Docstoc

Asas NL

Document Sample
Asas NL Powered By Docstoc
					                       ASAS (Non-Linear)
                                 User Manual

                                       Version 12




ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
ansysinfo@ansys.com
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494


                 © Copyright 2009. Century Dynamics Limited. All Rights Reserved.
                         Century Dynamics is a subsidiary of ANSYS, Inc.
                    Unauthorised use, distribution or duplication is prohibited.

                             ANSYS, Inc. is certified to ISO 9001:2008
                                           Revision Information
The information in this guide applies to all ANSYS, Inc. products released on or after this date, until superseded
  by a newer version of this guide. This guide replaces individual product installation guides from previous
                                                   releases.

                               Copyright and Trademark Information

      © 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.

   ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT 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 located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
    under license. 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 documentation are furnished by ANSYS, Inc.,
   its subsidiaries, or affiliates under a software license agreement that contains provisions 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, duplication, 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

 The products described in this document contain the following licensed software that requires reproduction of
                                           the following notices.

Formula One is a trademark of Visual Components, Inc.
The product contains Formula One from Visual Components, Inc. Copyright 1994-1995. All rights reserved.

    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.
            ASAS (Non-Linear) User Manual
                              Update Sheet for Version 12
                                              April 2009



Modifications:


The following modifications have been incorporated:

Section          Page(s)           Update/Addition    Explanation

All              All               Update             Conversion to Microsoft® Word format

Table 5.1        5-4               Update             Changes for neutral RAO input

5.1.1            5-6               Update             Allow 32 character hydrodynamic file name

5.1.6            5-11              Addition           Add Note 4 on frequency analysis

5.1.11           5-16              Update             Add HYDR command

                                                      Allow 32 character hydrodynamic file name

5.1.18           5-24              Update             AP20 option replaced by APIW

App I.1          I-1               Update             Delete references to legacy programs ASDIS, PICASO

App I.2          I-2               Update             Delete references to legacy programs ASDIS, PICASO

App I.3          I-2               Update             Delete Section I.3 (ASDIS Interface)

App I.6          I-15              Update             Delete Section I.6 (PICASO Interface )

App M.3.2        M-3               Update             AP20 option replaced by APIW

Table M.1        M-7 – M-8         Update             AP20 option replaced by APIW

App M.6.5        M-11              Update             AP20 option replaced by APIW

App M.6.17       M-34              Update             AP20 option replaced by APIW

App M.6.387      M-53              Update             AP20 option replaced by APIW

App M.6.45       M-58, M-59        Addition           Add definition of phase offset data

App M.7          M-65 – M-66       Update             AP20 option replaced by APIW
         ASAS (Non-Linear) User Manual                                                                                            Contents



                                                    Table of Contents

1. Introduction ............................................................................................................................. 1-1
   1.1 General Capabilities ....................................................................................................... 1-1
   1.2 Using this Manual .......................................................................................................... 1-1
2. Types of Analysis Available.................................................................................................... 2-1
   2.1 General ........................................................................................................................... 2-1
      2.1.1 Static Linear Elastic Solution .................................................................................. 2-1
      2.1.2 Static Non-Linear Incremental Solution ................................................................. 2-2
      2.1.3 Transient Non-Linear Incremental Solution ........................................................... 2-2
      2.1.4 Eigenvalue Extraction ............................................................................................. 2-3
      2.1.5 Steady State Heat Solution ...................................................................................... 2-4
      2.1.6 General Field Analysis ............................................................................................ 2-4
      2.1.7 Piezo-resistivity Analysis ........................................................................................ 2-4
3. Program Features ..................................................................................................................... 3-1
   3.1 Types of Element ........................................................................................................... 3-1
      3.1.1 Uniaxial Element..................................................................................................... 3-1
      3.1.2 Plane Stress/Strain Elements ................................................................................... 3-1
      3.1.3 Axi-symmetric Solid Elements ............................................................................... 3-2
      3.1.4 Three-Dimensional Solids....................................................................................... 3-2
      3.1.5 Gap/Interface Elements ........................................................................................... 3-3
      3.1.6 Plates, Shells and Beams ......................................................................................... 3-3
      3.1.7 Spring/Dashpot Elements ........................................................................................ 3-5
      3.1.8 Linespring Elements................................................................................................ 3-5
      3.1.9 Uniaxial Field Elements .......................................................................................... 3-5
      3.1.10 Two Dimensional Plane Field Elements ............................................................... 3-6
      3.1.11 Three Dimensional Solid Field Elements ............................................................. 3-6
      3.1.12 Axisymmetric Solid Field Elements ..................................................................... 3-6
   3.2 Material Model Types .................................................................................................... 3-6
      3.2.1 Elasticity.................................................................................................................. 3-7
      3.2.2 Plasticity .................................................................................................................. 3-7
         3.2.2.1 Yield Criteria ................................................................................................... 3-8
         3.2.2.2 Hardening Rules .............................................................................................. 3-9
      3.2.3 Creep ....................................................................................................................... 3-9
      3.2.4 Failure ................................................................................................................... 3-10
      3.2.5 Field....................................................................................................................... 3-10
      3.2.6 Piezo-Resistivity ................................................................................................... 3-10
      3.2.7 Heat Convection .................................................................................................... 3-10
      3.2.8 Heat Radiation ....................................................................................................... 3-10
   3.3 Loading ........................................................................................................................ 3-10
      3.3.1 Nodal Loads .......................................................................................................... 3-11
      3.3.2 Prescribed Displacements ..................................................................................... 3-11
      3.3.3 Pressure Loads ...................................................................................................... 3-11
      3.3.4 Distributed Loads .................................................................................................. 3-11
      3.3.5 Temperature Loads................................................................................................ 3-11




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                    i
         ASAS (Non-Linear) User Manual                                                                                          Contents


      3.3.6 Face Temperature .................................................................................................. 3-12
      3.3.7 Body Forces .......................................................................................................... 3-12
      3.3.8 Centrifugal Loads .................................................................................................. 3-12
      3.3.9 Angular Accelerations ........................................................................................... 3-13
      3.3.10 Nodal Fluxes ....................................................................................................... 3-13
      3.3.11 Prescribed Field Variables .................................................................................. 3-13
      3.3.12 Flux Densities...................................................................................................... 3-13
      3.3.13 Wave Load .......................................................................................................... 3-13
      3.3.14 Tank Loads .......................................................................................................... 3-13
      3.3.15 Load History........................................................................................................ 3-14
   3.4 Node Numbers and Coordinates .................................................................................. 3-14
   3.5 Element Numbering ..................................................................................................... 3-15
   3.6 Global and Local Axis Systems ................................................................................... 3-15
      3.6.1 Coordinate Local Axes .......................................................................................... 3-16
      3.6.2 Element Local Axes .............................................................................................. 3-16
      3.6.3 Skew Systems........................................................................................................ 3-16
   3.7 Structural Suppressions and Constraints ...................................................................... 3-17
   3.8 Solution Procedures ..................................................................................................... 3-17
      3.8.1 Non-Linear Static Solution Procedures ................................................................. 3-17
      3.8.2 Non-Linear Transient Solution Procedures ........................................................... 3-19
      3.8.3 Contact Analysis Solution Procedures .................................................................. 3-19
      3.8.4 Fracture Mechanics Solution Procedures .............................................................. 3-19
   3.9 Program Organisation .................................................................................................. 3-19
   3.10     Post-Processing ....................................................................................................... 3-20
   3.11     Data Units ................................................................................................................ 3-20
4. Data Preparation ...................................................................................................................... 4-1
   4.1 General ........................................................................................................................... 4-1
      4.1.1 Data ......................................................................................................................... 4-1
      4.1.2 Data Formats ........................................................................................................... 4-3
         4.1.2.1 General Principles ........................................................................................... 4-3
      4.1.3 Special Symbols ...................................................................................................... 4-6
   4.2 Data Generation Facilities .............................................................................................. 4-8
      4.2.1 Repeat Facilities ...................................................................................................... 4-8
      4.2.2 Re-Repeat Facilities ................................................................................................ 4-9
      4.2.3 List Generation in the Preliminary Data Section .................................................. 4-11
         4.2.3.1 A Simple List................................................................................................. 4-11
         4.2.3.2 Generating a List with a Topological Variable ............................................. 4-11
   4.3 Description of Each Data Block................................................................................... 4-13
      4.3.1 The Preliminary Data ............................................................................................ 4-13
         4.3.1.1 General .......................................................................................................... 4-13
         4.3.1.2 System Control .............................................................................................. 4-13
         4.3.1.3 Solution Algorithm ........................................................................................ 4-14
         4.3.1.4 Model Behaviour ........................................................................................... 4-15
         4.3.1.5 Output Control ............................................................................................... 4-16
      4.3.2 Structural Description Data - see Section 5.2 ....................................................... 4-16
      4.3.3 Boundary Condition Data - see Section 5.3 .......................................................... 4-18




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                ii
         ASAS (Non-Linear) User Manual                                                                                           Contents


      4.3.4 Loading Data - see Section 5.4 ............................................................................. 4-19
         4.3.4.1 Proportional Loading ..................................................................................... 4-19
         4.3.4.2 Load Functions .............................................................................................. 4-20
         4.3.4.3 Pseudo Times ................................................................................................ 4-20
      4.3.5 Additional Mass Data - see Section 5.5 ................................................................ 4-21
      4.3.6 Initial Conditions Data - see Section 5.6 ............................................................... 4-21
   4.4 Description of Output................................................................................................... 4-21
      4.4.1 Data Input Echo and Checking ............................................................................. 4-21
      4.4.2 Analysis Results .................................................................................................... 4-22
      4.4.3 Analysis Summary ................................................................................................ 4-24
      4.4.4 Journal Files .......................................................................................................... 4-24
      4.4.5 ASASNL Output Markers ..................................................................................... 4-24
5. Data Formats ........................................................................................................................... 5-1
   5.1 The Preliminary Data ..................................................................................................... 5-2
      5.1.1 AQWA Command ................................................................................................... 5-5
      5.1.2 BLOCK Command.................................................................................................. 5-5
      5.1.3 COMMENT Command ........................................................................................... 5-6
      5.1.4 CONVERGENCE Command ................................................................................. 5-7
      5.1.5 EGEN Command .................................................................................................... 5-8
      5.1.6 EIGN Command...................................................................................................... 5-8
      5.1.7 ELGROUP Command - (Group Section Only) ...................................................... 5-9
      5.1.8 END Command ..................................................................................................... 5-10
      5.1.9 FILE Command ..................................................................................................... 5-10
      5.1.10 GROUP Command - (Group Section Only) ....................................................... 5-11
      5.1.11 HYDR Command ................................................................................................ 5-12
      5.1.12 INTEGRATION Rule Command ....................................................................... 5-14
      5.1.13 ITERATION Command ...................................................................................... 5-15
      5.1.14 JOB Command .................................................................................................... 5-16
      5.1.15 LOCYCLE Load Cycle Command ..................................................................... 5-17
      5.1.16 MONITOR Command ........................................................................................ 5-17
      5.1.17 NEWSTRUCTURE Command ........................................................................... 5-20
      5.1.18 OPTION Command ............................................................................................ 5-21
      5.1.19 OUTPUT Command ........................................................................................... 5-23
      5.1.20 PARAMETER Command ................................................................................... 5-25
      5.1.21 PASS Command.................................................................................................. 5-27
      5.1.22 PINO Pressure Interpolation Order Command ................................................... 5-27
      5.1.23 PROBLEM and TITLE Command ..................................................................... 5-28
      5.1.24 PROJECT Command .......................................................................................... 5-29
      5.1.25 RESTART Command ......................................................................................... 5-30
      5.1.26 RESU (or POST) Commands.............................................................................. 5-31
      5.1.27 SAVE Command ................................................................................................. 5-33
      5.1.28 SCALING Command .......................................................................................... 5-34
      5.1.29 SKIP Command - (Group Section Only) ............................................................ 5-34
      5.1.30 SLEEP Command ............................................................................................... 5-35
      5.1.31 SOLUTION Command ....................................................................................... 5-36
      5.1.32 SOLVE Command .............................................................................................. 5-39




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                iii
       ASAS (Non-Linear) User Manual                                                                               Contents


    5.1.33 SPIT Command ................................................................................................... 5-40
    5.1.34 SRESTART Special Solution Restart Command ............................................... 5-42
    5.1.35 START Command .............................................................................................. 5-43
    5.1.36 STRUCTURE Command .................................................................................... 5-43
    5.1.37 SYSPAR Command ............................................................................................ 5-44
    5.1.38 SYSTEM Command ........................................................................................... 5-45
    5.1.39 TEMPORAL Command...................................................................................... 5-46
    5.1.40 TEXT Command ................................................................................................. 5-47
    5.1.41 TITLE Command ................................................................................................ 5-48
    5.1.42 UNITS Command ............................................................................................... 5-48
       5.1.42.1 Global UNITS Definition ............................................................................ 5-48
    5.1.43 UPDATE Command ........................................................................................... 5-50
    5.1.44 WAKE Command ............................................................................................... 5-51
    5.1.45 WEIGHTS Command ......................................................................................... 5-52
 5.2 Structural Description Data .......................................................................................... 5-53
    5.2.1 UNITS Command ................................................................................................. 5-53
    5.2.2 COORDINATE Data ............................................................................................ 5-56
       5.2.2.1 Local Coordinate System Header .................................................................. 5-57
       5.2.2.2 Local Coordinate System Orientation ........................................................... 5-57
       5.2.2.3 Node Coordinates .......................................................................................... 5-60
       5.2.2.4 Coordinate Imperfection Data ....................................................................... 5-62
    5.2.3 Element Topology Data ........................................................................................ 5-65
    5.2.4 Material Property Data .......................................................................................... 5-67
       5.2.4.1 Elastic Material Properties ............................................................................ 5-70
          5.2.4.1.1 Isotropic material properties .................................................................. 5-70
          5.2.4.1.2 Orthotropic material properties.............................................................. 5-72
          5.2.4.1.3 Woven material properties ..................................................................... 5-74
          5.2.4.1.4 Anisotropic material properties ............................................................. 5-75
          5.2.4.1.5 Hyper-elastic material properties ........................................................... 5-77
          5.2.4.1.6 Laminated Material Properties .............................................................. 5-78
          5.2.4.1.7 User Material Properties ........................................................................ 5-80
          5.2.4.1.8 Field Material Properties ....................................................................... 5-81
          5.2.4.1.9 Piezo-resistivity Material Properties...................................................... 5-81
          5.2.4.1.10 Convective Heat Material Properties ................................................... 5-82
          5.2.4.1.11 Radiant Heat Material Properties......................................................... 5-83
       5.2.4.2 Plastic Material Properties............................................................................. 5-84
       5.2.4.3 Creep Material Properties .............................................................................. 5-89
       5.2.4.4 Failure Material Properties ............................................................................ 5-91
          5.2.4.4.1 Lamina Failure Values ........................................................................... 5-92
          5.2.4.4.2 Plastic Lamina Failure FLW1 Values.................................................... 5-93
          5.2.4.4.3 Plastic Lamina Failure FLW2 Values.................................................... 5-94
          5.2.4.4.4 Laminate Failure Values ........................................................................ 5-95
    5.2.5 Geometric Properties Data .................................................................................... 5-98
       5.2.5.1 Geometric Properties - (WST4 and SST4) .................................................... 5-99
       5.2.5.2 Geometric Properties - (SPR1 and SPR2) ................................................... 5-101
       5.2.5.3 Geometric Properties - (Laminated Construction) ...................................... 5-103




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    iv
       ASAS (Non-Linear) User Manual                                                                                    Contents


       5.2.5.4 Geometric Properties - (Rigid Surface Elements) ....................................... 5-106
       5.2.5.5 Definition of geometric properties for beam elements having local axes
       definition and/or rigid offsets ..................................................................................... 5-108
    5.2.6 Section Data ........................................................................................................ 5-114
       5.2.6.1 Section Types and Dimensions ................................................................... 5-116
       5.2.6.2 Fabricated Plate Sections............................................................................. 5-120
    5.2.7 Skew System Data............................................................................................... 5-123
       5.2.7.1 Skew Systems - Direction Cosines .............................................................. 5-123
       5.2.7.2 Skew Systems - Nodal Definition ............................................................... 5-125
 5.3 BOUNDARY Conditions Data .................................................................................. 5-126
    5.3.1 UNITS Command ............................................................................................... 5-126
    5.3.2 FREEDOM Release Data .................................................................................... 5-126
    5.3.3 SUPPRESSED Freedoms Data ........................................................................... 5-129
    5.3.4 Prescribed Freedom Data .................................................................................... 5-131
    5.3.5 CONSTRAINT Equation Data ........................................................................... 5-133
    5.3.6 RIGID Constraints Data ...................................................................................... 5-137
 5.4 Loading Data .............................................................................................................. 5-140
    5.4.1 UNITS Command ............................................................................................... 5-140
    5.4.2 LOADING Data .................................................................................................. 5-142
    5.4.3 NODAL LOADS Data ........................................................................................ 5-143
    5.4.4 PRESCRIBED Displacements, Velocities and Accelerations Data ................... 5-145
    5.4.5 PRESSURE Load Data ....................................................................................... 5-146
       5.4.5.1 UNIFORM Pressure Load Data .................................................................. 5-148
       5.4.5.2 NON-UNIFORM Pressure Load Data ........................................................ 5-149
    5.4.6 DISTRIBUTED Load Data ................................................................................. 5-154
       5.4.6.1 Local Beam Distributed Loads .................................................................... 5-158
          5.4.6.1.1 BL1 and BL2 Load Patterns ................................................................ 5-161
          5.4.6.1.2 BL3 Load Pattern ................................................................................. 5-162
          5.4.6.1.3 BL4 Load Pattern ................................................................................. 5-163
          5.4.6.1.4 BL5 Load Pattern ................................................................................. 5-164
          5.4.6.1.5 BL6 Load Pattern ................................................................................. 5-165
          5.4.6.1.6 BL7 Load Pattern ................................................................................. 5-166
          5.4.6.1.7 BL8 Load Pattern ................................................................................. 5-167
       5.4.6.2 Global Beam Distributed Loads .................................................................. 5-168
          5.4.6.2.1 GL1 and GP1 Load Patterns ................................................................ 5-171
          5.4.6.2.2 GL4 and GP4 Load Patterns ................................................................ 5-173
          5.4.6.2.3 GL5 Load Pattern ................................................................................ 5-174
          5.4.6.2.4 GL6 and GP6 Load Patterns ................................................................ 5-175
          5.4.6.2.5 GL7 and GP7 Load Patterns ................................................................ 5-176
       5.4.6.3 Panel Edge Distributed Loads ..................................................................... 5-178
       5.4.6.4 Curved Beam Distributed Loads ................................................................. 5-181
    5.4.7 TEMPERATURE Load Data .............................................................................. 5-183
       5.4.7.1 NODAL Temperature Data ......................................................................... 5-183
       5.4.7.2 ELEMENT Temperature Data .................................................................... 5-185
       5.4.7.3 UNIFORM Element Temperature Data ...................................................... 5-186
       5.4.7.4 NON-UNIFORM Element Temperature Data ............................................ 5-187




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                          v
         ASAS (Non-Linear) User Manual                                                                                          Contents


      5.4.8 FACE TEMPERATURE Data ............................................................................ 5-191
         5.4.8.1 Nodal Face Temperature ............................................................................. 5-191
         5.4.8.2 ELEMENT FACE TEMPERATURE Data ................................................ 5-192
         5.4.8.3 UNIFORM Element Face Temperature Data .............................................. 5-193
         5.4.8.4 NON-UNIFORM Element Face Temperature Data .................................... 5-194
      5.4.9 BODY FORCE Data ........................................................................................... 5-197
      5.4.10 CENTRIFUGAL Loads Data ............................................................................ 5-198
      5.4.11 ANGULAR ACCELERATION Loads Data .................................................... 5-199
      5.4.12 NODAL FLUX Data ......................................................................................... 5-201
      5.4.13 PRESCRIBED Field Variable Data .................................................................. 5-202
      5.4.14 FLUX DENSITY Data ...................................................................................... 5-203
            5.4.14.1.1 UNIFORM Flux Density Data........................................................... 5-204
            5.4.14.1.2 NON-UNIFORM Flux Density Data................................................. 5-206
      5.4.15 WAVE LOAD Data .......................................................................................... 5-212
      5.4.16 TANK LOAD data ............................................................................................ 5-213
      5.4.17 LOAD Functions ............................................................................................... 5-215
   5.5 DIRECT Mass Input Data .......................................................................................... 5-217
      5.5.1 UNITS command ................................................................................................ 5-217
      5.5.2 LUMP ADDED MASS Data .............................................................................. 5-218
   5.6 Initial Conditions Data ............................................................................................... 5-220
      5.6.1 UNITS Command ............................................................................................... 5-220
      5.6.2 RESIDUAL Initial Stresses................................................................................. 5-221
      5.6.3 RESIDUAL Initial Stresses for Stiffeners WST4 and SST4 .............................. 5-222
      5.6.4 Initial Conditions................................................................................................. 5-224
   5.7 STOP Command ........................................................................................................ 5-226
6. Running Instructions ............................................................................................................... 6-1
   6.1 DATA AREA Requirement ........................................................................................... 6-1
   6.2 Data-Manager Parameters .............................................................................................. 6-1
   6.3 File Status ....................................................................................................................... 6-3
   6.4 Warnings and Errors ...................................................................................................... 6-4
   6.5 Running Instructions ...................................................................................................... 6-5
   6.6 ASAS Initialisation File ................................................................................................. 6-8
   6.7 Extended Syntax in Data Files ....................................................................................... 6-9
      6.7.1 IF/THEN/ELSE ....................................................................................................... 6-9
      6.7.2 DATA REPLACEMENT...................................................................................... 6-12
      6.7.3 The DEFINE Command ........................................................................................ 6-12
   6.8 Secondary Data Files within ASAS-NL Data .............................................................. 6-13
      6.8.1 Use of @filename command ................................................................................. 6-13
      6.8.2 Notes about the @ Command ............................................................................... 6-14
   6.9 Soft Halt Facility .......................................................................................................... 6-15
Appendix - A Element Description Sheets ............................................................................... A-1
   A.1      Facilities Available for each Element Type ............................................................. A-1
   A.2      Element Axes Systems ............................................................................................. A-8
      A.2.1 Local Axes on Beam Elements ............................................................................. A-8
   A.3      Beam Offsets .......................................................................................................... A-11
      A.3.1 OFFS Command .................................................................................................. A-11




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                               vi
         ASAS (Non-Linear) User Manual                                                                                         Contents


     A.3.2 OFFG and OFSK Commands ............................................................................. A-12
     A.3.3 OFCO Command................................................................................................. A-13
     A.3.4 Finite Element Description Sheets ...................................................................... A-14
  A.4      References ............................................................................................................ A-136
Appendix - B Material Models ................................................................................................. B-1
  B.1 Linear Elasticity ............................................................................................................ B-1
     B.1.1 Isotropic Material .................................................................................................. B-1
     B.1.2 Anisotropic Material .............................................................................................. B-1
     B.1.3 Orthotropic Material .............................................................................................. B-1
     B.1.4 Laminated Material for Shell Elements ................................................................. B-2
     B.1.5 Woven Material ..................................................................................................... B-4
  B.2 Non-Linear Elasticity .................................................................................................... B-5
     B.2.1 Hyperelastic Material ............................................................................................ B-5
  B.3 Plasticity ........................................................................................................................ B-6
     B.3.1 Yield Criteria ......................................................................................................... B-6
        B.3.1.1 Von Mises ...................................................................................................... B-6
        B.3.1.2 Tresca ............................................................................................................. B-6
        B.3.1.3 Ivanov ............................................................................................................ B-6
        B.3.1.4 Mohr-Coulomb .............................................................................................. B-7
        B.3.1.5 Drucker-Prager .............................................................................................. B-8
        B.3.1.6 Stress Resultant Plasticity for Beams ............................................................ B-8
        B.3.1.7 Coulomb Friction ........................................................................................... B-9
        B.3.1.8 Tension Cut-off .............................................................................................. B-9
        B.3.1.9 Inelastic Spring .............................................................................................. B-9
     B.3.2 Hardening Rules .................................................................................................. B-10
        B.3.2.1 Isotropic ....................................................................................................... B-10
        B.3.2.2 Kinematic ..................................................................................................... B-11
        B.3.2.3 Combined ..................................................................................................... B-11
     B.3.3 Equivalent Strain ................................................................................................. B-12
  B.4 CREEP ........................................................................................................................ B-12
     B.4.1 In-Built Creep Laws ............................................................................................ B-13
     B.4.2 User Supplied Creep Laws .................................................................................. B-14
  B.5 Composite Failure ....................................................................................................... B-16
     B.5.1 Lamina Failure Criteria ....................................................................................... B-16
     B.5.2 Laminate Failure Criteria .................................................................................... B-20
     B.5.3 Failure Laws ........................................................................................................ B-22
        B.5.3.1 In-Built Failure Law .................................................................................... B-22
        B.5.3.2 User-Defined Failure Laws.......................................................................... B-24
  B.6 User Material............................................................................................................... B-26
  B.7 References ................................................................................................................... B-31
Appendix - C Solution Strategies in ASAS-NL ....................................................................... C-1
  C.1 Introduction ................................................................................................................... C-1
  C.2 Incremental - Iterative Procedures ................................................................................ C-3
     C.2.1 Introduction ........................................................................................................... C-3
     C.2.2 Basic Definitions ................................................................................................... C-7
     C.2.3 Incrementation procedures .................................................................................... C-8




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                             vii
         ASAS (Non-Linear) User Manual                                                                                             Contents


      C.2.4 Iteration procedures ............................................................................................... C-9
         C.2.4.1 Type of constraint surface ............................................................................. C-9
         C.2.4.2 Iteration techniques ...................................................................................... C-11
      C.2.5 Solution methods ................................................................................................. C-14
         C.2.5.1 Euler-Cauchy method .................................................................................. C-14
         C.2.5.2 Self-correcting Euler-Cauchy ...................................................................... C-15
         C.2.5.3 Full incremental - iterative method.............................................................. C-15
      C.2.6 Conclusions ......................................................................................................... C-16
  C.3 Computation of Stresses.............................................................................................. C-17
      C.3.1 Forward Euler Integration Scheme ...................................................................... C-17
      C.3.2 Backward Euler Integration Scheme ................................................................... C-19
  C.4 Convergence and Auto-Recovery ............................................................................... C-20
      C.4.1 Convergence Check ............................................................................................. C-20
      C.4.2 Auto-Recovery .................................................................................................... C-20
  C.5 Eigenvalue Analysis .................................................................................................... C-21
      C.5.1 Linear Pre-buckling Case .................................................................................... C-21
      C.5.2 Non-linear Pre-buckling Case ............................................................................. C-21
      C.5.3 Spectral Analysis ................................................................................................. C-22
      C.5.4 Natural Frequency Analysis ................................................................................ C-23
  C.6 Contact Analysis ......................................................................................................... C-23
      C.6.1 Penalty Method .................................................................................................... C-23
      C.6.2 Augmented Lagrangian Method .......................................................................... C-24
  C.7 References ................................................................................................................... C-24
Appendix - D Restarts .............................................................................................................. D-1
  D.1       Introduction .............................................................................................................. D-1
  D.2       Initial Analysis ......................................................................................................... D-1
  D.3       Restarted Jobs ........................................................................................................... D-2
  D.4       Examples .................................................................................................................. D-3
Appendix - E Example Data Files ............................................................................................ E-1
  E.1 Example 1: BM3D Plasticity Model (T0574) ............................................................... E-1
  E.2 Example 2: TCS9 Geometric non-linearity (T0533) .................................................... E-3
  E.3 Example 3: QUX4 Incompressible behaviour (T0540) ................................................ E-4
  E.4 Example 4: QUS4 Elasto-plastic stiffened shell (T0553) ............................................. E-6
  E.5 Example 6: QUS4 transient dynamics (T0591) .......................................................... E-12
Appendix - F List of Freedom Names .......................................................................................F-1
Appendix - G Isoparametric Elements ..................................................................................... G-1
  G.1       Curvilinear Axes....................................................................................................... G-1
  G.2       Integration Rules ...................................................................................................... G-1
Appendix - H ASAS/ASAS-NL Compatibility........................................................................ H-1
Appendix - I POSTNL General Post-Processor Interface Program .......................................... I-1
  I.1 Introduction ......................................................................................................................... I-1
  I.2 Usage .................................................................................................................................. I-1
  I.3 FEMVIEW Interface........................................................................................................... I-2
      I.3.1 Primary Nodal Variables ......................................................................................... I-4
      I.3.2 Primary Element Based Variables ........................................................................... I-5
         I.3.2.1 Rotation of Shell Element Based Variables ..................................................... I-5




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                 viii
         ASAS (Non-Linear) User Manual                                                                                           Contents


      I.3.3 Secondary Element Based Variables ....................................................................... I-6
         I.3.3.1 Laminated Composite Shells ........................................................................... I-6
         I.3.3.2 Surface and Global Failure Indices .................................................................. I-7
         I.3.3.3 Laminated Composite Bricks ........................................................................... I-7
  I.4 PATRAN Interface ............................................................................................................. I-8
  I.5 Printer Interface ................................................................................................................ I-10
  I.6 Time Histories................................................................................................................... I-15
  I.7 Rotation of Element Based Variables for Shells .............................................................. I-23
      I.7.1 Introduction ............................................................................................................ I-23
      I.7.2 Restrictions ............................................................................................................ I-23
      I.7.3 The Plane Stress Transformation ........................................................................... I-23
      I.7.4 Determination of the Rotational Angle, θ.............................................................. I-24
      I.7.5 User Definition of New Local Axes Direction ...................................................... I-24
      I.7.6 User Definition of Element Top and Bottom Surfaces .......................................... I-26
      I.7.7 References .............................................................................................................. I-27
  I.8 Fracture Mechanics Processing ........................................................................................ I-28
      I.8.1 Introduction ............................................................................................................ I-28
      I.8.2 Restrictions ............................................................................................................ I-28
      I.8.3 Notes on the use of Fracture Parameters ............................................................... I-29
      I.8.4 Format of Contour Definition File ......................................................................... I-29
      I.8.5 Example ................................................................................................................. I-29
Appendix - J Creep Analysis ..................................................................................................... J-1
  J.1Overview ............................................................................................................................. J-1
  J.2Creep Solution Methods ..................................................................................................... J-2
  J.3Convergence of Creep Solutions ........................................................................................ J-3
  J.4Automatic Timestepping..................................................................................................... J-3
  J.5Example Preliminary Data .................................................................................................. J-5
  J.6Recommendations for Creep Analysis ............................................................................... J-5
  J.7References ........................................................................................................................... J-6
Appendix - K Transient Dynamics Analysis ............................................................................ K-1
  K.1       Overview .................................................................................................................. K-1
  K.2       Time Integration Algorithm ..................................................................................... K-2
  K.3       Automatic Timestepping .......................................................................................... K-3
  K.4       References ................................................................................................................ K-9
Appendix - L References .......................................................................................................... L-1
Appendix - M Wave Loading On Offshore Jacket Structures ................................................. M-1
  M.1       Introduction ............................................................................................................. M-1
  M.2       Water Axes .............................................................................................................. M-1
  M.3       Wave Theories ......................................................................................................... M-2
      M.3.1 Conventional wave theories................................................................................. M-2
      M.3.2 Shell New Wave .................................................................................................. M-2
      M.3.3 Irregular Wave ..................................................................................................... M-3
  M.4       Wave load data format ............................................................................................ M-5
  M.5       WAVE LOAD Data ................................................................................................ M-6
  M.6       Description of the Wave Load Data Block ............................................................. M-8
      M.6.1 WAVE LOAD Data............................................................................................. M-8




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                ix
       ASAS (Non-Linear) User Manual                                                                                      Contents


      M.6.2       AMAS Command ................................................................................................ M-9
      M.6.3       BEAM Element Command................................................................................ M-10
      M.6.4       Current BLOCKAGE Factor Command ........................................................... M-10
      M.6.5       BUOYANCY Command ................................................................................... M-11
      M.6.6       CURRENT Command ....................................................................................... M-12
      M.6.7       DRAG Coefficients ........................................................................................... M-14
      M.6.8       ELEVATION Command ................................................................................... M-15
      M.6.9       END Command ................................................................................................. M-16
      M.6.10       EXECUTE Command ..................................................................................... M-16
      M.6.11       FREE Flooding Command .............................................................................. M-17
      M.6.12       GRAVITY Command...................................................................................... M-18
      M.6.13       GRID Wave Command ................................................................................... M-20
      M.6.14       Marine GROWTH Command ......................................................................... M-27
      M.6.15       HYDR Command ............................................................................................ M-28
      M.6.16       Keulegan-Carpenter Number Tables ............................................................... M-32
      M.6.17       Wave KINEMATICS Factor Command ......................................................... M-33
      M.6.18       LFUN Data ...................................................................................................... M-34
      M.6.19       MASS Inertia Coefficients .............................................................................. M-35
      M.6.20       MOVE Command ............................................................................................ M-36
      M.6.21       NANG Command ............................................................................................ M-37
      M.6.22       NOBM Command............................................................................................ M-38
      M.6.23       NOBO Command ............................................................................................ M-38
      M.6.24       NOFR Command ............................................................................................. M-38
      M.6.25       NOLO Command ............................................................................................ M-39
      M.6.26       NOSW Command ............................................................................................ M-40
      M.6.27       NOWI Command ............................................................................................. M-41
      M.6.28       NOWL Command............................................................................................ M-42
      M.6.29       OFFSET Command ......................................................................................... M-43
      M.6.30       OUTPUT Control Command........................................................................... M-44
      M.6.31       PEXT Command.............................................................................................. M-44
      M.6.32       POINT Current Command............................................................................... M-45
      M.6.33       PHASE Command ........................................................................................... M-47
      M.6.34       PRINT Command ............................................................................................ M-49
      M.6.35       Reynolds Number Tables ................................................................................ M-49
      M.6.36       SLWT Command............................................................................................. M-51
      M.6.37       SPECTRAL Command.................................................................................... M-52
      M.6.38       Wave SPREADING Command ....................................................................... M-53
      M.6.39       STOP Command .............................................................................................. M-54
      M.6.40       TIDE Command .............................................................................................. M-54
      M.6.41       TOLERANCE Command ................................................................................ M-56
      M.6.42       UNITS Command ............................................................................................ M-56
      M.6.43       VAXS Command ............................................................................................. M-57
      M.6.44       VISCOSITY Command ................................................................................... M-58
      M.6.45       VPOS Command ............................................................................................. M-58
      M.6.46       WAVE Command............................................................................................ M-59
      M.6.47       WIND Command ............................................................................................. M-60




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                            x
         ASAS (Non-Linear) User Manual                                                                                       Contents


    M.6.48 WPAR Command ............................................................................................ M-61
    M.6.49 XMAS Data ..................................................................................................... M-63
    M.6.50 ZONE Data ...................................................................................................... M-64
  M.7      Valid Options Controlling Wave Load Calculation .............................................. M-65
Appendix - N Heat Analysis ..................................................................................................... N-1
  N.1      Introduction .............................................................................................................. N-1
  N.2      Heat Equations ......................................................................................................... N-1
  N.3      Convection................................................................................................................ N-2
  N.4      Radiation .................................................................................................................. N-2
  N.5      Controlling a Heat Analysis ..................................................................................... N-2
  N.6      Saving Heat Analysis Results................................................................................... N-3
  N.7      Interfacing with Stress Analysis ............................................................................... N-4
Appendix - O Coupled Wind and Wave Load Analysis of Offshore Wind Turbine ............... O-1
  O.1      Introduction .............................................................................................................. O-1
  O.2      The Analysis ............................................................................................................. O-1
  O.3      Data for FLXG job ................................................................................................... O-3
    O.3.1 JOB Command ...................................................................................................... O-3
    O.3.2 Generalized Mode Definition ................................................................................ O-3
  O.4      Output from FLXG job............................................................................................. O-5
    O.4.1 Generalized Matrix Files ....................................................................................... O-5
    O.4.2 Generalized External Force File ............................................................................ O-5




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                            xi
      ASAS (Non-Linear) User Manual                                                                               Introduction


1. Introduction

1.1    General Capabilities

ASAS-NL is a computer program for the static and dynamic analysis of engineering structures and components
which exhibit some form of non-linear response. It is designed for engineers to use, specifically for problems
involving plasticity, creep and large displacement effects, including buckling and gapping. For linear elastic
problems the parent program ASAS is usually more appropriate. The program is based on a finite element
formulation of the structural behaviour and uses an incremental procedure to represent the loading process and
response of the structure. A displacement formulation of the finite element method is used.

An extensive range of finite elements is provided for modelling both structures and continua. The material
models available include most popular theories of elasto-plastic behaviour and some specialist models for
failure. Large displacement effects may be taken into account where appropriate. Extensions to handle other
nonlinear effects have been allowed for in the program’s modular design, and are being developed.

ASAS-NL can treat a wide range of loadings. Loads may be presented as any combination of point forces or
moments, prescribed displacements, pressures, temperatures, body forces, centrifugal loads or angular
accelerations and may be applied incrementally or specified as a function of time.

The program is a further development of the ASAS family and, although a separate program, it is fully
compatible with other ASAS programs. Wherever appropriate the data input and output is ‘standard ASAS’.

The following ASAS programs interface with ASAS-NL through the interactive post-processing program,
POSTNL:

       FEMGEN/FEMVIEW                           Interactive graphical model building and results display.


In addition a number of proprietary general purpose graphics programs including PATRAN interface with
ASAS-NL to provide capabilities for model generation and results viewing.

ASAS-NL is written in FORTRAN and is readily transportable to differing computer types. The present version
is available on PC only.

ASAS-NL is thoroughly described in its documentation. This User Manual contains full instructions for using
the system, including choice of facilities, data preparation and running instructions.                  Revisions of this User
Manual are circulated to all registered holders.

1.2    Using this Manual

This document is intended to serve both as a reference manual for the experienced ASAS-NL user and also as an
introduction to the program. In general the introductory and explanatory sections are contained in the first few
sections and the reference sections are placed at the end or in Appendices. The level of presentation and
background knowledge assumed of the user is adjusted to suit the complexity of the subject matter. No attempt
is made to cover the theory of finite elements or structural mechanics, but useful references are provided in
Appendix -L.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Page 1-1
       ASAS (Non-Linear) User Manual                                                                                Introduction


Section 2 is an introduction to the types of analysis available. It contains brief descriptions of the program’s
various capabilities and also introduces terminology used in later sections.

Section 3 describes the modelling facilities that are contained in ASAS-NL. It includes information and advice
on the element and material types available and information on key features such as node numbering, local axis
systems, supports, loading and control of the program.

The data required to run the program is described in outline, in Section                   4 The function of each data block type
is explained and the procedures for controlling the operations of the program are presented. This section is
essential reading for both new and experienced users.

Section 5 is intended as a reference section. It describes the format of each block of ASAS-NL data and gives
examples of their use.

In   Section 6 information relevant to specific machine installations is presented. Users should ensure that this
corresponds to their version. It contains running instructions and information for estimating size and cost
parameters together with any restrictions.

Various reference material is presented in Appendices.

Appendix -A is a key feature of the manual. It contains ‘element description sheets’, giving detailed
information about each element in the ASAS-NL library.

Appendix -B provides details of and reference to each material model available.

Appendix -C gives a description of the solution procedures used in ASAS-NL with an account of the control
options available to the user.

Appendix -D describes the Restart facility.

Appendix -E gives details of some example data files. A comprehensive series of test, verification and
educational input data files can be included with the computer programs.

Appendix -F gives a list of the names of the freedoms which may be present at a node.

Appendix -G explains the conventions for setting up local axes and the integration rules used for all
isoparametric elements.

Appendix -H lists necessary differences in data format between ASAS and ASAS-NL. These may impose
restrictions in modelling problems which are to run on both programs.

Appendix -I describes the interface program POSTNL required by various post-processors.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                      Page 1-2
     ASAS (Non-Linear) User Manual                                                                     Introduction


Appendix -J gives additional instructions for creep analyses.

Appendix -K describes transient dynamic analysis.

Appendix -L contains a list of general references.

Appendix -M describes the wave loading capability in ASAS-NL.

Appendix - N describes heat analysis

Appendix - O describes coupled wind and wave load analysis of offshore wind turbines




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                        Page 1-3
     ASAS (Non-Linear) User Manual                                                                     Introduction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                        Page 1-4
ASAS (Non-Linear) User Manual                                                                 Types of Analysis Available



2.      Types of Analysis Available

2.1     General

ASAS-NL is a general purpose computer program aimed at providing solutions to non-linear problems across
the broad field of structural mechanics. Therefore the facilities included in the program are subject to continual
enhancement as new problems arise and solution methods are improved. To accommodate this development to
the ‘state of the art’, the program has a highly modular structure communicating with a ‘data manager’ which is
tailored to the needs of non-linear analysis.

The analysis capabilities currently available include the following:

•           Static linear elastic

•           Static, non-linear incremental - STAT type

•           Transient, non-linear incremental - TRAN type

•           Eigenvalue extraction - buckling or natural frequency

•           General field

•           Piezo-resistivity - PIER type

•           Steady state heat - HEAT type

•           Transient heat - HTRA type


It should be noted that this categorisation influences the type of solution procedure which is employed by the
program and not the actual structural behaviour (thus for example a solution could be obtained to a linear elastic
problem using the non-linear incremental procedure - albeit inefficiently).

ASAS-NL solves the system of equations using the frontal solution technique. As well as an ordinary frontal
solver, an optimised frontal solution is also available that can greatly reduce the solution time and storage
requirements in medium to large problems.




2.1.1       Static Linear Elastic Solution

In general, a linear elastic problem is better tackled using the ASAS program. However, the linear elastic option
is included for applications where the model can be classified as small and/or where a linear elastic analysis is
the first tentative step in the design analysis before launching into a more expensive non-linear run. The
facilities available in ASAS-NL are generally the same as those in ASAS. The main differences are a somewhat




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 2-1
ASAS (Non-Linear) User Manual                                                                 Types of Analysis Available


reduced element library (see Section 3.1), treatment of a single loadcase at a time and the absence of the
substructuring facility. An important addition in ASAS-NL is the ability to handle generalised plane strain.




2.1.2       Static Non-Linear Incremental Solution

This category includes problems in which the non-linearity is due to any combination of the following:

•           large displacement effects

•           non-linear elastic material behaviour

•           plasticity

•           laminated composite failure behaviour

•           soil and rock-like material behaviour

•           non-linear boundary conditions (gaps and rigid surface contact)


The loading may be applied in a proportional or quite general non-proportional manner. In the latter case a
‘pseudo’ time scale is defined by the user to specify the sequence of loading.

Any given type of non-linear behaviour can be restricted to certain areas of the structural model, by use of
‘groups’ of elements and by use of different material identifiers.

The analysis procedure for these problems requires that the load is applied incrementally and the program then
provides several alternative methods for determining the structural response. These methods are a completely
flexible combination of various incremental-iterative procedures such as load or displacement incrementation
complemented by a selection of Newton-Raphson iteration techniques.

In the absence of other directives, the program automatically selects the Initial Stiffness iteration for all
increments. However experienced users can control the type of method or combination of methods, to be used
for each increment together with the order of non-linear theory required. A full explanation of the incremental
and iterative methods available is contained in Appendix -C.




2.1.3       Transient Non-Linear Incremental Solution

This category includes all problems where the material or structural response is a function of real time.

(a)     Creep Analysis


Creep is the generic term used in ASAS-NL to denote the time dependent material response associated with long
timescales. See Appendix -J for further details. Allowance has been made within the modular design of ASAS-




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 2-2
ASAS (Non-Linear) User Manual                                                                 Types of Analysis Available


NL for the more rapid time dependent material response associated with high velocity impact and metal forming
processes. These capabilities are planned for future development.

(b)     Non-Linear Transient Dynamic Analysis


Problems which require the inertia effects of the mass of the structure to be included come under the category of
transient dynamic analysis. Such an analysis is required where loading varies rapidly such as during blast from
an explosion or ground motion from an earthquake. In ASAS-NL the equations of motion are solved at discrete
points in time with the solution advancing in a stepwise manner. All the non-linear effects associated with a
static non-linear incremental solution (see Section 2.1.2) may be included in the analysis if required.

For transient dynamic analysis, the modelling of inertia (mass) is just as important as ensuring that the stiffness
characteristics are adequately represented. Three basic forms of mass matrix are available in ASAS-NL:

(i)     The program assembles the mass matrix from user specified lumped mass values at appropriate nodes to
        produce a Direct Input Mass Matrix.

(ii)    The program assembles the mass matrix from the mass of each element lumped at its nodes (the Element
        Lumped Mass Matrix).

(iii)   (The program assembles the mass matrix from the actual distribution of mass within each element (the
        Element Consistent Mass Matrix).


These three forms can be mixed within a structure if required. The mass of selected elements can be omitted by
flagging the appropriate element topology commands. If no mass type is selected specifically, the type of
element mass matrix defaults to that given in Appendix -A.




2.1.4       Eigenvalue Extraction

In ASAS-NL, the two main applications of eigenvalue analysis are to provide solutions for stability and free
vibration problems.        The subspace iteration technique is employed to solve the eigenproblem which will
compute the lowest few eigenvalues requested by the user.

(a)       Stability Analysis


This type of analysis is used to determine the buckling loads and associated modes of the structures. The pre-
buckling behaviour can either be linear or non-linear. Full details concerning stability analysis are given in
Appendix C.5.1 and C.5.2.

(b)     Natural Frequency Analysis


This type of analysis provides the natural frequencies and associated vibration mode shapes of unloaded or pre-
loaded structures.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 2-3
ASAS (Non-Linear) User Manual                                                                 Types of Analysis Available


In ASAS-NL, natural frequency analysis can be performed on free-free structures provided that a suitable shift is
specified.

Loading data need not be present for free vibration analysis but a warning message will be given. This facility
allows the user to determine natural frequencies of an unloaded structure.

Full explanation of natural frequency analysis can be found in Appendix C.5.4.




