD analysis into a the Mechanical application analysis.

This one way transfer of face forces (tractions) at a fluid-structure interface allows you to investigate the effects
of fluid flow in a static or transient structural (ANSYS) analysis. Similarly the one way transfer of temperatures
or convection information from a CFD analysis can be used in determining the temperature distribution on
a structure in a steady-state or transient thermal analysis.

After the solution is complete, a CFD Load Transfer Summary is displayed as a Comment in the particular
CFD load branch. The summary contains the following information:

 •    For a CFD Pressure load: the net force, due to shear stress and normal pressure, on the face computed
      in CFD and the net force transferred to the Mechanical application faces.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
108                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  Fluid-Structure Interaction (FSI)

 •   For a CFD Temperature load: the average computed temperature on the CFD boundary and the corres-
     ponding average mapped temperature on the Mechanical application faces.
 •   For a CFD Convection load: the total heat flow across the face, and the average film coefficient and
     ambient temperature on the face.

The computed and mapped face data may be compared in order to get a qualitative assessment of the ac-
curacy of the mapped data. The following is an example of a CFD Load Transfer Summary for a CFD Pressure
load.




     Note

     The force values shown in the CFD Load Transfer Summary should only be used as a qualitative
     measure of the load transferred from CFD to the Mechanical application mesh. In the example
     above, the closer the CFD Computed forces are to the Mechanical application Mapped Forces,
     the better the mapping. The actual force transferred to the Mechanical application is reflected in
     the reaction forces.

The following topics are covered in this section:
 Face Forces at Fluid-Structure Interface
 Face Temperatures and Convections at Fluid-Structure Interface
 CFD Results Mapping

Face Forces at Fluid-Structure Interface
You can use results at a fluid-structure interface from a CFD analysis as face forces (from the vector sum of
the normal pressures and shear stresses) on corresponding faces in the Mechanical application. The import
process involves interpolating a CFD solution onto the Mechanical application face mesh. This requires that
the following conditions are met:

 •   The fluid-structure interface must be a defined boundary in CFD.
 •   The location of the CFD boundary (with respect to the global Cartesian coordinate system) must be the
     same as the corresponding face(s) in the Mechanical application model.

Refer to the Imported Loads (p. 325) section for more information.

Face Temperatures and Convections at Fluid-Structure Interface
This feature allows the transfer of either of the following thermal solutions from a CFD solution boundary
to a corresponding face in the Mechanical application model:

 •   Temperatures at the fluid-structure interface.
 •   Film coefficients and bulk temperature values at the fluid-structure interface.

The import process involves interpolating an CFD solution onto the Mechanical application face mesh. This
requires that the following conditions are met:

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                          109
The Mechanical Application Approach

 •    The fluid-structure interface must be a defined boundary in CFD.
 •    The location of the CFD boundary (with respect to the global Cartesian coordinate system) must be the
      same as the corresponding face(s) in the Mechanical application model.

Refer to the Imported Loads section for more information.

CFD Results Mapping
When mapping CFD results onto the Mechanical application face(s) the Mechanical nodes are projected on
to the CFD face. All the Mechanical application face nodes will map to the CFD face according to the following
rules:

 a.    Project normal to the CFD mesh faces.
 b.    If rule a fails, project to the closest edge.
 c.    If rule b. fails, project to the closest node on the CFD face.

Rule c. will always work, so in the end every node will get some kind of mapping. However the most accurate
load mapping occurs for nodes projected normal to the mesh face. The percentage of the Mechanical ap-
plication nodes that mapped successfully using rule a. above is reported in the diagnostics. When the
Mechanical application mesh is very coarse, there can be some misses near the edges of the CFD boundary.
However all nodes become mapped eventually. The accuracy of force transfer improves as the Mechanical
application mesh is refined.

Load Transfer Summary

To provide some feedback on how well the mapped loads match the CFD solution, images of both CFD
solution and the mapped load values are created. In addition a CFD Load Transfer Summary is also created
that shows the net loading on the face computed in CFD and the net loading transferred to the Mechanical
application faces. Refer to Imported Loads for further information.

Fluid-Structure Interaction (FSI) - Two Way Transfer
This feature enables you to perform a two way fluid structure interaction problem by setting up the static
or transient structural (ANSYS) portion of the analysis in the Mechanical application that includes defining
faces associated with the fluid-structure interface, continuing the analysis in CFD-Solve, and viewing the
structural results in the Mechanical application. Two way FSI is only supported between ANSYS and CFX
solvers.

Overall Workflow for FSI Analysis with Two Way Transfer
 1.    Perform all steps for a static structural or transient structural (ANSYS) analysis in the Mechanical applic-
       ation but do not solve the analysis in the Mechanical application.
       a.   Use the Fluid Solid Interface (p. 317) load to identify faces associated with the fluid-structure interface.
            You can define multiple interfaces, for example when different types of fluids are present in the
            CFD analysis you may want to individually identify the interface between each fluid and the cor-
            responding parts of the structure.
       b.   Specify mesh controls, boundary conditions, and solution settings as you normally would.
 2.    Highlight the Solution object folder and choose Tools> Write Input File... from the main menu.
 3.    Use ANSYS CFX-Pre to set up the CFD analysis as well as the multi-field analysis controls. The multi-
       field analysis controls define the loads transferred between ANSYS CFX and the Mechanical application
       as well as solution settings that define the conditions for an acceptable multi-field solution. More details

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
110                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Wizards

       can be found in “Using ANSYS CFX-Pre in the Mechanical APDL application Multi-field Mode” with in
       the ANSYS CFX-Pre Help.
 4.    Use CFX-Solver to solve the analysis. The procedure for using the input file created in step 2 is outlined
       in the CFX-Solver Modeling Guide under “Coupling ANSYS CFX to an External Solver”: ANSYS Multi-
       field the Mechanical applications> Pre-Processing> ANSYS Input File Specification. Typically the dis-
       placements from a the Mechanical application static or transient structural (ANSYS) solution are passed
       to ANSYS CFX to change the boundary of the CFX mesh. In turn the surface forces at the fluid-structure
       interface from the CFD solution are transferred to the Mechanical application as a load.
 5.    The above solution procedure creates the Mechanical APDL application results file (.rst file) for the
       Mechanical application portion of the analysis. The directory location of the Mechanical APDL application
       results file is determined by the ANSYS CFX-Solve setup. The directory location of the Mechanical APDL
       application solution is determined by the ANSYS CFX-Solve setup.
 6.    You can associate the above results file with your the Mechanical application model by highlighting
       the Solution object folder and choosing Tools> Read Results File... from the main menu. Browse to
       the folder that contains the result file (jobname.rst) and the error file (jobname.err). They will have a
       jobname of ”ANSYS”  .
 7.    Once associated, you can review the results of the two way FSI analysis on your the Mechanical applic-
       ation model.

Wizards
Wizards provide a layer of assistance above the standard user interface. They are made up of tasks or steps
that help you interpret and work with simulations. Conceptually, the wizards act as an agent between you
and the standard user interface.

Wizards include the following features:

 •    An interactive checklist for accomplishing a specific goal
 •    A reality check of the current simulation
 •    A list of a variety of high-level tasks, and guidance in performing the tasks
 •    Links to useful resources
 •    A series of Callout windows which provide guidance for each step

      Note

      Callouts close automatically, or you may click inside a Callout to close it.

Wizards use hyperlinks (versus command buttons) because they generally represent links to locations within
the standard user interface, to content in the help system, or to a location accessible by a standard HTML
hyperlink. The status of each step is taken in context of the currently selected Tree Outline (p. 118) object.
Status is continually refreshed based on the Outline state (not on an internal wizard state). As a result you
may:

 •    Freely move about the Tree Outline (p. 118) (including between branches).
 •    Make arbitrary edits without going through the wizards.
 •    Show or hide the wizards at any time.

Wizards are docked to the right side of the standard user interface for two reasons:


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                  111
The Mechanical Application Approach

 •    The Tree Outline (p. 118) sets the context for status determination. That is, the wizards interpret the
      Outline rather than control it. (The user interface uses a top-down left-right convention for expressing
      dependencies.)
 •    Visual symmetry is maintained.

To close wizards, click the . To show/hide tasks or steps, click the section header. Options for wizards are
set in the Wizard (p. 171) section of the Options dialog box under the Mechanical application.

The The Mechanical Wizard (p. 112) is available for your use in the Mechanical application.

The Mechanical Wizard

The Mechanical Wizard appears in the right side panel whenever you click the      in the toolbar. You can
close the Mechanical Wizard at any time by clicking   at the top of the panel. To show or hide the sections
of steps in the wizard, click the section header.

Features of the Mechanical Wizard
The Mechanical Wizard works like a web page consisting of collapsible groups and tasks. Click a group title
to expand or collapse the group; click a task to activate the task.

When activated, a task navigates to a particular location in the user interface and displays a callout with a
message about the status of the task and information on how to proceed. Activating a task may change
your tab selection, cursor mode, and Tree Outline (p. 118) selection as needed to set the proper context for
proceeding with the task.

You may freely click tasks to explore the Mechanical application. Standard tasks WILL NOT change any in-
formation in your simulation.

Callouts close automatically based on your actions in the software. Click inside a callout to close it manually.

Most tasks indicate a status via the icon to the left of the task name. Rest your mouse on a task for a descrip-
tion of the status. Each task updates its status and behavior based on the current Tree Outline (p. 118) selection
and software status.

Tasks are optional. If you already know how to perform an operation, you don't need to activate the task.

Click the Choose Wizard task at the top of the Mechanical Wizard to change the wizard goal. For example,
you may change the goal from Find safety factors to Find fatigue life. Changing the wizard goal does not
modify your simulation.

At your discretion, simulations may include any available feature not covered under Required Steps for a
wizard. The Mechanical Wizard does not restrict your use of the Mechanical application.

You may use the Mechanical Wizard with databases from previous versions of the Mechanical application.


To enable the Mechanical Wizard, click                     or select View> Windows> the Mechanical Wizard.

Types of the Mechanical Wizards
There are wizards that guide you through the following simulations:

 •    Safety factors, stresses and deformation

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
112                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                               Types of the Mechanical Wizards

•   Fatigue life and safety factor
•   Natural frequencies and mode shapes
•   Optimizing the shape of a part
•   Heat transfer and temperatures
•   Magnetostatic results
•   Contact region type and formulation




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      113
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
114                               of ANSYS, Inc. and its subsidiaries and affiliates.
The Mechanical Application Basics
 •   The Mechanical Application Interface
 •   Customizing the Mechanical Application

The Mechanical Application Interface
The following topics are covered in this section:
 The Mechanical Application Window
 Tree Outline Conventions
 Tree Outline
 Environment Filtering
 Interface Behavior Based on License Levels
 Suppress and Unsuppress Items
 Tabs
 Geometry
 Legend Functionality
 Graphical Selection
 Named Selections
 Details View
 Worksheet Tab
 Graph and Tabular Data Windows
 Parameters
 Toolbars
 Messages Window
 Workbench Windows Manager
 Print Preview
 Triad and Rotation Cursors

The Mechanical Application Window
The following is an example of the Mechanical application interface.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               115
The Mechanical Application Basics




The functional elements of the interface include the following.

Window Component                    Description
Main Menu                           This menu includes the basic menus such as File and Edit.
Standard Toolbar                    This toolbar contains commonly used application commands.
Graphics Toolbar                    This toolbar contains commands that control pointer mode or cause an action
                                    in the graphics browser.
Context Toolbar                     This toolbar contains task-specific commands that change depending on
                                    where you are in the Tree Outline.
Unit Conversion Toolbar             Not visible by default.This toolbar allows you to convert units for various
                                    properties.
Named Selection Toolbar             Not visible by default.This toolbar contains options to manage named selec-
                                    tions.
Tree Outline                        Outline view of the simulation project. Always visible. Location in the outline
                                    sets the context for other controls. Provides access to object's context menus.
                                    Allows renaming of objects. Establishes what details display in the Details
                                    View.
Details View                        The Details View corresponds to the Outline selection. Displays a details win-
                                    dow on the lower left panel of the Mechanical application window which
                                    contains details about each object in the Outline.
Geometry                            Displays and manipulates the visual representation of the object selected
                                    in the Outline. This window displays:

                                    •     3D Geometry
                                    •     2D/3D Graph
                                    •     Spreadsheet


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
116                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Status Symbols

Window Component                     Description
                                     •     HTML Pages

                                              Note

                                              The Geometry window may include splitter bars for dividing
                                              views.


Reference Help                       Opens an objects reference help page for the highlighted object.
Tabs                                 The document tabs that are visible on the lower right portion of the
                                     Mechanical application Window.
Status Bar                           Brief in-context tip. Selection feedback.
Splitter Bar                         Application window has up to 3 splitter bars.

Tree Outline Conventions
The Tree Outline uses the following conventions:

 •   A symbol to the left of an item's icon indicates that it contains associated subitems . Click to expand
     the item and display its contents.
 •   To collapse all expanded items at once, double-click the Project name at the top of the tree.
 •   Drag-and-drop function to move and copy objects.
 •   To delete a tree object from the Tree Outline (p. 118), right-click on the object and select Delete. A con-
     firmation dialog asks if you want to delete the object.

Status Symbols
A small status icon displays just to the left of the main object icon in the Tree Outline (p. 118)

Status Symbol Name           Symbol                                                   Example
Underdefined                                                                          A load requires a nonzero magnitude.
Error                                                                                 Load attachments may break during an Update.
Mapped Face or Match                                                                  Face could not be mapped meshed, or mesh
Control Failure                                                                       of face pair could not be matched.
Ok                                                                                    Everything is ok.
Needs to be Updated                                                                   Equivalent to "Ready to Answer!"
Hidden                                                                                A body or part is hidden.
Meshed                                                                                A part is meshed.The symbol appears only for
                                                                                      a meshed part or multibody part (not for the
                                                                                      individual bodies) within the Geometry folder.
Suppress                                                                              An object is suppressed.
Solve                                                                                 •    Yellow lightning bolt: Item has not yet
                                                                                           been solved.
                                                                                      •    Green lightning bolt: Solve in progress.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         117
The Mechanical Application Basics

Status Symbol Name            Symbol                                                   Example
                                                                                       •    Green check mark: Successful solution.
                                                                                       •    Red lightning bolt: Failed solution.
                                                                                       •    Green down arrow: Successful background
                                                                                            solution ready for download.
                                                                                       •    Red down arrow: Failed background solu-
                                                                                            tion ready for download.


See also Tree Outline (p. 118).

      Note

      The state of an environment folder can be similar to the state of a Solution folder. The solution
      state can indicate either solved (check mark) or not solved (lightening bolt) depending on
      whether or not an input file has been generated.


Tree Outline
The object Tree Outline matches the logical sequence of simulation steps. Object sub-branches relate to the
main object. For example, an analysis environment object, such as Static Structural, contains loads. You
can right-click on an object to open a context menu which relates to that object. You can rename objects,
provided the objects are not being solved. Refer to the Mechanical application objects reference pages for
more information.

      Note

      Numbers preceded by a space at the end of an object's name are ignored. This is especially crit-
      ical when you copy objects or duplicate object branches. For example, if you rename two force
      loads as Force 1 and Force 2, then copy the loads to another analysis environment, the copied
      loads will be named Force and Force 1. However, if you rename the loads as Force_1 and Force_2,
      the copied loads will retain the same names as the two original loads.


Environment Filtering
The Mechanical interface includes a filtering feature that only displays model-level items applicable to the
particular analysis type environments in which you are working. This provides a simpler and more focused
interface.

The environment filter has the following characteristics:

 •    Model-level objects in the tree that are not applicable to the environments under a particular model
      are hidden.
 •    The user interface inhibits the insertion of model-level objects that are not applicable to the environments
      of the model.
 •    Model-level object properties (in the Details view of objects) that are not applicable to the environments
      under the model are hidden.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
118                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       How to Suppress/Unsuppress an Item

The filter is enabled by default when you enter the Mechanical application. You can disable the filter by
highlighting the Model object, clicking the right mouse button, and choosing Disable Filter from the context
menu. To enable the filter, repeat this procedure but choose Auto Filter from the context menu. You can
also check the status of the filter by highlighting the Model object and in the Details view, noting whether
Control under Filter Options is set to Enabled or Disabled.

The filter control setting (enabled or disabled) is saved when the model is saved and returns to the same
state when the database is resumed.

Interface Behavior Based on License Levels
The licensing level that you choose automatically allows you to exercise specific features and blocks other
features that are not allowed. Presented below are descriptions of how the interface behaves when you at-
tempt to use features not allowed by a license level.

 •   If the licensing level does not allow an object to be inserted, it will not show in the Insert menus.
 •   If you open a database with an object that does not fit the current license level, the database changes
     to "read-only" mode.
 •   If a Details view option is not allowed for the current license level, it is not shown.
 •   If a Details view option is not allowed for the current license level, and was preselected (either through
     reopening of a database or a previous combination of settings) the Details view item will become invalid
     and shaded yellow.

     Note

     When you attempt to add objects that are not compatible with your current license level, the
     database enters a read-only mode and you cannot save data. However, provided you are using
     any license, you can delete the incompatible objects, which removes the read-only mode and
     allows you to save data and edit the database.


Suppress and Unsuppress Items
Several items in the Mechanical application tree outline can be suppressed, meaning that they can be indi-
vidually removed from any further involvement in the analysis. For example, suppressing a part removes
the part from the display and from any further loading or solution treatment.

How to Suppress/Unsuppress an Item
If available, set the Suppressed option in the Details view to Yes. Conversely, you can unsuppress items by
setting the Suppressed option to No.

You can also suppress/unsuppress these items through context menu options available via a right mouse
button click. Included is the context menu option Invert Suppressed Body Set, which allows you to reverse
the suppression state of all bodies (unsuppressed bodies become suppressed and suppressed bodies become
unsuppressed). You can suppress the bodies in a named selection using either the context menu options
mentioned above , or through the Named Selection Toolbar.

Another way to suppress a body is by selecting it in the graphics window, then using a right mouse button
click in the graphics window and choosing Suppress Body in the context menu. Conversely, the Unsuppress
All Bodies option is available for unsuppressing bodies. Options are also available in this menu for hiding



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                119
The Mechanical Application Basics

or showing bodies. Hiding a body only removes the body from the display. A hidden body is still active in
the analysis.

Tabs

The bottom of the browser pane in the application window contains the four main document tabs shown
above. The Worksheet tab is available when tabular, graphic, or text data concerning the object is available.

The tabs provide alternative views of the current Outline object. You can move among the Geometry (p. 120),
Worksheet Tab (p. 140), Print Preview (p. 163), and Report Preview (p. 494) at any time by clicking the tabs. The
Outline remains visible.

Geometry
The Geometry window displays the geometry model. All view manipulation, geometry selection and
graphics display of a model occurs in the Geometry window. The window contains:
 •    3D Graphics.
 •    A scale ruler.
 •    A legend and a triad control (when you display the solution).
 •    Contour results objects.

      Note

      When you insert a Comment, the Geometry window splits horizontally, and the HTML comment
      editor displays in the bottom of the window. The Geometry representation of the model displays
      at the top. For more information about editing comments, refer to the Comment object reference.


Legend Functionality
To view the legend, confirm that Legend is selected in the View menu. The legend is displayed in the top
left corner of the graphics window when you select an object in the tree outline. Note that the legend is
not accessible via any of the toolbars in any of the modules.

Repositioning Legend
To reposition the legend within the graphics window, select the legend with your mouse, hold down the
left mouse button and drag the mouse. Note that the multiple view window configuration does not allow
for the legend to be permanently saved in a unique location. Resumption of a database file and toggling
between a single view and multiple views will result in the legend being saved to its default position in the
upper left corner of the graphics window.

Discrete Legends in the Mechanical Application
 •    Geometry Legend: Contents is driven by Display Style selection in the Details view panel.
 •    Joint Legend: Depicts the free degrees of freedom characteristic of the type of joint.
 •    Results Legend: Content is accessible via the right mouse when the legend for a solved object in the
      Solution folder is selected.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
120                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Rotation Cursors for Display

Graphical Selection
Tips for working with graphics
 •    You can use the ruler, shown at the bottom of the Geometry window, to obtain a good estimate of the
      scale of the displayed geometry or results (similar to using a scale on a geographic map). The ruler is
      useful when setting mesh sizes.
 •    You can rotate the view in a geometry selection mode by dragging your middle mouse button. You
      can zoom in or out by rolling the mouse wheel.
 •    Hold the control key to add or remove items from a selection. You can paint select faces on a model by
      dragging the left mouse button.
 •    You can pan the view by using the arrow keys. You can rotate the view by using the control key and
      arrow keys.
 •    Click the interactive Triad and Rotation Cursors (p. 163) to quickly change the graphics view.
 •    Use the stack of rectangles in the lower left corner of the Geometry (p. 120) to select faces hidden by
      your current selection.
 •    To rotate about a specific point in the model, switch to rotate mode and click the model to select a
      rotation point. Click off the model to restore the default rotation point.
 •    To multi-select one or more faces, hold the CTRL key and click the faces you wish to select, or use Box
      Select to select all faces within a box. The CTRL key can be used in combination with Box Select to
      select faces within multiple boxes.
 •    Click the Viewports (p. 128) icon to view up to four images in the Geometry (p. 120) window.
 •    Controls are different for Graphs & Charts.

     Rotation Cursors for Display (p. 121)
     Pointer Modes (p. 122)
     Defining Direction (p. 122)
     Direction Defaults (p. 122)
     Highlighting Geometry in Select Direction Mode (p. 122)
     Selecting Direction by Face (p. 122)
     Selecting Direction Using the Triad and Rotation Cursors (p. 163)
     Highlighting (p. 123)
     Picking (p. 123)
     Blips (p. 123)
     Painting (p. 124)
     Depth Picking (p. 124)
     Selection Filters (p. 124)
     The Extend Selection Command (p. 125)
     The Select Command
     Viewports (p. 128)
     Graph Chart Control (p. 129)

Rotation Cursors for Display

   Activates rotational controls in the Geometry window (left mouse button). The cursor changes appearance
depending on its window location.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                          121
The Mechanical Application Basics

Pointer Modes
The pointer in the graphics window is always either in a picking filter mode or a view control mode. When
in a view control mode the selection set is locked. To resume the selection, repress a picking filter button.

The Graphics Toolbar offers several geometry filters and view controls as the default state, for example, face,
edge, rotate, and zoom.

If a Geometry field in the Details View (p. 134) has focus, inappropriate picking filters are automatically disabled.
For example, a pressure load can only be scoped to faces.

If the Direction field in the Details View (p. 134) has focus, the only enabled picking filter is Select Direction.
Select Direction mode is enabled for use when the Direction field has focus; you never choose Select
Direction manually. You may manipulate the view while selecting a direction. In this case the Select Direction
button allows you to resume your selection.

Defining Direction
Orientation may be defined by any of the following geometric selections:

 •    A planar face (normal to).
 •    A straight edge.
 •    Cylindrical or revolved face (axis of ).
 •    Two vertices.

Direction Defaults
If you insert a load on selected geometry that includes both a magnitude and a direction, the Direction
field in the Details view states a particular default direction. For example, a force applied to a planar face
by default acts normal to the face. One of the two directions is chosen automatically. The load annotation
displays the default direction.

Highlighting Geometry in Select Direction Mode
Unlike other picking filters (where one specific type of geometry highlights during selection) the Select
Direction filter highlights any of the following during selection:

 •    Planar faces
 •    Straight edges
 •    Cylindrical or revolved faces
 •    Vertices

If one vertex is selected, you must hold down the CTRL key to select the other. When you press the CTRL
key, only vertices highlight.

Selecting Direction by Face
The following figure shows the graphic display after choosing a face to define a direction. The same display
appears if you edit the Direction field later.

 •    The selection blip indicates the hit point on the face.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
122                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Blips

 •   Two arrows show the possible orientations. They appear in the lower left corner of the Geometry (p. 120)
     window.



     If either arrow is clicked, the direction flips.

When you finish editing the direction, the hit point (initially marked by the selection blip) becomes the default
location for the annotation. If the object has a location as well as a direction (e.g. Remote Force), the location
of the annotation will be the one that you specify, not the hit point.




     Note

     The scope is indicated by painting the geometry.

Highlighting
Highlighting provides visual feedback about the current pointer behavior (e.g. select faces) and location of
the pointer (e.g. over a particular face).

The face edges are highlighted in colored dots.




Picking
A pick means a click on visible geometry. A pick becomes the current selection, replacing previous selections.
A pick in empty space clears the current selection.

By holding the CTRL key down, you can add unselected items to the selection and selected items can be
removed from the selection. Clicking in empty space with CTRL depressed does not clear current selections.

Blips
A crosshair blip appears at the location where you release the mouse button:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                123
The Mechanical Application Basics




A blip serves to:

 •    Mark a picked point on visible geometry.
 •    Represent a ray normal to the screen passing through all hidden geometry.

      Note

      This is important for depth picking, a feature discussed below.

Blips disappear when you clear the selection or make another pick.

Painting
Painting means dragging the mouse on visible geometry to select more than one entity. A pick is a trivial
case of painting. Without holding the CTRL key down, painting picks all appropriate geometry touched by
the pointer.

Depth Picking
Depth Picking allows you to pick geometry through the Z-order behind the blip.

Whenever a blip appears above a selection, the graphics window displays a stack of rectangles in the lower
left corner. The rectangles are stacked in appearance, with the topmost rectangle representing the visible
(selected) geometry and subsequent rectangles representing geometry hit by a ray normal to the screen
passing through the blip, front to back. The stack of rectangles is an alternative graphical display for the
selectable geometry. Each rectangle is drawn using the same edge and face colors as its associated geometry.

Highlighting and picking behaviors are identical and synchronized for geometry and its associated rectangle.
Moving the pointer over a rectangle highlights both the rectangle its geometry, and vice versa. CTRL key
and painting behaviors are also identical for the stack. Holding the CTRL key while clicking rectangles picks
or unpicks associated geometry. Dragging the mouse (Painting (p. 124)) along the rectangles picks geometry
front-to-back or back-to-front.

Selection Filters
The mouse pointer in the graphics window is either in a picking filter mode or a view control mode. A depressed
button in the graphics toolbar indicates the current mode.

Filter       Behavior
Vertices     Vertices are represented by concentric circles about the same size as a blip.The circumference of
             a circle highlights when the pointer is within the circle.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
124                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                The Extend Selection Command

Filter     Behavior
Edges      Painting may be used to pick multiple edges or to "paint up to" an edge (to avoid tediously posi-
           tioning the pointer prior to clicking).
Faces      Allows selection of faces. Highlighting occurs by dotting the banding edges of the face.
Bodies     Picking and painting: select entire bodies. Highlighted by drawing a bounding box around the
           body.The stack shows bodies hidden behind the blip (useful for selecting contained bodies).

The Extend Selection Command
The Extend Selection drop-down menu is enabled only for edge or face selection mode and only with a
selection of one or more edges or faces. The following options are available in the drop-down menu:

•   Extend to Adjacent
    –    For faces, Extend to Adjacent searches for faces adjacent to faces in the current selection that meet
         an angular tolerance along their shared edge.




         Single face selected in part on the left.                   Additional adjacent faces selected after Extend to Ad-
                                                                     jacent option is chosen.

    –    For edges, Extend to Adjacent searches for edges adjacent to edges in the current selection that
         meet an angular tolerance at their shared vertex.




         Single edge selected in part on the left.                                             Additional adjacent edges selected after Extend t
                                                                                               Adjacent option is chosen.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   125
The Mechanical Application Basics

 •    Extend to Limits
      –   For faces, Extend to Limits searches for faces that are tangent to the current selection as well as
          all faces that are tangent to each of the additional selections within the part. The selections must
          meet an angular tolerance along their shared edges.




          Single face selected in part on the left.                   Additional tangent faces selected after Extend to Limits
                                                                      option is chosen.

      –   For edges, Extend to Limits searches for edges that are tangent to the current selection as well as
          all edges that are tangent to each of the additional selections within the part. The selections must
          meet an angular tolerance along their shared vertices.




          Single edge selected in part on the left.                              Additional tangent edges selected after Extend
                                                                                 to Limits option is chosen.

 •    Extend to Instances (available only if CAD pattern instances are defined in the model): When a CAD
      feature is repeated in a pattern, it produces a family of related topologies (for example, vertices, edges,
      faces, bodies) each of which is named an "instance". Using Extend to Instances, you can use one of
      the instances to select all others in the model.

      As an example, consider three parts that are instances of the same feature in the CAD system. First select
      one of the parts.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
126                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    The Select Command




     Then, choose Extend to Instances. The remaining two part instances are selected.




     See CAD Instance Meshing for further information.

For all options, you can modify the angle used to calculate the selection extensions in the Workbench Options
dialog box setting Extend Selection Angle Limit under Graphics Interaction.

The Select Command
The Select Mode toolbar button allows you to select items designated by the Selection Filters through the
Single Select or Box Select drop-down menu options.

 •   Single Select (default): Click on an item to select it.
 •   Box Select: Define a box that selects filtered items. When defining the box, the direction that you drag
     the mouse from the starting point determines what items are selected, as shown in the following figures:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                             127
The Mechanical Application Basics




      –   Dragging to the right to form the box selects entities that are completely enclosed by the box.
      –   Visual cue: 4 tick marks completely inside the box.




      –   Dragging to the left to form the box selects all entities that touch the box.
      –   Visual cue: 4 tick marks that cross the sides of the box.

You can use the CTRL key for multiple selections in both modes.

Viewports
The Viewports toolbar button allows you to split the graphics display into a maximum of four simultaneous
views. You can see multiple viewports in the Geometry (p. 120) window when any object in the tree is in focus
except Project. You can choose one, horizontal, vertical, or four viewports. Each viewport can have separate
camera angles, labels, titles, backgrounds, etc. Any action performed when viewports are selected will occur
only to the active viewport. For example, if you animate a viewport, only the active viewport will be animated,
and not the others.




A figure can be viewed in a single viewport only. If multiple viewports are created with the figure in focus,
all other viewports display the parent of the figure.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
128                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Named Selections


      Note

      Each viewport has a separate Slice tool, and therefore separate Slice Plane. The concept of copying
      a Slice Plane from one window to the next does not exist. If you want Slice Planes in a new window,
      you must create them in that window.

      Viewports are not supported in stepped analyses.

Graph Chart Control
The following controls are available for Graphs/Charts for Adaptive Convergence (p. 432), and Fatigue Over-
view (p. 499) result items.

Feature                          Control
Pan                              Right Mouse Button
Zoom                             Middle Mouse Button
Box Zoom                         Alt+Left Mouse Button
Rotate (3D only)                 Left Mouse Button
Perspective Angle (3D            Shift+Left Mouse Button
only)
Display Coordinates (2D          Ctrl+Left Mouse Button along graph
only)                            line

Tips for working with graphs and charts:

 •    Some features are not available for certain graphs.
 •    Zoom will zoom to or away from the center of the graph. Pan so that your intended point of focus is
      in the center prior to zooming.
 •    If the graph has a Pan/Zoom control box, this can be used to zoom (shrink box) or pan (drag box).
 •    Double-clicking the Pan/Zoom control box will return it to its maximum size.

Named Selections
Named Selections enable you to specify and control like-grouped items such as types of geometry.

Use named selections with large models to improve the visibility of selected parts. Named selections are
automatically created in the event of a mesher failure so that problem faces can be identified.

The following topics are covered in this section:
 Creating Named Selections
 Managing Named Selections
 Scoping to Named Selections
 Inspecting Large Meshes Using Named Selections
 Importing Named Selections
 Converting Named Selection Groups to Mechanical APDL Application Components

Creating Named Selections
To create a named selection:

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                           129
The Mechanical Application Basics

 1.   Select geometry items in the graphics window that are to be members of the named selection group.
      The controls in the Named Selection Toolbar remain grayed out until you select one or more items,
      or ...

      Select one or more bodies under the Geometry tree object.
 2.   If you selected geometry items in the graphics window, click the Create Selection Group button
      (located on the left of the Named Selection Toolbar) or right mouse click in the Geometry window
      after a selection, and choose Create Selection Group in the context menu.

      If you selected bodies under the Geometry tree object, right mouse click on one of the body objects
      and choose Create Selection Group in the context menu.
 3.   Type a name for the group (or accept a default name), in the Selection Name dialog box. A Named
      Selections branch object is added to the Mechanical application tree. The name of the selection appears
      as a selectable item in the Named Selection display (located to the right of the Create Selection
      Group button), and as an annotation on the selected graphic items that make up the group.

Managing Named Selections
To use a named selection:

 1.   Select the name of the group in the Named Selection display.
 2.   Choose any of the following options that are available using the remaining controls in the Named
      Selection Toolbar:
      •   Selection drop-down menu (or in context menu from a right mouse button click on individual
          named selection object): controls selection options on items that are part of the group whose name
          appears in the Named Selection display.
          –   Select Items in Group: selects only those items in the named group.
          –   Add to Current Selection: Selects items in the named group combined with other items that
              are already selected. This option is grayed out if the geometry type in the named selection does
              not match the geometry type of the other selected items.
          –   Remove from Current Selection: Removes the selection of items in the named group from
              other items that are already selected. Selected items that are not part of the group remain se-
              lected. This option is grayed out if the geometry type in the named selection does not match
              the geometry type of the other selected items.

               Note

               Choosing any of these options affects only the current selections in the Geometry view,
               These options have no effect on what is included in the named selection itself.


      •   Visibility drop-down menu: controls display options on bodies that are part of the group whose
          name appears in the Named Selection display.
          –   Hide Bodies in Group: Turns off display of bodies in the named group (toggles with next item).
              Other bodies that are not part of the group are unaffected.
          –   Show Bodies in Group: Turns on display of bodies in the named group (toggles with previous
              item). Other bodies that are not part of the group are unaffected.
          –   Show Only Bodies in Group: Displays only items in the named group. Other items that are
              not part of the group are not displayed.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
130                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Named Selections

           You can also hide or show bodies associated with a named selection using a right mouse button
           click on the particular tree item under the Named Selections object and choosing Hide or Show
           from the context menu.
       •   Suppression drop-down menu: controls options on items that affect if bodies of the group whose
           name appears in the Named Selection display are to be suppressed, meaning that, not only are
           they not displayed, but they are also removed from any treatment such as loading or solution.
           –   Suppress Bodies in Group: Suppresses bodies in the named group (toggles with next item).
               Other bodies that are not part of the group are unaffected.
           –   Unsuppress Bodies in Group: Unsuppresses bodies in the named group (toggles with previous
               item). Other bodies that are not part of the group are unaffected.
           –   Unsuppress Only Bodies in Group: Unsuppresses only bodies in the named group. Other
               bodies that are not part of the group are suppressed.

           You can also suppress or unsuppress bodies associated with a named selection using a right mouse
           button click on the particular tree item under the Named Selections object and choosing Suppress
           or Unsuppress from the context menu. The Suppress and Unsuppress options are also available
           if you select multiple named selection items under a Named Selections object. The options will
           not be available if your multiple selection involves invalid conditions (for example, if you want to
           suppress multiple items you have selected and one is already suppressed, the Suppress option
           will not be available from the context menu.

The status bar shows the selected group area only when the areas are selected. The group listed in the
toolbar and in the Details View (p. 134) provides statistics that can be altered.

The Named Selection Toolbar is on by default and can be turned off or on by selecting View> Toolbars>
Named Selections.

Scoping to Named Selections
Many items can be scoped to named selections. Some examples are contact regions, mesh controls, loads,
and supports.

To scope an item to a named selection:

 1.    Insert or select the item in the tree.
 2.    Under the Details view, in the Scoping Method drop-down menu, choose Named Selection.
 3.    In the Named Selection drop-down menu, choose the particular name.

Notes on scoping items to a named selection:

 •    Only valid named selections will show in the Named Selection drop-down menu. If there are no valid
      named selections, the drop-down menu will be empty. No two Named Selections branches can have
      the same name. It is recommended that you use unique and intuitive names for the Named Selections.
 •    If you change a named selection that is used by an item, the associated geometry will update accordingly.
 •    If you delete a named selection used by an item, the item becomes underdefined.
 •    If all the components in a named selection cannot be applied to the item, the named selection is not
      valid for that item. This includes components in the named selection that may be suppressed. For ex-
      ample, in the case of a bolt pretension load scoped to cylindrical faces, only 1 cylinder can be selected
      for its geometry. If you have a named selection with 2 cylinders, one of which is suppressed, that par-
      ticular named selection is still not valid for the bolt pretension load.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                           131
The Mechanical Application Basics

Inspecting Large Meshes Using Named Selections
You can use named selections to inspect only a portion of the total mesh. Although this feature is available
regardless of mesh size, it is most beneficial when working with a large mesh (greater than 5 - 10 million
nodes). After you have designated a named selection group, you can use any of the following features to
assist you in this task:

 •    Display as Meshed object property in the Details view of the Named Selections folder object. By setting
      this property to Yes, if a mesh was generated, all items in the named selection groups within the Named
      Selections folder object are displayed in their meshed state. An example is shown below of a named
      selection that is comprised of 3 faces in their meshed display.




 •    Visible object property in the Details view of an individual named selection object (that is, a child object
      within the Named Selections folder object). By setting this property to No, the name selection can be
      made invisible meaning it will not be drawn and more importantly not taken into consideration for
      picking or selection. This should allow easier inspection inside complicated models having many layers
      of faces where the inside faces are hardly accessible from the outside. You can define named selections
      and make them invisible as you progress from outside to inside, similar to removing multiple shells
      around a core. The example shown below displays the same 3 face named selection where Visible has
      been set to No.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
132                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Notes




•   View> Wireframe in the Main Menu (p. 144). By displaying the model as a wireframe and setting the
    named selection Display as Meshed to Yes, you can display an enhanced version of the meshed items
    in the named selection as shown below.




Notes
•   The Visible option is different from the Hide or Suppress options in the right mouse button context
    menu. These two options will hide/suppress the full body containing a given name selection. However,
    the Visible option will hide only the specified name selection. When a named selection's Visible setting
    is set to No, just the faces from that name selection are not drawn, but the edges are always drawn.
•   When a named selection's Visible setting is set to No, it will not appear in any drawing of the geometry
    (regardless of which object is selected in the tree). But if a named selection is displayed as meshed it
    will display the mesh only if you have selected that specific named selection object or the Named Se-
    lections folder object. This behavior is the same as the behavior of the red annotation in the Geometry
    window for named selections (that is, the annotation appears only when the current selected object is
    the specific named selection object or the Named Selections folder object).




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                133
The Mechanical Application Basics

 •    When the View> Wireframe option is set, both the named selections (displayed as mesh) and the full
      geometry are drawn in wireframe, not just the meshes. Also, just the exterior faces of the meshed
      models are shown, not the interior elements.
 •    After at least one named selection is hidden, normally you can see the inside of a body, so displaying
      both sides of each face is enabled (otherwise displaying just the exterior side of each face is enough).
      But if a selection is made, the selected face is always displayed according to the option in Tools> Op-
      tions> Mechanical> Graphics> Single Side (can be one side or both sides).

Importing Named Selections
You can import named selections that you defined in a CAD system or in DesignModeler. A practical use in
this case is if you want the entities of the named selection group to be selected for the application of loads
or boundary conditions.

To import a named selection from a CAD system or from DesignModeler:

 1.    In the Geometry preferences, located in the Workbench Properties of the Geometry cell in the Project
       Schematic, check Named Selections and complete the Named Selection Key; or, in the Geometry
       Details view under Preferences, set Named Selection Processing to Yes and complete the Named
       Selection Prefixes field (refer to these entries under Geometry Preferences for more details).
 2.    A Named Selections branch object is added to the Mechanical application tree. In the Named Selection
       Toolbar, the name of the selection appears as a selectable item in the Named Selection display (located
       to the right of the Create Selection Group button), and as an annotation on the graphic items that
       make up the group.

Converting Named Selection Groups to Mechanical APDL Application Components
When you write a Mechanical APDL application input file that includes a named selection group, the group
is transferred to the Mechanical APDL application as a component provided the name contains only standard
English letters, numbers, and underscores. The following actions occur automatically to the group name in
the Mechanical application to form the resulting component name in the Mechanical APDL application:

 •    A name exceeding 32 characters is truncated.
 •    A name that begins with a number is renamed to include “C_” before the number.
 •    Spaces between characters in a name are replaced with underscores.

Example: The named selection group in the Mechanical application called 1 Edge appears as component
C_1_Edge in the Mechanical APDL application input file.

      Note

      Named selections starting with ALL, STAT, or DEFA will not be sent to the Mechanical APDL ap-
      plication.


Details View
The Details view is located in the bottom left corner of the window. It provides you with information and
details that pertain to the object selected in the Tree Outline (p. 118). Some selections require you to input
information (e.g., force values, pressures). Some selections are drop-down dialogs, which allow you to select
a choice. Fields may be grayed out. These cannot be modified.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
134                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Features

The following example illustrates the Details view for the object called Geometry.




For more information, see:
     Features (p. 135)
     Header (p. 136)
     Categories (p. 136)
     Undefined or Invalid Fields (p. 136)
     Decisions (p. 136)
     Text Entry (p. 137)
     Numeric Values (p. 137)
     Ranges (p. 139)
     Increments (p. 139)
     Geometry (p. 140)
     Exposing Fields as Parameters (p. 140)
     Options (p. 140)

Features
The Details view allows you to enter information that is specific to each section of the Tree Outline. It
automatically displays details for branches such as Geometry, Model, Connections, etc. Features of the Details
view include:

 •    Collapsible bold headings.
 •    Dynamic cell background color change.
 •    Row selection/activation.
 •    Auto-sizing/scrolling.
 •    Sliders for range selection.
 •    Combo boxes for boolean or list selection.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                   135
The Mechanical Application Basics

 •    Buttons to display dialog box (e.g. browse, color picker).
 •    Apply / Cancel buttons for geometry selection.
 •    Obsolete items are highlighted in red.

Header
The header identifies the control and names the current object.




The header is not a windows title bar; it cannot be moved.

Categories
Category fields extend across both columns of the Details Pane:




This allows for maximum label width and differentiates categories from other types of fields. To expand or
collapse a category, double-click the category name.

Undefined or Invalid Fields
Fields whose value is undefined or invalid are highlighted in yellow:




Decisions
Decision fields control subsequent fields:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
136                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Numeric Values




     Note

     The left column always adjusts to fit the widest visible label. This provides maximum space for
     editable fields in the right column. You can adjust the width of the columns by dragging the
     separator between them.

Text Entry
Text entry fields may be qualified as strings, numbers, or integers. Units are automatically removed and re-
placed to facilitate editing:




Inappropriate characters are discarded (for example, typing a Z in an integer field). A numeric field cannot
be entered if it contains an invalid value. It is returned to its previous value.

Numeric Values
You can enter a value in a numeric field as an expression, similar to using a calculator. The details view
evaluates the expression and applies the value. For example, enter 2 + (3 * 5) + pow(2,3) in the numeric
field. The details view evaluates this expression and applies 25 for the value.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         137
The Mechanical Application Basics




The supported operators are: + - , *, /, ^ (for power) and % (integer Modulus)

Sample usage:

   2+3
   10.5 – 2.5
   3.5 * 3.3
   10.12 / 1.89
   2 ^ 10
   10 % 3
   2 * (3 + 5)

The order of operator precedence is:

   parentheses
   intrinsic functions (like sin or cos)
   power (^)
   multiplication (*), division (/) and integer modulus (%)
   addition (+) and subtraction (-)

The supported intrinsic functions are:

  Supported In-               Sample Usage                                                                Usage
trinsic Functions
sin(x)               sin(3.1415926535/2)                             Calculate sines and hyperbolic sines. (x - Angle in ra-
sinh(x)              sinh(3.1415926535/2)                            dians)
cos(x)               cos(3.1415926535/2)                             Calculate the cosine (cos) or hyperbolic cosine
cosh(x)              cosh(3.1415926535/2)                            (cosh).(x - Angle in radians)
tan(x)               tan(3.1415926535/4)                             Calculate the tangent (tan) or hyperbolic tangent
tanh                 tanh(1.000000)                                  (tanh). (x - Angle in radians)
asin(x)              asin(0.326960)                                  Calculates the arcsine. (x - Value whose arcsine is to
                                                                     be calculated)
acos(x)              acos(0.326960)                                  Calculates the arccosine. (x - Value between –1 and
                                                                     1 whose arccosine is to be calculated)
atan(x)              atan(-862.42)                                   Calculates the arctangent of x (atan) or the arctangent
atan2(y,x)           atan2(-                                         of y/x (atan2). (x,y Any numbers)
                     862.420000,78.514900)


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
138                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Increments

  Supported In-                Sample Usage                                                                Usage
trinsic Functions
pow(x,y)             pow(2.0,3.0)                                     Calculates x raised to the power of y. (x – Base y - Ex-
                                                                      ponent)
sqrt(x)              sqrt(45.35)                                      Calculates the square root. ( x should be a Nonnegat-
                                                                      ive value )
exp(x)               exp(2.302585093)                                 Calculates the exponential. (x - Floating-point value)
log(x)               log(9000.00)                                     Calculates the natural logarithm. (x - Value whose
                                                                      logarithm is to be found)
log10(x)             log10(9000.00)                                   Calculates the common logarithm. (x - Value whose
                                                                      logarithm is to be found)
rand()               rand()                                           Generates a pseudorandom number.
ceil(x)              ceil(2.8)                                        Calculates the ceiling of a value. It returns a floating-
                     ceil(-2.8)                                       point value representing the smallest integer that is
                                                                      greater than or equal to x. (x - Floating-point value)
floor(x)             floor(2.8)                                       Calculates the floor of a value. It returns a floating-
                     floor(-2.8)                                      point value representing the largest integer that is
                                                                      less than or equal to x. (x - Floating-point value)
fmod(x,y)            fmod(-10.0, 3.0)                                 Calculates the floating-point remainder.The fmod
                                                                      function calculates the floating-point remainder f of
                                                                      x / y such that x = i * y + f, where i is an integer, f has
                                                                      the same sign as x, and the absolute value of f is less
                                                                      than the absolute value of y. (x,y - Floating-point val-
                                                                      ues).

You can also enter hexadecimal (starting with 0x) and octal (starting with &) numbers, for example 0x12 and
&12.

Ranges
If a numeric field has a range, a slider appears to the right of the current value:




If the value changes, the slider moves; if the slider moves the value updates.

Increments
If a numeric field has an increment, a horizontal up/down control appears to the right of the current value:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     139
The Mechanical Application Basics




The arrow button controls behave the same way a slider does.

Geometry
Geometry fields filter out inappropriate selection modes. For example, a bearing load can only be scoped
to a face. Geometries other than face will not be accepted.




Direction fields require a special type of selection:




Clicking Apply locks the current selection into the field. Other gestures (clicking Cancel or selecting a different
object or field) do not change the field's preexisting selection.

Exposing Fields as Parameters
A P appears beside the name of each field that may be treated as a parameter. Clicking the box exposes the
field as a parameter. For more information, see Parameters (p. 144).

Options
Option fields allow you to select one item from a short list. Options work the same way as Decisions (p. 136),
but don't affect subsequent fields. Options are also used for boolean choices (true/false, yes/no, enabled/dis-
abled, fixed/free, etc.) Double-clicking an option automatically selects the next item down the list.

Selecting an option followed by an ellipsis causes an immediate action.

Worksheet Tab
The Worksheet tab contains predominately tabular or text data (but may also contain graphical data) about
the following types of Mechanical application objects:


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
140                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                       Worksheet Tab

 •   Geometry
 •   Coordinate Systems
 •   Connections
 •   Fatigue Tool
 •   Contact Tool
 •   Solution
 •   Solution Information
 •   Solution Combination
 •   Contact Tool Initial Information
 •   Commands
 •   Analysis Settings
 •   Thermal Conditions
 •   Convergence

Figure: A Worksheet Tab View of a Geometry Folder




Displaying Information The Worksheet tab lists the information for child objects of an Outline Tree's
folder. The information can be displayed graphically for comparison. For example, with harmonic loads you
can select multiple loads to compare to one another for variance.

Go To Selected items A useful feature in the worksheets associated with most of the folders mentioned
above is the ability to instantly select items in the tree that you pick in the Name column (leftmost column)
on the worksheet. The graphical equivalents of the items also display in the Geometry window. This feature
allows you to quickly change properties in the Details view, and is available for worksheets associated with
the Geometry, Coordinate Systems, Connections, Environment, Frequency, and Buckling folders.

To use this feature, select one or more items in the Name column of the worksheet (standard Windows
controls for multiple selection apply), right-click on one of the selected items and choose Go To Selected
Items in Tree. The items are selected in the tree, and the Geometry window replaces the worksheet and
displays graphics associated with the selected items. An example is shown here:

The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the
help. Interface names and other components shown in the demo may differ from those in the released product.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                        141
The Mechanical Application Basics




Viewing Selected Columns for Contact When viewing a worksheet that includes contact information,
you can choose which columns will display.

To choose the columns that will display, right mouse click anywhere inside the worksheet table. From the
context menu, click on any of the column names. A check mark signifies that the column will appear. There
are some columns in the worksheet that will not always be shown even if you check them. For example, if
all the contact regions have a Pinball Region set to Program Controlled and the Pinball Radius column
is checked, Pinball Radius will not show because you have not set any of this data.

Graph and Tabular Data Windows
Whenever you highlight the following objects in the Mechanical application tree, a Graph window and
Tabular Data window appear beneath the Geometry window.

 •    Analysis Settings
 •    Loads
 •    Contour Results
 •    Probes
 •    Charts

These windows are designed to assist you in managing analysis settings and loads and in reviewing results.
The Graph window provides an instant graphical display of the magnitude variations in loads and/or results,
while the Tabular Data window provides instant access to the corresponding data points.

Below are some of the uses of these windows.

Analysis Settings
For analyses with multiple steps, you can use these windows to select the step(s) whose analysis settings
you want to modify. The Graph window also displays all the loads used in the analysis.

Loads
Inserting a load updates the Tabular Data window with a grid to enable you to enter data on a per-step
basis. As you enter the data, the values are reflected in the Graph window.




A check box is available for each component of a load in order to turn on or turn off the viewing of the load
in the Graph window. Components are color-coded to match the component name in the Tabular Data
window. Clicking on a time value in the Tabular Data window or selecting a row in the Graph window will


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
142                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Context Menu Options

update the display in the upper left corner of the Geometry window with the appropriate time value and
load data.

As an example, if you use a Displacement load in an analysis with multiple steps, you can alter both the
degrees of freedom and the component values for each step by modifying the contents in the Tabular Data
window as shown above.

If you wish for a load to be active in some steps and removed in some other steps you can do so by following
the steps outlined in Activation/Deactivation of Loads Within a Step (p. 268).

Contour Results and Probes
For contour results and probes, the Graph and Tabular Data windows display how the results vary over
time. You can also choose a time range over which to animate results. Typically for results the minimum
and maximum value of the result over the scoped geometry region is shown.

To view the results in the Geometry window for the desired time point, select the time point in the Graph
window or Tabular Data window, then click the right mouse button and choose Retrieve Results. The
Details view for the chosen result object will also update to the selected step.

Charts
With charts, the Graph and Tabular Data windows can be used to display loads and results against time
or against another load or results item.

Context Menu Options
Presented below are some of the commonly used options available in a context menu that displays when
you click the right mouse button within the Graph window and/or the Tabular Data window. The options
vary depending on how you are using these windows (for example, loads vs. results).

 •   Retrieve This Result: Retrieves and presents the results for the object at the selected time point.
 •   Insert Step: Inserts a new step at the currently selected time in the Graph window or Tabular Data
     window. The newly created step will have default analysis settings. All load objects in the analysis will
     be updated to include the new step.
 •   Delete Step: Deletes a step.
 •   Copy Cell: Copies the cell data into the clipboard for a selected cell or group of cells. The data may
     then be pasted into another cell or group of cells. The contents of the clipboard may also be copied
     into Microsoft Excel. Cell operations are only valid on load data and not data in the Steps column.
 •   Paste Cell: Pastes the contents of the clipboard into the selected cell, or group of cells. Paste operations
     are compatible with Microsoft Excel.
 •   Delete Rows: Removes the selected rows. In the Analysis Settings object this will remove corresponding
     steps. In case of loads this modifies the load vs time data.
 •   Select All Steps: Selects all the steps. This is useful when you want to set identical analysis settings for
     all the steps.
 •   Select All Highlighted Steps: Selects a subset of all the steps. This is useful when you want to set
     identical analysis settings for a subset of steps.
 •   Activate/Deactivate at this step!: This allows a load to become inactive (deleted) in one or more steps.
     By default any defined load is active in all steps.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                          143
The Mechanical Application Basics

 •    Zoom to Range: Zooms in on a subset of the data in the Graph window. Click and hold the left mouse
      at a step location and drag to another step location. The dragged region will highlight in blue. Next,
      select Zoom to Range. The chart will update with the selected step data filling the entire axis range.
      This also controls the time range over which animation takes place.
 •    Zoom to Fit: If you have chosen Zoom to Range and are working in a zoomed region, choosing Zoom
      to Fit will return the axis to full range covering all steps.

Result data is charted in the Graph window and listed in the Tabular Data window. The result data includes
the Maximum and Minimum values of the results object over the steps.

Parameters
To parameterize a variable, click the box next to it. A P appears in the box. Items that cannot be parameterized
do not display a check box and are left-aligned to save space.




The boxes that appear in the Mechanical application apply only to the Parameter Workspace. Checking or
unchecking these boxes will have no effect on which CAD parameters are transferred to Design Exploration.

For more information, see Parameters (p. 496).

Toolbars
Toolbars are displayed across the top of the window, below the menu bar. Toolbars can be docked to your
preference. The layouts displayed are typical. You can double-click the vertical bar in the toolbar to automat-
ically move the toolbar to the left.

     Main Menu (p. 144)
     Standard Toolbar (p. 147)
     Graphics Toolbar (p. 148)
     Context Toolbar (p. 151)
     Unit Conversion Toolbar (p. 161)
     Named Selection Toolbar

Main Menu
The Main Menu includes the following items.



File Menu

Function               Description
Refresh All Data       Updates the geometry, materials, and any imported loads that are in the tree.
Save Project           Allows you to save the project.
Export                 Allows you to export outside of the project.You can export a .mechdat file (when run-
                       ning the Mechanical application) that later can be imported into a new Workbench

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
144                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  View Menu

Function            Description
                    project. Note that only the data native to the Mechanical application is saved to the
                    .mechdat file. External files (such as solver files) will not be exported.You can also export
                    the mesh for input to any of the following: FLUENT (.msh), POLYFLOW (.poly), CGNS
                    (.cgns), and ICEM (.prj).
Clean               Clears all results and meshing data from the database depending on the object selected
                    in the tree.
Save to TcEng       (Displayed only if you have access to the Teamcenter Engineering database.) Allows
                    you to save the file to the Teamcenter Engineering database.This capability is available
                    only on Windows platforms and runs only with the NX plug-in (UG NX V1.0 and UG NX
                    V2.0).
Close Mechanical    Exits the Mechanical application session.

Edit Menu

Function            Description
Duplicate           Duplicates the object you highlight.The model and environment duplication is per-
                    formed at the Project Schematic level (see Duplicating, Moving, Deleting, and Replacing
                    Systems for details).This option is not available for User Defined Results.
Duplicate Without   (Only available on solved result objects) Duplicates the object you highlight, including
Results             all subordinate objects. Because the duplicated objects have no result data the process
                    is faster than performing Duplicate.This option is not available for User Defined Results.
Copy                Copies an object.
Cut                 Cuts the object and saves it for pasting.
Paste               Pastes a cut or copied object.
Delete              Deletes the object you select.
Select All          Selects all items in the Model of the current selection filter type. Select All is also
                    available in a context menu if you click the right mouse button in the Geometry window.

View Menu

Function            Description
Shaded Exterior     Displays the model in the graphics window with shaded exteriors and distinct edges.
and Edges           This option is mutually exclusive with Shaded Exterior and Wireframe.
Shaded Exterior     Displays the model in the graphics window with shaded exteriors only.This option is
                    mutually exclusive with Shaded Exterior and Edges and Wireframe.
Wireframe           Displays the model in the graphics window with distinct edges only (recommended
                    for seeing gaps in surface bodies).This option is mutually exclusive with Shaded Exter-
                    ior and Edges and Shaded Exterior. A model's geometry, mesh, or named selection
                    displayed as a mesh can be viewed in wireframe mode.
Thick Shells and    Toggles the visibility of the thickness applied to a shell or beam in the graphics window
Beams               when the mesh is selected.
Annotations         Toggles the visibility of annotations in the graphics window.
Custom Annota-      Toggles the visibility of custom user annotations in the graphics window.
tions
Ruler               Toggles the visibility of the visual scale ruler in the graphics window.

                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                     145
The Mechanical Application Basics

Function                Description
Legend                  Toggles the visibility of the results legend in the graphics window.
Triad                   Toggles the visibility of the axis triad in the graphics window.
Eroded Nodes            Toggles the visibility of eroded nodes for explicit dynamics analyses.
Outline                 Expand All - Restores tree objects to their original expanded state.
                        Collapse Environments - Collapses all tree objects under the Environment object(s).
                        Collapse Models - Collapses all tree objects under the Model object(s).
Toolbars                Named Selections - Displays the Named Selection Toolbar
                        Unit Conversion - Displays the Unit Conversion Toolbar
Windows                 Messages - Toggles the display of the Messages window.
                        Mechanical Wizard - Toggles the display of a wizard on the right side of the window
                        which prompts you to complete tasks required for an analysis.
                        Annotations - Toggles the display of the Annotations window.
                        Section Planes - Toggles the display of the Section Planes window.
                        Reset Layout - Restores the Window layout back to a default state.

Units Menu

Function                Description
Metric (m, kg, N, s,    Sets unit system.
V, A)
Metric (cm, g,
dyne, s, V, A)
Metric (mm, kg, N,
s, mV, mA)
Metric (mm, t, N,
s, mV, mA)
Metric (mm, dat,
N, s, mV, mA)
Metric (µm, kg,
µN, s, V, mA)
U.S. Customary
(ft, lbm, lbf, °F, s,
V, A)
U.S. Customary
(in, lbm, lbf, °F, s,
V, A)
Degrees                 Sets angle units to degrees.
Radians                 Set angle units to radians.
rad/s                   Sets angular velocity units to radians per second.
RPM                     Sets angular velocity units to revolutions per minute.
Celsius                 Sets the temperature values to degree Celsius.
Kelvin                  Sets the temperature values to Kelvin.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
146                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Help Menu

Tools Menu

Function              Description
Write Input File...   Writes the Mechanical APDL application input file from the active Solution branch.
                      This option does not initiate a Solve.
Read Result File...   Reads the Mechanical APDL application result files (.rst, solve.out, and so on) in a direct-
                      ory and copies the files into the active Solution branch.
Solve Process Set-    Allows you to configure solve process settings.
tings
Addins                Launches the Addins manager dialog that allows you to load/unload third-party add-
                      ins that are specifically designed for integration within the Workbench environment.
Options               Allows you to customize the application and to control the behavior of Mechanical
                      application functions.
Variable Manager      Allows you to enter an application variable.
Run Macro...          Opens a dialog box to locate a script (.vbs , .js ) file.

Help Menu

Function              Description
Mechanical Help       Displays the Help system in another browser window.
About Mechanical      Provides copyright and application version information.


     Note

     View menu settings are maintained between Mechanical application sessions except for the
     Outline items and Reset Layout in the Windows submenu.

Standard Toolbar


The Standard Toolbar contains application-level commands, configuration toggles and important general
functions. Each icon button and its description follows:

Icon Button                                 Application-level command                                          Description
                                            the Mechanical Wizard                              Activates the Mechanical Wizard
                                                                                               in the user interface.
                                            Solve analysis with a given                        Drop-down list to select a solve
                                            solve process setting.                             process setting.


                                            New Section Plane                                  View a section cut through the
                                                                                               model (geometry, mesh and res-
                                                                                               ults displays) as well as obtained
                                                                                               capped displays on either side of
                                                                                               the section. Refer to the New Sec-
                                                                                               tion Plane section for details.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                    147
The Mechanical Application Basics

Icon Button                                Application-level command                                          Description
                                           New Graphics Annotation                            Adds a text comment for a partic-
                                                                                              ular item in the Geometry win-
                                                                                              dow.To use:

                                                                                              •     Select button in toolbar.
                                                                                              •     Click a placement location
                                                                                                    on the geometry. A chisel-
                                                                                                    shaped annotation is
                                                                                                    anchored in 3D.
                                                                                              •     A blank annotation appears
                                                                                                    and the Annotation window
                                                                                                    is made visible or brought
                                                                                                    forward.
                                                                                              •     A new row is created for the
                                                                                                    annotation.
                                                                                              •     Type entry.

                                                                                              To edit, double click the corres-
                                                                                              ponding entry in the Annotation
                                                                                              window and type new informa-
                                                                                              tion.To delete, select the entry
                                                                                              and press the delete key.To
                                                                                              move, select the annotation in
                                                                                              the geometry window and move
                                                                                              while pressing down the left
                                                                                              mouse button.To exit without
                                                                                              creating an annotation, re-click
                                                                                              the annotation button.
                                           New Chart and Table                                Refer to the Chart and Table sec-
                                                                                              tion for details.
                                           Comment                                            Adds a comment within the cur-
                                                                                              rently highlighted outline branch.
                                           Figure                                             Captures any graphic displayed
                                                                                              for a particular object in the Geo-
                                                                                              metry window.
                                           Image                                              Adds an image within the cur-
                                                                                              rently highlighted outline branch.
                                           Image from File                                    Imports an existing graphics im-
                                                                                              age.
                                           Image to File                                      Saves the current graphics image
                                                                                              to a file (.png, .jpg, .tif, .bmp, .eps).

Graphics Toolbar




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
148                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Help Menu

The Graphics Toolbar sets the selection/manipulation mode for the cursor in the graphics window. The
toolbar also provides commands for modifying a selection or for modifying the viewpoint. Each icon button
and its description follows:

Icon But-           Tool Tip Name Displayed                                                                Description
ton
            Label                                                          Allows you to move and place the label of a load any-
                                                                           where along the feature that the load is currently
                                                                           scoped to.
            Direction                                                      Chooses a direction by selecting either a single face,
                                                                           two vertices, or a single edge (enabled only when
                                                                           Direction field in the Details view has focus). See
                                                                           Pointer Modes.
            Coordinates                                                    (Active only if you are setting a location, for example,
                                                                           a local coordinate system.) Enables the exterior coordin-
                                                                           ates of the model to display adjacent to the cursor and
                                                                           updates the coordinate display as the cursor is moved
                                                                           across the model. If you click with the cursor on the
                                                                           model, a label displays the coordinates of that location.
            Select Mode                                                    Sets selection as either Single Select or Box Select;
                                                                           used in conjunction with the selection filters.
            Vertex                                                         Designates vertices only for picking or viewing selec-
                                                                           tion.
            Edge                                                           Designates edges only for picking or viewing selection.

            Face                                                           Designates faces only for picking or viewing selection.

            Body                                                           Designates bodies only for picking or viewing selec-
                                                                           tion.
            Extend Selection                                               Adds adjacent faces (or edges) within angle tolerance,
                                                                           to the currently selected face (or edge) set, or adds
                                                                           tangent faces (or edges) within angle tolerance, to the
                                                                           currently selected face (or edge) set.
            Rotate                                                         Activates rotational controls based on the positioning
                                                                           of the mouse cursor.
            Pan                                                            Moves display model in the direction of the mouse
                                                                           cursor.
            Zoom                                                           Displays a closer view of the body by dragging the
                                                                           mouse cursor vertically toward the top of the graphics
                                                                           window, or displays a more distant view of the body
                                                                           by dragging the mouse cursor vertically toward the
                                                                           bottom of the graphics window.
            Box Zoom                                                       Displays selected area of a model in a box that you
                                                                           define.
            Fit                                                            Fits the entire model in the graphics window.

            Toggle Magnifier Window On/Off                                 Displays a Magnifier Window, which is a shaded box
                                                                           that functions as a magnifying glass, enabling you to



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                    149
The Mechanical Application Basics

Icon But-         Tool Tip Name Displayed                                                                    Description
ton
                                                                             zoom in on portions of the model. When you toggle
                                                                             the Magnifier Window on, you can:

                                                                             •     Pan the Magnifier Window across the model by
                                                                                   holding down the left mouse button and drag-
                                                                                   ging the mouse.
                                                                             •     Increase the zoom of the Magnifier Window by
                                                                                   adjusting the mouse wheel, or by holding down
                                                                                   the middle mouse button and dragging the
                                                                                   mouse upward.
                                                                             •     Recenter or resize the Magnifier Window using a
                                                                                   right mouse button click and choosing an option
                                                                                   from the context menu. Recenter the window
                                                                                   by choosing Reset Magnifier. Resizing options
                                                                                   include Small Magnifier, Medium Magnifier,
                                                                                   and Large Magnifier for preset sizes, and Dy-
                                                                                   namic Magnifier Size On/Off for gradual size
                                                                                   control accomplished by adjusting the mouse
                                                                                   wheel.

                                                                             Standard model zooming, rotating, and picking are
                                                                             disabled when you use the Magnifier Window.
            Previous View                                                    To return to the last view displayed in the graphics
                                                                             window, click the Previous View button on the tool-
                                                                             bar. By continuously clicking you can see the previous
                                                                             views in consecutive order.
            Next View                                                        After displaying previous views in the graphics win-
                                                                             dow, click the Next View button on the toolbar to
                                                                             scroll forward to the original view.
            Set (ISO)                                                        The Set ISO button allows you to set the isometric
                                                                             view.You can define a custom isometric viewpoint
                                                                             based on the current viewpoint (arbitrary rotation), or
                                                                             define the "up" direction so that geometry appears
                                                                             upright.
            Look at                                                          Centers the display on the currently selected face or
                                                                             plane.
            Rescale Annotation                                               Adjusts the size of annotation symbols, such as load
                                                                             direction arrows.
            Viewports                                                        Splits the graphics display into a maximum of four
                                                                             simultaneous views.

Keyboard Support
The same functionality is available via your keyboard provided the NumLock key is enabled.. The numbers
correlate to the following functionality:

   0 = View Isometric
   1 = +Z Front

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
150                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Keyboard Support

     2 = -Y Bottom
     3 =+X Right
     4 = Previous View
     5 = Default Isometric
     6 = Next View
     7 = -X Left
     8 = +Y Top
     9 = -Z Back
     . (dot) = Set Isometric




Context Toolbar
The Context Toolbar configures its buttons based on the type of object selected in the Tree Outline (p. 118).
The Context Toolbar makes a limited number of relevant choices more visible and readily accessible.

Context Toolbars include:

 •    Model Context Toolbar (p. 152)
 •    Geometry Context Toolbar (p. 153)
 •    Virtual Topology Context Toolbar (p. 153)
 •    Symmetry Context Toolbar (p. 153)
 •    Connections Context Toolbar (p. 153)
 •    Coordinate Systems Context Toolbar
 •    Meshing Context Toolbar (p. 154)
 •    Gap Tool Context Toolbar (p. 154)
 •    Environment Context Toolbar (p. 154)
 •    Solution Context Toolbar (p. 154)
 •    Vector Display Context Toolbar
 •    Result Context Toolbar (p. 155)
 •    Capped Isosurface Context Toolbar
 •    Comment Context Toolbar (p. 160)
 •    Print Preview Context Toolbar (p. 161)
 •    Report Preview Context Toolbar (p. 161)


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                           151
The Mechanical Application Basics


      Note
      •   Some Context Toolbar items, such as Connections or Mesh Controls, can be hidden.
      •   The Context Toolbar cannot be hidden (for simplicity and to avoid jumbling the screen). The
          toolbar appears blank when no options are relevant.
      •   The toolbar displays a text label for the current set of options.
      •   A Workbench Options dialog box setting turns off button text labels to minimize context
          toolbar width.


Model Context Toolbar


The Model Context toolbar becomes active when a Model is selected in the tree. The Model Context toolbar
contains options for creating objects related to the model, as described below.

Construction Geometry
See Path (p. 178) for details.

Virtual Topology
You can use the Virtual Topology option to reduce the number of elements in a model by merging faces
and lines. This is particularly helpful when small faces and lines are involved. The merging will impact
meshing and selection for loads and supports. See Virtual Topology Overview for details.

Symmetry
For symmetric bodies, you can remove the redundant portions based on the inherent symmetry, and replace
them with symmetry planes. Boundary conditions are automatically included based on the type of analyses.

Remote Point
See Remote Point (p. 180) for details.

Connections
Connection objects include contact regions, joints, and springs. The Connections button is available only
if a connection object is not already in the tree (such as a model that is not an assembly), and you wish to
create a connections object.

You can transfer structural loads and heat flows across the contact boundaries and “connect” the various
parts. See the Contact section for details.

A joint typically serves as a junction where bodies are joined together. Joint types are characterized by their
rotational and translational degrees of freedom as being fixed or free. See the Joints section for details.

You can define a spring (longitudinal or torsional) to connect two bodies together or to connect a body to
ground. See the Springs section for details.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
152                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                      Connections Context Toolbar

Solution Combination
Use the Solution Combination option to combine multiple environments and solutions to form a new solution.
A solution combination folder can be used to linearly combine the results from an arbitrary number of load
cases (environments). Note that the analysis environments must be static structural with no solution conver-
gence. Results such as stress, elastic strain, displacement, contact, and fatigue may be requested. To add a
load case to the solution combination folder, right click on the worksheet view of the solution combination
folder, choose add, and then select the scale factor and the environment name. An environment may be
added more than once and its effects will be cumulative. You may suppress the effect of a load case by using
the check box in the worksheet view or by deleting it through a right click. For more information, see Solution
Combinations (p. 400).

Geometry Context Toolbar


The Geometry Context toolbar is active when you select the Geometry branch in the tree or any items
within the Geometry branch. Using the Geometry toolbar you can also apply a Point Mass. You can also
add a Commands object to individual bodies.

Construction Geometry


See Path (p. 178) for details.

Virtual Topology Context Toolbar


The Virtual Topology Context toolbar includes an option to insert Virtual Cell objects where you can group
faces or edges.

Symmetry Context Toolbar


The Symmetry Context toolbar includes an option to insert Symmetry Region or Periodic Region objects
where you can define symmetry planes.

Connections Context Toolbar

The Connections context toolbar includes the following settings and functions:

 •   Contact drop down menu: Inserts one of the following: a manual Contact Region object set to a spe-
     cific contact type, a Contact Tool object (for evaluating initial contact conditions), or a Solution Inform-
     ation object.
 •   Spot Weld button: Inserts a Spot Weld object.
 •   Body Interactions See Body Interactions in Explicit Dynamics Analyses (p. 523) for details.
 •   Body-Ground drop-down menu: Inserts a type of Joint object, Spring object, or a Beam object, whose
     reference side is fixed.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                       153
The Mechanical Application Basics

 •    Body-Body drop-down menu: Inserts a type of Joint object, Spring object, or a Beam object, where
      neither side is fixed.
 •    Body Views toggle button: For joints, displays reference and mobile parts in separate auxiliary windows.
 •    Sync Views toggle button: When the Body Views button is engaged, any manipulation of the model
      in the Geometry window will also be reflected in both auxiliary windows.
 •    Configure, Set, and Revert buttons: Graphically configures the initial positioning of a joint. Refer to
      Example: Configuring Joints (p. 210) for details.
 •    Assemble button: For joints, performs the assembly of the model, finding the closest part configuration
      that satisfies all the joints.
 •    Commands icon button: Inserts a Commands object.

Meshing Context Toolbar


The Meshing Context toolbar includes the following controls.

 •    Update button - for updating a cell that references the current mesh. This will include mesh generation
      as well as generating any required outputs.
 •    Mesh drop down menu - for implementing meshing ease of use features or for editing meshes in CFX-
      Mesh.
 •    Mesh Control drop down menu - for adding Mesh Controls to your model.
 •    Options button - for displaying the Meshing Options panel that allows you to define a physics preference
      and an initial Method control.

Gap Tool Context Toolbar


The Gap Tool Context toolbar is used to have the Mechanical application search for face pairs within a specified
gap distance that you specify.

Environment Context Toolbar
The Environment Context toolbar allows you to apply loads to your model.

The toolbar display varies depending on the type of simulation you choose. For example, the toolbar for a
Static Structural analysis is shown below.



Solution Context Toolbar
The Solution toolbar applies to Solution level objects that either:

 •    Never display contoured results (such as the Solution object), or
 •    Have not yet been solved (no contours to display).

The options displayed on this toolbar are based on the type of analysis that is selected. The example shown
below displays the solution options for a static structural analysis.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
154                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            Scaling Deformed Shape




Objects created via the Solution toolbar are automatically selected in the Outline. Prior to a solution this
toolbar always remains in place (no contours to display).

A table in the Results Based on Geometry (p. 398) section indicates which bodies can be represented by the
various choices available in the drop-down menus of the Solution toolbar.

Inserting some other tools changes the solution context toolbar to other toolbars (e.g., Solution Information).



Result Context Toolbar


The Result toolbar applies to Solution level objects that display contour or vector results.

Scaling Deformed Shape
For results with an associated deformed shape, the Scaling combo box provides control over the on-screen
scaling:




Scale factors precede the descriptions in parentheses in the list. The scale factors shown above apply to a
particular model's deformation and are intended only as an example. Scale factors vary depending on the
amount of deformation in the model.

You can choose a preset option from the list or you can type a customized scale factor relative to the scale
factors in the list. For example, based on the preset list shown above, typing a customized scale factor of
0.6 would equate to approximately 3 times the Auto Scale factor.

 •   Undeformed does not change the shape of the part or assembly.
 •   True Scale is the actual scale.
 •   Auto Scale scales the deformation so that it's visible but not distorting.
 •   The remaining options provide a wide range of scaling.

The system maintains the selected option as a global setting like other options in the Result toolbar.

As with other presentation settings, figures override the selection.

For results that are not scaled, the combo box has no effect.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         155
The Mechanical Application Basics


      Note

      Most of the time, a scale factor will be program chosen to create a deformed shape that will show
      a visible deflection to allow you to better observe the nature of the results. However, under certain
      conditions, the True Scale displaced shape (scale factor = 1) is more appropriate and is
      therefore the default if any of the following conditions are true:

       •   Rigid bodies exist.
       •   A user-defined spring exists in the model.
       •   Large deflection is on.

      This applies to all analyses except for modal and linear buckling analyses (in which case True
      Scale has no meaning).

Relative Scaling
The combo list provides five "relative" scaling options. These options scale deformation automatically relative
to preset criteria:

 •    Undeformed
 •    True Scale
 •    0.5x Auto
 •    Auto Scale
 •    2x Auto
 •    5x Auto

Geometry
You can observe different views from the Geometry drop-down menu.




 •    Exterior

This view displays the exterior results of the selected geometry.

 •    IsoSurfaces

This view displays the interior only of the model at the transition point between values in the legend, as
indicated by the color bands.

 •    Capped IsoSurfaces

This view displays contours on the interior and exterior. When you choose Capped IsoSurfaces, a Capped
Isosurface toolbar appears beneath the Result context toolbar. Refer to Capped Isosurfaces for a description
of the controls included in the toolbar.

 •    Slice Planes

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
156                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Edges Options

This view displays planes cutting through the result geometry; only previously drawn slice planes are visible.

The model image changes to a wireframe representation.

Contours Options
To change the way you view your results, click any of the options on this toolbar.




 •   Smooth

     This view displays gradual distinction of colors.
 •   Contour

     This view displays the distinct differentiation of colors.
 •   Isolines

     This view displays a line at the transition between values.
 •   Solid

     This view displays the model only with no contour markings.

Edges Options
You can switch to wireframe mode to see gaps in surface body models. Red lines indicate shared edges.

In addition, you can choose to view wireframe edges, include the deformed model against the undeformed
model, or view elements.

Showing a subdued view of the undeformed model along with the deformed view is especially useful if you
want to view results on the interior of a body yet still want to view the rest of the body's shape as a reference.
An example is shown here.




The Show Undeformed Model option is useful when viewing any of the options in the Geometry drop-
down menu.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        157
The Mechanical Application Basics




 •    No Wireframe

      This view displays a basic picture of the body.
 •    Show Undeformed Wireframe

      This view shows the body outline before deformation occurred.
 •    Show Undeformed Model

      This view shows the deformed body with contours, with the undeformed body in translucent form.
 •    Show Elements

      This view displays element outlines.

Vector Display Context Toolbar
Using the Graphics button, you can display results as vectors with various options for controlling the display.


 •    Click the Graphics button on the Result context toolbar to convert the result display from contours
      (default) to vectors.
 •    When in vector display, a Vector Display toolbar appears with controls as described below.




                                                                      Displays vector length proportional to the magnitude of
                                                                      the result.
                                                                      Displays a uniform vector length, useful for identifying
                                                                      vector paths.
                                                                      Controls the relative length of the vectors in incremental
                                                                      steps from 1 to 10 (default = 5), as displayed in the tool
                                                                      tip when you drag the mouse cursor on the slider handle.
                                                                      Displays all vectors, aligned with each element.

                                                                      Displays vectors, aligned on an approximate grid.

                                                                      Controls the relative size of the grid, which determines
                                                                      the quantity (density) of the vectors.The control is in
                                                                      uniform steps from 0 [coarse] to 100 [fine] (default = 20),
                                                                      as displayed in the tool tip when you drag the mouse
                                                                      cursor on the slider handle.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
158                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Vector Display Context Toolbar


                                                                               Note

                                                                               This slider control is active only when the
                                                                               adjacent button is chosen for displaying
                                                                               vectors that are aligned with a grid.


                                                                      Displays vector arrows in line form.

                                                                      Displays vector arrows in solid form.


 •   When in vector display, click the Graphics button on the Result context toolbar to change the result
     display back to contours. The Vector Display toolbar is removed.

Presented below are examples of vector result displays.




Uniform vector lengths identify paths using vector arrows in line form.




Course grid size with vector arrows in solid form.                 Same using wireframe edge option.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                       159
The Mechanical Application Basics




Uniform vector lengths , grid display on slice plane with vector arrows in solid form.




Zoomed-in uniform vector lengths , grid display with arrow scaling and vector arrows in solid form.

Max, Min, and Probe Annotations


Toolbar buttons allow for toggling Max and Min annotations and for creating probe annotations.

See also Annotations (p. 229).

Comment Context Toolbar




When you select the Comment button in the standard toolbar or when you select a Comment object already
in the tree, the Comment Context toolbar and Comment Editor appear. The buttons at the top allow you
to insert an image or apply various text formatting.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
160                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Messages Window

To insert an image, click the button whose tool tip is Insert Image, then complete the information that
appears in the dialog box . For the Image URL, you can use a local machine reference (C:\...) or a web reference
(http:\\...).

Print Preview Context Toolbar


The Print Preview toolbar allows you to print the currently-displayed image, or send it to an e-mail recipient
or to a Microsoft Word or PowerPoint file.

Report Preview Context Toolbar


The Report Preview toolbar allows you to select a language for the report and adjust the image resolution.
The graphics browser exports images to a specific resolution (e.g. 512x384 pixels); the HTML page specifies
the display resolution for images. By default the resolutions match. By increasing the resolution of the bitmap
while holding the HTML resolution constant the print quality of image may be increased. The options below
correspond to 100%, 200% and 400% image resolutions. Changing the language or the image quality setting
forces regeneration of the HTML page.

You can also print the report, save it to a file, send it to an e-mail recipient or to a Microsoft Word or
PowerPoint file, refresh the images, and adjust the font size.

Unit Conversion Toolbar

The Unit Conversion Toolbar is a built-in conversion calculator. It allows conversion between six consistent
unit systems.

The Units menu sets the active unit system. The status bar shows the current unit system. The units listed
in the toolbar and in the Details View (p. 134) are in the proper form (i.e. no parenthesis).

The Unit Conversions toolbar is hidden by default. To see it, select View> Toolbars> Unit Conversion.

Named Selection Toolbar


Named Selections enable you to specify and control like-grouped items such as types of geometry. See the
Named Selections (p. 129) section for details.

Messages Window
The Messages Window is a Mechanical application feature that prompts you with feedback concerning the
outcome of actions you have taken in the Mechanical application. For example, Messages display when you
resume a database, Mesh a model, or when you initiate a Solve.

Messages come in three forms:

 •   Error
 •   Warning
 •   Information


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                           161
The Mechanical Application Basics

By default the Messages Window is hidden, but displays automatically as a result of irregularities during
Mechanical application operations. To display the window manually: select View>Windows>Messages. An
example of the Messages Window is shown below.




In addition, the status bar provides a dedicated area (shown above) to alert you should one or more messages
become available to view. The Messages Window can be auto-hidden or closed using the buttons on the
top right corner of the window.

      Note

      You can toggle between the Graph and Messages windows by clicking a tab.

Once messages are displayed, you can:

 •    Double-click a message to display its contents in a pop-up dialog box.
 •    Highlight a message and then press the key combination CTRL+C to copy its contents to the clipboard.
 •    Press the Delete key to remove a selected message from the window.
 •    Select one or more messages and then use the right mouse button click to display the following context
      menu options:
      –   Go To Object - Selects the object in the tree which is responsible for the message.
      –   Show Message - Displays the selected message in a popup dialog box.
      –   Copy - Copies the selected messages to the clipboard.
      –   Delete - Removes the selected messages.
      –   Refresh - Refreshes the contents of the Messages Window as you edit objects in the Mechanical
          application tree.

Workbench Windows Manager
The Workbench window contains a number of panes that house graphics, outlines, details and other views
and controls. The window manager allows you to move, resize, tab dock and autohide panes.

Tab dock means that two or more panes reside in the tabs in the same space on screen.

Autohide means that a pane (or tab docked group of panes) automatically collapses when not in use to free
screen space.

The following topics are covered in this section.
 Restore Original Window Layout

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
162                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Triad and Rotation Cursors

 Window Manager Features

Restore Original Window Layout
Choose "Restore Original Window Layout" from the View menu to return to the default original pane config-
uration.

Window Manager Features
AutoHiding

Panes are either pinned       or unpinned              . Toggle this state by clicking the icon in the pane title bar.

A pinned pane occupies space in the Workbench window. An unpinned pane collapses to a tab on the
periphery of the window when inactive.

To work with an unpinned pane, move the mouse pointer into the tab; the pane will fly out on top of other
panes in the Workbench window. The pane will remain visible as long as it is active or contains the mouse
pointer. Pin the pane to restore its previous configuration.

Moving and Docking
Drag the title bar to move a pane, or drag a tab to undock panes. Once the drag starts a number of dock
targets (blue-filled arrows and circle) appear overtop the Workbench window:

Move the mouse pointer over a target to preview the resulting location for the pane. Arrow targets indicate
adjacent locations; a circular target allows tab-docking of two or more panes (to share screen space). Release
the button on the target to move the pane.

Abort the drag operation by pressing the ESC key.

Resize panes by dragging the borders.

Print Preview
Print Preview runs a script to generate an HTML page and image. The purpose of the Print Preview tab is
to allow you to view your results or graphics image.

The title block is an editable HTML table. The table initially contains the Author, Subject, Prepared For and
Date information supplied from the details view of the Project tree node. To change or add this information,
double click inside the table. The information entered in the table does not propagate any changes back to
the details view and is not saved after exiting the Print Preview tab.

The image is generated in the same way as figures in Report.

Triad and Rotation Cursors
The triad and rotation cursors allow you to control the viewing orientation as described below.

Triad          •   Located in lower right corner.
               •   Visualizes the world coordinate system directions.
               •   Positive directions arrows are labeled and color-coded. Negative direction arrows display
                   only when you hover the mouse cursor over the particular region.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                          163
The Mechanical Application Basics

               •   Clicking an arrow animates the view such that the arrow points out of the screen.
               •   Arrows and the isometric sphere highlight when you point at them.
               •   Isometric sphere visualizes the location of the isometric view relative to the current
                   view.
               •   Clicking the sphere animates the view to isometric.