2.1.5        Steady State Heat Solution

This category provides solution to steady state heat transfer problems. The procedure is principally applied to
heat conductivity problems although secondary convective and radiative heat transfer effects may also be
included.

For this type of solution, non-linearity arises from the temperature dependency of heat transfer coefficients.
Their variations with temperature may be specified as temperature dependent material property data.

As in stress analysis, the heat input (cf loading) may be applied in a proportional or quite general non-
proportional manner.

A selection of Newton-Raphson iteration techniques is available for non-linear solution as described in the static
non-linear stress analysis solution.




2.1.6        General Field Analysis

There are a wide range of engineering problems, eg electrical conductivity, ideal fluid flow and seepage through
a porous medium that are governed by Laplace’s equation. Field elements with a single degree of freedom at
each node are available for the solution of such problems.




2.1.7        Piezo-resistivity Analysis

A piezo-resistive material is one which experiences a change in electrical conductivity when the applied stress
field changes. ASAS-NL is capable of solving both the stress and the electrical field problem simultaneously.
THIS CAPABILITY IS CURRENTLY RESTRICTED AND IS NOT GENERALLY AVAILABLE.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 2-4
ASAS (Non-Linear) User Manual                                                                 Types of Analysis Available




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 2-5
ASAS (Non-Linear) User Manual                                                                          Program Features



3.      Program Features

3.1     Types of Element

The ASAS-NL library contains elements which are capable of modelling both continuum and structural forms.
The great majority are identical in their linear format to parent elements in ASAS, so that compatibility is
maintained. Specialisations are, however, introduced as required for non-linear applications.

Each type of element has a distinctive four character name, which indicates its form and number of nodes.

e.g. TCS8 - Thick Curved Shell with 8 nodes

A full description of each element type is provided in the element description sheets of Appendix -A.

Most element types are ‘isoparametric’ and have considerable versatility to model geometric and material
variations. However, excessive distortions from rectangular (or equilateral triangular) planform should be
avoided. Most element matrices are evaluated using numerical integration. The number of integration points in
the direction of the local curvilinear axes can be specified by the user, but the default values implemented in the
program are normally recommended.                  The default integration rule generally corresponds to the ‘reduced
integration technique’. Appendix -G gives details of the various integration rules available, and an explanation
of local curvilinear axes.

In all elements, large displacement effects are taken into account by updating the geometry and using the
geometric stiffness matrix and non-linear geometrical relations. These relations are defined employing an
Updated Lagrangian formulation.

Elements may be placed together in ‘groups’. This is advantageous where it is required to vary, from group to
group, the type of behaviour modelled or the output printed. Certain elements must belong to their own groups
(see Appendix -A).

In the following sections elements are described according to their family.




3.1.1       Uniaxial Element

FLA2 - 2 node uniaxial constant stress element.

This element has some use as a tie/strut element, but its principal application is in association with other
elements, to represent boundary conditions and stiffeners.




3.1.2       Plane Stress/Strain Elements

These elements are essentially 2-D and are intended for problems in which a state of plane stress or plane strain
exists in the plane of the element.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-1
ASAS (Non-Linear) User Manual                                                                          Program Features


        TRM3         -   3 node isoparametric triangle

        QUM4         -   4 node isoparametric quadrilateral

        TRM6         -   6 node isoparametric triangle

        QUM8         -   8 node isoparametric quadrilateral


Unless specifically requested, the elements are plane stress elements lying in 3-D space with three degrees of
freedom per node. Special options convert them to plane strain, generalised (engineering) plane strain, or plane
stress forms with two degrees of freedom per node. In generalised plane strain, the strain normal to the plane is
everywhere uniform, but not zero. As a general rule, quadrilateral elements are to be preferred to triangles and
the higher order elements with mid-side nodes to the lower order ones.




3.1.3       Axi-symmetric Solid Elements

These elements are intended for the idealisation of 3-D solids with a rotational axis of symmetry, under
rotationally symmetric loading and support conditions

        TRX3         -   3 node isoparametric triangular toroid

        QUX4         -   4 node isoparametric quadrilateral toroid

        TRX6         -   6 node isoparametric triangular toroid

        QUX8         -   8 node isoparametric quadrilateral toroid


In general the higher order elements (QUX8 and TRX6) are better performers than the lower order ones and
quadrilaterals are to be preferred to triangles.




3.1.4       Three-Dimensional Solids

The brick family are applicable to general 3-D solids under arbitrary loading.

        BRK6         -   6 node isoparametric pentahedron (wedge)

        BRK8         -   8 node isoparametric hexahedron

        BR15         -   15 node isoparametric pentahedron (wedge)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-2
ASAS (Non-Linear) User Manual                                                                          Program Features


        BR20         -   20 node isoparametric hexahedron

        LB15         -   15 node isoparametric laminated pentahedron (wedge)

        LB20         -   20 node isoparametric laminated hexahedron


BR15 and BR20 are to be preferred in most situations to BRK6 and BRK8 due to their superior performance and
versatile shape.




3.1.5       Gap/Interface Elements

A family of gap/contact and interface elements are available to model interface problems in two and three
dimensions. Frictional forces can be included.

Gap elements are available to model node-to-node contact between two flexible structures.

        GAP2 -can be used freely with the 2-D and 3-D elements but it is recommended that they interface with
        the lower order elements.

        GAPR-can be used to model tube-in-tube or external contact between two parallel tubes.

        GAPX -is compatible with all the axisymmetric elements, but the lower order elements are to be
        preferred.


Rigid surface interface elements are available to model contact between a structure and a rigid surface.

        RGX3-rigid surface interface for use with lower order axisymmetric solid elements

        RGX4-rigid surface interface for use with higher order axisymmetric solid elements

        RG23-rigid surface interface for use with lower order 2-D plane elements

        RG24-rigid surface interface for use with higher order 2-D plane elements




3.1.6       Plates, Shells and Beams

The plate and shell elements are isoparametric elements with six degrees of freedom per node. They are thick
curved elements with transverse shear flexibility. The interpolation for the in-plane stretching behaviour is quite
independent of the interpolation for bending. By using reduced integration they are in general satisfactory for
both thick and thin shells (say diameter- thickness ratios of up to 1000).

        QUS4         -   4 node quadrilateral facet shell.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-3
ASAS (Non-Linear) User Manual                                                                          Program Features


       TCS6          -   6 node generally curved triangular shell

       TCS8          -   8 node generally curved quadrilateral shell

       TCS9          -   9 node generally curved quadrilateral shell


Three elements are available to model stiffeners.

       STF4          -   3 node isoparametric beam element with range of (closed) cross-sections

       SST4          -   3 node isoparametric beam element with arbitrary open cross-section (no warping)

       WST4          -   3 node isoparametric beam element with arbitrary open cross-section allowing warping
                         (7 degrees of freedom per node)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-4
ASAS (Non-Linear) User Manual                                                                          Program Features


Two two-noded engineering beams are available.
        BEAM         -    2 node 3-D beam element, transmitting both axial forces and bending moments and
                          suitable for most 3-D frames includes rigid offsets

        BM2D         -    2 node 2-D beam for plane frames subject to in-plane loading, allows for rigid offsets.

        BM3D         -    2 node 3-D beam element, transmitting both axial forces and bending moments, suitable for
                          most 3-D frames, which allows for the effect of shear deformation, arbitrary local axes, and
                          rigid offsets.

        TUBE         -    2 node 3-D beam element with hollow circular cross-section which allows for arbitrary
                          local axes and rigid offsets.




3.1.7       Spring/Dashpot Elements

These elements are linear or non-linear spring and/or dashpot elements with stiffness and/or damping in one
specific direction. This line of action can be fixed or varied with deformation.

        SPR1         -   2 node spring/dashpot element with translational freedoms

        SPR2         -   2 node spring/dashpot element with rotational freedoms




3.1.8       Linespring Elements

These elements are used to model surface flaws on a shell structure. Plasticity can be included.

        LSP3         -   3 node linespring element for use with higher order shell elements on a symmetric
                         boundary

        LSP6         -   6 node linespring element for use with higher order shell elements




3.1.9       Uniaxial Field Elements

These elements are 1-D field elements used to represent uniaxial conduction, etc.

        FAT2        -    2 node uniaxial field elements

        FAT3        -    3 node uniaxial field elements




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-5
ASAS (Non-Linear) User Manual                                                                          Program Features


3.1.10      Two Dimensional Plane Field Elements

These elements are used to represent plane or 2-D regions in a field analysis. No through-thickness variations of
the field variable is permitted.

       TMT3         -    3 node triangular field element

       QMT4         -    4 node quadrilateral field element

       TMT6         -    6 node curved triangular field element

       QMT8         -    8 node curved quadrilateral field element




3.1.11      Three Dimensional Solid Field Elements

These elements are used to represent 3-D continuum regions in a field analysis.

       BRT6         -     6 node isoparametric wedge field element

       BRT8         -     8 node isoparametric hexahedron field element

       BT15         -     15 node isoparametric wedge field element

       BT20         -     20 node isoparametric hexahedron field element




3.1.12      Axisymmetric Solid Field Elements

These elements are used to represent 3-D axisymmetric continuum regions in a field analysis.

       TXT3         -     3 node isoparametric triangular field toroid

       QXT4         -     4 node isoparametric quadrilateral field toroid

       TXT6         -     6 node isoparametric triangular field toroid

       QXT8         -     8 node isoparametric quadrilateral field toroid


3.2    Material Model Types

Several constitutive laws are available for material modelling. They are divided into groups of elasticity,
plasticity, creep and failure. In general all material models require elastic material data and usually data for a
plasticity, creep or composite failure model also. In addition, a user material interface is provided for users to
define their own constitutive behaviour for a material. Details of all material models are given in Appendix -B.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-6
ASAS (Non-Linear) User Manual                                                                          Program Features


Each material used in the analysis is identified by a number (the material integer) which is referenced by all
elements comprised of that material. The same material integer is used for all the properties of a single material
(i.e. for elastic, plastic and creep data).

All material properties may be temperature dependent. The relevant material values are specified at a set of
reference temperatures and the program interpolates between them for the material properties at any required
temperature.




3.2.1       Elasticity

Elasticity covers both linear elastic and non-linear elastic (temperature dependent or hyperelastic material)
models. For linear elasticity, the material can be either isotropic, orthotropic, woven, anisotropic or laminate.

For isotropic linear elastic material, the modulus of elasticity, Poissons ratio, coefficient of linear expansion and
density are generally required.

For orthotropic or woven material, the density, the three principal values of Young’s modulus, shear modulus,
Poisson’s ratio and expansion coefficient are required.

Anisotropy is defined by giving either the coefficients of the general material elasticity matrix (i.e. the stress-
strain relation) or the coefficients of the compliance matrix (i.e. strain-stress relation), together with the
coefficients of linear expansion and density. The amount of information required for anisotropic material will
vary with the type of element for which it is being used. The requirements of each element type are detailed in
Appendix -A.

Laminate material is used to define composite shells and the density of the laminate may be provided. The layup
configuration and the materials used in the laminate are defined as geometric properties.

The hyperelastic material model implemented in ASAS-NL is a modified form of the Mooney-Rivlin model
which extends the original model to the compressible range. The Mooney-Rivlin model is associated with the
analysis of rubber-like materials which are almost incompressible with the bulk modulus a few orders of
magnitude larger than the shear modulus. The well known difficulties associated with this incompressibility for
finite element solutions are overcome in ASAS-NL by modifying the volumetric part of the strain-displacement
relationship. This involves a reduced order of pressure interpolation which is specified by the user as required.
The Mooney-Rivlin hyperelastic material model requires two constants, C10 and C01 to be specified by the user.




3.2.2       Plasticity

Plasticity is the generic term used in ASAS-NL to describe all time-independent non-reversible material
behaviour. It includes not only the classical plasticity theories applicable to most metals, but also some simple
theories to account for the behaviour of soils, rocks and concrete.

There are two requirements of any definition of plastic behaviour:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-7
ASAS (Non-Linear) User Manual                                                                          Program Features


(i)        A yield criterion to define the stress level at which plastic deformation first occurs and which also
           provides the constitutive relationship between plastic strains and stresses. ASAS-NL has been developed
           to allow separate specification of yield criterion and flow rule and hence wide generality. However, all
           material models of the current version have an associative flow rule implemented and the more general
           capability is not yet utilised.

(ii)       A hardening rule to define how the yield criterion is modified by subsequent plastic deformation.



3.2.2.1 Yield Criteria

The following yield criteria are available:
       •      Von Mises

       •      Tresca

       •      Ivanov

       •      Mohr-Coulomb

       •      Drucker-Prager

       •      Tension Cut

       •      Beam Stress Resultant

       •      Coulomb Friction

       •      Inelastic Spring


Both von Mises and Tresca criteria are widely applied to the behaviour of metals, but experimental evidence
generally favours von Mises. The Tresca criterion is frequently used, on account of its simplicity, in analytical
solutions and is useful for validation purposes.

The Ivanov yield criterion is applicable only to plate and shell behaviour and thus is restricted to certain
elements. Yield is defined in terms of through thickness stress resultants (i.e. forces and moments per unit
width).

Both Mohr-Coulomb and Drucker-Prager criteria are applicable to soils and rock-like materials. Implicit in
these criteria is a dependence on the hydrostatic stress, which is a pre-requisite of any attempt to model soil
behaviour.

The tension cutcriterion is applicable to model concrete cracking. Failure is defined in terms of principal
stresses.

The beam stress resultant yield criterion is applicable only to the engineering beams. Yield is defined in terms of
stress resultants and the whole section is assumed to plastify instantaneously.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-8
ASAS (Non-Linear) User Manual                                                                          Program Features


The Coulomb friction criterion is only available for rigid surface elements (and implicitly to gap elements) to
model the interface behaviour.

The inelastic spring model is only applicable to the spring elements. This can be used to model the hysteretic
behaviour under cyclic loading.


3.2.2.2 Hardening Rules

Unless specifically requested, the program assumes that isotropic hardening (or softening) occurs.                   This
corresponds to the yield surface expanding uniformly about the origin (for example a uniaxial model under
cyclic loading yields at the same value in both tension and compression and no Bauschinger effect is
reproduced). Isotropic hardening is usually satisfactory for problems where unloading does not occur and indeed
for cyclic loading of work hardened metals.

Kinematic hardening is available on request. The yield surface translates as a rigid surface upon plastic
deformation. With the Prager type the direction of travel is normal to the yield surface at the point concerned
and is applicable only to solids and axisymmetric solid elements. Ziegler type hardening is an attempt to
generalise Prager’s hypothesis to reduced stress spaces and results in the yield surface translating in the direction
of the stress vector. A combination of either kinematic forms with isotropic hardening is available by giving the
ratio of kinematic to isotropic hardening (see Appendix -B for further details).

The work hardening behaviour is defined by the material’s uniaxial stress-strain curve. This curve is specified
by a tabular representation of point values for varying temperatures. Linear interpolation between these point
values is used which effectively idealises the curve as a series of line segments and can be considered as
equivalent to specifying a series of slopes. A special case of this type of description gives a bi-linear work
hardening or perfectly plastic model if required.

In the absence of other directives then von Mises yield criteria and the associated Prandtl-Reuss flow equations
with isotropic hardening are assumed. The user then need take no further action.




3.2.3       Creep

Creep is the generic term used in ASAS-NL to describe all time dependent material behaviour. Creep and
plasticity models cannot be used concurrently in any one load step.

The creep material model requires the definition of a uniaxial creep strain rate and to extend this to multiple axes
the Mises potential function and associative flow rule are used. Four general ‘In-Built’ equations (“Laws”) are
available for the uniaxial creep strain rate and these optionally include strain or time hardening. The constants
for the equations are supplied by the user to match the material being modelled. If the required behaviour cannot
be defined by these then user-supplied subroutines may be added to the program to define the uniaxial rate as a
function of stress, strain, time and temperature.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 3-9
ASAS (Non-Linear) User Manual                                                                          Program Features


If supplying a creep subroutine users should note that many commonly used primary creep laws yield an infinite
creep rate at zero time which can cause numerical problems in the program. This can be avoided by suitable
adjustment of the creep law for times close to zero, or by providing a small offset to the time axis.

It is also important to ensure that any implied system of units in the creep law is consistent with the units being
used in the analysis.




3.2.4       Failure

Failure material models are used in ASAS-NL to describe the material failure behaviour of composite laminates.
Failure material properties may be specified to define the strength properties of a lamina, the strength properties
of the whole laminate, or, the parameters required for in-built or user defined failure laws.




3.2.5       Field

Field material properties are used in ASAS-NL to describe the ‘material’ properties for the field elements. The
actual type of properties will depend on the field problem being analysed. For example, if the electrical field
problem is being analysed, the properties will relate to the electrical conductivities.




3.2.6       Piezo-Resistivity

Piezo-resistivity material properties are used in ASAS-NL to describe the properties of a piezo-resistive material
for the coupled stress/electrical conduction problem.




3.2.7       Heat Convection

This type of material is used in ASAS-NL to model general non-linear convective heat transfer in a heat
analysis.




3.2.8       Heat Radiation

This type of material is used in ASAS-NL to model radiant heat transfer in a heat analysis.

3.3     Loading

Within ASAS-NL the word ‘LOAD’ signifies any externally imposed influence and includes prescribed
displacements and temperatures. Any number of different load types may be combined together and their




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-10
ASAS (Non-Linear) User Manual                                                                          Program Features


proportions may vary over the load history (i.e. the loading can be ‘non-proportional’). Only one loadcase can
be analysed in a single analysis.

The individual load types are listed in the following sections.




3.3.1       Nodal Loads

A nodal load is a force or moment associated with a freedom at a node. Loads may be applied in skew directions
by use of skew systems (see Section 3.6).




3.3.2       Prescribed Displacements

Prescribed displacements may be imposed on any nodal freedoms, in skew directions if required. The user first
specifies which freedoms are to be prescribed and then quotes displacement values for them. The nodal
reactions associated with each prescribed freedom are calculated automatically by the program.




3.3.3       Pressure Loads

A constant or spatially varying pressure distribution may be applied to any set of element faces. The distribution
is defined by the pressure values at the nodes on the faces. The default direction in which the pressure acts
depends on the element type and is described for each element in Appendix -A. Pressure can also be applied in
a specific direction.

For large displacement problems the pressure load is of non-conservative (follower) character. If required, this
however can be changed by the user to conservative load type (see Section 5.1 GROU/PROB/TITL command).




3.3.4       Distributed Loads

Distributed loads and intermediate point loads can be applied to some types of element as described in
Apprendix A




3.3.5       Temperature Loads

The effect of thermal straining due to a given temperature distribution can be determined. The distribution can
be defined at the nodes or on elements. Temperature loads are calculated from the difference between the
supplied nodal temperatures and a pre-specified reference temperature. (The latter is taken as zero unless
specified otherwise - see Section 4.3.4.) The required nodal temperatures can either be specified directly or




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-11
ASAS (Non-Linear) User Manual                                                                          Program Features


obtained from ASASHEAT using the HOTRAN program. (For details of the latter see the ASASHEAT User
Manual).

On higher order elements, with mid-side nodes, only corner node temperatures are required. The program will
over-ride, with interpolated values, any supplied temperatures for mid-side nodes.

Temperature fields which are discontinuous across element boundaries, can either be applied by using Groups
with nodal temperatures or element temperatures.

For problems with temperature dependent material data, material properties are evaluated at the supplied nodal
temperatures and the reference temperature is not used.




3.3.6       Face Temperature

The effect due to a difference of temperature through the thickness of a shell element can be determined. The
program requires the temperatures of both faces at some or all of the nodes. Alternatively, the face temperature
values on some or all of the elements can be specified.

On higher order elements, with mid-side nodes, only corner node temperatures are required. The program will
over-ride, with interpolated values, any supplied temperatures for mid-side nodes.

Temperature fields which are discontinuous across element boundaries, can be applied by using Groups.

For problems with temperature dependent material data, material properties are evaluated at the mid- surface
temperatures (i.e. average of top and bottom surfaces) and the reference temperature is not used.




3.3.7       Body Forces

Self weight, or the effect of uniform acceleration fields, are provided by this load type. The user specifies the
components of acceleration along each of the three global axes, and the body forces are automatically
determined for these acceleration components for all elements in the model. A density value must be specified
for all materials. The units of density and acceleration must be consistent with the units used in the remainder of
the data (see Section 3.11).




3.3.8       Centrifugal Loads

Centrifugal loading is available for most elements. It is applied by specifying the centre of rotation, together
with the angular velocity about each of the three global axes. A density value is required for all materials. The
units of density and angular velocity must be consistent with the units used in the remainder of the data (see
Section 3.11).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-12
ASAS (Non-Linear) User Manual                                                                          Program Features


3.3.9       Angular Accelerations

Angular acceleration loading is available for most elements. It is applied by specifying the centre of rotation
together with the values of angular acceleration and/or velocity about each of the three global axes. A density
value is required for all materials. The units of density, angular acceleration and velocity must be consistent
with the units used in the remainder of the data (see Section 3.11).




3.3.10      Nodal Fluxes

A nodal flux is a flux associated with freedom T at a node. This load type applies to field analysis only.




3.3.11      Prescribed Field Variables

A prescribed field variable may be imposed on the nodal freedom in a field analysis. The user first specifies
which freedoms are to be prescribed and then quotes values for them. The nodal reacted fluxes associated with
each prescribed freedom are calculated automatically by the program.




3.3.12      Flux Densities

A constant or spatially varying flux density distribution may be applied to any set of element faces or volumes.
The distribution is defined by the flux density values at the nodes on the faces or elements.




3.3.13      Wave Load

The loading due to wave, wind and current on fixed offshore structures may be included with this load type. The
envionmental loads are only applied to BEAM, BM3D and TUBE elements.




3.3.14      Tank Loads

If a floating structure has internal tanks that are filled with fluid, the combination of gravity and any motion of
the vessel will cause pressure loads on the walls of those tanks. By specifying the tank geometries together with
the internal fluid levels and densities, ASAS(NL) can automatically calculate the pressure loads on the tank
walls.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-13
ASAS (Non-Linear) User Manual                                                                          Program Features


3.3.15      Load History

The load history (or load sequence in time independent problems) and the corresponding response of the model
is defined by reference to a ‘pseudo-time’ axis. For other than creep or dynamic analyses pseudo-times have no
physical meaning; their values are used only to sequence the application of load and identify the increments.

Unless directed otherwise the program assumes a load history corresponding to a single application of a
proportionately increasing load.

More complex load histories may be specified in one of two ways. Firstly, the complete spatial load distribution
can be defined explicitly at each required pseudo-time. Proportional loading is implied between each load state.
This is usually the most convenient way when there are relatively few such load sets. Alternatively, a load
history may be specified by supplying a set of ‘load functions’ to define a few reference load states. The
functions define the proportion of each of the reference load’s components to be applied at any pseudo-time.
This allows quite general application of non-proportional loading.

For problems with cyclic loading, there is provision to repeat automatically a given load history any number of
times.

3.4      Node Numbers and Coordinates

Each node in the finite element idealisation must be given a unique positive integer number, so that an element
can be identified unambiguously by the node numbers on its boundaries. The shape and orientation of an
element is determined by the coordinates of these nodes.

If the structure has N nodes, the node number need not necessarily be within the range 1 to N; gaps in the
numbering are allowed and are often helpful. The gaps should preferably be small (eg. less than N).

The geometry of the elements and of the structural model is defined by the coordinates of the nodes. In general,
the coordinates must be supplied for all nodes on the structure. However, for elements with straight edges the
coordinates of any mid-side nodes can be calculated by the program.

The coordinates of a node or group of nodes may be defined in any convenient rectangular cartesian, cylindrical
polar or spherical polar coordinate system. An idealisation may use several of these coordinate systems. The
only exception is an axisymmetric idealisation where the cylindrical polar coordinates which are implicit in the
element must be input as a cartesian system.

The relationship of coordinate local axes or skew systems to the global system is given by the direction cosines
of their axes relative to the global axes. Each direction cosine gives the projection of a unit vector along the
skew axis on to the global axis. Skew systems must be right-handed and orthogonal.

It is only necessary to specify two of the axes; the third is computed automatically. If X’, Y’, Z’ represent the
skew axes, and X, Y, Z the global axes, ASAS-NL requires the six direction cosines:

         X’X, X’Y, X’Z, Y’X, Y’Y, Y’Z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-14
ASAS (Non-Linear) User Manual                                                                          Program Features


where, for example X’X is the projection on to the global X axis of a unit vector along the skew X’ axis. For a
2-D system within the X-Y plane, both X’Z and Y’Z will be zero.

As an alternative to specifying the direction cosines of the local axis system with respect to the global axis
system, a set of three node numbers may be used to identify the skew system, with ASAS-NL automatically
calculating the direction cosines (see Section 5.2.7.2).

3.5    Element Numbering

The program numbers elements automatically in the order in which they are first defined (the “input element
number”). Alternatively users can number each element explicitly (“user element number”). The user element
number (which defaults to the input element number if it is not given) is used as an identifier to specify the
group structure, integration rules and order of output.

Elements are defined by their constituent node numbers. The starting node and order of numbering (clockwise
or counter-clockwise) determines the direction of the local curvilinear axes. (See Appendix -G).

The program reorders the elements internally (the “system element number”) in an attempt to keep the maximum
frontwidth as small as possible. It allocates system element numbers on the basis of least node number order.
Elements are then assembled into the front of this order. Special options may be used, however, to suppress this
reordering and to use either the user or input element order within the solution process. (See MYEL and INEL
options)

If no attention has been paid to the node number sequence, which will effect the order of system element
numbering, the frontwidth optimiser can be invoked, using the PASS command, to reduce the incore frontwidth.
Five different methods are available in the program, namely CUTHILL-MCKEE, KING, LEVY, PINA and
SLOAN. CUTHILL-MCKEE is basically an algorithm for out-of-core bandwidth reduction but it may also be
used to optimise the incore frontwidth effectively. The others, however, are all methods for incore frontwidth
optimisation but, apart from SLOAN, they do take significantly more time to do the optimising (typically an
order of magnitude or more per pass compared with CUTHILL-MCKEE). This increase can be offset by use of
the user defined START node facility to reduce the number of passes attempted. The revised system element
ordering is carried out internally without renumbering the nodes and therefore its operation is transparent to the
user. Since the element ordering will be changed when using the frontwidth optimiser, the user or input element
order options should not be specified.

3.6    Global and Local Axis Systems

Regardless of the system(s) used to define coordinates, the displacement freedoms within ASAS-NL are usually
referred to the global axis system. This is a right-handed rectangular cartesian (X,Y,Z) system, except for the
axisymmetric elements, which use a cylindrical polar system (R,Θ,Z). In some cases the global axis system is
replaced for selected nodes or elements by a local axis system. There are three broad types of these: coordinate
local axes, element local axes and nodal local axes. The latter are known as ‘skew systems’.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-15
ASAS (Non-Linear) User Manual                                                                          Program Features


3.6.1       Coordinate Local Axes

Coordinate local axes are used to define the positions of nodes in space. Any required combination of cartesian,
cylindrical polar or spherical polar systems may be used; all of them are transformed to the global system within
the program. For each local system, the user provides the origin and the direction cosines relative to the global
system. Coordinates may, of course, be entered directly in the global system if required.




3.6.2       Element Local Axes

Many types of element have their own local axes. These are used as the reference frame for stress and strain
results and also, in certain elements, for the geometric properties. The direction of the element local axes is
defined by the order and location of the nodes on the elements and in large displacement analyses will vary
throughout the analysis. Full details are given in the relevant element description sheets in Appendix -A.




3.6.3       Skew Systems

Skew systems, otherwise known as nodal local axes, can be used for three purposes:

(i)     To specify suppressions, prescribed displacements or constrained freedoms (see Section 3.7) in directions
        other than those of the global axis system. All output of displacements and reactions is related to this new
        axis system. Only one such skew system is permitted at a node.

(ii)    To specify nodal loads in a direction other than the reference system, where the reference system is either
        the global system or the global system as modified by a skew system defined in (i). For example, if a
        node is skewed to allow a skew suppression, and a nodal load is required in the global direction, then a
        further skew system is required to ‘re-skew’ the load back to the global system. Nodal loads applied with
        a skew system are transformed to their components in the reference system described above. The axis
        system at the node is not altered and hence any number of skew systems may be applied at a node to
        accommodate various skewed nodal loads.

        Each skew system is defined by a unique integer number - the skew integer. The same skew system may
        be referred to in several places in the data.

        The relationship of coordinate local axes or skew systems to the global system is given by the direction
        cosines of their axes relative to the global axes. Each direction cosine gives the projection of a unit vector
        along the skew axis onto the global axis. Skew systems must be right-handed and orthogonal. See
        Section 5.2.7.1.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-16
ASAS (Non-Linear) User Manual                                                                          Program Features


        It is only necessary to specify two of the axes: the third is computed automatically. If X’, Y’, Z’
        represent the skew axes and X,Y,Z the global axes, ASAS-NL requires the six direction cosines:



                                                X’X, X’Y, X’Z, Y’X, Y’Y, Y’Z

        where, for example, X’X is the projection onto the global X axis of a unit vector along the skew X’ axis.
        For a two-dimensional system within the X-Y plane, both X’Z and Y’Z will be zero.

        A skew system may also be defined in terms of 3 points whose coordinates are defined in the coordinate
        data. See Section 5.2.7.2.

(iii)   To specify the direction of the data supplied for anisotropic material properties. Anisotropic material
        properties normally align with the element local axis system or the global axis system. By specifying a
        skew integer on the material property data line it is possible to input material data in an alternative
        direction. See Appendix B.1 for further details.


3.7     Structural Suppressions and Constraints

The movement of a node in any direction may be restrained by applying ‘suppressions’, or given a value by
applying ‘prescribed displacements’. These may be applied to any freedom existing at the node and may be
related to the global axis system or to a skew system defined for the purpose. (The freedoms at a node are
determined by the elements meeting at the node.) ASAS-NL automatically calculates the reactions associated
with such restraints. A freedom may also be made to depend linearly on any number of other freedoms by
means of ‘constraint equations’.

For static analysis, it is essential to ensure that there are sufficient restraints on the idealised model to prevent
any possibility of it behaving as a mechanism. In particular, the model or any part of it,should be prevented
from moving or rotating as a rigid body.

3.8     Solution Procedures



3.8.1       Non-Linear Static Solution Procedures

The non-linear static solution procedures available in ASAS-NL are conventional incremental ones, with
iterative correction within the increment. The user has wide ranging capabilities to control the nature and size of
the increment, and to vary the frequency of updating of the stiffness matrix, the required number of iterations,
convergence criteria and restart procedures to be invoked in the event of non-convergence.

The solution procedure commences by incrementing one of the following quantities (chosen by the user)

                Generalised Load




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-17
ASAS (Non-Linear) User Manual                                                                          Program Features


                Single Displacement Component

                Displacement Vector Length (“arc-length” method)

                External Work Measure


and then holding a value of the selected quantity constant throughout the iteration process.

The above procedures may be freely combined with any of the following iteration techniques

                Standard Newton Raphson

                Modified Newton Raphson

                Initial Stiffness.


In all cases the iteration process can be accelerated by employing

                Secant-Newton

        or      Line Search


techniques.

The Load Incrementation procedure is most suitable for cases of non-proportional loading. The other procedures
are useful for problems involving multi-valued load-displacement relationships such as ‘snap-through’.

Solution procedures usually can be changed during the course of an analysis. In addition analyses may be re-
started from previous load increments using a different solution strategy if required.

Appendix -C describes the inter-relationship of the different methods.

The size of increment, which may be either load or displacement, is normally determined by the user. However,
in problems with proportional loading, the program can automatically determine initial plastic yield (or scale to a
user defined level).

Convergence is, by default, assessed against residual forces. Displacements, element strains, stresses or total
work may also be used.

Computation of stresses adopts the Forward Euler Integration Scheme by default and sub-incremental
procedures for plastic stress redistribution may be used in conjunction with any solution procedure upon request.
For von Mises yield criterion, Backward Euler integration scheme may also be used.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-18
ASAS (Non-Linear) User Manual                                                                          Program Features


3.8.2       Non-Linear Transient Solution Procedures

Non-linear transient solution procedures are used in ASAS-NL to solve creep (time-dependent material
response) problems, structural dynamics problems and transient thermal problems. These types of problems use
a finite difference in time where the solution is advanced in a stepwise fashion using finite increments of time
(time steps). Two distinct types of solution procedures are available; implicit and explicit schemes. The implicit
scheme has the advantages of unconditional stability and allows larger timesteps compared to the alternative
explicit scheme. The iterative nature of the implicit scheme ensures, in general, greater accuracy but at a much
computational cost. In structural dynamics the two schemes may be combined in a single analysis to take of the
benefits of both schemes. In addition to defining the list of solution times manually, automatic timestepping
procedures are also available for both types of transient analyses. Further details concerning creep analysis may
be found in Appendix -J. Further details concerning structural dynamics analysis may be found in Appendix -K.
Further details concerning transient thermal analysis may be found in Appendix N.




3.8.3       Contact Analysis Solution Procedures

By default, the penalty method is adopted to solve problems involving gap and rigid surface elements. For rigid
surface contact, the augmented Lagrangian method may be used upon request. Further details for these two
methods are given in Appendix C.6.




3.8.4       Fracture Mechanics Solution Procedures

Depending on the nature of an analysis, fracture mechanics analysis may be performed in one of the following
ways:

(i)     Surface flaws on shell structures - use linespring elements and perform the analysis using any of the non-
        linear static solution procedures

(ii)    Cracks on 2-D planar or axisymmetric structures - perform the analysis as usual and save the appropriate
        results on the post-processing file for POSTNL to evaluate the fracture mechanics parameters (e.g. J-
        integral) (see Appendix I.8)


3.9     Program Organisation

ASAS-NL makes extensive use of files and it is helpful to classify these as either internal or external files.
INTERNAL files are used for intermediate storage within a program and are deleted upon successful completion
of the program.        EXTERNAL files are permanent and are used for transporting information between the
programs and between successive restarts. The user need not normally concern himself with internal files, but
some understanding of the external file organisation is required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-19
ASAS (Non-Linear) User Manual                                                                          Program Features


When a restart is attempted information describing the current state of the analysis is required. Thus ASAS-NL
allows the user to archive (or save) all relevant information at the end of any increment. This information is
stored on two labelled external backing files. One file, called the STIFFNESS MATRIX ARCHIVE FILE (or
stiffness file) contains all the element stiffness matrices for the model. The other file, the DATA-MANAGER
ARCHIVE FILE (sometimes abbreviated to archive file) contains all other necessary information such as model
description, control parameters, load history, stresses and displacements. When the information is written to the
archive files, an integer number known as the CHECKPOINT number is used to identify the position of the
archived information on the backing file for that load increment and is printed in the output file when the
archiving has been accomplished. The two backing files are checkpointed separately.

When a restart is attempted, the internal file structure is re-created from the archived backing files using the
checkpoint number supplied by the user in the restart data.

Distinction is made between ‘OLD’ and ‘NEW’ files in ASAS-NL to distinguish between the two pairs of files
used in a restarted analysis.           Backing files created by ASAS-NL (as output) are referred to as ‘NEW’
(Newarchive and Newstiffness) whilst backing files read by ASAS-NL (as input in restarts for instance) are
referred to as ‘OLD’ (Oldarchive and Oldstiffness). For example, the data manager archive file named, say
NLARCHIVE, by the user is understood to be the newarchive file when created but the oldarchive file when
read by ASAS-NL when the restart is attempted.

ASAS-NL also makes full use of the ASAS file system. All the runs associated with a particular analysis, i.e.
the initial run and any restarts and post-processing runs, must be under a common project name. This name is
used to set up a project index file (the 10 file) which stores the details of every run carried out in this project.

The ASAS backing files created during a run are controlled by the structure name specified. A unique structure
name must be assigned for each run within the same project.

3.10 Post-Processing

A post-processing program called POSTNL is available to provide an interface for transferring ASAS-NL results
to a number of graphical display programs and to perform certain additional post-processing calculations. The
information saved on the post-processing file is specified by the POST or RESU command in the preliminary
data.

In addition, post-processing of ASAS-NL results may also be carried out using standard ASAS post-processors
such as BEAMST, AXL and AMC. As before, the POST/RESU Command in the preliminary data is required to
specify the information to be saved on the ASAS database. The increment number where results are saved will
be recognised as the user load case number by the ASAS post-processors.

3.11 Data Units
The user is free to choose any system of units for his data, provided that the units employed form a consistent
system so that all data are defined using the same units of force and length. It is also possible to define explicitly
the units for the analysis. These can be locally overridden or changed within each data block if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-20
ASAS (Non-Linear) User Manual                                                                          Program Features


The basic global units to be employed are defined in the Preliminary data using the UNITS command (see
Section 5.1.42) where the units of force, length and, where appropriate, temperature are supplied. (Time is
assumed to be in seconds). These basic units will be utilised as the default input and results units.

In order to facilitate the utilisation of different units for the various types of data, a units command can be used
within the main body of the data to locally override the basic units defined in the Preliminary data. This facility
enables each data block to have one or more different sets of data units which may or may not be the same as the
global definitions.

The following example shows a simple structure where the basic global units are Newtons and Metres but the
geometric properties have been supplied in both millimetres and inches.

                                                                 Defined units                           Derived units
SYSTEM DATA AREA 5000000
PROJECT ASAS
STRUCTURE ASAS
JOB STAT
TITLE *EXAMPLE
SOLV 1.0
OPTIONS GOON END
UNITS    N    M                                                  Newtons Metres Kg
END                                                              Centigrade (default)
COOR
CART
1     0.0 0.0 0.0
2    10.0 0.0 0.0
3    20.0 0.0 0.0
END
ELEM
MATP 1
BEAM 1      2   1
BEAM 2      3   2
END
GEOM
UNITS    MM                                                      Newtons Millimetres                          Kgx10-3
1 BEAM 108.0 90.0 90.0 25.5
UNITS    INCHES                                                  Newtons Inches. See note 3 below
2 BEAM     12.0   5.0    5.0   3.2
END
MATE                                                             Newtons Metres                               Kg
1    2.0E11 0.3       0.0    0.0
END
..
.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-21
ASAS (Non-Linear) User Manual                                                                          Program Features



Notes


1.      The units defined in the Preliminary data must be given for both force and length. The temperature unit is
        optional and defaults to centigrade. The mass unit is a derived quantity consistent with the units of length
        and force specified.

2.      Locally defined units will be reset at the end of each data block or sub data block (see Section 5.1.42).
        Thus in the example above the units for the MATE data are reset to the global terms Newtons and metres
        automatically.

3.      In the second units definition in the GEOM data, the force and length units do not form a consistent set
        and so a mass unit cannot be derived. This is acceptable to the program provided that the data being
        defined do not require a mass or density input. Thus units of Newtons and inches would be unacceptable
        in the MATE data where the density is specified. Table 3.1 provides a list of unit definitions which
        permit the calculation of a consistent mass unit.

4.      Where mass data has to be supplied, the input can be simplified by locally choosing the appropriate units
        of force and length to provide a consistent unit of mass of either 1kg (using Newtons and metres) or 1lb
        (using Poundals and feet).

If units are employed, the cross checks and results will, by default, be printed in the basic global units defined in
the Preliminary data and any data defined using local unit definitions will be factored appropriately.

Where the UNITS command is not used, the user must ensure that all data utilise a consistent system of units
throughout. Three examples of consistent sets are shown below.
1.    SI Units :        Force in Newtons, length in metres, mass in kilograms, time in seconds, acceleration
                                 in metres/sec2
2.      Imperial Units :         Force in pounds, length in feet, mass in slugs, time in seconds, acceleration in
                                 feet/sec2
3.      Imperial Units :         Force in poundals, length in feet, mass in pounds, time in seconds, acceleration in
                                 feet/sec2

For any other set of units, the unit of consistent mass will be a multiple of the basic unit of mass because it is a
derived unit. The consistent unit of mass is obtained by dividing the unit of force by the acceleration due to
gravity, which itself has units of length divided by time squared. A change in the unit of length, for example
from feet to inches or metres to millimetres, requires a corresponding change to the unit of mass used for
calculating the density.

A list of sets of consistent units is given in Table 3.1




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-22
ASAS (Non-Linear) User Manual                                                                                  Program Features




                        Unit of         Typical value                               Consistent          Density (mass/unit volume)
Unit of force                                                         G
                        length           of E for steel                            unit of mass         Steel          Concrete
                                                 11
Newton             metre                2.1x10                 9.81               1Kg                   7850           2400
                                                 7                                                                -5
Newton             cm                   2.1x10                 981                100Kg                 7.85x10        2.40x10-5
Newton             mm                   2.1x105                9810               1000Kg                7.85x10-9      2.40x10-9
Kilopond           metre                2.14x1010              9.81               9.81Kg                800            245
Kilopond           cm                   2.14x106               981                981Kg                 8.00x10-6      2.45x10-6
Kilopond           mm                   2.14x104               9810               9810Kg                8.00x10-10     2.45x10-10
KNewton            metre                2.1x108                9.81               103Kg                 7.85           2.40
KNewton            cm                   2.1x104                981                105Kg                 7.85x10-8      2.40x10-8
KNewton            mm                   2.1x102                9810               106Kg                 7.85x10-12     2.40x10-12
Tonne (f)          metre                2.14x107               9.81               9.81x103Kg            0.800          0.245
Tonne (f)          cm                   2.14x103               981                9.81x105Kg            8.00x10-9      2.45x10-9
Tonne (f)          mm                   2.14x101               9810               9.81x106Kg            8.00x10-13     2.45x10-13
Poundal            foot                 1.39x1011              32.2               1lb                   491            150
                                                     8                                                            -2
Poundal            inch                 9.66x10                386                12lbs                 2.37x10        7.23x10-3
Pound (f)          foot                 4.32x1011              32.2               32.2lbs               15.2           4.66
                                                                                  (1 slug)
                                                 7
Pound (f)          inch                 3.0x10                 386                386lbs                7.35x10-4      2.25x10-4
Kip                foot                 4.32x106               32.2               3.22x104lbs           1.52x10-2      4.66x10-3
Kip                inch                 3.0x104                386                3.86x105lbs           7.35x10-7      2.25x10-7
Ton (f)            foot                 1.93x106               32.2               7.21x104lbs           6.81x10-3      2.08x10-3
Ton (f)            inch                 1.34x104               386                8.66x105lbs           3.28x10-7      1.0x10-7




                                       Table 3.1 Examples of Consistent Sets of Units

                                                         1 Kip = 1000 pounds force
                                                     1 Kilopond = 1 Kilogram force
                                                          All times are in seconds
                                            Assumed specific gravity of steel = 7.85
                                           Assumed specific gravity of concrete = 2.4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 3-23
ASAS (Non-Linear) User Manual                                                                          Program Features




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 3-24
ASAS (Non-Linear) User Manual                                                                          Data Preparation



4.      Data Preparation

4.1     General



4.1.1        Data

Data for ASAS-NL is prepared as a series of ‘data blocks’, each specifying a particular feature of the problem.
The data blocks are grouped into a number of sections such as structural description, boundary conditions,
loading, etc. These data blocks are shown in Table 4.1.

The various sections must be entered in order, but within each section the order of the data blocks can be varied,
although the user is advised to adopt the order shown. The sections for structural description, boundary
conditions, loading, additional mass and initial conditions collectively define the finite element idealisation. The
Preliminary data controls the solution of the problem including the type of material and structural behaviour that
is sought.

The Preliminary data is compulsory and all the data blocks of the structural description section must be present
except for the geometric properties and skew systems which are not always needed.

At least one data block from the boundary conditions section and one from the loading section must be present
for static analysis. For natural frequency analysis loading is optional. Other sections are optional.

In a restarted analysis only the Preliminary data, suppressions, displaced freedoms, loading and additional mass
can be changed. Initial conditions have no relevance.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-1
ASAS (Non-Linear) User Manual                                                                                                   Data Preparation



      Data Block Contents                                                                                                          Section
      Preliminary Data
                              Control Parameters.......... ....................................................................... 5.1
      Structural Description - Shape and Properties of the Model
                        Coordinates ..................... .................................................................... 5.2.2
                              Element Topology ........... .................................................................... 5.2.3
                              Material Properties .......... .................................................................... 5.2.4
                              Geometric Properties ...... .................................................................... 5.2.5
                              Section Information ............................................................................. 5.2.6
                              Skew System ................... .................................................................... 5.2.7
      Boundary Conditions - Restraints on the Model
                      Suppressions ................... .................................................................... 5.3.3
                              Displaced Freedoms ........ .................................................................... 5.3.4
                              Constraint Equations ....... .................................................................... 5.3.5
                              Rigid Constraints ............ .................................................................... 5.3.6
      Loading Applied to the Model
                      Nodal Loads .................... .................................................................... 5.4.3
                              Prescribed Displacements .................................................................... 5.4.4
                              Pressure Loads ................ .................................................................... 5.4.5
                              Distributed Loads ............ .................................................................... 5.4.6
                              Temperature Loads ......... .................................................................... 5.4.7
                              Face Temperatures .......... .................................................................... 5.4.8
                              Body Forces .................... .................................................................... 5.4.9
                              Centrifugal Loads............ .................................................................. 5.4.10
                              Angular Acceleration ...... .................................................................. 5.4.11
                              Nodal Flux ...................... .................................................................. 5.4.12
                              Prescribed Field Variable ................................................................... 5.4.13
                              Flux Density .................... .................................................................. 5.4.14
                              Wave Load ...................... .................................................................. 5.4.15
                              Tank Loads ..................... .................................................................. 5.4.16
                              Load Functions................ .................................................................. 5.4.17
      Additional Mass
                              Lumped Mass Values ...... ....................................................................... 5.5
      Initial Conditions
                              Residual Initial Stresses             ................................................................... 5.6.2
                              Stiffener Residual Initial Stresses ........................................................ 5.6.3
                              Initial Conditions for Transient Dynamic Analysis ............................. 5.6.4
      End of File
                              STOP Command ............. ....................................................................... 5.7

                                            Table 4.1 Data Blocks for ASAS-NL Data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                           Page 4-2
ASAS (Non-Linear) User Manual                                                                          Data Preparation


4.1.2       Data Formats


4.1.2.1 General Principles

The input data for ASAS-NL are specified according to syntax diagrams similar to that shown below. The
conventions adopted are described in the following pages. Detailed descriptions for each of the data blocks can
be found in Section 5

                     HEADER

                     KEYWORD                     (alpha)                               /integer/

                                                 KEYWORD1
                     real                                                              //integer//
                                                 KEYWORD2

                     integer                     KEYWORD3                              real

                     END




Each data block commences with a compulsory header line and terminates with an END command which delimit
the information from the other data. The sequence of the input data follows the vertical line down the left hand
side of the page. If a data block can be omitted, this will be indicated as shown below.