Rotation
               Click the Rotate button                    to display and activate the following rotation cursors:
Cursors
               •
                         Free rotation.
               •
                         Rotation around an axis that points out of the screen (roll).
               •
                         Rotation around a vertical axis relative to the screen ("yaw" axis).
               •
                         Rotation around a horizontal axis relative to the screen ("pitch" axis).


Cursor Location Determines Rotation Behavior
The type of rotation depends on the starting location of the cursor. In general, if the cursor is near the
center of the graphics window, the familiar 3D free rotation occurs. If the cursor is near a corner or edge, a
constrained rotation occurs: pitch, yaw or roll.

Specifically, the circular free rotation area fits the window. Narrow strips along the edges support pitch and
yaw. Corner areas support roll. The following figure illustrates these regions.




Customizing the Mechanical Application
   The Mechanical Application Options (p. 164)
   Variables (p. 171)
   Macros (p. 172)

The Mechanical Application Options
You can control the behavior of functions in the Mechanical application through the Options dialog box.
To access the Mechanical application options:

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
164                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                         Connections

 1.       From the main menu, choose Tools> Options. An Options dialog box appears and the Mechanical
          application options are displayed on the left.
 2.       Click on a specific option.
 3.       Change any of the option settings by clicking directly in the option field on the right. You will first see
          a visual indication for the kind of interaction required in the field (examples are drop-down menus,
          secondary dialog boxes, direct text entries).
 4.       Click OK.

The following Mechanical application options appear in the Options dialog box:

      Connections
      Convergence
      Export
      Fatigue
      Frequency
      Geometry
      Graphics
      Miscellaneous
      Report
      Analysis Settings and Solution
      Visibility
      Wizard

Connections
The Auto Detection category allows you to change the default values in the Details view for the following:

 •    Auto Detect Contact on Attach: Indicates if contact detection should be computed upon geometry
      import or not. The default is Yes.
 •    Tolerance: Sets the default for the contact detection slider; i.e., the relative distance to search for contact
      between parts. The higher the number, the tighter the tolerance. In general, creating contacts at a toler-
      ance of 100 finds less contact surfaces than at 0. The default is 0. The range is from -100 to +100.
 •    Face/Face: Sets the default preference1 for automatic contact detection between faces of different
      parts. The choices are Yes or No. The default is Yes.
 •    Face/Edge: Sets the default preference1 for automatic contact detection between faces and edges of
      different parts. The choices are:
      –     Yes
      –     No (default)
      –     Only Solid Body Edges
      –     Only Surface Body Edges
 •    Edge/Edge: Sets the default preference1 for automatic contact detection between edges of different
      parts. The choices are Yes or No. The default is No.
 •    Priority: Sets the default preference1 for the types of contact interaction priority between a given set
      of parts. The choices are:
      –     Include All (default)
      –     Face Overrides
      –     Edge Overrides

                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                      165
The Mechanical Application Basics

    •   Revolute Joints: Sets the default preference for automatic joint creation of revolute joints. The choices
        are Yes and No. The default is Yes.
    •   Fixed Joints: Sets the default preference for automatic joint creation of fixed joints. The choices are
        Yes and No. The default is Yes.
1
Unless changed here in the Options dialog box, the preference remains persistent when starting any
Workbench project.

The Transparency category includes the following exclusive controls for this category. There are no coun-
terpart settings in the Details view.

    •   Parts With Contact: Sets transparency of parts in selected contact region so the parts are highlighted.
        The default is 0.8. The range is from 0 to 1.
    •   Parts Without Contact: Sets transparency of parts in non-selected contact regions so the parts are not
        highlighted. The default is 0.1. The range is from 0 to 1.

The Default category allows you to change the default values in the Details view for the following:

    •   Type: Sets the definition type of contact. The choices are:
        –   Bonded (default)
        –   No Separation
        –   Frictionless
        –   Rough
        –   Frictional
    •   Formulation: Sets the type of contact formulation method. The choices are:
        –   Augmented Lagrange
        –   Pure Penalty (default)
        –   MPC
        –   Normal Lagrange
    •   Update Stiffness: Enables an automatic contact stiffness update by the program. The choices are:
        –   Never (default)
        –   Each Equilibrium Iteration
        –   Each Substep
    •   Auto Rename Connections: Automatically renames joint, spring, contact region, and joint condition
        objects when Type or Scoping are changed. The choices are Yes and No. The default is Yes.

Convergence
The Convergence category allows you to change the default values in the Details view for the following:

    •   Target Change: Change of result from one adapted solution to the next. The default is 20. The range
        is from 0 to 100.
    •   Allowable Change: This should be set if the criteria is the max or min of the result. The default is Max.

The Solution category allows you to change the default values in the Details view for the following:



                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
166                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                        Fatigue

 •   Max Refinement Loops: Allows you to change the number of loops . The default is 1. The range is
     from 1 to 10.

Export
The Export category includes the following exclusive controls for this category. There are no counterpart
settings in the Details view.

 •   Automatically Open Excel: Excel will automatically open with exported data. The default is Yes.
 •   Include Node Numbers: Nodal numbers will be included in exported file. The default is Yes.
 •   Include Node Location: Nodal location can be included in exported file. The default is No.

Fatigue
The General category allows you to change the default values in the Details view for the following:

 •   Design Life: Number of cycles that indicate the design life for use in fatigue calculations. The default
     is 1e9.
 •   Analysis Type: The default fatigue method for handling mean stress effects. The choices are:
     –   SN - None (default)
     –   SN - Goodman
     –   SN - Soderberg
     –   SN - Gerber
     –   SN - Mean Stress Curves

     The Goodman, Soderberg, and Gerber options use static material properties along with S-N data to ac-
     count for any mean stress while Mean-Stress Curves use experimental fatigue data to account for mean
     stress.

The Cycle Counting category allows you to change the default values in the Details view for the following:

 •   Bin Size: The bin size used for rainflow cycle counting. A value of 32 means to use a rainflow matrix of
     size 32 X 32. The default is 32. The range is from 10 to 200.

The Sensitivity category allows you to change the default values in the Details view for the following:

 •   Lower Variation: The default value for the percentage of the lower bound that the base loading will
     be varied for the sensitivity analysis. The default is 50.
 •   Upper Variation: The default value for the percentage of the upper bound that the base loading will
     be varied for the sensitivity analysis. The default is 150.
 •   Number of Fill Points: The default number of points plotted on the sensitivity curve. The default is 25.
     The range is from 10 to 100.
 •   Sensitivity For: The default fatigue result type for which sensitivity is found. The choices are:
     –   Life (default)
     –   Damage
     –   Factor of Safety




                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                  167
The Mechanical Application Basics

Frequency
The Frequency category allows you to change the default values in the Details view for the following:

 •    Max Number of Modes: The number of modes that a newly created frequency branch will contain.
      The default is 6. The range is from 1 to 200.
 •    Limit Search to Range: You can specify if a frequency search range should be considered in computing
      frequencies. The default is No.
 •    Min Range: Lower limit of search range. The default is 0.
 •    Max Range: Upper limit of search range. The default is 100000000.

Geometry
The Geometry category allows you to change the default values in the Details view for the following:

 •    Nonlinear Material Effects: Indicates if nonlinear material effects should be included (Yes), or ignored
      (No). The default is Yes.
 •    Thermal Strain Calculation: Indicates if thermal strain calculations should be included (Yes), or ignored
      (No). The default is Yes.

      Note

      This setting applies only to newly attached models, not to existing models.

Graphics
The Default Graphics Options category allows you to change the default values in the Details view for the
following:

 •    Show Min Annotation: Indicates if Min annotation will be displayed by default (for new databases).
      The default is No.
 •    Show Max Annotation: Indicates if Max annotation will be displayed by default (for new databases).
      The default is No.
 •    Contour Option: Selects default contour option. The choices are:
      –   Smooth Contour
      –   Contour Bands (default)
      –   Isolines
      –   Solid Fill
 •    Edge Option: Selects default edge option. The choices are:
      –   No Wireframe (default)
      –   Show Undeformed Wireframe
      –   Show Undeformed Model
      –   Show Elements
 •    Highlight Selection: Indicates default face selection. The choices are:
      –   Single Side (default)


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
168                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Report

     –   Both Sides

Miscellaneous
The Miscellaneous category allows you to change the default values in the Details view for the following:

 •   Load Orientation Type: Specifies the orientation input method for certain loads. This input appears in
     the Define By option in the Details view of the load, under Definition.
     –   Vector (default)
     –   Component

The Image category includes the following exclusive controls for this category. There are no counterpart
settings in the Details view.

 •   Image Transfer Type: Defines the type of image file created when you send an image to Microsoft
     Word or PowerPoint, or when you select Print Preview. The choices are:
     –   PNG (default)
     –   JPEG
     –   BMP

Report
The Figure Dimensions (in Pixels) category includes the following controls that allow you to make changes
to the resolution of the report for printing purposes.

 •   Chart Width - Default value equals 600 pixels.
 •   Chart Height - Default value equals 400 pixels.
 •   Graphics Width - Default value equals 600 pixels.
 •   Graphics Height - Default value equals 500 pixels.
 •   Graphics Resolution - Resolution values include:
     –   Optimal Onscreen Display (1:1)
     –   Enhanced Print Quality (2:1)
     –   High-Resolution Print Quality (4:1)

The Customization category includes the following controls:

 •   Maximum Number of Table Columns - (default = 6 columns) Changes the number of columns used
     when a table is created.
 •   Merge Identical Table Cells - Merges cells that contain identical values. The default value is Yes.
 •   Omit Part and Joint Coordinate System Tables - Chooses whether to include or exclude Coordinate
     System data within the report. This data can sometimes be cumbersome. The default value is Yes.
 •   Include Figures - Specifies whether to include Figure objects as pictures in the report. You may not
     want to include figures in the report when large solved models or models with a mesh that includes
     many nodes and elements are involved. In these cases, figure generation can be slow, which could
     significantly slow down report generation. The default value is Yes.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 169
The Mechanical Application Basics


           Note

           This option applies only to Figure objects as pictures. Graph pictures, Engineering Data
           graphs, and result graphs (such as phase response in a harmonic analysis) are not affected
           and will appear regardless of this option setting.


 •    Custom Report Generator Folder - Reports can be run outside of the Workbench installation directory
      by copying the Workbench Report2006 folder to a new location. Specify the new folder location in this
      field. Please see the Customize Report Content section for more information.

Analysis Settings and Solution
The Solver Controls category allows you to change the default values in the Details view for the following:

 •    Solver Type: Specifies which ANSYS solver will be used. The choices are:
      –   Program Controlled (default)
      –   Direct
      –   Iterative
 •    Use Weak Springs: Specifies whether weak springs are added to the model. The Programmed Controlled
      setting automatically allows weak springs to be added if an unconstrained model is detected, if unstable
      contact exists, or if compression only supports are active. The choices are:.
      –   Program Controlled (default)
      –   On
      –   Off

The Output Controls category allows you to change the default values in the Details view for the following
(all are originally set to Yes):

 •    Calculate Stress
 •    Calculate Strain
 •    Calculate Thermal Flux

The Solution Information category allows you to change the default value in the Details view for the fol-
lowing:

 •    Refresh Time: Specifies how often any of the result tracking items under a Solution Information object
      get updated while a solution is in progress. The default is 2.5 s.

Visibility
The Visibility category includes the following exclusive controls for this category. There are no counterpart
settings in the Details view.

 •    Mesh Folder: Indicates if mesh folder should appear in the Tree Outline. You may not want to see or
      know about meshes. The default is Visible.
 •    Part Mesh Statistics: Indicates if mesh information (the number of nodes and elements) should show
      in the Details view of a part. The default is Visible.
 •    Fatigue Tool: Turns on/off Fatigue tool capability. The default is Visible.


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
170                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Variables

 •   Shape Finder: Turns on/off Shape finder capability. The default is Visible.
 •   Contact Tool: Turns on/off Contact Tool capability. The default is Visible.

Wizard
The Wizard Options category includes the following exclusive controls for this category. There are no
counterpart settings in the Details view.

 •   Default Wizard: This is the URL to the XML wizard definition to use by default when a specific wizard
     isn't manually chosen or automatically specified by a simulation template. The default is StressWiz-
     ard.xml.
 •   Flash Callouts: Specifies if callouts will flash when they appear during wizard operation. The default is
     Yes.

The Skin category includes the following exclusive controls for this category. There are no counterpart settings
in the Details view.

 •   Cascading Style Sheet: This is the URL to the skin (CSS file) used to control the appearance of the
     Mechanical Wizard. The default is Skins/System.css.

The Customization Options category includes the following exclusive controls for this category. There are
no counterpart settings in the Details view.

 •   Mechanical Wizard URL: For advanced customization. See Appendix: Workbench Mechanical Wizard
     Advanced Programming Topics for details.
 •   Enable WDK Tools: Advanced. Enables the Wizard Development Kit. The WDK adds several groups of
     tools to the Mechanical Wizard. The WDK is intended only for persons interested in creating or modifying
     wizard definitions. The default is No. See the Appendix: Workbench Mechanical Wizard Advanced Program-
     ming Topics for details.

     Note
      •   URLs in the Mechanical Wizard follow the same rules as URLs in web pages.
      •   Relative URLs are relative to the location of the Mechanical Wizard URL.
      •   Absolute URLs may access a local file, a UNC path, or use HTTP or FTP.


User Preferences File
The Mechanical application stores the configuration information from the Options dialog box in a file called
a User Preference File on a per user basis. This file is created the first time you start the Mechanical application.
Its default location is:

C:\Documents and Settings\<user initials>\Application Data\Ansys\v120\en-
us\dsPreferences.xml

Variables
Variables provide you the capability to override default settings.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                    171
The Mechanical Application Basics

 To set variables:
 1.     Choose Variable Manager from the Tools menu.
 2.     Right-click in the row to add a new variable.
 3.     Enter a variable name and type in a value.
 4.     Click OK.

      Variable name         Allowable Values                                                           Description
DSMESH OUTPUT             filename                                Writes mesher messages to a file during solve (default = no
                                                                  file written). If the value is a filename, the file is written to
                                                                  the temporary working folder (usually c:\temp).To write
                                                                  the file to a specific location, specify the full path.
DSMESH DEFEA-             a number between                        Tolerance used in simplifying geometry (default = .0005).
TUREPERCENT               1e-6 and 1e-3

Status
The status box indicates if a particular variable is active or not. Checked indicates that the variable is active.
Unchecked indicates that the variable is available but not active. This saves you from typing in the variable
and removing it.

Macros
The Mechanical application allows you to execute custom functionality that is not included in a standard
Mechanical application menu entry via its Run Macro feature. The functionality is defined in a macro - a
script that accesses the Mechanical application programming interface (API).

Macros can be written in Microsoft's JScript or VBScript programming languages. Several macro files are
provided with the ANSYS Workbench installation under \ANSYS
Inc\v120\AISOL\DesignSpace\DSPages\macros. Macros cannot currently be recorded from the
Mechanical application.

 To access a macro from the Mechanical application:
 1.     Choose Run Macro... from the Tools menu.
 2.     Navigate to the directory containing the macro.
 3.     Open the macro. The functionality will then be accessible from the Mechanical application.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
172                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Using the Mechanical Application Features
The following topics are included in this section:
 Geometry in the Mechanical Application
 Coordinate Systems Overview
 Graphics
 Analysis Settings
 Applying Loads
 Results in the Mechanical Application
 Solving Overview
 Commands Objects
 Report Preview
 Customize Report Content
 Meshing in the Mechanical Application
 Parameters
 Fatigue Overview
 Contact
 Body Interactions in Explicit Dynamics Analyses
 Virtual Topology in the Mechanical Application

Geometry in the Mechanical Application
The following topics are included in this section:
 Assemblies, Parts, and Bodies
 Solid Bodies
 Surface Bodies
 Rigid Bodies
 Path
 Remote Point
 Point Mass
 Contact
 Spot Welds
 Joints
 Springs
 Beam
 Virtual Topology

Assemblies, Parts, and Bodies
While there is no limit to the number of parts in an assembly that can be treated, large assemblies may require
unusually high computer time and resources to compute a solution. Contact boundaries can be automatically
formed where parts meet. The application has the ability to transfer structural loads and heat flows across
the contact boundaries and to "connect" the various parts.

Parts are a grouping or a collection of bodies. Parts can include multiple bodies and are referred to as
multibody parts. The mesh for multibody parts created in DesignModeler will share nodes where the bodies


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               173
Using the Mechanical Application Features

touch one another, that is, they will have common nodes at the interfaces. This is the primary reason for
using multibody parts.

Parts may consist of:

 •    One or more solid bodies.
 •    One or more shell bodies.
 •    One or more line bodies.
 •    Combinations of line and shell bodies.

All other combinations are not practically supported.

      Note

      Body objects in the tree that represent a multibody part do not report centroids or moments of
      inertia in their respective Details view.

Multibody Behavior
When transferring multibody parts from DesignModeler to the Meshing application, the multibody part has
the body group (part) and the prototypes (bodies) beneath it. When the part consists of just a single body
the body group is hidden. If the part has ever been imported as a multibody part you will always see the
body group for that component, regardless of the number of bodies present in any subsequent update.

Working with Parts
There are several useful and important manipulations that can be performed with parts in an assembly.

 •    Each part may be assigned a different material.
 •    Parts can be hidden for easier visibility.
 •    Parts can be suppressed, which effectively eliminates the parts from treatment.
 •    The contact detection tolerance and the contact type between parts can be controlled.
 •    When a model contains a Coordinate Systems object, by default, the part and the associated bodies
      use the Global Coordinate System to align the elements. If desired, you can apply a local coordinate
      system to the part or body. When a local coordinate system is assigned to a Part, by default, the bodies
      also assume this coordinate system but you may modify the system on the bodies individually as desired.

Integration Schemes
Parts can be assigned Full or Reduced integration schemes. The full method is used mainly for purely linear
analyses, or when the model has only one layer of elements in each direction. This method does not cause
hourglass mode, but can cause volumetric locking in nearly incompressible cases. The reduced method helps
to prevent volumetric mesh locking in nearly incompressible cases. However, hourglass mode might
propagate in the model if there are not at least two layers of elements in each direction.

Color Coding of Parts
You can visually identify parts based on a property of that part. For example if an assembly is made of parts
of different materials you can color the parts based on the material, that is all structural steel parts have the
same color, all aluminum parts with the same color and so on.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
174                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Working with Bodies

Select a color via the Display Style field of the Details view when the Geometry branch in the feature Tree
is selected. The default is Part Color which will assign different colors to different parts. You can also specify
colors based on:

 •   Material: The part colors are based on the material assignment. For example in a model with five parts
     where three parts use structural steel and two parts use aluminum, you will see the three structural
     steel parts in one color and the two aluminum parts in another color. The legend will indicate the color
     used along with the name of the material.
 •   Nonlinear Material Effects: Indicates if a part includes nonlinear material effects during analysis. If you
     chose to exclude nonlinear material effects for some parts of a model, then the legend will indicate
     Linear for these parts and the parts will be colored accordingly.
 •   Stiffness Behavior: Identifies a part as Flexible or Rigid during analysis.

     Note

     A maximum of 15 distinct materials can be shown in the legend. If a model has more then 15
     materials, coloring by material will not have any effect unless enough parts are hidden or sup-
     pressed.

Example 1 Color by Parts




Working with Bodies
There are several useful and important manipulations that can be performed with bodies in a part.

 •   Bodies grouped into a part result in connected geometry and shared nodes in a mesh.
 •   Each body may be assigned a different material.
 •   Bodies can be hidden for easier visibility.
 •   Bodies in a part group can be individually suppressed, which effectively eliminates these bodies from
     treatment. A suppressed body is not included in the statistics of the owning part or in the overall stat-
     istics of the model.
 •   Bodies can be assigned Full or Reduced integration schemes, as described above for parts.
 •   When bodies in part groups touch they will share nodes where they touch. This will connect the bodies.
     If a body in a part group does not touch another body in that part group, it will not share any nodes.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              175
Using the Mechanical Application Features

      It will be free standing. Automatic contact detection is not performed between bodies in a part group.
      Automatic contact detection is performed only between part groups.
 •    Bodies that are not in a part group can be declared as rigid bodies.
 •    When a model contains a Coordinate Systems object, by default, bodies use the Global Coordinate
      System. If desired, you can apply a local coordinate system.

To Hide or Suppress Bodies
For a quick way to hide bodies (that is, turn body viewing off ) or suppress bodies (that is, turn body viewing
off and remove the bodies from further treatment in the analysis), select the bodies in the tree or in the
Geometry window (choose the Body select mode, either from the toolbar or by a right-click in the Geometry
window). Then right-click and choose Hide Body or Suppress Body from the context menu. Choose Show
Body, Show All Bodies, Unsuppress Body, or Unsuppress All Bodies to reverse the states.

The following options are also available:

 •    Hide All Other Bodies, allows you to show only selected bodies.
 •    Suppress All Other Bodies, allows you to unsuppress only selected bodies.

Assumptions and Restrictions for Assemblies, Parts, and Bodies
Thermal and shape analysis is not supported for surface bodies or line bodies.

In order for multiple bodies inside a part to be properly connected by sharing a node in their mesh the
bodies must share a face or edge. If they do not share a face or an edge the bodies will not be connected
for the analysis which could lead to rigid body motion.

Automatic contact detection will detect contact between bodies within a multibody part.

Solid Bodies
You can process and solve solid models, including individual parts and assemblies. An arbitrary level of
complexity is supported, given sufficient computer time and resources.

Surface Bodies
You can import surface bodies from an array of sources (see Geometry Preferences (p. 604)). Surface bodies
are often generated by applying mid-surface extraction to a pre-existing solid. The operation abstracts away
the thickness from the solid and converts it into a separate modeling input of the generated surface.

Surface body models may be arranged into parts. Within a part there may be one or more surface bodies;
these may even share the part with line bodies.

Parts that feature surface bodies may be connected with the help of spot welds and contacts.

Importing Surface Body Models
To import a surface body model (called a sheet body in NX), open the model in the CAD system and import
the geometry as usual. If your model mixes solid bodies and surface bodies, you should select which type
of entity you want to import via the Geometry preferences in the Workbench Properties of the Geometry
cell in the Project Schematic. Once in the Mechanical application, you can adjust the Geometry preferences
in the Details view, where they take effect upon updating.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
176                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Rigid Bodies


     Note

     If you want to retain a preference selection in the Workbench Properties, you must first save
     before exiting the ANSYS Workbench.

Importing Surface Body Thickness
Surface body thickness will be imported from CAD (including DesignModeler) if, and only if, the existing
surface body thickness value in the Mechanical application is set to 0 (zero). This is true on initial attach and
if you set the surface body thickness value to zero prior to an update. This allows you the flexibility of up-
dating surface body thickness values from CAD or not.

Thickness Mode
You can determine the source that controls the thickness of a surface body using the Thickness Mode in-
dication combined with the Thickness field, both located in the Details view of a surface Body object. Upon
attaching a surface body, the Thickness Mode reads either Auto or Manual.

 •   In Auto Mode the value of thickness for a given surface body is controlled by the CAD source. Future
     CAD updates will synchronize its thickness value with the value in the CAD system.
 •   In Manual mode the thickness for the surface body is controlled by the Mechanical application, so future
     updates from the CAD system will leave this value undisturbed.
 •   A Thickness Mode will be Automatic until the Thickness is changed to some non-zero value. Once in
     Manual mode, it can be made Automatic once again by changing the Thickness value back to zero.
     A subsequent CAD update will conveniently synchronize the thickness with the value in the CAD system.

Thicknesses for all surface bodies are represented in a dedicated column on the Worksheet tab that is dis-
played when you highlight the Geometry object.

Surface Body Offsets
You can build in offsets for a surface body using the Offset Type drop down menu located in the Details
view of a surface Body object. Upon attaching a surface body, the Offset Type setting includes the following
options for offsetting the surface body:
 •   Top
 •   Middle Membrane (default)
 •   Bottom
 •   User Defined - If chosen, a Membrane Offset field is also available where you can enter a positive or
     negative offset value in length units.
 •   User Defined - If chosen, a Membrane Offset field is also available where you can enter a positive or
     negative offset value in length units.

Rigid Bodies
You can declare the stiffness behavior of a single solid body (a body that is not a component of a multibody
part), a body group, surface bodies, and 2D models to be rigid or flexible. A rigid body will not deform during
the solution. This feature is useful if a mechanism has only rigid body motion or, if in an assembly, only
some of the parts experience most of the strains. It is also useful if you are not concerned about the
stress/strain of that component and wish to reduce CPU requirements during meshing or solve operations.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       177
Using the Mechanical Application Features

 To set the stiffness behavior in the Mechanical application
 1.    Select a body in the tree.
 2.    In the Details view, set Stiffness Behavior to Rigid or Flexible.

To define a rigid body, set the field of the Details view to Rigid when the body object is selected in the
tree. If rigid, the body will not be meshed and will internally be represented by a single mass element during
the solution. (The mass element’s mass and inertial properties will be maintained.) The mass, centroid, and
moments of inertia for each body can be found in the Details view of the body object.

The following restrictions apply to rigid bodies:

 •    Rigid bodies are only valid in static structural, transient structural (ANSYS) , transient structural (MBD) ,
      and modal analyses for the objects listed below. Animated results are available for all analysis types
      except modal.
      –       Point mass
      –       Joint
      –       Spring
      –       Remote displacement
      –       Remote force
      –       Moment
      –       Contact
 •    Rigid bodies are valid when scoped to solid bodies, surface bodies, or line bodies in Explicit Dynamics
      Analysis (p. 20) for the following objects:
      –       Fixed support
      –       Displacement
      –       Velocity

The following outputs are available for rigid bodies, and are reported at the centroid of the rigid body:

 •    Results: Displacement, Velocity, and Acceleration
 •    Probes: Deformation, Position, Rotation, Velocity, Acceleration, Angular Velocity, and Angular Acceleration

      Note
          •    If you highlight Deformation results in the tree that are scoped to rigid bodies, the corres-
               ponding rigid bodies in the Geometry window are not highlighted.
          •    You cannot define a line body, 2D plane strain, and axisymmetric model as rigid.
          •    All the bodies in a body group must have similar stiffness behavior.


Path
A path is categorized as a form of construction geometry and is represented as a spatial curve to which you
can scope path results. The results are evaluated at discrete points along this curve.

A path can be defined in two principal ways:


                             Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
178                                                      of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                Defining a Path using Two Points

 •    By start point and end point.

      These points can be specified directly or can be calculated from the entry and exit point (intersections)
      of the positive X-axis of a coordinate system through a mesh. The path may be a straight line segment
      or a curve depending on the type of coordinate system (Cartesian or Cylindrical). You can control the
      discretization by specifying the number of sampling points, and these will be evenly distributed along
      the path up to a limit of 200.
 •    By an edge.

      The discretization will include all nodes in the mesh underlying the edge.

For each result scoped to a Path, the Graph Controls category provides an option to display the result in
the Graph on X-axis, as a function of Time or with S, the length of the path. Note that Path results have
the following restrictions: They are calculated on solids and surfaces but not on lines. They can be collected
into charts as long as all of the other objects selected for the chart have the same X-axis (Time or S). You
can define a path in the geometry by specifying two points, an edge, or an axis. Before you define a path,
you must first add the Path object from the Construction Geometry context toolbar. You can then define
the path using any of the three methods presented below.




Defining a Path using Two Points
Using this method you can define the path by specifying the coordinates for the two points or by selecting
an edge, face or vertex. To define the Path using coordinates:

 1.    In the Details view, select Two Points in the Path Type list.
 2.    Under Start, enter the X, Y, and Z coordinates for the starting point of the path.
 3.    Under End, enter the X, Y, and Z coordinates for the ending point of the path.

To define a Path using a vertex, edge or face:

 1.    In the Details view, select Two Points in the Path Type list.
 2.    Select a vertex, edge or face where you want to start the path, and then click Apply under Start,
       Location.
 3.    Select a vertex, edge, or face where you want to end the path, and then click Apply under End, Loca-
       tion.
 4.    Enter the Number of Sampling Points.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                      179
Using the Mechanical Application Features

Defining a Path using an Edge
This method helps you define a path by selecting an edge. To define a path:

 1.    In the Details view, select Edge in the Path Type list.
 2.    Select a geometry edge, and then click Apply under Scope.

Defining a Path using X-axis Intersection
Depending on the coordinate system you select, Workbench creates a Path from the coordinate system
origin to the point where the X-axis of the selected coordinate system intersects a geometry boundary.
Workbench computes intersections of the axis with the mesh and displays more precise locations for path
endpoints for the path results. The endpoints for the path are not modified, and remain as the intersections
with the geometry.

 1.    In the Details view, select X Axis Intersection in the Path Type list.
 2.    Select the coordinate system you want to use to define the x-axis.
 3.    Enter the Number of Sampling Points.

Exporting Path Data
You can export coordinate data for a defined path by clicking the right mouse button on a Path object and
choosing Export from the context menu.

Remote Point
The following topics are addressed in this section:
 Remote Point Overview
 Connection Lines
 Promote Remote Point
 Remote Point Commands Objects

Remote Point Overview
You use a Remote Point as a scoping mechanism for remote boundary conditions. Remote points are a way
of abstracting connection to geometry. They are similar to the various remote loads available in the Mech-
anical application (displayed in the list below). Remote points provide a way to establish a point in space
associated to a portion of geometry that can have multiple boundary conditions scoped to it. The single
remote association will avoid overconstraint conditions that can occur when multiple remote loads are
scoped to the same geometry. The overconstraint occurs because multiple underlying contact elements are
used for the individual remote loads when applied as usual to the geometry. When the multiple remote
loads are applied to a single remote point scoped to the geometry the possibility of overconstraint is greatly
reduced.

To insert a Remote Point, select a Model branch and either select the Remote Point button from the
toolbar, or right-click the mouse and select Insert> Remote Point from the context menu. You then apply
it to:

 •    A face, edge, or vertex of a solid body or of a 3D surface body.
 •    An edge or vertex of a 2D surface body or a line body.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
180                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Remote Point

A remote point or multiple remote points work in tandem with the remote boundary conditions listed below.
Remote Point definable settings include a Geometry selection, a Coordinate System, Location, Behavior
(Deformable or Rigid) as well as a Pinball Region.

 •   Point Mass
 •   Joints
 •   Springs
 •   Remote Displacement
 •   Remote Force
 •   Moment

These objects acquire data from remote points and eliminate the need to define the objects individually.
You can scope one or more of the above objects to a defined Remote Point. This provides a central object
to which you can make updates that will affect the scoping of multiple objects.

     Caution

     A Remote Point can reference only one Remote Force and one Moment. If you scope a Remote
     Point to multiple remote forces or moments, duplicate specifications are ignored and a warning
     message is generated.

The Details view of each of the above objects contains a Scoping Method setting that can be set to Remote
Point, once a Remote Point is defined, as illustrated below for the details of a Remote Force. Once you
scope the object with a Remote Point and define which remote point (Remote Point or Remote Point2)
if more than one exists, all of the inputs from that remote point become read-only for the object and use
the remote point's data.

Scope to Remote Point




Choose Appropriate Remote Point



                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                       181
Using the Mechanical Application Features




Example Data for Selected Remote Point




Once a remote force is directed to a Remote Point, additional data may be required, such as Magnitude,
as shown above.

Connection Lines
The connection between the underlying geometry associated with a remote point and the remote point itself
can be visualized by connection lines. You can enable this feature through the Show Connection Lines
property under Graphics in the Details view of the Remote Points object.

If a mesh was generated, the connection lines are drawn between a remote point and the nodes on the
corresponding meshed underlying geometry.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
182                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Point Mass

The connection lines take the Pinball radius into account, and only those nodes that are inside that radius
will be connected with the remote point.

Any remote loads that have been promoted to reference remote points will have these lines drawn when
their object is selected as well.

An example illustration of connection lines is shown below.




Promote Remote Point
The Promote Remote Point feature helps you add a remote point from the context menu for remote
boundary conditions. When you use Promote Remote Point, Workbench adds a remote point object with
the remote boundary condition name and the associated data in the Project tree. To add a remote point
from the remote boundary conditions:

 1.   On the Environment context toolbar, click the appropriate boundary condition.
 2.   Right-click the remote boundary condition object, and then click Promote Remote Point. A remote
      point with the boundary condition name and data is added to the Project tree.
 3.   In the Project tree, select the new remote point object and modify its data as necessary.

Remote Point Commands Objects
A Command object can be placed in the tree as a child object of a Remote Point providing you program-
mable access to the Remote Point pilot node. This is useful if you wish to apply conditions to the Remote
Point that are not supported in Workbench, such as beam or constraint equations.

Point Mass
You can idealize the inertial effects from a body using a Point Mass. Applications include applying a force
with an acceleration or any other inertial load; or adding inertial mass to a structure, which affects modal
and harmonic solutions.

To insert a Point Mass, select a Geometry branch and either choose Point Mass from the toolbar, or right
mouse button click and choose Insert> Point Mass from the context menu. You then apply it on a face of
a solid or surface model, or on an edge of a surface model.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                     183
Using the Mechanical Application Features

You cannot apply a Point Mass on any shared topology surface. Also, the scoping of a Point Mass cannot
span multiple bodies if the Stiffness Behavior of the bodies is declared as Rigid (see Rigid Bodies section
for additional information).

The location of the Point Mass can be anywhere in space and can also be defined in a local coordinate
system if one exists. The default location is at the centroid of the geometry. You can also input moment of
inertia values for each direction. The Point Mass will automatically be rotated into the selected coordinate
system if that coordinate system differs from the global coordinate system.

A Point Mass is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 319)
section for a listing of all remote boundary conditions and their characteristics.

Contact
You can transfer loads and heat flows across the contact boundaries and “connect” the various parts. See
the Contact section for details.

Spot Welds
Spot welds are used to connect individual surface body parts together to form surface body model assemblies,
just as contact is used for solid body part assemblies. Structural loads are transferred from one surface body
part to another via the spot weld connection points, allowing for simulation of surface body model assemblies.

Spot Weld Details
Spot welds are usually defined in the CAD system and automatically generated upon import, although you
can define them manually in the Mechanical application after the model is imported. Spot welds then become
hard points in the geometric model. Hard points are vertices in the geometry that are linked together using
beam elements during the meshing process.

Spot weld objects are located in the Connections object in the Tree Outline (p. 118). When selected in the
tree, they appear in the graphical window highlighted by a black square around a white dot on the under-
lying vertices, with an annotation.

If a surface body model contains spot weld features in the CAD system, then spot welds are auto-generated
when the model is read into the Mechanical application or when Generate Contact on Update is set to
Yes in the Details view of the Connections object in the Tree Outline (p. 118). This is similar to the way in
which the Mechanical application automatically constructs contact condition when reading in assemblies
of solid models.

You can manually generate spot welds as you would insert any new object into the Outline tree. Either insert
a spot weld object from the context menu and then pick two appropriate vertices in the model, or pick two
appropriate vertices and then insert the spot weld object.

You can define spot welds for CAD models that do not have a spot weld feature in the CAD system, as long
as the model contains vertices at the desired locations. You must define spot welds manually in these cases.

Spot Weld Assumptions and Restrictions
Spot welds do not act to prevent penetration of the connected surface body in areas other than at the spot
weld location. Penetration of the joined surface body is possible in areas where spot welds do not exist.

Spot welds only transfer structural loads and structural effects between surface body parts. Therefore they
are appropriate for displacement, stress, elastic strain, and frequency solutions.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
184                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Joint Initial Conditions

DesignModeler generates spot welds. The only CAD system whose spot welds can be fully realized in ANSYS
Workbench at this time is NX. The APIs of the remaining CAD systems either do not handle spot welds, or
the ANSYS Workbench software does not read spot welds from these other CAD systems.

Joints
The following topics are covered in this section:
 Joint Characteristics
 Types of Joints
 Joint Properties and Application
 Example: Assembling Joints
 Example: Configuring Joints
 Automatic Joint Creation
 Joint Stops and Locks
 Ease of Use Features
 Detecting Overconstrained Conditions

Joint Characteristics
A joint typically serves as a junction where bodies are joined together. Joint types are characterized by their
rotational and translational degrees of freedom as being fixed or free.

Nature of Joint Degrees of Freedom
 •   For all joints that have both translational degrees of freedom and rotational degrees of freedom, the
     kinematics of the joint is as follows:
     1.   Translation: The moving coordinate system translates in the reference coordinate system. If your
          joint is a slot for example, the translation along X is expressed in the reference coordinate system.
     2.   Once the translation has been applied, the center of the rotation is the location of the moving
          coordinate system.
 •   For the ANSYS Mechanical solver, the relative angular positions for the spherical, general, and bushing
     joints are characterized by the Cardan (or Bryant) angles. This requires that the rotations about the
     local Y axis be restricted between –π/2 to +π/2. Thus, the local Y axis should not be used to simulate
     the axis of rotation if the expected rotation is large.

Joint Abstraction
Joints are considered as point to point in the solution but the user interface shows the actual geometry.
Due to this abstraction to a point to point joint, geometry interference and overlap between the two parts
linked by the joint can be seen during an animation.

Joint Initial Conditions
The nature of the degrees of freedom differs based on the selected solver. For the ANSYS Rigid Dynamics
solver, the degrees of freedom are the relative motion between the parts. For the ANSYS Mechanical solver,
the degrees of freedom are the location and orientation of the center of mass of the bodies. Unless specified
otherwise by using joint conditions, both solvers will start with initial velocities equal to zero, but that means
two different things, as explained below.

 •   For the ANSYS Mechanical solver, not specifying anything means that the bodies will be at rest.
 •   For the ANSYS Rigid Dynamics solver, not specifying anything means that the relative velocities will
     be at rest.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                               185
Using the Mechanical Application Features

Taking the example of an in-plane double pendulum, and prescribing a constant velocity for the first
grounded link will be interpreted as follows:

 •    The second link has the same rotational velocity as the first one for the ANSYS Rigid Dynamics solver,
      as the relative velocity is initially equal to zero.
 •    The second link will start at rest for the ANSYS Mechanical solver.

Joint DOF Zero Value Conventions
Joints can be defined using one or two coordinate systems: the Reference Coordinate System and the
Mobile Coordinate System.

The use of two coordinate systems provides benefits. An example is when a CAD model is not imported in
an assembled configuration. In addition, it is important to define two coordinate systems so that you can
employ the Configure and Set (see Applying Joints (p. 198)) features as well as having the ability to update
a model following a CAD update.

For the ANSYS Rigid Dynamics solver, the zero value of the degrees of freedom corresponds to the
matching reference coordinate system and moving coordinate system.

If a joint definition includes only the location of the Mobile Coordinate System (see Joint Coordinate Sys-
tems (p. 194)), then the DOF of this joint are initially equal to zero for the geometrical configuration where
the joints have been built.

If the Reference Coordinate System is defined using the Override option, then the initial value of the degrees
of freedom can be a non-zero value.

Consider the example illustrated below. If a Translational joint is defined between the two parts using two
coordinate systems, then the distance along the X axis between the two origins is the joint initial DOF value.
For this example, assume it is 65 mm.




On the other hand, if the joint is defined using a single coordinate, as shown below, then the same geomet-
rical configuration has a joint degree of freedom that is equal to zero.




For the ANSYS Mechanical solver, having one or two coordinate systems has no impact. The initial config-
uration corresponds to the zero value of the degrees of freedom.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
186                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                              Joint DOF Zero Value Conventions

Joint Condition Considerations

When applying a Joint Condition, differences between the two solvers can arise. For example, consider the
right part illustrated above moving 100 mm towards the other part over a 1 second period. (The distance
along the X axis is 65 mm.)

                       Solver                                                                Displacement Joint Condition
                                                                        Time                                         Displacement
ANSYS Rigid Dynamics – Two Coordinate Systems                           0                                            65
                                                                        1                                            165
ANSYS Rigid Dynamics – One Coordinate System                            0                                            0
                                                                        1                                            100
ANSYS Mechanical – Two Coordinate Systems                               0                                            0
                                                                        1                                            100
ANSYS Mechanical – One Coordinate System                                0                                            0
                                                                        1                                            100

You can unify the joint condition input by using a Velocity Joint Condition.

                       Solver                                                                    Velocity Joint Condition
                                                                        Time                                         Displacement
ANSYS Rigid Dynamics – Two Coordinate Systems                           0                                            100
                                                                        1                                            100
ANSYS Rigid Dynamics – One Coordinate System                            0                                            100
                                                                        1                                            100
ANSYS Mechanical – Two Coordinate Systems                               0                                            100
                                                                        1                                            100
ANSYS Mechanical – One Coordinate System                                0                                            100
                                                                        1                                            100

Types of Joints
You can create the following types of joints in the Mechanical application:

 •   Fixed Joint (p. 188)
 •   Revolute Joint (p. 188)
 •   Cylindrical Joint (p. 188)
 •   Translational Joint (p. 189)
 •   Slot Joint (p. 189)
 •   Universal Joint (p. 190)
 •   Spherical Joint (p. 190)
 •   Planar Joint (p. 191)
 •   General Joint (p. 191)


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                    187
Using the Mechanical Application Features

 •    Bushing Joint (p. 191)

The following sections include animated visual joint representations. Please view online if you are reading the
PDF version of the help.

Fixed Joint
 •    Constrained degrees of freedom: All

Revolute Joint
 •    Constrained degrees of freedom: UX, UY, UZ, ROTX, ROTY




 •    Example:




Cylindrical Joint
 •    Constrained degrees of freedom: UX, UY, ROTX, ROTY




 •    Example:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
188                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                 Slot Joint




Translational Joint
•   Constrained degrees of freedom: UY, UZ, ROTX, ROTY, ROTZ




•   Example:




Slot Joint
•   Constrained degrees of freedom: UY, UZ




•   Example:


                   Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                               of ANSYS, Inc. and its subsidiaries and affiliates.                                     189
Using the Mechanical Application Features




Universal Joint
 •    Constrained degrees of freedom: UX, UY, UZ, ROTY




 •    Example:




Spherical Joint
 •    Constrained degrees of freedom: UX, UY, UZ




 •    Example:




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
190                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Bushing Joint




Planar Joint
•   Constrained degrees of freedom: UZ, ROTX, ROTY




•   Example:




General Joint
•   Constrained degrees of freedom: Fix All, Free X, Free Y, Free Z, and Free All.