                     HEADER



                     END




Within each data block, each horizontal branch represents a possible input instruction. Input instructions are
composed of keywords (shown in upper case), numerical values or alphanumerics (shown in lower case
characters), and special symbols. Each item in the list is separated from each other by a comma or one or more
blank spaces.

Numerical values have to be given in one of two forms:

(i)     If an integer is specified a decimal point must not be supplied.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-3
ASAS (Non-Linear) User Manual                                                                          Data Preparation


(ii)    If a real is specified the decimal point may be omitted if the value is a whole number.


Exponential formats may be utilised where real numbers are required.

        for example               0.004         4.0E-3       4.0D-3       are equivalent

        similarly                 410.0         410          4.10E2       are the same.


Alphanumerics are any non-numeric strings which may include the letters A-Z, numbers 0-9, and the characters :
. , +     - and /. The letters A-Z may be supplied in either upper or lower case but no distinction is made
between the upper and lower case form. Hence “A” is assumed identical with “a”, “B” with “b” and so on.

        For example               CASE          are all permissible alphanumeric strings
                                  STR1
                                  END
                                  3mm

        also                      COMB          are all identical strings
                                  Comb
                                  comb


Alphanumeric strings must not include any special symbols (see below).

If certain lines are optional, these are shown by an arrow which bypasses the line(s)


                       real                               integer




In order to build up a data block, a line or series of lines may be repeated until the complete set has been defined.
These are shown by an arrow which loops back.

                        HEADER

                       real                               integer

                       END




Some data lines require an integer or real list to be input whose length is variable. This is shown by a horizontal
arrow around the list variable.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-4
ASAS (Non-Linear) User Manual                                                                          Data Preparation




                       real                               integer




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-5
ASAS (Non-Linear) User Manual                                                                          Data Preparation


Where one or more possible alternative items may appear in the list, these are shown by separate branches for
each
                                               KEYWORD1
                                                                                    integer
                   integer                     KEYWORD2


                                               KEYWORD3                             real




An optional item in a line will be enclosed in brackets e.g.

                   KEYWORD                             (alpha)                       integer




The relevant data block description in Section 5 will detail the default value adopted if the item is omitted.

An input line must not be longer than 80 characters. Certain input instructions may extend onto continuation
lines. Where this is allowable, the syntax diagram line is shown ending with an arrow (see Section 4.1.3).

                     KEYWORD                           integer




4.1.3          Special Symbols

The following is a list of characters which have a special significance to the ASAS-NL input.

*       An asterisk is used to define the beginning of a comment, whatever follows on the line will not be
        interpreted. It may appear anywhere on the line, any preceding data will be processed as normal. For
        example

        (i)          *     THIS IS A COMMENT FOR THE WHOLE LINE

        (ii)         X Y RZ 1 16 24 27 *support conditions at ground level*

’       single quotes are used to enclose some text strings which could contain otherwise inadmissible characters.
        The quotes are placed at each end of the string. They may also be used to provide in-line comments
        between data items on a given line. For example

                 BM3D         ’NODES’           1       2       ’GEOM PROP’               5




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-6
ASAS (Non-Linear) User Manual                                                                          Data Preparation



,      A comma or a blank will act as a delimiter between items in the line. For example

                5, 10, 15 is the same as 5                   10      15

       Note that two commas together signify that an item has been omitted. This may be permissible for
       certain data blocks. For example

                5,, 15

       Unless otherwise stated in the section describing the data block omitted numerical values are zero.

:      A colon at the start of the line signifies that the line is a continuation from the previous line.
       For example

                5                          is the same as             5     10     15
                :     10
                :     15

       Note that this facility is only available in certain data blocks. See the appropriate detailed description of
       each data block for details.

@      A command @filename may appear anywhere in a data file. When such a command is encountered, the
       input of data switches to the file filename and data continues to be read from that file until either the end-
       of-file is reached or an @ command is encountered in the secondary file.

       When the end of the secondary file is reached, that file is closed and input switches back to the previous
       data file. If, however, an @ command is found in the secondary file, input switches to yet another file.
       This process can continue until a maximum of 5 secondary files are open simultaneously.

       For example

                @prelim.dat
                @section1.dat
                @section2.dat
                @load.dat

       section1.dat might then contain the lines

                @coor.dat
                @elem.dat
                @mate.dat
                @geom.dat




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-7
    ASAS (Non-Linear) User Manual                                                                          Data Preparation


           finally

                     coor.dat contains the coordinate data
                     elem.dat contains the element data
                     etc


4.2        Data Generation Facilities



4.2.1           Repeat Facilities

Lists of regular data can often be shortened by use of a repeat facility. A block of one or more lines of data may
be identified by a delimiter character(/) and terminated by a repeat command (RP). The repeat command
contains information on how many times the set of lines of data is to be generated and how the data is to be
incremented for each generation. The general form is:

                       /

                       KEYWORD                               real                       /integer/

                       RP                                    nrep                        incr




/                     : delimiter character to identify the start of the data to be generated. It must be on a line of its
                           own

KEYWORD               : items not enclosed within two slashes will be repeated without any increment for generated
                           real            :        data

/integer/             : indicates the data in the line which may be generated using the repeat facility. The slashes
                           must not appear in the actual data

RP                    : command word to identify the end of the data to be generated

nrep                  : number of times the set of lines is to be generated, including the original data line(s)

incr                  : the increment to be added to the data items each time the block is generated

For example, suppose the data format is specified as

                      KEYWORD                                       /integer/




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 4-8
ASAS (Non-Linear) User Manual                                                                               Data Preparation


It is required to generate integers 1,6,11,16,21,26,31,36,41,46. If the keyword is ALL the data could be

        ALL            1    6       11       16        21       26       31        36       41          46

or

        ALL        1
        ALL       6
        ALL      11
        .
        .
        .
        ALL      46

Using the repeat facility, the following examples all produce the same identical data

        /
        ALL
        RP         10       5

or

        /
        ALL            1    6
        RP             5   10

or

        /
        ALL            1
        ALL            6
        RP             5   10




4.2.2        Re-Repeat Facilities

The repeat facility can be extended to include a double repeat whereby data which has been expanded by use of
the RP command may be repeated again with different increment values. The general form is




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 4-9
    ASAS (Non-Linear) User Manual                                                                          Data Preparation




                      //

                      /

                      KEYWORD                               real                       //integer//

                      RP                                    nrep                        incr1


                      RRP                                  nrrep                        incr2




//                    : identifies the start of the data to be re-repeated. It must precede a / line

/                     : identifies the start of the data to be repeated

KEYWORD               : items not enclosed within two slashes will be repeated without any increment for generated
                           real            :        data

//integer//           : an item enclosed by // characters indicates data which can be modified using the re-repeat or
                           repeat facility. The slashes must not appear in the actual data

RP                    : identifies the end of the data to be generated with the repeat facility

nrep                  : number of times the block of data is to be generated, including the original data line(s)

incr1                 : the increment to be added to the data items for the second and subsequent generated blocks.
                           (The first block corresponds to the original data)

RRP                   : identifies the end of the data to be generated with the re-repeat facility

nrrep                 : the number of times the expanded data from the repeat block is to be further generated,
                           including the original repeat block

incr2                 : the increment to be added to each of the expanded data items for the second and subsequent re-
                           generated blocks. (The first block corresponds to the expanded data items)

For example, taking the previous example, if the data syntax was specified as

                          KEYWORD                          integer




then the data could be

           //
           /
           ALL         1




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-10
ASAS (Non-Linear) User Manual                                                                          Data Preparation


        RP         5      10                           generates 1,11,21,31,41
        RRP        2       5                           generates 6,16,26,36,46

Note, the order of the numbers generated by this example in Section 4.2.1 using RP and in Section 4.2.2 using
RP and RRP is different. This may be important in a few cases where the order of the data supplied matters, for
example, the generation of user element numbers.




4.2.3       List Generation in the Preliminary Data Section

Many of the commands in the Preliminary data require a list of integer data items following the keyword. This
list can be created in a number of ways.


4.2.3.1 A Simple List

A simple list of integers can be written in free format with each number separated by a space or comma up to
column 80.

        Example:         1    6    11    16    17     18
                         1, 6, 11, 16, 17, 18



4.2.3.2 Generating a List with a Topological Variable

By use of ’topological variables’, a list of integers can be generated. This is very valuable for generating lists of
regular numbers. It is not so useful for irregular lists.

GENERATING A LIST OF NUMBERS USING ONE MODIFIER

The most basic form of topological variable has the form (L)(N,M1). This is used to generate a list of L numbers
at equal intervals. The first pair of brackets encloses the number L. The second pair of brackets encloses two
integers, separated by a comma. The first of these integers, N, is the start value and the second integer, M1, is
the increment for modifying the start value. Thus, the numbers N, N+M1, N+2M1, N+3M1 .......N+(L-1)M1 will
be generated.

Example:                 (4) (3, 5)

        This example will generate data for the four nodes 3, 8, 13, 18.


GENERATING A LIST OF NUMBERS USING TWO MODIFIERS

A more general form of the topological variables is as follows:

        (L)(N,M1,M2)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-11
ASAS (Non-Linear) User Manual                                                                          Data Preparation


This is used to generate a list of numbers at unequal intervals. Its application is similar to the topological variable
with a single modifier. The second modifier M2 is used to change the value of M1 every time the latter is used.
Modifiers may be positive or negative. The rules are as follows:

        (a)          The first number generated is the basic number N.

        (b)          The second number generated is N+M1.

        (c)          M1 is now modified by M2.

        (d)          The next number generated is the previous number modified by the new M1.

        (e)          Stages (c) and (d) are repeated until L numbers are generated.


Examples:

(i)     The topological (5) (7,3,12) variable will create a list 7, 10, 25, 52, 91 by expanding in the following way:

                First number generated:                      7

                Second number generated:             7+3         10

                New M1 = 3 + 12 = 15

                Third number generated:             10+15         25

                New M1 = 15 + 12 = 27

                Fourth number generated:            25+27          52

                New M1 = 27 + 12 = 39

                Fifth number generated:            52+39         91

(ii)    (4) (25,2,-6) generates 25,27,23,13

(iii)   (4) (2,0,3)                             generates 2,2,5,11

(iv)    (4) (25,2,-6)     (3) (2,3,3)           generates 25,27,23,13,2,5,11




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-12
ASAS (Non-Linear) User Manual                                                                          Data Preparation


4.3     Description of Each Data Block



4.3.1       The Preliminary Data


4.3.1.1 General

The Preliminary data is the first block of ASAS-NL data and consists of all the information required to control
the execution of the analysis. It can be divided into two sections, depending on whether the data applies to the
problem as a whole (Problem section) or whether it is specific to a given group (Group section). Commands for
the Problem section appear first and are then followed by Group section commands for each group in turn.
Groups are defined by their constituent elements, if none are explicitly given then the program treats all elements
as being in Group 1.

Collectively the Preliminary data fulfils the following functions

•       System control (see Section 4.3.1.2)

        This includes commands for naming and controlling backing files and setting the data area size. These
        commands only appear in the Problem section.

•       Solution algorithm definition (see Section 4.3.1.3)

        These commands determine the solution method to be used and control its performance (e.g.
        convergence) and again can only appear in the Problem section.

•       Model behaviour (see Section 4.3.1.4)

        Commands in this category control the type of structural and material behaviour that is to be modelled.
        This can vary from group to group.

•       Output control (see Section 4.3.1.5)

        This includes not only the control of printed results and diagnostic monitoring, which can vary from
        group to group, but also the saving of results on file for subsequent post-processing.



4.3.1.2 System Control

Commands in this category establish values of certain parameters controlling internal data storage and
workspace, and also control the use of backing files.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-13
ASAS (Non-Linear) User Manual                                                                          Data Preparation


The data area (freestore) required may be specified using the SYSTEM command. Its value is dependent on the
size of problem; guidelines are given in Section 6

The data-manager parameters are automatically set by the program, but may be re-set using the SYSPAR
command. Normally this will only be necessary for unusual jobs.

External files may be named and controlled by the data given with the PROJECT, STRUCTURE,
NEWSTRUCTURE, FILE, SAVE and, (in restarted jobs) JOB commands. Although the program has defaults
built in, it is recommended that, in all but the simplest of jobs, file names and status should be explicitly given.

Names of the files created by ASAS-NL are defined using FILE commands (except for the old data manager
archive file required in restart jobs, which is given with the JOB command). In addition, depending on the file
type, directives may also be required to define the file status (i.e. whether it is to be a ‘new’ file or whether an
existing one, and in the latter case whether information is to be appended or overwritten). These directives are
given using SAVE and FILE commands.

The ASAS backing file names are controlled by the PROJECT, STRUCTURE and NEWSTRUCTURE
(restarted jobs only) commands. These provide identification of the model for use by ASAS postprocessing
programs. As additional security, a label is attached to all external files. This label can be specified using the
PROJECT command. Subsequent restart jobs making use of the files must then have the same PROJECT
command.


4.3.1.3 Solution Algorithm

The solution procedure is controlled by information using the following commands.

1.     Either STAT using the JOB command, specifying the request for a nonlinear static incremental solution

       or TRAN using the JOB command, specifying the request for a transient solution procedure, i.e. including
       creep or dynamic effects.

       or HEAT using the JOB command, specifying the request for a steady state heat solution procedure.


2.     Either SOLVE or RESTART commands specifying the times (Pseudo or real times) at which a solution is
       to be performed. The SOLVE command is used for initial analyses; the RESTART command whenever
       an analysis is restarted. SOLVE/RESTART are mandatory for JOB type TRAN involving creep

       or SOLUTION or SRESTART commands specifying the number, size and nature of incremental steps at
       which a solution is to be performed. SOLUTION is used for initial analysis, SRESTART for restarts.
       Note that SOLUTION/SRESTART are not available with JOB type TRAN involving creep.
       SOLUTION/SRESTART should be used for structural dynamics problems employing an automatic
       timestepping procedure.

       Full details about the above methods are given in Appendix -C and Appendix -K.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-14
ASAS (Non-Linear) User Manual                                                                          Data Preparation


3.     UPDATE command specifying the frequency of reformation of the global stiffness matrix (UPDA STIF),
       the global mass matrix (UPDA MASS) and updating loads and geometry (UPDA GEOM). Using these
       commands, a range of Newton-Raphson type iteration techniques are available.

       The iteration can be accelerated with Secant Newton or Line Search techniques by using options SECN or
       LINS respectively using the OPTION command.

       Two methods of stress recovery are available. The default method is the Forward Euler integration
       scheme. Sub-incremental procedures for plastic stress redistribution compatible with this scheme can be
       requested by specifying the number of sub-increments using the PARAMETER command.                             The
       alternative is the Backward Euler integration scheme, requested by option BAKE using the OPTIONS
       command. Note that the Backward Euler integration scheme is only available with von Mises yield
        criterion.

        In case of diverging iteration an auto-recovery facility is available by specifying option AUTO using the
       OPTION command.

       In problems with proportional loading, an analysis may be scaled to first yield using the SCALE
       command. The analysis must then be restarted.


4.     CONVERGENCE command. The program will normally iterate until convergence is achieved. The
       required convergence criteria are defined using this command. If not given, appropriate default values
       are used.

5.     ITERATION command. The maximum number of iterations attempted within a load step is set by
       default to 10. The ITERATION command provides a means of modifying this. If convergence is not
       achieved within this number then the analysis will terminate unless the option OVIT is given using the
       OPTIONS command. In this latter case out of balance residual forces are carried over to the next load
       increment and the program continues. Directive NRES with the GROUP or PROBLEM/TITLE
       command will set the out of balance forces to zero at the start of a new increment.

6.     EIGN command specifies the times at which an eigenvalue analysis is to be performed. The type of
       eigenvalue analysis and the control parameters are defined using the SPIT command.


4.3.1.4 Model Behaviour

The material or structural behaviour is defined for each group as required. Each group is defined using a
GROUP command containing four character directives which, together with the directive using the JOB
command, determines the behaviour of the group. (If no group is explicitly given, then the PROBLEM/TITLE
command serves the same purpose). Thus, for example, static large deflection elasto-plastic shell behaviour is
specified by directives LARG and PLAS using the GROUP command, together with STAT using the JOB
command. (Note that the actual solution is determined also by the commands discussed in Section 4.3.1.3
above.)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-15
ASAS (Non-Linear) User Manual                                                                          Data Preparation


Each GROUP command is followed by an ELGROUP command defining the elements within the group. There
is provision to vary the integration rule used in each element using the INTEGRATION command. There is also
provision for elements to be ‘put-to-sleep’ and ‘woken-up’ using the SLEEP and WAKE commands.


4.3.1.5 Output Control

A range of commands are required to control output, depending on the type (e.g. results, data echoes,
diagnostics) and whether it is to be printed or saved on file for subsequent post-processing.

In the absence of any explicit directives, the program will print ‘standard’ output consisting of an echo of the
input data, expanded data lists, problem parameter summaries and the convergence details for each load
increment followed by the tail sheet. NO DISPLACEMENT, VELOCITY, ACCELERATION, STRESS OR
STRAIN RELATED QUANTITIES ARE PRINTED UNLESS ASKED FOR.

The printing of displacements, velocities, accelerations, stresses and strains and associated quantities is
controlled by OUTPUT and BLOCK commands. The stress and strain related output depends on the element
type (see Appendix A). The axis system (local or global) to which it refers can be controlled for some elements
by directives specified using the GROUP command.

The printing of data lists and echoing of input data can be controlled by options using the OPTIONS command.
The Preliminary data can also be interspersed with COMMENT and TEXT commands.

Diagnostic monitoring of the two constituent programs is controlled using PRENL and MONITOR commands.

Archiving of results to file for post-processing or viewing is controlled using the POST or RESU command. No
results will be saved unless POST/RESU Command is specified and hence its usage is highly recommended.

Details of output are given in Section 4.4.




4.3.2       Structural Description Data - see Section 5.2

The Structural Description data defines the shape and physical properties of the idealisation. The following data
blocks are involved:

(a)     Coordinates Data (see Section 5.2.2)

        This data defines the positions of the nodes.                   Coordinates may be given in rectangular cartesian,
        cylindrical polar or spherical polar coordinate systems or in any combination of these. ASAS-NL
        transforms all these local coordinates into a global rectangular cartesian system. If a list of coordinates is
        requested, they are printed in the global system.

(b)     Element Topology Data (see Section 5.2.3)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-16
ASAS (Non-Linear) User Manual                                                                          Data Preparation


       This data defines the location of each of the elements by reference to its node numbers. It also defines the
       material properties associated with the element by reference to a material property integer.                 Most
       elements must have their nodes listed in a given sequence. For details, see the element description sheets
       in Appendix A.

       Each element topology line contains an integer number which refers to the Geometric Property Data
       (except for brick and axisymmetric solid elements). Each line also contains a flag which indicates
       whether the element mass matrix is to be lumped, consistent or not used at all. If it is left blank in a
       natural frequency analysis, the mass matrix for the element will default to the type indicated in Appendix
       A.

       The user may also assign a unique ‘element number’ to each element. This ‘user element number’
       controls the order in which the results are printed and is also referred to by several commands in the
       Preliminary data. The numbers are also used to reference elements for post-processing. If numbers are
       not given by the user, the program numbers elements automatically in the order in which they first
       appear.

(c)    Material Properties Data (see Section 5.2.4)

       This data defines the material properties which are referred to by the material property integers in the
       Element Topology Data.

       For each material sufficient data must be provided to fully define the behaviour and solution required.
       All materials require elastic data. If PLAS or CREP appears with the PROBLEM, TITLE or appropriate
       GROUP commands in the Preliminary data then data for a plastic (failure) or creep model respectively
       are also required.

       If the material is temperature dependent, the data for each type of behaviour (i.e. Elastic and Plastic) is
       repeated in turn for a set of reference temperatures. The program interpolates linearly for data at
       intermediate temperatures.

(d)     Geometric Properties Data (see Section 5.2.5)

       This data defines the geometric properties of the element, such as thickness and cross-sectional area.
       Solid elements such as the brick family have no geometric properties.

       For selected beam elements e.g. BEAM, BM2D, BM3D and TUBE, the properties may optionally be
       input using section definitions which provide additional information with regard to shape and physical
       dimensions (see Sections 5.2.6).

(e)    Section Data (see Section 5.2.6)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-17
ASAS (Non-Linear) User Manual                                                                          Data Preparation


        This data is used as an alternative means to define properties for beam element types BM2D, BM3D,
        BEAM and TUBE. In order to generate the flexural properties for the structural analysis, the section
        shape and dimensions are supplied and the program automatically calculates the required geometric
        properties. If required, user defined flexural properties may also be supplied which will override those
        calculated from the section dimensions.

        The section type and dimensions are stored so that the post-processor, BEAMST, can automatically
        calculate extreme fibre stresses without additional information.

(f)     Skew Systems Data (see Section 5.2.7)

        This data defines the relationship between the global axis system and any local axis system required at a
        node. Each skew system can be defined either in terms of direction cosines or by 3 node points.




4.3.3       Boundary Condition Data - see Section 5.3

The Boundary Condition data defines how the idealisation is restrained or constrained.

(a)     Suppression Data (see Section 5.3.3)

        This data lists all the freedoms which are to be suppressed. If a freedom is suppressed in a direction other
        than parallel to the global axis, then Skew Systems Data is also required (see Section 3.6.3).

(b)     Prescribed Freedom Data (see Section 5.3.4)

        All freedoms which are to be given a prescribed value of displacement, velocity or acceleration are listed
        in this data. Freedoms may be prescribed in skew directions by reference to a skew system. The actual
        values of displacements, velocities or accelerations to be applied are listed separately, in the Prescribed
        Displacement, Velocities and Accelerations Data of Loading Data.

(c)     Constraint Equations Data (see Section 5.3.5)

        This data defines any required linear dependence between freedoms. The dependent freedom on the left
        hand side of the constraint equation may be skewed by reference to a skew system.                       The linear
        dependence must be meaningful; it is not valid for example, to have a suppressed freedom on the left side
        of a constraint equation.

(d)     Rigid Constraint Data (see Section 5.3.6)

        This data block defines rigid connections between freedoms. A selection of rigid ‘elements’ is available
        comprising rigid links, 2-D and 3-D rigid beams, rigid link systems and rigid beam systems. Systems are
        also available to connect shell elements to brick elements.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-18
ASAS (Non-Linear) User Manual                                                                          Data Preparation


        The first node specified must be the independent node. The dependent freedoms may be skewed by
        reference to a skew system.

(e)     Freedom Release Data (see Section 5.3.2)

        This data block defines freedoms which are to be disconnected on specified elements at specified nodes.
        A released freedom may be skewed by reference to a skew system. The user element number and node
        number is then given to describe each freedom to be released.

        The facility is only available for beam elements with release provided in the beam local axis system. This
        may be used to model pin joints and sliding connections.

        If any of the freedoms specified in this data are referenced in any other Boundary Condition Data then the
        Freedom Release Data block must be the first data block specified in the Boundary Condition Data.




4.3.4       Loading Data - see Section 5.4

The Loading data defines the loading history applied to the model.

Load histories may be defined in one of three ways (see Section 3.3.15):

•           Proportional Loading - Section 4.3.4.1

•           Load Functions - Section 4.3.4.2

•           Specific Pseudo Times - Section 4.3.4.3


The three methods of defining load history cannot be mixed. The load history defined with Loading data may be
cycled using the LOCYCLE command in the Preliminary data.


4.3.4.1 Proportional Loading

To specify proportional loading:

•           Define a single load set containing as many load types (e.g. pressure, nodal temperatures) as necessary

•           Leave the Pseudo Time blank on the SET data line

•           A Load Function Data block is not required

•           All nodal temperatures are taken as the reference temperature TREFLD (default 0.0) at zero pseudo
            time.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-19
ASAS (Non-Linear) User Manual                                                                          Data Preparation


The loads so defined are factored by a multiplier equal to the corresponding pseudo time to give the value at
each load step.


4.3.4.2 Load Functions

To use load functions:

•           For each load function, define a load set containing as many load types as necessary that describe the
            load distribution. Each load set references a load function

•           Leave the Pseudo Time blank on the SET data line

•           Define load functions in the Load Function Data


Each load function is a tabulated table of pseudo times and factors giving the proportion of the load to be applied
at that pseudo time. Proportional loading is assumed between tabulated values. Load set without a load function
defined is assumed to have proportional loading.


4.3.4.3 Pseudo Times

To use pseudo times:

•           For each time on the pseudo time axis that the total load distribution is known, define a load set of
            (possibly many) load types describing the load state

•           The Pseudo Time for the load set is given on the SET data line

•           A Load Function Data block must not be present

•           All loads not defined within a particular load set are taken as zero at that pseudo time

•           All nodal temperatures are taken as the reference temperature TREFLD (default 0.0) at pseudo time
            TIMBEG (default 0.0). All other loads are taken to be zero at pseudo time TIMBEG

•           TREFLD and TIMBEG may be redefined using the PARAMETER command in the Preliminary data

•           All temperatures explicitly defined within a load set at pseudo time TIMBEG are interpreted as a set
            of user-supplied reference temperatures unless a solution is attempted at time TIMBEG in which case
            the constant reference temperature TREFLD is assumed for all nodes. This facility allows the
            reference temperature to be varied throughout the structure.


Proportional loading is assumed between load sets.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-20
ASAS (Non-Linear) User Manual                                                                           Data Preparation


4.3.5       Additional Mass Data - see Section 5.5

The Additional Mass data defines the direct mass input values.

This data lists the freedoms and associated lumped mass (inertia) values which are to be added to the finite
element model. With this ADDED MASS facility the mass matrix so described can augment the finite element
mass. Each lumped mass must only be associated with the existing freedoms present on the elements generated
by the element topology data.

Apart from natural frequency or transient dynamics analyses, only x, y, z masses are allowed; all others are
ignored.

The added mass data specified are usually included in all relevant calculations (i.e. load when body loading
applied and mass when inertia required). It is also possible to account for their effects selectively, enabling
greater modelling flexibility.




4.3.6       Initial Conditions Data - see Section 5.6

The Initial Conditions Data defines an initial (residual) stress state. This should be self-equilibrating; if it is not,
the ‘out of balance’ forces will be redistributed within the first load increment, but convergence may be poor.

The Initial Conditions Data also allows for the definition of initial displacements and/or velocities at the start of
a transient dynamic analysis. Care should be taken that any initial conditions so specified are compatible with
any prescribed displacements/velocities/accelerations.

4.4     Description of Output

The output file from ASAS-NL contains listings of checked and unchecked data and cross-reference tables
describing the model as well as results of the non-linear analysis. In addition, two journal files may be produced
from each run.




4.4.1       Data Input Echo and Checking

The following are produced during data input and checking stages:

PRELIMINARY DATA ECHO

A complete listing of the Preliminary data as supplied by the user is given.

PROGRAM CONTROL PARAMETERS

A complete listing of Program Control Parameters is given.                         These, in general, are controlled using the
PARAMETER command in the Preliminary data, but default values are supplied automatically by the program.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 4-21
ASAS (Non-Linear) User Manual                                                                          Data Preparation


Typical program parameters are the reference temperature for temperature loads and whether a sub-incremental
analysis has been requested.

INPUT DATA ECHO

A complete echo of the rest of the input data as supplied by the user is given.

CHECKED DATA

A listing of all data describing the model after being checked is given. Error and Warning messages, as
appropriate, are printed. This section contains expanded lists of coordinates, material properties, geometric
properties, suppressions, constraints and load tables for each load set. This is followed by listings of checked
residual stresses and results from further temperature checking if appropriate. Cross-reference tables giving
group structure, integration rules and nodes are also given.




4.4.2       Analysis Results

The amount of output produced depends on the results requested by the user in the Preliminary data. The order
of the load increments is dictated by the order of the solution times as given using the SOLVE command.
Output for each increment will be as follows:

STIFFNESS REFORMATION

A message is given if the stiffness matrices of elements in any group are reformed in any iteration during any
incremental step.

GEOMETRY REFORMATION

A message is given if the geometry is reformed in any iteration during any incremental step.

MASS REFORMATION

A message is given if the mass is reformed at any incremental step.

CONVERGENCE MONITORING

The incremental and total values of the convergence criterion are given for each iteration. This allows the rate of
convergence to be monitored.

ARCHIVING

Checkpoint numbers on the data-manager archive file and element stiffness matrix file are given if the user
specifically requests an archive at this load step using the SAVE command. The checkpoint number for the
Data-Manager archive file is required in the Preliminary data when a restart is being attempted. An archive is
always made following the final load increment if a SAVE command is present and the checkpoint number is
then found on the Data-Manager Tail Sheet.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-22
ASAS (Non-Linear) User Manual                                                                          Data Preparation


In addition, messages about information saved on the file for post-processing and plotting by ancillary program
are also given.

OUTPUT

Displacements and Reactions, if requested, are given first. By default maximum values of displacements and
summed reactions are printed for all increments for a linear or nonlinear static analysis. For a transient dynamics
analysis, maximum values of velocities and accelerations are additionally output. If requested the program also
prints values of displacements (velocities, accelerations) and reactions at all or selected nodes for all selected
increments.     Reactions include forces arising from application of prescribed displacements and constraint
equations.

Other than displacements (velocities, accelerations) and reactions, the output depends on the type of analysis and
the elements used. In the most general case, current stress, current total strain, elastic, inelastic and creep strain,
current yield stress and yield strain, equivalent stress, equivalent strain, equivalent plastic strain and work may
be requested for any element and any load increment. For shell and beam elements stress resultants at the
centroidal surface sample points are available. If no directives are given then no stress and strains will be
printed.

All stress and strain related quantities are computed and output at element integration points (see Appendix -G)
referred to either global or element local axes. The choice of axis systems can be varied, if required, from group
to group, but cannot be changed during the analysis.

In addition to stress and strain quantities, the material ‘status’ of an integration point is also printed under the
column INDR/STATUS according to the following convention:

All relevant elements except gaps and rigid surfaces
        E       -        0        -        elastic
       U        -        1        -        elastic unloading (or reloading) following yield
       P        -        2        -        yielded and loading
       C        -        3        -        Cracking
       F        -        4        -        fibre failure for composite analysis
       M        -        5        -        matrix failure for composite analysis
       L        -        6        -        lamina failure for composite analysis
       S        -        7        -        transverse shear/normal stress failure for composite analysis
       MS       -        8        -        M and S modes failure for composite analysis


Rigid surface or gap elements
       1        -        no contact
       2        -        stick
       3        -        slide in Y direction
       4        -        slide in Z direction
       5        -        slide in both Y and Z directions




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-23
ASAS (Non-Linear) User Manual                                                                          Data Preparation


Maximum values of displacements and largest equivalent stress, equivalent total strain, equivalent plastic strain
and equivalent creep strain, where appropriate, are also given.




4.4.3       Analysis Summary

The following information is given at the end of a run:

DATA MANAGER TAIL SHEET

A complete listing of system control parameters is given. These, in general, are controlled using the SYSTEM
and SYSPAR commands in the Preliminary data. The information may be used to monitor the efficiency of the
analysis. This information is intended only for the experienced user. The checkpoint number of the data-
manager file for a default archive on the last load increment is also given.

FILE STATUS

The status and disposition of all backing files accessed and created is given. The status is NEW for a virgin file
or OLD for an existing one. The disposition is OPEN, CLSE (closed) or DEL (deleted). DEL files have been
successfully deleted and CLSE files closed and saved.

MAIN RUN PARAMETERS

Listings of the main program parameters such as number of nodes and elements in the model are given.
Solution characteristics such as number of accumulated iterations and maximum frontwidth are also given.




4.4.4       Journal Files

Two journal files are printed during an ASAS-NL run. The first file, called pnamJF (pnam is the project name),
contains a summary of the run information of all the runs in the project. The second file, called INCRJF,
contains condensed information about the main analysis, enabling the user to monitor interactively the
incremental iterative solution process. File INCRJF is normally deleted at the end of the analysis but it may be
saved using option SAVJ.




4.4.5       ASASNL Output Markers

Certain values which are helpful for either the assessment or control of the analysis are periodically output by
ASASNL. To help find them using text editors, they are marked by a character string **nnnnnnnn, in columns 1
to 10, where nnnnnnnn is an indicative keyword.

Keyword                  Description




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-24
ASAS (Non-Linear) User Manual                                                                          Data Preparation


ACCL                     Summary information about acceleration technique used

ADJUST                   Adjusted value of next step size

AUCR                     Automatic creep timestepping. Summary information for automatically selected solution
                         times

AUGMENT                  Augmentation of Lagrangian multipliers required

CHANGE                   Gives number of sampling points (INDR) to have changed state for increment

CONV                     Convergence performance parameters

CURRENT                  Current value of step size

DETK                     Stiffness determinant and number of negative stiffness and constraint pivots

DISP                     Start of displacement output

DMTAIL                   Data Manager tail sheet

DPCOM                    Constant Increment of Displacement Component - iteration performance parameters

DPVEC                    Constant Increment of Displacement Vector - iteration performance parameters

DPVECL                   Constant Increment of Displacement Vector, Linearised version - iteration performance
                         parameters

DUMP                     Solution state saved for possible future restart or post-processing

EIGN                     Start of eigenvalue output

ELEM                     Start of element based output

ERROR                    Error flag

EXWRK                    Constant Increment of External Work Measure - iteration performance parameters

EXWRKL                   Constant Increment of External Work Measure, Linearised version - iteration performance
                         parameters

FREQ                     No natural frequency analysis performed due to non +ve definite stiffness matrix

FILES                    Active files summary

FINISH                   Abnormal exit path following error

GEOM                     Geometry reformed

INCRnnnn                 Start of increment nnnn and pseudo time (Always 1.0 for SOLU)

LEVEL                    Load/displacement level exceeds preset value, job terminating

LINS                     Line Search performance information

MASS                     Mass reformed

MAXP                     Gives highest PLASTIC strain and position for increment

MAXS                     Gives highest STRESS and position for increment




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-25
ASAS (Non-Linear) User Manual                                                                          Data Preparation


MAXT                     Gives highest TOTAL strain and position for increment

PERT                     Perturbation introduced

POST                     Post-processing identifier saved to porthole file

SECN                     Secant-Newton performance information

STIFF                    Stiffness reformed

SUMM                     Summary information for this increment

TRACE                    Start of subroutine trace back




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-26
ASAS (Non-Linear) User Manual                                                                          Data Preparation




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 4-27
ASAS (Non-Linear) User Manual                                                                                    Data Formats



5.     Data Formats

ASAS-NL data is organised into a series of data blocks, each containing a particular type of data. This chapter
describes each data block individually. The layout of each block is explained, and some examples are given.
The user need only refer to the sections describing the data blocks required for his current analysis.

Each block, except the Preliminary data, begins with a block header line. This header line defines the type of
data which follows. The final line in each block must be an END, written on a line on its own. The final line in
the data file must be a STOP, written on a line on its own.

The data blocks described in this chapter are:


                        Preliminary Data ..... ................ ................ ................ Section 5.1

                        Structural Data ........ ................ ................ ................ Section 5.2

                        Boundary Condition Data ......... ................ ................ Section 5.3

                        Loading Data .......... ................ ................ ................ Section 5.4

                        Additional Mass Data .............. ................ ................ Section 5.5

                        Initial Conditions Data ............. ................ ................ Section 5.6

                        STOP Data .............. ................ ................ ................ Section 5.7




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-1
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



5.1    The Preliminary Data

The preliminary data is the first block of ASAS-NL data. It defines the:

   •        memory size to be used for data handling

   •        job type (eg whether statics or dynamics)

   •        identity of the project

   •        structure or component to be processed within that project

   •        options which will affect the course of the run

   •        amount of printing produced

   •        files saved for further processing


All commands are identified by a unique command word at the start of the line. The first 4 characters of each
command word are mandatory, others are optional. Free format is used, with ‘topological variables’ (see Section
4.2.3) used as an optional shorthand method for generating lists of required numbers.

The majority of commands are optional and can be placed in any order. However, the following are mandatory
and must be supplied in the order given.

        JOB
        PROBLEM or TITLE
        One of SOLVE or RESTART, SOLUTION, SRESTART or SCALE
        END


Table 5.1 lists all possible commands in the preliminary data section. Mandatory commands are shown in bold.
An asterisk against optional commands signifies that defaults are implied, details of which are given below:

       SYSTEM                     Data area 1000000
       PROJ                       Default project title is ‘ASAS-NL ARCHIVE FILE’ and project name is ASNL
       STRUCTURE                  Default name is ASNL
       NEWSTRUCTURE               Default name is ASNN
       SYSP                       The various default values are given in Section 6, Table 6.1.
       CONV                       Residual convergence with Euclidean norm and tolerance 0.001.
       FILE                       The various default file names are given in Section 6, Table 6.1.
       INTE                       Use default integration rules.
       ITER                       Limit of 10 iterations for each load increment.
       PARA                       Various default values. See the PARAMETER command for details.
       PINO                       The default pressure interpolation order is that implied by the particular element
                                  displacement variation.
       SAVE                       Archive data manager and global stiffness matrix for last increment only.
       SPIT                       Various default values. See the SPIT command for details.
       UPDA                       Reform stiffness matrix on first iteration of first increment only.
       WEIG                       The default values are unity for all freedom types.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-2
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


The preliminary data commands fall into two sections, referred to as the problem and group sections. The
problem section includes all the commands following the PROBLEM command up to the first occurrence of the
GROUP command. All subsequent commands fall into the group section. The group section allows elements
to be assigned to a particular group. The division of the finite element model into groups of elements is strongly
recommended as many of the post-processing options in POSTNL are group related. Some elements, such as the
bar element FLA2, have to be assigned to a separate group (or groups) if the model includes other element types.
Table 5.1 indicates which section each command should appear in. The preliminary data commands invoke
procedures (eg frontwidth optimisation) and sets parameters (eg the subspace iteration convergence tolerance)
which are global in nature. Commands allowed within the group section control procedures and parameters that
may be assigned to groups of elements, eg output of stresses and strains.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-3
ASAS (Non-Linear) User Manual                                                                            Preliminary Data



 Name                          Description                                       Section       Category   Comments


 SYSTEM                    *    Sets size of data area                                           O
 PROJECT                   *    Sets project name and title                                      O        Must be the
 STRUCTURE                 *    Sets structure name                                              O        first section
 NEWSTRUCTURE              *    Sets new structure name                                          O
 SYSPAR                    *    Sets system parameters                                           O
 JOB                                                                                             M
 PROBLEM                        Titles output                                       P            M        One only,
 TITLE                                                                              P                     must follow JOB

 SOLVE                          Solution times                                      P                     One only,
 RESTART                        Restart times                                       P                     must follow
 SOLUTION                       Special solution control                            P            M        PROB or TITL
 SRESTART                       Special solution restart                            P
 SCALE                          Controls scaling of loads                           P            O
 COMMENT                        Comments in data                                    PG           O
 CONVERGENCE               *    Sets convergence criteria                           PG           O
 EGEN                           Replaces ELGROUP for coupled                        G            O
                                analysis
 EIGN                           Eigenvalue solution                                 P            M        for eigenvalues
 FILE                      *    Backing file names                                  P            O        recommended
 GROUP                          Group Titles                                        G            O
 ELGROUP                        Elements in group                                   G            O        must follow GROUP
 SKIP                           Skip elements in group                              G            O        only use with
                                                                                                          ELGROUP
 HYDR                           Hydrodynamic database name                          P            O        mandatory for
                                                                                                          accessing hydrodynamic
                                                                                                          data
 INTEGRATION               *    Integration rules                                   P            O
 ITERATION                 *    Iteration limits                                    P            O
 LOCYCLE                        Controls cyclic loading                             P            O
 MONITOR                        Diagnostic monitoring in ASASNL                     P            O
 OPTION                         Controlling options                                 P            O
 OUTPUT                         Controls output                                     PG           O
 BLOCK                          Controls output                                     PG           O        must follow OUTput
 PARAMETER                 *    Sets problem parameters                             P            O
 PASS                           Invokes frontwidth optimiser                        P            O
 START                          Sets starting vectors                               P            O        must have PASS
 PINO                      *    Defines pressure interpolation order                P            O
 POST                           Post-processing requirements                        P            O        recommended,
 RESU                                                                                                     one only
 SAVE                      *    Archive times                                       P            O
 SPIT                      *    Set eigenvalue soln. parameters                     P            O
 TEMPORAL                       Controls temporal integration for
                                transient analysis                                  P            O
 TEXT                           Printed comments in output                          P            O
 UNITS                          Defines global analysis units                       P            O        recommended
 UPDATE                    *    Controls solution procedure                         PG           O
 WEIGHTS                   *    Weighting factors for convergence                   P            O
 WAKE                           Sets wake up time for elements                      P            O
 SLEEP                          Sets sleep time for elements                        P            O
 END                            Signifies end of Preliminary Data                                M        last command




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-4
ASAS (Non-Linear) User Manual                                                                             Preliminary Data


Note
P -         Problem Section                                      G -         Group Section
PG -        Problem and Group Section                            M -         Mandatory
O -         Optional                                             * -         Default available

                                                Table 5.1 Preliminary Data Commands



5.1.1        AQWA Command

This command defines the name of the AQWA hydrodynamic database files. The command (or HYDR) is
mandatory if linkage to the hydrodynamic database is required, e.g. import of AQWA RAOs via the load
function type RAOS.


         AQWA                      aqwaid               (istr)




Parameters

AQWA              : Command keyword

aqwaid            : name of the AQWA model to be processed. This is the name associated with the .RES file
                     generated by AQWA-LINE. (Alphanumeric, up to 32 characters)

istr              : identification number of the structure in the hydrodynamic model. If omitted defaults to 1.
                     (Integer)

Notes

1.     If the file name contains space, the specified name must be embedded in double quotes (“).




5.1.2        BLOCK Command

This command defines the type of output to be printed under control of the OUTPUT command(s). Optional


              BLOCK                       blocno                          ident                         (ndelno)




Parameters




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-5
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


BLOCK             : command keyword

blocno            : identifying number of block

ident             : output identifier, one or more of the following:

                     DISP         displacements (problem section)
                     STRS         stresses
                     STRN         total strains
                     INST         inelastic strains
                     ELAS         elastic strains
                     SRES         stress resultants (beam and shell elements only)
                     CRSN         creep strains
                     ESTR         end segment smoothed stresses
                     SSTR         all segments smoothed stresses                         for WST4 and SST4 elements
                     SSRE     smoothed stress resultants
                     ORIG origin of yield locus (for kinematic hardening)

ndelno            : user defined list of nodes (for displacement only) or element numbers (for stresses or strains)
                     given in topological format. If blank defaults to all nodes or elements (in group)

Notes

1.      If GROUPS are used, then all commands controlling output (i.e. OUTPUT, BLOCK) must
        appear in the GROUP section other than commands controlling displacement output which
        always appear in the PROBLEM section.
2.      BLOCK commands should immediately follow the parent OUTPUT command(s).
3.      For a transient analysis including inertia effects, if DISP is specified, then velocities and
        accelerations are also output.



5.1.3       COMMENT Command

Any number of these commands may be used anywhere in the Preliminary data. They are not included in the
descriptive text block. Optional


             COMMENT                     alpha




Parameters

COMMENT           : command keyword

alpha             : any alphanumeric comment




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-6
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


Note


COMMENT commands may only be used in the preliminary data. For comment lines in the main body of the
data, use an asterisk at the start of the comment.




5.1.4       CONVERGENCE Command

This command defines the convergence criteria. Optional


         CONVERGE                  nmtype               refvar             tol




Parameters

CONVERGE : command keyword

nmtype            : type of norm, one of the following:

                     ABSN         absolute norm
                     EUCN         euclidean norm (Default)
                     MAXN         maximum value
                     SCAL         scaled using diagonal stiffness terms

refvar            : reference variable, one of the following:

                     DISP              displacement Increments
                     RESF         residual forces (Default)
                     STRN         strain
                     STRS         stress

tol               : tolerance value for convergence, default is 0.001. (Real)

Notes

1.       For creep analysis, a reference variable may be chosen by the program according to the form of the
         solution. For details, see Appendix -J.
2.       STRN and STRS Convergence Criteria are not available for shells using Ivanov yield criterion or
         engineering beams, ie BM2D, BM3D and TUBE.

Examples


The default convergence criterion

         CONV      EUCN       RESF         0.001

Convergence criterion based on displacements




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-7
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


         CONV      EUCN       DISP       1.0




5.1.5       EGEN Command

This command defines the elements to be generated in a group and must follow immediately its parent GROUP
command. The command is only used in coupled analysis in place of ELGROUP command for the automatic
generation of field elements.


         EGEN                  grpno                    elincr




Parameters

EGEN              : compulsory keyword

grpno             : group number from which the elements are generated

elincr            : user element number increment with respect to corresponding element in group grpno

Notes

1.       The topology of elements specified in EGEN will be generated automatically by the program, and should
         not be given explicitly in the ELEM data.
2.       Automatically generated field elements will have material property integer (1000+IMAT) and geometric
         property integer (1000+IGEOM) assigned. IMAT and IGEOM are the material property integer and
         geometric property integer respectively of the parent displacement element.