Bushing Joint
•   Constrained degrees of freedom: UX, UY, ROTX, ROTY, ROTZ




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                        191
Using the Mechanical Application Features




 •    Example:




 •    Similar to a general joint, a Bushing has six degrees of freedom, three translations and three rotations,
      all of which can potentially be characterized by their rotational and translational degrees of freedom
      as being free or constrained by stiffness.

      For a Bushing, the rotational degrees of freedom are defined as follows:
      –   The first is a rotation around the reference coordinate system X Axis.
      –   The second is a rotation around the Y Axis after the first rotation is applied.
      –   The third is a rotation around the Z Axis after the first and second rotations are applied.

      The three translations and the three rotations form a set of six degrees of freedom. In addition, the
      bushing behaves, by design, as an imperfect joint, that is, some forces developed in the joint oppose
      the motion.

      The three translational degrees of freedom expressed in the reference coordinate system and the three
      rotations are expressed as: Ux, Uy, Uz, and φ, Θ, φ. The relative velocities in the reference coordinate
      system are expressed as: Vx, Vy, and Vz. The three components of the relative rotational velocity are
      expressed as: Ωx, Ωy, and Ωz. Please note that these values are not the time derivatives of [φ, Θ, φ].
      They are a linear combination.

      The forces developed in the Bushing are expressed as:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
192                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Applying a Bushing




    Where:

    [F] is force and [T] is Torque, and [K] and [C] are 6x6 matrices (defined using Stiffness Coefficients and
    Dampening Coefficients options). Off diagonal terms in the matrix are coupling terms between the
    DOFs.

    You can use these joints to introduce flexibilities to an over-constrained mechanism. Please note that
    very high stiffness terms introduce high frequencies into the system and may penalize the solution time
    when using the ANSYS Rigid Dynamics solver. If you want to suppress motion in one direction entirely
    , it is more efficient to use Joint DOF Zero Value Conventions instead of a very high stiffness.

Scoping
    You can scope a bushing to single or multiple faces, single or multiple edges, or to a single vertex. The
    scoping can either be from body-to-body or body-to-ground. For body-to-body scoping, there is a ref-
    erence and mobile side. For body-to-ground scoping, the reference side is assumed to be grounded
    (fixed); scoping is only available on the mobile side. In addition to setting the scoping (where the
    bushing attaches to the body), you can set the bushing location on both the mobile and reference side.
    The bushing reference and mobile location cannot be the same.

Applying a Bushing

    To add a bushing:
    1.   After importing the model, highlight the Connections object in the tree.
    2.   Choose either Body-Ground>Bushing or Body-Body>Bushing from the toolbar, as applicable.
    3.   Highlight the new Bushing object and enter information in the Details view.

    Note that matrix data for the Stiffness Coefficients and Dampening Coefficients is entered in the
    Worksheet. Entries are based on a Full Symmetric matrix.

Joint Properties and Application
This section discusses joint properties and manual joint creation in the Mechanical application. Joints can
also be created automatically as discussed in Automatic Joint Creation (p. 215).

A Joint is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 319) section
for a listing of all remote boundary conditions and their characteristics.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                             193
Using the Mechanical Application Features

Connection Type
You can scope a joint to single or to multiple faces. The scoping can either be from body-to-body or body-
to-ground. For body-to-body scoping, there is a reference and mobile side. For body-to-ground scoping,
the reference side is assumed to be grounded (fixed); scoping is only available on the mobile side.

Type
Refer to the Types of Joints (p. 187) section for descriptions of each type of joint you can create in the
Mechanical application. In addition to these types, you can create a General joint where you can specify
each degree of freedom as being either Fixed or Free.

Torsional Stiffness
Torsional stiffness is the measure of the resistance of a shaft to a twisting or torsional force. You can add
torsional stiffness only for cylindrical and revolute joints.

Torsional Damping
Torsional damping is the measure of resistance to the angular vibration to a shaft or body along its axis of
rotation. You can add torsional damping only for cylindrical and revolute joints.

Joint Coordinate Systems
The scoping of a joint must be accompanied by the definition of a joint coordinate system. This coordinate
system defines the location of the joint. It is imperative that the joint coordinate system be fully associative
with the geometry, otherwise, the coordinate system could move in unexpected ways when the Configure
tool is used to define the initial position of the joint (see step 5 in the “Applying Joints” section below). A
warning message is issued if you attempt to use the Configure tool with a joint whose coordinate system
is not fully associative.

The following types of coordinate systems apply specifically to joints:

 •    A reference coordinate system accompanies a joint when the joint is added to the tree. This applies
      for joints whose connection type is either body-to ground or body-to-body. When a joint is added, an
      associated coordinate system is automatically generated at a location based on your face selection.
 •    To support the relative motion between the parts of a joint, a mobile coordinate system is also auto-
      matically defined but is only displayed in the tree when the Initial Position is set to Override in the
      Details view of the Joint object.

For either reference or mobile joint coordinate systems, both the original location and the orientation of
the coordinate system can be changed as shown below.

      Caution

      If you are scoping a joint to a Remote Point, you cannot scope the Initial Position setting of a
      Joint's Mobile group as Unchanged. The Unchanged setting indicates the use of the same co-
      ordinate system for the Reference group and the Mobile group.

 To move a joint coordinate system to a particular face:
 1.    Highlight the Coordinate System field in the Details view of the Joint object. The origin of the co-
       ordinate system will include a yellow sphere indicating that the movement “mode” is active.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
194                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                         Joint Coordinate Systems




2.   Select the face that is to be the destination of the coordinate system. The coordinate system in
     movement mode relocates to the centroid of the selected face, leaving an image of the coordinate
     system at its original location.




3.   Click the Apply button. The image of the coordinate system changes from movement mode to a
     permanent presence at the new location.




To change the orientation of a joint coordinate system:
1.   Highlight the Coordinate System field in the Details view of the Joint object. The origin of the co-
     ordinate system will include a yellow sphere indicating that the movement “mode” is active.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                          195
Using the Mechanical Application Features




 2.   Click on any of the axis arrows you wish to change. Additional “handles” are displayed for each axis.




 3.   Click on the handle or axis representing the new direction to which you want to reorient the initially
      selected axis.




      The axis performs a flip transformation.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
196                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Pinball Region

 4.    Click the Apply button. The image of the coordinate system changes from movement mode to a
       permanent presence at the new orientation.




       You can change or delete the status of the flip transformation by highlighting the Reference Coordinate
       System object or a Mobile Coordinate System object and making the change or deletion under the
       Transformations category in the Details view of the child joint coordinate system.




When selecting either a Reference Coordinate System object or a Mobile Coordinate System object,
various settings are displayed in the Details view. These are the same settings that apply to all coordinate
systems, not just those associated with joints. See the following section on coordinate systems: Initial Creation
and Definition (p. 225) for an explanation of these settings.

Behavior
Use the Behavior property to specify scoped geometry as either Rigid or Deformable. Refer to the Geometry
Behavior (p. 320) section for more information. In addition, if you scope a Joint's Reference group and a
Joint's Mobile group to separate Remote Points, you can scope the Behavior of each group independently.

Pinball Region
Use the Pinball Region to define where the joint attaches to face(s) if the default location is not desirable.
By default, the entire face is tied to the joint element. This may not be desirable, warranting the input of a
Pinball Region setting, for the following reasons:

 •    If the scoping is to a topology with a large number of nodes, this can lead to an inefficient solution in
      terms of memory and speed.
 •    Overlap between the joint scoped faces and other displacement type boundary conditions can lead to
      over constraint and thus solver failures.

      Note

      The Pinball Region and Behavior settings are applicable to underlying bodies that are flexible.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                         197
Using the Mechanical Application Features

Stops
See Joint Stops and Locks (p. 216).

Applying Joints

 To add a joint manually:
 1.   After importing the model, highlight the Model object in the tree and choose the Connections button
      from the toolbar.
 2.   Highlight the new Connections object and choose either Body-Ground> {type of joint} or Body-
      Body> {type of joint} from the toolbar, as applicable. Refer to the Types of Joints (p. 187) section for
      details.
 3.   Highlight the new Joint object and scope the joint to a face.
 4.   Reposition the coordinate system origin location or orientation as needed.

      The Body Views button in the toolbar displays Reference and Mobile bodies in separate windows
      with appropriate transparencies applied. You have full body manipulation capabilities in each of these
      windows.
 5.   Configure the joint. The Configure button in the toolbar positions the Mobile body according to the
      joint definition. You can then manipulate the joint interactively (for example, rotate the joint) directly
      on the model. See the Example: Configuring Joints (p. 210) section for an application of using the Con-
      figure tool. Also see the “Notes on the Configure and Assemble Tools” below for more information.

      The Set button in the toolbar locks the changed assembly for use in the subsequent analysis.

           Note

           The triad position and orientation may not display correctly until you click on the Set button.

      The Revert button in the toolbar restores the assembly to its original configuration from DesignModeler
      or the CAD system.
 6.   Consider renaming the joint objects based on the type of joint and the names of the joined geometry.
 7.   Display the Joint DOF Checker and modify joint definitions if necessary.
 8.   Create a redundancy analysis to interactively check the influence of individual joint degrees of freedom
      on the redundant constraints.

Notes on the Configure and Assemble Tools
The Configure and Assemble tools are a good way to exercise the model and joints before starting to perform
a transient analysis. They are also a way to detect locking configurations.

The Assemble tool performs the assembly of the model, finding the closest part configuration that satisfies
all the joints.

The Configure tool performs the assembly of the model, with a prescribed value of the angle or translational
degree of freedom that you are configuring.

For the Assemble tool, all the joints degrees of freedom values are considered to be free. For the Configure
joint, the selected DOF is considered as prescribed.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
198                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                              Notes on the Configure and Assemble Tools

In both cases, the solver will apply all constraint equations, solve the nonlinear set of equations, and finally
verify that all of them are satisfied, including those having been considered as being redundant. The violation
of these constraints is compared to the model size. The model size is not the actual size of the part – as the
solver does not use the actual geometry, but rather a wireframe representation of the bodies. Each body
holds some coordinate systems – center of mass, and joint coordinate systems. For very simple models,
where the joints are defined at the center of mass, the size of the parts is zero. The violation of the constraint
equations is then compared to very small reference size, and the convergence becomes very difficult to
reach, leading the Configure tool or the Assemble tool to fail.

Example: Assembling Joints
This section illustrates the details of assembling geometry using an example of a three-part a pendulum
joint model.

The Assemble feature allows you to bring in CAD geometry that may initially be in a state of disassembly.
After importing the CAD geometry, you can actively assemble the different parts and Set them in the as-
sembled configuration for the start of the analysis.

The geometry shown for the example in Figure : Initial Geometry (p. 199) was imported into a Transient
Structural (MBD) Analysis System.

Figure: Initial Geometry




This geometry consists of three bodies. In Figure : Initial Geometry (p. 199) they are (from left to right) the
Basis, the Arm, and the PendulumAxis. These three bodies have been imported completely disjointed/separate
from each other.

The first step to orient and assemble the bodies is to add a Body-Ground Fixed joint to the body named
Basis. To do this:

 1.   Select Connections from the Outline.
 2.   From the context sensitive menu, choose Body-Ground > Fixed.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               199
Using the Mechanical Application Features




 3.   Click on a flat external face on the Basis body as seen in Figure : Selecting a Face for a Body-Ground
      Fixed Connection (p. 201).
 4.   In the Details view under Mobile, click in the Scope field and select Apply.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
200                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                             Notes on the Configure and Assemble Tools

      Figure: Selecting a Face for a Body-Ground Fixed Connection




Next, you need to join the PendulumAxis to the Basis. Since they are initially disjoint, you need to set two
coordinate systems, one for the Basis and the other for the PendulumAxis. Additionally, to fully define the
relative position and orientations of the two bodies, you must define a fixed joint between them. To do this:

 1.   From the context sensitive menu, click on Body-Body > Fixed.
 2.   Highlight the face on the Basis as shown below.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               201
Using the Mechanical Application Features




 3.   In the Details view, click on the Scope field under Reference and select Apply.
 4.   Select the cylindrical face on the PendulumAxis.
 5.   In the Details view, select the Scope field under Mobile and select Apply.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
202                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                              Notes on the Configure and Assemble Tools

      Figure: Creating a Mobile Coordinate System




 6.   Also, change the Initial Position value under Mobile from Unchanged to Override.

Now, the joint has two coordinate systems associated with it: A Reference and a Mobile coordinate system.

Next, you must associate the Reference and the Mobile Coordinate Systems to the respective bodies with
the appropriate orientations. To associate the Reference Coordinate System to the respective bodies:

 1.   In the Outline, highlight Reference Coordinate System.
 2.   In the Details view, click on the box next to Geometry under Origin.
 3.   Select the two internal rectangular faces on the Basis as shown in Figure : Creating the Reference Coordin-
      ate System (p. 204) and in the Details view, select Apply. This will center The Reference Coordinate
      System at the center of the hole on the Basis.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               203
Using the Mechanical Application Features

      Figure: Creating the Reference Coordinate System




To associate the Reference Coordinate System to the respective bodies:

 1.   Highlight the Mobile Coordinate System (this coordinate system is associated with the Basis).
 2.   In the Details view, click in the Geometry field under Origin.
 3.   Select the cylindrical surface on the PendulumArm.
 4.   In the Details view, click Apply.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
204                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                             Notes on the Configure and Assemble Tools

      Figure: Creating the Mobile Coordinate System




Next, you will need to orient the PendulumAxis coordinate system so that it is oriented correctly in the as-
sembly:

 1.   In the Mobile Coordinate System associated with the PendulumAxis, click in the box next to Geometry
      under Principal Axis (set to Z).
 2.   Select one of the vertical edges on the PendulumAxis such that the Z axis is parallel to it as shown in
      Figure : Orienting the Pendulum Axis (p. 206). In the Details view, click Apply.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               205
Using the Mechanical Application Features

      Figure: Orienting the Pendulum Axis




 3.   With Mobile Coordinate System highlighted in the Outline, select the x-offset button in the context
      sensitive menu.
 4.   In the Details view, enter an Offset X value of 2.5mm to align the faces of the PendulumAxis with the
      Basis.

           Note

           The transformations available allow you to manipulate the coordinate systems by entering
           offsets or rotations in each of the 3 axis.


The two coordinate systems that were just defined should look similar to the figure below.

Figure: Oriented Coordinate Systems




Next, you will need to define the coordinate systems to join the Arm to the PendulumAxis during assembly.

 1.   From the context sensitive menu, select Body-Body > Fixed.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
206                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                            Notes on the Configure and Assemble Tools

2.   To define the Reference Scope, choose one of the faces of the Arm that will be connected to the
     PendulumAxis then select Apply.

     Figure: Selecting an Arm Face for Connection




3.   Now, configure the Mobile Scope by selecting the flat end face of the PendulumAxis as shown in Fig-
     ure : Scoping the Mobile Coordinate Systems (p. 208), then select Apply.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                               207
Using the Mechanical Application Features

      Figure: Scoping the Mobile Coordinate Systems




 4.   Set the Initial Position under Mobile from Unchanged to Override.
 5.   Finally, set the Origin of the Reference Coordinate System to the center of the hole in the Arm using
      the same procedure described above for the Basis.

Next, you will need to offset the Coordinate System associated with the Arm so that the faces on the Arm
are aligned with the end face of the PendulumAxis.

 1.   With Reference Coordinate System highlighted, choose the x-offset button in the context sensitive
      menu.
 2.   Enter an Offset X value of -5mm.

           Note

           The transformations available allow you to manipulate the coordinate systems by entering
           offsets or rotations in each of the 3 axis.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
208                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                             Notes on the Configure and Assemble Tools

 3.   Next, Highlight the Mobile Coordinate System. This coordinate system is associated with the Arm. Click
      the box next to Geometry under Origin
 4.   Select the flat surface on the PendulumArm and click Apply.




Now you will need to orient the PendulumAxis so that its faces are aligned with the faces on the Arm during
the Assemble process.

 1.   Highlight the Mobile Coordinate System that is assigned to the PendulumAxis.
 2.   From the Details view, click the in the Geometry field under Principal Axis and select an edge of the
      PendulumAxis as shown in the figure.

      Figure: Choose an Edge to Orient the PendulumAxis Geometry




 3.   Under Principal Axis In the Details view, select Apply in the Geometry field to orient the PendulumAxis
      to this edge.

Now that the three bodies have been oriented and aligned, they are ready to be assembled.

 1.   In the Outline, highlight Connections.
 2.   From the context sensitive menu, click Assemble.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               209
Using the Mechanical Application Features

The parts should snap together in place and resemble Figure : Assembled Geometry (p. 210). If the geometry
you're attempting to assemble has not snapped into place as expected, you should retrace your previous
steps to make sure that the coordinate systems are properly oriented. If your assembly has been successfully
performed, then click Set in the context sensitive menu to place the assembly in its assembled position to
start the analysis.

Figure: Assembled Geometry




Example: Configuring Joints
This section illustrates the details of configuring joints using an example of creating a pendulum from the
two links shown below.




To achieve the result, the following two revolute joints were configured:

 •    The first joint is intended to allow rotation of the top link's upper hole referenced to a stationary point.
 •    The second joint is intended to allow rotation of the bottom link's upper hole referenced to the top
      link's lower hole.

The following steps illustrate the details of the joint configurations:

 1.    After attaching the model to the Mechanical application, create the first joint.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
210                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                             Notes on the Configure and Assemble Tools

     •   Highlight Model object folder and choose Connections from the toolbar. Then choose Body-
         Ground> Revolute from the toolbar.




2.   Scope the mobile side of the first joint to the top link's upper hole.
     •   Select inside surface of hole, then under Mobile in the Details view, click the Apply button for
         Scope.




3.   Create the second joint.
     •   Choose Body-Body> Revolute from the toolbar.
4.   Scope the reference side of the second joint to the top link's lower hole.
     •   Select inside surface of hole, then under Reference in the Details view, click the Apply button for
         Scope.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               211
Using the Mechanical Application Features




 5.   Scope the mobile side of the second joint to the bottom link's upper hole.
      •   Select inside surface of hole, then under Mobile in the Details view, click the Apply button for
          Scope.




 6.   The two holes intended to form the second joint are not aligned to correctly create the joint.




      To align the holes, first create a coordinate system for the mobile side of the second joint, then align
      the mobile and reference coordinate systems. Create the mobile coordinate system in this step.
      •   Highlight Joint 2 in the tree and choose Override in the Initial Position drop down list. Note the
          creation of the new coordinate system.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
212                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                             Notes on the Configure and Assemble Tools




7.   Scope the new mobile coordinate system to the back edge of the bottom link's upper hole.
     •   Select the back edge of the bottom link's upper hole, then under Mobile, click the Coordinate
         System field and the Apply button.




8.   Scope the existing reference coordinate system to the back edge of the top link's lower hole.
     •   Select the back edge of the top link's lower hole, then under Reference, click the Coordinate
         System field and the Apply button.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               213
Using the Mechanical Application Features

          The holes are now correctly aligned for creation of the joint.




 9.   Establish the initial position of each joint.
      •   Highlight one of the joint objects in the tree and click the Configure button in the toolbar. The
          joint is graphically displayed according to your configuration. In addition, a triad appears with
          straight lines representing translational degrees of freedom and curved lines representing rotational
          degrees of freedom. Among these, any colored lines represent the free degrees of freedom for the
          joint type. For the joint that is being configured, the translational displacement degrees of freedom
          always follow the Geometry units rather than the current Mechanical units.




          By dragging the mouse cursor on a colored line, the joint will move allowing you to set the initial
          position of the joint through the free translational or rotational degrees of freedom.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
214                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                      Creating Joints Automatically




          For rotations, holding the Ctrl key while dragging the mouse cursor will advance the rotation in
          10 degree increments. You can also click the Configure button again to cancel the joining and
          positioning of the joint.
 10. Create the joints.
      •   After configuring a joint's initial position, click the Set button to create the joint.




          At this point, you also have the option of returning the configuration to the state it was in before
          joint creation and upon attaching to the Mechanical application by clicking the Revert toolbar
          button.

Automatic Joint Creation
This section discusses the automatic joint creation in the Mechanical application. You can also create joints
manually as discussed in Joint Properties and Application (p. 193).

Creating Joints Automatically
You can direct the Mechanical application to analyze your assembly and automatically create fixed joints
and/or revolute joints.

 To create joints automatically:
 1.   Configure the types of joints (fixed and/or revolute) you want the Mechanical application to create
      automatically through the appropriate Yes or No settings in the Details view. You can set defaults for
      these settings using the Options dialog box under Connections.
 2.   After importing the model, highlight the Model object in the tree and choose the Connections button
      from the toolbar.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                         215
Using the Mechanical Application Features

 3.   Click the right mouse button on the Connections object and choose Create Automatic Joints from
      the context menu. Appropriate joint types are created and appear in the tree as objects. Each joint
      also includes a reference coordinate system that is represented as a child object to the joint object.
 4.   Consider renaming the joint objects based on the type of joint and the names of the joined geometry.
 5.   Display the Joint DOF Checker or the redundancy analysis and modify joint definitions if necessary.

      Note

      The process of automatic joint creation is additive. To avoid creation of multiple joints, you should
      first delete any existing joints that were created automatically before choosing Create Automatic
      Joints.

Joint Stops and Locks
Stops and Locks are optional constraints that may be applied to restrict the motion of the free relative de-
gree(s) of freedom (DOF) of most types of joints. Any analysis that includes a valid joint type can involve
Stops and/or Locks. For the applicable joint types, you can define a minimum and maximum (min, max)
range inside of which the degrees of freedom must remain.

A Stop is a computationally efficient abstraction of a real contact, which simplifies geometry calculations.
For Stops, a shock occurs when a joint reaches the limit of the relative motion. A Lock is the same as a Stop
except that when the Lock reaches the specified limit for a degree of freedom the Lock becomes fixed in
place.

For joints with free relative DOFs, the Details view displays a group of options labeled Stops. This grouping
displays the applicable free DOFs (UX, UY, UZ, ROTX. etc.) for the joint type from which you specify the
constraint as a Stop or a Lock. By default, no Stop or Lock is specified, as indicated by the default option,
None. You can select any combination of options. For stops and locks, the minimum and maximum values
you enter are relative to the joint’s coordinate system.




Stops and Locks are applied to the following Joint Types.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
216                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Creating Joints Automatically

                      Joint Type                                                                               Stop/Lock
                        Revolute                                                                                     Yes
                       Cylindrical                                                                                   Yes
                      Translational                                                                                  Yes
                           Slot                                                                              Translational
                       Universal                                                                                     Yes
                       Spherical                                                                                     No
                         Planar                                                                                      Yes
                        General                                                                              Translational


     Note
      •   When using the ANSYS Mechanical solver, Stops and Locks are active only when Large
          Deflection is set to On (under Analysis Settings (p. 535)). This is because Stops and Locks make
          sense only in the context of finite deformation/rotation. If Large Deflection is Off, all calcu-
          lations are carried out in the original configuration and the configuration is never updated,
          preventing the activation of the Stops and Locks.
      •   It is important to apply sensible Stop and Lock values to ensure that the initial geometry
          configuration does not violate the applied stop/lock limits. Also, applying conflicting
          boundary conditions (for example, applying Acceleration on a joint that has a Stop, or applying
          Velocity on a joint that has a Stop) on the same DOF leads to non-physical results and
          therefore is not supported.


Solver Implications

Stops and Locks are available for both the ANSYS Rigid Dynamics and ANSYS Mechanical solvers, but are
handled differently in certain circumstances by the two independent solvers.

 •   For the ANSYS Rigid Dynamics solver the shock is considered as an event with no duration, during
     which the forces and accelerations are not known or available for postprocessing, but generate a relative
     velocity "jump".
 •   For the ANSYS Mechanical solver the stop and lock constraints are implemented via the Lagrange
     Multiplier method. The constraint forces due to stop and lock conditions are available when stop is es-
     tablished

Coefficient of Restitution

For the ANSYS Rigid Dynamics solver, Stops require you to set a coefficient of restitution value. This value
represents the energy lost during the shock and is defined as the ratio between the joint’s relative velocity
prior to the shock and the velocity following the shock. This value can be between 0 and 1. For a restitution
value of zero, a Stop is released when the force in the joint is a traction force, while a Lock does not release.
A restitution factor equal to 1 indicates that no energy is lost during the shock, that is, the rebounding ve-
locity equals the impact velocity (a perfectly elastic collision).

The coefficient of restitution is not applicable to the stops on the joints when using the ANSYS Mechanical
solver.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         217
Using the Mechanical Application Features

Ease of Use Features
The following ease of use features are available when defining joints:

 •    Renaming Joint Objects Based on Definition (p. 218)
 •    Joint Legend (p. 218)
 •    Disable/Enable Transparency (p. 219)
 •    Hide All Other Bodies (p. 219)
 •    Flip Reference/Mobile (p. 219)
 •    Joint DOF Checker (p. 219)
 •    Analyze Joint Redundancies (p. 220)

Renaming Joint Objects Based on Definition
When joints are created they are represented in the tree as objects named Joint, Joint 2, Joint 3, and so
on. For ease of identification, you can have the Mechanical application automatically rename each of the
joint objects to replace the generic Joint # name with a name that includes the type of joint followed by
the names of the joined parts included as child objects under the Geometry object folder. For example, if
revolute Joint 2 connects a part named ARM to a part named ARM_HOUSING, then after renaming, the
object name becomes Revolute - ARM To ARM_HOUSING.

To rename a joint object, click the right mouse button on the object and choose Rename Based on Defin-
ition from the context menu. You can rename all joints by clicking the right mouse button on the Connections
object then choosing Rename Based on Definition. The behavior of this feature is very similar to renaming
manually created contact regions. See Renaming Contact Regions Based on Geometry Names (p. 519) for further
details including an animated demonstration.

Joint Legend
When you highlight a joint object, the accompanying display in the Geometry window includes a legend
that depicts the free degrees of freedom characteristic of the type of joint. A color scheme is used to asso-
ciate the free degrees of freedom with each of the axis of the joint's coordinate system shown in the
graphic. An example legend is shown below for a slot joint.




You can display or remove the joint legend using View> Legend from the main menu.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
218                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Joint DOF Checker

Disable/Enable Transparency
The Enable Transparency feature allows you to graphically highlight a particular joint that is within a group
of other joints, by rendering the other joints as transparent. The following example shows the same joint
group presented in the Joint Legend (p. 218) section above but with transparency enabled. Note that the slot
joint alone is highlighted.




To enable transparency for a joint object, click the right mouse button on the object and choose Enable
Transparency from the context menu. Conversely, to disable transparency, click the right mouse button on
the object and choose Disable Transparency from the context menu. The behavior of this feature is very
similar to using transparency for highlighting contact regions. See Controlling Transparency for Contact Re-
gions (p. 519) for further details including an animated demonstration.

Hide All Other Bodies
You can hide all bodies except those associated with a particular joint.

To use this feature, click the right mouse button on the object and choose Hide All Other Bodies from the
context menu. Conversely, to show all bodies that may have been hidden, click the right mouse button on
the object and choose Show All Bodies from the context menu.

Flip Reference/Mobile
For body-to-body joint scoping, you can reverse the scoping between the Reference and Mobile sides in
one action. To use this feature, click the right mouse button on the object and choose Flip Reference/Mobile
from the context menu. The change is reflected in the Details view of the joint object as well as in the color
coding of the scoped entity on the joint graphic. The behavior of this feature is very similar to the Flip
Contact/Target feature used for contact regions. See Flipping Contact and Target Scope Settings (p. 520) for
further details including an animated demonstration.

Joint DOF Checker
Once joints are created, fully defined, and applied to the model, a Joint DOF Checker calculates the total
number of free degrees of freedom. The number of free degrees of freedom should be greater than zero in
order to produce an expected result. If this number is less than 1, a warning message is displayed stating
that the model may possibly be overconstrained, along with a suggestion to check the model closely and
remove any redundant joint constraints.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                            219
Using the Mechanical Application Features

To display the Joint DOF Checker information, highlight the Connections object and click the Worksheet
tab. The Joint DOF Checker information is located just above the Joint Information heading in the worksheet.

Analyze Joint Redundancies
Using this feature allows you to analyze an assembly which is held together by joints. Also, this analysis will
assist in helping you solve over constrained assemblies. Each body in an assembly has a limited degree of
freedom set. The joint constraints must be consistent to the motion of each body, otherwise the assembly
can be locked or the bodies may move in directions other than you want. The redundancy analysis checks
the joints you define and indicates the joints that over constrain the assembly. To analyze an assembly for
joint redundancies:

 1.    Right-click the Connections object, and then click Redundancy Analysis to open a worksheet with a
       list of joints.
 2.    Click Analyze to perform a redundancy analysis. All the over constrained joints are indicated as redund-
       ant.
 3.    Click the Redundant label, and then select Fixed or Free to resolve the conflict manually.

       or

       Click Convert Redundancies to Free to remove all over constrained degrees of freedom.
 4.    Click Set to update the Joint definitions.

            Note

            Click Export to save the worksheet to an Excel/text file.


Detecting Overconstrained Conditions
Overconstrained conditions can occur when more constraints than are necessary are applied to a joint's
degrees of freedom. These conditions may arise when rigid bodies are joined together using multiple joints.
The overconstraints could be due to redundant joints performing the same function, or contradictory motion
resulting from improper use of joints connecting different bodies.

 •    For the transient structural (ANSYS) analysis type, when a model is overconstrained, nonconvergence
      of the solution most often occurs, and in some cases, overconstrained models can yield incorrect results.
 •    For the transient structural (MBD) analysis type, when a model is overconstrained, force calculation
      cannot be done properly.

The following features exist within the Mechanical application that can assist you in detecting possible
overconstrained conditions:

 •    Use the Joint DOF Checker (p. 219) for detecting overconstrained conditions before solving (highlight
      Connections object and view the Worksheet tab). In the following example, the original display of the
      Joint DOF Checker warns that the model may be overconstrained.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
220                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Preloading




     After modifying the joint definitions, the user displays the Joint DOF Checker again, which shows that
     the overconstrained condition has been resolved.




 •   After solution, you can highlight the Solution Information object, then scroll to the end of its content
     to view any information that may have been detected on model redundancies that caused overcon-
     strained conditions. An example is presented below.




Springs
A spring is an elastic element that is used to store mechanical energy and which retains its original shape
after a force is removed. Springs are typically defined in a stress free or “unloaded” state. This means that
no longitudinal loading conditions exist unless preloading is specified (see below). In Workbench, the Con-
figure feature is used to modify a Joint. If you configure a joint that has an attached spring, the spring must
be redrawn in the Geometry window. In effect, the spring before the Configure action is replaced by a new
spring in a new unloaded state.

Springs are defined as longitudinal and they connect two bodies together or connect a body to ground.
Longitudinal springs generate a force that depends on linear displacement. Longitudinal springs can be
used as a damping force, which is a function of velocity or angular velocity, respectively. Springs can also
be defined directly on a Revolute Joint (p. 188) or a Cylindrical Joint (p. 188).

Preloading
Workbench also provides you with the option to preload a spring and create an initial “loaded” state. Use
the Preload field in the Details `View to define one of the following spring types:


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     221
Using the Mechanical Application Features

 •    Longitudinal spring – the detail options allow you to define a preload as a length using Free Length
      or to specify a specific Load. Positive values create tension and negative values create compression.

Scoping
You can scope a spring to single or multiple faces, single or multiple edges, or to a single vertex. The scoping
can either be from body-to-body or body-to-ground. For body-to-body scoping, there is a reference and
mobile side. For body-to-ground scoping, the reference side is assumed to be grounded (fixed); scoping is
only available on the mobile side. In addition to setting the scoping (where the spring attaches to the body),
you can set the spring location on both the mobile and reference side. Since this is a unidirectional spring,
these 2 locations determines the spring’s line of action. As such the spring reference and mobile location
cannot be the same as this would result in a spring with zero length.

Advanced Features
Springs include Pinball Region and Behavior as advanced properties.

Use the Pinball Region to define where the spring attaches to face(s), edge(s), or a single vertex if the default
location is not desirable. By default, the entire face/edge/vertex is tied to the spring element. This may not
be desirable, warranting the input of a Pinball Region setting, for the following reasons:

 •    If the scoping is to a topology with a large number of nodes, this can lead to an inefficient solution in
      terms of memory and speed.
 •    Overlap between the spring scoped faces and other displacement type boundary conditions can lead
      to over constraint and thus solver failures.

Use the Behavior property to specify scoped geometry as either Rigid or Deformable. Refer to the Geometry
Behavior (p. 320) section for more information.

      Note

      The Pinball Region and Behavior settings are applicable to underlying bodies that are flexible.

A Spring is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 319) section
for a listing of all remote boundary conditions and their characteristics.

Output
Several outputs are available via a spring probe.

Applying Springs
 To add a spring:
 1.    After importing the model, highlight the Model object in the tree and choose the Connections button
       from the toolbar.
 2.    Highlight the new Connections object and choose either Body-Ground> Spring or Body-Body>
       Spring from the toolbar, as applicable.
 3.    Highlight the new Spring object and enter information in the Details view. Note that Longitudinal
       Damping is applicable only to transient analyses.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
222                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                            Example: Longitudinal Spring with Damping


     Note

     The length of the spring connection must be greater than 0.0 with a tolerance of 1e-8 mm.

Example: Longitudinal Spring with Damping
This example shows the effect of a longitudinal spring connecting a rectangular bar to ground to represent
a damper. A transient structural (ANSYS) analysis was performed in the environment shown:




The following are the Details view settings of the Spring object:




Presented below is the Total Deformation result:


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               223
Using the Mechanical Application Features

The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the
help. Interface names and other components shown in the demo may differ from those in the released product.




Beam
A beam is a structural element that carries load primarily in bending (flexure). Using beams, you can establish
a body to body or a body to ground connection. You can use beams for structural analyses. To add a beam:

 1.   In the Project tree, select Model to make the Model toolbar available.
 2.   On the Model toolbar, click Connections .
 3.   On the Connections toolbar, click Body-Ground or Body-Body, and then click Beam to add a circular
      beam under connections.
 4.   In the Details View, under Definition, click the Material fly-out menu, and then select a material for
      the beam.
 5.   Type the beam radius.
 6.   Under Reference, type the X, Y, and Z coordinate to define the reference point, or select a face, edge,
      or vertex, and then click Apply. This step is not required if you chose Body-Ground above.
 7.   Under Mobile, type the X, Y, and Z coordinate to define the reference point, or select a face, edge, or
      vertex, and then click Apply.

      Note
      •   For Body-Ground beam connections, the reference side is fixed. For Body-Body beam con-
          nections, you must define the reference point for each body.
      •   The length of the beam connection must be greater than 0.0 with a tolerance of 1e-8 mm.


The Beam Probe results provide you the forces and moments in the beam from your analysis.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
224                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Creating Coordinate Systems

Virtual Topology
You can use virtual topology to aid you in reducing the number of elements in the model, simplifying small
features out of the model, and simplifying load abstraction. See Virtual Topology Overview for details.

Coordinate Systems Overview
All geometry in the Mechanical application is displayed in the global coordinate system by default. The
global coordinate system is the fixed Cartesian (X, Y, Z) coordinate system originally defined for a part.

In addition, you can create unique local coordinate systems to use with springs, joints, various loads, supports,
and result probes.

Cartesian coordinates apply to all local coordinate systems. In addition, you can apply cylindrical coordinates
to parts, displacements, and forces applied to surface bodies.

      Note

      Cylindrical coordinate systems are not supported by the Explicit Dynamics solvers, but may be
      used for some postprocessing operations.

The following topics are covered in this section:
 Creating Coordinate Systems
 Importing Coordinate Systems
 Applying Coordinate Systems as Reference Locations
 Using Coordinate Systems to Specify Joint Locations
 Transferring Coordinate Systems to the Mechanical APDL Application

Creating Coordinate Systems
The following topics involve the creation of local coordinate systems:
 Initial Creation and Definition
 Establishing Origin for Associative and Non-Associative Coordinate Systems
 Setting Principal Axis and Orientation
 Using Transformations

Initial Creation and Definition
Creating a new local coordinate system involves adding a Coordinate System object to the tree and ad-
dressing items under the Definition category in the Details view.

 To create and define a new local coordinate system:
 1.   Highlight the Coordinate Systems folder in the tree and choose the Coordinate Systems button
      from the toolbar or from a right mouse click (Insert> Coordinate System). A Coordinate System
      object is inserted into the tree.



      The remainder of the toolbar buttons involve the use of transformations discussed in a later section.
 2.   In the Details view Definition group, set the following:


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       225
Using the Mechanical Application Features

       •   Type: to Cartesian or Cylindrical.
       •   Ansys System: to Program Controlled or Manual. This assigns the coordinate system reference
           number (the first argument of the ANSYS LOCAL command). Choose Program Controlled to have
           the reference number assigned automatically, or choose Manual to assign a particular reference
           number in the Ansys System Number field for identification or quick reference of the coordinate
           system within the input file. You should set the Ansys System Number to a value greater than or
           equal to 12. If you create more than one local coordinate system, you must ensure that you do not
           duplicate the Ansys System Number.


Establishing Origin for Associative and Non-Associative Coordinate Systems
After creating a local coordinate system, you can further designate it as being associative or non-associative
with geometry and define its origin.

 •    An associative coordinate system is joined to the face or edge on which it is applied, such that the co-
      ordinate system moves with the face or edge. Its translation and rotation are dependent on the geometry.
 •    A non-associative coordinate system is independent of any geometry. It remains as originally defined
      regardless of translation or rotation of any geometry.

You establish the origin for either an associative or non-associative coordinate system in the Origin category
in the Details view.

 To establish the origin for an associative coordinate system:
 1.    In the Details view Origin group of a Reference Coordinate System, set Define By to Geometry
       Selection. For a Reference Coordinate System attached to a joint, work with the Orientation About
       Principal Axis group to make the coordinate system associative.
 2.    Select a vertex or vertices, edge, face, cylinder, circle, or circular arc.
 3.    Choose Click to Change in the Geometry row.
 4.    Click Apply. A coordinate system symbol displays at the origin location as determined by the following:

       •   Select a vertex. The origin will be on the vertex.
       •   Select multiple vertices. The origin will be at the center of the area or volume enclosed by the se-
           lected vertices.
       •   Select a face or an edge. The origin will be at the centroid of the face or edge.
       •   Select a cylinder. The origin will be at the center of the cylinder.
       •   Select a circle or a circular arc. The origin will be at the center of the circle or circular arc.

       Preselecting one or more topologies and then inserting a Coordinate System will automatically locate
       its origin as stated above.

 To establish the origin for a non-associative coordinate system:
 •     In the Details view Origin group, set Define By to Global Coordinates. You then define the origin in
       either of the following ways:

       •   Selecting any point on the exterior of the model:
           1.   Set Define By to Global Coordinates.
           2.   Choose Click to Change in the Location row.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
226                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                       Creating Coordinate Systems

           3.   Depress the Coordinate toolbar button.
           4.   Move the cursor across the model and notice that the coordinates display and update as you
                reposition the cursor.
           5.   Click at the desired origin location. A small cross hair appears at this location. You can click
                again to change the cross hair location.
           6.   Click Apply. A coordinate system symbol displays at the origin location. Also, the coordinates
                display in the Details view. You can change the location by repositioning the cursor, clicking
                at the new location, and then clicking Click to Change and Apply, or by editing the coordinates
                in the Details view.
       •   Entering the coordinates directly in the Details view.
           1.   Set Define By to Global Coordinates.
           2.   Type the Origin X, Y, Z coordinates. The origin will be at this location.


Setting Principal Axis and Orientation
The definition of the coordinate system involves two vectors, the Principal Axis vector and the Orientation
About Principal Axis vector. The coordinate system respects the plane formed by these two vectors and
aligns with the Principal Axis. Use the Principal Axis category in the Details view to define one of either the
X, Y, or Z axes in terms of a:

 •    Geometry Selection - Associatively align axis to a topological feature in the model. When a change
      occurs to the feature, the axis automatically updates to reflect the change.
 •    Fixed Vector – Depending upon the Geometry Selection, this option preserves the current Geometry
      Selection without associativity. When a change occurs to the feature the axis will not update automat-
      ically to reflect that change.
 •    Global X, Y, Z axis – Force the axis to align to a global X, Y, or Z axis.

Use the Orientation About Principal Axis category in the Details view to define one of the orientation X,
Y, or Z axes in terms of the Default, Geometry Selection, the Global X, Y, Z axes, or Fixed Vector.

Using Transformations
Transformations allow you to “fine tune” the original positioning of the coordinate system. Options are
available for offsetting the origin by a translation in each of the x, y and z directions, as well as by rotation
about each of the three axes. Flipping of each axis is also available. To exercise transformations, you use
buttons on the Coordinate Systems toolbar and settings in the Transformations category in the Details
view .

 To transform a coordinate system:
 1.    Choose a transformation (translation, rotation, or flip) from the Coordinate Systems toolbar.




       Entries appear in the Details view as you add transformations.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                       227
Using the Mechanical Application Features

 2.   Enter information in the Details view for each transformation.
 3.   If required:

      •   Reorder a transformation by highlighting it in the Details view and using the Move Transform Up
          or Move Transform Down toolbar button.
      •   Delete a transformation by highlighting it in the Details view and using the Delete Transform
          toolbar button.


Importing Coordinate Systems
Coordinate systems defined when geometry is imported from DesignModeler, Pro/ENGINEER, or SolidWorks
will automatically be created in the Mechanical application. For more information, see the Attaching Geo-
metry section under DesignModeler, or see the Notes section under Pro/ENGINEER or SolidWorks.

If you update the model in the Mechanical application, coordinate systems from these products are refreshed,
or newly defined coordinate systems in these products are added to the model.

If a coordinate system was brought in from one of these products but changed in the Mechanical application,
the change will not be reflected on an update. Upon an update, a coordinate system that originated from
DesignModeler, Pro/ENGINEER, or SolidWorks will be re-inserted into the object tree. The coordinate system
that was modified in the Mechanical application will also be in the tree.