5.1.6       EIGN Command

This command invokes an eigenvalue analysis. Compulsory for eigenvalue analysis.
                                   ALL

                EIGN

                                    ptinc1

                                                                                              SELP      (ptinc2)




Parameters




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-8
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


EIGN              : command keyword

ptinc1            : list of pseudo times (Real) or increments (Integer) at which an eigen solution is to be
                     attempted.       These must occur with the preceding SOLVE, SOLUTION, RESTART,
                     SRESTART or SCALE commands

SELP              : keyword (optional but required for perturbation analysis)

ptinc2            : selected pseudo time (Real) or increment (Integer) for inclusion of perturbation load vector
                     (default is the first pseudo time or increment on the list)

Notes

1.      The type of eigenvalue analysis is determined by the matrix specified with the SPIT command, together
        with other control information.
2.      The pseudo times must be in ascending order.
3.      Pseudo times are required for SOLVE problems: increment numbers are required for special solution
        problems, e.g. ARCL.
4.      To achieve results similar to a frequency analysis with ASAS (Linear), use EIGN 0.0 in a static job
        solving at time 0.0 (assuming that at time 0.0 the loading is zero). Note that if a frequency analysis is
        performed with loading, then natural frequencies may change due to load stiffening and other non-linear
        effects.




5.1.7       ELGROUP Command - (Group Section Only)

This command defines the elements in a group and must follow immediately its parent GROUP command. It is
valid only in conjunction with a GROUP command. If no group is defined, then all elements are assumed to be
in group 1. Conversely, if groups are used, then every element must be explicitly assigned to one or other group.
Optional


                ELGROUP                           elno




Parameters

ELGROUP           : command keyword

elno              : list of element numbers given in topological format. (Integer)

Note

1.      Gaps and FLA2 elements must always belong to their own group and must not be mixed with other
        element types.
2.      The SKIP command can be used to switch off some elements defined in the ELGROUP command. The
        order of ELGROUP and SKIP commands within a group is not important.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-9
ASAS (Non-Linear) User Manual                                                                               Preliminary Data


Examples


Assign elements 1 to 10 to group 3

        GROU       3    *     BEAM       ELEMENTS
        ELGR       1    2     3     4    5     6     7    8     9     10

Alternative method using topological format

        ELGR       (10)       (1,1)




5.1.8       END Command

This must be the last command in the preliminary data. Compulsory



          END




Parameter

END               : command keyword




5.1.9       FILE Command

Defines names and attributes of files. Recommended
                                                                               NEW                      (APPEND)
             FILE                   ftype                 fname
                                                                               OLD                       OVER



Parameters

FILE              : command keyword

ftype             : keyword to identify file type, one of the following:

                       ARCH       new archive file
                       NSTF       new stiffness file                NEW should be given on SAVE command
                       OSTF       old stiffness file
                       POST       post-processor file
                       MODL       ‘PATRAN’ or ‘FEMVIEW’ formatted model file




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-10
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


fname             : filename of up to 12 characters (including extension)

NEW               : keyword to denote file is new

OLD               : keyword to denote file already exists

APPEND            : keyword required to append new information to end of file (default)

OVER              : keyword required if new information is to overwrite existing information

Notes

1.       The old archive file, if required, is defined with the JOB command.
2.       The default values for existing files is given in Section 6
3.       Keywords APPEND and OVER are applicable to file types POST and MODL only. Leave blank for
         ARCH, NSTF and OSTF.
4.       If the old stiffness file is omitted in a restart, the required filename will be retrieved from information
         stored in the old archive file.

Example


Naming the porthole file for post-processing with POSTNL

         FILE        POST         CRANEPST




5.1.10      GROUP Command - (Group Section Only)

A Group is a subset of elements in the structural model, all of which have the same non-linear behaviour. This
behaviour can vary between Groups. The Group command defines the behaviour by means of directives. In
some cases it is possible to define the same directives at Group and Problem level, in which case the lower level
Group definition applies. Optional

The Group command must be followed immediately by the ELGR command.


            GROUP              grpno                     (direct)                (*         title)




Parameters

GROUP             : command keyword

grpno             : identifying number of the group. (Integer, 1-9999)

direct            : 4 character directives defining structural and material model. May be one or more of the
                     following:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-11
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     PLAS         take plasticity effects into account
                     LARG         include large displacement effects in the calculation of strains and geometric
                                  stiffness matrices.         This directive should be accompanied by the command
                                  UPDATE GEOM (see UPDATE command)
                     CONL         use conservative pressure loading - i.e. calculate pressure loads using original
                                  geometry throughout.            Only applicable with UPDATE GEOM (see UPDATE
                                  command)
                     NRES         do not carry forward residuals into next increment
                     FLNS         form natural stiffness (i.e. Young’s modulus*Area) for FLA2 and FAT2 elements
                     CREP         creep analysis
                     NREC         (only use with the GROUP command). The stresses will not be recovered nor
                                  element stiffnesses be reformed for elements in the group
                     EXPL         user explicit temporal integration scheme for transient analysis

*                 : character to indicate the following text (up to and including column 80) forms a title for this
                     group

title             : any alphanumeric group title. It must be preceded by an asterisk (*). The title is used in the
                     output from ASASNL to describe the group

Notes

1.      If no directives are given, linear elastic behaviour is assumed with the default implicit temporal
        integration scheme for transient analysis.
2.      Gaps and FLA2/FAT2 elements must always belong to their own group and must not be mixed with other
        element types. In general, it is strongly recommended that each group defined comprises only one
        element type to facilitate post-processing of the analysis results.




5.1.11      HYDR Command

This command defines the name and details of the file containing the hydrodynamic information. The command
is mandatory if linkage to the hydrodynamic data is required, e.g. import of RAOs via the load function type
RAOS.



        HYDR                  AQWA                aqwaid               (istr)


                              NRAO                filename             (wfform)            (wdform)     (raoform)   (rotform)




Parameters




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-12
ASAS (Non-Linear) User Manual                                                                           Preliminary Data



HYDR             command keyword
AQWA             keyword to signify that hydrodynamic data is obtained from AQWA
aqwaid           name of the AQWA model to be processed. This is the name associated with the .RES file
                 generated by AQWA-LINE. (Alphanumeric, up to 32 characters)
istr             identification number of the structure in the hydrodynamic model. If omitted defaults to 1.
                 (Integer)
NRAO             keyword to signify that hydrodynamic data is obtained from a neutral RAO data file
filename         name of the neutral RAO file. (Alphanumeric, up to 32 characters)
wfform           format of wave frequency data, one of the following:
                 FREQ          frequency in rad/s (Default)
                 PERD          period in s
                 HRTZ          frequency in Hz
wdform           format of wave direction data, one of the following:
                 XPOS          positive X direction is 0° (Default)
                 XNEG          negative X direction is 0°
raoform          format of RAO data, one of the following:
                 AP            amplitude and phase angles (Default)
                 RI            real and imaginary parts
rotform          format of rotational units in RAO data, one of the following:
                 DEG           degrees (Default)
                 RAD           radians

Notes

1.     The format of the neutral file is described as follows:

       Frequency/Period value
       Direction value
       X (surge)    X (surge)               Y (sway)               Y (sway)              Z (heave)       Z (heave)
       RX (roll)    RX (roll)               RY (pitch)             RY (pitch)            RZ (yaw)        RZ (yaw)

       The 6 numbers representing the RAO are in pairs of Amplitude and Phase or Real and Imaginary.

       The data lines are repeated for each wave frequency and direction.

2.     Maximum number of wave frequencies allowed is 50. Maximum number of wave directions allowed is 40.

3.     Wave directions are assumed to be in degrees and in the range -100 to +180.

4.     The rotational units specified apply to all phase and rotational RAO values.

5.     If the file name contains space, the specified name must be embedded in double quotes (“).

6.     A positive phase angle is considered as lagging.

Example

Example of a neutral RAO data file with data supplied at 2 frequencies 0.34907 rad/s and 0.36960 rad/s and 5
directions 0°, 45°, 90°, 135°, and 180°.

0.34907
   0.00
 0.6997              88.98            0.0000           -104.31              2.0823               13.11
 0.0000               0.31            0.1507             88.35              0.0000               46.90




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-13
ASAS (Non-Linear) User Manual                                                                            Preliminary Data


0.34907
  45.00
 0.5048             89.01             0.5046               89.02            2.0826             13.09
 0.0874            -91.84             0.0954               88.15            0.0000           -134.89
0.34907
  90.00
 0.0000            123.22             0.6994               88.98            2.0823              13.11
 0.1382            -91.64             0.0000               23.57            0.0000             -94.99
0.34907
 135.00
 0.5048            -90.99             0.5046              89.02             2.0826              13.09
 0.0874            -91.84             0.0954             -91.85             0.0000             -47.76
0.34907
 180.00
 0.6997            -91.02             0.0000              87.73             2.0823              13.11
 0.0000            162.66             0.1507             -91.65             0.0000             146.91
0.36960
   0.00
 0.6585            88.53              0.0000           -177.96              3.0661             36.08
 0.0000          -159.88              0.1134             87.68              0.0000           -152.22
0.36960
  45.00
 0.4780             88.59             0.4779               88.60            3.0668              36.06
 0.0630            -92.74             0.0682               87.26            0.0000             -62.60
0.36960
  90.00
 0.0000            104.89             0.6583               88.53            3.0661              36.08
 0.1047            -92.32             0.0000               19.68            0.0000             -42.51
0.36960
 135.00
 0.4780            -91.41             0.4779              88.60             3.0668             36.06
 0.0630            -92.74             0.0682             -92.74             0.0000           -120.04
0.36960
 180.00
 0.6585            -91.47             0.0000              91.21             3.0661              36.08
 0.0000            -35.18             0.1134             -92.32             0.0000             -24.82



5.1.12      INTEGRATION Rule Command

This command defines the integration rules to be used by specified elements. If not present the default rule is
used. Optional


           INTEGRATION                   intx              inty              intz                (elno)




Parameters

INTEGRATION : command keyword

intx                 : integration order or rule number in element local directions. All three numbers must be




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-14
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


inty                     given. (Integer)
intz

elno                   : list of element numbers in topological format. (Integer)
                         If blank, defaults to all elements (in group)

Notes

1.      See Appendix -G for default integration rules for each element type.
2.      intz should be 1 for 2-D elements.
3.      If zero is specified for any rule number then that rule number is set at the default value.
4.      If an invalid integration rule is specified for an element then that element’s default values will be used.
5.      If more than one set of integration rules is specified for any given element then the final set will be used.

Examples


Allow for five layers through the thickness for QUS4 shell element numbers 1 to 25 in a plasticity analysis.

        INTE       1     1     5    (25)       (1,1)

Similar example but for TCS8 shell elements

        INTE       2     2     5    (25)       (1,1)




5.1.13      ITERATION Command

This command specifies the maximum number of iterations to be performed within a load increment. Optional
                                                                                 ptminc

           ITERATION                n                      TO
                                                                                 END



Parameters

ITERATION : command keyword

n                 : maximum number of iterations in every increment up to and including the solution time/
                       increment ptminc, if specified. (Integer)

TO                : keyword

ptminc            : solution pseudo-time/time (Real) or increment (Integer) up to which this specification of n is to
                       apply

END               : keyword indicating that n applies for all solutions times/increments to the end of the analysis




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-15
ASAS (Non-Linear) User Manual                                                                            Preliminary Data


Notes

1.      If no ITERATION command is present a maximum of 10 iterations are assumed for each increment.
2.      The run will terminate if convergence is not achieved within the specified number of iterations, unless
        option OVIT (OVerride ITeration limit) is specified in the OPTION command.
3.      If a solution is performed at a pseudo-time/time/increment greater than the last pseudo-
        time/time/increment specified with an ITERATION command, then the maximum number of iterations
        performed will be that specified on the last ITERATION command. To revert to the default, specify
        ITERATION 10 TO END as the last ITERATION command.

Example


Allow up to 20 iterations to time 5.0, 15 iterations from time 5.0 to 7.0 and revert to default for all remaining
times

        ITER       20     TO      5.0
        ITER       15     TO      7.0
        ITER       10     TO      END




5.1.14      JOB Command

Defines analysis type and for restart jobs the old archive file name and required checkpoint number on the old
archive file. Compulsory
                                                STAT                       oldarch             (nchkpt)
                           (NEW)
        JOB                (OLD)                TRAN

                           (REPL)               PIER
                                                HEAT
                                                HTRA



Parameters

JOB               : command keyword

NEW               : optional keyword indicating that this run will create a new project data base

OLD               : optional keyword indicating that this run will add to an existing project data base

REPL              : optional keyword indicating that this run will replace a previous run of the same structure on
                     the project database

STAT              : keyword indicating static analysis

TRAN              : keyword indicating a transient analysis, ie including creep or inertia effects




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-16
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


PIER              : keyword indicating a piezo-restivity analysis

HEAT              : keyword indicating a steady state heat analysis

HTRA              : keyword indicating a transient heat analysis

oldarch           : old archive file name up to 8 characters. This is only required for restarts

(nchkpt)          : number of the required restart checkpoint on the old archive file (brackets must appear). If
                     omitted the highest checkpoint on the old archive file is taken. This is only required for
                     restarts. (Integer)

Notes

1.      The default project status is OLD for a restart job and NEW otherwise




5.1.15      LOCYCLE Load Cycle Command

This command defines cyclic loading. Optional


     LOCYCLE           ptime1              ptime2




Parameters

LOCYCLE           : command keyword

ptime1            : pseudo time for start of cycle - T1. (Real)

ptime2            : pseudo time at finish of cycle - T2. (Real)

Notes

1.      The starting and finishing times, T1 and T2 respectively, refer to the first cycle. Cyclic loading, period T2
        minus T1, follows.
2.      T1 need not necessarily be the first time specified with the SOLVE command but T1 minus T0 must be
        less than T2 minus T1.
3.      The load cycle times and the parameters TREFLD and TIMBEG cannot be redefined in a restart. This
        means that if the loads are redefined on restart they must lie within the load cycle range of the initial run.




5.1.16      MONITOR Command

This command controls diagnostic monitoring in ASASNL. Optional and not normally required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-17
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


(i)         For the main analysis stage.


          MONITOR                 stage                      subkey




Parameters

MONITOR           : command keyword

stage             : stage identifier, one of the following:

                     INIT             initialisation stage
                     LOAD             load generation
                     STIF             stiffness
                     REDU             reduction
                     SOLV             solve
                     UPDT             update
                     STRE             stress recovery
                     UPD1             update 1
                     UPD2             update 2
                     SCAL             scaling to first yield
                     MASS             mass generation
                     EIGN             eigenvalue extraction
                     SPIT             eigenvalue extraction
                     OUTP             output
                     PORT             post-processing output file
                     AUTM             automatic timestepping
                     AUGM             augmented Lagrangian
                     ALL              monitoring on all stages

subkey            : names of subroutines and/or keywords to be monitored. Keywords (set throughout the stage)
                     may be one or more of the following:

                     ALL              monitor all subroutines in stage
                     STOPnn           abort program run at start of this stage in increment nn, where nn is zero filled
                                      and right justified
                     CLAIM            monitor dynamic storage allocator
                     TOTAL            print contents of freestore area on CLEAR
                     COMMON print common block contents at start of stage
                     EXTEND           set extended logging mode for subroutine tracing package
                     BRIEF            set compact logging mode for subroutine tracing package
                     DTAILS           print length and type of each record in Data Manager tail section
                     DTAILL           print length, type and contents of each record in Data Manager tail section
                     VPUTS            print length and type of each VPUTI or VPUTR




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-18
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     VPUTL            print length, type and contents of each VPUTI or VPUTR
                     VGETS            print length and type of each VGETI or VGETLR
                     VGETL            print length, type and contents of each VGETI or VGETR
                     MODMAN monitor data manager page file in Data Manager tail section
                     PCHAIN           call subroutine PCHAIN in stage header
                     PUSAGE           monitor page usage in the stage
                     PUFULL           as for PUSAGE but with more information
                     OVROFF           switch off overflow check
                     DISKFL           monitor status of disc files
                     ROTAWS includes rotations in the initial configuration in the stress recovery stage when an
                                      element wakes up so that they will not cause straining (rotations not included by
                                      default) usage MONI STRE ROTAWS
                     TEMPWS assumes that there is no sudden change of temperature when an element wakes up
                                      in the load generation stage (by default newly activated elements are set to the
                                      reference temperature)
                                      usage MONI LOAD TEMPWS

Note


Several MONITOR commands can be used to monitor different stages with different subkey values if required.

(ii)        For all other stages:
                               FULL
                                                                        ALL
                                   READ
         MONITOR                   WRITE                                 file
                                   BRIEF
                                                                       INDEX
                                   FREESTORE

                                   SYOP
                                                           option             v alue
                                   FLAG
                                   SENTRY




Parameters

MONITOR                : keyword

FULL                   : print the contents of the file transfers on reading and writing

READ                   : print the contents of the file transfers on reading only. Print the header only (not contents)
                         on writing




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-19
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


WRITE                  : print the contents of the file transfers on writing only. Print the header only (not contents)
                         on reading

BRIEF                  : print the headers for the file transfers but not the contents on reading and writing

ALL                    : monitor all ASAS logical files

file                   : list of ASAS logical file numbers to be monitors

INDEX                  : monitor the ASAS Project Index file

FREESTORE              : monitor the allocation of space in the Data Area

SYOP                   : the ASAS program has a number of system monitoring options which can be switched on

FLAG                     using this command

option                 : the number of the system option

value                  : the value assigned to the system option

SENTRY                 : monitor the entry into each Fortran subroutine

Notes

1.      Specific information relating to these monitoring features can be found in the ASAS Programmer’s
        Manual.
2.      Many of these features produce large amount of formatted output.
3.      Several MONITOR commands can be used in the same run.

Example


        MONITOR BRIEF 13 15 3
        MONITOR FREESTORE




5.1.17      NEWSTRUCTURE Command

To define the new structure name to be associated with the results created by a restarted run. Required by
restarted jobs only but highly recommended.


         NEWSTRUCTURE                          nsname




Parameters




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-20
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


NEWSTRUCTURE                  :   keyword

nsname            : structure name to be associated with the results being created by the current restarted run in
                     order to identify these results from others in the project. nsname must be unique for this
                     project (alphanumeric, 4 characters).

Notes

1.      If the NEWSTRUCTURE command is omitted then nsname defaults to the name ASNN. However,
        since the structure name must be unique within a project, the default must not be assumed more than once
        if the project contains a series of restarts.
2.      A STRUCTURE command is normally required in conjunction with NEWSTRUCTURE to define the
        name of the existing structure




5.1.18      OPTION Command

This command defines options applicable to the problem. Optional


               OPTION                     option




Parameters

OPTION            : command keyword

option            : 4-character keyword to identify option. May be one or more of the following:
                     APIW             complete wave load to the requirements of API RP2A (See Appendix M.7)
                     APIC             vary current profile using non-linear stretching as recommended in the API RP2A
                                      Code of Practice. Default when APIW is selected (See Appendix M.7)
                     AUCR             automatic timestepping for creep (see Appendix -J)
                     AUTO             automatic restart of increment with reduced size (see MXAUTO and STEPRF
                                      with PARAMETER command) when solution is not available, divergence or
                                      slow convergence. Used only with SOLUTION command. Not applicable for
                                      creep
                     BAKE             backward Euler method for plasticity (see Appendix C.3)
                     BODY             check for sensible density values
                     BRIG             rigorous buoyancy load calculation (See Appendix M.7)
                     CCOG             calculate centre of gravity of the model
                     CCON             print the constraint equations input data
                     CCOO             print the coordinate input data
                     CDIR             print the direct mass input data
                     CDIS             print the displaced freedoms input data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-21
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     CELE             print the element topology input data
                     CGEO             print the geometric property input data
                     CLOA             print the load input data
                     CLST             solve constraint equations last. Note that this method cannot remove local
                                      singularities. High speed frontal solver only
                     CMAT             print the material property input data
                     CONV             Include convective acceleration terms when APIW is operative. Default for non
                                      APIW analyses (See Appendix M.7)
                     COOR             print coordinate data
                     CORE             write element stiffnesses etc. to data manager instead of backing files
                     CSKE             print the skew systems input data
                     CSUP             print the suppressions input data
                     DDEC             delete the decomposed stiffness disc file before an eigenvalue analysis
                     DATA             perform a data check run only
                     DIRE             print the direct mass input data
                     DTRS             initial conditions supplied in a transient dynamic restart to the previous solution
                     ELAX             print offset and local axes information for each beam and tube element in the
                                      structure
                     ELEM             print the element topology data
                     EPSN             engineering plane strain model for membranes
                     FCRO             print full summary for automatically selected creep solution times (summary is
                                      short by default)
                     FDMS             print a list of freedoms at each node
                     FEMV             produce ‘FEMVIEW’ analysis model file (see note)
                     FIXD             read data input in fixed format
                     FNUM             print a list of freedom numbers (I.e position of freedom in solution vector)
                     FSOL             instruct the program to use the ordinary frontal solver
                     GAUS             print out stress sampling points for elements with stress output
                     GEOM             print the geometric property data
                     GLST             global stress output (see Appendix -A for valid element types)
                     GOON             continue with solution even when warnings present in data
                     HYDR             print detailed elemental hydrodynamic information (see Appendix M.7)
                     IEST             use initial elastic stiffness for first iteration when there is residual stress input
                     INEL             use input element order for solution order
                     LINS             use line search procedure (cannot be used with CONSIT with the SOLUTION
                                      command)
                     LOWE             convert all higher order element types to lower order ones in steady state heat
                                      analysis. When used, the geometric properties data must refer to the lower order
                                      element types only
                     MATE             print the material properties data
                     MCON             vary current profile to maintain mass conservation. This is not recommended for
                                      use with API analyses (See Appendix M.7)
                     MYEL             use user element order for solution order




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-22
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     NODL             print only selected expanded data (“No Data List”)
                     NOKC             no centrifugal stiffness to be included in tangent stiffness matrix
                     NOKP             no pressure load stiffness to be included in tangent stiffness matrix
                     NOPF             no porthole file created for post-processing using POSTNL
                     NOPG             suppress page throws in output
                     NORE             no resultants calculated for applied loads during data checking
                     OVIT             override iteration limit (i.e. continue to next load increment when iteration limit
                                      exceeded)
                     PATN             produce ‘PATRAN’ neutral file for analysis model (see note)
                     PLSN             plane strain model for membrane elements
                     PRNO             print only selected input data
                     RELC             vary current profile such that the velocities are not at absolute depths, but relative
                                      depths (See Appendix M.7)
                    RVOF              switch off relative velocity formulation in Morison’s equation for wave load
                                      calculation (See Appendix M.7)
                     SAVJ             save journal file INCRJF
                     SECN             use Secant-Newton acceleration (SOLVE solution procedure only)
                     SKEW             print the skew systems data
                     SURF             use temperature at node 1 to determine material properties. Only apply to FAT2
                                      elements with FLNS option (see GROUP or PROBLEM commands)
                     TRAP             trapezoidal rule used for through thickness integration for shells
                     TWOD             convert plane stress membranes and FLA2 to 2-D forms
                     VEXT             no modification to current profile in the presence of wave, simple extrapolation is
                                      used above still water level. Default for non-APIW analyses. (See Appendix
                                      M.7)
                     VISC             use viscoplastic creep solution method (See Appendix -J). Not available for
                                      creep law LAW4.

Note

FEMV and PATN are mutually exclusive options.




5.1.19      OUTPUT Command

This command defines the points in time at which results are to be output.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-23
ASAS (Non-Linear) User Manual                                                                            Preliminary Data


                                                             TGEN               stime             timei    ntime

                                                             IGEN               incst             iinc     nincs

             OUTPUT              blocno                      ALL

                                                             INCR               incno


                                                             TIME               ptime




Parameters

OUTPUT            : command keyword

blocno            : number of the block controlled by this command. A BLOC command is then required.
                     (Integer)

TGEN              : keyword indicating that a list of times is to be generated

stime             : start time for list of generated times. (Real)

timei             : time increment to be added to start time for list of generated times. (Real, ≥ 0.0)

ntime             : total number of generated times, including start time. (Integer, > 0)

IGEN              : keyword indicating that a list of increments is to be generated

incst             : start increment for list of generated increments. (Integer)

iinc              : increment to be added to start increment for list of generated increments. (Integer, > 0)

nincs             : total number of generated increments, including start increment. (Integer, > 0)

ALL               : keyword indicating that output is required at all times/ increments

INCR              : keyword indicating that a list of increment numbers are supplied

incno             : increment number for which results are to be output. (Integer)

TIME              : keyword indicating that a list of pseudo-times are supplied

ptime             : pseudo-time for which results are to be output. (Real)

Notes

1.      If GROUPS are used, then all commands controlling output (i.e. OUTPUT, BLOCK) must appear in the
        GROUP section other than commands controlling DISPlacement output which always appear in the
        PROBLEM section.
2.      INCR or IGEN may only be used with SOLUTION solution method.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-24
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


3.      TIME or TGEN may only be used with SOLVE solution method.
4.      If the list of pseudo times/increments at which output is required is too long for one line, specify further
        OUTPUT commands with the same block number.
5.      If a time or increment is re-specified with a subsequent OUTPUT command the output identifiers with
        the associated BLOCK command(s) are overwritten.




5.1.20      PARAMETER Command

This command enables the values of certain problem parameters to be set. Optional


            PARAMETER                         ident                 pv al



Parameters

PARAMETER : command keyword

ident                : alphanumeric identifier. See table below.

pval                 : value of parameter ident. See table below. (Real or Integer)

                     Identifier            Definition and value

                     SUBINC                Number of plasticity subincrements (default 1) (see Appendix C.3). (Integer)

                     SUBTOL                Plasticity strain tolerance used to calculate a number of plasticity sub-
                                           increments (see Appendix C.3). (Real)

                     MXSUBI                Limit for number of plasticity subincrements (default 20). (Integer)

                     TREFLD                Reference temperature for temperature loads. (Real)

                     TAZERO                Absolute zero temperature for radiation calculations. (Real)

                     GAPSTF                Gap stiffness factor (default 1.0E3). (Real)

                     GAPSMA                Gap residual stiffness factor (default 1.0E-8) See GAP element description
                                           sheets (Appendix -A). (Real)

                     TIMBEG                Pseudo time corresponding to zero load state (default 0.0). (Real)

                     DRILF                 Stiffness multiplier for fictitious local RZ stiffness for shells (default 1.0E-
                                           08). (Real)

                     PENFUN                Penalty function multiplier for fictitious local RZ stiffness for shells (used in
                                           conjunction with FLATOL) (default 1.0). (Real)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-25
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     FLATOL                Shell flatness threshold to activate penalty function control of local RZ
                                           stiffness (largest angle between opposite diagonal normals in degrees)
                                           (default 90.0). (Real)

                     SHEARL                Shear locking reduction factor for TCS and TSD elements (default 19.2).
                                           (Real)

                     LNMULT                Line search multiplier for control parameter adjustment. (Real)

                     EIGCNV                Subspace iteration convergence tolerance (default 1.0E-05). (Real)

                     MXAUTO                Limit for number of repeated AUTO restarts for special solution methods
                                           (default 3). (Integer)

                     FINCMX                Maximum step increasing actor for special solution methods. (default 1.5 for
                                           LOAD, 10.0 for ARCL, TARCL and CONSIT). (Real)

                     TINCMX                Maximum timestep for special solution method LOAD. (Real)

                     TINCMN                Minimum timestep for special solution methods LOAD. (Real)

                     KSIGNL                Number of consecutive step increasing signal before actual increase is made
                                           for special solution method LOAD (default 2). (Integer)

                     STEPRF                Step reduction factor in auto-restart for special solution methods (default
                                           0.5). (Real)

                     SCONLO                Solution diagonal decay ratio - warning threshold (default 1.0E5). (Real)

                     SCONHI                Solution diagonal decay ratio - abort threshold (default 1.0E12). (Real)

                     SERCH1                Line search tolerance for interpolation (default 1.0). (Real)

                     SERCH2                Line search tolerance for extrapolation (default 0.7). (Real)

                     SERCL1                Lower limit for line search factor (default 0.01). (Real)

                     SERCL2                Upper limit for line search factor (default 10.0). (Real)

                     FACLSP                Line spring factor (default 0.4). (Real)

                     MXAUGM                Maximum number of Lagrangian augmentations (default 0). (Integer)

                     GAPCVG                Penetration tolerance for Lagrangian augmentations (default 0.001). (Real)

                     TANCVG                Tangential relative displacement tolerance at stick positions for Lagrangian
                                           augmentation (default 0.001). (Real)

Notes

1.      SUBINC and SUBTOL are mutually exclusive.
2.      TREFLD and TIMBEG cannot be redefined on a restart.
3.      Some identifiers may be specified in both the PARAMETER and TEMPORAL command. If an
        identifier is defined more than once, the last definition will be assumed.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-26
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


5.1.21      PASS Command

This command invokes the frontwidth optimisation facility. Optional


         PASS                   (method)                 (npass)




Parameters

PASS              : command keyword

method            : optional word; KING, LEVY, PINA, or SLOAN, to indicate method of optimising. If blank,
                     CUTHILL-MCKEE is assumed. However, when the optimised frontal solver is adopted, the
                     default method is SLOAN.

npass             : number of attempts to reduce the frontwidth. If blank, defaults to 2 for SLOAN and 10 for
                     other methods. (Integer)

Note

1.      The frontwidth optimiser assumes that all elements with the same node number are connected together
        according to data given in element topology data. In the situation where elements contain an auxiliary
        node (SST4, STF4, and WST4), it is advisable to assign a unique node number to each auxiliary node so
        that the final outcome of the optimisation process will not be affected.

2.      Two passes are always performed with SLOAN unless npass is explicitly set to 1.

3.     The SLOAN method is only available with the optimised frontal solver.




5.1.22      PINO Pressure Interpolation Order Command

The PINO command defines the pressure interpolation order to be used by specified elements. To avoid
numerical problems with incompressible or nearly incompressible materials, this command may be used to
specify a different (lower) interpolation order for the volumetric strain. If the PINO command is not present the
normal displacement formulation is used. Optional


            PINO                   inpr                     (elno)




Parameters

PINO          : command keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-27
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


inpr          : pressure interpolation order. (Integer)

elno          : list of element numbers in topological format. (Integer)
                If blank, defaults to all elements (in group)

Notes

1.       This command is recommended for use with the hyperelastic material model
2.       The recommended pressure interpolation orders and the associated element types are given below:

Interpolation            Elements
order

     1                   BRK6          BRK8         BR15         BR20
                         QUM4          QUM8         TRM3         TRM6
                         QUX4          QUX8         TRX3         TRX6

     3                   QUM8          TRM6         QUX8         TRX6

     4                   BR15          BR20

Example


A rubber membrane with a mesh of 100 high order membrane elements (QUM8’s and TRM6’s)

         PINO 3 (100) (1,1)



5.1.23      PROBLEM and TITLE Command

This command is mandatory and must immediately follow the JOB command.

                 PROBLEM
                                                   (direct)                 (*          title)

                    TITLE




Parameters

PROBLEM           : command keyword

TITLE             : command keyword

direct            : 4 character directives defining structural and material model to be used. May be one or more
                     of the following:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-28
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


                     GLST         compute stresses/strains in global axis system
                     LOST         compute stresses/strains in local axis system
                     PLAS         take plasticity effects into account
                     LARG         include large displacement effects in the calculation of strains and geometric
                                  stiffness matrices.         This directive should be accompanied by the command
                                  UPDATE GEOM (see UPDATE command)
                     CONL         use conservative pressure loading - i.e. calculate pressure loads using original
                                  geometry throughout.            Only applicable with UPDATE GEOM (see UPDATE
                                  command)
                     NRES         do not carry forward residuals into next increment.
                     FLNS         form natural stiffness (i.e. Young’s modulus*Area) for FLA2 and FAT2 elements
                     CREP         creep analysis
                     EXPL         use explicit temporal integration scheme for transient analysis

*                 : character to indicate the following text forms the title

title             : any alphanumeric title of up to 60 characters including blanks. It must be preceded by an
                     asterisk (*). This title will be printed at the top of each page of ASASNL output

Notes

1.      If no directives are given linear elastic behaviour is assumed with the default implicit temporal integration
        scheme for transient analysis and stresses are computed in the element default axis system.
2.      This is a global switch and will set these directives for all groups regardless of what is put on the GROUP
        commands. You can, however, add other directives with the GROUP commands.
3.      The first six characters of the title are used for the problem name.
4.      The PROBLEM command and TITLE command are identical and interchangeable.




5.1.24      PROJECT Command

To define a name and title for the project. Optional but project name is recommended.


         PROJECT                     (pname)                 (*         title)




Parameters

PROJECT           : command keyword

pname             : project name for current run (Alphanumeric, 4 characters, first character must be alphabetic). If
                     pname is omitted, then pname defaults to the name ASNL

*                 : character to indicate following text forms the project title.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-29
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


title             : any alphanumeric title of up to 60 characters including blanks. It must be preceded by an
                     asterisk (*). The default project title is ‘ASAS-NL ARCHIVE FILE’

Notes

1.      All runs with the same project name access the same ASAS data base and hence this must be the same in
        all restarts. A project data base consists of one project file (with a file name consisting of the 4 characters
        of pname with the number 10 appended) which acts as an index to other files created under this project,
        together with those other files.
2.      The title is used by the program as an identifier for the archive files saved. Subsequent jobs requiring to
        use those files must have the same identifying title (in addition to the correct file names with the FILE
        command).




5.1.25      RESTART Command

This command is used in restarted runs in place of the SOLVE command. It defines times at which a solution is
to be attempted. It must follow the PROBLEM or TITLE command. Compulsory

                                     TGEN                stime               timei              ntime
        RESTART

                                      time




Parameters

RESTART           : command keyword

TGEN              : keyword indicating that a list of times is to be generated

stime             : start time for list of generated times. (Real)

timei             : time increment to be added to start time for list of generated times. (Real, ≥ 0.0)

ntime             : total number of generated times, including start time. (Integer, >0)

time              : time for solution. (Real)

Notes

1.      All times must be non-negative.
2.      The first time, time1, must correspond with the time on the restart file for the chosen checkpoint and
        agree within 3 decimal places. The checkpoint number is defined using the JOB command.
3.      No solution is attempted at time, time1.
4.      Solution times may be continued using subsequent RESTART commands.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-30
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


5.      All solution times specified must be greater than or equal to zero. (In general they must be greater than or
        equal to TIMBEG, the zero load start time.)
        The list must also be in ascending order i.e. time (i+1) ≥ time(i).
6.      If load functions are used, then all solution times specified must be greater than, or equal to the first
        pseudo time specified with each load function.
7.      On a restart, only the preliminary data, suppressions, displaced freedoms, loading and additional mass can
        be changed. Material property data may also be changed but only if the analysis type has been changed
        from the initial run.
8.      If temperature data is redefined on restart, the number of load sets must be the same as on the initial run.




5.1.26      RESU (or POST) Commands

This command defines the points and the information to be saved for post-processing with POSTNL, on the file
specified on a corresponding FILE command. It also defines the points where information is to be saved on the
ASAS database. Recommended




Parameters

RESU              : command keyword

POST              : command keyword (same meaning as RESU)

outid             : output identifier, one or more of the following:

                     DISP         displacements (temperatures for heat)
                     VELO         velocities (temperature rates for heat)
                     ACCN         accelerations
                     REAC         reactions (reactive nodal heat for heat)
                     STRS         stresses (fluxes for heat)
                     STRN         total strain (field for heat)
                     INST         inelastic strains
                     ELAS         elastic strains
                     SRES         stress resultants
                     WORK         element mechanical work (NOT saved to ASAS database)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-31
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     TEMP         temperatures (NOT saved to ASAS database)
                     EIGN         mode shapes
                     CRSN         creep strains
                     SUMR         output summary of maximum displacements, velocities, accelerations, summed
                                  reactions and solution control information (only summed reactions saved to ASAS
                                  database)

TGEN              : keyword indicating that a list of times is to be generated

stime             : start time for list of generated times. (Real)

timei             : time increment to be added to start time for list of generated times. (Real, ≥ 0.0)

ntime             : total number of generated times, including start time. (Integer, > 0)

IGEN              : keyword indicating that a list of increments is to be generated

incst             : start increment for list of generated increments. (Integer)

iinc              : increment to be added to start increment for list of generated increments. (Integer, > 0)

nincs             : total number of generated increments, including start increment. (Integer, > 0)

ALL               : keyword indicating that information is to be stored for all increments

INCR              : keyword indicating that a list of increment numbers is supplied

incno             : increment number for which results are to be stored. (Integer)

TIME              : keyword indicating that a list of times is supplied

time              : time for which results are to be stored. (Real)

Notes

1.      SRES must be saved if layer stresses/strains or failure indices are required to be recovered in POSTNL
        for an elastic laminated shell analysis.
2.      DISP, STRS, STRN, ELAS and INST (if plasticity) must be saved if fracture mechanics processing is
        required in POSTNL. For creep fracture, CRSN must also be saved in addition and results from at least
        two increments must be available.
3.      INCR or IGEN may only be used with SOLUTION solution method.
4.      TIME or TGEN may only be used with SOLVE solution method.
5.      Information written to the ASAS database consists of two parts. The first part is equivalent to the
        specification of SAVE LOCO FILES in ASAS. Data which will only be generated for ASAS
        compatible element types, are written to the “35 file”. The second part concerns with saving of results.
        This information is written to the “45 file”.
6.      If post-processing using POSTNL is not required, option NOPF can be used to supress the generation of
        porthole file. Data will always be written to the ASAS database




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-32
ASAS (Non-Linear) User Manual                                                                                   Preliminary Data


7.     POST/RESU command alone will cause saving of DISP, STRS and SUMR in all increments/times. In
       addition, the SURFACE FAILURE results will be saved to the ASAS database in a job involving
        plasticity or failure.
8.      If the results database is to be used in any post-processing run then a RESU command must be included
       in the initial ASAS run to initialise the database.
9.     The last POST/RESU command at a time overrides all the previous specifications.




5.1.27      SAVE Command

This command defines points at which run information is stored on the stiffness and data manager archive files.
File names are defined on appropriate FILE commands. Optional
                                                        STEP                     ninc

                          NEW
       SAVE
                          OLD                                                                           ALL
                                                         (ROLL                 nsol)
                                                                                                        ptminc




Parameters

SAVE              : command keyword

NEW               : keyword to indicate that new files are to be created

OLD               : keyword to indicate that existing files are to be used - information is appended to the old files
                     (except that a restarted run from an intermediate checkpoint will override previously dumped
                     information for higher checkpoints)

STEP              : keyword to indicate that information is to be stored every ‘ninc’ increments

ninc              : see above. (Integer)

ROLL              : keyword to indicate that a rotating set of ‘nsol’ solutions will be stored on the archive file

nsol              : see above. (Integer)

ALL               : keyword to indicate that information is to be stored after all load increments

ptminc            : pseudo time (Real) or increment (Integer) for which restart information is to be stored




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 5-33
ASAS (Non-Linear) User Manual                                                                           Preliminary Data


Notes

1.      If OLD then there should not be any FILE commands referring to new stiffness and archive files.
2.      Information is saved on the stiffness archive file only if stiffnesses have been updated since the previous
        checkpoint.
3.      Information is always saved on both files on the last increment of a successful analysis.
4.      ROLL should not be used to hold less than 3 increments.




5.1.28      SCALING Command

Controls scaling of applied loads for proportional loading to a factor times yield stress on first load increment.
See Note.


          SCALE                      ident             v al




Parameters

SCALE             : command keyword

ident             : an alphanumeric identifier. If no identifier is specified, then applied loads are scaled until first
                     yield is reached. Allowable identifiers are as follows:

                     RPROP             Reference proportion for scaling.               The reference value for scaling is this
                                       proportion multiplied by the yield stress. The default value is one.

                     SCALIM            This specifies a ceiling value to the load factor. If omitted no limiting value is
                                       enforced.

val               : value for selected identifier. (Real)

Note


This command is an alternative to the SOLVE command. The job terminates after scaling to the value given
and can be restarted as requested. No SAVE command is required.




5.1.29      SKIP Command - (Group Section Only)

This command defines the elements to be skipped from a group. It is valid only in conjunction with an
ELGROUP command.

Optional




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-34
ASAS (Non-Linear) User Manual                                                                          Preliminary Data




                SKIP                              elno




Parameters

SKIP          : command keyword

elno          : list of element numbers given in topological format. (Integer)

Notes


The order of ELGROUP and SKIP Commands within a group is not important.

Example


Assign elements 1, 2, 4, 6, 9, 10 to group 3

            GROU         3             *            BEAM         ELEMENTS
            ELGR         (10)          (1,1)
            SKIP         3             5
            SKIP         (2)           (7,1)




5.1.30      SLEEP Command

This command defines the elements which will become inactive (sleep) during part of the analysis. Optional

                                ptime
         SLEEP                                                elno
                                incno




Parameters

SLEEP         : command keyword

ptime         : pseudo time at which element sleeps (SOLVE). (Real)

incno         : increment number at which element sleeps (SOLUTION). (Integer)

elno          : list of element numbers in topological format. (Integer)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-35
ASAS (Non-Linear) User Manual                                                                             Preliminary Data


Notes

1.      The same element number cannot be specified more than once in the entire list of SLEEP commands.
        This means that an element cannot sleep more than once during a run.
2.      The element is put to sleep before the solution for the specified time/increment number is obtained. Thus
        the element is inactive for the time/increment number specified and for all times/increment numbers
        thereafter. It is important to note that global mass, damping and stiffness matrices are not updated unless
        specifically requested. Appropriate UPDATE commands should be specified at the time/increment
        number specified with the SLEEP command.
3.      If the pseudo time specified is within the lower and upper limits of solution times given on the SOLVE
        (or RESTART) commands, then it must coincide with one of the solution times.
4.      If both WAKE and SLEEP times/increment numbers are present for an element, the wake
        time/increment has to be before the sleep time/increment number.
5.      The list of element numbers specified with the WAKE/SLEEP commands cannot be changed during any
        subsequent restart analysis.
6.      Care should be taken using the WAKE/SLEEP commands when load type NODAL LO has been
        specified. Internally, ASAS-NL attaches all nodal loads to the element with the highest system element
        number which references the freedom to which the nodal load is applied. When an element which has
        nodal loads attached in this manner is woken up or put to sleep, the nodal load is also woken up or put to
        sleep, as are all element loads.




5.1.31      SOLUTION Command

Defines automatic load (or time) stepping procedure for static and transient dynamics analysis in a virgin run
(used instead of SOLVE command). If used this command must immediately follow the PROBLEM or TITLE
commands. For restarted runs, the SOLUTION command is replaced by the SRESTART command. Note that
SOLUTION (and SRESTART) cannot be used for creep analysis. Instead, the creep automatic timestepping
procedure is activated by specifying AUCR in the OPTION command together with SOLVE (or RESTART)


            SOLUTION                    method              ninc                      direct            v al




Parameters

SOLUTION:                command keyword

method        : special solution method name (Alphanumeric). Valid methods are:

                LOAD              Constant load control. This method is applicable to static analysis with any load
                                  history types. It is not suitable for predicting limit point or snap behaviour.
                ARCL              Cylindrical arc-length control (i.e. constant displacement vector increment
                                  (DPVEC)). Constraint on the step size has quadratic form, thus no distinction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-36
ASAS (Non-Linear) User Manual                                                                             Preliminary Data


                                  between the positive and negative path direction is available.                 This method is
                                  applicable to static analysis with proportional loading only. It can deal with limit
                                  point or snap behaviour.
                TARCL             Linearised cylindrical arc-length control.                 This method is applicable to static
                                  analysis with proportional loading only.                 It can deal with limit point or snap
                                  behaviour.
                CONSIT            Constant displacement component increment (DPCOM) control. Constraint on the
                                  step size has linear form, thus positive and negative value of an increment is
                                  recognised. This method is applicable to static analysis with proportional loading
                                  only. It can deal with limit point or snap behaviour.
                DOMFRQ            Dominant frequency control. This method is applied to transient dynamics analysis
                                  using implicit time integration only.
                MAXFRQ            Maximum frequency control. This method is applied to transient dynamics analysis
                                  using explicit time integration only
ninc:           maximum number of increments to be attempted.
direct:         alphanumeric directive. See table below
val:            value(s) associated with the directive. (Integer, Real or Character, see table below)




Below are the directives for use with the SOLUTION and SRESTART commands.

(A)         For method LOAD

            Identifier Definition and value

            FIRTIM         The first solution pseudo-time. (Real, ≥last solution time)
            FIRTIN         The initial pseudo-time increment. (Real, >0.0)
            MAXTIM The maximum solution time. (Real, ≥last solution time)
            ITERD          Desired number of iterations per increment. If set to zero step size adjustment is
                                       independent of number of iterations (default 4). (Integer, ≥0)

Notes


1          FIRTIM and/or FIRTIN must be specified. If FIRTIM is omitted, the first solution time is assumed to
           be the last solution time in the previous run (or 0.0 for a new run). Conversely, if FIRTIN is omitted,
           the initial time step size is taken as the difference between FIRTIM and the last solution time (or 0.0
           for a new run). If both are specified, the first solution time will be FIRTIM while the next step (i.e. the
           second step) will have a step size of FIRTIN.
2          Additonal control parameters are available in the PARA commands.                             These include FINCMX,
           TINCMN, TINCMX, KSIGNL, STEPRF and MXAUTO.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-37
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



3          The automatic load procedure may not be effective when there is a sudden change of loading from the
           previous increments. If difficulty arises, a restart should be carried out with the load stepping control
           parameters re-defined.
4          The run terminates when either the maximum number of increments or the maximum solution time is
           reached. In the latter case, the last solution will always be attempted at time MAXTIM.
5          Further details are given in Appendix C.

(B)        For methods ARCL, TARCL and CONSIT

            Identifier        Definition and value

            WORKC             Adopts constant external work increment control in conjunction with ARCL or
                              CONSIT. May not be used on first restart following standard solution procedure.
                              Switch tolerance. If set to zero this procedure is used in all increments. (Real)
            AUTO              Automatic selection of displacement component to be controlled. Used with CONSIT
                              only.
                              Size of incremental displacement. (Real)
            INITPR            Defines initial step size. Used with ARCL and TARCL only.
                              Initial proportion of reference load. (Real)
            INCDIS            Defines initial step size.          Mandatory with CONSIT and optional for ARCL and
                              TARCL. Three parameters to follow:
                              Nominated node. (Integer)
                              Nominated freedom name. (Alphanumeric)
                              Initial incremental displacement of nominated freedom. (Real)
            ITERD             Desired number of iterations per increment. If set to zero step size adjustment is
                              independent of number of iterations (default 4). (Integer, ≥0)
            MAXIPR            Maximum incremental proportion of reference load. used with CONSIT only. (Real)
            MAXLOD            Terminates the run when this proportion of reference load is exceeded. (Real)
            MAXDIS            Terminates the run when total displacement of the specified freedom is exceeded. Three
                              parameters to follow:
                              Nominated node. (Integer)
                              Nominated freedom name. (Alphanumeric)
                              Maximum displacement of nominated freedom. (Real)
            CONDIR            Controls loading direction. Used on restarts with ARCL and TARCL only..
                              Controlling parameter taking value +1.0 or -1.0. (Real)

Notes


1          INITPR or INCDIS must be specified when ARCL or TARCL is used.
2          Additional control parameters are available in the PARA commands.
3          These procedures can only be applied to static analysis with proportional loading.
4          For analysis containing a dead load set (i.e. non-proportional part) and a live load set (i.e. proportional
           part), the dead loads may be applied in a SOLVE run followed by restart using the special solution
           procedure for the live loads.              In this case, only the proportional load data is required in the
           SRESTART run.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-38
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


(C)         For methods DOMFRQ and MAXFRQ

            Identifier        Definition and value



            FIRTIM            The first solution time. (Real, ≥last solution time)
            FIRTIN            The initial timestep size. (Real, >0.0)
            MAXTIM            The maximum solution time. (Real, ≥last solution time)
            ITERD             Desired number of iterations per increment. if set to zero step size adjustment is
                              independent of number of iterations (default 4). (Integer, ≥0)

Notes


1          FIRTIM and/or FIRTIN must be specified. If FIRTIM is omitted, the first solution time is assumed to
           be the last solution time in the previous run (or 0.0 for a new run). This setting is useful for
           determining the consistent initial accelerations from given initial conditions and/or initial loading.
           Conversely, if FIRTIN is omitted, the initial time step size is taken as the difference between FIRTIM
           and the last solution time (or 0.0 for a new run). If both are specified, the first solution time will be
           FIRTIM while the next step (i.e. the second step) will have a step size of FIRTIN.
2          Additional control parameters are available in the PARA and TEMP commands.
3          Further details are given in Appendix K.




5.1.32      SOLVE Command

This command invokes the classical solution method (incremental Newton-Raphson) and defines points at which
a solution is to be attempted for a virgin run. It must follow either the PROBLEM/TITLE command. In
restarted runs it is replaced by the RESTART command.

                                TGEN                   stime             timei             ntime
         SOLVE
                                   time




Parameters

SOLVE             : command keyword

TGEN              : keyword indicating that a list of times is to be generated

stime             : start time for list of generated times. (Real)

timei             : time increment to be added to start time for list of generated times. (Real, ≥ 0.0)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-39
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


ntime             : total number of generated times, including start time. (Integer, > 0)

time              : time at which a solution is to be attempted. Times must be non-negative. (Real)

Notes

1.      List of times may be continued using subsequent SOLVE commands.
2.      The solution method activated by the SOLVE command can be used for static problems of proportional
        or non-proportional loading. The latter is defined by explicitly specifying load history. Otherwise
        proportional loading is assumed with the load multiplier equal to the time at each solution point.
3.      This solution method is compulsory for creep analysis.
4.      All solution times specified must be greater than or equal to zero. (In general they must be greater than or
        equal to TIMBEG, the zero load start time.)
        The list must also be in ascending order i.e. time(i+1) ≥ time(i).
5.      If load functions are used for solution times specified outside the pseudo times specified with each load
        function, extrapolation will be used.




5.1.33      SPIT Command

This command sets the parameters for the Subspace Iteration Eigen Solution. If present it must be accompanied
by an EIGN command. Optional and only for Eigen Solution.
                      KGEOM

             SPIT                 UNITM                       ident               v al

                                  MASS



Parameters

SPIT              : command keyword

KGEOM             : keyword to indicate that the current small displacement stiffness Ko and the geometric stiffness
                     KG matrices are to be used for a buckling analysis

UNITM             : keyword to indicate that the current small displacement stiffness Ko and the unit I matrices are
                     to be used for a spectral analysis

MASS              : keyword to indicate that the current tangential stiffness KT and the mass M matrices are to be
                     used for a natural frequency analysis

ident             : alphanumeric identifier. See table below

val               : value associated with the specified identifier. (Integer and Real)

                     Identifier            Definition and value




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-40
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     NORME                 Eigenvector normalisation. (Integer)
                                           0 Maximum component is 1.0 (default)
                                           1 Euclidean norm is 1.0

                     SCOPE                 Scope of solution. (Integer)
                                           0 Eigenvalues and modes (default)
                                           1 Eigenvalues only

                     NHIGHF                Number of eigenvalues required. (Integer)
                                           1≤NHIGHF≤NSUBSP                    (default to 1)

                     NSUBSP                Number of eigenvalues to iterate over (size of subspace). If omitted then
                                           default value is calculated automatically by the program. (Integer)
                                           0≤NSUBSP≤NFREE, where NFREE is the number of free freedoms.

                     LMSPIT                Maximum number of iterations in eigenvalue solution (default 45) (Integer)

                     EIGCNV                Convergence tolerance in eigenvalue solution (default 0.00001). (Real)

                     SELMOD                Number of mode selected for perturbation.
                                           1<SELMOD<NHIGHF (default 1). (Integer)

                     PERTMG                Relative magnitude of perturbation (default 0.005). (Real)

                     STURM                 Sturm sequence check flag. (Integer)
                                           0 =      no check (default)
                                           1 =      check required

                     SHIFT                 Eigenvalue shift (default 0.0). (Real)
                                           The shift should be specified in eigenvalue units for buckling problems.
                                           The shift should be specified in frequency units (Hz) for natural frequency
                                           problems

                     STARTV                Method for forming the Starting Vectors
                                           0    =    Vectors generated based on the stiffness to mass ratio (default)
                                           1    =    Use last calculated eigenvectors as starting vectors

Notes

1.      To obtain the KG matrix for SST4/WST4 elements the LARG directive must be specified with the
        GROUP or PROBLEM/TITLE commands.
2.      See Appendix C.5 for further details concerning eigenvalue analysis.
3.      Load stiffness will only be ignored if CONL is specified with the GROUP or PROBLEM/TITLE
        commands.
4.      A shift must be applied if there are not enough suppressions in the model to remove all the rigid body
        motions. Eigenvalue analysis of a free structure is allowed for UNITM and MASS provided no loading is
        applied. The structure must have adequate suppressions for KGEOM.
5.      NHIGHF and NSUBSP will be reset if their specified values are outside the allowable bounds.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-41
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


6.       The eigenvalues of a shifted problem are arranged in ascending order of their distance from the shift
         origin. The eigenvalues of the original problem, which are reported in the output file, will be given in the
         same order.
7.       The sturm sequence check implemented assumes that the lowest modes have been computed and the
         eigenvalues are monotonially increasing. It should not be applied to problems where these conditions are
         not satisfied. One such example is when a shift is applied to determine the higher modes directly.
8.       The use of last calculated eigenvectors as starting vectors is only allowed in a restart analysis if the
         subspace size NSUBSP remains unchanged between runs.




5.1.34      SRESTART Special Solution Restart Command

Defines special solution options for restart run. (Used instead of RESTART command and must follow the
PROBLEM or TITLE command.)

       SRESTART            FROM           incno           method          ninc               direct       v al




Parameters

SRESTART : command keyword

FROM              : keyword

incno             : increment number of increment immediately before start. (Integer)

method            : special solution method name. See SOLUTION command for valid names.

ninc              : maximum number of increments to be attempted.

direct            : alphanumeric directive The directives used vary according to the special solution option
                     selected. See the table detailed with the SOLUTION command, and below.

val               : value(s) associated with the directive. (Integer, Real or Character)

The directive below is for use with SRESTART command only.

                     Identifier            Definition and value

                     STEP                  Defines directly step size. Used with ARCL only.
                                           Length of incremental displacement vector. Is used as an alternative to
                                           INITPR or INCDIS. (Real)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-42
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


Notes
1.      The loading information will not be correctly transferred to the ASAS database if the restart adopts a
        variable load solution procedure (e.g. ARCL) while the initial run adopts a fixed load procedure (SOLV
        or SOLU LOAD). This may affect the results of code checking using BEAMST.



5.1.35      START Command

This command defines the list of starting node numbers for any renumbering attempt specified with the PASS
command. This command must only be used in conjunction with the PASS command and need not be present.
If absent the renumbering will commence from a point chosen by the program. (A maximum of 3 START
commands can be provided and each one can consist of up to 10 nodes). Optional


             START                      nodeno




Parameters

START             : command keyword

nodeno            : node number with which to start any renumbering attempt. A maximum of 10 node numbers
                     may be specified. (Integer)

Notes


1           Up to 3 starting vectors may be specified.

2           Number of passes will be equal to number of starting vectors if START is used.

3           START will have no effect on the Sloan method and, thus, is not required when adopting this method.




5.1.36      STRUCTURE Command

To define the structure name for a new run or an existing model name for a restarted run. Optional but
recommended.


         STRUCTURE                      sname




Parameters

STRUCTURE :                   keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-43
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


sname             : structure name. The name must be unique from all other structure names in this project.
                              (Alphanumeric, 4 characters, the first character must be alphabetic)

Notes

1.      sname is used as a prefix for all ASAS backing files created during a new run. The four characters are
        appended with two digits to create each individual file. In a restarted job, this defines an existing
        structure from which the current run is based upon.
2.      If the STRUCTURE command is omitted then the project name pname is used in place of sname

Example


        STRUCTURE             SHIP




5.1.37      SYSPAR Command

This command, if present, must precede the JOB command. It allows the values of certain system parameters to
be reset. Optional


            SYSPAR                     ident           v al




Parameters

SYSPAR            : command keyword

ident             : alphanumeric identifier. See table below

val               : value associated with the specified identifier. (Integer or Logical)

                     Identifier            Definition and value

                     LPGSIZ                Data manager page size. (Integer, must not exceed 16383)

                     MINPAG                Minimum number of incore pages reserved for data manager. (Integer)

                     LTPAGE                Maximum length of page directory. (Integer, must not exceed 65535)

                     LMJIA                 Length of archive file major index. (Integer, must not exceed 16383)

                     MANREC                Default length of subindex. (Integer)

                     IPERM                 1 = use permanent files; 0 = use temporary files. (Integer)

                     NOPAG                 Block multiplier for LENTRK (length solution backing files). (Integer)

                     SINDEC                .TRUE. if reduced stiffness to be archived (if .FALSE., this file will be
                                           reformed by decomposing the stiffness file on restarts) (Logical)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-44
ASAS (Non-Linear) User Manual                                                                              Preliminary Data



                     LEVSYS                System abort level. (Integer)

                     MXCONS                The maximum of MXCONS and NCONEQ constraint equations will be
                                           allowed for restarts. (Integer.)             NCONEQ is the number of constraint
                                           equations in the initial run.

                     OPENFL                Default number of keys with which an internal ASAS file is opened (integer)

Notes

1.      See Table 6.1 for default values and Section 6.2 for the significance of some of the system parameter.
2.      In a restart, new constraint equations can be added but cannot contain a constant term.
3.      LPGSIZ and LMJIA must be the same and the program will ensure this if either is specified.




5.1.38      SYSTEM Command

To define the amount of data space to be allocated during the run. Optional.
                             SMALL


        SYSTEM                      (MEDIUM)                   DATA              AREA                   memory    (initm)


                                    LARGE



Parameters

SYSTEM            : command keyword

SMALL             : keyword indicating data manager page size

MEDIUM            : keyword indicating data manager page size (default size)

LARGE             : keyword indicating data manager page size

DATA              : keyword

AREA              : compulsory keyword

memory            : amount of memory (in 4 byte words) to be used by this run. A minimum of 1000000 is
                     assumed. (Integer)

initm             : initial memory reserved. Not normally used. (Integer)

Note


See Table 6.1 for optional page sizes.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-45
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


5.1.39      TEMPORAL Command

This command allows the user to vary the temporal integration scheme used for transient analysis and the
parameters associated with automatic timestepping.


             TEMPORAL                        ident               v al




Parameters

TEMPORAL             :        command keyword

ident             : alphanumeric identifier. See table below.

val               : value of identifier. See table below.

                     Identifier            Definition and value

                     TALPHA                Temporal integration scheme coefficient (default 0.0). (Real)

                     TBETA                 Temporal integration scheme coefficient (default 0.5). (Real)

                     TGAMMA                Temporal integration scheme coefficient (default 0.25). (Real)

                     VALPHA                Creep integration weighting factor. Any value between 0.0 and 1.0 may be
                                           used. (Default 0.0). (Real)

                     DCSTMX                Autocreep control parameter (use with OPTION AUCR only). Maximum
                                           incremental creep strain. (Real)

                     DCESMX                Autocreep control parameter (use with OPTION AUCR only). Maximum
                                           ratio of incremental creep strain to total strain. (Real)

                     DSIGMX                Autocreep control parameter (use with OPTION AUCR only). Maximum
                                           ratio of incremental stress to total stress. (Real)

                     TINCMX                Automatic timestepping control parameter for creep and transient dynamics.
                                           Maximum timestep. (Real)

                     TINCMN                Automatic timestepping control parameter for creep and transient dynamics.
                                           Minimum timestep. (Real)

                     FINCMX                Automatic timestepping control parameter for creep and transient dynamics.
                                           Maximum ratio of new timestep to previous timestep. (Real)

                     FIRSTP                Autocreep control parameter (use with OPTION AUCR only).                  First
                                           timestep for this solution or restart. (Real)

                     MXINCS                Autocreep control parameter (use with OPTION AUCR only). Maximum
                                           number of timesteps for this solution or restart. (Integer)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-46
ASAS (Non-Linear) User Manual                                                                          Preliminary Data



                     TFACLO                Automatic timestepping control parameter for transient dynamics. Lower
                                           limit on ξ for no change in timestep. (Real)

                     TFACHI                Automatic timestepping control parameter for transient dynamics. Upper
                                           limit on ξ for no change in timestep. (Real)

                     TFACRJ                Automatic timestepping control parameter for transient dynamics. Limit on ξ
                                           below which the current solution will be rejected. (Real)

                     FRAPRD                Automatic timestepping control parameter for transient dynamics. Desired
                                           fraction of the characteristic period for determining the timestep. (Real)

                     KSIGNL                Automatic timestepping control parameter for transient dynamics. Number
                                           of consecutive timestep increasing signal before an actual increase is made.
                                           (Integer)

                     IPDICT                Predictor type for transient dynamics. (Integer)
                                           1. Predictor acceleration equals to 0.0. (Default)
                                           2. Predictor displacement equals to displacement at end of last step. Note
                                           that this must not be used in explicit analysis or when TBETA=0.0.

                     HGAMMA                Temporal integration scheme parameter for transient heat (default 1.0).
                                           (Real)

Notes

1.      See Appendix -J for full details concerning the individual parameters for creep analysis.
2.      See Appendix -K for full details concerning the individual parameters for transient dynamic analysis.
3.      See Appendix N for full details concerning the individual parameters for transient heat analysis
4.      Some identifiers may be specified in both the PARAMETER and TEMPORAL commands. If an
        identifier is defined more than once, the last definition will be assumed.




5.1.40      TEXT Command

To define a line of text to be printed once only at the beginning of the output. Several TEXT lines may be
defined to give a fuller description of the current analysis on the printed output.

Optional




                TEXT                     text



Parameters

TEXT        :   command keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-47
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


text        :   this line of text will be printed once, at the beginning of the output. (Alphanumeric, up to 75
            characters)

Example

       TEXT     THIS EXAMPLE OF THE TEXT
       TEXT     COMMAND IS SPREAD
       TEXT     OVER THREE LINES




5.1.41      TITLE Command

See PROBLEM Command for full details of this command.




5.1.42      UNITS Command

Recommended.

This command allows the user to define the units to be employed in the analysis and the default units for the
input data. The defined unit set will appear on each page of the printout as part of the page header. If this
command is omitted then no units information will be reported and the units of all data supplied must be
consistent (see Section 3.11).

If the UNITS command is employed, facilities exist to locally modify the input data units within each main data
block. See Sections 5.2.1, 5.3.1, 5.4.1, 5.5.1 and 5.6.1 for further details.


5.1.42.1 Global UNITS Definition

This specifies the units to be employed for the analysis and provides the default units for input and printed
output.

                 UNITS                       unitnm




Parameters

UNITS                  : keyword

unitnm                 : name of unit to be utilised (see below)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-48
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


The units of force and length must be supplied. Temperature is optional and defaults to centigrade. A time unit
of seconds is assumed. A default angular unit of radians is used for results reporting. The default input angular
unit varies according to the data block and must not be specified on the basic UNITS command.

Restriction


The program calculates a consistent unit of MASS based upon the length and force units supplied. The
permitted combinations of force and length are given in Table 3.1.

Valid unit names


Length unit                                              METRE(S),                          M
                                                         CENTIMETRE(S),                     CM
                                                         MILLIMETRE(S),                     MM
                                                         MICROMETRE(S)                      MICM
                                                         NANOMETRE(S)                       NANM
                                                         FOOT, FEET,                        FT
                                                         INCH, INCHES,                      IN

Force unit                                               NEWTON(S)                          N
                                                         KILONEWTON(S)                      KN
                                                         MEGANEWTON(S)                      MN
                                                         TONNEFORCE(S)                      TNEF
                                                         POUNDAL(S)                         PDL
                                                         POUNDFORCE,                        LBF
                                                        KIP(S)                              KIP
                                                        TONFORCE(S)                         TONF
                                                        KGFORCE(S)                          KGF

Temperature unit                                        CENTIGRADE,                         C
                                                        FAHRENHEIT,                         F



Example
1.     Input data units and results units to be in units of Kips and feet

       UNITS KIPS FEET

       The derived consistent unit of mass will be 3.22x104 lbs.

Please also refer to Example 1 of Section 5.1.19.1 of the ASAS user manual.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-49
ASAS (Non-Linear) User Manual                                                                                Preliminary Data


5.1.43      UPDATE Command

These commands determine the type of solution procedure, by controlling the frequency with which the stiffness
and mass matrices are reformed and the structure geometry updated. If no update commands are specified, the
program defaults to the initial (elastic) stiffness procedure.
                                  GEOM

             UPDATE                     MASS                                   INCR                     ALL

                                        STIF              (ELAS)               ITER                     ptminc

                                                                               KT1

                                                                               KT2

                                                                               KT0



Parameters

UPDATE : command keyword

GEOM          : keyword to update the structure coordinates each iteration

MASS          : keyword to reform the mass matrix to account for changes in geometry

STIF          : keyword to reform the stiffness matrix to account for changes in stress/strain level and/or
                geometry

ELAS          : keyword to reform stiffness using elastic material properties

INCR          : keyword to reform matrix on first iteration only

ITER          : keyword to reform matrix on every iteration

KTO           : keyword to reform stiffness matrix on first iteration of first increment only (default)

KT1           : keyword to reform stiffness matrix on first iteration

KT2           : keyword to reform stiffness matrix on second iteration

ALL           : keyword to perform update specified for all increments

ptminc        : pseudo time/time (Real) or increment number (Integer) at which update is to be performed




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-50
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


Notes

1.      Except for cases when the nonlinearity is low, updating of the geometry and the stiffness matrix should be
        combined with the directive LARG with the PROBLEM/GROUP command.
2.      For the case of pressure loading, the current geometry is always used to calculate the equivalent nodal
        loads. Therefore, using UPDATE GEOM will result in non-conservative pressure loading.
3.      If OPTION VISC is set (for viscoplastic creep solution) the stiffness matrix is automatically updated at
        each iteration.




5.1.44      WAKE Command

This command defines the elements which will become active (wake up) during part of the analysis. Optional

                             ptime
         WAKE                                                 elno

                             incno




Parameters

WAKE          : command keyword

ptime         : pseudo time at which element wakes up (SOLVE). (Real)

incno         : increment number at which element wakes up (SOLUTION). (Integer)

elno          : list of element numbers in topological format. (Integer)

Notes

1.      The same element number cannot be specified more than once in the entire list of WAKE commands.
        This means that an element cannot wake up more than once during a run.
2.      The element is woken up after the solution for the specified time/increment number has been obtained,
        including any eigensolution requested. Thus, the element is effectively active from the time/increment
        number following the time/increment number specified with the WAKE command. It is important to
        note that global mass, damping and stiffness matrices are not updated unless specifically requested.
        Appropriate UPDATE commands should be specified for the time/increment number when the element
        becomes active, i.e. at the time/increment number following the time/increment number specified with the
        WAKE command.
3.      If the pseudo time specified is within the lower and upper limits of solution times given on the SOLVE
        (or RESTART) commands, then it must coincide with one of the solution times.
4.      If both WAKE and SLEEP times/increment numbers are present for an element, the wake time
        increment number has to be before the sleep time/increment number.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-51
ASAS (Non-Linear) User Manual                                                                          Preliminary Data


5.      The list of element numbers specified with the WAKE/SLEEP commands cannot be changed during any
        subsequent restart analysis.
6.      Care should be taken using the WAKE/SLEEP commands when load type NODAL LO has been
        specified. Internally, ASAS-NL attaches all nodal loads to the element with the highest system element
        number which references the freedom to which the nodal load is applied. When an element which has
        nodal loads attached in this manner is woken up or put to sleep, the nodal load is also woken up or put to
        sleep, as are all element loads.




5.1.45      WEIGHTS Command

This command is used in conjunction with the DISP or RESF options of the CONVERGE command to enable
the user to weight each term when calculating the convergence criteria.


         WEIGHTS                  freedom                  rv al




Parameters

WEIGHTS           : command keyword

freedom           : freedom name. (Alphanumeric)

rval              : weight associated with the specified freedom. (Real)

Notes

1.      See Appendix -F for list of valid freedom names.
2.      Freedom names omitted will have a weight of unity.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-52
ASAS (Non-Linear) User Manual                                                                           Structural Data



5.2     Structural Description Data

These data blocks define the physical properties and shape of the structure.

The following data blocks are defined

                         Coordinates ............. ................ ................ see Section 5.2.2

                         Element Topology ... ................ ................ see Section 5.2.3

                         Material Properties .. ................ ................ see Section 5.2.4

                         Geometric Properties ................ ................ see Section 5.2.5

                         Section Information .................. ................ see Section 5.2.6

                         Skew Systems.......... ................ ................ see Section 5.2.7




5.2.1       UNITS Command

If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally to each data block by the inclusion of a UNITS command. The local
units are only operational for the data block concerned and will return to the default global units when the next
data block is encountered.

In general, one or more UNITS commands may appear in a data block (but see notes below) thus permitting the
greatest flexibility in data input. The form of the command is similar to that used in the Preliminary data.

                 UNITS               unitm




Parameters

UNITS         : keyword

unitnm        : name of unit to be utilised (see below)

Notes


1.      Force, length, temperature and angular unit may be specified. Only those terms which are required to be
        modified need to be specified, undefined terms will default to those supplied on the global units definition
        unless previously overwritten in the current data block. In the case of the angular unit, the default
        depends on the data block concerned, see below.

2.      Valid unit names are as defined in Section 5.1.42.1.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-53
ASAS (Non-Linear) User Manual                                                                          Structural Data


3.     The mass unit is derived from the force and length unit currently defined. In order to determine the
       consistent mass unit the force and length terms must both be either metric or imperial. Valid
       combinations are shown in Table 3.1. This requirement is only necessary where mass or density data is
       being specified, in other cases inconsistencies are permitted. See Note 4 below and Section 3.11.

4.     Applications for each data type
        COOR                           -   Coordinate data - only one UNITS command is permitted for each co-
                                           ordinate system defined and must appear immediately after the header
                                           command. If different units are required, a new co-ordinate system must be
                                           defined. The default angular unit is DEGREES.
        ELEM                           -   Element data - UNITS not applicable.
        MATE                           -   Material data - UNITS command may appear anywhere. Force and length
                                           units must be within a consistent set.
        GEOM                           -   Geometric data - UNITS command may appear anywhere. Refer to data
                                           definitions for individual element type for the default angular unit assumed.
        SKEW and NSKW                  -   Skew systems - UNITS not applicable.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-54
ASAS (Non-Linear) User Manual                                                                               Structural Data


Example


   Data                                                         Operational Units                       Notes

   SYSTEM DATA AREA 5000000
   PROJECT ASAS
   JOB STAT                                                                                             TITLE                *
   EXAMPLESOLV 1.0
   OPTIONS GOON
   UNITS KIPS FEET                                              Kips, feet, centigrade                  Global definition
   END
   *
   COOR
   CART
   UNITS MM                                                     Kips, mm, centigrade,                   Default angular
   1       0.0        100.0          0.0                        degs                                    unit is degrees
   2   0.0            200.0          0.0                                                                for co-ordinates
   FIN
   CART FRED
   UNITS M                                                      Kips, m, centigrade,                    Requires M as unit
   101        0.1           0.1      0.0                        degs                                    Therefore define
   102        0.1           0.2      0.0                                                                new coor system
   END
   *
   ELEM                                                                                                 Units not used in
   *                                                                                                    elem topology
   MATP 1
   BEAM 1         2     1
   BEAM 101 102 1
   BEAM 2 102 2
   END
   MATE                                                         Kips, feet, centigrade                  Units revert to
   1     4.32E06          0.3      0.0      1.52E-02                                                    global input
   END                                                                                                  Mass unit is
   *                                                                                                    3.22 x 10 4 lbs
   GEOM                                                         Kips, feet, centigrade
   1 BEAM             0.3     0.18       0.18       0.03
   UNITS IN                                                     Kips, inch, centigrade
   2 BEAM 8.4                 24.7       29.8       1.13
   END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-55
ASAS (Non-Linear) User Manual                                                                                  Structural Data


5.2.2       COORDINATE Data

The coordinate data may comprise one or more local coordinate systems. Each of these systems must be headed
by a Coordinate System Header Line and all except the last terminated by a FIN keyword. The last system of
coordinate data is terminated by an END keyword.

                    COOR

                                CART               (name)

                                CYLI

                                SPHE               name                (units)

                    DCOS                           x'x            x`y            x'z            y'x      y'y          y'z

                    ORIG                           x-origin              y-origin            z-origin



                    node                           x               y              z


                    RP                             nrep                  inode            x-inc         y-inc         z-inc

                    RRP                            nrrep                 iinode           x-inc         y-inc         z-inc
                                                    x             SIN                 hleng1            SIN           hleng2
                    IMPE          ampl              y
                                                    z             COS                 harno1            COS           harno2
                    FIN

                    END




Parameters

COOR              : compulsory header keyword to denote the start of the coordinate data

CART              : keywords to denote the start of each local coordinate system
                     CYLI
                     SPHE

IMPE              : keyword to denote imperfection data

FIN               : keyword to denote the end of each local coordinate system, except the last

END               : compulsory keyword to denote the end of the entire coordinate data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-56
ASAS (Non-Linear) User Manual                                                                          Structural Data


Notes


1.       The coordinate values are in the current local coordinate system or in the global system if no local system
         has been defined.

2.       For cylindrical systems (CYLI) x,y,z are replaced by r, θ, z.

3.       For spherical systems (SPHE) x,y,z are replaced by r, θ, φ.

4.       For a detailed description of each parameter see Sections 5.2.2.1 to 5.2.2.4.


5.2.2.1 Local Coordinate System Header

To define the type of local coordinate system. Optional, if omitted CART is assumed.
                CART           (name)

                  CYLI                                    DEG

                  SPHE               name                  RAD




Parameters

CART          : cartesian system, global or local

CYLI          : cylindrical polar system

SHPE          : spherical polar system

name          : name of the coordinate system. Optional for CART and if blank, the global cartesian system is
                assumed. Compulsory for CYLI and SPHE. (4 character alphanumeric, 1st character must be
                alphabetic.)

DEG           : keyword used when the angular unit is degrees for θ and φ. If both DEG and RAD are omitted,
                degrees are assumed.

RAD           : keyword used when the angular unit is radians.

Note


For an axisymmetric model the global axis system is the unnamed cartesian system with x and z equivalent to r
and z.


5.2.2.2 Local Coordinate System Orientation

One DCOS command and one ORIG command must be included for each cylindrical or spherical system, and
for each named cartesian system. Neither is needed for the global cartesian system with the name omitted.
These lines define the origin and direction of the local axis system.

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-57
ASAS (Non-Linear) User Manual                                                                                Structural Data




           DCOS                  x’x              x’y          x’z           y’x            y’y         y’z

           ORIG                   x-origin                  y-origin                   z-origin




Parameters

DCOS              : keyword

x’x, x’y, x’z     : 6 directional cosines. See Section 5.2.7.1 for a full description. (Real)
                    y’x, y’y, y’z

ORIG              : keyword

x-origin          : 3 global coordinates of the origin of the local system. (Real)
y-origin
z-origin




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-58
ASAS (Non-Linear) User Manual                                                                           Structural Data




                                                                 Coordinates for Cartesian Systems

                                                                 x Distance from the local origin in the local x’ direction

                                                                 y Distance from the local origin in the local y’ direction

                                                                 z Distance from the local origin in the local z’ direction




Coordinates for Cylindrical Polar Systems

R Distance from the local origin in the local x’y’ plane.

θ Angle from the +ve side of the local x’ axis in the local                     x’y’
plane (+ve for right-hand screw rule applied to +ve                local z’).
z         Distance from the local origin in the local z’ direction.




                                                        Coordinates for Spherical Polar Systems

                                                        R Distance from the local origin in 3-D.

                                                        θ Angle from the +ve side of the local x’ axis in the local x’y’
                                                            plane (+ve for right-hand screw rule applied to +ve local z’).

                                                        φ Angle from the +ve side of the local z’ axis to the radius,
                                                            measured in 3-D.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-59
ASAS (Non-Linear) User Manual                                                                          Structural Data


5.2.2.3 Node Coordinates




Parameters

node          : node number. (Integer, 1-999999)

x, y, z       : 3 coordinates for the node in a cartesian system. (Real)

r, θ, z       : 3 coordinates for the node in a cylindrical polar system

r, θ, φ       : 3 coordinates for the node in a spherical polar system

RP            : keyword to indicate data generation from the previous / symbol

nrep          : the number of times the data is to be generated. (Integer)

inode         : node number increment to be added each time the data is generated. (Integer)

x-inc         : cartesian coordinate increments to be added each time the data is generated. (Real)
y-inc
z-inc

r-inc         : cylindrical coordinate increment to be added each time the data is generated. (Real)
θ-inc
z-inc

r-inc         : spherical coordinate increment to be added each time the data is generated. (Real)


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-60
ASAS (Non-Linear) User Manual                                                                          Structural Data


θ-inc
φ-inc

RRP           : keyword to indicate data generation from the previous // symbol.

nrrep         : the number of times the data is to be generated. (Integer)

iinode        : node number increment to be added each time the data is generated. (Integer)

Examples


Example of single coordinate data block using the global cartesian axis system.

   COOR
   CART
   1                   0.0         0.0        0.0
   2                  10.0         0.0        0.0
   /
   3                   0.0       10.0         0.0
   RP 4         1     10.0        0.0         0.0
   /
   7                    5.0      20.0         0.0
   RP 2         1       0.0       0.0         4.0
   END

Example of a coordinate data block which uses several local axis systems beginning with the global cartesian
axis system.

   COOR
   ****     THE GLOBAL CARTESIAN SYSTEM, 8 NODES DEFINED
   CART
   //
   /
   66                      20.1          0.0        -1.0
   RP       3,1             0.0          4.0         0.0
   RRP      2,4           -10.0          0.0         0.0
   69                      20.0          0.0        -1.0
   73                      11.0          0.0         0.0
   FIN
   ****     A CYLINDRICAL SYSTEM, NAMED BWL2, 20 NODES DEFINED
   CYLI       BWL2   DEG
   DCOS        1.0    0.0   0.0   0.0   1.0   0.0
   ORIG        0.0    0.0   0.0
   /
   1                      5.0         0.0         0.0
   9                      5.0        22.5         0.0
   7                      6.0         0.0         0.0
   12                     6.0        22.5         0.0
   11                     6.0        22.5         8.0
   RP       4,12          0.0        45.0         0.0
   FIN
   ****     2ND CYLINDRICAL SYSTEM, NAMED HNDL, 7 NODES DEFINED
   CYLI       HNDL   DEG
   DCOS        1.0   0.0   0.0   0.0   -1.0   0.0
   ORIG       26.0   0.0   0.0
   /

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-61
ASAS (Non-Linear) User Manual                                                                          Structural Data


     85                   10.0          0.0         -1.0
     RP     3,1            0.0         30.0          0.0
     /
     92                   10.0          0.0         -5.0
     RP     2,-4           0.0         60.0          0.0
     /
     93                     9.5         0.0         -0.5
     RP     2,1             0.0        60.0          0.0
     END


5.2.2.4 Coordinate Imperfection Data

Defines variations from the nodal coordinate values in the current local coordinate system.

Notes


1.      Up to 10 IMPE lines are allowed in each local coordinate system.

2.      All variation data is calculated for a node from the original local system coordinates and is then applied to
        these coordinate values before any conversion to the global cartesian system.

3.      To input a variation depending on one direction only, use the COS parameter and hleng or harno value
        of zero for the term corresponding to the direction of constant variation.



Cartesian Systems




Parameters

IMPE          : keyword to denote imperfection data

ampl          : amplitude of imperfection

X,Y,Z         : keywords to denote which coordinate direction is effected

SIN, COS        :        keywords to denote a sine or cosine variation

hlengx        : half-wavelength value for variation in corresponding coordinate direction
hlengy
hlengz

Variation data will be generated of the form:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-62
ASAS (Non-Linear) User Manual                                                                                Structural Data




Cylindrical Systems
                                                                SIN                                     SIN
                  IMPE                  ampl                                      harno                           hleng
                                                                COS                                     COS




Parameters

IMPE          : keyword to denote imperfection data

ampl          : amplitude of imperfection

SIN,COS : keywords to denote a sine or cosine variation

harno         : harmonic number of angular variation

hleng         : half wavelength value for variation in location z direction


Radial variation data will be generated of the form:




Spherical Systems
                                                               SIN                                      SIN
                 IMPE                  ampl                                       harno1                          harno2
                                                               COS                                      COS




Parameters


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-63
ASAS (Non-Linear) User Manual                                                                          Structural Data


IMPE          : keyword to denote imperfection data

ampl          : amplitude of imperfection

SIN,COS : keywords to describe a sine or cosine variation

harno1        : harmonic number of angular variation in θ direction

harno2        : harmonic number of angular variation in φ direction


Radial variation data will be generated of the form:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-64
ASAS (Non-Linear) User Manual                                                                          Structural Data




Example


Example of a coordinate data block which uses several local axis systems and imperfection data.

        COOR
        ****     THE GLOBAL CARTESIAN SYSTEM, 8 NODES DEFINED
        CART
        //
        /
        66                  20.1             0.0        -1.0
        RP       3,1         0.0             4.0         0.0
        RRP      2,4       -10.0             0.0         0.0
        69                  20.0             0.0        -1.0
        73                  11.0             0.0         0.0
        IMPE           0.01 X COS            4.0       COS 0.0
        FIN
        ****     A CYLINDRICAL SYSTEM, NAMED BWL2, 20 NODES DEFINED
        CYLI       BWL2   DEG
        DCOS        1.0    0.0   0.0   0.0   1.0   0.0
        ORIG        0.0    0.0   0.0
        /
        1               5.0               0.0          0.0
        9               5.0              22.5          0.0
        7               6.0               0.0          0.0
        12              6.0              22.5          0.0
        11              6.0              22.5          8.0
        RP       4,12   0.0              45.0          0.0
        IMPE        0.01 COS             4 COS         4.0
        FIN
        ****     2ND CYLINDRICAL SYSTEM, NAMED HNDL, 7 NODES DEFINED
        CYLI       HNDL   DEG
        DCOS        1.0   0.0   0.0   0.0   -1.0   0.0
        ORIG       26.0   0.0   0.0
        /
        85                    10.0          0.0          -1.0
        RP       3,1           0.0         30.0           0.0
        /
        92                    10.0          0.0          -5.0
        RP       2,-4          0.0         60.0           0.0
        /
        93                      9.5    0.0  -0.5
        RP       2,1            0.0   60.0    0.0
        IMPE       0.01         COS 6 COS 0.0
        END



5.2.3       Element Topology Data

To define each element which makes up the structure.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-65
ASAS (Non-Linear) User Manual                                                                              Structural Data



                    ELEM

                    MATP                 material


                    eltype               (mtype)                   //nodes//               geom         (elno)


                    RP                   nrep                       inode

                    RRP                  nrrep                      iinode

                    END




Parameters

ELEM              : compulsory header keyword to denote the start of the element data.

MATP              : keyword to define the material to be assigned to all following elements until another MATP
                     line is used.

material          : material property integer. The material properties are defined in Section 5.2.4. (Integer,1-9999)

eltype            : element type. (Alphanumeric, 4 characters.) See Appendix -A for a full list of elements
                     available.

mtype             : type of mass matrix for this element (natural frequency analysis). For defaults, see Appendix -
                     A.
                     Permitted Values:                  C - consistent mass
                                                        L - lumped mass
                                                        N - no mass

nodes             : list of node numbers to define the element. (Integer, 1-99999)

geom              : geometric property integer. (Integer, 1-9999.) Not required for certain element types, see
                     Appendix -A.

elno              : user number for the element. Every user element number, whether user defined or program
                     generated, must be unique. Generated elements are numbered successively in increments of 1.
                     If omitted the element numbers are assigned by the program, numbered according to the input
                     order of the elements, see Section 4.3.2. (Integer, 1-99999)

RP                : keyword to indicate the generation of data from the previous / symbol.

nrep              : the number of times the data is to be generated. (Integer)

inode             : node number increment. (Integer)

RRP               : keyword to indicate the generation of data from the previous // symbol.


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-66
ASAS (Non-Linear) User Manual                                                                          Structural Data


nrrep             : the number of times the data is to be generated. (Integer)

iinode            : node number increment. (Integer)

END               : compulsory key word to denote the end of the element topology data.

Notes


1.      Continuation lines may be used if needed to define nodes, geom and elno.

2.      Where mid-side nodes are at the midpoint and their coordinates have not been defined in the COOR data,
        the node number must be included in the nodes list.

Examples


An example of a simple element topology data block.

        ELEM
        MATP         1
        FLA2         8     9          1
        FLA2         9    10          2
        FLA2         8    10          1
        FLA2       10     11          1
        END

An example of element topology data using data generation.

        ELEM
        MATP         1
        /
        FLA2         1    21      3
        FLA2         1    41      2
        FLA2       41     21      2
        RP       10,1
        END

An example of the use of element numbers and continuation lines.

        BR15         1      2         3    4       5      6
        :          21     23      25
        :          41     42      43      44     45      46     130




5.2.4       Material Property Data

This data block defines the material models which will be used in the analysis. For each material required the
user should associate an integer number (the ‘material property integer’) which applies to all the properties of a
material and is used to cross-reference the material from other data blocks such as element topology. The types
of behaviour which may be associated with each material are:



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-67
ASAS (Non-Linear) User Manual                                                                          Structural Data


   •        Elastic, either isotropic, orthotropic, woven, anisotropic, hyperelastic or laminated (for shells)
            (see Section 5.2.4.1).

   •        Plastic, or more generally, time independent irreversible behaviour according to various
            theories (see Section 5.2.4.2).

   •        Creep or time dependent material behaviour (see Section 5.2.4.3).

   •        Failure properties associated with limiting values for stresses and/or strains for laminated
            composites (seeSection 5.2.4.4).

   •        User defined material (see Section 5.2.4.1).

   •        Material properties for general field analysis problems, eg electric conduction. (see Section
            5.2.4.1)

   •        Piezo-resistive material properties (see Section 5.2.4.1)

   •        Convection and radiation models for heat analysis. (see Section 5.2.4.1)

A material may be defined by a combination of the above properties with the same integer identifier.

In general, all properties may be a function of temperature. This is specified by repeating material data at a
number of temperatures. The program interpolates linearly between these temperatures. The same temperatures
should be used for all material data types.

The material integer is unique to the problem and the same number cannot be used to reference different
materials in different groups.

Elasticity data must precede any plasticity data, which in turn must precede any creep data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-68
ASAS (Non-Linear) User Manual                                                                          Structural Data




Parameters

MATE              : compulsory header keyword to denote the start of the material properties data

mat               : material property integer used to label different materials. (Integer, 1-9999)

ISO               : keyword to define an isotropic material

ORTH              : keyword to define an orthotropic material

WOVE              : keyword to define a woven material

AISO              : keyword to define an anisotropic material

AISI              : keyword to define an anisotropic material by specifying the inverse of the stress-strain relations
                     i.e. strain-stress relations

HYPE              : keyword to define a hyperelastic material. (Continuum elements only)

LAMI              : keyword to define a laminated material. (Shell and laminated brick elements only)

UMAT              : keyword to define a user supplied material


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-69
ASAS (Non-Linear) User Manual                                                                               Structural Data


FIEL               : keyword to define general field properties

PIER               : keyword to define piezo-resistive material properties

CVEC               : keyword to define heat convection properties

RADI               : keyword to define heat radiation properties

PLAS               : keyword to define plastic material properties

CREP               : keyword to define creep material properties

FAIL               : keyword to define failure data for orthotropic and laminated materials only

END                : compulsory keyword to denote the end of the material properties data block


Notes


1.      For full details for each type of material see Sections 5.2.4.1, 5.2.4.2, 5.2.4.3, 5.2.4.4 and Appendix -B.

2.      Every material referenced in the element topology data must be fully defined in this data block.

3.      PLAS not available with AISO, AISI, ORTH, WOVE or HYPE materials.

4.      FAIL only available with ISO, AISO, ORTH, WOVE and LAMI materials.


5.2.4.1 Elastic Material Properties

To define the properties for isotropic and anisotropic elastic material.


5.2.4.1.1         Isotropic material properties

           mat          ISO          elas        pois       (expan)         (dens)       (dampm)        (dampk) (temp)
                                          kn

              :        (ISO)        elas        pois         expan          dens          dampm         dampk   temp




Parameters

mat                : material property integer. (Integer, 1-9999)

ISO                : keyword to define the material as isotropic

elas               : modulus of elasticity. (Real)

poisson            : Poisson’s ratio. (Real, 0.0 <poisson< 0.5)

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-70
ASAS (Non-Linear) User Manual                                                                          Structural Data


expan             : linear coefficient of thermal expansion. (Real)

dens              : density, mass per unit volume. (Real)

dampm             : damping factor for mass. (Real)

dampk             : damping factor for elastic stiffness. (Real)

temp              : temperature at which these properties apply. (Real)

kn                : effective contact stiffness for gap elements and normal contact stiffness parameter for rigid
                     surface elements. (Real)

Notes


1.      The expansion coefficient is optional and is only required if temperatures are to be included in any of the
        loading applied to the structure.

2.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency or transient dynamics analysis is to be
        performed.

3.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

4.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure.

5.      If an optional value is specified, all preceding optional values must also be specified.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-71
ASAS (Non-Linear) User Manual                                                                               Structural Data


Examples


A simple example with one material and no temperature or inertia type loading.

       MATE
       1       ISO        21.0E4           0.3
       END

An example with several materials including the expansion coefficient and the density.

        MATE
        10       ISO        0.298E8            0.3        0.1182E-4              0.283
        20       ISO        0.312E8            0.31       0.1212E-4              0.298
        30       ISO        0.151E8            0.3        0.1566E-4              0.206
        END

An example with one material which is temperature dependent but with no inertia type loading

        MATE
        1        ISO        7.200E10             0.3        16.32E-6             0.0      0.0       0.0     0.0
        :                   7.200E10             0.3        16.32E-6             0.0      0.0       0.0    70.0
        :                   7.098E10             0.3        18.26E-6             0.0      0.0       0.0   100.0
        :                   7.047E10             0.3        18.16E-6             0.0      0.0       0.0   200.0
        :                   6.895E10             0.3        18.92E-6             0.0      0.0       0.0   300.0
        :                   6.767E10             0.3        19.60E-6             0.0      0.0       0.0   400.0
        :                   6.640E10             0.3        20.20E-6             0.0      0.0       0.0   500.0
        :                   6.462E10             0.3        20.76E-6             0.0      0.0       0.0   600.0
        END


5.2.4.1.2       Orthotropic material properties




Parameters

mat               : material property integer. (Integer, 1-9999)

skew              : optional skew system identifier, see Section 5.2.7. (Integer)

ORTH              : keyword to define the material as orthotropic

density           : density, mass per unit volume. (Real)


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-72
ASAS (Non-Linear) User Manual                                                                             Structural Data


dampm             : damping factor for mass. (Real)

dampk             : damping factor for elastic stiffness. (Real)

temp              : temperature at which these properties apply. (Real)

E11-E33           : Young’s moduli in local 1, 2 and 3 directions respectively. (Real)
                     (The program will set E33=E22 if E33 is specified as zero.)

G12-G31           : shear moduli in local 12, 23 and 31 planes respectively. (Real)

ν12-ν13           : Poisson’s ratios in local 12, 23 and 13 planes respectively. (Real)
                     (The program will set ν23= ν12 and/or               ν13= ν12 if any of these is specified as zero.)

α11-α33           : coefficients of thermal expansion in the local 1, 2 and 3 directions respectively. (Real)

fl                : loss factor, i.e. volume fraction of material with no stiffness. If not specified, fl = 0.0. (Real)

Notes


1.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
        performed.

2.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

3.      The orthotropic properties must start on the first continuation line and may then spread onto further
        continuation lines as required.

4.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure.

5.      If an optional value is specified, all preceding optional values must also be specified.

6.      Up to 13 properties are expected but if less than 13 are specified, then the remaining properties default to
        zero.

7.      The Poisson’s ratios ν21, ν32 and ν31 are determined inside the program from
                                E 22                             E33                              E33
                 ν 21 = ν12                      ν32 = ν 23                        ν31 = ν13
                                E 11                             E 22                             E 11


Examples


An example of an orthotropic material for a QUM8 element.