Applying Coordinate Systems as Reference Locations
Any local coordinate systems that were created in the Mechanical application, or imported from Design-
Modeler, Pro/ENGINEER, or SolidWorks, can be applied to a part, or to a Point Mass, Spring, Acceleration,
Standard Earth Gravity, Rotational Velocity, Force, Bearing Load, Remote Force, Moment, Displacement, Remote
Displacement, or Contact Reaction. This feature is useful because it avoids having to perform a calculation
for transforming to the global coordinate system.

 To apply a local coordinate system:
 1.   Select the tree object that represents one of the applicable items mentioned above.
 2.   For an Acceleration, Rotational Velocity, Force, Bearing Load, or Moment, in the Details view, set Define
      By, to Components, then proceed to step 3. For the other items, proceed directly to step 3.
 3.   In the Details view, set Coordinate System to the name of the local coordinate system that you want
      to apply. The names in this drop-down list are the same names as those listed in the Coordinate
      Systems branch of the tree outline.

           Note

           If you define a load by Components in a local coordinate system, changing the Define By
           field to Vector will define the load in the global coordinate system. Do not change the
           Define By field to Vector if you want the load defined in a local coordinate system.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
228                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                      Basics

Using Coordinate Systems to Specify Joint Locations
Whenever you create a joint, an accompanying reference coordinate system is also created. The intent of
this coordinate system is for positioning the joint. See the Joint Properties and Application (p. 193) section for
further details.

Transferring Coordinate Systems to the Mechanical APDL Application
You can transfer coordinate systems to the Mechanical APDL application using any of the following methods:

 •    Main Menu> Tools > Write Input File...
 •    Load the Mechanical APDL application.
 •    Commands Objects

Any coordinate system defined in the Mechanical application and sent to the Mechanical APDL application
as part of the finite element model, will be added to the Mechanical APDL application input file as LOCAL
commands. For example:
 /com,*********** Send User Defined Coordinate System(s) ***********
 local,11,0,0.,0.,0.,0.,0.,0.
 local,12,1,11.8491750582796,3.03826387968126,-1.5,0.,0.,0.
 csys,0


Graphics
The following topics are covered in this section:
 Annotations
 Lighting Controls
 New Section Plane
 Comments, Images, Figures

Annotations
     Basics (p. 229)
     Highlight and Selection Graphics (p. 230)
     Scope Graphics (p. 230)
     Annotation Graphics and Positioning (p. 230)
     Environment Annotations (p. 231)
     Rescaling Annotations (p. 231)
     Solution Annotations (p. 232)
     Message Annotations (p. 233)

Basics
Annotations provide the following visual information:

 •    Boundary of the scope region by coloring the geometry for edges, faces or vertices.
 •    An explicit vertex within the scope.
 •    A 3D arrow to indicate direction, if applicable.
 •    Text description or a value.
 •    A color cue (structural vs. thermal, etc.).


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                 229
Using the Mechanical Application Features


      Note

      The custom annotations you add using Label remain visible even when you suppress the body.

Highlight and Selection Graphics
You can interactively highlight a face. The geometry highlights when you point to it.




See Graphical Selection (p. 121) for details on highlighting and selection.

Scope Graphics
In general, selecting an object in the Tree Outline (p. 118) displays its Scope by painting the geometry and
displays text annotations and symbols as appropriate. The display of scope via annotation is carried over
into the Report Preview (p. 494) if you generate a figure.

Contours are painted for results on the scoped geometry. No boundary is drawn.




Annotation Graphics and Positioning
A label consists of a block arrow cross-referenced to a color-coded legend. For vector annotations, a 3D arrow
originates from the tip of the label to visualize direction relative to the geometry.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
230                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Rescaling Annotations

Figure: Annotation of a force on a face




Use the pointer after selecting the Label toolbar button                                  for managing annotations and to drag the
annotation to a different location within the scope.

 •   If other geometry hides the 3D point (e.g. the point lies on a back face) the block arrow is unfilled
     (transparent).
 •   The initial placement of an annotation is at the pick point. You can then move it by using the Label
     toolbar button for managing annotations.
 •   Drag the label to adjust the placement of an annotation. During the drag operation the annotation
     moves only if the tip lies within the scope. If the pointer moves outside the scope, the annotation stops
     at the boundary.

Environment Annotations
With an environment object selected in the Tree Outline (p. 118), an annotation for each load and support
appears on the geometry (limit 10, based on selection in tree):




The scope of loads and supports is usually displayed.

Rescaling Annotations
This feature modifies the size of annotation symbols, such as load direction arrows, displayed in the Mech-
anical application. For example, and as illustrated below, you can reduce the size of the pressure direction


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            231
Using the Mechanical Application Features

arrow when zooming in on a geometry selection. To change the size of an annotation, click the Rescale
Annotation toolbar button (             ).




Solution Annotations
Solution annotations work similar to Environment Annotations (p. 231). The Max annotation has red background.
The Min annotation has blue background. Probe annotations have cyan backgrounds.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
232                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Message Annotations

Figure: Max and Min annotations and two "probe" annotations:




 •   By default, annotations for Max and Min appear automatically for results but may be controlled by
     buttons in the Result Context Toolbar (p. 155).
 •   You may create "probe" annotations by clicking           in the Result Context Toolbar (p. 155). Probe
     annotations show the value of the result at the location beneath the tip, when initially constructed.
     When probe annotations are created, they do not trigger the database to be marked as save being
     needed (i.e. you will not be prompted to save). Be sure to issue a save if you wish to retain these newly
     created probe annotations in the database. Changes to the unit system deletes active probe annotations.
     In addition, probe annotations are not displayed if a Mechanical application database is opened in a
     unit system other than the one in which it was saved; however, the probe annotations are still available
     and display when the Mechanical application database is opened in the original unit system.
 •   If you apply a probe annotation to a very small thickness, such as when you scope results to an edge,
     the probe display may seem erratic or non-operational. This is because, for ease of viewing, the colored
     edge result display is artificially rendered to appear larger than the actual thickness. You can still add
     a probe annotation in this situation by zooming in on the thin region before applying the probe annota-
     tion.
 •
     To delete a probe annotation, activate the Label button                                    , select the probe, and then press the
     Delete key.
 •   Probes will be cleared if the results are re-solved.
 •   After adding one or more probe annotations, if you increase the number of viewports, the probe an-
     notations only appear in one of the viewports. If you then decrease the number of viewports, you must
     first highlight the header in the viewport containing the probe annotations in order to preserve the
     annotations in the resulting viewports.
 •   See the Solution Context Toolbar (p. 154) for more information.

Message Annotations
If an error occurs during meshing, the application attempts to annotate the problem geometry.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              233
Using the Mechanical Application Features




Lighting Controls
When you click Model in the Tree Outline (p. 118), you can view details that control lighting in the Geo-
metry (p. 120) window.

New Section Plane

Selecting the New Section Plane icon button in the graphics toolbar displays the Section Planes panel
where the Details View is normally located in the lower left panel of the Mechanical application window,
and initiates the New Section Plane function.




Icon Button    Application-level command
               New Section Plane

               Delete Section Plane

               Show Whole Elements

Example 2 Section Plane Usage




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
234                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   New Section Plane

•   You can add a Section Plane by selecting the New Section Plane button and then dragging the mouse
                                                                                ,                 ,
    across the part. Each plane is created with a default name, “Section Plane 1” “Section Plane 2” etc. The
    newly created section plane will become active as indicated by the checkmark next to the plane’s name.
    To view the newly created plane, rotate the model.




•   You can construct additional Section Planes by clicking the New Section Plane button and dragging
    additional lines across the model.
•   Activating multiple planes displays multiple sections




•   You can highlight a section plane’s name in the pane to display the plane’s anchor.
•   Click on the line on either side of the anchor to view the exterior on that side of the plane. The anchor
    displays a solid line on the side where the exterior is being displayed. Clicking on the same side a second
    time toggles between solid line and dotted line, i.e. exterior display back to section display. Note that
    for Geometry, display a capped view is always shown.
•   Drag the Section Plane or Capping Plane anchor to change the position of the plane.
•   You can maneuver between multiple planes by simply highlighting the plane names
•   To delete the selected Section Plane or Capping Plane, use the Delete Section Plane button.
•   When you are on a Mesh display you can use the Show Whole Elements button to display the adjacent
    elements to the slice plane which may be desirable in some cases.
•   Unchecking all the planes effectively turns the Section Plane feature off.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                            235
Using the Mechanical Application Features




Note that in incidences such as very large models where the accessible memory is exhausted, the New
Section Plane tool will revert to a Hardware Slice Mode that prohibits visualization of the mesh on the cut-
plane.

The Section Plane acts differently depending if you are viewing a result, mesh, or geometry display. When
viewing a result or a mesh, the cut is performed by a software algorithm. When viewing geometry, the cut
is performed using a hardware clipping method. This hardware clipping cuts away the model in a subtractive
method. The software algorithm cuts away the model but always starts with the whole model.

Note that the software algorithm caps the surfaces created by the section plane as opposed to the hardware
clipping method. When capping, the software algorithm creates a visible surface at the intersection of the
object and the section plane."

As an example, consider the model shown below that is subjected to a horizontal and a vertical slice.




The mesh display will show 75 % of the model while the geometry display will show 25 % of the model.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
236                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                          Comments, Images, Figures




Comments, Images, Figures
You can insert Comment objects, Image objects, or Figure objects under various parent objects in the
Mechanical tree to add text or graphical information that pertain specifically to those parent objects. Refer
to their individual objects reference pages for descriptions. Additional information on Figure objects is
presented below.

Figures allow you to:

 •   Preserve different ways of viewing an object (viewpoints and settings).
 •   Define illustrations and captions for a report.
 •   Capture result contours, mesh previews, environment annotations etc., for later display in Report.

Clicking the Figure button in the Standard Toolbar (p. 147) creates a new Figure object inside the selected
object in the Tree Outline (p. 118). Any object that displays 3D graphics may contain figures. The new figure
object copies all current view settings and gets focus in the Outline automatically.

View settings maintained by a figure include:

 •   Camera settings
 •   Result toolbar settings
 •   Legend configuration

A figure's view settings are fully independent from the global view settings. Global view settings are main-
tained independently of figures.

Behaviors:

 •   If you select a figure after selecting its parent in the Outline, the graphics window transforms to the
     figure's stored view settings automatically (e.g. the graphics may automatically pan/zoom/rotate).
 •   If you change the view while a figure is selected in the Outline, the figure's view settings are updated.
 •   If you reselect the figure's parent in the Outline, the graphics window resumes the global view settings.
     That is, figure view settings override but do not change global view settings.
 •   Figures always display the data of their parent object. For example, following a geometry Update and
     Solve, a result and its figures display different information but reuse the existing view and graphics


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                        237
Using the Mechanical Application Features

      options. Figures may be moved or copied among objects in the Outline to display different information
      from the same view with the same settings.
 •    You may delete a figure without affecting its parent object. Deleting a parent object deletes all figures
      (and other children).
 •    In the Tree Outline (p. 118), the name of a figure defaults to simply Figure appended by a number as
      needed.
 •    You may enter a caption for a figure as a string in the figure's details. It is your responsibility to maintain
      custom captions when copying figures.

Analysis Settings
The following topics are covered in this section.

 •    Analysis Settings for Most Analysis Types (p. 238)
 •    Analysis Settings for Explicit Dynamics Analyses (p. 247)
 •    Steps and Step Controls for Static and Transient Analyses (p. 262)
      –   Role of Time in Tracking (p. 262)
      –   Steps, Substeps, and Equilibrium Iterations (p. 263)
      –   Automatic Time Stepping (p. 264)
      –   Guidelines for Integration Step Size (p. 264)
      –   Step Controls (p. 266)
 •    Nonlinear Controls (p. 269)
 •    Output Controls (p. 270)
 •    Solver Controls (p. 271)
 •    Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses (p. 273)
 •    Damping Controls (p. 276)
 •    Visibility (p. 277)
 •    Analysis Data Management (p. 277)

Analysis Settings for Most Analysis Types
When you define an analysis type, an Analysis Settings object is automatically inserted in the Mechanical
application tree. With this object selected, you can define various solution options in the Details view that
are customized to the specific analysis type, such as enabling large deflection for a stress analysis.

The available control groups as well as the control settings within each group vary depending on the ana-
lysis type you have chosen. The following table and the Explicit Dynamics table presents the controls available
for each analysis type. Follow the links in the table for more detailed information on specific controls.




                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
238                                                     of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                        Analysis Settings for Most Analysis Types

 Analysis
 Settings
  Details
   View                                                                       Analysis Type
                                                                                       Ran-
                           Tran-                                                       dom
                           si-         Tran-                                           Vi-
                           ent         si-                                             bra-
                  Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                  Sae
        Con-      ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                              Se d         Tran-         Mag-
Con-    trol      Struc-   al          tur-        ic                      ear         sos
                                                                                        p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                         Teml
trol    Set-      tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p    ting      al       SYS)        ( B)
                                       MD           p ne
                                                   sos         al          ling        trum       tion         hr a
                                                                                                              T eml        T eml
                                                                                                                            hr a         ic      tric    tric
Solv-   Solv-
er      er
Con-    Type
trols   W eak
         pi g
        S rn s
        Large
        De-
        flec-
        tion
        Iner-
        tia
        Re-
        lief
        Time
        In-
        teg-
        ra-
        tion
        and
        Con-
        straint
        Sta-
        bil-
        iza-
        tion
Step    Num-
Con-    ber
trols   of
        Steps
        Time
                    2         2                                                                                  2           2
        Step
        Num-
        ber
        of          2         2                                                                                  2           2
        Sub-
        steps


                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                                  239
Using the Mechanical Application Features

 Analysis
 Settings
  Details
   View                                                                     Analysis Type
                                                                                     Ran-
                         Tran-                                                       dom
                         si-         Tran-                                           Vi-
                         ent         si-                                             bra-
                Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                Sae
       Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                            Se d         Tran-         Mag-
Con-   trol     Struc-   al          tur-        ic                      ear         sos
                                                                                      p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                       Teml
trol   Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p   ting     al       SYS)        ( B)
                                     MD           p ne
                                                 sos         al          ling        trum       tion         hr a
                                                                                                            T eml        T eml
                                                                                                                          hr a         ic      tric    tric
       Cur-
       rent
       Step       2         2           2                                                                      2           2
       Num-
       ber
       Step
       End        2         2                                                                                  2           2
       Time
       Auto
       Time
                  2         2                                                                                  2           2
       Step-
       ping
       Define
                  2         2                                                                                  2           2
       By
       Ini-
       tial
       Time
                  2         2                                                                                  2           2
       /
       Sub-
       steps
       Min-
       im-
       um
       Time       2         2                                                                                  2           2
       /
       Sub-
       steps
       Max-
       im-
       um
       Time       2         2                                                                                  2           2
       /
       Sub-
       steps
       Time
                            2                                                                                              2
       In-


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
240                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Analysis Settings for Most Analysis Types

 Analysis
 Settings
  Details
   View                                                                      Analysis Type
                                                                                      Ran-
                          Tran-                                                       dom
                          si-         Tran-                                           Vi-
                          ent         si-                                             bra-
                 Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                 Sae
        Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                             Se d         Tran-         Mag-
Con-    trol     Struc-   al          tur-        ic                      ear         sos
                                                                                       p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                        Teml
trol    Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p    ting     al       SYS)        ( B)
                                      MD           p ne
                                                  sos         al          ling        trum       tion         hr a
                                                                                                             T eml        T eml
                                                                                                                           hr a         ic      tric    tric
        teg-
        ra-
        tion
Non-    Force
lin-    Con-
                   2         2
ear     ver-
Con-    gence
trols   Mo-
        ment
        Con-       2         2
        ver-
        gence
        Dis-
        place-
        ment
                   2         2
        Con-
        ver-
        gence
        Ro-
        ta-
        tion
                   2         2
        Con-
        ver-
        gence
        Heat
        Con-
                                                                                                                2           2
        ver-
        gence
        Tem-
        per-
        at-
        ure                                                                                                     2           2
        Con-
        ver-
        gence



                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                                  241
Using the Mechanical Application Features

 Analysis
 Settings
  Details
   View                                                                     Analysis Type
                                                                                     Ran-
                         Tran-                                                       dom
                         si-         Tran-                                           Vi-
                         ent         si-                                             bra-
                Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                Sae
       Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                            Se d         Tran-         Mag-
Con-   trol     Struc-   al          tur-        ic                      ear         sos
                                                                                      p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                       Teml
trol   Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p   ting     al       SYS)        ( B)
                                     MD           p ne
                                                 sos         al          ling        trum       tion         hr a
                                                                                                            T eml        T eml
                                                                                                                          hr a         ic      tric    tric
       CSG
       Con-
       ver-
       gence
        MS
       A P
       Con-
       ver-
       gence
       Line
                  2         2                                                                                  2           2
        e rh
       S ac
       Non-
       lin-
       ear
       For-
       mu-
       la-
       tion
       Rel-
       at-
       ive
       As-
        eb
       sm ly
       Tol-
       er-
       ance
       En-
       ergy
       Ac-
       cur-
       acy
       Tol-
       er-
       ance
        og
         t
       V la e
       Con-



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
242                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Analysis Settings for Most Analysis Types

 Analysis
 Settings
  Details
   View                                                                      Analysis Type
                                                                                      Ran-
                          Tran-                                                       dom
                          si-         Tran-                                           Vi-
                          ent         si-                                             bra-
                 Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                 Sae
        Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                             Se d         Tran-         Mag-
Con-    trol     Struc-   al          tur-        ic                      ear         sos
                                                                                       p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                        Teml
trol    Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p    ting     al       SYS)        ( B)
                                      MD           p ne
                                                  sos         al          ling        trum       tion         hr a
                                                                                                             T eml        T eml
                                                                                                                           hr a         ic      tric    tric
        ver-
        gence
        Cur-
        rent
        Con-
        ver-
        gence
Out-    Cal-
put     cu-
Con-    late
trols   Stress
        Cal-
        cu-
        late
        Strain
        Cal-
        cu-
        late
         hr a
        Teml
        Flux
        Cal-
                                                                                        6
        cu-
        late
        Ve-
        lo-
        city
        Cal-
                                                                                        6
        cu-
        late
        Ac-
        cel-
        era-
        tion
        Cal-
        cu-        2         2                                                                                  2           2
        late


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                                  243
Using the Mechanical Application Features

 Analysis
 Settings
  Details
   View                                                                      Analysis Type
                                                                                      Ran-
                          Tran-                                                       dom
                          si-         Tran-                                           Vi-
                          ent         si-                                             bra-
                 Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                 Sae
        Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                             Se d         Tran-         Mag-
Con-    trol     Struc-   al          tur-        ic                      ear         sos
                                                                                       p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                        Teml
trol    Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p    ting     al       SYS)        ( B)
                                      MD           p ne
                                                  sos         al          ling        trum       tion         hr a
                                                                                                             T eml        T eml
                                                                                                                           hr a         ic      tric    tric
        Res-
        ults
        At
        Num-
        ber
        of         2         2                                                                                  2           2
        Time
        Points
Op-     Vari-
                                                     1           1          1           1
tions   ous
 ap
Dm -    Con-
ing     stant
Con-     ap
        Dm -
trols   ing
        Ra-
        tio
        Beta
         ap
        Dm -
        ing
         ei d
          n
        Df e
        By
        Beta
         ap
        Dm -
        ing
        Fre-
         uny
        qec
        Beta
         ap
        Dm -
        ing
        Meas-
        ure
        Beta
         ap
        Dm -
        ing
        Value



                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
244                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Analysis Settings for Most Analysis Types

 Analysis
 Settings
  Details
   View                                                                      Analysis Type
                                                                                      Ran-
                          Tran-                                                       dom
                          si-         Tran-                                           Vi-
                          ent         si-                                             bra-
                 Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                 Sae
        Con-     ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                             Se d         Tran-         Mag-
Con-    trol     Struc-   al          tur-        ic                      ear         sos
                                                                                       p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                        Teml
trol    Set-     tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p    ting     al       SYS)        ( B)
                                      MD           p ne
                                                  sos         al          ling        trum       tion         hr a
                                                                                                             T eml        T eml
                                                                                                                           hr a         ic      tric    tric
        Nu-
        mer-
        ical
         ap
        Dm -
        ing
Vis-    (Load)
ibil-   Res-
ity     ults
        Track-
        er
Ana-    Solv-
lys-    er
is      File
Data    Dir-
Man-    ect-
age-    ory
ment    Fu-
        ture
        Ana-
        lys-
        is
         cac
        S r th
        Solv-
        er
        Files
        Dir-
        ect-
        ory
        Save
        AN-
        SYS
        DB
        De-
        lete
        Un-



                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                                  245
Using the Mechanical Application Features

 Analysis
 Settings
  Details
   View                                                                       Analysis Type
                                                                                       Ran-
                           Tran-                                                       dom
                           si-         Tran-                                           Vi-
                           ent         si-                                             bra-
                  Stat-    Struc-      ent         Har-                                tion        hp
                                                                                                  Sae
          Con-    ic       tur-        Struc-      mon-                    Lin-        / Re-      Op-           ta y
                                                                                                              Se d         Tran-         Mag-
Con-      trol    Struc-   al          tur-        ic                      ear         sos
                                                                                        p ne      tim-        -            si-           neto-            hr a
                                                                                                                                                         Teml
trol      Set-    tur-     (AN-        al          Re-         Mod-        Buck-       Spec-      iza-        State        ent           stat-   Elec-   Elec-
 ru
Go p      ting    al       SYS)        ( B)
                                       MD           p ne
                                                   sos         al          ling        trum       tion         hr a
                                                                                                              T eml        T eml
                                                                                                                            hr a         ic      tric    tric
           edd
          ne e
          File
          Non-
          lin-
          ear
          Solu-
          tion
          Solv-
          er
          Units
          Solv-
          er
          Unit                                                                                                                            4       5       5
          Sys-
          tem3

1 - Refer to the following links for specific control settings in the Options control group:

 •     Modal Analysis
 •     Harmonic Response Analysis
 •     Linear Buckling Analysis
 •     Random Vibration Analysis
 •     Response Spectrum Analysis

2 - Indicates control setting is ”step aware” meaning that the setting can be different for each step.

3 - Read-only display if Solver Units is set to Active System.

4 - Read-only display of mks, regardless of whether Solver Units is set to Active System or Manual. A
Magnetostatic analysis can only be solved in the mks unit system.

5 - mks and µmks are the only unit system choices available when solving an Electric or Thermal Electric
analysis.

6 - Available for response spectrum analyses only.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
246                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                 Analysis Settings for Explicit Dynamics Analyses

Analysis Settings for Explicit Dynamics Analyses
Category                 Fields                                       Options                                     Description
Step Controls            Resume From Cycle                                                                        Allows you to select the
                                                                                                                  cycle (time increment
                                                                                                                  for explicit integration)
                                                                                                                  from which to start the
                                                                                                                  solution upon selecting
                                                                                                                  Solve. A cycle of zero
                                                                                                                  (default) indicates the
                                                                                                                  solution will clear any
                                                                                                                  previous progress and
                                                                                                                  start from time zero. A
                                                                                                                  non-zero cycle, on the
                                                                                                                  other hand, allows you
                                                                                                                  to revisit a previous
                                                                                                                  solution and extend it
                                                                                                                  further in time. A solu-
                                                                                                                  tion obtained from a
                                                                                                                  non-zero cycle is con-
                                                                                                                  sidered to have been
                                                                                                                  "resumed" or "restarted".

                                                                                                                  Note that the list will
                                                                                                                  only contain non-zero
                                                                                                                  selections if a solve was
                                                                                                                  previously executed and
                                                                                                                  restart files have been
                                                                                                                  generated.

                                                                                                                  When resuming an ana-
                                                                                                                  lysis, changes to analysis
                                                                                                                  settings will be respec-
                                                                                                                  ted where possible. For
                                                                                                                  example, you may wish
                                                                                                                  to resume an analysis
                                                                                                                  with an extended termin-
                                                                                                                  ation time. Changes to
                                                                                                                  any other features in the
                                                                                                                  model (geometry sup-
                                                                                                                  pression, connections,
                                                                                                                  loads, and so on) will
                                                                                                                  prevent restarts from
                                                                                                                  taking place.

                                                                                                                  See Resume Capability
                                                                                                                  for Explicit Dynamics
                                                                                                                  (ANSYS) Analyses (p. 488)
                                                                                                                  for more information.
                                                                                                                  This field is not available
                                                                                                                  for Explicit Dynamics (LS-
                                                                                                                  DYNA Export) systems.

                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                            of ANSYS, Inc. and its subsidiaries and affiliates.                                            247
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                              Maximum Number of                                                                        The maximum number
                              Cycles                                                                                   of cycles allowed during
                                                                                                                       the analysis.The analysis
                                                                                                                       will stop once the spe-
                                                                                                                       cified value is reached.
                                                                                                                       Enter a large number to
                                                                                                                       have the analysis run to
                                                                                                                       the defined End Time.
                              End Time                                                                                 (Required input) The
                                                                                                                       maximum length of time
                                                                                                                       (starting from zero
                                                                                                                       seconds) to be simulated
                                                                                                                       by the explicit analysis.
                                                                                                                       You should enter a reas-
                                                                                                                       onable estimate to cover
                                                                                                                       the phenomena of in-
                                                                                                                       terest.
                              Maximum Energy Error                                                                     Energy conservation is a
                                                                                                                       measure of the quality of
                                                                                                                       an explicit dynamics
                                                                                                                       analysis. Large deviations
                                                                                                                       from energy conserva-
                                                                                                                       tion usually imply a less
                                                                                                                       than optimal model
                                                                                                                       definition.This paramet-
                                                                                                                       er allows you to automat-
                                                                                                                       ically stop the solution if
                                                                                                                       the deviation from en-
                                                                                                                       ergy conservation be-
                                                                                                                       comes unacceptable.
                                                                                                                       Enter a fraction of the
                                                                                                                       total system energy
                                                                                                                       (measured at the Refer-
                                                                                                                       ence Energy Cycle) for
                                                                                                                       which you want the ana-
                                                                                                                       lysis to stop. For ex-
                                                                                                                       ample, the default value
                                                                                                                       of 0.1 will cause the ana-
                                                                                                                       lysis to stop if the energy
                                                                                                                       error exceeds 10% of the
                                                                                                                       energy at the reference
                                                                                                                       cycle.

                                                                                                                       For Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems this field requires
                                                                                                                       a percentage to be
                                                                                                                       entered. Thus the field
                                                                                                                       name changes to Max-
                                                                                                                       imum Energy Error (%).


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
248                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description
                    Reference Energy Cycle                                                                   The cycle at which you
                                                                                                             want the solver to calcu-
                                                                                                             late the reference energy,
                                                                                                             against which it will calcu-
                                                                                                             late the energy error.
                                                                                                             Usually this will be the
                                                                                                             start cycle (cycle = 0).You
                                                                                                             may need to increase this
                                                                                                             value if the model has
                                                                                                             zero energy at cycle = 0
                                                                                                             (for example if you have
                                                                                                             no initial velocity
                                                                                                             defined).

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                    Initial Time Step                                                                        Enter an initial time step
                                                                                                             you want to use, or use
                                                                                                             the Program Controlled
                                                                                                             default. If left on Pro-
                                                                                                             gram Controlled, the
                                                                                                             time step will be automat-
                                                                                                             ically set to ½ the com-
                                                                                                             puted element stability
                                                                                                             time step.The Program
                                                                                                             Controlled setting is re-
                                                                                                             commended.

                                                                                                             For Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems if this field is left
                                                                                                             on Program Controlled,
                                                                                                             the initial time step will
                                                                                                             be determined by the
                                                                                                             solver.
                    Minimum Time Step                                                                        Enter the minimum time
                                                                                                             step allowed in the ana-
                                                                                                             lysis, or use the Program
                                                                                                             Controlled default. If the
                                                                                                             time drops below this
                                                                                                             value the analysis will
                                                                                                             stop. If set to Program
                                                                                                             Controlled, the value
                                                                                                             will be chosen as 1/10th
                                                                                                             the initial time step.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics


           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                             249
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              Maximum Time Step                                                                        Enter the maximum time
                                                                                                                       step allowed in the ana-
                                                                                                                       lysis, or use the Program
                                                                                                                       Controlled default.The
                                                                                                                       solver will use the minim-
                                                                                                                       um of this value or the
                                                                                                                       computed stability time
                                                                                                                       step during the solve.
                                                                                                                       The Program Controlled
                                                                                                                       setting is recommended.
                              Time Step Safety Factor                                                                  It is not wise to run at the
                                                                                                                       stability limit, so a safety
                                                                                                                       factor is applied to the
                                                                                                                       computed stability time
                                                                                                                       step.The default value of
                                                                                                                       0.9 should work for most
                                                                                                                       analyses.
                              Automatic Mass Scaling                                                                   If set to Yes, activates
                                                                                                                       automatic mass scaling
                                                                                                                       and exposes the follow-
                                                                                                                       ing options.
                                                                           Minimum CFL Time                            The CFL time step that
                                                                           Step                                        you want to achieve in
                                                                                                                       the analysis.

                                                                                                                                   Caution

                                                                                                                                   Mass scaling
                                                                                                                                   introduces
                                                                                                                                   additional
                                                                                                                                   mass into
                                                                                                                                   the system
                                                                                                                                   to increase
                                                                                                                                   the CFL time
                                                                                                                                   step. Introdu-
                                                                                                                                   cing too
                                                                                                                                   much mass
                                                                                                                                   can lead to
                                                                                                                                   non-physical
                                                                                                                                   results.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
250                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description

                                                                                                                         Note

                                                                                                                         Employ User
                                                                                                                         Defined Res-
                                                                                                                         ults (p. 404)
                                                                                                                         MASS_SCALE
                                                                                                                         (ratio of
                                                                                                                         scaled
                                                                                                                         mass/physic-
                                                                                                                         al mass) and
                                                                                                                         TIMESTEP to
                                                                                                                         review the
                                                                                                                         effects of
                                                                                                                         automatic
                                                                                                                         mass scaling
                                                                                                                         on the mod-
                                                                                                                         el.


                                                                 Maximum Element                             This value limits the ratio
                                                                 Scaling                                     of scaled mass/physical
                                                                                                             mass that can be applied
                                                                                                             to each element in the
                                                                                                             model.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Maximum Part Scaling                        This value provides a
                                                                                                             check on the total ratio
                                                                                                             of scaled mass/physical
                                                                                                             mass that can be applied
                                                                                                             to an individual body. If
                                                                                                             this value is exceeded,
                                                                                                             the analysis will stop and
                                                                                                             an error message is dis-
                                                                                                             played.

                                                                                                             For Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems this field requires
                                                                                                             a percentage to be
                                                                                                             entered. Thus the field
                                                                                                             name changes to Max-
                                                                                                             imum Part Scaling (%).
                                                                 Update Frequency                            Allows you to control the
                                                                                                             frequency at which the
                                                                                                             mass scaling will be calcu-
                                                                                                             lated during the solve.


           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                               251
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                                                                                                                       The frequency equates
                                                                                                                       to the increment in
                                                                                                                       cycles at which the mass
                                                                                                                       scale factor will be recom-
                                                                                                                       puted, based on the cur-
                                                                                                                       rent shape of the ele-
                                                                                                                       ments.The default of 0 is
                                                                                                                       recommended and
                                                                                                                       means that the mass
                                                                                                                       scale factor is only calcu-
                                                                                                                       lated once, at the start of
                                                                                                                       the solve.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
Solver Controls               Solve Units                                                                              All model inputs will be
                                                                                                                       converted to this set of
                                                                                                                       units during the solve.
                                                                                                                       Results from the analysis
                                                                                                                       will be converted back
                                                                                                                       to the user units system
                                                                                                                       in the GUI.
                                                                                                                       For Explicit Dynamics
                                                                                                                       systems, this setting is al-
                                                                                                                       ways mm, mg, ms.

                                                                                                                       For Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems this field is termed
                                                                                                                       Unit System.
                              Beam Solution Type                           Bending                                     Any line bodies will be
                                                                                                                       represented as beam
                                                                                                                       elements including a full
                                                                                                                       bending moment calcula-
                                                                                                                       tion.
                                                                           Truss                                       Any line bodies will be
                                                                                                                       represented as truss ele-
                                                                                                                       ments. No bending mo-
                                                                                                                       ments are calculated.
                              Beam Time Step Safety                                                                    An additional safety
                              Factor                                                                                   factor you may apply to
                                                                                                                       the stability time step
                                                                                                                       calculated for beam ele-
                                                                                                                       ments.The default value
                                                                                                                       ensures stability for most
                                                                                                                       cases.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
252                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description
                    Hex Integration Type                         Exact                                       Provides an accurate cal-
                                                                                                             culation of element
                                                                                                             volume, even for warped
                                                                                                             elements.
                                                                 1pt Gauss                                   Approximates the
                                                                                                             volume calculation and
                                                                                                             is less accurate for ele-
                                                                                                             ments featuring warped
                                                                                                             faces.This option is more
                                                                                                             efficient.
                    Shell Sublayers                                                                          The number of integra-
                                                                                                             tion points through the
                                                                                                             thickness of an isotropic
                                                                                                             shell.The default of 3 is
                                                                                                             suitable for many applic-
                                                                                                             ations however this
                                                                                                             number can be increased
                                                                                                             to achieve better resolu-
                                                                                                             tion of through thickness
                                                                                                             plastic deformation
                                                                                                             and/or flow.
                    Shell Shear Correction                                                                   The transverse shear in
                    Factor                                                                                   the element formulation
                                                                                                             is assumed constant over
                                                                                                             the thickness.This correc-
                                                                                                             tion factor accounts for
                                                                                                             the replacement of the
                                                                                                             true parabolic variation
                                                                                                             through the thickness in
                                                                                                             response to a uniform
                                                                                                             transverse shear stress.
                                                                                                             Using a value other than
                                                                                                             the default is not recom-
                                                                                                             mended.
                    Shell BWC Warp Correc-                                                                   The Belytschko-Lin-Tsay
                    tion                                                                                     element formulation be-
                                                                                                             comes inaccurate if the
                                                                                                             elements are warped.To
                                                                                                             overcome this, the ele-
                                                                                                             ment formulation has an
                                                                                                             optional correction to in-
                                                                                                             clude warping. Setting
                                                                                                             this correction to Yes is
                                                                                                             recommended.




           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                           253
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                              Shell Thickness Update                       Nodal                                       Changes in shell thick-
                                                                                                                       ness are calculated at the
                                                                                                                       nodes of shell elements.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                                                                           Elemental                                   Changes in shell thick-
                                                                                                                       ness are calculated at the
                                                                                                                       element integration
                                                                                                                       points.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              Full Shell Integration                                                                   Available only for Explicit
                                                                                                                       Dynamics (LS-DYNA Ex-
                                                                                                                       port) systems.

                                                                                                                       Provides a very fast and
                                                                                                                       accurate shell element
                                                                                                                       formulation.
                              Tet Pressure Integra-                        Average Nodal                               The tetrahedral element
                              tion                                                                                     formulation includes an
                                                                                                                       average nodal pressure
                                                                                                                       integration.This formula-
                                                                                                                       tion does not exhibit
                                                                                                                       volumetric locking, and
                                                                                                                       can be used for large de-
                                                                                                                       formation, and nearly in-
                                                                                                                       compressible behavior
                                                                                                                       such as plastic flow or
                                                                                                                       hyperelasticity.This for-
                                                                                                                       mulation is recommen-
                                                                                                                       ded for the majority of
                                                                                                                       tetrahedral meshes.
                                                                           Constant                                    Uses the constant pres-
                                                                                                                       sure integrated tetrahed-
                                                                                                                       ral formulation.This for-
                                                                                                                       mulation is more efficient
                                                                                                                       than Average Nodal,
                                                                                                                       however it suffers from
                                                                                                                       volumetric locking under
                                                                                                                       constant bulk deforma-
                                                                                                                       tion.
                              Shell Inertia Update                         Recompute                                   The principal axes of
                                                                                                                       rotary inertia are by de-


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
254                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description
                                                                                                             fault recalculated each
                                                                                                             cycle.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Rotate                                      Rotates the axes, rather
                                                                                                             than recomputing each
                                                                                                             cycle.This option is more
                                                                                                             efficient, however it can
                                                                                                             lead to numerical instabil-
                                                                                                             ities due to floating point
                                                                                                             round-off for long run-
                                                                                                             ning simulations.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                    Density Update                               Program Controlled                          The solver decides
                                                                                                             whether an incremental
                                                                                                             update is necessary
                                                                                                             based on the rate and
                                                                                                             extent of element de-
                                                                                                             formation.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Incremental                                 Forces the solver to al-
                                                                                                             ways use the incremental
                                                                                                             update.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Total                                       Forces the solver to al-
                                                                                                             ways recalculate the
                                                                                                             density from element-
                                                                                                             volume and mass.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                    Minimum Velocity                                                                         The minimum velocity
                                                                                                             you want to allow in the

           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                              255
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                                                                                                                       analysis. If any model ve-
                                                                                                                       locity drops below this
                                                                                                                       Minimum Velocity, it
                                                                                                                       will be set to zero.The
                                                                                                                       default is recommended
                                                                                                                       for most analyses.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              Maximum Velocity                                                                         The maximum velocity
                                                                                                                       you want to allow in the
                                                                                                                       analysis. If any model ve-
                                                                                                                       locity rises above the
                                                                                                                       Maximum Velocity, it
                                                                                                                       will be capped.This can
                                                                                                                       improve the stability/ro-
                                                                                                                       bustness of the analysis
                                                                                                                       in some instances.The
                                                                                                                       default is recommended
                                                                                                                       for most analyses.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              Radius Cutoff                                                                            At the start of your calcu-
                                                                                                                       lation, if a node is within
                                                                                                                       the specified radius of a
                                                                                                                       symmetry plane, it will be
                                                                                                                       placed on the symmetry
                                                                                                                       plane. If a node is outside
                                                                                                                       the specified radius from
                                                                                                                       a symmetry plane at the
                                                                                                                       start of your calculation,
                                                                                                                       it will not be allowed to
                                                                                                                       come closer than this ra-
                                                                                                                       dius to the symmetry
                                                                                                                       plane as your calculation
                                                                                                                       proceeds.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
Damping Controls              Linear Artificial Viscos-                                                                A linear coefficient of arti-
                              ity                                                                                      ficial viscosity.This coeffi-
                                                                                                                       cient smooths out shock
                                                                                                                       discontinuities over the


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
256                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description
                                                                                                             mesh. Using a value oth-
                                                                                                             er than the default is not
                                                                                                             recommended.
                    Quadratic Artificial Vis-                                                                A quadratic coefficient of
                    cosity                                                                                   artificial viscosity.This
                                                                                                             coefficient damps out
                                                                                                             post shock discontinuity
                                                                                                             oscillations. Using a value
                                                                                                             other than the default is
                                                                                                             not recommended.
                    Linear Viscosity in Ex-                                                                  Artificial viscosity is nor-
                    pansion                                                                                  mally applied to materi-
                                                                                                             als in compression only.
                                                                                                             This option allows you to
                                                                                                             apply the viscosity for
                                                                                                             materials in compression
                                                                                                             and expansion.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                    Hourglass Damping                            AUTODYN Standard                            The method of hourglass
                                                                 Flanagan Belytschko                         damping to be used with
                                                                                                             solid hexahedral ele-
                                                                                                             ments.
                    Stiffness Coefficient                                                                    The stiffness coefficient
                                                                                                             for Flanagan Belytschko
                                                                                                             hourglass damping in
                                                                                                             solid hexahedral ele-
                                                                                                             ments.
                    Viscous Coefficient                                                                      The viscous coefficient
                                                                                                             for hourglass damping
                                                                                                             used in hexahedral solid
                                                                                                             elements and quadrilater-
                                                                                                             al shell elements.
                    Static Damping                                                                           A static damping con-
                                                                                                             stant may be specified
                                                                                                             which changes the solu-
                                                                                                             tion from a dynamic
                                                                                                             solution to a relaxation
                                                                                                             iteration converging to a
                                                                                                             state of stress equilibri-
                                                                                                             um. For optimal conver-
                                                                                                             gence, the value chosen
                                                                                                             for the damping con-
                                                                                                             stant, R, may be defined
                                                                                                             by: R = 2*timestep/T
                                                                                                             where timestep is the ex-

           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                             257
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                                                                                                                       pected average value of
                                                                                                                       the timestep and T is
                                                                                                                       longest period of vibra-
                                                                                                                       tion for the system being
                                                                                                                       analyzed.
Erosion Controls              On Geometric Strain                                                                      If set to Yes, elements
                              Limit                                                                                    will automatically erode
                                                                                                                       if the geometric strain in
                                                                                                                       the element exceeds the
                                                                                                                       specified limit.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              Geometric Strain Limit                                                                   The geometric strain lim-
                                                                                                                       it for erosion. Recommen-
                                                                                                                       ded values are in the
                                                                                                                       range from 0.75 to 3.0.
                                                                                                                       The default value is 1.5.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              On Material Failure                                                                      If set to Yes, elements
                                                                                                                       will automatically erode
                                                                                                                       if a material failure prop-
                                                                                                                       erty is defined in the ma-
                                                                                                                       terial used in the ele-
                                                                                                                       ments, and the failure
                                                                                                                       criteria has been
                                                                                                                       reached. Elements with
                                                                                                                       materials including a
                                                                                                                       damage model will also
                                                                                                                       erode if damage reaches
                                                                                                                       a value of 1.0.

                                                                                                                       This field is not available
                                                                                                                       for Explicit Dynamics
                                                                                                                       (LS-DYNA Export) sys-
                                                                                                                       tems.
                              On Minimum Element                                                                       If set to Yes, elements
                              Time Step                                                                                will automatically erode
                                                                                                                       if their calculated time
                                                                                                                       step falls below the spe-
                                                                                                                       cified value.
                              Minimum Element Time                                                                     The minimum controlling
                              Step                                                                                     time step that an ele-
                                                                                                                       ment can have. If the ele-

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
258                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                   Analysis Settings for Explicit Dynamics Analyses

Category                   Fields                                       Options                                     Description
                                                                                                                    ment time step drops
                                                                                                                    below the specified
                                                                                                                    value, the element will be
                                                                                                                    eroded.

                                                                                                                    This field is not dis-
                                                                                                                    played for Explicit Dy-
                                                                                                                    namics (LS-DYNA Ex-
                                                                                                                    port) systems when On
                                                                                                                    Minimum Element
                                                                                                                    Time Step is set to No.
                           Retain Inertia of Eroded                                                                 If all elements that are
                           Material                                                                                 connected to a node in
                                                                                                                    the mesh erode, the in-
                                                                                                                    ertia of the resulting
                                                                                                                    free node can be re-
                                                                                                                    tained if this option is
                                                                                                                    set to Yes. The mass
                                                                                                                    and momentum of the
                                                                                                                    free node is retained
                                                                                                                    and can be involved in
                                                                                                                    subsequent impact
                                                                                                                    events to transfer mo-
                                                                                                                    mentum in the system.

                                                                                                                    If set to No, all free
                                                                                                                    nodes will be automatic-
                                                                                                                    ally removed from the
                                                                                                                    analysis.
                                                                                                                    This field is not displayed
                                                                                                                    for Explicit Dynamics (LS-
                                                                                                                    DYNA Export) systems
                                                                                                                    when On Minimum Ele-
                                                                                                                    ment Time Step is set to
                                                                                                                    No.
Output Controls            Save Results on                                                                          During the solve of an
                                                                                                                    explicit dynamics system,
                                                                                                                    results are saved to disk
                                                                                                                    at a frequency defined
                                                                                                                    through this control.The
                                                                                                                    following settings are
                                                                                                                    available.
                                                                        Cycles                                      Save results files after a
                                                                                                                    specified increment in
                                                                                                                    the number of cycles. Ex-
                                                                                                                    poses a Cycles field
                                                                                                                    where you enter the in-
                                                                                                                    crement in cycles.




                  Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                              of ANSYS, Inc. and its subsidiaries and affiliates.                                           259
Using the Mechanical Application Features

Category                      Fields                                       Options                                     Description
                                                                                                                       This setting is not avail-
                                                                                                                       able for Explicit Dynam-
                                                                                                                       ics (LS-DYNA Export)
                                                                                                                       systems.
                                                                           Time                                        Save results file after a
                                                                                                                       specified increment in
                                                                                                                       time. Exposes a Time
                                                                                                                       field where you enter a
                                                                                                                       time increment.
                                                                           Equally Spaced Time                         (Default) Save a specified
                                                                           Points                                      number of result files
                                                                                                                       during the analysis.The
                                                                                                                       frequency is defined by
                                                                                                                       the termination time /
                                                                                                                       number of points. Ex-
                                                                                                                       poses a Number of
                                                                                                                       Points field where you
                                                                                                                       enter the number of res-
                                                                                                                       ults files required.
                              Save Restart Files on                                                                    During the solve of an
                                                                                                                       explicit dynamics system,
                                                                                                                       restart files are saved to
                                                                                                                       disk at a frequency
                                                                                                                       defined through this
                                                                                                                       control.The following
                                                                                                                       settings are available.
                                                                           Cycles                                      Save restart files after a
                                                                                                                       specified increment in
                                                                                                                       the number of cycles. Ex-
                                                                                                                       poses a Cycles field
                                                                                                                       where you enter the in-
                                                                                                                       crement in cycles.
                                                                           Time                                        Save restart files after a
                                                                                                                       specified increments in
                                                                                                                       time. Exposes a Time
                                                                                                                       field where you enter a
                                                                                                                       time increment.

                                                                                                                       This setting is not avail-
                                                                                                                       able for Explicit Dynam-
                                                                                                                       ics (LS-DYNA Export)
                                                                                                                       systems.
                                                                           Equally Spaced Time                         (Default) Save a specified
                                                                           Points                                      number of restart files
                                                                                                                       during the analysis.The
                                                                                                                       frequency is defined by
                                                                                                                       the termination time /
                                                                                                                       number of points. Ex-
                                                                                                                       poses a Number of

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
260                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Analysis Settings for Explicit Dynamics Analyses

Category            Fields                                       Options                                     Description
                                                                                                             Points field where you
                                                                                                             enter the number of re-
                                                                                                             start files required.
                    Save Result Tracker                                                                      Result tracker data ob-
                    Data on                                                                                  jects are scoped to specif-
                                                                                                             ic regions in a model.
                                                                                                             This data can be output
                                                                                                             at much higher fre-
                                                                                                             quency than the entire
                                                                                                             model results set.These
                                                                                                             controls below allow you
                                                                                                             to set the frequency at
                                                                                                             which result tracker data
                                                                                                             is saved to disk.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Cycles                                      Save results tracker data
                                                                                                             after a specified incre-
                                                                                                             ment in the number of
                                                                                                             cycles. Exposes a Cycles
                                                                                                             field where you enter the
                                                                                                             increment in cycles.The
                                                                                                             default value is 1.
                                                                 Time                                        Save result tracker data
                                                                                                             after a specified incre-
                                                                                                             ment in time. Exposes a
                                                                                                             Time field where you
                                                                                                             enter a time increment.
                    Save Solution Output                                                                     Solution output provides
                    on                                                                                       a summary of the state of
                                                                                                             the solution as the solve
                                                                                                             proceeds. Use this con-
                                                                                                             trol to define the fre-
                                                                                                             quency at which solution
                                                                                                             output is generated.

                                                                                                             This field is not available
                                                                                                             for Explicit Dynamics
                                                                                                             (LS-DYNA Export) sys-
                                                                                                             tems.
                                                                 Cycles                                      Save solution output
                                                                                                             data after a specified in-
                                                                                                             crement in the number
                                                                                                             of cycles. Enter the incre-
                                                                                                             ment in cycles. Exposes
                                                                                                             a Cycles field where you


           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                            261
Using the Mechanical Application Features

Category                       Fields                                       Options                                     Description
                                                                                                                        enter the increment in
                                                                                                                        cycles.
                                                                            Time                                        Save solution output
                                                                                                                        data after a specified in-
                                                                                                                        crement in time. Exposes
                                                                                                                        a Time field where you
                                                                                                                        enter a time increment.
Analysis Data Manage-          Solver Files Directory                                                                   The permanent location
ment                                                                                                                    for all the files generated
                                                                                                                        during a solve.This is a
                                                                                                                        read-only field provided
                                                                                                                        for information.
                               Scratch Solver Files Dir-                                                                A temporary location for
                               ectory                                                                                   all files generated during
                                                                                                                        a solve.These files are
                                                                                                                        then moved to the Solv-
                                                                                                                        er Files Directory for
                                                                                                                        completed solves.This is
                                                                                                                        a read-only field
                                                                                                                        provided for information.
                                                                                                                        See Analysis Data Man-
                                                                                                                        agement for more inform-
                                                                                                                        ation.

                                                                                                                        This field is not available
                                                                                                                        for Explicit Dynamics
                                                                                                                        (LS-DYNA Export) sys-
                                                                                                                        tems.

Steps and Step Controls for Static and Transient Analyses
The following topics are covered in this section:
 Role of Time in Tracking
 Steps, Substeps, and Equilibrium Iterations
 Automatic Time Stepping
 Guidelines for Integration Step Size
 Step Controls

Role of Time in Tracking
Time is used as a tracking parameter in all static and transient analyses, whether or not the analysis is truly
time-dependent. The advantage of this is that you can use one consistent "counter" or "tracker" in all cases,
eliminating the need for analysis-dependent terminology. Moreover, time always increases monotonically,
and most things in nature happen over a period of time, however brief the period may be.

Obviously, in a transient analysis time represents actual, chronological time in seconds, minutes, or hours.
In a static analysis, however, time simply becomes a counter that identifies steps and substeps. By default,
the program automatically assigns time = 1.0 at the end of step 1, time = 2.0 at the end of step 2, and so
on. Any substeps within a step will be assigned the appropriate, linearly interpolated time value. By assigning
your own time values in such analyses, you can establish your own tracking parameter. For example, if a

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
262                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                          What are substeps and equilibrium iterations?

load of 100 units is to be applied incrementally over one step, you can specify time at the end of that step
to be 100, so that the load and time values are synchronous.

Steps, Substeps, and Equilibrium Iterations
What is a step?
A step corresponds to a set of loads for which you want to obtain a solution and review results. In this way
every static or transient dynamic analysis has at least one step. However there are several scenarios where
you may want to consider using multiple steps within a single analysis, that is, multiple solutions and result
sets within a single analysis.

A static or transient analysis starts at time = 0 and proceeds until a step end time that you specify. This time
span can be further subdivided into multiple steps where each step spans a different time range.

As mentioned in the Role of Time in Tracking (p. 262) section, each step spans a ‘time’ even in a static analysis.

When do you need Steps?
Steps are required if you want to change the analysis settings for a specific time period. For example in an
impact analysis you may want to manually change the allowable minimum and maximum time step sizes
during impact. In this case you can introduce a step that spans a time period shortly before and shortly after
impact and change the analysis settings for that step.

Steps are also useful generally to delineate different portions of an analysis. For example, in a linear static
structural analysis you can apply a wind load in the first step, a gravity load in the second step, both loads
and a different support condition in the third step, and so on. As another example, a transient analysis of
an engine might include load conditions corresponding to gravity, idle speed, maximum power, back to idle
speed. The analysis may require repetition of these conditions over various time spans. It is convenient to
track these conditions as separate steps within the time history.

In addition steps are also required for deleting loads or adding new loads such as specified displacements
or to set up a pretension bolt load sequence. Steps are also useful in setting up initial conditions for a
transient analysis.

How do you define steps?
See the procedure, ”Specifying Analysis Settings for Multiple Steps” located in the Establish Analysis Set-
tings (p. 8) section.

What are substeps and equilibrium iterations?
Solving an analysis with nonlinearities requires convergence of an iterative solution procedure. Convergence
of this solution procedure requires the load to be applied gradually with solutions carried out at intermediate
load values. These intermediate solution points within a step are referred to as substeps. Essentially a substep
is an increment of load within a step at which a solution is carried out. The iterations carried out at each
substep to arrive at a converged solution are referred to as equilibrium iterations.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               263
Using the Mechanical Application Features

      Load
                        Substep


                        Load step



                            1                2
Final

load

value                                                      Equilibrium

                                                           iterations




                                                           Substeps



Automatic Time Stepping
Auto time stepping, also known as time step optimization, aims to reduce the solution time especially for
nonlinear and/or transient dynamic problems by adjusting the amount of load increment. If nonlinearities
are present, automatic time stepping gives the added advantage of incrementing the loads appropriately
and retreating to the previous converged solution (bisection) if convergence is not obtained. The amount
of load increment is based on several criteria including the response frequency of the structure and the
degree of nonlinearities in the analysis.

The load increment within a step is controlled by the auto time stepping procedure within limits set by you.
You have the option to specify the maximum, minimum and initial load increments. The solution will start
with the “initial” increment but then the automatic procedure can vary further increments within the range
prescribed by the minimum and maximum values.

You can specify these limits on load increment by specifying the initial, minimum, and maximum number
of substeps that are allowed. Alternatively, since a step always has a time span (start time and end time),
you can also equivalently specify the initial, minimum and maximum time step sizes.

Although it seems like a good idea to activate automatic time stepping for all analyses, there are some cases
where it may not be beneficial (and may even be harmful):

 •     Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies),
       where the low-frequency energy content of part of the system may dominate the high-frequency areas.
 •     Problems that are constantly excited (for example, seismic loading), where the time step tends to change
       continually as different frequencies are excited.
 •     Kinematics (rigid-body motion) problems, where the rigid-body contribution to the response frequency
       term may dominate.

Guidelines for Integration Step Size
The accuracy of the transient dynamic solution depends on the integration time step: the smaller the time
step, the higher the accuracy. A time step that is too large introduces an error that affects the response of
the higher modes (and hence the overall response). On the other hand too small a time step size wastes
computer resources.

An optimum time step size can depend on several factors:


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
264                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                           What are substeps and equilibrium iterations?

1.   Response frequency: The time step should be small enough to resolve the motion (response) of the
     structure. Since the dynamic response of a structure can be thought of as a combination of modes,
     the time step should be able to resolve the highest mode that contributes to the response. The solver
     calculates an aggregate response frequency at every time point. A general rule of thumb it to use ap-
     proximately twenty points per cycle at the response frequency. That is, if f is the frequency (in
     cycles/time), the integration time step (ITS) is given by:

     ITS = 1/(20f )

     Smaller ITS values will be required if accurate velocity or acceleration results are needed.

     The following figure shows the effect of ITS on the period elongation of a single-DOF spring-mass
     system. Notice that 20 or more points per cycle result in a period elongation of less than 1 percent.

                       10


                          9

       Period
                          8
     Elongation

         (%)
                          7


                          6


                          5


                          4


                          3


                          2                                  recommended



                          1


                          0
                                    0               20               40               60              80               100
                                            10               30              50               70               90

                                                Number of Time Steps Per Cycle


2.   Resolve the applied load-versus-time curve(s). The time step should be small enough to “follow” the
     loading function. For example, stepped loads require a small ITS at the time of the step change so
     that the step change can be closely followed. ITS values as small as 1/180f may be needed to follow
     stepped loads.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               265
Using the Mechanical Application Features

      ü                                                                 ü

                            Input

                            Response




                                                     t                                                                              t




 3.   Resolve the contact frequency. In problems involving contact (impact), the time step should be small
      enough to capture the momentum transfer between the two contacting faces. Otherwise, an apparent
      energy loss will occur and the impact will not be perfectly elastic. The integration time step can be
      determined from the contact frequency (fc) as:

      ITS=1/Nfc                   fc =(1/ 2π) k /m

      where k is the gap stiffness, m is the effective mass acting at the gap, and N is the number of points
      per cycle. To minimize the energy loss, at least thirty points per cycle of (N = 30) are needed. Larger
      values of N may be required if velocity or acceleration results are needed. See the description of the
      Predict for Impact option within the Time Step Controls contact Advanced settings for more inform-
      ation.

      You can use fewer than thirty points per cycle during impact if the contact period and contact mass
      are much less than the overall transient time and system mass, because the effect of any energy loss
      on the total response would be small.
 4.   Resolve the nonlinearities. For most nonlinear problems, a time step that satisfies the preceding
      guidelines is sufficient to resolve the nonlinearities. There are a few exceptions, however: if the structure
      tends to stiffen under the loading (for example, large deflection problems that change from bending
      to membrane load-carrying behavior), the higher frequency modes that are excited will have to be
      resolved.

After calculating the time step sizes using the above guidelines, you need to use the minimum value for
your analysis. However using this minimum time step size throughout a transient analysis can be very inef-
ficient. For example in an impact problem you may need small time step sizes calculated as above only
during and for a short duration after the impact. At other parts of the time history you may be able to get
accurate results with larger time steps sizes. Use of the Automatic Time Stepping (p. 264) procedure lets the
solver decide when to increase or decrease the time step during the solution.

Step Controls
Step Controls play an important role in static and transient dynamic analyses. Step controls are used to
perform two distinct functions: 1) Defining Steps, and 2) Specifying analysis settings for each step.

Defining Steps
See the procedure, ”Specifying Analysis Settings for Multiple Steps” located in the Establish Analysis Set-
tings (p. 8) section.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
266                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 Specifying Analysis Settings for Each Step

Specifying Analysis Settings for Each Step
The following items can be changed on a per step basis: Step Controls, Nonlinear Controls, and Output
Controls. Nonlinear Controls and Output Controls are discussed in their own sections.

Details of Step Controls:




Current Step Number shows the step ID for which the settings in Step Controls, Nonlinear Controls, and
Output Controls are applicable. The currently selected step is also highlighted in the bar at the bottom of
the Graph window. You can select multiple steps by selecting rows in the data grid or the bars at the bottom
of the Graph window. In this case the Current Step Number will be set to multi-step. In this case any
settings modified will affect all selected steps.

Step End Time shows the end time of the current step number. When multiple steps are selected this will
indicate multi-step.

Auto Time Stepping is discussed in detail in the Automatic Time Stepping (p. 264) section.

Automatic time stepping is available for static and transient analyses, and is especially useful for nonlinear
solutions. Settings for controlling automatic time stepping are included in a drop down menu under Auto
Time Stepping in the Details view. The following options are available:

 •   Program Controlled (default): The Mechanical application automatically switches time stepping on and
     off as needed. A check is performed on nonconvergent patterns. The physics of the simulation is also
     taken into account. The Program Controlled settings are presented in the following table:

                                   Auto Time Stepping Program Controlled Settings
              Analysis Type                         Initial Substeps                 Minimum Substeps                        Maximum Substeps
     Linear Static Structural                                    1                                  1                                1
     Nonlinear Static Structural                                 1                                  1                                10
     Linear Steady-State Thermal                                 1                                  1                                10
     Nonlinear Steady-State Thermal                              1                                  1                                10
     Transient Thermal                                         100                                 10                               1000



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       267
Using the Mechanical Application Features

 •    On: You control time stepping by completing the following fields that only appear if you choose this
      option. No checks are performed on nonconvergent patterns and the physics of the simulation is not
      taken into account.
      –   Initial Substeps: Specifies the size of the first substep. The default is 1.
      –   Minimum Substeps: Specifies the minimum number of substeps to be taken (that is, the maximum
          time step size). The default is 1.
      –   Maximum Substeps: Specifies the maximum number of substeps to be taken (that is, the minimum
          time step size). The default is 10.
 •    Off: No time stepping is enabled. You are prompted to enter the Number Of Substeps. The default is
      1.

Define By allows you to set the limits on load increment in one of two ways. You can specify the Initial,
Minimum and Maximum number of substeps for a step or equivalently specify the Initial, Minimum and
Maximum time step size.

Carry Over Time Step is an option available when you have multiple steps. This is useful when you do not
want any abrupt changes in the load increments between steps. When this is set the Initial time step size
of a step will be equal to the last time step size of the previous step.

Time Integration is valid only for a transient structural (ANSYS) or transient thermal analysis. This field in-
dicates whether a step should include transient effects (for example, structural inertia, thermal capacitance)
or whether it is a static (steady-state) step. This field can be used to set up the Initial Conditions for a tran-
sient analysis.

 •    On: Default for transient analyses.
 •    Off: Do not include structural inertia or thermal capacitance in solving this step.

      Note

      With Time Integration set to Off in transient structural (ANSYS) analyses, Workbench does not
      compute velocity results. Therefore spring damping forces, which are derived from velocity will
      equal zero. This is not the case for transient structural (MBD) analyses.

Activation/Deactivation of Loads Within a Step
There is a mechanism by which a load can be activated (included) or deactivated (deleted) from being used
in the analysis within the time span of a step. See “To activate/deactivate loads in a stepped analysis” under
How to Apply Loads (p. 317) for the procedure. For most loads (for example, pressure or force) deleting the
load is the same as setting the load value to zero. But for certain loads such as specified displacement this
is not the case.

      Note

      For displacements and remote displacements, it is possible to deactivate only one degree of
      freedom within a step.

Some scenarios where load deactivation is useful are:

 •    Springback of a cantilever beam after a plasticity analysis (see example below).
 •    Bolt pretension sequence.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
268                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 Nonlinear Controls for Static and Transient

 •   Specifying different initial velocities for different parts in a transient analysis.

Example: Springback of a cantilever beam after a plasticity analysis

In this case a Y displacement of -2.00 inch is applied in the first Step. In the second step this load is deactivated
(deleted). Deactivated portions of a load are shown in gray in the Graph and also have a red stop bars in-
dicating the deactivation. The corresponding cells in the data grid are also shown in gray.




In this example the second step has a displacement value of -1.5. However since the load is deactivated this
will not have any effect until the third step. In the third step a displacement of -1.5 will be step applied from
the sprung-back location.

Nonlinear Controls
Various controls are available under the Nonlinear Controls category for the following:

 •   Static and Transient Analyses
 •   Transient Thermal Analyses
 •   Transient Structural (MBD) Analyses

Nonlinear Controls for Static and Transient
Convergence Criterion

When solving nonlinear static or transient analyses an iterative procedure (equilibrium iterations) is carried
out at each substep. Successful solution is indicated when the out-of-balance loads are less than the specified
convergence criteria. Criteria appropriate for the analysis type and physics are displayed in this grouping.

The following criteria are available: Force, Moment, Displacement, Rotation, Heat, Temperature, CSG,
and AMP. The following convergence controls are available for each of these criteria:

 •   Program Controlled (default): The Mechanical application sets the convergence criteria.
 •   On: You specifically would like for this convergence criterion to be activated.
     –   Value: This is the reference value that the solver uses to establish convergence. It may be program
         controlled (recommended) in which case the solver automatically calculates the value based on ex-
         ternal forces including reactions, or you can input a constant value.

         When Temperature Convergence is set to On, the Value field includes a drop down option list
         where you can choose either ANSYS Calculated or User Input. Choosing User Input displays an
         Input Value field where you can add a value.

         When any other convergence is set to On, simply clicking on ANSYS Calculated allows you to add
         a value that will replace the ANSYS Calculated display.
     –   Tolerance times Value determines the convergence criterion




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                  269
Using the Mechanical Application Features

      –   Minimum Reference: This is useful for analyses where the external forces tend to zero. This can
          happen, for example, with free thermal expansion where rigid body motion is prevented. In these
          cases the larger of Value or Minimum Reference will be used as the reference value.
 •    Remove: Indicates that an attempt will be made to remove this criterion during solution.

Line Search

Line search can be useful for enhancing convergence, but it can be expensive (especially with plasticity).
You might consider setting Line Search on in the following cases:

 •    When your structure is force-loaded (as opposed to displacement-controlled).
 •    If you are analyzing a "flimsy" structure which exhibits increasing stiffness (such as a fishing pole).
 •    If you notice (from the program output messages) oscillatory convergence patterns.

Nonlinear Controls for Transient Thermal Analyses
Nonlinear Formulation

Nonlinear Formulation controls how nonlinearities are to be handled for the solution. The following options
are available:

 •    Program Controlled (default) - Workbench automatically chooses between the Full or Quasi setting
      as described below. The Quasi setting is based on a default Reformulation Tolerance of 5%. The Quasi
      option is used by default, but the Full option is used in cases when a Radiation load is present or when
      a distributed solver is used during the solution.
 •    Full - Manually sets formulation for a full Newton-Raphson solution.
 •    Quasi - Manually sets formulation based on a tolerance you enter in the Reformulation Tolerance field
      that appears if Quasi is chosen.

Nonlinear Controls for Transient Structural (MBD) Analyses
Relative Assembly Tolerance

Allows you to specify the criterion for determining if two parts are connected. Setting the tolerance can be
useful in cases where initially, parts are far enough away from one another that, by default, the program
will not detect that they are connected. You could then increase the tolerance as needed.

Energy Accuracy Tolerance

This is the main driver to the automatic time stepping. The automatic time stepping algorithm measures
the portion of potential and kinetic energy that is contained in the highest order terms of the time integration
scheme, and computes the ratio of the energy to the energy variations over the previous time steps. Com-
paring the ratio to the Energy Accuracy Tolerance, Workbench will decide to increase or decrease the time
step. See the Transient Structural (MBD) Analysis (p. 84) section for more information.

Output Controls
Specify the time points at which results should be available for postprocessing. The default is to write results
at every solution point. For large, nonlinear analyses this could lead to a large results file.

The Output Controls are as follows:



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
270                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Weak Springs

 •   Calculate Stress and Calculate Strain for Static Structural, Transient Structural (ANSYS), Modal, and
     Linear Buckling analyses.
 •   Calculate Thermal Flux for Steady-State Thermal and Transient Thermal analyses.
 •   Calculate Velocity and Calculate Acceleration for Response Spectrum analyses.

The above output controls are not step-aware, meaning that the settings are constant across multiple steps.

In addition, the following settings allow you to define when data is calculated and written to the result file
for Static Structural, Transient Structural (ANSYS), Transient Structural (MBD), Steady-State Thermal, and
Transient Thermal analyses:

 •   Calculate Results At: Specify this time to be All Time Points (default), Last Time Point, or Equally
     Spaced Time Points.
 •   Number of Time Points: Displayed only if Calculate Results At is set to Equally Spaced Time Points.

The controls that define when data is calculated are step aware, meaning that the settings can vary across
multiple steps.

Limitations When Using the ANSYS Solver

 •   The maximum number of results sets allowed on the results file in a single analysis is 1000 by default.
     If your analysis requires more than 1000 results sets, you can raise the default limit by inserting a
     Commands object for the /CONFIG,NRES command.
 •   The Mechanical application cannot post process split result files produced by the ANSYS solver. Try
     either of the following workarounds should this be an issue:
     –   Use Output Controls to limit the result file size. Also, the size can more fully be controlled (if needed)
         by inserting a Commands object for the OUTRES command.
     –   Increase the threshold for the files to be split by inserting a Commands object for the /CONFIG,FSPLIT
         command.

Solver Controls
Solver Type
If you want to specify a Solver type for the Mechanical application to use, select the Solver Type field. You
can choose between Program Controlled, Direct, or Iterative solvers. A direct solver works better
with thin flexible models. An iterative solver works better for bulky models. In most cases, the program
controlled option does select the optimal solver.

Weak Springs
For stress or shape simulations, the addition of weak springs can facilitate a solution by preventing numer-
ical instability, while not having an effect on real world engineering loads. The following Weak Springs
settings are available in the Details view:

 •   Programmed Controlled (default): Workbench determines if weak springs will facilitate the solution,
     then adds a standard weak springs stiffness value accordingly.
 •   On: Workbench always adds a weak spring stiffness. Choosing On causes a Spring Stiffness option to
     appear that allows you to control the amount of weak spring stiffness. Your choices are to use the
     standard stiffness mentioned above for the Programmed Controlled setting of Weak Springs or to


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       271
Using the Mechanical Application Features

      enter a customized value. The following situations may prompt you to choose a customized stiffness
      value:
      a.    The standard weak spring stiffness value may produce springs that are too weak such that the
            solution does not occur, or that too much rigid body motion occurs.
      b.    You may judge that the standard weak spring stiffness value is too high (rare case).
      c.    You many want to vary the weak spring stiffness value to determine the impact on the simulation.

      The following Spring Stiffness settings are available:
      –    Programmed Controlled (default): Adds a standard weak spring stiffness (same as the value added
           for the Programmed Controlled setting of Weak Springs).
      –    Factor: Adds a customized weak spring stiffness whose value equals the Programmed Controlled
           standard value times the value you enter in the Spring Stiffness Factor field (appears only if you
           choose Factor). For example, setting Spring Stiffness Factor equal to 20 means that the weak
           springs will be 20 times stronger than the Programmed Controlled standard value.
      –    Manual: Adds a customized weak spring stiffness whose value you enter (in units of force/length)
           in the Spring Stiffness Value field (appears only if you choose Manual).
 •    Off: Weak springs are not added. Use this setting if you are confident that weak springs are not necessary
      for a solution.

Large Deflection
This field, applicable to static structural and transient structural (ANSYS) analyses, determines whether the
solver should take into account large deformation effects such as large deflection, large rotation, and large
strain. Set Large Deflection to On if you expect large deflections (as in the case of a long, slender bar under
bending) or large strains (as in a metal-forming problem).

When using hyperelastic material models, you must set Large Deflection On.

Inertia Relief - Linear Static Structural Analyses Only
Calculates accelerations to counterbalance the applied loads. Displacement constraints on the structure
should only be those necessary to prevent rigid-body motions (6 for a 3-D structure). The sum of the reaction
forces at the constraint points will be zero. Accelerations are calculated from the element mass matrices and
the applied forces. Data needed to calculate the mass (such as density) must be input. Both translational
and rotational accelerations may be calculated.

This option applies only to the linear static structural analyses. Displacements and stresses are calculated as
usual.

Time Integration Type - Transient Analysis of Multiple Rigid Bodies Only
This feature is applicable to a Transient Structural (MBD) analysis.

The Time Integration Type feature employs the fourth and fifth order polynomial approximation of the
Runge-Kutta algorithm to enable the Mechanical application to integrate the equations of motion during
analyses. This feature allows you to choose time integration algorithms and specify whether to use constraint
stabilization. The fifth order approximation usually allows for larger time steps and can therefore reduce the
total simulation time.

The Details view Solver Controls options for the Time Integration Type include:


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
272                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                            Harmonic Response Analysis - Options Control Settings

 •   Time Integration Type field. Available time integration algorithms include:
     –   Runge-Kutta 4 (Default) - Fourth Order Runge-Kutta
     –   Runge-Kutta 5 - Fifth Order Runge-Kutta
 •   Use Stabilization field. When specified, this option provides the numerical equivalent for spring and
     damping effects and is proportional to the constraint violation and its time derivative. If there is no
     constraint violation, the spring and damping has no effect. The addition of artificial spring and damping
     does not change the dynamic properties of the model. Stabilization options include:
     –   Off (Default) - constraint stabilization is ignored.
     –   On - Because constraint stabilization has a minimal impact on calculation time, its use is recommen-
         ded. When specified, the Stabilization Parameters field also displays. Stabilization Parameters
         options include:
     –   Program Controlled - valid for most applications.
     –   User Defined - manual entry of spring stiffness (Alpha) and damping ratio (Beta) required.

          Note

          Based on your application, it may be necessary to enter customized settings for Alpha and
          Beta. In this case, start with small values and use the same value in both fields. Alpha and
          Beta values that are too small have little effect and values that are too large cause the time
          step to be too small. The valid values for Alpha and Beta are Alpha >=0 and Beta >=0. If
          Both Alpha and Beta are zero, the stabilization will have no effect.



Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Re-
sponse Spectrum Analyses
An Options control group is included in the Analysis Settings Details view for the following analysis types:

 •   Modal
 •   Harmonic Response
 •   Linear Buckling
 •   Random Vibration
 •   Response Spectrum

Modal Analysis - Options Control Settings
Max Modes to Find specifies the number of natural frequencies to solve for in a modal analysis.

Limit Search Range allows you to specify a frequency range within which to find the natural frequencies.
The default is set to No. If you set this to Yes, you can enter a minimum and maximum frequency value. If
you specify a range the solver will strive to extract as many frequencies as possible within the specified
range subject to a maximum specified in the Max Modes to Find field.

Harmonic Response Analysis - Options Control Settings
Frequency Sweep Range
    This is set by defining the Range Minimum and Range Maximum values under Options in the Details
    view.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               273
Using the Mechanical Application Features

Solution Intervals
    This sets the number of the solution points between the Frequency Sweep Range. You can request any
    number of harmonic solutions to be calculated. The solutions are evenly spaced within the specified
    frequency range, as long as clustering is not active. For example, if you specify 10 solutions in the range
    30 to 40 Hz, the program will calculate the response at 31, 32, 33, ..., 39, and 40 Hz. No response is cal-
    culated at the lower end of the frequency range.

Two solution methods are available to perform harmonic response analysis: Mode Superposition method
and Direct Integration (Full) method. Below are some details regarding each of these methods.

Mode Superposition Method Specific Options:

Mode Superposition is the default method, and generally provides results faster than the Full method. In
the Mode Superposition method a modal analysis is first performed to compute the natural frequencies
and mode shapes. Then the mode superposition solution is carried out where these mode shapes are com-
bined to arrive at a solution.




Modal Frequency Range
  Specifies the range of frequencies over which mode shapes will be computed in the modal analysis:
       •   Program Controlled: The modal sweep range is automatically set to 200% of the upper harmonic
           limit and 50% of the lower harmonic limit. This setting is adequate for most simulations.
       •   Manual: Allows you to manually set the modal sweep range. Choosing Manual displays the Modal
           Range Minimum and Modal Range Maximum fields where you can specify these values.
Cluster Results and Cluster Number (Mode Superposition only)
    This option allows the solver to automatically cluster solution points near the structure’s natural frequen-
    cies ensuring capture of behavior near the peak responses. This results in a smoother, more accurate
    response curves.

      Cluster Number specifies the number of solutions on each side of a natural frequency. The default is
      to calculate four solutions, but you may specify any number from 2 to 20.

      Options:
       •   Solution Method = Mode Superposition
       •   Cluster Number = Yes

Solution Intervals = 15: Here 15 solutions are evenly spaced within the frequency range. Note how
the peak can be missed altogether.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
274                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                          Harmonic Response Analysis - Options Control Settings




Cluster = 5: Here 5 solutions are performed automatically on either side of each natural frequency
capturing the behavior near the peaks.




Store Results At All Frequencies
    Upon solution, harmonic environments store data specified in the Output Controls for all intervals in
    the frequency range. Consequently, seeking additional results at new frequencies will no longer force a
    solved harmonic environment to be resolved. This choice will lead to a better compromise between
    storage space (results are now stored in binary form in the RST file) and speed (by reducing the need
    to resort to the solver to supply new results).

   Should storage become an issue, you can set Store Results At All Frequencies to No to request that
   only minimal data be retained to supply just the harmonic results requested at the time of solution. This
   option is especially useful for Mode Superposition harmonic analyses with frequency clustering. It is
   unavailable for harmonic analyses solved with the Full method.

        Note

        With this option set to No, the addition of new frequency or phase responses to a solved
        environment will require a new solution. The addition of new contour results does not share
        this requirement; data from the closest available frequency will be displayed (the reported
        frequency is noted on each result). However, data at an even closer frequency may be obtained
        with a new solution as needed. Note that the values of frequency and type of contour results
        (displacement, stress or strain) at the moment of the solve determine the contents of the
        result file and the subsequent availability of data. Forethought on these choices can significantly
        reduce the need to re-solve an analysis.

Full Method Specific Options:

There are no special options for Full method.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               275
Using the Mechanical Application Features




Linear Buckling - Options Control Settings
Max Modes to Find: You need to specify the number of buckling load factors and corresponding buckling
mode shapes of interest. Typically only the first (lowest) buckling load factor is of interest.

Random Vibration - Options Control Settings
Number of Modes to Use
  Specifies the number of modes to use from the modal analysis. A conservative rule of thumb is to include
  modes that cover 1.5 times the maximum frequency in the PSD excitation table.
Exclude Insignificant Modes
   When set to Yes, allows you to not include modes for the mode combination as determined by the
   threshold value you set in the Mode Significant Level field. The default value of 0 means all modes are
   selected (same as setting Exclude Insignificant Modes to No) while a value of 1 means that no modes
   are selected. The higher the threshold is set, the fewer modes are selected for mode combination.

Response Spectrum - Options Control Settings
Number of Modes to Use
  Specify the number of modes to use from the modal analysis. It is suggested to have modes that span
  1.5 times the maximum frequency defined in input excitation spectrum.
Spectrum Type
   Specify either Single Point or Multiple Points. If two or more input excitation spectrums are defined
   on the same fixed degree of freedoms, use Single Point, otherwise use Multiple Points.
Modes Combination Type
  Specify a method to be used for response spectrum calculation. Choices are SRSS, CQC, and ROSE. In
  general, the SRSS method is more conservative than the other methods.

      The SRSS method assumes that all maximum modal values are uncorrelated. For a complex structural
      component in three dimensions, it is not uncommon to have modes that are coupled. In this case, the
      assumption overestimates the responses overall. On the other hand, the CQC and the ROSE methods
      accommodate the deficiency of the SRSS by providing a means of evaluating modal correlation for the
      response spectrum analysis. Mathematically, the approach is built upon random vibration theory assuming
      a finite duration of white noise excitation. The ability to account for the modes coupling makes the re-
      sponse estimate from the CQC and ROSE methods more realistic and closer to the exact time history
      solution.

Damping Controls
Damping is present in most systems and should be specified in a transient structural (MBD), transient
structural (ANSYS), harmonic response, random vibration, or response spectrum analysis. The following forms
of damping are available in the program:

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
276                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Analysis Data Management

 •   Alpha and Beta Damping (Rayleigh Damping). Beta damping defines the stiffness matrix multiplier for
     damping. You can input the value of beta damping directly or the value can be computed from a
     damping ratio at a specified frequency. You define beta damping in the Details view of the Analysis
     Settings object.

     The value of β is not generally known directly, but is calculated from the modal damping ratio, ξi. ξi is
     the ratio of actual damping to critical damping for a particular mode of vibration, i. If ωi is the natural
     circular frequency, then the beta damping is related to the damping ratio as β = 2 ξi/ωi . Only one value
     of β can be input in a step, so choose the most dominant frequency active in that step to calculate β.
 •   Material-Dependent Damping. You define material-dependent damping as a material property in Engin-
     eering Data.
 •   Constant Material Damping Coefficient - only applicable for harmonic response analyses. You define
     the constant material damping coefficient as a material property in Engineering Data.
 •   Constant Damping Ratio - only applicable for harmonic response, random vibration, and response
     spectrum analyses. This is the simplest way of specifying damping in the structure. If you set this in
     conjunction with beta damping, the effects are cumulative. You define the constant damping ratio in
     the Details view of the Analysis Settings object.
 •   Element Damping from Spring elements – only applicable for transient structural (MBD), transient
     structural (ANSYS), and harmonic response analyses. You define the element damping from spring ele-
     ments in the Details view of the Spring object.

Numerical damping, also referred to as amplitude decay factor (γ), controls numerical noise produced by
the higher frequencies of a structure. Usually the contributions of these high frequency modes are not ac-
curate and some numerical damping is preferable. A default value of 0.1 is used.

You can specify more than one form of damping in a model. The program will formulate the damping
matrix as the sum of all the specified forms of damping.

Visibility
Allows you to selectively display loads in the Graph window by choosing Display or Omit for each load.

Analysis Data Management
This grouping indicates where the solution files are located.

 •   Solver Files Directory: Indicates the location of the solution files for this analysis. The directory location
     is automatically determined by the program as detailed in File Management in the Mechanical Applica-
     tion (p. 435). You can change the default location in the Options dialog box under the Analysis Settings
     and Solution category.
 •   Future Analysis: Indicates if the results of this analysis will be used as a load or an initial condition in
     a subsequent analysis. Below are possible future analysis options for each analysis type. Refer to Define
     Initial Conditions (p. 13) for further details.
     –   Static Structural analysis
         ¡ Pre-Stressed Modal analysis
         ¡ Linear Buckling analysis
     –   Modal analysis
         ¡ Prerequisite for a random vibration (PSD) or response spectrum analysis.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       277
Using the Mechanical Application Features

 •    Scratch Solver Files Directory: This is a read-only indication of the directory where a solve “in progress”
      occurs. All files generated after the solution is done (including but not limited to result files) are then
      moved to the Solver Files Directory. The files generated during solves on My Computer or files reques-
      ted from RSM for postprocessing during a solve remain in the scratch directory. For example, an early
      result file could be brought to the scratch folder from a remote machine through RSM during postpro-
      cessing while solving. With the RSM method, the solve may even be computed in this folder (for example,
      using the My Computer, Background SolveProcess Settings). The Mechanical application maintains
      the Scratch Solver Files Directory on the same disk as the Solver Files Directory.

      The scratch directory is only set for the duration of the solve (with either My Computer or My Computer,
      Background). After the solve is complete, this directory is set to blank.

      The use of the Scratch Solver Files Directory prevents the Solver Files Directory from ever getting
      an early result file.
 •    Save Ansys DB: No (default) / Yes. Some Future Analysis settings will require the db file to be written.
      In these cases this field will be set to Yes automatically.
 •    Delete Unneeded File: Yes (default) / No. If you prefer to save all the solution files for some other use
      you may do so by setting this field to No.
 •    Nonlinear Solutions: Read only indication of Yes / No depending on presence of nonlinearities in the
      analysis.
 •    Solver Units: You can select one of two options from this field:
      –   Active System - This instructs the solver to use the currently active unit system (determined via the
          toolbar Units menu) for the very next solve.
      –   Manual - This allows the you to choose the unit system for the solver to use by allowing them access
          to the second field, "Solver Unit System".
 •    Solver Units System:
      –   If Active System is chosen for the Solver Units field, then this field is read only and displays the
          active system.
      –   If Manual is chosen for the Solver Units field, this field is a selectable drop down menu.
      –   If a Magnetostatic analysis is being performed, the field is read only because the only system available
          to solve the analysis is the mks system.
      –   If a Thermoelectric or Electric analysis is being performed, only mks and µmks systems can be selected
          because they are the only systems currently allowed for these analyses.

Applying Loads
All loads and supports are applicable to a 2-D or 3-D simulation except where noted in the description of
the specific load or support.

The following topics are addressed in this section
 Types of Loads and Conditions
 How to Apply Loads
 Remote Boundary Conditions
 Harmonic Loads
 Spatial Varying Loads and Displacements
 Tabular and Function Loads
 Imported Loads
 Resolving Thermal Boundary Condition Conflicts

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
278                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Magnetostatic Loads

Direction
Scope
Types of Supports

Types of Loads and Conditions
Inertial Loads
  Acceleration (p. 280)
  Standard Earth Gravity (p. 282)
  Rotational Velocity (p. 283)

Structural Loads
  Pressure (p. 284)
  Hydrostatic Pressure (p. 285)
  Force (p. 285)
  Remote Force
  Bearing Load (p. 288)
  Bolt Pretension
  Moment (p. 291)
  Generalized Plane Strain (p. 292)
  Line Pressure (p. 293)
  PSD Base Excitation (p. 293)
  RS Base Excitation (p. 294)
  Joint Load (p. 295)
  Imported Body Temperature (p. 297)
  Thermal Condition (p. 297)

Thermal Loads
  Temperature (p. 298)
  Convection (p. 298)
  Radiation (p. 300)
  Heat Flow (p. 300)
  Perfectly Insulated (p. 302)
  Heat Flux (p. 302)
  Internal Heat Generation (p. 303)
  Imported Heat Generation (p. 303)

Electric Loads
  Voltage (p. 303)
  Current (p. 304)

Magnetostatic Loads
  Electromagnetic Boundary Conditions and Excitations (p. 305)
  Magnetic Flux Boundary Conditions (p. 305)
  Conductor (p. 307)




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                              279
Using the Mechanical Application Features

CFD Loads
The following loads involve interactions between the Mechanical application and CFD.