        MATE
        1      ORTH
        :      7.8E6        2.6E6        0.0


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-73
ASAS (Non-Linear) User Manual                                                                                 Structural Data


       :       1.3E6        0.0           0.0
       :       0.25         0.0           0.0
       END

An example of an orthotropic material with temperature dependency for a QUX8 element.

       MATE
       1    ORTH          0.0       0.0      0.0       20.0
       :       4.3E6        2.1E6         3.4E5        8.8E5        0.0      0.0       0.25       0.13   0.0
       :       0.13E-5 0.23E-5 -0.12E-6
       1       ORTH 0.0 0.0 0.0 80.0
       :       4.3E6 1.8E6 3.2E5 4.4E5                              0.0      0.0       0.21       0.17   0.0
       :       0.17E-5 0.25E-5 -0.12E-6
       END


5.2.4.1.3       Woven material properties




Parameters

mat               : material property integer. (Integer, 1-9999)

skew              : optional skew system identifier, see Section 5.2.7. (Integer)

WOVE              : keyword to define the material as woven

density           : density, mass per unit volume. (Real)

dampm             : damping factor for mass. (Real)

dampk             : damping factor for elastic stiffness. (Real)

temp              : temperature at which these properties apply. (Real)

E11-E33           : Young’s moduli in local 1, 2 and 3 directions respectively of the orthotropic sub-lamina. (Real)
                     (The program will set E33=E22 if E33 is specified as zero.)

G12-G31           : shear moduli in local 12, 23 and 31 planes respectively of the orthotropic sub-lamina. (Real)

ν12-ν13           : Poisson’s ratios in local 12, 23 and 13 planes respectively of the orthotropic sub-lamina. (Real)
                     (The program will set ν23= ν12 and/or               ν13= ν12 if any of these is specified as zero.)


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-74
ASAS (Non-Linear) User Manual                                                                           Structural Data


α11-α33           : coefficients of thermal expansion in the local 1, 2 and 3 directions respectively. (Real)

fl                : loss factor, i.e. volume fraction of material with no stiffness. If not specified, fl = 0.0. (Real)

Notes


1.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
        performed.

2.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

3.      The woven properties must start on the first continuation line and may then spread onto further
        continuation lines as required.

4.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure.

5.      If an optional value is specified, all preceding optional values must also be specified.

6.      Up to 13 properties are expected but if less than 13 are specified, then the remaining properties default to
        zero.

7.      The Poisson’s ratios ν21, ν32 and ν31 are determined inside the program from
                                E 22                             E33                              E33
                 ν 21 = ν12                      ν32 = ν 23                        ν31 = ν13
                                E 11                             E 22                             E 11


Examples


An example of an orthotropic material for a TCS8 element with loss factor 0.2.

        MATE
        1      WOVE
        :      150E9            10E9             0.0
        :      5.7E9            3.4E9            5.7E9
        :      0.25             0.0              0.0
        :   0.17E-5             0.25E-5          0.0        0.2
        END


5.2.4.1.4       Anisotropic material properties

There are two options available to anisotropic behaviour. The first specifies the matrix C in relation σ=Cε (in
which σ is stress and ε strain). The second specifies the inverse of C to give strains as a function of stress.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-75
ASAS (Non-Linear) User Manual                                                                              Structural Data




                                         AISO
         mat         (skew )                                 (density)          (dampm)           (dampk)     (temp)
                                         AISI

           :           properties



Parameters

mat               : material property integer. (Integer, 1-9999)

skew              : optional skew system identifier, see Section 5.2.7. (Integer)

AISO              : keyword to define the material as anisotropic with properties defining the stress-strain relations

AISI              : keyword to define the material as anisotropic with properties defining the strain-stress relations

density           : density, mass per unit volume. (Real)

dampm             : damping factor for mass. (Real)

dampk             : damping factor for mass. (Real)

temp              : temperature at which these properties apply

properties        : coefficients of the anisotropic stress-strain matrix (AISO) or the strain-stress matrix (AISI) and
                     linear coefficients of expansion. See Appendix -A for a full definition of which terms are
                     required for each type of element. (Real)

Notes


1.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
        performed.

2.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

3.      The anisotropic properties must start on the first continuation line and may then spread onto further
        continuation lines as required.

4.      A total of 30 properties is always needed, composed of up to 24 material constants and 6 coefficients of
        thermal expansion. The coefficients of thermal expansion must start at position 25.

5.      If an optional value is specified, all preceding optional values must also be specified.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-76
ASAS (Non-Linear) User Manual                                                                                 Structural Data


Examples


An example of an anisotropic material for a BR20 element.

           MATE
           1    AISI
           :    0.536044 -0.16081 0.536044 -0.16081 -016081                                         0.536044
           :    0.0       0.0     0.0       0.139372 0.0                                            0.0
           :    0.0       0.0     0.139372 0.0       0.0                                            0.0
           :    0.0       0.0     0.139372 0.00172 0.00172                                          0.00172
           :    0.0       0.0     0.0       0.0      0.0                                            0.0
           END

An example of an anisotropic material for a QUM8 element

           MATE
           1    AISO
           :    23600.0 5720.0 20575.0   0.0     0.0 16750.0
           :         0.0   0.0     0.0 12650.0   0.0     0.0
           :         0.0   0.0     0.0   0.0     0.0     0.0
           :         0.0   0.0     0.0 0.16E-4 0.14E-4   0.01E-4
           :         0.0   0.0     0.0   0.0     0.0     0.0
           END


5.2.4.1.5       Hyper-elastic material properties

   mat        HYPE          bulk       con1       con2        (expan)         (dens)        (dampm)     (dampk)     (temp)


       :     (HYPE)         bulk       con1       con2         expan           dens          dampm       dampk      temp




Parameters

mat               : material property integer. (Integer, 1-9999)

HYPE              : keyword to define the material as hyper-elastic

bulk              : bulk modulus. (Real)

con1              : Mooney-Rivlin constant, C10. (Real)

con2              : Mooney-Rivlin constant, C01. (Real)

expan             : linear coefficient of thermal expansion. (Real)

dens              : density, mass per unit volume. (Real)

dampm             : damping factor for mass. (Real)



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-77
ASAS (Non-Linear) User Manual                                                                                Structural Data


dampk             : damping factor for stiffness. (Real)

temp              : temperature at which these properties apply. (Real)

Notes


1.      The damping factor for stiffness is currently restricted to be zero.

2.      The expansion coefficient is optional and is only required if temperatures are to be included in any of the
        loading applied to the structure.

3.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency analysis is to be performed.

4.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

5.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure.

6.      If an optional value is specified, all preceding optional values must also be specified.

Example


A simple example with one material and no temperature or inertia type loading.

        MATE
        1    HYPE           1.0E4          80.0          20.0
        END


5.2.4.1.6       Laminated Material Properties


     mat          (skew)              LAMI             (density)             (dampm)                (dampk)      (temp)




Parameters

mat           : material property integer. (Integer, 1-9999)

skew          : optional skew system identifier, see Section 5.2.7. (Integer)

LAMI          : keyword to define the material as a laminated shell

density       : density, mass per unit volume. (Real)

dampm         : damping factor for mass. (Real)

dampk         : damping factor for stiffness. (Real)

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-78
ASAS (Non-Linear) User Manual                                                                          Structural Data


temp          : temperature at which these properties apply. (Real)

Notes


1.      The skew system identifier is optional and is only required if the laminate material reference axis system
        does not coincide with the global axis system.

2.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
        performed. If the density is specified both here and with the materials forming the laminate, the density
        specified here will be used. If the density is omitted (or given a value of 0.0) the density for the laminate
        will be calculated from the laminae densities in the manner described in Appendix -B.

3.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis. If damping factors are specified both here and with the materials forming the laminate, the
        factors specified here will be used. If the damping factors are omitted (or given a value of 0.0) the
        damping factors for the laminate will be calculated from the laminae damping factors in the manner
        described in Appendix -B.

4.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure. If the properties specified here are temperature dependent
        then the materials forming the laminate must be specified with the same range of temperatures.

5.      If an optional value is specified, all preceding optional values must be specified.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-79
ASAS (Non-Linear) User Manual                                                                                   Structural Data


Example


A simple example of a laminated material where the material axes coincide with the global axis system (no skew
required), where the density is to be calculated from the laminae densities but where the damping factors for the
laminate are specified.

        MATE
        1 LAMI 0.0 0.039 0.0102
        END


5.2.4.1.7       User Material Properties

        mat          UMAT           (density)            (dampm)                 (dampk)                (temp)


        :           up to 24 user material properties                                    up to 6 thermal coefficients




Parameters

mat           : material property integer. (Integer, 1-9999)

UMAT          : keyword

density       : density, mass per unit volume. (Real)

dampm         : damping factor for mass. (Real)

dampk         : damping factor for stiffness. (Real)

temp          : temperature at which these properties apply. (Real)

Notes


1.      If thermal coefficients are supplied they must start at the 25th position as for AISO material properties.

2.      See Appendix B.6 for details concerning the user material interface.

3.      The density is optional and is only required if acceleration or centrifugal loads are to be included in any
        loading applied to the structure, or if a natural frequency analysis is to be performed.

4.      The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
        analysis.

5.      The temperature is optional and is only required if the material properties vary with temperature and
        temperature loading is applied to the structure.

6.      If an optional value is specified, all preceding optional values must also be specified.


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-80
ASAS (Non-Linear) User Manual                                                                                   Structural Data


5.2.4.1.8             Field Material Properties

            mat           (skew )     FIEL      kxx       (kyy)        (kzz )     (kxy)     (k yz)      (kzx)    (dens)    (temp)


              :                      (FIEL)     kxx        kyy         kzz        kxy       kyz         kzx       dens     temp




Parameters

mat               : material property integer. (Integer, 1-9999)

skew              : skew system integer

FIEL              : keyword to define the material as field

kxx,kyy,kyy           : conductivities in xx direction, yy direction, etc. (Real)
kxy,kyz,kzx

dens              : generalised density. (Real)

temp              : temperature at which these properties apply. (Real)

Notes


1.        If only kxx is specified, it is assumed that the material is isotropic
          (ie kxx = kyy = kzz and kxy = kyz = kzx = 0)

2.        If an optional value is specified, all preceding optional values must also be specified.

3.        For heat analysis, the generalised density is defined as the product of the specific heat capacity and the
          density.


5.2.4.1.9             Piezo-resistivity Material Properties

        mat                (skew)         PIER            (dum)                 (dum)             (dum)          (temp)


      :           q           n         µn            p           µp              π11             π12           π44




Parameters

mat               : material property integer. (Integer, 1-9999)



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-81
ASAS (Non-Linear) User Manual                                                                          Structural Data


skew            : skew system integer. (Integer, 1-9999)

PIER            : keyword to define material as piezo-resistivity

dum             : dummy

temp            : temperature at which these properties apply. (Real)

q               : unit charge

n               : carrier concentration (n)

µn              : carrier mobility (n)

p               : carrier concentration (p)

µp              : carrier mobility (p)

π11             : Piezo-resistance coefficient, 11

π12             : Piezo-resistance coefficient, 12

π44             : Piezo-resistance coefficient, 44

Notes


1.      A total of 8 properties are always needed.

2.      If an optional value is specified, all preceding optional values must also be specified.

3.      The piezo-resistivity properties must start on the first continuation line and may then spread onto further
        continuation lines as required.


5.2.4.1.10 Convective Heat Material Properties


          mat         CVEC          h          r         (temp)


            :        (CVEC)          h          r          temp




Parameters

mat                : material property integer. (integer, 1 - 9999)

CVEC               : keyword to define the material as convective heat

h                  : film coefficient in the heat transfer equation. (Real)



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-82
ASAS (Non-Linear) User Manual                                                                          Structural Data


r                 : power index in the heat transfer equation. (Real)

temp              : temperature at which the properties apply. (Real)

Notes


1.      This material type is used to model convective heat transfer of the form:

        q=h.(T1-T2)r

2.      CVEC material can only be used with FAT2 element in a heat analysis


5.2.4.1.11 Radiant Heat Material Properties




Parameters

mat               : material property integer. (integer, 1 - 9999)

RADI              : keyword to define the material as radiant heat

σ                 : Stefan-Boltzmann constant (Real)

ε                 : effective surface emissivity. (Real)

temp              : temperature at which the properties apply. (Real)

Notes


1.      This material type is used to model radiant heat transfer of the form:

        q=σ.ε.(Τ14-Τ24)

2.      The temperatures required in the radiation equation are relative to absolute zero temperature. The default
        temperature units assumed by ASAS(NL) are degrees Centigrade. If other temperature units are used for
        an analysis, the correct absolute zero temperature in the appropriate units must be specified using the
        PARA TAZERO command.

3.      RADI material can only be used with FAT2 element in a heat analysis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-83
ASAS (Non-Linear) User Manual                                                                          Structural Data


5.2.4.2 Plastic Material Properties

To define the properties for a plastic material. Plastic material properties must be preceded by the elastic
isotropic material properties for any individual material integer.

A number of different plasticity models are available which are activated by 4-character directives defined on the
first line together with other basic data. Depending on the directives, so additional types of commands may also
be necessary. The directives fall into three categories:

(1)         Yield Criteria

            MISE         -    Mises yield criterion to be used
            TRES         -    Tresca yield criterion to be used
            MOHR         -    Mohr-Coulomb yield criterion to be used
            DRUC         -    Drucker-Prager yield criterion to be used
            TCUT         -    Tension cutcriterion to be used
            COUL         -    Coulomb friction yield criterion to be used (rigid surface elements only)
            IVAN         -    Ivanov (gross section) yield criterion to be used (shell elements only)
            BEM2         -    Beam stress resultant (gross section) yield criterion to be used (BM2D element only)
            BEM3         -    Beam stress resultant (gross section) yield criterion to be used
                              (BEAM/BM3D/TUBE elements only)
            BEAM         -    Generalised beam stress resultant (gross section) yield criterion to be used
                              (BEAM/BM3D/TUBE elements only)
            SPRG         -    Inelastic model for spring elements

            If no directive is given, then MISE’s criterion is assumed.


(2)         Post-Yield Behaviour

            TABL         -    Tabular definition of uniaxial post-yield behaviour to be used.

            If this directive is not given bi-linear behaviour is assumed.


(3)         Hardening Rule

            PPRA         -    Prager type of kinematic hardening (see Note 2)
            PZIG         -    Ziegler type of kinematic hardening

            If no directive is given isotropic hardening is assumed.

Notes


1.      Associative flow rules are used in all cases.

2.      Prager type kinematic hardening is inapplicable to elements using a reduced stress space - i.e. plane stress
        membranes, beams and shells.

3.      Temperature loads cannot be used in conjunction with IVANOV yield criterion.


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-84
ASAS (Non-Linear) User Manual                                                                                    Structural Data


4.     Kinematic hardening is only available for MISE and TRES criteria
                                         (MISE)

               (mat)            PLAS                                         sigy           (ep)          (temp)
                                                    TRES
                                                                          PPRA

                                                   TCUT                                  sigy           ep      hard     (temp)
                                                                            PZIG
               :                sigy             ep            (hard)                temp

                                                      MOHR
               (mat)            PLAS                                        c            phi            (temp)
                                                      DRUC
               (mat)            PLAS                   COUL                 kt           mu              shrlmt

               (mat)            PLAS                   IVAN                 sigy


               (mat)            PLAS                   BEM2                 Po           Mpz            (temp)

                                                       BEM3                 Po           M pz           M py       (temp)

               (mat)            PLAS                   BEAM                 Po           Mpz            Mpy        (temp)


               :                C1                (C2)            (C3)            (C4)             (C5)           (C6)

                                                    (MISE)
               (mat)            PLAS                                      TABL                   sigy              (temp)
                                                      TRES
                                                                                         PPRA
                                                     TCUT                                                sigy      hard       (temp)
                                                                                         PZIG


                   :               properties




                (mat)           PLAS                   SPRG                 K1           K2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-85
ASAS (Non-Linear) User Manual                                                                          Structural Data


Parameters

mat               : property integer. (Integer, 1-9999)

PLAS              : keyword to define the material as plastic

MISE              : yield criterion keyword

TRES              : yield criterion keyword

TCUT              : yield criterion keyword

sigy              : uni-axial yield stress. (Real)

ep                : slope of post yield stress/strain relation. (Real)

temp              : temperature at which these properties apply. (Real)

PPRA              : kinematic hardening keyword

PZIG              : kinematic hardening keyword

hard              : for keywords PPRA and PZIG, the ratio of isotropic to kinematic hardening. 1.0 for isotropic
                     hardening, 0.0 for pure kinematic hardening. (Real)

MOHR              : yield criterion keyword

DRUC              : yield criterion keyword

c                 : cohesion

phi               : angle of friction

COUL              : yield criterion keyword

kt                : tangential contact stiffness parameter (unit: stress per unit length). (Real)

mu                : coefficient of friction. (Real)

shrlmt            : limiting shear stress. (Real)

IVAN              : yield criterion keyword

BEM2              : yield criterion keyword

Po                : yield force. (Real)

Mpz               : yield moment about beam local z axis. (Real)

BEM3              : yield criterion keyword

Mpy               : yield moment about beam local y axis. (Real)

BEAM              : yield criterion keyword



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-86
ASAS (Non-Linear) User Manual                                                                          Structural Data


C1 - C6           : yield function constants in the equation:
                    C1(P/Po)C2 + C3(Mz/Mpz)C4 + C5(My/Mpy)C6 = 1 (Real)

SPRG              : inelastic spring model keyword

K1                : unloading stiffness factor (Real)
                     (set to 1.0 if zero specified)

K2                : kinematic hardening factor (Real)

TABL              : keyword required if a tabular definition of the uni-axial post yield behaviour is to be specified

properties        : if TABL is specified, properties will consist of pairs of stress/strain values defining the
                     uniaxial post yield behaviour. The strains required are total strains. (Real)

Notes


1.      All elastic material property data must appear before the plastic material property data for any individual
        material integer.

2.      For details of the various models, see Appendix B.3.

3.      The slope of the post yield stress/strain curve must be less than the elastic modulus. Apart from tension
        cutmaterial, the slope must be non negative (i.e. ≥0.0). For tension cutmaterial, the slope must not be less
        than -E/ν

4.      If the material properties vary with temperature, each set of data should be repeated for a different
        temperature.

5.      The following notes apply to tabulated definition only:
(a)     The stress-strain table may be continued on as many lines as necessary.

(b)     For linear elastic/plastic material the first point in the table (σ,ε) will correspond to a point after yield.
        The coordinates of the yield point are computed from the elastic modulus and yield stress.

(c)     The program interpolates linearly for intermediate points.

(d)     There are a maximum of 40 different strain values allowed.

(e)     A slope defined in the table should not be equal to the elastic modulus. Apart from tension cutmaterial
        the slope must be non negative (i.e. ≥ 0.0) For tension cutmaterial, the slope must not be less than -E/ν.

(f)     If curves are specified for different temperatures (see third example) then the order the plasticity data is
        presented should correspond to the order in which the elastic data is presented.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-87
ASAS (Non-Linear) User Manual                                                                          Structural Data


Examples


Simple elastic-perfectly plastic model with isotropic hardening.

       MATE
       1       ISO        21000.0            0.3
       PLAS        MISE         250.0
       END

Simple elastic-plastic model with isotropic hardening.

        MATE
        1   ISO   21000.0                    0.3
        PLAS MISE    250.0                    30.0
        END

Metal satisfying MISE’s yield criterion and associated flow rule with isotropic hardening. Uniaxial behaviour is
as in figure below.




        MATE
        10       ISO        21900.0             0.3        0.276E-6            0.0        T1
       20900.0            0.3         0.276E-6             0.0        T2
       20500.0            0.3         0.276E-6             0.0        T3
       PLAS         MISE   TABL     σy1   T1
       :           σ11   ε11    σ12     ε12                        σ13         ε13
       :           σ14   ε14    σ15     ε15
       PLAS         MISE   TABL     σy2     T2
       :           σ21         ε21        σ22         22          σ23         ε23
       PLAS         MISE          TABL     σy3   T3
       :           σ31           ε31   σ32     ε32                 σ33         ε33
       END

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-88
ASAS (Non-Linear) User Manual                                                                            Structural Data


5.2.4.3 Creep Material Properties

To define the properties for a material with creep. Creep material properties must be preceded by elastic
isotropic material properties and plastic material properties if present.

This data defines the creep law to be used for each material type. The user may choose from 4 in-built laws.
Alternatively up to 5 user supplied laws (in subroutine form) can be used. Appendix B.4 gives full details. In-
built laws require creep constants which are given in the data. Creep constants for use with the user supplied
laws may be defined if required.
                                                                                       NORT
                                                                                       LAW2
                                                                                       LAW3
                                                                                       LAW4
               (mat)                   CREP                                            USE1             (temp)
                                                                                       USE2
                                                                                       USE3
                                                                                       USE4
                   :                 constants
                                                                                       USE5




Parameters

mat           : material property integer. (Integer, 1-9999)

CREP          : keyword to define the material properties for creep
NORT
LAW2          : keyword to define ASAS-NL creep law
LAW3
LAW4

USE1
USE2          : keyword to define user supplied creep law
USE3
USE4

temp          : temperature at which these properties apply. (Real)

constants : creep law constants. (Real)

Note


Refer to creep law expressions in Appendix B.4 for definition of creep constants.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-89
ASAS (Non-Linear) User Manual                                                                              Structural Data


Examples


Norton (power) law for a Cr-Mo-V ferritic stainless steel. No temperature or time dependence.
Units: N, mm.
                 ε c = 2.05 x 10-28 σ 10.42
                 

MATE
1     ISO     1.41E5         0.3
CREP NORT
: 2.05E-28             10.42        0.0
END

Norton (power) law with temperature dependence but no time dependence. Units: N, mm, °C.

                 ε c = 2.05 x 10-28 σ 10.42
                                                                  T=525°C


                 ε c = 6.72 x 10-28 σ 10.42
                                                                  T=550°C


                 ε c = 2.05 x 10-27 σ 10.42
                                                                  T=575°C


MATE
1 ISO         1.41E5         0.3      16.0E-6          7.93E-9          0.0       0.0      525.0
:             1.36E5         0.3      16.0E-6          7.93E-9          0.0       0.0      550.0
:             1.31E5         0.3      16.0E-6          7.93E-9          0.0       0.0      575.0
CREP          NORT 525.0
:             2.05E-28 10.42                  0.0
CREP          NORT       550.0
:             6.72E-28 10.42                  0.0
CREP          NORT 575.0
:             2.05E-27           10.42        0.0
END

Creep law 2 which represents primary/secondary creep or secondary/tertiary creep. Note that the creep law is
implicitly temperature dependent. Further versatility is available by allowing the coefficients to vary with
temperature as illustrated in the example above. This example is for a Cr-Mo-V ferritic stainless steel for a
temperature range of approximately 565° ± 50°, Units: N, mm, seconds and °C.
                 ε c = 7.46 x 10-5 σ 5.4 e-3.116 x10 /T + 9.69 x 10-16 σ 5.4 t1.364 e-3.116 x10 /T
                                                        4                                               4
                 

MATE
1     ISO     1.31E5         0.3      16.0E-6          7.9E-9
CREP LAW2
: 7.46E-5              5.4       0.0          3.11E4
: 9.69E-16             5.4       1.364        3.116E4
END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-90
ASAS (Non-Linear) User Manual                                                                          Structural Data


Blackburn law for 316 stainless steel. Note that no numerical creep data is required and that the units assumed
by ASAS-NL are N, mm, seconds and °C.

MATE
1     ISO     1.53E5         0.3      14.0E-6          7.93E-9          0.0       0.0      450.0
:             1.48E5         0.3      14.0E-6          7.93E-9          0.0       0.0      537.0
:             1.43E5         0.3      14.0E-6          7.93E-9          0.0       0.0      580.0
:             1.38E5         0.3      14.0E-6          7.93E-9          0.0       0.0      593.0
:             1.33E5         0.3      14.0E-6          7.93E-9          0.0       0.0      648.0
:       1.28E5               0.3      14.0E-6          7.93E-9          0.0       0.0      700.0
CREP LAW4
END


5.2.4.4 Failure Material Properties

To define the failure (limiting) values for lamina stresses and strains and laminate stress/strain resultants.

                                                              FLW1
                                                              FLW2
               (mat)               FAIL                       FLW3                     (temp)
                                                              FLW4
                                                              FLW5

                   :             up to 14 failure v alues




Parameters

mat               : material property integer. (Integer, 1-9999)

FAIL              : keyword to define the properties as failure values

FLW1
FLW2
FLW3               : keyword to define failure law type
FLW4
FLW5
temp              : temperature at which these properties apply. (Real)

Notes


1.      FLW1 and FLW2 are in-built lamina failure laws.                         FLW3 to FLW5 are user-defined laws.   See
        Appendix B.5.3 for further details.

2.      The actual failure values required depend upon whether lamina or laminate values are being defined (see
        following sections).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-91
ASAS (Non-Linear) User Manual                                                                          Structural Data




5.2.4.4.1       Lamina Failure Values

The following data input is required for an elastic laminated composite.




Parameters

mat         : material property integer. (Integer, 1-9999)

FAIL        : keyword to define the properties as failure values

temp        : temperature at which these properties apply. (Real)

xt, xc      : limiting direct tensile and compressive stresses respectively in fibre direction. (Real)

yt, yc      : limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)

zt, zc      : limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)

s12         : limiting shear stress of lamina in 1-2 plane. (Real)

s23         : limiting shear stress of lamina in 2-3 plane. (Real)

s31         : limiting shear stress of lamina in 3-1 plane. (Real)

zl          : limiting interlaminar tensile stress. (Real)

sl          : limiting interlaminar shear stress. (Real)

ε1t, ε1c : limiting direct tensile and compressive strains respectively in fibre direction. (Real)

ε2t, ε2c : limiting direct tensile and compressive strains respectively normal to fibre in direction 2. (Real)

ε3t, ε3c : limiting direct tensile and compressive strains respectively normal to fibre in direction 3. (Real)

γ12         : limiting shear strain of lamina in 1-2 plane. (Real)


γ23         : limiting shear strain of lamina in 2-3 plane. (Real)


γ31         : limiting shear strain of lamina in 3-1 plane. (Real)

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-92
ASAS (Non-Linear) User Manual                                                                          Structural Data


Notes


1.       Up to 20 failure values are expected but if less are specified then the remaining values default to zero.

2.       If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.

3.       Isotropic, orthotropic or anisotropic failure material properties must be preceded by material properties.

4.       Using the above data, a number of lamina failure criteria are evaluated in POSTNL when options FEMV-
         LAMI are selected. See Appendix B.5.1 for further details.


5.2.4.4.2       Plastic Lamina Failure FLW1 Values

The following data input is required for a ‘plastic’ laminated composite i.e. when an element referencing this
material belongs to a group of elements with directive PLAS.




Parameters

mat         : material property integer. (Integer, 1-9999)

FAIL        : keyword to define the properties as failure values

FLW1          : keyword to denote that the in-built failure law type 1 is to be used. See Appendix B.5.3.1 for
              details

ftype       : failure criterion for matrix failure. Valid keywords are:
                TSWU              -        Tsai-Wu (default)
                TSAI              -        Azzi-Tsai
                HOFF              -        Hoffman
                NORR              -        Norris
                MISE              -        von Mises
                MXCS              -        maximum stress

temp        : temperature at which these properties apply. (Real)

xt, xc      : limiting direct tensile and compressive stresses respectively in fibre direction. (Real)

yt, yc      : limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)

zt, zc      : limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)

s12         : limiting shear stress of lamina in 1-2 plane. (Real)

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-93
ASAS (Non-Linear) User Manual                                                                           Structural Data


s23         : limiting shear stress of lamina in 2-3 plane. (Real)

s31         : limiting shear stress of lamina in 3-1 plane. (Real)

zl          : limiting interlaminar tensile stress. (Real)

sl          : limiting interlaminar shear stress. (Real)


βE            : dimensionless material parameter            β E defining the reduction in fibre stiffness after matrix failure.
              0≤     β E ≤ 1.0. A value of β E=0.0 means no reduction in fibre stiffness, a value of 1.0 means a
              complete loss of fibre stiffness. (Real)


β2            : dimensionless material parameter β2 defining the reduction in fibre stiffness after fibre failure. (0

              ≤   β 2 ≤ 1.0). By default, β 2=0.0 and this means that the matrix stiffness is assumed after fibre
              failure. For    β 2 •0.0, the fibre stiffness after failure is (1- β 2) times its value before failure.

Notes


1.      Up to 13 failure values are expected but if less are specified then the remaining values default to zero.

2.      If the failure law type is left blank, the failure data will have the same meaning as for an elastic laminated
        composite. When analysis beyond first ply failure is required, FLW1 will be assumed with
        β E= β 2=0.0.

3.      If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.


5.2.4.4.3         Plastic Lamina Failure FLW2 Values

The following data input is required for a ‘plastic’ laminated composite, i.e. when an element referencing this
material belongs to a group of elements with directive PLAS.




Parameters

mat         : material property integer. (Integer, 1-9999)

FAIL        : keyword to define the properties as failure values

FLW2        : keyword to denote that the in-built failure law type 2 is to be used. See Appendix B.5.3.1 for details




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-94
ASAS (Non-Linear) User Manual                                                                                Structural Data


ftype          : failure criterion for matrix failure. Valid keywords are:
                   TSWU            -       Tsai-Wu (default)
                   TSAI            -       Azzi-Tsai
                   HOFF            -       Hoffman
                   NORR            -       Norris
                   MISE            -       von Mises
                   MXCS            -       maximum stress

temp           : temperature at which these properties apply. (Real)

xt, xc         : limiting direct tensile and compressive stresses respectively in fibre direction. (Real)

yt, yc         : limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)

zt, zc         : limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)

s12            : limiting shear stress of lamina in 1-2 plane. (Real)

s23            : limiting shear stress of lamina in 2-3 plane. (Real)

s31            : limiting shear stress of lamina in 3-1 plane. (Real)

zl             : limiting interlaminar tensile stress. (Real)

sl             : limiting interlaminar shear stress. (Real)

β 1- β 8 : dimensionless material parameters defining the reduction in lamina stiffness after different modes of
                 failure. (0 ≤   β i ≤ 1.0). The default of all the β s are β =0.0. See Appendix B.5.3.1 for details

Notes


1.          Up to 18 failure values are expected but if less are specified then the remaining values default to zero.

2.          If a failure strength is set (or defaults) to zero, the relevant term in the failure criterion is ignored.


5.2.4.4.4          Laminate Failure Values

The following data input is required for an elastic laminated composite when it is required that failure criteria in
terms of the shell stress/strain resultants are to be calculated.

      (mat)              FAIL            (temp)


        :                 εx
                          ˆ         εy
                                    ˆ        εxy
                                             ˆ           ψx
                                                          ˆ          ψy
                                                                      ˆ         ψxy
                                                                                 ˆ            εxz
                                                                                              ˆ         εyz
                                                                                                        ˆ




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-95
ASAS (Non-Linear) User Manual                                                                          Structural Data


Parameters

mat           : material property integer. (Integer, 1-9999)

FAIL          : keyword to define the properties as failure values

temp          : temperature at which these properties apply. (Real)


εx
ˆ             : allowable direct strain in element local x direction. (Real)


εy
ˆ             : allowable direct strain in element local y direction. (Real)


εxy
ˆ             : allowable shear strain in element local xy plane. (Real)


ψx
 ˆ            : allowable bending curvature in element local x direction. (Real)


ψy
 ˆ            : allowable bending curvature in element local y direction. (Real)


ψxy
 ˆ            : allowable torsional curvature in element local xy plane. (Real)


εxz
ˆ             : allowable shear strain in element local xz plane. (Real)


εyz
ˆ             : allowable shear strain in element local yz plane. (Real)

Notes


1.      Using the above data, the laminate failure criterion as described in Appendix B.5.2 is evaluated in
        POSTNL when options FEMV-GFAI are selected. Note that up to four further user defined criteria may
        be evaluated and that up to 14 failure values may be specified. To be consistent with the calculation of
        the first failure criterion, the first 8 failure values should be those defined above.

2.      The laminate failure data must be specified immediately after the LAMI material property data.

3.      If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-96
ASAS (Non-Linear) User Manual                                                                          Structural Data


Examples


A simple example of an orthotropic lamina for a laminated shell with failure values specified for the direct
stresses in the fibre directions only.

        MATE
        1      LAMI
        10     ORTH 1350.0
        : 84.0E6 6.0E6 0.0 2.1E6 2.1E6 2.1E6 0.34 0.0 0.0
        : -3.0E-6 35.OE-6 0.0
       10 FAIL
       : 1280.0E3 290.0E3
       END

An example showing the data for 3 different orthotropic laminae for a laminated shell with failure values for all
stress components.

       MATE
       1       LAMI
       10 ORTH 1350.0
       : 84.0E6 6.0E6 0.0 2.1E6 2.1E6 2.1E6 0.34 0.0 0.0
       : -3.0E-6 35.OE-6 0.0
       10 FAIL
       : 1280.0E3 290.0E3 39.0E3 150.0E3 52.0E3
       20 ORTH 1610.0
       : 130.0E6 9.0E6 0.0 4.8E6 4.8E6 4.8E6 0.28 0.0 0.0
       : -0.1E-6 28.0E-6 0.0
       20 FAIL
       : 1370.0E3 1000.0E3 42.0E3 200.0E3 60.OE3
       30 ORTH 1800.0
       : 40.0E6 8.0E6 0.0 4.0E6 4.0E6 4.0E6 0.25 0.0 0.0
       : 6.3E-6 36.0E-6 0.0
       30 FAIL
       : 800.0E3 600.0E3 36.0E3 150.0E3 60.0E3
       END

An example showing the data for a non-linear composite material composed of layers of orthotropic material
obeying failure law 1 (FLW1)

       MATE
       11 ORTH
       : 5.72E4 3.9E3 3.9E3 2.3E3 2.3E3 2.3E3 0.35 0.35 0.35
       11 FAIL FLW1
       : 1.3E3 1.3E3 12.0 53.0 34.0 0.8
       1 LAMI
       END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-97
ASAS (Non-Linear) User Manual                                                                          Structural Data


An example showing the data for a linear elastic composite material composed of two different orthotropic
materials with a laminate failure criterion based on limiting curvatures only.

        MATE
        1     LAMI
        1     FAIL
        : 0.0 0.0 0.0 0.015 0.015 0.015
        2 ORTH
        : 5.72E4 3.9E3 3.9E3 2.3E3 2.3E3 2.3E3 0.35 0.35 0.35
        3 ORTH
        : 3.81E4 4.75E3 4.7E3 2.3E3 2.3E3 2.3E3 0.32 0.32 0.32
        END




5.2.5        Geometric Properties Data

To define the geometric properties, such as thickness, area, or bending inertia, for every element used in the
structure.

               GEOM

                geom              eltype              (sect)               properties

                 :                CABL                properties

                END




Parameters

GEOM                 : compulsory header keyword to denote the start of the geometric property data

geom                 : identifying number of the geometric properties integer. This number must be unique, and
                       independent of the type of element. (Integer, 1-999999)

eltype               : element type. This must correspond with the element type defined in the element topology
                       data for this geometric property integer

sect                 : keyword to denote cross-section type for element STF4

properties           : list of geometric properties. See Appendix -A for the details of which properties are required
                       for each element type. Continuation lines may be used if necessary. (Real)

CABL                 : keyword to denote the cable option for element FLA2. See Appendix -A for further details

END                  : keyword to denote the end of the geometric properties data block

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-98
ASAS (Non-Linear) User Manual                                                                              Structural Data


Notes


1.      Geometric property data for elements SST4 and WST4 must be input in a different format. Details are
        given in Section 5.2.5.1.

2.      Geometric property data for elements SPR1 and SPR2 must have stiffness and/or damping properties.
        Details are given in Section 5.2.5.2.

3.      Geometric property data for laminated shells requires additional information concerning the layup
        sequence. Details are given in Section 5.2.5.3.

4.      Geometric property data for rigid surface elements requires additional information concerning the
        definition of rigid surface geometry. Details are given in Section 5.2.5.4.

5.      Geometric property data for beam elements where local axes orientation and/or offsets may be defined is
        given in section 5.2.5.5

Example


A simple example of geometric property data for a model composed of beams and shells.

        GEOM
        1 STF4          RECT        0.05       0.05       0.0       0.0      0.0
        :                           0.05       0.05       0.0       0.0      0.0
        :                           0.05       0.05       0.0       0.0      0.0
        2 TCS8          0.010
        3 TCS8          0.008
        END


5.2.5.1 Geometric Properties - (WST4 and SST4)

To define geometric properties for stiffeners (WST4 and SST4) the following format is used in the geometric
properties data.

                geom                eltype            (isec)               rmul

                MCOR

                 mn                 scoor            tcoor

                SCON

                segno              nstart            nfinish               nstat            nlay        thick

                 FIN




Parameters



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-99
ASAS (Non-Linear) User Manual                                                                          Structural Data


geom              : identifying number of the geometric properties integer. This number must be unique, and
                    independent of the type of element. (Integer, 1-999999)

eltype            : element type. This must correspond with the element type defined in the element topology
                     data for this geometric property integer. (One of WST4 or SST4)

isec              : median point corresponding to warping origin (WST4 only). (Integer)

rmul              : rigidity multiplier (1.0 for full cross-section, 0.5 for half symmetric section). (Real)

MCOR              : compulsory header keyword to denote start of median point coordinate definition

mn                : median point number (consecutive). (Integer)

scoor             : s coordinate of median point. (Real)

tcoor             : t coordinate of median point. (Real)

SCON              : compulsory header keyword to denote start of segment connectivity data

segno             : segment number (consecutive)

nstart            : start median point of segment. (Integer)

nfinish           : finish median point of segment. (Integer)

nstat             : number of stations along segment. (Integer)

nlay              : number of layers through the thickness of segment. (Integer)

thick             : segment thickness. (Real)

FIN               : indicates end of the property set

Notes


1.       See element description sheet (Appendix -A) for details of stiffener elements.

2.       Median point numbers can be assigned in any convenient manner. Segment numbering however is not
         arbitrary but must adhere to the following rules:

        (a)     The first segment starts at a free edge.

        (b)     Each subsequent segment starts from the end of a previously defined segment.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-100
ASAS (Non-Linear) User Manual                                                                          Structural Data




3.     The full cross-section geometry must always be defined irrespective of the value specified for rmul

Example


An example of a tee-section stiffener with the origin at the junction of web and flange

       GEOM
       1             SST4         1.0
       MCOR
       1         -0.2           0.0
       2             0.0        0.0
       3             0.2        0.0
       4             0.0        0.256
       SCON
       1         1          2       3        3         0.012
       2         2          3       3        3         0.012
       3         2          4       5        3         0.015
       FIN
       END


5.2.5.2 Geometric Properties - (SPR1 and SPR2)

Stiffness and/or damping characteristics are required for springs SPR1 and SPR2 in the following format.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-101
ASAS (Non-Linear) User Manual                                                                          Structural Data




                    geom                eltype           px             py            pz



                       :                 STIF                stifprops



                        :                DAMP                 dampprops




Parameters

geom              : identifying number of the geometric properties. This number must be unique and independent
                     of the element type. (Integer, 1-999999)

eltype            : element type (one of SPR1 or SPR2)

Px,Py,Pz          : global coordinates of a point which defines the line of action of the spring. (Real)

STIF              : keyword to denote that stiffness characteristics are to be defined for springs

stifprops         : linear stiffness, K, or tabulated values of displacement (or rotation) and force (or moment)
                     (δ1, F1, δ2, F2....... δn, Fn). (Real)

DAMP              : keyword to denote that damping characteristics are to be defined for springs

dampprops : linear damping factor, C, or tabulated values of velocity (or angular velocity ) and force (or
                     moment) (v1, F1, v2, F2....... vn, Fn). (Real)

Notes


1.      STIF and DAMP must be the first item on a line after the continuation marker (:).

2.      If px, py and pz are zero, the line of action of the spring coincides with the local X axis (see element
        description in Appendix -A).

3.      The stiffness and damping properties are extrapolated beyond the user defined points.

4.      A maximum of 20 pairs of (δ,F) and (v,F) are allowed.

5.      The angular unit must be radians and this cannot be changed

6.      S and V must be specified in ascending order.

7.      The spring curve must pass through the origin when applied to an inelastic material model.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-102
ASAS (Non-Linear) User Manual                                                                                   Structural Data


Examples


An example of a rotational spring with constant stiffness, no damping and aligned with the element local axis
system.

       GEOM
       1 SPR2
       : STIF 200.0
       END



An example of a translational spring/dashpot with piecewise linear definition of stiffness and damping with a
fixed line of action.
                           F                                                                            F




                                                                                                                              .
                                                               δ                                                              v




       GEOM
       2 SPR1            1.0               1.0             0.0
       : STIF           -0.5            -300.0            -0.2            -200.0
       :                  0.1            400.0              0.4            600.0            0.7          650.0
       : DAMP          -60.0          -3000.0            -30.0          -2500.0
       :                 0.0              0.0             20.0           4000.0           50.0          5000.0
       END


5.2.5.3 Geometric Properties - (Laminated Construction)

To define the geometric properties and layup data for laminated elements.
                  geom                eltype              properties

                  :                   LAMI                nlam              (sym)


                  :                   mat                 thick             theta                 (layno)

                  RP                  nrep




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-103
ASAS (Non-Linear) User Manual                                                                          Structural Data


Parameters

geom              : identifying number of the geometric properties integer. This number must be unique and
                     independent of the type of element. (Integer, 1-999999)

eltype            : element type. This must correspond with the element type defined in the element topology
                     data for this geometric property integer. (One of QUS4, TCS6, TCS8, TCS9, LB15 or
                     LB20)

properties        : list of geometric properties. These must be specified for shells and omitted for bricks. See
                     Appendix -A for details of which properties are required for each element type. Continuation
                     lines may be used if necessary. (Real)

LAMI              : compulsory keyword to denote that the data for a laminate is to be defined

nlam              : number of laminae of which the laminate is composed or half the number of laminae if sym is
                     set to 1. See below. (Integer)

sym               : optional flag to be set to 1 if a symmetrical laminate. By default sym will be set to zero which
                     implies that data for all laminae is to be supplied. (Integer)

mat               : material property integer defining the material for this lamina. (Integer)

thick             : the thickness of this lamina. (Real)

theta             : the angle between the principal material axis direction for this lamina and the laminate
                     principal material axis direction. Default unit is degrees. (Real) Note: -90° ≤ theta ≤ + 90°

layno             : layer number to be assigned to layer.                      If omitted, layers are numbered sequentially
                     commencing at one. The layer number is only used for post-processing purposes at present.
                     (Integer)

RP                : keyword to indicate the generation of lamina data from the previous / command.

nrep              : number of times the data is to be repeated. (Integer)

Notes


1.      The shell nodal thicknesses must be specified and be non-zero. The laminae data specified here are used
        to calculate the equivalent anisotropic material matrix coefficients C1 to C24 in the manner described in
        Appendix -B. The thickness terms appearing in the C matrix as described in Appendix -A are
        interpolated from the nodal thicknesses supplied here. For laminated brick elements, the laminated
        thickness is directly obtained from the element geometry and the nodal thickness data are not required.

2.      The properties mat, thick, theta and layno are repeated nlam times. There is no limit to the number of
        laminae that may be used to define a laminate.

3.      The material for a lamina may be defined as isotropic, orthotropic or anisotropic.

4.      Layer number 1 lies on the bottom surface of an element as defined by the element local axis system. See
        Appendix -A.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-104
ASAS (Non-Linear) User Manual                                                                                 Structural Data


5.     A number of layers, delimited by a / command and an RP command, may be repeated nrep times to
       create a regular region of the laminate. See example 3.

Examples


A simple example of the geometric property data for a laminated QUS4 shell element of constant thickness equal
to the sum of the thicknesses for all laminae. The laminate is composed of 5 laminae using 2 different material
types. The layup sequence is [-90/-45/0/45/90].

       GEOM
       1    QUS4        7.0
       :    LAMI        5
       : 10 1.0         -90.0
       : 10 1.0         -45.0
       : 20 3.0            0.0
       : 10 1.0           45.0
       : 10 1.0           90.0
       END


An example showing the geometric property data for a laminated and tapered TCS8 shell element where the sum
of the thicknesses of all the laminae equals the average thickness for the element as defined by the nodal
thicknesses. Note that the laminate is formed of 4 laminae but as the layup is symmetrical sym is set to 1. The
layup sequence is [90/0/0/90] or in abbreviated form [90/0]s.

       GEOM
       1    TCS8        5.0 5.0 5.0 4.0
       :                3.0 3.0 3.0 4.0
       :    LAMI        2 1
       : 98 1.0         90.0
       : 99 1.0          0.0
       END

An example showing the use of both the symmetry option and the repeat facility for a laminate brick composed
of a total of 60 layers. Two materials are used, one is orthotropic and the other is isotropic. The corresponding
material data is also shown.

        GEOM
        1    LB20
        :    LAMI 30 1
        /
        : 11 0.045 0.0
        : 12 0.06 0.0
        : 11 0.045 90.0
        RP 10
        END
        *
        MATE
        1    LAMI
        11 ORTHO
        : 25.0E6 1.0E6 1.0E6                         0.5E6        0.2E6        0.5E6        0.25        0.25   0.25
        12 ISO     3.7E6 0.3
        END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-105
ASAS (Non-Linear) User Manual                                                                          Structural Data


5.2.5.4 Geometric Properties - (Rigid Surface Elements)

To define the geometric properties, if present, and rigid surface geometry for rigid surface elements.

               geom            eltype                  (thick)


               :               RIGS                    nseg

                                LINE                   node1                node2
               :
                                CIRC                   node1                node2               node3




Parameters

geom               : identifying number of the geometric properties integer. This number must be unique, and
                     independent of the type of element. (Integer, 1-999999)

eltype             : element type. This must correspond with the element type defined in the element topology
                     data for this geometric property integer, (one of RG23, RG24, RGX3 or RGX4)

thick              : nodal thickness, only required for element types RG23 and RG24 when attached to plane
                     stress membrane elements. See Appendix -A for details of which properties are required for
                     each element type. Continuation lines may be used if necessary. (Real)

RIGS               : keyword to denote that geometry of the rigid surface is to be defined

nseg               : number of segments defining the rigid surface. (Integer)

LINE               : keyword to denote that the current segment type is linear

CIRC               : keyword to denote that the current segment type is circular

node1              : node number at start of segment. (Integer)

node2              : node number at end of segment. (Integer)

node 3             : node number defining centre of the segment if circular. (Integer)

Notes


1.      The coordinates of the node numbers must be defined in the Coordinate data.

2.      The order of input of the nodes defines the direction of positive progression along the rigid surface
        (indicated by s in the example below). A right handed rotation of 90° from the positive tangent direction
        then defines the outward normal to the surface (i.e. n in example below).