   CFD Imported Pressure (p. 314)
   CFD Imported Temperature (p. 314)
   CFD Imported Convection (p. 314)

Interaction Loads
The following loads involve interactions between the Mechanical application and other products.

   Motion Load (p. 315)
   Fluid Solid Interface (p. 317)

Acceleration
Translational acceleration accounts for the structural effects of a constant linear acceleration.




 Translational acceleration vector

The global Acceleration load defines a linear acceleration of a structure in each of the global Cartesian axis
directions.

If desired, acceleration can be used to simulate gravity (by using inertial effects) by accelerating a structure
in the direction opposite of gravity (the natural phenomenon of ). That is, accelerating a structure vertically
upwards (+Y) at 9.80665 m/s2 (in metric units), applies a force on the structure in the opposite direction (-
Y) inducing gravity (pushing the structure back towards earth). Units are length/time2.

Alternatively, you can use the Standard Earth Gravity load to produce the effect of gravity. Gravity and Ac-
celeration are essentially the same type of load except they have opposite sign conventions and gravity has
a fixed magnitude. For applied gravity, a body tends to move in the direction of gravity and for applied ac-
celeration, a body tends to move in the direction opposite of the acceleration.

The illustrations shown below compare how Acceleration and Gravity can be used to specify a gravitational
load with the same result.

Acceleration Example




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
280                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                  Interaction Loads




Global Acceleration load applied in the +Y direction to simulate gravity.




Resulting deformation.

Standard Earth Gravity Example




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                            281
Using the Mechanical Application Features




Standard Earth Gravity applied.




Resulting deformation.

Define the Acceleration vector in terms of either:

 •    a magnitude and direction (based on selected geometry) [Define By: Vector]
 •    components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
      ents]

      Note

      While loads are associative with geometry changes, load directions are not. This applies to any
      load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and
      bearing load.

Standard Earth Gravity
Applies gravitational effects on a body in the form of an external force.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
282                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                          Interaction Loads




     Gravitational vector

 •     Define the vector in terms of any of the following directions in the world coordinate system or local co-
       ordinate system, if applied:+x, -x, +y, -y, +z, -z.
 •     Gravity is a specific example of acceleration with an opposite sign convention and a fixed magnitude.
       Gravity loads cause a body to move in the direction of gravity. Acceleration loads cause a body to move
       in the direction opposite of acceleration. Refer to the example shown under Acceleration (p. 280) for
       details.
 •     The magnitude is set: 9.80665 m/s2 (in metric units)
 •     The direction is changeable.
 •     The vector is added to acceleration when it is present.

Rotational Velocity
Rotational velocity accounts for the structural effects of a part spinning at a constant rate.

Define rotational velocity in terms of either:

 •     a magnitude and an axis of rotation (based on selected geometry) [Define By: Vector]
 •     a point and components (in the world coordinate system or local coordinate system, if applied) [Define
       By: Components]




     Magnitude

     Axis of rotation




     Point

     Vector

For 2-D axisymmetric simulations, a Rotational Velocity load can only be applied about the y-axis.




                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                        of ANSYS, Inc. and its subsidiaries and affiliates.                                            283
Using the Mechanical Application Features


        Note

        While loads are associative with geometry changes, load directions are not. This applies to any
        load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and
        bearing load.

Pressure
For 3-D simulations, a pressure load applies a constant pressure or a varying pressure in a single direction
(x, y, or z) to one or more flat or curved faces.

The following illustration applies to a constant pressure load:




     Uniform positive pressure

Define the vector as one of the following:

 •     the displacement constraint acting normal to the surface to which it is attached (essentially a frictionless
       support with a non-zero displacement) [Define By: Normal To]

       During a structural analysis, you can also create a spatially varying load using this vector type option.
       A spatially varying load allows you to define the pressure in tabular form or as a function.

       Applying a pressure load normal to faces (3-D) or edges (2-D) could result in a pressure load stiffness
       contribution that plays a significant role in a linear buckling analysis. This additional effect is computed
       during a buckling analysis using the pressure value in the static analysis at time = 0. Because of this, if
       you perform static analysis for a subsequent buckling analysis, you must apply pressure loads as a
       separate step in the static analysis.
 •     a magnitude and direction (based on selected geometry) [Define By: Vector]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

Pressure is uniform and acts normal to a face at all locations on the face. A positive value for pressure acts
into the face, compressing the solid body.

If you select multiple faces when defining the pressure, the same pressure value gets applied to all selected
faces.

If a constant pressurized face enlarges due to a change in CAD parameters, the total load applied to the
face increases, but the pressure (force per unit area) value remains constant.

For 2-D simulations, a pressure load applies a pressure to one or more edges.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
284                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Interaction Loads

Hydrostatic Pressure
A hydrostatic pressure load simulates pressure that occurs due to fluid weight.

Presented below is a typical procedure showing the use of a hydrostatic pressure load:

 1.   Define a Static Structural analysis system and import the fluid container model.
 2.   Double-click the Model cell to enter the Mechanical application, then choose a Hydrostatic Pressure
      load. See How to Apply Loads (p. 317).
 3.   Scope all faces that will potentially enclose the fluid.
 4.   Specify the Shell Face, defined as the side of the shell on which to apply the hydrostatic pressure
      load. (The Shell Face option appears only for surface bodies.)
 5.   Specify the magnitude and direction of the Hydrostatic Acceleration. This is typically the acceleration
      due to gravity, but can be other acceleration values depending on the modeling scenario. For example,
      if you were modeling rocket fuel in a rocket’s fuel tank, the fuel might be undergoing a combination
      of acceleration due to gravity and acceleration due to the rocket accelerating while flying.
 6.   Enter the Fluid Density.
 7.   Specify the Free Fluid Location, defined as the location of the top of the fluid in the container. You
      can specify this location by using coordinate systems, by entering coordinate values, or by clicking a
      location on the model.
 8.   Mesh the model, then highlight the Hydrostatic Pressure load object to display the pressure contours.

The following example shows the simulation of a hydrostatic pressure load on the wall of an aquarium. Here
the wall is modeled as a single surface body. The load is scoped to the bottom side of the face. A fixed
support is applied to the bottom edge. Acceleration due to gravity is used and the fluid density is entered
as 1000 kg/m3. Coordinates representing the top of the fluid are also entered.

Shown below is a load plot that clearly illustrates the hydrostatic pressure gradient.




Force
There are three types of forces:



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            285
Using the Mechanical Application Features

      Face (p. 286)
      Edge (p. 286)
      Vertex (p. 287)

Face
Distributes a force vector across one or more flat or curved faces.




     Force vector

     Resulting uniform traction across the face

Define the vector in terms of either:

 •     a magnitude and direction (based on selected geometry) [Define By: Vector]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

The force is applied by converting it to a pressure, based on the total area of all the selected faces.

If a face enlarges due to a change in CAD parameters, the total load magnitude applied to the face remains
constant.

If you try to apply a force to a multiple face selection that spans multiple parts, the face selection is ignored.
The geometry property for the load object displays 'No Selection' if the load was just created, or it maintains
its previous geometry selection if there was one.

Edge
Distributes a force vector along one or more straight or curved edges.




     Force vector

     Resulting uniform line load along the edge

Define the vector in terms of either:



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
286                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Vertex

 •     a magnitude and direction (based on selected geometry) [Define By: Vector]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

If you select multiple edges when defining the force, the magnitude of the force is distributed evenly across
all selected edges.

If an edge enlarges due to a change in CAD parameters, the total load applied to the edge remains constant,
but the line load (force per unit length) decreases.

A force applied to an edge is not realistic and leads to singular stresses (that is, stresses that approach infinity
near the loaded edge). You should disregard stress and elastic strain values in the vicinity of the loaded
edge.

If you try to apply a force to a multiple edge selection that spans multiple parts, the edge selection is ignored.
The geometry property for the load object displays 'No Selection' if the load was just created, or it maintains
its previous geometry selection if there was one.

Vertex
Applies a force vector to one or more vertices.




     Force vector

Define the vector in terms of either:

 •     a magnitude and direction (based on selected geometry) [Define By: Vector]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

If you select multiple vertices when defining the force, the magnitude of the force is distributed evenly
across all selected vertices.

A force applied to a vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity
near the loaded vertex). You should disregard stress and elastic strain values in the vicinity of the loaded
vertex.

While loads are associative with geometry changes, load directions are not. This applies to any load that
requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load.

If you try to apply a force to a multiple vertex selection that spans multiple parts, the vertex selection is ig-
nored. The geometry property for the load object displays 'No Selection' if the load was just created, or it
maintains its previous geometry selection if there was one.

Remote Force
A Remote Force is equivalent to a regular force load on a face or a force load on an edge, plus some moment.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                 287
Using the Mechanical Application Features

A Remote Force can be used as an alternative to building a rigid part and applying a force load to it. The
advantage of using a remote force load is that you can directly specify the location in space from which the
force originates.




You apply a Remote Force like you apply a force load except that the location of the load origin can be
replaced anywhere in space either by picking or by entering the XYZ locations directly. The default location
is at the centroid of the geometry. The location and the direction of a remote force can be defined in the
global coordinate system or in a local coordinate system.

A Remote Force can be applied to a face of a solid model, or to an edge or a face of a surface model.

While loads are associative with geometry changes, load directions are not. This applies to any load that
requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load.

A Remote Force is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 319)
section for a listing of all remote boundary conditions and their characteristics.

Bearing Load
Applies a variable distribution of force to one complete right cylinder in a 3-D simulation, or to a circular
edge in a 2-D simulation.

In a 3-D simulation, a complete right cylinder is capped on both ends by circles normal to the axis of the
cylinder.




 Load direction

 Radial component distribution

 Region of loaded cylinder not affected by radial distribution

You must apply a Bearing load in the cylinder's radial direction using local coordinate systems. If the
Mechanical application detects a portion of the load to be in the axial direction, the solver will block the
solve and issue an appropriate error message.

Define the vector in terms of either:


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
288                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Vertex

 •   a magnitude and direction (based on selected geometry) [Define By: Vector]
 •   components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
     ents]

If the loaded face enlarges (e.g., due to a change in parameters), the total load applied to the face remains
constant, but the pressure (force per unit area) decreases.

     Note

      •   While loads are associative with geometry changes, load directions are not. This applies to
          any load that requires a vector input, such as: moment, acceleration, rotational velocity, force,
          and bearing load.
      •   If your CAD system split the cylinder into two or more faces, select all of the faces when
          defining the bearing load.
      •   Use one bearing load per cylinder. Do not use multiple select to apply a bearing load to
          different cylinders. If you do, the load is divided among the multiple cylindrical faces by area
          ratio, as shown in the following example of a single bearing load applied to two cylinders.
          The length of the cylinder on the right is twice the length of the cylinder on the left. Note
          that the reactions are proportional to each cylinder's area as a fraction of the total load area.
      •   Although loading across multiple steps may appear as an application of tabular loading, you
          cannot set the magnitude of a bearing load in terms of either tabular or functional data. You
          must set a constant or ramped magnitude for each step such that one value corresponds to
          each step.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 289
Using the Mechanical Application Features

Bolt Pretension
Available for 3-D simulations only.

Applies a pretension load to a cylindrical face, to a single body, or to multiple bodies, typically to model a
bolt under pretension. If you apply the Bolt Pretension load to a body, you will need to have a local Co-
ordinate System object in the tree. The application of the load will be at the origin and along the z-axis of
the local coordinate system. You can place the coordinate system anywhere in the body and reorient the
z-axis.

Body scoping of a Bolt Pretension load can now be to more than one body. In this case all the scoped
bodies will be cut. There is still only a single Bolt Pretension load created but this feature allows you to
apply a bolt load to a bolt that has been cut into several bodies. This feature is illustrated in the following
figure.




This load is applicable to pure structural or thermal-stress analyses. You specify how the Bolt Pretension
load is applied by choosing one of the following options under the Define By setting in the Details view.

 •    Load: Applies a force as a preload. A Load field is displayed where you enter the value of the load in
      force units.
 •    Adjustment: Applies a length as a preadjustment (for example, to model x number of threads). An
      Adjustment field is displayed where you enter the value of the adjustment in length units.
 •    Lock: Fixes all displacements. You can set this state for any step except the first step.
 •    Open: Use this option to leave the Bolt Pretension load open so that the load has no effect on the
      applied step, effectively suppressing the load for the step. Note that in order to avoid convergence issues
      from having underconstrained conditions, a small load (0.01% of the maximum load across the steps)
      will be applied. You can set this state for any step.

Presented below is the same model showing a Bolt Pretension load as a preload force and as a preadjustment
length:




The following animation shows total deformation:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
290                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Limitations

The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the
help. Interface names and other components shown in the demo may differ from those in the released product.




Limitations
The following limitations apply to using Bolt Pretension loads:

 •   Do not try to preload a body more than once, that is, do not apply multiple Bolt Pretension loads to
     the same body, even at different locations.
 •   If you try to apply a preload on the same face more than once, all definitions except the first one are
     ignored.
 •   Be sure that a sufficiently fine mesh exists on a face or body that contains Bolt Pretension loads so
     that the mesh can be correctly partitioned along the axial direction (that is, at least 2 elements long).
 •   For simulating one Bolt Pretension through multiple split faces, you should apply only one Bolt Pre-
     tension load to one of the split faces, as the Bolt Pretension load will slice though the whole cylinder
     even though only part of the cylinder is selected.
 •   Care should be used when applying a Bolt Pretension load to a cylindrical face that has bonded contact.
     There is a possibility that if you apply a Bolt Pretension load to a cylinder that had a bonded contact
     region, the bonded contact will block the ability of the Bolt Pretension to deform properly.
 •   The Bolt Pretension load should be applied to cylindrical faces that contain the model volume (that
     is, do not try to apply the Bolt Pretension load to a hole).

Moment
Distributes a moment about an axis across one or more flat or curved faces, as illustrated below, or about
one or more edges or vertices.

Face and edge selections for the moment load can span multiple parts, however, multiple vertex selections
must be of the same part type (solid, 3D surface or line bodies) or the selection is ignored.

When specifying the Scoping Method, faces and edges can be scoped to either the geometry where the
load is to be applied (Geometry Selection), to a Named Selection, or to a Remote Point. Vertices cannot
be scoped to Remote Point.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      291
Using the Mechanical Application Features




     Load direction

     Moment load

     Affected face

Define the moment vector in terms of either:

 •     a magnitude and direction (based on selected geometry) [Define By: Vector]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

The moment is applied "about" the vector. Use the right-hand rule to determine the sense of the moment.

If you select multiple faces when defining the moment, the magnitude is apportioned across all selected
faces.

If a face enlarges (e.g., due to a change in parameters), the total load applied to the face remains constant,
but the load per unit area decreases.

        Note

        While loads are associative with geometry changes, load directions are not. This applies to any
        load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and
        bearing load.

A Moment is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 319)
section for a listing of all remote boundary conditions and their characteristics.

Generalized Plane Strain
Used in 2-D applications involving generalized plane strain behavior.

The Details view includes settings for controlling the items listed below. Refer to Using Generalized Plane
Strain (p. 97) for detailed information on these settings and on the overall application of this load.

 •     Setting the x and y coordinates of the reference (starting) point.
 •     Establishing the magnitude and boundary conditions of the fiber direction. Choices for the boundary
       condition are:
       –   Free
       –   Force
       –   Displacement
 •     Establishing the boundary conditions for rotation about the x-axis and the y-axis. Choices for the
       boundary conditions are:
       –   Free

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
292                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Limitations

     –   Moment
     –   Rotation

Specific reactions are also reported in the Details view of a Generalized Plane Strain probe after solving.

Line Pressure
For 3-D simulations, a line pressure load applies a distributed force on one edge only, using force density
loading in units of force per length. You can define the force density on the selected edge in various ways.




Define the load in terms of one of the following:

 •   a magnitude and direction (based on selected geometry) [Define By: Vector]
 •   components (in the world coordinate system or local coordinate system, if applied for both Cartesian
     and cylindrical coordinate systems) [Define By: Components]
 •   a magnitude and tangent. You can also apply time and spatially varying loads. [Define By: Tangential]

If a pressurized edge enlarges due to a change in CAD parameters, the total load applied to the edge increases,
but the pressure (force per unit length) remains constant.

PSD Base Excitation
PSD Base Excitation loads are used exclusively in random vibration analyses to provide excitation in terms
of spectral value vs. frequency to your choice of the supports that were applied in the prerequisite modal
analysis. The Boundary Condition setting in the Details view includes a drop down list where you can
specify any of the following supports for excitation that are defined in the modal analysis: Fixed Support,
Displacement, Remote Displacement, and Body-to-Ground Spring. If multiple fixed supports are defined
in the modal analysis, you can apply the excitation load to all fixed supports by choosing the All Fixed
Supports option.

     Note

     Only fixed degrees of freedom of the supports are valid for excitations.

You can also specify the excitation direction (X Axis, Y Axis, or Z Axis).

The user-defined PSD data table is created in the Tabular Data window. You can create a new PSD table
or import one from a library that you have created, via the fly-out of the Load Data option in the Details
view.

     Note

     Only positive table values can be input when defining this load.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      293
Using the Mechanical Application Features

When creating PSD loads for a Random Vibration analysis in the Mechanical application, Workbench evaluates
your entries by performing a "Goodness of Fit" to ensure that your results will be dependable.

Click the fly-out of the Load Data option and choose Improved Fit after entering data points for viewing
the graph and updating the table. Interpolated points are displayed if they are available from the goodness
of fit approximation. Once load entries are entered, the table provides one of the following color-code indic-
ators per segment:

 •    Green - Values are considered reliable and accurate.
 •    Yellow - This is a warming indicator. Results produced are not considered to be reliable and accurate.
 •    Red - Results produced are not considered trustworthy. If you choose to solve the analysis, the Mech-
      anical APDL application executes the action, however; the results are almost certainly incorrect. It is re-
      commended that you modify your input PSD loads prior to the solution process.

Four types of base excitation are supported:

 •    PSD Acceleration
 •    PSD G Acceleration
 •    PSD Velocity
 •    PSD Displacement

The direction of the PSD base excitation is defined in the nodal coordinate of the excitation points.

Multiple PSD excitations (uncorrelated) can be applied. Typical usage is to apply 3 different PSDs in the X,
Y, and Z directions. Correlation between PSD excitations is not supported.

RS Base Excitation
RS Base Excitation loads are used exclusively in response spectrum analyses to provide excitation in terms
of a spectrum. For each spectrum value, there is one corresponding frequency. Use the Boundary Condition
setting in the Details view to apply an excitation to all of the fixed supports that were applied in the pre-
requisite modal analysis.

      Note

      Only fixed DOFs of the supports are valid for excitations.

You can also specify the excitation in a given direction (X Axis, Y Axis, or Z Axis).

The user-defined RS data table is created in the Tabular Data window. You can create a new RS table or
import one from a library that you have created, via the fly-out of the Load Data option in the Details view.

      Note

      Only positive table values can be used when defining this load.

Three types of base excitation are supported:

 •    RS Acceleration
 •    RS Velocity


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
294                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Limitations

 •   RS Displacement

You should specify the direction of the RS base excitation in the global Cartesian system.

Multiple RS excitations (uncorrelated) can be applied. Typical usage is to apply 3 different RS excitations in
the X, Y, and Z directions. Correlation between RS excitations is not supported.

The following additional settings are included in the Details view of an RS Base Excitation load:

 •   Scale Factor: Scales the entire table of input excitation spectrum for a Single Point response spectrum.
     The factor must be greater than 0.0. The default is 1.0.
 •   Missing Mass Effect: Set to Yes to include the contribution of high frequency modes in the total response
     calculation. Including these modes is normally required for nuclear power plant design.

     The responses contributed by frequency modes higher than those of rigid responses, specifically frequency
     modes beyond Zero Period Acceleration (ZPA) are called residual rigid responses. The frequency modes
     beyond ZPA are defined as frequency modes at which the spectral acceleration returns to the Zero
     Period Acceleration. In some applications, especially in the nuclear power plant industry, it is critical
     and required to include the residual rigid responses to the total responses. Ignoring the residual rigid
     responses will result in an underestimation of responses in the vicinity of supports. There are two
     methods available to calculate residual rigid responses: the Missing Mass and Static ZPA methods. The
     Missing Mass method is named based on the fact that the mass associated with the frequency modes
     higher than that of ZPA are missing from the analysis. As a result, the residual rigid responses are
     sometimes referred to missing mass responses. When set to Yes, the Missing Mass Effect is used in a
     response spectrum analysis.
 •   Rigid Response Effect: Set to Yes to include rigid responses to the total response calculation. Rigid
     responses normally occur in the frequency range that is lower than that of missing mass responses, but
     higher than that of periodic responses.

     In many cases, it is impractical and difficult to accurately calculate all natural frequencies and mode
     shapes for use in the response spectrum evaluation. For high-frequency modes, rigid responses basically
     predominate. To compensate for the contribution of higher modes to the responses, the rigid responses
     are combined algebraically to the periodic responses, which occur in the low-frequency modes that are
     calculated using one the methods above. The most widely adopted methods to calculate the rigid re-
     sponses are the Gupta and Lindley-Yow methods. These two methods are available for a response
     spectrum analysis under Rigid Response Effect Type when Rigid Response Effect is set to Yes.

Joint Load
When you are using joints in a Transient Structural (ANSYS) or Transient Structural (MBD) analysis, you
use a Joint Load object to apply a kinematic driving condition to a single degree of freedom on a Joint
object. Joint Load objects are applicable to all joint types except fixed, general, universal, and spherical
joints. For translation degrees of freedom, the Joint Load can apply a displacement, velocity, acceleration,
or force. For rotation degrees of freedom, the Joint Load can apply a rotation, angular velocity, angular ac-
celeration, or moment. The directions of the degrees of freedom are based on the reference coordinate
system of the joint and not on the mobile coordinate system.

A positive joint load will tend to cause the mobile body to move in the positive degree of freedom direction
with respect to the reference body, assuming the mobile body is free to move. If the mobile body is not
free to move then the reference body will tend to move in the negative degree of freedom direction for the
Joint Load. One way to learn how the mechanism will behave is to use the Configure feature. For the joint
with the applied Joint Load, dragging the mouse will indicate the nature of the reference/mobile definition
in terms of positive and negative motion.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      295
Using the Mechanical Application Features

 To apply a Joint Load:
 1.     Highlight the Transient environment object and insert a Joint Load from the right mouse button
        context menu or from the Loads drop down menu in the Environment toolbar.
 2.     From the Joint drop down list in the Details view of the Joint Load, select the particular Joint object
        that you would like to apply to the Joint Load. You should apply a Joint Load to the mobile bodies
        of the joint. It is therefore important to carefully select the reference and mobile bodies while defining
        the joint.
 3.     Select the unconstrained degree of freedom for applying the Joint Load, based on the type of joint.
        You make this selection from the DOF drop down list. For joint types that allow multiple unconstrained
        degrees of freedom, a separate Joint Load is necessary to drive each one. Further limitations apply
        as outlined under Joint Load Limitations (p. 296) below. Joint Load objects that include velocity, accel-
        eration, rotational velocity or rotational acceleration are not applicable to static structural analyses.
 4.     Select the type of Joint Load from the Type drop down list. The list is filtered with choices of Displace-
        ment, Velocity, Acceleration, and Force if you selected a translational DOF in step 3. The choices are
        Rotation, Rotational Velocity, Rotational Acceleration, and Moment if you selected a rotational
        DOF.
 5.     Specify the magnitude of the Joint Load type selected in step 4 as a constant, in tabular format, or
        as a function of time using the same procedure as is done for most loads in the Mechanical application.
        Refer to How to Apply Loads (p. 317) for further information.

        On Windows platforms, an alternative and more convenient way to accomplish steps 1 and 2 above
        is to drag and drop the Joint object of interest from under the Connections object folder to the
        Transient object folder. When you highlight the new Joint Load object, the Joint field is already
        completed and you can continue at step 3 with DOF selection.

Joint Load Limitations
Some joint types have limitations on the unconstrained degrees of freedom that allow the application of
joint loads as illustrated in the following table:

           Joint Type                   Unconstrained Degrees of                          Allowable Degrees of Freedom for
                                               Freedom                                          Applying Joint Loads
Fixed                                  None                                               Not applicable
Revolute                               ROTZ                                               ROTZ
Cylindrical                            UZ, ROTZ                                           UZ, ROTZ
Translational                          UX                                                 UX
Slot                                   UX, ROTX, ROTY, ROTZ                               UX
Universal                              ROTX, ROTZ                                         None
Spherical                              ROTX, ROTY, ROTZ                                   None
Planar                                 UX, UY, ROTZ                                       UX, UY, ROTZ
General                                UX, UY and UZ, Free X, Free                        All unconstrained degrees of freedom
                                       Y, Free Z, and Free All
Bushing                                UX, UY, UZ, ROTX, ROTY,                            All unconstrained degrees of freedom
                                       ROTZ




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
296                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Joint Load Limitations


      Note

      Where applicable, you must define all three rotations for a Joint Load before proceeding to a
      solve.

Imported Body Temperature
When temperatures are transferred from one analysis to another with data transfer, an Imported Body
Temperature object is automatically inserted.

      Note
       •   Adaptive Convergence objects inserted under an environment that is referenced by a Im-
           ported Body Temperature object will invalidate the Imported Body Temperature object,
           and not allow a solution to progress.
       •   For a particular load step, an active Imported Body Temperature load will overwrite any
           Thermal Condition loads on common geometry selections.


Thermal Condition
You can insert a known temperature (not from data transfer) boundary condition in a Structural or Electric
analysis by inserting a Thermal Condition object and specifying the value of the temperature in the Details
view under the Magnitude property. If the load is applied to a surface body, by default the temperature is
applied to both the top and bottom surface body faces. You do have the option to apply different temper-
atures to the top and bottom faces by adjusting the Shell Face entry in the details view. When you apply
a thermal condition load to a solid body, the Shell Face property is not available in the Details view. You
can add the thermal condition load as time-dependent or spatially varying. To apply a thermal condition:

 1.   In the Project tree, right-click the environment folder, point to Insert, and then click Thermal Condition.
 2.   Select a surface body face, a solid body or a line body, and then click Apply in the Details view.
 3.   For surface bodies, in the Details view, click the Shell Face list, and then select Top, Bottom, or Both
      to apply the thermal condition to the selected face.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                                 297
Using the Mechanical Application Features


      Note
       •   When you have only one Thermal Condition load and you select only a top or bottom face,
           Workbench applies the environment temperature value to the opposite face unless it is
           otherwise specified from another load object.
       •   For an assembly of bodies with different topologies, you must define a separate Thermal
           Condition load for each topology, that is, you must define one load scoped to line bodies,
           define a second load scoped to surface bodies, and so on.
       •   For a particular load step, an active Imported Body Temperature load will overwrite any
           Thermal Condition loads on common geometry selections.

           Thermal Condition loads are written out to the solver for every step that the load is active.
           Deactivating the load at a step will delete the load if it was active at the previous step.

           For each load step, an active Thermal Condition load will overwrite other previously added
           Thermal Condition loads that are applied on common geometry selections.

           A deactivated Thermal Condition load that was active at the previous step will overwrite
           other previously added active Thermal Condition loads that are applied on common geometry
           selections.


Temperature
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.

You can apply a temperature load to one or more faces, edges, or vertices, as well as to an entire body.
When scoping a load to a body, you need to specify whether the temperature is applied to Exterior Faces
Only or to the Entire Body using the Apply To option. The same temperature value is applied when multiple
faces, edges, or vertices are selected.

You can also define a temperature load as a spatially varying load during a thermal analysis. A spatially
varying load allows you to vary the magnitude of a temperature in a single coordinate direction and as a
function of time using the Tabular Data or Function features. Please see the How to Apply Loads section
for the specific steps to apply tabular and/or function loads.

The following illustrate geometry selection for the temperature load.

      Curved Surface                               Edge                                                            Vertex




 Temperature

Convection
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
298                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            Convective Heat Transfer

Causes convective heat transfer to occur through one or more flat or curved faces (in contact with a fluid).




 Ambient fluid temperature.

 Film coefficient and Face Temperature.

The bulk fluid temperature is uniform and measured at a distance from the face outside of the thermal
boundary layer. The face temperature refers to the temperature at the face of the simulation model.

Film Coefficient
The film coefficient (also called the heat transfer coefficient or unit thermal conductance) is based on the
composition of the fluid in contact with the face, the geometry of the face, and the hydrodynamics of the
fluid flow past the face. It is possible to have a time or temperature dependent film coefficient. Refer to heat
transfer handbooks or other references to obtain appropriate values for film coefficient.

Coefficient Type
This field is available when the film coefficient is temperature dependent. Its value can be evaluated at the
average film temperature (average of surface and bulk temperatures), the surface temperature, the bulk
temperature, or the absolute value of the difference between surface and bulk temperatures.

     Note

     If you change the units from Celsius to Fahrenheit, or Fahrenheit to Celsius, when the convection
     coefficient type Difference between surface and bulk is in use, the displayed temperature values
     indicate a temperature difference only. The addition or subtraction of 32o for each temperature
     in the conversion formula offset one another. In addition, switching to or from the Difference
     between surface and bulk Coefficient Type option from any other option, clears the values in
     the Convection Coefficient table. This helps to ensure that you enter correct temperature values.

Ambient Temperature
The ambient temperature is the temperature of the surrounding fluid. It is possible to have a time dependent
ambient temperature.

Edit Tabular Data
This field is available when the Film Coefficient is temperature dependent and the Ambient Temperature is
time dependent. It allows you to switch the data being edited in the Tabular Data pane.

Convective Heat Transfer
Convection is related to heat flux by use of Newton's law of cooling:

q/A = h(ts - tf)

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                           299
Using the Mechanical Application Features

where

 •    q/A is heat flux out of the face (calculated within the application)
 •    h is the film coefficient (you provide)
 •    ts is the temperature on the face (calculated within the application)
 •    tf is the bulk fluid temperature (you provide)

When the fluid temperature exceeds face temperature, energy flows into a part. When the face temperature
exceeds the fluid temperature, a part loses energy.

If you select multiple faces when defining convection, the same bulk fluid temperature and film coefficient
is applied to all selected faces.

Radiation
Applies thermal radiation to a face of a 3-D model, or to an edge of a 2-D model. All the radiation energy
is exchanged with the Ambient Temperature, that is, the Form Factor1 is assumed to be 1.0.

You can set the following radiation properties in the Details view of a Radiation object:

 •    Emissivity: The ratio of the radiation emitted by a face to the radiation emitted by a black body at the
      same temperature.
 •    Ambient Temperature: The temperature of the surrounding space.

      Note
      1
       Radiation exchange between faces is restricted to gray-diffuse faces. Gray implies that emissivity
      and absorptivity of the face do not depend on wavelength (either can depend on temperature).
      Diffuse signifies that emissivity and absorptivity do not depend on direction. For a gray-diffuse
      face, emissivity = absorptivity; and emissivity + reflectivity = 1. Note that a black body face has
      a unit emissivity.

1 - Refer to the Radiation chapter in the Thermal Analysis Guide within the Mechanical APDL Help for more
information.

Heat Flow
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.

There are three types of Heat Flow Rates:

     Face Heat Flow Rate (p. 300)
     Edge Heat Flow Rate (p. 301)
     Vertex Heat Flow Rate (p. 301)

Face Heat Flow Rate
Specifies the rate of heat flow through one or more flat or curved faces.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
300                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Vertex Heat Flow Rate




 Positive heat flow

A positive heat flow acts into a face, adding energy to a body. Heat flow is defined as energy per unit time.

If you select multiple faces when defining the heat flow rate, the magnitude is apportioned across all selected
faces.

If a face enlarges due to a change in CAD parameters, the total load applied to the face remains constant,
but the heat flux (heat flow rate per unit area) decreases.

If you try to apply a heat flow to a multiple face selection that spans multiple bodies, the face selection is
ignored. The geometry property for the load object displays No Selection if the load was just created, or it
maintains its previous geometry selection if there was one.

Edge Heat Flow Rate
Specifies the rate of heat flow through one or more straight or curved edges.




 Positive heat flow

A positive heat flow acts into an edge, adding energy to a body. Heat flow is defined as energy per unit
time.

If you select multiple edges when defining the heat flow rate, the magnitude is apportioned across all selected
edges.

If an edge enlarges due to a change in CAD parameters, the total load applied to the edge remains constant,
but the line load (heat flow rate per unit length) decreases.

If you try to apply a heat flow to a multiple edge selection that spans multiple bodies, the edge selection
is ignored. The geometry property for the load object displays No Selection if the load was just created, or
it maintains its previous geometry selection if there was one.

Vertex Heat Flow Rate
Specifies the rate of heat flow through one or more vertices.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                                301
Using the Mechanical Application Features




 Positive heat flow

A positive heat flow acts into a vertex, adding energy to the body. Heat flow is defined as energy per unit
time.

If you select multiple vertices when defining the heat flow rate, the magnitude is apportioned among all
selected vertices.

If you try to apply a heat flow to a multiple vertex selection that spans multiple bodies, the vertex selection
is ignored. The geometry property for the load object displays No Selection if the load was just created, or
it maintains its previous geometry selection if there was one.

Perfectly Insulated
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.

Overrides or applies a "no load" insulated condition to a face.

An insulated face is a no load condition meant to override any thermal loads scoped to a body. The heat
flow rate is 0 across this face. This load is useful in a case where most of a model is exposed to a given
condition (such a free air convection) and only a couple of faces do not share this condition (such as the
base of a cup that is grounded). This load will override only thermal loads scoped to a body. See Resolving
Thermal Boundary Condition Conflicts for a discussion on thermal load precedence.

If you select multiple faces when defining an insulated face, all selected faces will be insulated.

Heat Flux
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.

Applies a uniform heat flux to one or more flat or curved faces.




 Uniform positive heat flux

A positive heat flux acts into a face, adding energy to a body. Heat flux is defined as energy per unit time
per unit area.

If you select multiple faces when defining the heat flux, the same value gets applied to all selected faces.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
302                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Vertex Heat Flow Rate

If a face enlarges due to a change in CAD parameters, the total load applied to the face increases, but the
heat flux remains constant.

Internal Heat Generation
Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only.

Applies a uniform generation rate internal to a body.

A positive heat generation acts into a body, adding energy to it. Heat generation is defined as energy per
unit time per unit volume.

If you select multiple bodies when defining the heat generation, the same value gets applied to all selected
bodies.

If a body enlarges due to a change in CAD parameters, the total load applied to the body increases, but the
heat generation remains constant.

     Note

     For a particular load step, an active Imported Heat Generation load will overwrite any Internal
     Heat Generation loads on common geometry selections.

     Internal Heat Generation loads are written out to the solver for every step that the load is active.
     Deactivating the load at a step will delete the load if it was active at the previous step.

     For each load step, an active Internal Heat Generation load will overwrite other previously added
     Internal Heat Generation loads that are applied on common geometry selections.

     A deactivated Internal Heat Generation load that was active at the previous step will overwrite
     other previously added active Internal Heat Generation loads that are applied on common geometry
     selections.

Imported Heat Generation
When Thermal Heat is transferred from one analysis to another with data transfer, an Imported Heat Gen-
eration object is automatically inserted.

Imported Heat Generation applies Joule heating from an Electric analysis in a Steady-State Thermal or
Transient Thermal analysis.

     Note
      •   The Joule heating resulting from limited contact electric conductance is ignored during this
          data transfer.
      •   For a particular load step, an active Imported Heat Generation load will overwrite any Internal
          Heat Generation loads on common geometry selections.


Voltage
Applies an electric potential to a body during an electric analysis, a thermal-electric analysis, or a magneto-
static analysis.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                                303
Using the Mechanical Application Features

For each analysis type, you define the voltage by magnitude and phase angle in the Details view, according
to the following equation.

V = Vocos(ωt+φ)

Vo is the magnitude of the voltage (input value Voltage), ω is the frequency, and φ is the phase angle. For
a static analysis, ωt = 0.

The voltage load can be defined as a constant, in tabular form, or as a mathematical function.

Electric and Thermal-Electric Analysis Requirements
During an Electric / Thermal-Electric Analysis, a voltage is applied to a face, edge, or vertex.

To apply a voltage load to a body, select Voltage from the Environment toolbar or right-click the mouse
on the environment object in the tree and select Insert>Voltage.

      Caution

      During an Electric / Thermal-Electric Analysis, voltage loads cannot be applied to a face, edge,
      or vertex that is shared with another voltage or current load or a Coupling.

Magnetostatic Analysis Requirements
See Voltage Excitation for Solid Source Conductors (p. 309).

Current
Applies an electric current to a body during an electric analysis, a thermal-electric analysis, or a magnetostatic
analysis.

For each analysis type, you define the current by magnitude and phase angle in the Details view, according
to the following equation.

I = Iocos(ωt+φ)

Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a
static analysis, ωt = 0.

The current load is defined as a constant, or in tabular form, or as a mathematical function.

For electric, thermal-electric, and magnetostatic analyses, current loads assume that the scoped entities are
equipotential, meaning they behave as electrodes where the voltage degrees of freedom are coupled and
solve for a constant potential.

Electric and Thermal-Electric Analysis Requirements
During an Electric / Thermal Analysis, a current is applied to a face, edge, or vertex of a body. It is assumed
that the material properties of the body provide conductance. An applied current assumes that the body
surfaces and edges are equipotential. A positive current applied to a face, edge, or vertex flows into the
body. A negative current flows out of the body. To apply a current load to a body for an Electric / Thermal
Analysis, select Current from the Environment toolbar or right-click the mouse on the environment object
in the tree and select Insert> Current.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
304                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Magnetostatic Analysis Requirements


     Caution

     Current loads cannot be applied to a face, edge, or vertex that is shared with another voltage or
     current load or a Coupling.

Magnetostatic Analysis Requirements
See Current Excitation for Solid Source Conductors (p. 310).

Electromagnetic Boundary Conditions and Excitations
You can apply electromagnetic excitations and boundary conditions when performing a Magnetostatic
analysis in the Mechanical application. A boundary condition is considered to be a constraint on the field
domain. An excitation is considered to be a non-zero boundary condition which causes an electric or mag-
netic excitation to the system. Boundary conditions are applied to the field domain at exterior faces. Excitations
are applied to conductors.

 •   Magnetic Flux Boundary Conditions (p. 305)
 •   Conductor (p. 307)
     –   Solid Source Conductor Body (p. 307)
         ¡ Voltage Excitation for Solid Source Conductors (p. 309)
         ¡ Current Excitation for Solid Source Conductors (p. 310)
     –   Stranded Source Conductor Body (p. 311)
         ¡ Current Excitation for Stranded Source Conductors (p. 312)

Magnetic Flux Boundary Conditions
Available for 3-D simulations only.

Magnetic flux boundary conditions impose constraints on the direction of the magnetic flux on a model
boundary. This boundary condition may only be applied to faces. By default, this feature constrains the flux
to be normal to all exterior faces.

Selecting Flux Parallel forces the magnetic flux in a model to flow parallel to the selected face. In the figure
below, the arrows indicate the direction of the magnetic flux. It can be seen that the flux flows parallel to
the xy plane (for any z coordinate).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 305
Using the Mechanical Application Features




A flux parallel condition is required on at least one face of the simulation model. It is typically applied on
the outer faces of the air body to contain the magnetic flux inside the simulation domain or on symmetry
plane faces where the flux is known to flow parallel to the face.

To set this feature, right-click on the Magnetostatic environment item in the tree and select Magnetic Flux
Parallel from the Insert context menu or click on the Magnetic Flux Parallel button in the toolbar. It can
only be applied to geometry faces and Named Selections (faces).




Half-symmetry model of a keepered magnet system. Note that the XY-plane is a Flux Parallel boundary. The
flux arrows flow parallel to the plane.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
306                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Magnetostatic Analysis Requirements

Half-symmetry model of a keepered magnet system. Note that the YZ-plane is a Flux Normal boundary. The
flux arrows flow normal to the plane. This is a natural boundary condition and requires no specification.

     Note

     Applying the flux parallel boundary conditions to the exterior faces of the air domain may artificially
     capture more flux in the simulation domain than what physically occurs. This is because the
     simulation model truncates the open air domain. To minimize the effect, ensure the air domain
     extends far enough away from the physical structure. Alternatively, the exterior faces of the air
     domain may be left with an unspecified face boundary condition. An unspecified exposed exter-
     ior face imposes a condition whereby the flux flows normal to the face. Keep in mind that at least
     one face in the model must have a flux parallel boundary condition.

Conductor
Available for 3-D simulations only.

A conductor body is characterized as a body that can carry current and possible excitation to the system.

Solid CAD geometry is used to model both solid source conductors and stranded source conductors. In
solid conductors, such as bus bars, rotor cages, etc., the current can distribute non-uniformly due to geometry
changes, hence the program performs a simulation that solves for the currents in the solid conductor prior
to computing the magnetic field.

Stranded source conductors can be used to represent wound coils. Wound coils are used most often as
sources of current excitation for rotating machines, actuators, sensors, etc. You may directly define a current
for each stranded source conductor body.

 •   Solid Source Conductor Body (p. 307)
 •   Stranded Source Conductor Body (p. 311)

Solid Source Conductor Body

This feature allows you to tag a solid body as a solid source conductor for modeling bus bars, rotor cages,
etc. When assigned as a solid source conductor, additional options are exposed for applying electrical
boundary conditions and excitations to the conductor. These include applying an electrical potential (voltage)
or current.

To set this condition, right-click the Magnetostatic environment object in the tree and select Source Con-
ductor from the Insert drop-down menu, or click on the Source Conductor button in the toolbar. Select
the body you want to designate as a conductor body, then use the Details view to scope the body to the
conductor and set Conductor Type to Solid. The default Number of Turns is 1, representing a true solid
conductor.

A solid source conductor can be used to represent a stranded coil by setting the Number of Turns to > 1.
The conductor still computes a current distribution according to the physics of a solid conductor, but in
many cases the resulting current density distribution will not significantly effect the computed magnetic
field results. This “shortcut” to modeling a stranded conductor allows you to circumvent the geometry re-
strictions imposed by the stranded conductor bodies and still obtain acceptable results.