3.      The user should ensure that the rigid surface definition extends far enough to cover all expected motions
        of the deforming and rigid parts of the model.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-106
ASAS (Non-Linear) User Manual                                                                                  Structural Data


Example


An example of an axisymmetric rigid punch

       GEOM
       1     RGX3                                                                            n

       :     RIGS       3                                                                           s       2           n
                                                                                   1
       :     LINE       1     2                                                                                         s
       :     CIRC       2     3     5                                                                   5           3

       : LINE           3     4
       END                                                                                                                  n
                                                                                                                    s



                                                                                    CL
                                                                                                                4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                       Page 5-107
ASAS (Non-Linear) User Manual                                                                          Structural Data




5.2.5.5 Definition of geometric properties for beam elements having local axes definition
            and/or rigid offsets

There are four engineer’s theory of bending, two-node beam types in ASAS for which the user can define the
local axes and/or specify rigid offsets. In order to prevent confusion, the data requirements for each of these
have been presented explicitly. These definitions may be used in any combination together with the general
definition described in Section 5.2.5 to build a complete geometric data block (headed by the keyword GEOM
and terminated by the keyword END) for a structure consisting of a mixture of any of the ASAS elements.


a) BEAM

                                                             sectid
                      geom              BEAM
                                                            a       iz        iy     j

                                    OFFG             glboff

                                    OFFS             locoff
              :
                                    OFSK             skew                          skw off
                                    OFCO             coords




b) BM2D

                                                                    sectid
                      geom              BM2D
                                                                a        iz        ay

                                    OFFG             glboff

                                    OFFS             locoff
               :
                                    OFSK             skew                          skw off
                                    OFCO             coords




Notes


1.      Only 4 offset values are specified relating only to offsets in the global XY and local X’Y’ planes.

2.      Only skewed systems that are a rotation about the global Z may be used.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-108
ASAS (Non-Linear) User Manual                                                                                  Structural Data


c) BM3D
                                                     BETA         angle

                                                     NODE         nodeno

                                     sectid                                             (XY)
                                                     (COOR)       pcoor
            geom       BM3D                                                                      (SHAR)*   ay   az
                                    a iz iy j        GPOS                               XZ

                                                     GNEG

                                                                             axis
                                                                                                *
                                                                                         Shear areas must not be defined here if
                                                     SPOS
                                                                  skew                   section data has been referenced.
                                                     SNEG                                The shear areas should be given as part
                                                                                         of the section data.
                                                     VECT         vcoor

                                    OFFG             glboff

                                    OFFS             locoff
              :
                                    OFSK             skew                  skwoff

                                    OFCO             coords




d) TUBE
                                                     BETA         angle

                                                     NODE         nodeno
                                                                                        (XY)
                                  sectid             (COOR)       pcoor
            geom       TUBE
                                                     GPOS                               XZ
                                    dia thick
                                                     GNEG

                                                     SPOS                    axis
                                                                  skew
                                                     SNEG

                                                     VECT         vcoor


                                    OFFG             glboff

                                    OFFS             locoff
              :
                                    OFSK             skew                  skwoff

                                    OFCO             coords




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-109
ASAS (Non-Linear) User Manual                                                                          Structural Data


Parameters

a) General

geom                   : identifying number for the geometric property. This number must be unique, a separate
                         number being required for every different element type as well as for each differing
                         geometric definition. (Integer)

BEAM, BM2D,            : element type. This must correspond to the element type defined in the element topology
BM3D, TUBE               referencing this geometric property.

sectid                 : section identifier. (Alphanumeric up to 12 characters). This refers to a section input as
                         SECTION data. See Section 5.2.6.

b) Axes Definition

BETA                   : keyword to denote that local axis defined by beta angle (rotation of default local axes about
                         member X axis). See Appendix A.2.

angle                  : beta angle. (Real, degrees)

NODE                   : keyword to denote that local axis defined by third node point. See Appendix A.2.

nodeno                 : third node number. (Integer)

COOR                   : keyword to denote that local axis defined by third point coordinates. See Appendix A.2.

pcoor                  : global coordinates (x, y, z) of third point. (Real)

GPOS                   : keyword to denote that local axis defined by positive axis direction in global reference
                         plane. See Appendix A.2.

GNEG                   : keyword to denote that local axis defined by negative axis direction in global reference
                         plane. See Appendix A.2.

SPOS                   : keyword to denote that local axis defined by positive axis direction in a skewed reference
                         plane. See Appendix A.2.

SNEG                   : keyword to denote that local axis defined by negative axis direction in a skewed reference
                         plane. See Appendix A.2.

axis                   : axis defining global/skewed reference plane (X,Y or Z).

skew                   : skew integer for defining skewed reference plane. (Integer)

VECT                   : keyword to denote that local axis defined by vector. See Appendix A.2.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-110
ASAS (Non-Linear) User Manual                                                                          Structural Data


vcoor                  : global coordinates (x,y and z) which define a vector direction from the origin.

XY,XZ                  : keywords to denote that axis being defined is in local XY or local XZ plane. See Appendix
                         A.2.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-111
    ASAS (Non-Linear) User Manual                                                                          Structural Data


c) Offset Definition

OFFG                       : keyword to denote that offsets are to be defined using global coordinate axes.             See
                             Appendix A.3.

glboff                     : global offset values for both ends of the beam element. (Real)

OFFS                       : keyword to denote that offsets are to be defined using the elemental local axes. See
                             Appendix A.3.

locoff                     : local offset values for both ends of the beam element. (Real)

OFSK                       : keyword to denote that offsets are to be defined using a skewed coordinate axis system.
                             See Appendix A.3.

skew                       : integer for the skew system in which offsets are to be defined.

skwoff                     : skewed offset values for both ends of the beam element. (Real)

OFCO                       : keyword to denote that offsets are to be defined by explicit definition of the global end
                             coordinates of the physical member.

coords                     : coordinates of both ends of the physical member. (Real)


d) Basic properties (see Appendix A for full element specification)

a                          : cross-sectional area, constant for section. (Real)

iz                         : 2nd moment of area about local ZZ axis, constant for section. (Real)

iy                         : 2nd moment of area about local YY axis, constant for section. (Real)

j                          : torsion constant, constant for section. (Real)

SHAR                       : keyword indicating that shear areas follow.

ay                         : shear area in local Y, constant for section. (Real)

az                         : shear area in local Z, constant for sectio. (Real)




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-112
ASAS (Non-Linear) User Manual                                                                                 Structural Data


Notes


1.      Nonsections must not be assigned to TUBE elements.

2.      Only relevant flexural properties will be utilised for a given element type, for example


                                                            BEAM           BM2D           BM3D          TUBE

        Area                               A                     ♦              ♦             ♦

        Moment of Inertia                  IZ                    ♦              ♦             ♦

        Moment of Inertia                  IY                    ♦                            ♦

        Torsion constant                   J                     ♦                            ♦

        Shear Area                         AY                                   ♦             ♦

        Shear Area                         AZ                                                 ♦

        Diameter                           D                                                              ♦

        Thickness                          T                                                              ♦




3.      When the properties for some beams are to be given by section data and for others explicitly, the two
        types of definition may be mixed.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-113
ASAS (Non-Linear) User Manual                                                                                 Structural Data




5.2.6       Section Data

To define section type, dimensions and properties for sections to be used with element types BEAM, BM2D,
BM3D and TUBE elements.

               SECT

               sectid              type                   XSEC                    dimensions


               sectid              FAB                    ftype                   dimensions



               :                                          ftype                   dimensions




                                                            flexprops
               :                  FLEX
                                                            proptype                            property


                                                          TOP                  (zoff)                   LEFT            (yoff)

               :                  ORIG                    BOTT                 (zoff)                   RIGH            (yoff)

                                                                  (CENT)                                       (CENT)

               END




Parameters

SECT               : compulsory header to denote the start of the section data.

sectid             : section identifier. (Alphanumeric, up to 12 characters). This identifier must be unique and is
                     independent of the section type.

type               : type, or shape, of section being defined. (Alphanumeric, up to 4 characters).
                         Valid types are:           WF            wide flange
                                                    FBI           Fabricated I beam
                                                    TUB           tubular
                                                    RHS           rolled hollow section
                                                    BOX           fabricated box
                                                    CHAN          channel
                                                    ANGL          angle
                                                    TEE           tee
                                                    PRI           general prismatic section

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-114
ASAS (Non-Linear) User Manual                                                                          Structural Data


                         see Section 5.2.6.1

XSEC              : keyword to denote that cross-section dimensions are to be defined on this line. See Note 1

dimensions : list of section dimensions. See Section 5.2.6.1 for the details of which dimensions are required
                     for each section type. (Real)

FAB               : keyword to denote that a FABricated plate section is to be defined on this and subsequent lines.

ftype             : type of dimensional property being defined for Fabricated plate section (Alphanumeric, up to 4
                     characters).
                         Valid types are:           BLOC         flat plate section
                                                    CURB         curved plate section
                                                    CUT          cut line
                                                    POIN         stress point

                         see Section 5.2.6.2

FLEX              : keyword to denote that geometric properties are to be defined on this line. See Note 1

flexprops         : list of geometric properties. For all section types this is AX,IZ,IY,J,AY,AZ
                         where             AX       cross sectional area
                                           IZ       principal moment of inertia about element local Z axis
                                           IY       principal moment of inertia about element local Y axis
                                           J        torsion constant
                                           AY       effective shear area for forces in element local Y direction
                                           AZ       effective shear area for forces in element local Z direction

                         Shear strain is neglected for a given direction if AY and/or AZ is zero.

proptype          : name of geometric property to be defined. Valid names are AX,IZ,IY,J,AY,AZ with the
                     meaning as above.

property          : value to be assigned to the named geometric property.

Notes


1.      For any given section identifier XSEC and/or FLEX commands may be supplied with the following
        interpretations.

        If only XSEC is defined, the geometric properties will be automatically calculated by the program for use
        in the structural analysis.

        If only FLEX is defined, all property values must be supplied.

        If both XSEC and FLEX commands are utilised, any geometric properties explicitly defined will
        overwrite those calculated from the section dimensions. This feature permits modification to the stiffness
        of the section to model ring or web stiffeners, built up sections, etc.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-115
ASAS (Non-Linear) User Manual                                                                               Structural Data


2.      The FLEX and XSEC sub-commands and associated data are interchangeable, i.e. FLEX appears on the
        sectid line with the (optional) XSEC command on a continuation line.

        e.g     W24x100           WF       XSEC          24.0         12.0              0.775                         0.468
                :                          FLEX          29.11        2950.0            223.4                         4.405

        is the same as


                W24x100           WF       FLEX          29.11        2950.0 223.4 4.405
        :                                  XSEC          24.0         12.0     0.775 0.468

3.      For FABbricated plate sections, notes 1 and 2 also apply but XSEC replaced by BLOC, CURB, CUT or
        POIN. The order of these data lines are interchangeable, but a logical sequence is recommended.



4.      Only 4 POIN definitions may be used for each FABricated section.


5.2.6.1 Section Types and Dimensions

ASAS only requires areas and inertias to be specified for beam elements to determine the elemental forces. In
order to simplify data input the section dimensions may be supplied in lieu of, or in addition to, the flexural
properties. The following describes the dimensions required for each section type currently valid in ASAS.

Note


The axes shown correspond to the local axes of the member for element types BEAM, BM3D, TUBE and
BM2D.

Example


     SECT
     W24x100              WF         XSEC           24.0           12.0           0.775            0.468
     P3.5STD              TUB        XSEC           4.0          0.226
     :                               FLEX           2.68         4.79           4.79           1.34
     W18x105              WF         FLEX         30.621         1836.4             249.07              6.7164
     R10x6x3/8            RHS        XSEC         10.0         6.0            0.375
     :                               FLEX         IZ         184.0
     END



Tube - Type TUB

Two dimensions must be defined

Values are D T

where           D        is the outer diameter
                T        is the wall thickness



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-116
ASAS (Non-Linear) User Manual                                                                          Structural Data


Wide flange - Type WF

A maximum of five dimensions can be provided : the first four are obligatory.

Values are     D     B    TF TW (F)

where           D         is the beam depth
                B         is the flange width
                TF        is the flange thickness
                TW        is the web thickness
                F         is the fillet radius
                          (optional, assumed zero)




Fabricated I beam - Type FBI

A maximum of six dimensions can be provided : the first four are obligatory.

Values are     D     BT     TT TW BB             TB

where           D         is the beam depth
                BT        is the top flange width
                TT        is the top flange thickness
                TW        is the web thickness
                BB        is the bottom flange width
                          (optional, assumed same as BT)
                TB        is the bottom flange thickness
                          (optional, assumed same as TT)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-117
ASAS (Non-Linear) User Manual                                                                          Structural Data


Rolled Hollow Section - Type RHS

A maximum of four dimensions can be provided: the first three are obligatory.

Values are     D B T (F)

where           D        is the beam depth
                B        is the beam width
                T        is the thickness
                F        is the fillet radius (optional, assumed zero)




Fabricated Box - Type BOX

A maximum of five dimensions can be provided: the first four are obligatory.

Values are D B TT TS TB

where           D        is the beam depth
                B        is the beam width
                TT       is the thickness of the ‘top’ plate
                TS       is the thickness of the ‘side’ plates
                TB       is the thickness of the ‘bottom’ plate
                         (optional, assumed same as TT)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-118
ASAS (Non-Linear) User Manual                                                                          Structural Data


Channel - Type CHAN

A maximum of five dimensions can be provided: the first four are obligatory.

Values are D B TF TW (F)

where           D        is the beam depth
                B        is the flange width
                TF       is the flange thickness
                TW       is the web thickness
                F        is the fillet radius
                         (optional, assumed zero)




Angle - Type ANGL

A maximum of four dimensions can be provided: the first three are obligatory.

Values are     D B T (F)



where           D        is the beam depth
                B        is the flange width
                T        is the thickness
                F        is the fillet radius (optional, assumed zero)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-119
ASAS (Non-Linear) User Manual                                                                          Structural Data


Tee - Type TEE

A maximum of five dimensions can be provided: the first four are obligatory.

Values are D B TF TW (F)

        where D          is the beam depth
                B        is the flange width
                TF       is the flange thickness
                TW       is the web thickness
                F        is the fillet radius
                         (optional, assumed zero)




Prismatic section - Type PRI

Two dimensions must be defined. For this section type, the flexural properties must also be defined.




Values are D B

where           D        is the maximum depth crossing the Z axis
                B        is the maximum breadth crossing the Y axis


5.2.6.2 Fabricated Plate Sections

The Fabricated plate section is defined by a series of plate segments arranged to form the required cross-section.
These plate segments may either be straight (BLOC) or curved (CURB), and are defined by their dimensions and
location, with respect to an arbitrary origin on the cross-section. In addition, cut lines may be introduced, to
prevent adjacent segments being physically joined. Finally, up to four stress points may be defined on the
section for the purpose of stress evaluation in post-processing.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-120
ASAS (Non-Linear) User Manual                                                                          Structural Data



BLOC - Straight Plate Segment

A maximum of seven values can be provided: the first four are obligatory.

Values are L T YL ZL (AL C1 C2)

where       L        is the length of the plate segment
            T        is the thickness of the plate segment
            YL       is the Y location of plate centroid
            ZL       is the Z location of plate centroid
            AL       is the angular orientation of the plate
                     (optional, assumed zero)
            C1       is the integer for the first associated cell
            C2       is the integer for the second associated cell
                     (C1 and C2 are optional, assumed zero)

Note


AL must be in range -90° to +90°




CURB - Curved Plate Segment

A maximum of eight values can be provided: the first five are obligatory

Values are R T A YL ZL (AL C1 C2)

where       R        is the mean radius of plate segment
            T        is the thickness of the plate segment
            A        is the angle subtended by the plate
            YL       is the Y location of the plate centroid
            ZL       is the Z location of the plate centroid
            AL       is the angular orientation of the plate
                     (optional, assumed zero)
            C1       is the integer for the first associated cell
            C2       is the integer for the second associated cell
                     (C1 and C2 are optional, assumed zero)

Note


A and AL are measured anti-clockwise (AL from Z axis) in degrees.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-121
ASAS (Non-Linear) User Manual                                                                          Structural Data


CUT - Cut Line

A maximum of four values can be provided: the first two are obligatory

Values are Y1 Z1 (Y2 Z2)

where       Y1, Z1            give the position of start of cut line
            Y2, Z2            give the position of end of cut line
            (optional, assumed same as Y1, Z1)




Note


Cut line must occur at a segment boundary. If only two values specified, the nearest boundary will be cut.




POIN - Stress Point

Two values must be defined.

Values are Y1 Z1

where       Y1, Z1            give the position of the stress point




Example

SECT
FABSEC001        FAB      BLOC      50    10   45   25    0   1       *segment 1
:                         CURB      15    10   90   30   50   0 1     *segment 2
:                         BLOC      20    10   20   65   90   1       *segment 3
:                         BLOC      70    10    5   35    0   1       *segment 4
:                         BLOC      30    10   25   25   90   1       *segment 5
:                         BLOC      30    10   25   5    90           *segment 6
:                         CUT       40     5                          *segment 6&1
:                         POIN        0    0                          *stress point           1
:                         POIN      50     0                          *stress point           2
:                         POIN      50    70                          *stress point           3
:                         POIN      0     70                          *stress point           4
END

Notes


1.      The location of the segments may be defined in relation to any origin. The centroidal axes will be
        calculated automatically.


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-122
ASAS (Non-Linear) User Manual                                                                           Structural Data


2.      The axes used to define cut lines and stress points must be the same as that used to locate the segments.

3.      The positioning of stress points is not restricted in any way. Thus a stress point could be off the section.




5.2.7       Skew System Data

There are two methods of defining skew systems. These are by the ‘skew system’ data using direction cosines
and by the ‘nodal skew’ data using 3 node points. The two facilities are complementary, the user may use either
or both types of data as is convenient.


5.2.7.1 Skew Systems - Direction Cosines

To define skew systems in terms of six direction cosines.

             SKEW

             skew               x'x              x'y              x'z              y'x            y'y   y'z

             END



Parameters

SKEW          : compulsory header keyword to denote the start of the skew system data

skew          : skew system integer. (Integer, 1-9999)

x’x,x’y,x’z     :        6 directional cosines. (Real)
                y’x,y’y,y’z

END           : compulsory keyword to denote the end of the skew system data block

Notes


1.      The skew integers must be unique between the SKEW and NSKW data.

2.      The direction cosines supplied are checked for unity and orthogonality as follows:

3.


                 x ′ x 2 + x ′ y2 + x ′ z 2                       = 1.0 ± 0.001


                 y′ x 2 + y′ y2 + y′ z 2                          = 1.0 ± 0.001

               x ′x* y′x+ x ′y* y′y+ x ′z* y′z                    = 0.0 ± 0.001




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page 5-123
ASAS (Non-Linear) User Manual                                                                                    Structural Data


Example 1


Example of Skew Systems data

         SKEW
         1 0.8660             0.5000            0.0             -0.5000            0.8860            0.0
         2 0.6830             0.2588           -0.6830           0.1830           -0.9659           -0.1830
         END
                                                                                              Y
The first line gives the direction cosines for a local axis                    Y'
system which has local Z’ coincident with global Z, and
local X’ and local Y’ rotated by 30° in the global XY
plane.                                                                                                                       X'




                                                                                                        30°                       X




Angle between local X’ and global X                 = 30°               Direction cosine X’X             =        0.8660
Angle between local X’ and global Y                 = 60°               Direction cosine X’Y             =        0.5000
Angle between local X’ and global Z                 = 90°               Direction cosine X’Z             =        0.0
Angle between local Y’ and global X                 = 120°              Direction cosine Y’X             =       -0.5000
Angle between local Y’ and global Y                 = 30°               Direction cosine Y’Y             =        0.8660
Angle between local Y’ and global Z                 = 90°               Direction cosine Y’Z             =        0.0



Example 2                                                                    Z'
                                                                                                                                  X'
The second line gives the direction cosines for a local
axis system which is inclined to all the global axes.                                                               (46,27.789,27)

The local X’ axis is defined by the coordinates                                         (36,24,37)
(36,24,37) and (46,27.789,27). The distance between                                                           (37.895,14,35.105)
these points is:
           2               2           2
  (46 - 36) + (27.789 - 24) + (27 - 37) = 14.641

Hence, the direction cosines for local X’ are given by:                                                                 Y'
                     46 - 36                                  27.789 - 24                                          37
          X ′X =             = 0.6830              X ′Y =                 = 0.2588                X ′Z = 27 -           = -0.6830
                     14.641                                     14.641                                           14.641

Similarly, the local Y’ axis is defined by two points 10.353 apart and the direction cosines for local Y’ are given
by:

          37.895 − 36                                        14 − 24                                    35.150 − 37
Y ′X =                = 0.1830                    YY=                = -0.9659                Y ′Z =                = -0.1830
            10.353                                           10.353                                       10.353

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-124
ASAS (Non-Linear) User Manual                                                                                Structural Data


5.2.7.2 Skew Systems - Nodal Definition

To define skew systems in terms of three node points

              NSKW

              skew               node1             node2             node3

              END


Parameters

NSKW          : compulsory header keyword to denote the start of the nodal skew data

skew          : skew system integer. (Integer, 1-9999)
node1         : 3 node numbers. Used to define a local axis set in the following manner. The line from the first
node2           node to the second node defines the local x’ direction. The plane defined by the three nodes
node3           contains the local y’ direction which lies from the first node towards the third. The local z’ axis
                forms a right handed set with local x’ and y’

END            : compulsory keyword to denote the end of the nodal skew system data block

Notes

1.      The skew integers must be unique between SKEW and NSKW data.

2.      The nodes used to define a skew system must appear in the COOR data. It is not necessary for these
        nodes to be physically present on the structure i.e. they need not appear in the ELEM data.

Example

The first line in the example below describes a 2-D rotation in the x-y plane. Note, the global z axis points
towards the reader but the local z’ axis, forming a right handed set with x’ and y’,
points away from the reader.
                                                                                     z
       NSKW
        100       16       25         37
        101      109      216         54
        END                                                                                                                       x'

                                                                                                                             25
                                                                                                                                       y

                                                                                                        16


                                                                                                                   37
                                                                                                                                   x
                                                                                                             z'         y'




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-125
ASAS (Non-Linear) User Manual                                                                    Boundary Conditions Data



5.3     BOUNDARY Conditions Data

These data blocks define the various ways in which the structure is supported and constrained.

The following data blocks are defined

                         Freedom Releases .... ................ ................ see Section 5.3.2

                         Suppressions ............ ................ ................ see Section 5.3.3

                         Displaced Freedoms ................. ................ see Section 5.3.4

                         Constraint Equations ................ ................ see Section 5.3.5

                         Rigid Constraints ..... ................ ................ see Section 5.3.6

Note


Freedom Release Data, if it exists, must be the first data block in the Boundary Conditions Data.




5.3.1       UNITS Command

The units command is not valid in the Boundary Conditions Data and will be ignored. Therefore any constants
and factors utilised in constraint equations must be consistent with any global units (analysis units) defined in the
Preliminary Data (see Section 5.1.42).




5.3.2       FREEDOM Release Data

To define elements which are to have particular freedoms released from being rigidly connected to the
surrounding elements. Release can only apply to beam elements and the freedoms released are in their local axis
system. See Notes below for more details. If used, freedom release data must be the first data block in the
Boundary Conditions Data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-126
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



              RELE

             (skew )            dof              //elno//           //node//


               RP               nrep              ielem               inode

               RRP              nrrep             iielem              iinode

               END




Parameters

RELE          : compulsory header to define the start of the freedom release data.

skew          : skew system integer. (Integer) Optional.

dof           : name of freedom to be released. See notes.

elno          : user element number of element to be released. (Integer)

node          : node number on the element at which the freedom is to be released. (Integer)

RP            : keyword to indicate data generation from the previous / symbol.

nrep          : the number of times the data is to be generated.

ielem         : user element number increment. (Integer)

inode         : node number increment. (Integer)

RRP           : keyword to indicate data generation from the previous // symbol.

nrrep         : the number of times the data is to be generated.

iielem        : user element number increment. (Integer)

iinode        : node number increment. (Integer)

END           : compulsory keyword to denote the end of the freedom release data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-127
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Notes


1.      Only one skew system is allowed at a node. A node may not be given a different skew system in the
        suppression data from that defined in the freedom release data, etc.

2.      When beam offsets are used at an element and node which is to be released, the release is applied to the
        element at the offset position in the offset local axes.

3.      Care should be taken when using local releases on a beam which has its local axes defined by the
        coordinates of a 3rd point in the geometric property data. If the basic COOR data has been rotated by use
        of a DCOS command, the 3rd point is not similarly rotated.


Local Releases

Local releases are only available on the following element types: BEAM, BM2D, BM3D and TUBE. Valid
released freedom names are X, Y, Z, RX, RY and RZ. (only X, Y and RZ for BM2D)

Rotational releases may be used to put hinged or pinned connections into the member. Translational releases
will produce a sliding joint.

The user should not specify an excessive number of releases for an element. For example one release of a local
RX freedom will be adequate to prevent that member carrying torque, but if both RX local freedoms of an
element are released then that element can turn on its own axis as a local mechanism.

Displacements corresponding to the local releases are not calculated or printed.

If a skew is defined, all skewable degrees of freedom at the node are rotated to the new axis system, not only
those defined by dof.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-128
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Example


1.      In this example, three beam elements with User elements number 5, 7 and 10 meet at node 20. Elements
        7 and 10 have local RZ released to create a pinned joint. RZ on element 5 is not released. If a release had
        been applied to element 5, the original RZ freedom would be left with zero stiffness and would need to be
        suppressed to prevent a local singularity in the structure. (Note that the rotations on elements 7 and 10
        cannot be obtained).
                                                                                               10
                                                                          20



                                                                                                        Y
                                                                  5
                                                                                7
                                                                                                            X

            RELE
            RZ   7           20
            RZ     10        20
            END




5.3.3       SUPPRESSED Freedoms Data

This data defines the nodes and freedoms which are to be suppressed. Any degree of freedom defined here will
have a value of zero for displacement for all load cases in the results.

              SUPP

              (skew )                           dof                              //nodes//


              RP                   nrep           inode

              RRP                  nrrep           iinode

              END




Parameters

SUPP          : compulsory header to define the start of the suppressed freedom data

skew          : optional skew system identifier, see Section 5.2.7. (Integer)

dof           : names of the freedoms to be suppressed. Up to 5 freedoms may be defined. See Appendix -F




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-129
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data


nodes         : list of nodes at which the degrees of freedom are to be suppressed. Continuation lines may be
                used if required. (Integer)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : the number of times the data is to be generated. (Integer)

inode         : node number increment to be added each time the data is generated by the RP command. (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : the number of times the data is to be generated. (Integer)

iinode        : node increment to be added each time the data is generated by the RRP command. (Integer)

END           : compulsory keyword to define the end of the suppressed freedom data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-130
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Notes


1.       The word ALL may be used to indicate that all freedoms at the given node or nodes are to be suppressed.

2.       If a skew is defined, all skewable degrees of freedom at the node are rotated to the new axis system, not
         only those defined by dof.

3.       Reference to a node number or degrees of freedom which does not exist on the structure will produce a
         warning message. Reference to a node number outside the range of node numbers used on the structure
         will produce an error message.

Examples


A simple example of the use of several freedoms at a node, a skew system and the use of ALL.

     SUPP
     X    Y       RZ        15       25       35        39       40
     1      Z               19
     ALL                     1       20
     END

An example to suppress the Z degree of freedom for all nodes in a 2-D membrane structure, say 500 nodes.

     SUPP
     /
     Z      1
     RP 500            1
     END




5.3.4       Prescribed Freedom Data

This data defines the nodes and freedoms which can be given a prescribed non-zero value of displacement,
velocity or acceleration in the load data. See also Section 5.4.3.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-131
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



                   DISP
                   VELO
                   ACCN

              (skew )                           dof                              //nodes//


              RP                nrep              inode

              RRP               nrrep              iinode

              END




Parameters

DISP          : compulsory header to define the start of the prescribed displacement data

VELO          : compulsory header to define the start of the prescribed velocity data

ACCN          : compulsory header to define the start of the prescribed acceleration data

skew          : optional skew system identifier (see Section 5.2.7)

dof           : names of the freedoms to be displaced. Up to 5 freedom may be defined. See Appendix -F

nodes         : list of nodes at which the degrees of freedom are to be given a fixed displacement, velocity or
                acceleration. Continuation lines may be used if required. (Integer)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : the number of times the data is to be generated. (Integer)

inode         : node number increment to be added each time the data is generated by the RP command. (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : the number of times the data is to be generated. (Integer)

iinode        : node number increment to be added each time the data is generated by the RRP command.
                (Integer)

END           : compulsory keyword to define the end of the prescribed displaced freedom data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-132
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data


Notes


1.      Only one of the three compulsory headers is allowed in an analysis.

2.      The word ALL may be used to indicate that all freedoms at the given node or nodes are to have
        prescribed displacements, velocities or accelerations.

3.      If a skew is defined, all skewable degrees of freedom at a node are rotated to the new axis system, not
        only those defined by dof.

4.      If a skew is used at a node, the same skew integer must be defined when the prescribed displacement,
        velocity or acceleration is defined in the loading data. See Section 5.4.3.

5.      Prescribed velocities and accelerations may only be used in transient dynamic analyses.

6.      Reference to a node number or degrees of freedom which does not exist on the structure will produce a
        warning message. Reference to a node number outside the range of node numbers used on the structure
        will produce an error message.

7.      For transient analysis, non-zero prescribed displacements or velocities should not be applied at time t =
        0.0. Any such values specified will be ignored by the program. The initial conditions (INIT) data block
        should be used to specify initial conditions instead.

Example


An example to define nodes 126 and 128 as having displaced freedoms in the Y direction.

        DISP
        Y   126           128
        END




5.3.5       CONSTRAINT Equation Data

This data defines degrees of freedom on the structure whose displacements are to be linearly dependent on one
or more other degrees of freedom in the structure. Currently, constraint equation data is not allowed in explicit
transient dynamics analysis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-133
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data




              CONS

              (skew )          ddof         //dnode//                factor        dof        //node//


              RP               nrep             inode

              RRP              nrrep            iinode

              END


Parameters

CONS          : compulsory header to define the start of the constraint equation data

skew          : optional skew system identifier. Only the dependent node is skewed. (Integer)


Data for the dependent freedom on the left hand side of the constraint equation:

ddof          : dependent freedom name. See Appendix -F

dnode         : dependent node number. (Integer)


Data for the independent freedoms on the right hand side of the constraints equation:

factor        : multiplying factor for the following independent freedom. (Real)

dof           : independent freedom name. See Appendix -F

node          : independent node number. (Integer)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : the number of times the data is to be generated. (Integer)

inode         : node number increment to be added each time the data is generated by the RP command.
                (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : the number of times the data is to be generated

iinode        : node number increment to be added each time the data is generated by the RRP command.
                (Integer)

END           : compulsory keyword to define the end of the constraint equation data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-134
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Notes


1.      Continuation lines may be used where necessary.

2.      The word ALL cannot be used in the constraint equation data. Each equation must be separately and
        explicitly defined or generated with RP and RRP commands.

3.      If a skew is defined for a dependent node, all skewable degrees of freedom at the dependent node are
        rotated to the new axis system, not only the ddof freedom. Freedoms at the independent nodes are
        unaffected by this skew.

4.      The equations must be organised in such a way that a dependent freedom is never used in another
        constraint equation as an independent freedom.

        for example               Y18 = 0.5Y20 + 0.5Y21
                                  Y16 = Y18

        is not admissable since Y at node 18 is the dependent freedom in the first equation and an independent
        freedom in the second. These equations should be rearranged as

                                  Y18 = 0.5Y20 + 0.5Y21
                                  Y16 = 0.5Y20 + 0.5Y21


5.      Dependent freedoms must be truly free and not suppressed, displaced or otherwise restrained.

6.      A constant term may be introduced into the right hand side of the equation. In this case the node number
        and freedom of the first independent term should be omitted and the factor becomes the constant
        displacement. This is equivalent to constraining to a displaced freedom with the same displacement.
        (See example 3 below).

7.      Constraints may be used to remove local singularities in a structure. For example, an out-of-plane
        membrane freedom which has zero stiffness may be constrained to a suitable neighbouring point which
        has stiffness.

        However, constraints cannot be used to remove a rigid body motion from a whole structure which is due
        to a lack of overall support. This can only be done with suppressed or displaced nodes.


8.      The forces associated with the constraint systems are printed out as reactions.

9.      Note that constraint equations may sometimes be used to remove local singularity but this must be treated
        with caution. Consider the example where a model is created by joining together two detached
        components, one properly supported and one unrestrained, through the use of constraints, singularity can
        be removed if each dependent freedom of a constraint lies in the supported side of the model and the
        element that it is being attached to has a lower system number than the other side where the constraint is
        connecting to.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-135
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Examples

In this example, the displacements of node 19 in the global X and Y directions are to be tied to the global X, Y
and RZ displacements of nodes 30 and 33. Because the displacements are all related to the global axes, there is
no need for skew systems. The displacements are related by the following equations:

   X19 = 0.5 X30 + 0.5 X33
   Y19 = 0.3 X30 - 0.3 Y30 + 0.5 RZ30 - 0.3 X33 + 0.3 Y33


   CONS
   X       19       0.5      X     30           0.5       X    33
   Y       19      0.3       X     30          -0.3       Y 30               0.5      RZ      30
   :              -0.3       X     33           0.3       Y 33
   END

A Pin-ended Beam

The beam 88-89 is to be attached by a pin joint to the continuous
column 23-24-25. The nodes 24 and 89 have the same coordinates. In
this example the joint is taken to a ball joint, with complete freedom
of rotation. The details of some joints require the constraining of one
                                                                                                             25
or two of the rotational freedoms.

   CONS
   X       89       1.0      X     24                                                 88                89
   Y       89       1.0      Y     24                                                                        24
   Z       89       1.0      Z     24
   END

A Rigid Edge                                                                                                 23


The edge 1-2-3 of the structure is to be kept rigid whilst node 2 is to
be displaced by 0.2 units in the X-direction. The displacements are
                                                                  4                                     1
related by the equation:

X2 = 0.2 = (X1 + X3) /2                                                                5                2
                                                                                                             0.2
giving:
                                                                                       6                3
X2 = 0.2 (a prescribed displacement)

X3 = 0.4 - X1

   CONS
   X   3          0.4        -1.0          X      1
   END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-136
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data


5.3.6       RIGID Constraints Data

To define rigid regions of the structure. Rigid constraints (rigid elements) are a more convenient method of
specifying constraint equations for particular modelling situations. They can be considered as equivalent to a
string of one or more rigid elements linking the list of nodes. Currently, rigid constraint data is not allowed in
explicit transient dynamics analysis.

          RCON

          (skew )          eltype           //indep//                //nodelist//


          RP               nrep             inode

          RRP              nrrep            iinode

          END




Parameters

RCON          : compulsory header to denote the start of the rigid constraint data

skew          : optional skew system identifier. Only the dependent freedom is skewed. (Integer)

eltype        : rigid element type. See notes. Allowable element types are RLNK, RBM2, RBM3, RLSY,
                RBSY, SBRK, SBSY

indep         : independent node number. (Integer)

nodelist      : list of dependent nodes. (Integer) Continuation lines may be used if required

RP            : keyword to indicate data generation from the previous / symbol

nrep          : the number of times the data is to be generated. (Integer)

inode         : the increment for the independent node and the dependent nodes. (Integer)

RRP           : keyword to indicate data generation from the previous // symbol

nrrep         : the number of times the data is to be generated. (Integer)

iinode        : the increment for the independent node and the dependent nodes. (Integer)

END           : compulsory keyword to denote the end of the rigid constraint data




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-137
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data



Notes


1.      The following Rigid Element types are available:

                RLNK - 3-D rigid pin-ended link

                RBM2 - 2-D rigid beam

                RBM3 - 3-D rigid beam

                RLSY - 3-D rigid pin-ended link system

                RBSY - 3-D rigid beam system

                SBRK - shell-brick interface link

                SBSY - shell-brick interface system


2.      Currently, there is a restriction that the dependent node must not be skewed in large displacement
        analysis.

The characteristics of each element are as follows:

Name                      RLNK            RBM2            RBM3             RLSY             RBSY          SBRK           SBSY
No of Nodes                  2               2                2           arbitrary        arbitrary        2           arbitrary


Nodal                     X,Y,Z            X,Y             X,Y,Z           X,Y,Z            X,Y,Z         X,Y,Z          X,Y,Z
coordinates
                          X,Y,Z          X,Y,RZ            X,Y,Z           X,Y,Z            X,Y,Z         X,Y,Z          X,Y,Z
Degrees of                                             RX,RY,RZ                          RX,RY,RZ           for            for
Freedom linked                                                                                          dependent       dependent
by the element
(Minimum)                                                                                                 X,Y,Z          X,Y,Z
                                                                                                        RX,RY,RZ        RX,RY,RZ
                                                                                                            for            for
                                                                                                        independent    independent




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-138
ASAS (Non-Linear) User Manual                                                                   Boundary Conditions Data


Rigid Systems

RLSY            This is a 3-D pin-jointed rigid link system whereby one node can be rigidly connected to an
                arbitrary number of other nodes on a structure. The single independent node must have at least
                X,Y,Z degrees of freedoms. The dependent nodes will have X,Y,Z as dependent freedoms.

                Since the system reduces to a triangulated series of rigid links, it may not be entirely rigid in all
                three dimensions. For example, a RLSY with all nodes in a plane will not be rigid normal to the
                plane. If full rigidity is required, use RBSY.

RBSY            This is a 3-D rigid-jointed rigid beam system whereby one node can be rigidly connected to an
                arbitrary number of other nodes on a structure. The independent node and all dependent nodes
                must have X, Y, Z, RX, RY, RZ degrees of freedom.

SBSY            This is a shell-brick interface system whereby one node on a shell element is connected to an
                arbitrary number of nodes on brick elements that lie in the shell normal (thickness) direction. The
                independent node must be a shell node and have X,Y,Z,RX,RY,RZ degrees of freedom. The
                dependent nodes are brick nodes and will have X,Y,Z degrees of freedom.




Use of Rigid Elements

The following rules apply:

1.     All nodes used to define a rigid element must be connected to the structure. In the situation where a rigid
       element is connected between a node in space and a node on the structure a dummy element must first be
       used to connect the two nodes. Elements with compatible degrees of freedom must be used.

2.     Skew integers refer to the dependent node for rigid elements RLNK, RBM2, RBM3 and SBRK. Skew
       integers are not valid for RLSY, RBSY and SBSY and if specified will be ignored.

3.     An independent freedom can be suppressed, displaced, or constrained; dependent freedoms cannot.

4.     The addition of rigid elements may overcome local singularity in a structure but this must be treated with
       caution. See notes in Section 5.3.5.

5.     There are no limitations on the number of rigid elements joining at a node or the number of occurrences
       of a dependent node.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-139
ASAS (Non-Linear) User Manual                                                                                                  Loading Data



5.4      Loading Data

These data blocks define the various types of loading which can be applied to the structure.

The following load types are available

                           Nodal loads.............. ................ ................ ................ ................ see Section 5.4.3

                           Prescribed displacements, velocities and accelerations ............... see Section 5.4.4

                           Pressure loads .......... ................ ................ ................ ................ see Section 5.4.5

                           Distributed loads ..... ................ ................ ................ ................ see Section 5.4.6

                           Temperature loads ... ................ ................ ................ ................ see Section 5.4.7

                           Face temperature loads ............. ................ ................ ................ see Section 5.4.8

                           Body force loads...... ................ ................ ................ ................ see Section 5.4.9

                           Centrifugal loads ..... ................ ................ ................ ................ see Section 5.4.10

                           Angular acceleration loads ....... ................ ................ ................ see Section 5.4.11

                           Nodal flux ............... ................ ................ ................ ................ see Section 5.4.12

                           Prescribed Field Variable ......... ................ ................ ................ see Section 5.4.13

                           Flux density ............. ................ ................ ................ ................ see Section 5.4.14

                           Wave load................ ................ ................ ................ ................ see Section 5.4.15

                           Tank loads ............... ................ ................ ................ ................ see Section 5.4.16

                           Load functions ......... ................ ................ ................ ................ see Section 5.4.17




5.4.1         UNITS Command

If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally to load type by the inclusion of a UNITS command. The local units
are only operational for the current load type concerned and will return to the default global units when the next
load type, or loadcase, is encountered.

In general, one or more UNITS commands may appear in a data block thus permitting the greatest flexibility in
data input. The form of the command is similar to that used in the Preliminary data.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                  Page 5-140
ASAS (Non-Linear) User Manual                                                                                       Loading Data




          UNITS                           unitnm




Parameters

UNITS          : keyword

unitnm         : name of unit to be utilised (see below)

Notes


1.      Force, length, temperature and angular unit may be specified. Only those terms which are required to be
        modified need to be specified, undefined terms will default to those supplied on the global units definition
        unless previously overwritten in the current data block.

2.      The default angular unit for all load types is radians

3.      Valid unit names are as defined in Section 5.1.42.1.

Example


Data                                                                            Operational Units            Notes

SYSTEM DATA AREA 5000000
PROJECT ASAS
STRUCTURE ASAS
JOB STATTITLE * EXAMPLESOLV 1.0
UNITS NEWTON METRE                                                              Newtons, metres,             Global definition
END                                                                             centigrade
.
..LOAD 2
SET 1 ‘NODAL AND DISTRIBUTED LOADS’
NODAL LO
UNITS KN                                                                        Kilonewtons, metres,         Note default
X       10.0      5       6       7                                             radians                      angular unit
Y       15.0      1       2
UNITS MM                                                                        Kilonewtons,                 Note default
RY       250.0        8                                                         millimetres, radians         angular unit
RZ       300.0        5       6       7
END
DISTRIBU                                                                        Newtons, metres,             Units revert to
Y     BL1      1000.0             1200.0     5    6                             radians                      global units
Z     BL1        900.0            1050.0     5    6
UNITS KN                                                                        Kilonewtons, metres          Change force




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 5-141
ASAS (Non-Linear) User Manual                                                                                    Loading Data


Y       BL1     1.5      1.6      5     6                                                                   unit to KN
END
*
SET 2 ’DISTRIBUTED LOAD ONLY’
DISTRIBU                                                                       Newtons, metres,             New loadcase reverts
Z       BL5   1200.0         5    6                                            radians                      units to global
END
STOP




5.4.2         LOADING Data

The loading data consists of a header keyword followed by one or more sets of load data.


                 LOAD              (nset)



                 SET              setno              (ptime)              title


                 loadtype


                 data


                 END




Parameters

LOAD          : compulsory header keyword to denote the start of the loading data

nset          : total number of load sets to be specified. Optional. (Integer 1-9999). If supplied, nset must equal
                the number of load sets supplied.

SET           : compulsory keyword denoting the start of a load set

setno         : set number. Every set number must be unique. (Integer, 1-9999)

ptime         : pseudo time for load set, required only if loading is defined using pseudo-times. (Real)

title         : load case title. (Alphanumeric string, 40 characters)




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-142
ASAS (Non-Linear) User Manual                                                                                Loading Data


loadtype : keyword to denote the start of each type of load data

END             : compulsory keyword to denote the end of the data for each load type

Notes


1.       If the load history is defined using load functions, then the load function data must be after all other
         loading data have been specified.

2.       Proportional loading is assumed if there is only one load set and both pseudo-time and load function data
         are absent.

3.       Title must be specified in quotes if the first word is a number.




5.4.3         NODAL LOADS Data

To define the application of nodal loads to the structure. These may be forces or moments.

            NODAL LO

            (skew )           dof                     load                                //nodelist//


            RP               nrep             inode

            RRP              nrrep            iinode

            END




Parameters

NODAL LO            : compulsory header keyword to denote the start of nodal load data

skew                : skew system integer. (Integer)

dof                 : freedom name. See Appendix -F

load                : value of nodal load. (Real)

nodelist            : list of the node numbers which are being loaded. (Integer)

RP                  : keyword to indicate the generation of data from the previous / symbol

nrep                : the number of times the data is to be generated. (Integer)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-143
ASAS (Non-Linear) User Manual                                                                               Loading Data


inode               : node number increment to be added each time the data is generated by the RP command.
                      (Integer)

RRP                 : keyword to indicate the generation of data from the previous // symbol

nrrep               : the number of times the data is to be generated. (Integer)

iinode              : node number increment to be added each time the data is generated by the RRP command.
                      (Integer)

END                 : compulsory keyword to denote the end of the nodal load data for this load case

Notes


1.        Any of the degrees of freedom which exists at a node by virtue of the element types attached to it can be
          loaded with nodal loads.

2.        The nodal loads are applied in the global axis system or, if a skew system has been applied in the
          Boundary Condition data, in the node local axis system, as defined by that skew system.

3.        If a skew system integer is used in the nodal load data, the direction of the applied loads is the
          combination of this skew system and any skew system applied in the Boundary Condition data.

4.        Use of a skew system in the nodal load data does not cause the degrees of freedom at the node to be
          rotated by that amount. The nodal loads are resolved into separate components.

5.        If the same node and freedom are loaded more than once in the nodal loads for a load case, the loads are
          additive.

Example


An example of a single load set consisting only of nodal loads. A point load of 25.0 is applied in the X direction
at all nodes from 1 to 150.