After defining the conductor body, you may apply voltage and current conditions to arrive at the desired
state.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 307
Using the Mechanical Application Features


      Note

      Conductors require two material properties: relative permeability and resistivity. They also must
      not terminate interior to the model with boundary conditions that would allow current to enter
      or exit the conductor. Termination points of a conductor may only exist on a plane of symmetry.




      Only bodies can be scoped to a conductor. Solid conductor bodies must have at least one voltage
      excitation and either a second voltage excitation or a current excitation. Also, two solid conductor
      bodies may not 'touch' each other, i.e. they must not share vertices, edges, or faces.

To establish current in the conductor, you must apply excitation to at least two locations on the conductor,
typically at terminals. For example, you could

 •    apply a voltage drop at two terminals of a conductor body residing at symmetry planes.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
308                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Magnetostatic Analysis Requirements

 •   ground one end of a conductor (set voltage to zero) and apply the net current at the terminal's other
     end.




Voltage Excitation for Solid Source Conductors

This feature allows you to apply an electric potential (voltage) to a solid source conductor body. A voltage
excitation is required on a conductor body to establish a ground potential. You may also apply one to apply
a non-zero voltage excitation at another location to initiate current flow. Voltage excitations may only be
applied to faces of the solid source conductor body and can be defined as constant or time-varying.

To apply a voltage excitation to a solid source conductor body, right-click on the Conductor object under
the Magnetostatic environment object in the tree whose Conductor Type is set to Solid, and select Voltage
from the Insert drop-down menu, or click on the Voltage button in the toolbar.

You define the voltage by magnitude and phase angle in the Details view, according to the equation below.

V = Vocos(ωt+φ)

Vo is the magnitude of the voltage (input value Voltage), ω is the frequency, and φ is the phase angle. For
a static analysis, ωt = 0.

     Note

     Voltage excitations may only be applied to solid source conductor bodies and at symmetry planes.




An applied voltage drop across the terminals of a conductor body will induce a current. In this simple example,
the current in the conductor is related to the applied voltage drop, using the equations shown below. ∆V


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                 309
Using the Mechanical Application Features

= applied voltage drop, I = curent, ρ = resistivity of the conductor (material property), L = length of the
conductor, and Area = cross section area of the conductor.

∆V = IR

R = (ρ*L)/Area

Current Excitation for Solid Source Conductors

This feature allows you to apply a current to a solid source conductor or stranded source conductor body.
Use this feature when you know the amount of current in the conductor.

To apply a current excitation to a conductor body, right-click on the Conductor object under the Magneto-
static environment object in the tree whose Conductor Type is set to Solid, and select Current from the
Insert drop-down menu, or click on the Current button in the toolbar. A positive current applied to a face
flows into the conductor body. A negative current applied to a face flows out of the conductor body. For a
stranded source conductor, positive current is determined by the y-direction of a local coordinate system
assigned to each solid body segment that comprises the conductor.

You define the current by magnitude and phase angle in the Details view, according to the equation below.

I = Iocos(ωt+φ)

Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a
static analysis, ωt = 0.

      Note

      Current excitations may only be applied to a face of a solid source conductor body at symmetry
      planes. An excitation must be accompanied by a ground potential set at another termination
      point of the conductor body on another symmetry plane. No current may be applied to a con-
      ductor body face that is interior to the model domain. The symmetry plane on which the current
      excitation is applied must also have a magnetic flux-parallel boundary condition.




An applied current to a conductor face will calculate and distribute the current within the conductor body.
A ground potential (voltage = 0) must be applied to a termination point of the conductor body.

Both the applied current and voltage constraints must be applied at a symmetry plane.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
310                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Magnetostatic Analysis Requirements

Stranded Source Conductor Body

This feature allows you to tag solid multiple bodies as a stranded source conductor for modeling wound coils.
When assigned as a stranded source conductor, additional options are exposed for applying electric
boundary conditions and current excitation to the conductor.

Model a stranded source conductor using only isotropic materials and multiple solid bodies. Local coordinate
systems assigned to these bodies (via the Details view) are the basis for determining the direction of the
current that you later apply to a stranded source conductor. The model should include a separate solid body
to represent each directional “turn” of the conductor. Assign a local coordinate system to each body with
the positive current direction as the y-direction for each of the local coordinate systems. An illustration is
shown below.




After creating the body segments and assigning coordinate systems, right-click the Magnetostatic environ-
ment object in the tree and select Source Conductor from the Insert drop-down menu, or click on the
Source Conductor button in the toolbar. Select all body segments, then scope the bodies to the conductor
and, in the Details view, set Conductor Type to Stranded, then enter the Number of Turns and the Con-
ducting Area (cross section area of conductor). The stranded conductor is now ready for you to apply a
current. A step-by-step example is presented in the Current Excitation for Stranded Source Conductors (p. 312)
section.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                 311
Using the Mechanical Application Features


      Note

      Conductors require two material properties: relative permeability and resistivity. They also must
      not terminate interior to the model with boundary conditions that would allow current to enter
      or exit the conductor. Termination points of a conductor may only exist on a plane of symmetry.




Current Excitation for Stranded Source Conductors

Stranded source conductor bodies are applicable to any magnetic field problem where the source of excit-
ation comes from a coil. The coil must have a defined number of coil "turns." Stranded source body geometry
is limited to straight geometry or circular arc geometry sections with constant cross-section (see below)

Source loading for a coil is by a defined current (per turn) and a phase angle according to the equation
below.
I = Io cos(ωt + φ)

Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a
static analysis, ωt = 0. The direction of the current is determined by the local coordinate systems you assign
to each of the solid bodies that comprise the stranded source conductor. A positive or negative assigned
value of current will be respective to that orientation.

Use the following overall procedure to set up a Stranded Source Conductor and apply a current to the
conductor:



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
312                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Magnetostatic Analysis Requirements

1.   Define local coordinate systems that have the y-direction point in the direction of positive current
     flow.
     •   Use Cartesian coordinate systems for straight geometry sections and cylindrical coordinate systems
         for “arc” geometry sections.
2.   Assign a local coordinate system to each stranded source conductor body in the Details view of the
     body under the Geometry folder.




3.   Right-click on the Magnetostatic environment object in the tree and select Source Conductor from
     the Insert drop down menu, or click on the Source Conductor button in the toolbar.
     •   Scope the Source Conductor to all of the solid bodies.
     •   Set Conductor Type to Stranded.
     •   Enter the Number of Turns and Conducting Area for the conductor.

         For the Conducting Area, select a face that represents the conductor's cross-sectional area and
         read the surface area that displays in the Status Bar located at the bottom of the screen display.




         The Source Conductor graphic and Details view listing is shown below.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                 313
Using the Mechanical Application Features




 4.   Right-click on the Conductor object in the tree and select Current from the Insert drop down menu,
      or click on the Current button in the toolbar.
      •   Set Magnitude as constant or time-varying.
      •   Set Phase Angle.




          The Current automatically is scoped to the same bodies as the Source Conductor.

          The displayed current arrows give you visual validation that the current direction has been properly
          defined by the assigned local coordinate systems for each conductor body.

          Changing either the Type of Source Conductor or any coordinate system will invalidate the setup.

CFD Imported Pressure
When a CFD Pressure Load is applied from one analysis to another with data transfer, an Imported Pressure
object is automatically inserted to represent the transfer.

CFD Imported Temperature
When a CFD Imported Temperature load is applied from one analysis to another with data transfer, it is
automatically replaced with an Imported Temperature object.

CFD Imported Convection
When a CFD Imported Convection load is applied from one analysis to another with data transfer, it is
automatically replaced with an Imported Convection object.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
314                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                           Solving with Inertia Relief

Motion Load
The application interacts with motion simulation software such as Dynamic Designer™ from MSC, and Mo-
tionWorks from Solid Dynamics. This is not the motion feature that is built into the Mechanical application.
See the Transient Structural (MBD) Analysis (p. 84) and Transient Structural (ANSYS) Analysis (p. 76) sections
for information on the motion features built into the Mechanical application.

Motion simulation software allows you to define and analyze the motion in an assembly of bodies. One set
of computed results from the motion simulation is forces and moments at the joints between the bodies in
the assembly. See Inserting Motion Loads (p. 316) for the procedure on inserting these loads. These loads are
available for static structural analyses.

Single Body Capability
Insert Motion Loads is intended to work only with a single body from an assembly. If more than one body
is unsuppressed in the Model during Import, you will receive an error message stating that only one body
should be unsuppressed.

Frame Loads File
The application reads a text file produced by the motion simulation software. This file contains the load in-
formation for a single frame (time step) in the motion simulation. To study multiple frames, create multiple
environment objects for the Model and import each frame to a separate environment. The frame loads file
includes joint forces and inertial forces which "balance" the joint forces and gravity.

Inertial State
If the part of interest is a moving part in the assembly, the frame loads file gives the inertial state of the
body. This includes gravitational acceleration, translational velocity and acceleration, and rotational velocity
and acceleration. Of these inertial "loads" only the rotational velocity is applied in the environment. The re-
maining loads are accounted for by solving with inertia relief (see below).

If the part of interest is grounded (not allowed to move) in the motion simulation, corresponding supports
need to be added in the environment before solving.

Joint Loads
For each joint in the motion simulation, the frame loads file reports the force data - moment, force, and 3D
location - for the frame. Features are also identified so that the load can be applied to the appropriate face(s),
edge(s) or vertex(ices) within the application. These features are identified by the user in the motion simu-
lation software before exporting the frame loads file. For all nonzero moments and forces, a corresponding
"Moment" and "Remote Force" are attached to the face(s), edge(s) or vertex(ices) identified in the frame
loads file.

The Remote Force takes into account the moment arm of the force applied to the joint.

Solving with Inertia Relief
Inertia relief is enabled when solving an environment with motion loads. Inertia relief balances the applied
forces and moments by computing the equivalent translational and rotational velocities and accelerations.
Inertia relief gives a more accurate balance than simply applying the inertia loads computed in the motion
simulation.

Weak springs are also enabled. The computed reaction forces in the weak springs should be negligible.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                             315
Using the Mechanical Application Features

This option will automatically be turned on if you import any motion loads.

      Note

      Material properties have to be manually set to match density used in motion analysis.

Modifying Parts with Motion Loads
If you modify a part having a motion load, you should rerun the solution in the motion simulator software
(e.g., Dynamic Designer) and re-export the loads to the Mechanical application. Then, in the Mechanical
application, you must update the geometry, delete the load (from the Environment object) and re-insert
the motion load.

Modifying Loads
You can modify loads that have been inserted, but you should only do so with great care. Modifying loads
in the Mechanical application after importing from the motion simulation software will nullify the original
loading conditions sets in the motion simulation software. Therefore, you need to examine your results in
the Mechanical application carefully.

Inserting Motion Loads
You must make sure the files and data are up to date and consistent when analyzing motion loads. Use the
following procedure to ensure that the correct loads are applied for a given time frame.

 To insert motion loads after solving the motion simulation:
 1.   Advance the motion simulation to the frame of interest.
 2.   Export the frame loads file from the motion software.
 3.   Attach the desired geometry.
 4.   Choose any structural New Analysis type except Transient Structural (MBD) and Random Vibration.
 5.   Suppress all bodies except the one of interest.
 6.   Click the environment object in the tree, then right-click and select Insert> Motion Loads.
 7.   Select the Frame Load file that you exported from Dynamic Designer.
 8.   Click Solve. If more than one body is unsuppressed in the Model corresponding to the environment
      object, you will receive an error message at the time of solution stating that only one body should be
      unsuppressed.
 9.   View the results.

The exported loads depend on the part geometry, the part material properties, and the part's location relative
to the coordinate system in the part document. When any of these factors change, you must solve the motion
simulation again by repeating the full procedure. Verify that material properties such as density are consistent
in the motion simulation and in the material properties.

Insert Motion Loads is intended to work with a single body only. Results with grounded bodies (bodies not
in motion in the mechanism) are not currently supported.

If an assembly feature (such as a hole) is added after Dynamic Designer generates its Joint attachments for
FEA, the attachments may become invalid. These attachments can be verified by opening the Properties
dialog box for a Joint and selecting the FEA tab. An invalid attachment will have a red "X" through the icon.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
316                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     How to Apply Loads

To correct this problem, manually redefine the joint attachments using the FEA tab in the Joint Properties
dialog.

A .log file is created when motion loads are imported. This troubleshooting file has the same name (with
an .log extension) and file location as the load file. If the .log file already exists, it is overwritten by the new
file.

Fluid Solid Interface
A Fluid Solid Interface is used to apply loads from external field solvers like ANSYS CFX. These loads are
applicable on faces of solid or surface bodies in static structural and transient structural (ANSYS) analyses.
The integer Interface Number, found in the Details view, is incremented by default each time a new interface
is added. This value can be overridden if desired.

Once Fluid Solid Interfaces are identified, loads are transferred to and from body faces in the Mechanical
APDL model using the MFX variant of the ANSYS Multi-field solver (see “Chapter 4. Multi-field Analysis Using
Code Coupling” in the Coupled-Field Analysis Guide for details). This solver is accessed from either the
Mechanical APDL Product Launcher or CFX-Solver Manager, and requires both the Mechanical APDL and
CFX input files. To generate the Mechanical APDL input file, select the Solution object folder in the Mech-
anical Outline View, and then select Tools> Write Input File.... To generate the CFX input file, use the CFX
preprocessor, CFX-Pre.

Run time-monitoring is available in both the Mechanical APDL Product Launcher and CFX-Solver Manager.
Postprocessing of the Mechanical APDL results is available in the Mechanical application, and simultaneous
postprocessing of both the Mechanical APDL and CFX results is available in the CFX postprocessor, CFD-
Post.

How to Apply Loads
To apply a load, you must have an analysis type, existing load, support, or condition object selected in the
tree.

 To apply a load:
 1.   Select the appropriate geometry on the model and do one of the following:

      •    Click on the appropriate icon on the toolbar and choose the load.

      OR

      •    Click right mouse button, select Insert, and choose the load.

 2.   Go to the Details view and type in the appropriate values on any highlighted item, such as direction,
      magnitude, etc. See the Numeric Values section for more information about using expressions.

 To apply a tabular or function load:
 1.   Select the appropriate geometry on the model and do one of the following:

      •    Click on the appropriate icon on the toolbar and choose the load.

      OR

      •    Click right mouse button, select Insert, and choose the load.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                             317
Using the Mechanical Application Features

 2.   Go to the Details view and for loads that vary with temperature (Convections) or time (Load Histories)
      under Magnitude, click on the flyout field to classify the load as either Tabular (Time) or Function.

      •    You can enter tabular data, that is, load versus time in the Tabular Data window.
      •    You can type in a function such as "=1000*sin(10*time)" in the Magnitude field. Any time values
           that you are evaluating can exceed the final time value by as much as one time step. See the Nu-
           meric Values section for more information on available functions.

 3.   The Graph window displays the variation of load with time.
 4.   Annotations in the Geometry window display the current time in the Graph window along with the
      load value at that time.

 To import a load history from a library:
 1.   Select the appropriate geometry on the model and do one of the following:

      •    Click on the appropriate icon on the toolbar and choose the load.

      OR

      •    Click right mouse button, select Insert, and choose the load.

 2.   Go to the Details view and under Magnitude, click on the flyout field and choose Import....
 3.   Choose the desired load history if it is listed, then click OK. If it is not listed, click the Add... button,
      choose a load history or Browse... to one that is stored, then click OK in both dialog boxes.

 To export a load history:

 By default, any load history that you create in the Mechanical application remains in the Mechanical applic-
 ation. To save the load history (table or function) for future use:

 1.   Create a load history using the Graph or Tabular Data windows.
 2.   Go to the Details view and under Magnitude, click on the flyout field, choose Export, and save the
      file to a specific loaction.

 To activate or deactivate a load in a stepped analysis:
 1.   Highlight the load within a step in the Graph or a specific step in the Tabular Data window.
 2.   Click the right mouse button and choose Activate/Deactivate at this step!.

      Refer to Activation/Deactivation of Loads Within a Step (p. 268) for further details.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
318                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Remote Boundary Conditions


     Note

     Keep in mind the following:

      •   The Tabular and Function Loads (p. 324) section includes a listing of loads that can be applied
          as functions or in tabular format.
      •   Tables or functions defined in the Mechanical application for a load can be stored in a library
          for use in other Mechanical projects by choosing {fly-out}> Export.
      •   You can also import tabular or function load histories from an existing library into the
          Mechanical application by activating the flyout menu in the data input fields.
      •   You can use the The Mechanical Wizard (p. 112) to walk through these steps.


For most loads, the Details view includes settings for you to specify the Scoping Method to either the
geometry where the load is to be applied (Geometry Selection) or to a Named Selection. If you want to
move a load from one part of a model to another, click the Geometry field, click on the new model location,
then click Apply.

Loads that require you to define an associated direction include the Define By Details view control. Setting
Define By to Vector allows you to define the direction graphically, based on the selected geometry. Setting
Define By to Components allows you to define the direction by specifying the x, y, and z magnitude com-
ponents of the load.

     Note

     If you switch the load direction setting in the Define By field, the data is lost.


Remote Boundary Conditions
The following are classified as remote boundary conditions. These boundary conditions are considered as
”abstract” entities as opposed to boundary conditions that can be applied directly to the nodes or elements
of a solid model. You can scope the remote boundary conditions to a remote point using Promote Remote
Point in the RMB menu.

 •   Point Mass
 •   Springs
 •   Joints
 •   Remote Displacement
 •   Remote Force
 •   Moment

Presented below is an example showing a Remote Displacement:




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     319
Using the Mechanical Application Features




Remote boundary conditions have the following characteristics:

 •    All remote boundary conditions make use of MPC contact used in the Mechanical APDL application.
      See the Surface-Based Constraints section in the Contact Technology Guide - part of the Mechanical APDL
      Help, for more information.
 •    You are advised to check reaction forces to ensure that a remote boundary condition has been fully
      applied, especially if the boundary condition shares geometry with other remote boundary conditions,
      any type of constraint, or even MPC contact.
 •    You can set the geometry Behavior as Rigid or Deformable, as described and illustrated below.
 •    All remote boundary conditions are associative, meaning they remember their connection to the geo-
      metry. Their location however does not change. If you want the location to be associative, create a co-
      ordinate system on the particular face and set the location to 0,0,0 in that local coordinate system.
 •    Remote boundary conditions scoped to a large number of elements can cause the solver to consume
      excessive amounts of memory. Point masses in an analysis where a mass matrix is required and analyses
      that contain remote displacements are the most sensitive to this phenomenon. If this situation occurs,
      consider modifying the Pinball setting to reduce the number of elements included in the solver. Forcing
      the use of an iterative solver may help as well. Refer to the troubleshooting section for further details.

Geometry Behavior
You can specify the Behavior of the scoped geometry for a remote boundary condition in the Details view
as either Rigid or Deformable. This option dictates the behavior of the attached geometry. Rigid behavior
will not allow the scoped geometry to deform whereas Deformable behavior will allow it. You must determine
which Behavior best represents the actual loading. Note that this option has no effect if the boundary
condition is scoped to a Rigid Body in which case a Rigid behavior is always used. Presented below are ex-
amples of the Total Deformation resulting from the same Remote Displacement first using a Rigid formu-
lation, then using a Deformable formulation.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
320                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Harmonic Loads




     Note

     To apply a remote boundary condition scoped to a surface more than once (for example, two
     springs), you must do one of the following:

      •   Set scoped surface Behavior to Deformable.
      •   Change scoping to remove any overlap.
      •   Leverage the Pinball Region option (for Springs).


Harmonic Loads
You can use the following loads in a harmonic analysis:

   Acceleration
   Pressure
   Force (applied to a face, edge, or vertex)
   Bearing load
   Moment
   Given (Specified) displacement
   Remote Force

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         321
Using the Mechanical Application Features

     Remote Displacements

You can apply multiple loads to the same face. The following restrictions apply to harmonic loads:

 •    All loads must be sinusoidally time-varying.
 •    All loads must have the same frequency.
 •    No nonlinearities are permitted.
 •    Transient effects are not calculated.
 •    Thermal loads are not supported.

To apply a harmonic load, select Harmonic from the New Analysis drop-down menu on the Standard
Toolbar and then choose a load. For pressures, forces (vertex, edge, or face), and given (specified) displace-
ments, you can set the Phase Angle.




Spatial Varying Loads and Displacements
A spatially varying load has a variable magnitude in a single coordinate direction (x, y, or z). The following
load types qualify as varying loads and can be a function of time as well.

 •    Pressure - in a Normal direction only during a structural analysis
 •    Line Pressure - in a Tangential direction only during a structural analysis
 •    Temperature - during a thermal analysis
 •    Thermal Condition - during a structural analysis

For spatial varying loads, the spatial independent variable uses the origin of the coordinate system for its
calculations and therefore it does not affect the direction of the load.

To apply a spatial varying load, scope the Magnitude of the load as either Tabular or Function in the Details
view. See below for the specific scoping requirements.

Spatial Load Tabular Data
Selecting Tabular as the Magnitude option displays the Tabular Data and Graph Controls categories in
the Details view.

The Tabular Data category provides the following options:

 •    Independent Variable - specifies how the load varies, with Time (default), or in the X, Y, or Z spatial
      direction.
 •    Coordinate System - choose an existing coordinate system.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
322                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Spatial Varying Displacements

The Graph Controls category provides the option for the X-Axis. Use this option to change the Graph
window’s display to either Time or to the spatial direction specified in the Independent Variable field.
When the X-Axis field is defined as Time:

 •   Tabular Data content can be scaled against time.
 •   You can activate and deactivate the load at a solution load step.

Please see the How to Apply Loads section to additional information on the steps to apply loads.

Spatial Load Function Data
Selecting Function as the Magnitude option in the Details view presents an editable function field. Enter
a mathematical expression in this field. Expressions have the following requirements:

 •   For a Pressure load, the Define By option must be set to Normal To.
 •   You can use the spatial variation independent variables x, y, or z, and “time” (entered in lowercase) in
     the definition of the function.
 •   Define only one direction, x, y, or z after entering a direction, the Graph Controls category (see above)
     displays.

When the Details view property Magnitude is set to Function, the following categories automatically display.

 •   Function - properties include:
     –   Unit System – the active unit system.
     –   Angular Measure – the angular measure that is used to evaluate trigonometric functions.
 •   Graph Controls - based of the defined function, properties include:
     –   X-Axis – This provides options to display time or the spatial independent variable in the graph.
         When set to Time you can activate and deactivate the load at a solution step.
     –   Alternate Value – If the function combines time and a spatial independent variable, one of these
         values (alternate) must be fixed to evaluate the function for the two dimensional graph.
     –   Range Minimum – If the X-Axis property is set to a spatial independent variable, this is the minimum
         range of the graph. For time, this value defaults to 0.0 and cannot be modified.
     –   Range Maximum – If the X-Axis property is set to a spatial independent variable, this is the maximum
         range of the graph. For time this defaults to the analysis end time and can’t be modified.
     –   Number of Segments - The function is graphed with a default value of two hundred line segments.
         This value may be changed to better visualize the function.

Spatial Varying Displacements
You can also apply spatial varying displacements, which have the following additional or unique character-
istics:

 •   Edge scoping is available.
 •   Displacements are shown as vectors instead of contours except if you choose Normal To the surface.
     Vectors are only displayed if the model has been meshed. The vector arrows are color-coded to indicate
     their value. A contour band is included for interpretation of the values. The contour band is the vector
     sum of the possible three vector components and therefore will only display positive values.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       323
Using the Mechanical Application Features

 •    For one Displacement object, you can select up to three displacement components that can all vary
      using the same direction. If an additional direction is required, you can use an additional Displacement
      object.
 •    A constant value and a table cannot be used in different components. A table will be forced in any
      component having a constant value if another component has a table.

Please see the How to Apply Loads section to additional information on the steps to apply loads.

Tabular and Function Loads
You can enter the following loads and supports in tabular form or as a mathematical function:

Structural Tabular and Function Loads
 •    Acceleration
 •    Rotational Velocity
 •    Pressure
 •    Force
 •    Remote Force
 •    Moment
 •    Line Pressure
 •    Thermal Condition
 •    Joint Load
 •    Displacement
 •    Remote Displacement
 •    Velocity
 •    Fixed Rotation
 •    RS Base Excitation (RS Acceleration, RS Velocity, RS Displacement) - entry in tabular form only.
 •    PSD Base Excitation (PSD G Acceleration, PSD Acceleration, PSD Velocity, PSD Displacement) - entry in
      tabular form only.

Thermal Tabular and Function Loads
 •    Temperature
 •    Convection Coefficient
 •    Heat Flow
 •    Heat Flux
 •    Internal Heat Generation

Electromagnetic Tabular and Function Loads
 •    Voltage
 •    Current



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
324                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Imported Loads

Refer to the appropriate procedure under the How to Apply Loads (p. 317) section and the Numeric Values (p. 137)
section for more information.

Imported Loads
You can import results from one analysis and apply them as loads for a structural, thermal, electric or thermal-
electric analysis with data transfer. Using this feature you can include the loads from a CFD analysis, thermal
or thermal-electric analysis in the structural, thermal, electric, or thermal-electric analysis environments. The
following table shows valid environment interaction to import loads for an analysis with data transfer.

From                       To
CFD Pressure               Static Structural, Transient Structural, Shape Optimization
CFD Temperature            Steady State Thermal, Transient Thermal, Thermal - Electric
CFD Convection             Steady State Thermal, Transient Thermal, Thermal - Electric
Steady-State Thermal       Static Structural, Transient Structural, Shape Optimization, Electric
Transient Thermal          Static Structural, Transient Structural, Shape Optimization, Electric
Thermal-Electric           Static Structural, Transient Structural, Shape Optimization
Electric                   Steady State Thermal, Transient Thermal

You can work with imported loads only when you perform an analysis with data transfer. To import loads
for an analysis:

 1.   In the Project Schematic, add an appropriate analysis with data transfer to create a link between the
      solution of a previous analysis and the newly added analysis.
 2.   Attach geometry to the analysis system, and then double-click Setup to open the Mechanical window.
      A Imported Load folder is added under the environment folder, by default.
 3.   To add an imported load, click the Imported Load folder to make the Environment toolbar available
      or right mouse click on the Imported Load folder and select the appropriate load from the context
      menu.
 4.   On the Environment toolbar, click Imported Loads, and then select an appropriate load.
 5.   Select appropriate geometry, and then click Apply.
 6.   For CFD loads, select appropriate options in the Details view.

      a.   For CFD Pressure, in the Details view, under Transfer Definition, click the Surface list, and then
           select the corresponding surface.
      b.   For CFD Convection loads only: Select the appropriate Ambient Temperature Type.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                         325
Using the Mechanical Application Features


                  Note

                  CFD Near-Wall Ambient (bulk) Temperature (default): This option uses the fluid
                  temperature in the near-wall region as the ambient temperature for the film coefficient
                  calculation. This value will vary along the face.

                  Constant Ambient Temperature: This constant value applies to the entire scoped
                  face(s). The film coefficient will be computed based on this constant ambient temper-
                  ature value. Use of a constant ambient temperature value in rare cases may produce
                  a negative film coefficient if the ambient temperature is less than the local face tem-
                  perature. If this is the case, you can define a Supplemental Film Coefficient. This value
                  will be used in place of the negative computed film coefficient and the ambient tem-
                  perature adjusted to maintain the proper heat flow.



 7.     Under Worksheet, select the source time, for the imported load. You can also change the Analysis Time
        and if available, specify Scale and Offset values for the imported loads.
 8.     In the Project tree, right-click the imported load, and then click Import Load to import the load. When
        the load has been imported successfully, a contour plot will be displayed in the Geometry window.

       Note
        •   For structural analysis with data transfer, Imported Pressure or Imported Thermal Condition
            is added, by default.
        •   The Analysis Time must match the end time of one of the steps if you are using ANSYS
            solver.
        •   Convergence is not supported for environments with imported loads.


Resolving Thermal Boundary Condition Conflicts
Conflicts between boundary conditions scoped to parts and individual faces
Boundary conditions applied to individual geometry faces always override those that are scoped to a part(s).
For conflicts associated with various boundary conditions, the order of precedence is as follows:

 1.     Applied temperatures (Highest).
 2.     Convection, heat fluxes, and flows (Cumulative, but overridden by applied temperatures).
 3.     Insulated (Lowest. Overridden by all of the above).

Direction
There are four types of Direction:

      Planar Face (p. 327)
      Edge (p. 327)
      Cylindrical Face or Geometric Axis
      Two Vertices (p. 328)



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
326                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                 Cylindrical Face or Geometric Axis

Planar Face




  Selected planar face. The load is directed normal to the face.

     Note

     Not applicable to rotational velocity. Rotational velocity gets aligned along the normal to a planar
     face and along the axis of a cylindrical face.

Edge
Straight                                Colinear to the edge

Circular or Elliptical                  Normal to the plane containing the edge




  Selected straight edge

Cylindrical Face or Geometric Axis
Applies to cylinders, cones, tori, and cylindrical or conical fillets




  Selected cylinder




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                       327
Using the Mechanical Application Features

Two Vertices




  2 selected vertices

      Note

      Hold the CTRL key to select the second vertex.


Scope
Scope refers to geometry over which load/support applies. If you apply a force of 1000N in the X-direction,
applied to a vertex, the load is "scoped" to that vertex. You can "scope" that load to some other geometry
such as a face.

Environment objects in general can be scoped (such as force, pressure, temperature) to geometry that you
select, or to a named selection. Some environment objects, such as acceleration, cannot be scoped.

Shared faces exist in the case of multibody parts. Contact regions, pressures, surface body forces, surface
body moments, compression only supports, bearing loads, remote forces, convections, heat fluxes, and heat
flows are not allowed to be applied to shared faces.

Types of Supports
Fixed
   Fixed Face (p. 329)
   Fixed Edge (p. 329)
   Fixed Vertex (p. 330)

Displacement
   Displacement for Faces (p. 330)
   Displacement for Edges (p. 331)
   Displacement for Vertices (p. 332)
   Remote Displacement (p. 333)

Velocity
Velocity (p. 334)

Frictionless
   Frictionless Face (p. 334)




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
328                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Explicit Dynamics

Compression
Compression Only Support

Cylindrical
Cylindrical Support

Simply Supported
   Simply Supported Edge (p. 336)
   Simply Supported Vertex (p. 336)

Fixed Rotation
   Fixed Rotation

Elastic
Elastic Support (p. 338)

Coupling
Coupling (p. 338)

Explicit Dynamics
Impedance Boundary

Fixed Face
Prevents one or more flat or curved faces from moving or deforming.




 Immobilized face

Fixed Edge
Prevents one or more straight or curved edges from moving or deforming.




 Immobilized edge (e.g., of a bolt hole)




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            329
Using the Mechanical Application Features

A fixed edge is not realistic and leads to singular stresses (that is, stresses that approach infinity near the
fixed edge). You should disregard stress and elastic strain values in the vicinity of the fixed edge.

Fixed Vertex
Prevents one or more vertices from moving.




 Immobilized vertex

A fixed vertex fixes both translations and rotations on faces or line bodies.

A fixed vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity near the
fixed vertex). You should disregard stress and elastic strain values in the vicinity of the fixed vertex.

If you are using a surface body model, see Simply Supported Vertex (p. 336).

Displacement for Faces
Requires one or more flat or curved faces to displace relative to their original location by one or more
components of a displacement vector in the world coordinate system or local coordinate system, if applied.

      Note

      In a cylindrical coordinate system X, Y, and Z are used for R, Θ, and Z directions. When using a
      cylindrical coordinate system, non-zero Y displacements are interpreted as translational displace-
      ment quantities, ∆Y = R∆Θ. Since they are treated as linear displacements it is a reasonable ap-
      proximation only, for small values of angular motion ∆Θ.




  Nonzero X-, Y-, and Z-components. The face retains its original shape but moves relative to its original
location by the specified displacement vector. The enforced displacement of the face causes a model to
deform.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
330                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                           Displacements in a Stepped Analysis

     Zero Y-component. No part of the face can move, rotate, or deform in the Y-direction.

     Blank (undefined) X- and Z-components. The surface is free to move, rotate, and deform in the XZ plane.

Use multiple select to apply a displacement load to more than one surface.

Define the vector in terms of either:

 •     the displacement constraint acting normal to the surface to which it is attached (essentially a frictionless
       support with a non-zero displacement) [Define By: Normal To]
 •     components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
       ents]

        Note
         •   Entering a zero for a component prevents deformation in that direction.
         •   Entering a blank for a component allows free deformation in that direction.
         •   Avoid using multiple Displacements on the same face and on faces having shared edges.


Displacements in a Stepped Analysis
In a stepped analysis, you can vary both the degrees of freedom and component values for each step. It is
important to keep in mind that the orientation of the nodal coordinate system is modified to best suit the
applied displacements in the first step. By choosing an optimal configuration, the coordinate system will
prevent overconstraint, while specifying the displacement boundary conditions correctly. This configuration
may not be optimal for arbitrary displacement constraints in later steps. Furthermore, the orientation of the
nodal coordinate system is also affected by other constraints such as supports (fixed, simple, frictionless and
cylindrical), as well as symmetry.

Displacement for Edges
Requires one or more flat or curved edges to displace relative to their original location by one or more
components of a displacement vector in the world coordinate system or local coordinate system, if applied.

        Note

        In a cylindrical coordinate system X, Y, and Z are used for R, Θ, and Z directions. When using a
        cylindrical coordinate system, non-zero Y displacements are interpreted as translational displace-
        ment quantities, ∆Y = R∆Θ. Since they are treated as linear displacements it is a reasonable ap-
        proximation only, for small values of angular motion ∆Θ.




  Nonzero X-, Y-, and Z-components . The edge retains its original shape but moves relative to its original
location by the specified displacement vector. The enforced displacement of the edge causes a model to
deform.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                   331
Using the Mechanical Application Features




 Zero Y-component . No part of the edge can move, rotate, or deform in the Y-direction .

 Blank (undefined) X- and Z-components. The edge is free to move, rotate, and deform in the XZ plane.

Use multiple select to apply a displacement load to more than one edge.

      Note
       •   Entering a zero for a component prevents deformation in that direction.
       •   Entering a blank for a component allows free deformation in that direction.
       •   Avoid using multiple Displacements on the same edge and on edges having shared vertices.


Enforced displacement of an edge is not realistic and leads to singular stresses (that is, stresses that approach
infinity near the loaded edge). You should disregard stress and elastic strain values in the vicinity of the
loaded edge.

Displacement for Vertices
Requires one or more vertices to displace relative to their original location by one or more displacement
vector components in the world coordinate system or in an applied local coordinate system.

      Note

      In a cylindrical coordinate system X, Y, and Z are used for R, Θ, and Z directions. When using a
      cylindrical coordinate system, non-zero Y displacements are interpreted as translational displace-
      ment quantities, ∆Y = R∆Θ. Since they are treated as linear displacements it is a reasonable ap-
      proximation only, for small values of angular motion ∆Θ.




  Nonzero X-, Y-, and Z-components. The vertex moves relative to its original location by the specified dis-
placement vector. The enforced displacement of the vertex causes a model to deform.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
332                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                         Displacements in a Stepped Analysis




 Zero Y-component. The vertex cannot move in the Y-direction.

 Blank (undefined) X- and Z-components. The vertex is free to move in the XZ plane.

Use multiple select to apply a displacement load to more than one vertex.

     Note
      •   Entering a zero for a component prevents deformation in that direction.
      •   Entering a blank for a component allows free deformation in that direction.
      •   Avoid using multiple Displacements on the same vertex.


Enforced displacement of a vertex is not realistic and leads to singular stresses (that is, stresses that approach
infinity near the loaded vertex). You should disregard stress and elastic strain values in the vicinity of the
loaded vertex.

Remote Displacement
A Remote Displacement allows you to apply both displacements and rotations at an arbitrary remote location
in space. You specify the origin of the remote location under Scope in the Details view by picking, or by
entering the XYZ coordinates directly. The default location is at the centroid of the geometry. You specify
the displacement and rotation under Definition.

The location and the direction of a Remote Displacement can be defined in the global coordinate system
or in a local Cartesian coordinate system. A common application is to apply a rotation on a model at a
local coordinate system. An example is shown below along with a plot of the resulting Total Deformation.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   333
Using the Mechanical Application Features




A Remote Displacement is classified as a remote boundary condition. Refer to the Remote Boundary Condi-
tions (p. 319) section for a listing of all remote boundary conditions and their characteristics.

      Note

      For a modal analysis, only zero magnitude Remote Displacement values are valid. These function
      as supports. If non-zero magnitude remote displacements are needed for a pre-stress modal
      analysis, apply the Remote Displacement in the static structural environment.

Velocity
Apply a Velocity support to faces, edges, vertices, or bodies. Once geometry specifications are complete,
define the vector for this support in terms of either:

 •    components (in the world coordinate system or local coordinate system, if applied) [Define By: Compon-
      ents]. When defined by components, the following options are available for the component values.
      –   Constant
      –   Tabular
      –   Function
      –   Free (default)

      See the How to Apply Loads section of the Mechanical Help for additional information.
 •    the velocity constraint acting normal to the surface to which it is attached [Define By: Normal To], and
      is defined in the following forms:
      –   Constant (Free)
      –   Tabular
      –   Function

Note that:

 •    Entering a zero for a component sets the velocity to zero.
 •    Entering a blank for a component allows free velocity in that direction.
 •    Avoid using multiple velocities on the same vertex.

Frictionless Face
Prevents one or more flat or curved faces from moving or deforming in the normal direction.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
334                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                         Displacements in a Stepped Analysis




  Normal direction relative to the face. No portion of the surface body can move, rotate, or deform normal
to the face.

 Tangential directions. The surface body is free to move, rotate, and deform tangential to the face.

For a flat surface body, the frictionless support is equivalent to a symmetry condition.

Compression Only Support
Applies a compression only constraint normal to one or more faces.

Consider the following model with a bearing load and supports as shown.




Note the effect of the compression only support in the animation of total deformation.

The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the
help. Interface names and other components shown in the demo may differ from those in the released product.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   335
Using the Mechanical Application Features

Since the region of the face in compression is not initially known, a nonlinear solution is required and may
involve a substantial increase in solution time.

Cylindrical Support
For 3-D simulations, prevents one or more cylindrical faces from moving or deforming in combinations of
radial, axial, or tangential directions. Any combination of fixed and free radial, axial, and tangential settings
are allowed.




  Radial directions relative to the             Axial directions relative to the                            Tangential direction relative to
cylinder (Fixed). Such cylindrical            cylinder (Fixed). Such cylindrical                          the cylinder (Fixed). Such cyl-
faces cannot move or deform ra-               faces cannot move or deform axi-                            indrical faces cannot move or
dially to the cylinder.                       ally to the cylinder.                                       deform tangentially to the cylin-
                                                                                                          der.
  Axial and tangential directions               Radial and tangential directions
(Free). The cylinder is free to               (Free). The cylinder is free to                               Radial and axial directions
move, rotate, and deform axially              move, rotate, and deform radially                           (Free). The cylinder is free to
and tangentially.                             and tangentially.                                           move, rotate, and deform radially
                                                                                                          and axially.

For 2-D simulations, cylindrical supports can only be applied to circular edges.

Simply Supported Edge
Available for 3-D simulations only.




 Edge is fixed in all directions.

 Rotation, however, is permitted about the edge.

Applicable for surface body models or line models only.

Prevents one or more straight or curved edges from moving or deforming but rotations about the line are
allowed. If you want to fix the rotations as well, use Fixed Edge (p. 329).

Simply Supported Vertex
Available for 3-D simulations only.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
336                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                         Displacements in a Stepped Analysis




 Vertex is fixed in all directions.

 Rotations, however, are permitted.

Applicable for surface body models or line models only.

Prevents one or more vertices from moving. Rotation about the vertex is allowed. If you want to prevent
rotations, use Fixed Vertex (p. 330).

A simply supported vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity
near the simply supported vertex). You should disregard stress and elastic strain values in the vicinity of the
simply supported vertex.

Fixed Rotation
You can apply a fixed rotation support to faces, edges, and vertices of a surface body. When you only apply
a fixed rotation support to a surface body, the geometry is free in all translational directions. However, the
rotation of the geometry is fixed about the axis of the coordinate system that you select. To apply a fixed
rotation support:

 1.   In the Project tree, right-click the Analysis node to display the context menu.
 2.   On the context menu, point to Insert, and then click Fixed Rotation.
 3.   Select a face, edge, or vertex, and then click Apply .
 4.   Select the coordinate system that you want to use to specify the rotation constraint.
 5.   In the Details view, select Free or Fixed for Rotation X, Rotation Y, and Rotation Z to define the
      fixed rotation support.




 Face not free to rotate.




 Edge not free to rotate.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   337
Using the Mechanical Application Features




     Vertex not free to rotate.

        Note

         •   A fixed vertex rotation support is not realistic and leads to singular stresses (that is, stresses
             that approach infinity near the fixed vertex rotation support). You should disregard stress
             and elastic strain values in the vicinity of the fixed vertex rotation support.
         •   Rotation constraints are combined with other constraints that produce rotational DOF assign-
             ments to determine which values to apply. They are combined with all other constraints to
             determine the nodal coordinate system orientation (frictionless supports, cylindrical supports,
             given displacements, etc).
         •   There may be circumstances in which the rotational support and other constraints cannot
             resolve a discrepancy for preference of a particular node’s coordinate system .


Elastic Support
Allows one or more faces or edges to move or deform according to a spring behavior.

The Elastic Support is based on a Foundation Stiffness that you set in the Details view, which is defined
as the pressure required to produce a unit normal deflection of the foundation.

Coupling
While setting up a model for analysis, you can establish relationships among the different degrees of freedom
of the model by physically modeling the part or a contact condition. However, sometimes there is a need
to be able to model distinctive features of a geometry (joint and hinge effects or models that have equipo-
tential surfaces) which cannot be adequately described with the physical part or contact. In this instance,
you can create a set of surfaces/edges/vertices which have a coupled degree of freedom by using the
Coupling boundary condition.

Coupling the degrees of freedom of a set of geometric entity constrains the results calculated for one
member of the set to be the same for all members of