     LOAD      1
     SET       100                    ’TO GENERATE 150 NODAL LOADS’
     NODAL L0
     //
     /
     X      25.0         1
     RP      10      1
     RRP       15        10
     END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-144
ASAS (Non-Linear) User Manual                                                                                Loading Data


5.4.4         PRESCRIBED Displacements, Velocities and Accelerations Data

To define the values of displacements, velocities or accelerations to be applied in this load case to those
freedoms declared as prescribed freedoms in the Boundary Condition data (see Section 5.3.4).

              PRESCRIB

              (skew )          dof                                   prv al                 //nodelist//


              RP               nrep             inode

              RRP              nrrep            iinode

              END




Parameters

PRESCRIB            : compulsory header keyword to denote the start of prescribed freedoms data

skew                : skew system integer. Optional. (Integer)

dof                 : freedom name. See Appendix -F

prval               : value of prescribed displacement, velocity or acceleration. (Real)

nodelist            : list of the node numbers to which the prescribed displacement, velocity or acceleration is to be
                       applied. (Integer)

RP                  : keyword to indicate the generation of data from the previous / symbol

nrep                : the number of times the data is to be generated. (Integer)

inode               : node number increment to be added each time the data is generated by the RP command.
                       (Integer)

RRP                 : keyword to indicate the generation of data from the previous // symbol

nrrep               : the number of times the data is to be generated. (Integer)

iinode              : node number increment to be added each time the data is generated by the RRP command.
                       (Integer)

END                 : compulsory keyword to denote the end of prescribed freedoms data




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-145
ASAS (Non-Linear) User Manual                                                                               Loading Data


Notes


1.       All freedoms used in the prescribed displacements, velocities or accelerations data must have been
         defined in the prescribed freedoms data (see Section 5.3.4).

2.       In any load case, a prescribed displacement, velocity or acceleration is set to zero if it is not assigned a
         value and in this case a suppression is assumed for this freedom.

3.       If a skew system has been defined in the Boundary Conditions data for a prescribed freedom node, the
         same skew integer must appear in prescribed displacement, velocity or acceleration load data for that
         node.

Examples


An example of prescribed displacements for two load sets. In case 1, both nodes are given equal displacement.
In case 2, node 15 is given zero displacement and has become, in effect, a suppression.

     LOAD 2
     SET 1 1.0               ’EQUAL DISPLACEMENT OF 5mm’
     PRESCRIB
     Z     5.0     10
     Z     5.0     15
     END
     SET     2     2.0       ’NODE 10 DISPLACED, NODE 15 FIXED’
     PRESCRIB
     Z     5.0     10
     Z     0.0     15
     END
     STOP




5.4.5        PRESSURE Load Data

To define uniform pressure or varying pressure loading applied to the faces of panel or solid elements.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-146
ASAS (Non-Linear) User Manual                                                                                Loading Data




Parameters

PRESSURE             : compulsory header to denote the start of pressure load data.

LDIR                : keyword to define direction of pressure load.

dir                 : load direction. Optional. Valid names are:
                       GX       global X direction
                       GY       global Y direction
                       GZ       global Z direction
                       X        local X direction
                       Y        local Y direction
                       Z     local Z direction
                       Default direction is assumed if dir is omitted.

U                   : keyword to define data as uniform pressure.

F                   : keyword to define data as face definition.

P                   : keyword to define data as nodal pressure values.

FIN                 : keyword to denote the end of a block of U data, F data or P data.

END                 : compulsory keyword to denote the end of the pressure load data for this loadcase.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-147
ASAS (Non-Linear) User Manual                                                                                 Loading Data


Note


1.      The sign convention for pressure in the default direction on each element type is defined in the element
        description sheets in Appendix -A.

2.      Local pressure load direction is only permitted for shell elements.


5.4.5.1 UNIFORM Pressure Load Data

To define values of the uniform pressure and the element faces to which they are applied.


              U                     (lfunno)                         press                         //nodes//


              RP                    nrep                             inode

              RRP                   nrrep                            iinode

              FIN




Parameters

U              : keyword to define uniform pressure data

lfunno         : load function number; required if, and only if, LFUN specified. (Integer)

press          : value of the uniform pressure. (Real)

nodes          : the element faces to which the uniform pressure is applied. A face of an element is defined by up
                  to 3 corner nodes. (Integer)

RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment to be added each time the data is generated by the RP command.
                  (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment to be added each time the data is generated by the RRP command.
                  (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-148
ASAS (Non-Linear) User Manual                                                                               Loading Data


FIN            : keyword to denote the end of the uniform pressure data block

Notes


1.      A face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For TRX6 and QUX8
        a face is defined by the 3 nodes forming the loaded edge. For TRX3 and QUX4 a face is defined by the
        two nodes forming the loaded edge and any other node on the element.

2.      For panel elements, if 2 corner nodes are supplied, pressure is applied to the edge of the element, positive
        towards the centre of the element. If 3 corner nodes are supplied, pressure is applied normal to the face of
        the elementin the local element axes.

3.      For coincidental faces, for example where a panel overlays the face of a brick, the program will apply the
        pressure to the element with the lowest user number. The direction of the pressure load will be
        determined by this element’s local axis system.

4.      See Table 6.1 for default values and Section 6.2 for the significance of some of the system parameter.


5.4.5.2 NON-UNIFORM Pressure Load Data

To define non-uniform pressure on element faces. A face can have a different value of pressure at each node.
The data required is a set of face (F) definitions followed by a set of nodal pressure values (P). Unspecified
mid-side node pressures are interpolated between adjacent corner nodes.

FACE Data

To define the element faces to which non-uniform pressure is to be applied. This data must be followed by a list
of nodal pressure values.


              F                   //nodes//


              RP                     nrep                            inode

              RRP                    nrrep                           iinode

              FIN




Parameters

F              : keyword to define face data

nodes          : the element faces to which the non-uniform pressure is applied. A face is defined by up to 3
                  corner nodes. (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-149
ASAS (Non-Linear) User Manual                                                                               Loading Data


RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment to be added each time the data is generated by the RP command.
                 (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment to be added each time the data is generated by the RRP command.
                 (Integer)

FIN            : keyword to denote the end of set of face definitions




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-150
ASAS (Non-Linear) User Manual                                                                                 Loading Data



PRESSURE Data

To define the nodal pressure values which are to be applied to the previously defined set of element faces.


              P                     (lfunno)                         press                         //nodes//


              RP                     nrep                            inode

              RRP                    nrrep                           iinode

              FIN




Parameters

P              : keyword to denote nodal pressure data

lfunno         : load function number; required if, and only if, LFUN specified. (Integer)

press          : value of the pressure at the nodes. (Real)

nodes          : the nodes to which the pressure is applied. These nodes must exist on the faces defined by the
                  preceding set of face definitions. (Integer)

RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment. (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment. (Integer)

FIN            : keyword to denote the end of a nodal pressure block

Notes


1.      To define a region of non-uniform pressure, a set of one or more element faces is defined. The set of face
        data is terminated by a FIN keyword. This is immediately followed by a set of nodal pressure values
        which must be sufficient to completely define the pressure field over the selected faces. The nodal
        pressure data is also terminated by a FIN keyword, unless it is the final set in which case it is terminated
        by an END keyword.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-151
ASAS (Non-Linear) User Manual                                                                                     Loading Data


2.      Regions of uniform pressure and non-uniform pressure may be mixed in any order.

3.      A face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For TRX6 and QUX8
        elements, a face is defined by the 3 nodes forming the loaded edge. For TRX3, and QUX4 elements, a
        face is defined by the 2 nodes forming the loaded edge and any other node on the element.

Examples


Two Uniform Pressures are to be applied, a pressure of 10 over area 1-2-3-8-7-6, and a pressure of 20 over area
3-4-5-10-9-8. The following lines will generate the data.
                                                       8                                     9                10
                                    7
                 6


                               p = 10                  p = 10                  p = 20                p = 20




                       1                         2                       3                   4                5




        PRESSURE
        U     10.0         1   2     7
        U     10.0         2   3     8
        *     EXAMPLE OF GENERATING PRESSURE ON SEVERAL FACES
        /
        U     20.0         3   4     9
        RP 2          1
        END

Non-uniform Pressure on one face. The program will assign a pressure of 7.5 to node 2 and 11.0 to node 4 by
interpolation between the adjacent corner nodes.
                                                                                                 5
                                                                     6
                                             7                                         p = 12
                                                                   p = 10
                                                 p=5


                                                                                            4
                                         8       p=5



                                                 p=5                         p = 10
                                             1                 2                   3




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-152
ASAS (Non-Linear) User Manual                                                                                  Loading Data


      PRESSURE
      F        1       5       7
      FIN
      P   5.0                  1       7           8
      P        10.0            3       6
      P 12.0                   5
      END

Example of a complete block of Pressure data for Uniform and Non-uniform Pressures
        p = 20                                                                   15
                                       20


                                                                 10                10
                                                                                                                        5



               13                                  14                 15           16                      17           18



               7                                   8                      9        10                      11        12




           1                                   2                      3        4                      5             6




      PRESSURE
      U        20.0            1       2               8
      U 20.0                   7       8           14
      FIN
      //
      /
      F            2       3       9
      RP           2       6
      RRP 3                1
      FIN
      P 20.0                   2           8           14
      P        10.0            3        9              15   4   10    16
      P        15.0            5       11              17
      FIN
      /
      U            5.0         5           6           12




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-153
ASAS (Non-Linear) User Manual                                                                              Loading Data


        RP 2         6
        END




5.4.6        DISTRIBUTED Load Data

This type of loading consists of patterns of load applied to the element as opposed to being applied to the nodes.
Distributed Loads data can contain several load patterns, and an element can be loaded with several load patterns
of the same or different types within one load set.

The following load patterns are available:

BL1      -      Linearly varying normal load or bending moment on beams

BL2      -      Linearly varying axial load or torque on beams

BL3      -      Stepped uniform load on beams

BL4      -      Partial uniform axial or normal load, torque or bending moment on beams

BL5      -      Intermediate axial or normal point load, torque or bending moment on beams

BL6      -      Partial linearly varying normal or axial load, torque or bending moment on beams

BL7      -      Partial quadratically varying normal or axial load, torque or bending moment on beams

BL8             Equal and opposite axial or normal point load, torques or bending moments on beam elements
                applied at both ends

GL1      -      Linearly varying global load, torque or bending moment on beams

GP1      -      Linearly varying global load, torque or bending moment on projected length of beams

GL4      -      Partial uniform global load, torque or bending moment on beams

GP4      -      Partial uniform global load, torque or bending moment on projected length of beams

GL5      -      Intermediate global point load, torque or bending moment on beams

GL6      -      Partial linear varying global load, torque or bending moment on beams

GP6      -      Partial linear varying global load, torque or bending moment on projected length of beams

GL7      -      Partial quadratically varying global load, torque or bending moment on beams

GP7      -      Partial quadratically varying global load, torque or bending moment on projected length of beams

ML1      -      Varying shear load along the edge of membrane and shell elements

ML2      -      Varying normal load on the edge of membrane and shell elements




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-154
ASAS (Non-Linear) User Manual                                                                                  Loading Data


ML3        -       Varying transverse shear load on the edge of membrane and shell elements

CB1        -       Varying distributed load on STF4




The general form of the distributed loads data block is shown below. A detailed description of each type of
distributed load and its parameters are given in the following sections. See Appendix A, element descriptions.

           DISTRIBU                                                            //nodes//


           dof           type              v alues                     ELEM             //elno//


                                                                      EDGE           //edgeno//          ELEM   //elno//

           RP            nrep                 inc

           RRP           nrrep                iinc

           END




Parameters

DISTRIBU :                 compulsory header keyword to denote the start of distributed load data.

dof              : freedom code for the direction of loading.

type             : type of distributed loading to be applied.

values           : values of force and distance to describe the loading. (Real)

nodes            : node numbers to define the loaded elements. (Integer)

ELEM             : keyword to indicate following data are element numbers.

elno             : element numbers to define the loaded elements. (Integer)

EDGE             : keyword to indicate following data is an edge number.

edgeno           : edge number of the element to be loaded. (Integer)

RP               : keyword to indicate the generation of data from the previous / symbol.

nrep             : the number of times the data is to be generated. (Integer)

inc              : node or element number increment to be added each time the data is generated by the RP
                   command. (Integer)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-155
ASAS (Non-Linear) User Manual                                                                             Loading Data


RRP          : keyword to indicate the generation of data from the previous // symbol.

nrrep        : the number of times the data is to be generated. (Integer)

iinc         : node or element number increment to be added each time the data is generated by the RRP
               command. (Integer)




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-156
ASAS (Non-Linear) User Manual                                                                                  Loading Data



Example


To apply a uniformly distributed load (BL1) of 8/unit length in the local Y direction to a BM3D defined by
nodes 15 and 18.

           Y BL1 8.0 8.0 15 18

Notes


1.          For BL, GL and GP type loading, the elements to which the loads relate are defined by the two end nodes.
            If two or more beam elements are defined between the same two nodes (and in the same order), the
            loaded element cannot be uniquely identified and the program will apply the load to the element with the
            lowest user number. If this is not appropriate, the user may overcome this problem in a number of ways.

(i)         Use element number input.

(ii)        Alter the user element numbers.

(iii)      Reverse the order of the element topology and associated loading for the second beam.

(iv)       Subdivide second and subsequent elements into two or more beams.

(v)        Use different node numbering for the two beams and apply constraint equations to join them together.


2.         There is a restriction in the repeat facility where nodal type input and element type input may not be in
           the same repeat block.

3.         The continuation facility is available in both nodal and element type input. However, the first line must
           contain at least two nodes or one element. The continuation line must contain the keywords
           ELEM/EDGE if element type input is being used.

4.         The edge number follows the topology of the element, eg edge 2 is between nodes 2 and 3 of a 4-nodal
           quadrilateral element and edge 3 is between nodes 5 and 1 of a 6-noded triangular element.

Examples


           DISTRIBU
           ML2 10.0 10.0 10.0 EDGE                                1     ELEM       2     3     4
           : EDGE 2 ELEM 5 6 7
           DI STRIBU
           Y     BL6 10.0             10.0 0.0             8.5        ELEM     100       101
           :     ELEM 102             103 104
           DISTRIBU
           Y BL1 5.0                5.0      2     3
           :     3     4
           :     4     5




        Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-157
ASAS (Non-Linear) User Manual                                                                             Loading Data


5.4.6.1 Local Beam Distributed Loads

The local distributed loads on beams (BL types) are applied in terms of the local axis system, with X’ along the
length of the element. A load is +ve when applied to the beam in the +ve direction of the local axis as defined
by the element topology data and geometric property data. For normal loads which are not in a local axis plane,
the appropriate components must be derived.
The Load Patterns BL1, BL2, BL6 and BL7 can be used to apply uniform load as well as linearly varying load.
The Load Pattern BL7 can be used to apply linearly varying load as well as quadratically varying load.
Load pattern BL8 is useful particularly to impose initial strain conditions such as those arising from thermal
loading when nodal temperatures are not appropriate.




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-158
ASAS (Non-Linear) User Manual                                                                                    Loading Data



                       DISTRIBUTED LOAD PATTERNS BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
                                        on BEAM, BM2D, BM3D, TUBE
              BL1                                                          BL2
                         Y”                           Normal                         Y”
                                                                                                          Axial
                                                         X”                                                           X”
                              1                   2                                           1           2
                         Y”                           Bending                        Y”                   Torsion
                              1                           X”                              1                     X”
                                                  2                                                       2

               BL3                                                         BL4
                                                                                     Y”                   Normal
                                                                                              1           2   X”

                                                                                     Y”
                                                                                                          Axial
                         Y”                           Normal                                                          X”
                                                                                          1               2
                                                         X”
                                  1               2                                  Y”
                                                                                                          Bending
                                                                                                               X”
                                                                                          1               2
                                                                                     Y”
                                                                                                           Torsion
                                                                                                                 X”
                                                                                              1           2

               BL5       Y”                                                BL6
                                                   Normal                            Y”                    Normal
                                  1               2    X”
                                                                                                               X”
                                                                                              1           2
                         Y”                                                          Y”
                                                   Axial                                                  Axial
                                  1               2      X”                                                           X”
                                                                                              1           2
                         Y”                                                          Y”
                                                   Bending                                                Bending
                                                        X”                                                     X”
                              1                   2                                           1           2
                         Y”                        Torsion                           Y”                   Torsion
                                                         X”                                                     X”
                                  1               2                                           1           2

               BL7                                                         BL8
                         Y”                       Normal                             Y”                       Normal
                                                      X”                                                          X”
                                  1               2                                           1            2
                         Y”                       Axial                              Y”                       Axial
                                                          X”                                                          X”
                                  1               2                                           1           2
                         Y”                       Bending                            Y”                    Bending
                                                        X”                                1                     X”
                                  1               2                                                       2
                         Y”                       Torsion                            Y”                       Torsion
                                                        X”                                                         X”
                                  1               2                                       1                   2




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-159
ASAS (Non-Linear) User Manual                                                                                 Loading Data



Example of Distributed Load Data for BL Patterns

                                                          34


                                             8



                                                                                 p = 14
                         p = 20                                                                  p = 10
                                                                                                           6
                                         5




                                                   26




                                                                        p = 16

                            p = 15                                                               p = 10
                                                                                                           4
                                         3

                                             9

                                                               38



                                                   2000                             2000




                              p = 10                                                             p = 10
                                         1                                                                 2


Data

  DISTRIBU
  Y       BL1          -10.0         -15.0           1              3
  Y       BL1          -15.0         -20.0           3              5
  /
  Y       BL1          -10.0         -10.0           2              4
  RP       2       2
  Y       BL4          -14.0            8.0        34.0             5     6
  Y       BL4          -16.00           0.0        26.0             3     4
  Y       BL5          -2000            9.0                         3     4
  Y       BL5          -2000           38.00                        3     4
  END




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-160
ASAS (Non-Linear) User Manual                                                                                         Loading Data


5.4.6.1.1         BL1 and BL2 Load Patterns



Distributed Load Pattern BL1 - Linearly varying normal load or moment
              Element          Valid freedom directions              Y”
                                                                                                         Normal
   BEAM                 Y”     Z”      RY”      RZ”                                                            X”
                                                                              1                      2
   BM2D                 Y”                      RZ”
                                                                     Y”
   BM3D                 Y”     Z”      RY”      RZ”                                                      Bending
   TUBE                 Y”     Z”      RY”      RZ”                       1                                    X”
                                                                                                    2




Distributed Load Pattern BL2 - Linearly varying axial load or torque
              Element          Valid freedom directions              Y”

                                                                                                     Axial
   BEAM                 X”     RX”                                                                             X”
                                                                          1                         2
   BM2D                 X”
                                                                     Y”
   BM3D                 X”     RX”                                                                   Torsion
   TUBE                 X”     RX”                                                                             X”
                                                                          1
                                                                                                    2


Data Line
                         BL1                                                            //node1//          //node2//
        dof                              force1           force2
                         BL2                                                            ELEM              //elno//




Parameters

dof             : local freedom code for direction of loading. See list above.

BL1             : load pattern type
BL2

force1          : force/unit length at end 1. (Real)

force2          : force/unit length at end 2. (Real)
node1           : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM            : keyword to indicate following data are element numbers.

elno            : list of element numbers to which this loading applies. (Integer)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-161
ASAS (Non-Linear) User Manual                                                                                     Loading Data


Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.1.2         BL3 Load Pattern



Distributed Load Pattern BL3 - Stepped uniform normal load
               Element         Valid freedom directions              Y”

   BEAM                 Y”     Z”                                                                       Normal

   BM2D                 Y”                                                                                    X”
                                                                          1                         2
   BM3D                 Y”     Z”
   TUBE                 Y”     Z”




Data Line
                                                                                                      //node1//    //node2//
         dof            BL3             force1              force2            dist
                                                                                                        ELEM       //elno//




Parameters

dof             : local freedom code for direction of loading. See list above.

BL3             : load pattern type.

force1          : force/unit length at end 1. (Real)

force2          : force/unit length at end 2. (Real)

dist            : distance to load step from end 1. (Real)

node1           : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM            : keyword to indicate following data are element numbers.


elno            : list of element numbers to which this loading applies. (Integer)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page 5-162
ASAS (Non-Linear) User Manual                                                                                           Loading Data


Notes


(i)        The nodes must be listed in the same order as the element topology data.

(ii)       This loading must not be applied to stepped beams. Apply in two parts using BL4 or BL6 loading.

Example


See Section 5.4.6.1


5.4.6.1.3          BL4 Load Pattern



Distributed Load Pattern BL4 - Uniform normal or axial load, moment or torque
                            over a part of the element
                Element         Valid freedom directions                             Y”
                                                                                                                      Normal
       BEAM              X”     Y”      Z”      RX”      RY”      RZ”                                                           X”
                                                                                          1                       2
       BM2D              X”     Y”                                RZ”                Y”
       BM3D              X”     Y”      Z”      RX”      RY”      RZ”                                                 Axial
                                                                                                                                X”
       TUBE              X”     Y”      Z”      RX”      RY”      RZ”                     1                       2
                                                                                     Y”
                                                                                                                      Bending
                                                                                                                                X”
                                                                                          1                       2
                                                                                     Y”
                                                                                                                      Torsion
                                                                                                                                X”
                                                                                          1                       2



Data Line
                                                                                              //node1//        //node2//
          dof           BL4             force          dist1         dist2
                                                                                              ELEM             //elno//




Parameters

dof              : local freedom code for direction of loading. See list above.

BL4              : load pattern type.

force            : force/unit length. (Real)

dist1            : distance to start of loaded part from end 1. (Real)




       Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                         Page 5-163
ASAS (Non-Linear) User Manual                                                                                           Loading Data


dist2           : distance to finish of loaded part from end 1. (Real)

node1           : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM            : keyword to indicate following data are element numbers.


elno            : list of element numbers to which this loading applies. (Integer)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.1.4         BL5 Load Pattern



Distributed Load Pattern BL5 - Intermediate point load or moment
              Element          Valid freedom directions                            Y”
                                                                                                                    Normal
   BEAM                 X”     Y”      Z”      RX”      RY”      RZ”                    1                          2
                                                                                                                              X”
   BM2D                 X”     Y”                                RZ”               Y”
   BM3D                 X”     Y”      Z”      RX”      RY”      RZ”                                                Axial
   TUBE                 X”     Y”      Z”      RX”      RY”      RZ”                                                          X”
                                                                                        1                          2
                                                                                   Y”
                                                                                                                    Bending
                                                                                                                           X”
                                                                                        1                          2
                                                                                   Y”
                                                                                                                    Torsion
                                                                                                                              X”
                                                                                        1                          2




Data Line
                                                                                            //node1//         //node2//
           dof               BL5             force              dist
                                                                                            ELEM              //elno//




Parameters

dof             : local freedom code for direction of loading. See list above.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                        Page 5-164
ASAS (Non-Linear) User Manual                                                                                     Loading Data


BL5           : load pattern type.

force         : value of the point load or moment. (Real)

dist          : distance to load point from end 1. (Real)

node1         : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM          : keyword to indicate following data are element numbers.


elno          : list of element numbers to which this loading applies. (Integer)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.1.5       BL6 Load Pattern



Distributed Load Pattern BL6 -                     Linearly varying normal or axial load, torque or
                                                   moment over part of the element

                                                                                   Y”
             Element        Valid freedom directions                                                             Normal
                                                                                                                           X”
   BEAM              X”     Y”      Z”      RX”      RY”      RZ”                       1                    2
   BM2D              X”     Y”                                RZ”                  Y”
                                                                                                                 Axial
   BM3D              X”     Y”      Z”      RX”      RY”      RZ”                                                          X”
                                                                                        1                    2
   TUBE              X”     Y”      Z”      RX”      RY”      RZ”
                                                                                   Y”
                                                                                                                 Bending
                                                                                                                           X”
                                                                                        1                    2
                                                                                   Y”
                                                                                                                 Torsion
                                                                                                                           X”
                                                                                        1                    2


Data Line
                                                                                                     //node1//       //node2//
       dof        BL6          force1          force2           dist1         dist2
                                                                                                      ELEM          //elno//




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                        Page 5-165
ASAS (Non-Linear) User Manual                                                                                    Loading Data


Parameters

dof             : local freedom code for direction of loading. See above list

BL6             : load pattern type.

force1          : force/unit length at the start of the loaded part. (Real)

force2          : force/unit length at the end of the loaded part. (Real)

dist1           : distance to the start of the loaded part from end 1. (Real)

dist2           : distance to the finish of the loaded part from end 1. (Real)

node1           : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM            : keyword to indicate following data are element numbers.


elno            : list of element numbers to which this loading applies. (Integer)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.1.6         BL7 Load Pattern



Distributed Load Pattern BL7 - Quadratically varying normal or axial load, torque or
                                                  moment over part of the element
                                                                                      Y”
                                                                                                              Normal
              Element          Valid freedom directions
                                                                                                                        X”
                                                                                           1                  2
   BEAM                 X”     Y”      Z”      RX”      RY”      RZ”                  Y”
                                                                                                              Axial
   BM2D                 X”     Y”                                RZ”
                                                                                                                        X”
   BM3D                 X”     Y”      Z”      RX”      RY”      RZ”                       1                  2
   TUBE                 X”     Y”      Z”      RX”      RY”      RZ”                  Y”
                                                                                                              Bending
                                                                                                                        X”
                                                                                           1                  2
                                                                                      Y”
                                                                                                              Torsion
                                                                                                                        X”
                                                                                           1                  2




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 5-166
ASAS (Non-Linear) User Manual                                                                                        Loading Data




Data Line
                                                                                                          //node1//     //node2//
       dof       BL7         force1         force2         force3        dist1       dist2
                                                                                                          ELEM         //elno//




Parameters

dof             : local freedom code for direction of loading. See list above.

BL7             : load pattern type.

force1          : force/unit length at the start of the loaded part. (Real)

force2          : force/unit length at the centre of the loaded part. (Real)

force3          : force/unit length at the end of the loaded part. (Real)

dist1           : distance to the start of the loaded part from end 1. (Real)

dist2           : distance to the end of the loaded part from end 1. (Real)

node1           : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM            : keyword to indicate following data are element numbers.


elno            : list of element numbers to which this loading applies. (Integer)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.1.7         BL8 Load Pattern



Distributed Load Pattern BL8 - Equal and opposite point loads or moments at either
                               end of beam




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-167
ASAS (Non-Linear) User Manual                                                                                            Loading Data




                                                                                   Y”
              Element          Valid freedom directions                                                           Normal
                                                                                                                           X”
                                                                                          1                       2
   BEAM                 X”     Y”      Z”      RX”      RY”      RZ”               Y”
   BM2D                 X”     Y”                                RZ”                                              Axial
                                                                                                                           X”
   BM3D                 X”     Y”      Z”      RX”      RY”      RZ”                      1                   2
   TUBE                 X”     Y”      Z”      RX”      RY”      RZ”               Y”
                                                                                                                  Bending
                                                                                      1                                    X”
                                                                                                                      2
                                                                                   Y”
                                                                                                                  Torsion

                                                                                        1                                  X”
                                                                                                                      2
Data Line
                                                                      //node1//             //node2//
           dof              BL8               force
                                                                      ELEM                //elno//


Parameters

dof              : local freedom code for direction of loading. See list above.

BL8              : load pattern type.

force            : value of the load or moment. This value of load is applied to the beam (not the node) in an equal
                   and opposite sense at each end of the beam. (Real)

node1            : pairs of node numbers to define the elements to which this loading applies. (Integer)
node2

ELEM             : keyword to indicate following data are element numbers.


elno             : list of element numbers to which this loading applies. (Integer)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.1


5.4.6.2 Global Beam Distributed Loads

The global beam distributed loads (GL and GP types) are similar to the BL load types except that the loading is
applied in terms of the global axis system.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 5-168
ASAS (Non-Linear) User Manual                                                                                   Loading Data


The load for GL type loading is applied to the beam in one of the global directions with the value of loading
defined in terms of load per unit length of the beam element.

For GP type, loading is also applied in global direction but the value of loading is defined in terms of load per
unit length measure in the plane normal to the direction of the load.
                              DISTRIBUTED LOAD PATTERNS GL1, GP1, GL4, GP4, GL5, GL6, GP6,
                                        GL7, and GP7 on BEAM, BM2D, BM3D, TUBE
               GL1                                        Global X         GP1                                 Global X

                                                                 X”                                                   X”
                    Y”                                   2                                                      2
                                                                                Y”


                X        1                                                  X
                                                                                      1

                          Z                                  Global Z                Z                          Global Z

                                                                   X”
                                                             2                                                        X”
                    Y”
                                                                                                                2
                                                                                Y”

                             1
                                                                                     1

               GL4                                                         GP4
                                                          Global X                                             Global X
                                                              X”                                                    X”
                    Y”                                                          Y”
                                                     2                                                     2

                                 1                                                        1
                X                                                           X

                          Z                              Global RZ                   Z                         Global RZ
                                                              X”                                                     X”
                     Y”                              2                           Y”                        2

                                 1                                                        1

               GL5                                        Global X
                                                              X”
                     Y”
                                                     2
                X
                                 1

                          Z                              Global RY
                                                               X”
                     Y”
                                                     2

                                 1




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page 5-169
ASAS (Non-Linear) User Manual                                                                                        Loading Data



                        DISTRIBUTED LOAD PATTERNS GL1, GP1, GL4, GP4, GL5, GL6, GP6,
                                  GL7, and GP7 on BEAM, BM2D, BM3D, TUBE
             GL6                                                       GP6
                                                  Global X                                                 Global X
                                                          X”                                                       X”
                  Y”                                                        Y”
                                                  2                                                        2

              X             1                                           X             1

                                                Global RY                                                 Global RY
                        Z                                                         Z
                                                          X”                                                      X”
                   Y”                             2                         Y”                             2

                            1                                                         1


             GL7                                                       GP7
                                                 Global X                                                  Global X

                                                          X”                                                      X”
                  Y”                                                        Y”
                                                 2                                                         2
              X                                                         X
                        1                                                             1
                                              Global RY                                                   Global RY
                        Z                                                         Z
                                                          X”                                                          X”
                  Y”                             2                           Y”                            2

                        1                                                             1




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-170
ASAS (Non-Linear) User Manual                                                                                      Loading Data




Example


Example of Distributed Global Loads


                                                                                p = 10.0




                                           p = 10.0                                 3                              p = 10.0

                     p = 20.0                                                                                  4
                                                      2

                                                                                                                         5.0




                                                                                                                               p = 17.2




                                                                                    Z

                                                                                                  Y




                                1                                                                          X                              5
          p = 80.0                                                                 Global Axis Sy stem



Data

   DISTRIBU
   X      GP1            80.0       20.0         1        2
   /
   Z      GL1            10.0       10.0         2        3
   RP      2         1
   X      GL5            17.2       5.0      4        5
   END


5.4.6.2.1       GL1 and GP1 Load Patterns




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                       Page 5-171
ASAS (Non-Linear) User Manual                                                                                      Loading Data



Distributed Load Pattern GL1 - Linearly varying Global load or moment
Distributed Load Pattern GP1 - Linearly varying Global Projected load or moment



                                                                                                               GL1 - Global X

                                                                                                                                X”
                                                                                        Y”                              2

              Element          Valid freedom directions
                                                                                             1                GL1 - Global Z
   BM2D                 X      Y                                 RZ                                                             X”
   BM3D                 X      Y       Z       RX       RY       RZ                     Y”                              2
   TUBE                 X      Y       Z       RX       RY       RZ

                                                                           X                 1

                                                                                   Z                          GP1 - Global X


                                                                                                                                X”
                                                                                        Y”                              2



                                                                                             1
                                                                                                               GP1 - Global Z

                                                                                                                                X”
                                                                                         Y”                             2



Data Line                                                                                    1
                            GL1
           dof                                  (lfunno)             force1            force2           //node1//      //node2//
                            GP1



Parameters

dof             : global freedom code for direction of loading. See list above

GL1             : load pattern types
GP1

lfunno          : load function number; required if, and only if, LFUN specified. (Integer)

force1          : force/unit length at end 1. (Real)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-172
ASAS (Non-Linear) User Manual                                                                                          Loading Data


force2          : force/unit length at end 2. (Real)

Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.2.


5.4.6.2.2         GL4 and GP4 Load Patterns



Distributed Load Pattern GL4 - Uniform Global load or moment over a part of the
                                                  element

Distributed Load Pattern GP4                       - Uniform Global Projected load or moment over a part of
                                                                the element
                                                                                                              GL4 - Global X
                                                                                                                     X”
              Element          Valid freedom directions                     Y”
                                                                                                              2
   BM2D                 X     Y                         RZ                         1                          GL4 - Global RZ
   BM3D                 X     Y    Z     RX     RY      RZ                                                           X”
   TUBE                 X     Y    Z     RX     RY      RZ                   Y”                               2
                                                          X
                                                                                   1
                                                                                                              GP4 - Global X
                                                                  Z                                                  X”
                                                                            Y”
                                                                                                              2

                                                                                   1                          GP4 - Global RZ
                                                                                                                     X”
                                                                              Y”                              2

                                                                                   1


Data Line
                             GL4
           dof                                (lfunno)           force         dist1        dist2             //node1//         //node2//
                             GP4



Parameters

dof             : local freedom code for direction of loading. See list above




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                       Page 5-173
ASAS (Non-Linear) User Manual                                                                                    Loading Data


GL4          : load pattern type
               GP4

lfunno       : load function number; required if, and only if, LFUN specified. (Integer)

force        : force/unit length. (Real)

dist1        : distance to start of loaded part from end 1. (Real)

dist2        : distance to finish of loaded part from end 1. (Real)

node1        : element node numbers. (Integer)
node2
Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.2


5.4.6.2.3      GL5 Load Pattern



Distributed Load Pattern GL5 - Intermediate Global point load or moment
                                                                                                             Global X
            Element         Valid freedom directions                                                                 X”
                                                                               Y”
                                                                                                             2
   BM2D              X     Y                         RZ
                                                                                      1                      Global Z
   BM3D              X     Y    Z     RX     RY      RZ
                                                                                                                     X”
   TUBE              X     Y    Z     RX     RY      RZ
                                                                                Y”                           2
                                                             X
                                                                                      1
                                                                                                             Global RY
                                                                     Z                                               X”
                                                                               Y”
                                                                                                             2

                                                                                      1                      Global RZ
                                                                                                                     X”
                                                                                Y”                           2


Data Line                                                                             1



         dof              GL5            (lfunno)             force              dist            //node1//          //node2//




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 5-174
ASAS (Non-Linear) User Manual                                                                                        Loading Data


Parameters

dof             : local freedom code for direction of loading. See list above

GL5             : load pattern type

lfunno          : load function number; required if, and only if, LFUN specified. (Integer)

force           : value of the point load or moment. (Real)

dist            : distance to load point from end 1. (Real)

node1           : element node numbers. (Integer)
node2
Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.2


5.4.6.2.4         GL6 and GP6 Load Patterns


Distributed Load Pattern GL6 - Linearly varying Global load or moment over part of
                               the element

Distributed Load Pattern GP6 - Linearly varying Global Projected load or moment
                                                      over part of the element
                                                                                                              GL6 - Global X
              Element          Valid freedom directions                                                              X”
                                                                               Y”
                                                                                                              2
   BM2D                 X     Y                         RZ
   BM3D                 X     Y    Z     RX     RY      RZ                            1                       GL6 - Global RY
   TUBE                 X     Y    Z     RX     RY      RZ                                                           X”
                                                                                Y”                            2
                                                             X
                                                                                      1
                                                                                                              GP6 - Global X
                                                                     Z                                               X”
                                                                               Y”
                                                                                                              2

                                                                                      1                       GP6 - Global RY
                                                                                                                     X”
                                                                                 Y”                           2

Data Line                                                                             1




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 5-175
ASAS (Non-Linear) User Manual                                                                                            Loading Data



                    GL6
       dof                          (lfunno)        force1         force2        dist1       dist2            //node1//     //node2//
                   GP6

Parameters

dof             : local freedom code for direction of loading. See above list

GL6             : load pattern type
                  GP6

lfunno          : load function number; required if, and only if, LFUN specified. (Integer)

force1          : force/unit length at the start of the loaded part. (Real)

force2          : force/unit length at the end of the loaded part. (Real)

dist1           : distance to the start of the loaded part from end 1. (Real)

dist2           : distance to the finish of the loaded part from end 1. (Real)

node1           : element node numbers. (Integer)
node2
Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.2


5.4.6.2.5         GL7 and GP7 Load Patterns


Distributed Load Pattern GL7 - Quadratically varying Global load or moment over part
                                                      of the element




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-176
ASAS (Non-Linear) User Manual                                                                                       Loading Data



Distributed Load Pattern GP7 - Quadratically varying Global Projected load or moment
                                 over part of the element                 GL7 - Global X
                                                                                                                          X”
              Element          Valid freedom directions                              Y”
                                                                                                                 2

   BM2D                 X     Y                         RZ                                  1                   GL7 - Global RY
   BM3D                 X     Y    Z     RX     RY      RZ                                                             X”

   TUBE                 X     Y    Z     RX     RY      RZ                            Y”                         2
                                                                  X
                                                                                            1
                                                                                                                GP7 - Global X
                                                                          Z                                            X”
                                                                                     Y”
                                                                                                                 2

                                                                                            1                    GP7 - Global RY
                                                                                                                        X”
                                                                                      Y”                         2
Data Line
                                                                                             1
                   GL7
      dof                         (lfunno)       force1 force2             force3          dist1     dist2    //node1//        //node2//
                   GP7



Parameters

dof             : local freedom code for direction of loading. See list above

GL7             : load pattern type
                  GP7

lfunno          : load function number; required if, and only if, LFUN specified. (Integer)

force1          : force/unit length at the start of the loaded part. (Real)

force2          : force/unit length at the centre of the loaded part. (Real)

force3          : force/unit length at the end of the loaded part. (Real)

dist1           : distance to the start of the loaded part from end 1. (Real)

dist2           : distance to the end of the loaded part from end 1. (Real)

node1           : element node numbers. (Integer)
node2
Note


The nodes must be listed in the same order as the element topology data.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-177
ASAS (Non-Linear) User Manual                                                                              Loading Data


Example


See Section 5.4.6.2


5.4.6.3 Panel Edge Distributed Loads

Distributed Load Patterns ML1, ML2 and ML3 can be applied on element types QUM4, QUM8, QUS4, TCS6,
TCS8, TCS9, TRM3, TRM6.



Load Pattern ML1 - Varying axial load along an edge

The load is positive if it acts in the direction of the order of nodes in the element topology data. For QUM8,
TCS6, TCS8, TCS9, TRM6 a quadratic variation of the load is allowed, so linear variation and uniform loading
are also acceptable. For QUS4, QUM4, TRM3 a linear variation of load is allowed, so uniform loading is also
acceptable. For a curved edge, the loading is tangential at any point.




Load Pattern ML2 - Varying normal load along an edge

The load is positive if it acts away from the centre of the element. For QUM8, TCS6, TCS8, TCS9, TRM6 a
quadratic variation of load is allowed, so linear variation and uniform loading are also acceptable. For QUM4,
TRM3, QUS4, a linear variation of load is allowed, so uniform loading is also acceptable. For a curved edge,
the loading is normal to the edge at any point.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-178
ASAS (Non-Linear) User Manual                                                                                 Loading Data



Load Pattern ML3 - Varying Transverse Edge Shear Load

The load is positive if it acts in the positive local Z direction for the element.

For QUM8, TCS6, TCS8, TCS9 and TRM6 a quadratic variation of load is allowed, so linear variation and
uniform loading are also acceptable. For QUM4, QUS4 and TRM3 a linear variation of load is allowed, so
uniform loading is also acceptable. For a curved element the load is always normal to the surface of the element.




Data Line
          ML1
                                                                              //nodes//
          ML2            force1         force2          force3
                                                                            EDGE           //edgeno//       ELEM   //elno//
          ML3



Parameters

ML1           : load pattern types
ML2
ML3

lfunno        : load function number; required if, and only if, LFUN specified. (Integer)

force1        : value of the load/unit length at the first corner node on the edge. (Real)

force2        : value of the load/unit length at the second corner node on the edge. (Real)




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-179
ASAS (Non-Linear) User Manual                                                                             Loading Data


force3       : value of the load/unit length at the mid-side node for QUM8, TCS6, TCS8, TCS9, TRM6. This
               mid-side value must be calculated and given. Any value for low order elements. (Real)

nodes        : element node list of the edge of the element to be loaded. (Integer)

EDGE         : keyword to indicate following data are edge numbers.

edgeno       : edge number of the element to be loaded. (Integer)

ELEM         : keyword to indicate following data are element numbers.

elno         : element numbers to define the loaded elements. (Integer)

Notes


Order of the nodes in element node list

        1.     node number of first corner on the edge

        2.     node number of second corner on the edge

        3.     node number of any other corner on the element


Example


Example of Distributed Load Data for ML Patterns




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-180
ASAS (Non-Linear) User Manual                                                                                       Loading Data




Data

   DISTRIBU
   ML2   -10.0                 -10.0           -10.0          1      3       8
   ML2          -10.0          -10.0           -10.0          6      1       3
   ML2          -15.0          -10.0           -11.0          11     6       8
   ML2          -21.0          -15.0           -18.0          16     11      13
   ML1            -7.0           -7.0           -7.0          13     18      16
   ML1             8.0            8.0            8.0          18     16      11
   END


5.4.6.4 Curved Beam Distributed Loads



Distributed Load Pattern CB1 on element STF4

Normal (freedom Y’s or Z’s), axial (freedom X’s), torsional (freedom RX’s) and bending (freedom RY or RZ)
loads are allowed. The load is applied in terms of the local axis system, with X’ along the length of the element
and Y’ and Z’ as defined in Appendix -A.




Data Line
                                                                                              //nodes//
        dof         CB1           force1             force2              force3
                                                                                              ELEM            //elno//




Parameters

dof             : local freedom code for direction of loading

CB1             : load pattern type




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-181
ASAS (Non-Linear) User Manual                                                                             Loading Data


lfunno       : load function number; required if, and only if, LFUN specified. (Integer)

force1       : value of load/unit length at end 1. (Real)

force2       : value of load/unit length at mid-side node. (Real)

force3       : value of load/unit length at end 2. (Real)

nodes        : element node list. (Integer)

ELEM         : keyword to indicate following data are element numbers.

elno         : list of element numbers to define the loaded elements. (Integer)

Note


The nodes must be listed in the same order as the element topology data.




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-182
ASAS (Non-Linear) User Manual                                                                                     Loading Data



Example



Example of Distributed Load Data for Pattern CB1

                  Y'




                     q=34.4 (uniform)
                                                              43
                                                                                                             48
                                                                                                                        X'
             42



                                                          p=3.3


                  p=6.6


                                                                                                           p=9.9




Data

   DISTRIBU
   X      CB1        -34.4          -34.4          -34.4           42       43       48
   Y   CB1             -6.6           -3.3           -9.9          42       43       48
   END




5.4.7      TEMPERATURE Load Data


5.4.7.1 NODAL Temperature Data

To define the temperature values at node points throughout the structure.




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-183
ASAS (Non-Linear) User Manual                                                                                     Loading Data



                    TEMPERAT


                    GROU                   grpno


                                           temp                          //nodes//


                    RP                     nrep                  inode

                    RRP                    nrrep                 iinode
                    GRES                   sname                 (lc)       isub         (node1)             (node2)

                    END




Parameters

TEMPERAT : compulsory header keyword to denote the start of the nodal temperature data

GROU               : keyword to indicate that the following temperature data applies to a single group

grpno              : group number to which temperature data applies. (Integer)

temp               : temperature value at the nodes. (Real)

nodes              : list of nodes at which the given value of temperature applies. (Integer)

RP                 : keyword to indicate the generation of data from the previous / symbol

nrep               : number of times the data is to be generated. (Integer)

inode              : node increment to be added each time the data is generated by the RP command. (Integer)

RRP                : keyword to indicate the generation of data from the previous // symbol

nrrep              : number of times the data is to be generated. (Integer)

iinode             : node increment to be added each time the data is generated by the RRP command. (Integer)

GRES               : keyword to indicate reading temperatures from the database of a previous thermal analysis

sname              : 4 character structure name where temperature results are to be retrieved from.

Ic                 : user load case number in the thermal analysis. By default, Ic has the same user load case
                      number as that specified in the stress analysis. (Integer)

isub               : the load sub-case number. Default is 0. (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-184
ASAS (Non-Linear) User Manual                                                                               Loading Data


node1              : the lower limit of a node range where results will be transferred. The default value 0 means
                      from the lowest node on structure. (Integer)

node2              : the upper limit of a node range where results will be transferred. The default value 0 means to
                      the highest node on structure. (Integer)

END                : compulsory keyword to denote the end of the temperature data block



Notes


1.      Temperature values are actual temperatures. The thermal loads are calculated due to the difference
        between these and the reference temperatures.

2.      Any missing corner node temperature is taken as the reference temperature.

3.      Mid-side node temperatures, whether specified or not, are always linearly interpolated between adjacent
        corner nodes. For elements without mid-side nodes, the average temperature on element is taken to
        calculate the thermal strain.

4.      Loading due to temperatures and face temperatures is additive at common nodes

5.      Nodal and element temperature data must not be present in the same load set.

6.      If the material properties are temperature dependent, temperature load, if specified, must be present in all
        of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
        temperature should be specified in the data

7.      The following points are concerned with the usage of the GRES command.

        • Temperature results must have been saved in a previous thermal analysis under the same project.

        • It is assumed that all the structural corner nodes have the same node numbers as the thermal model.

        • The node range data node1 and node2 enable certain nodes to be excluded from the stress analysis.
             This facility is useful if non-structural nodes have been used in the thermal model, for example, to
             model ambient temperature in convection or radiation boundaries.

        • It is acceptable to have more than one GRES command in a local case.

        • GRES can be specified together with ordinary nodal temperature data in the same load case.



5.4.7.2 ELEMENT Temperature Data

To define uniform or varying temperatures on elements. See Section 5.4.7.3 for details of uniform element
temperature data and Section 5.4.7.4 for non-uniform element temperatures data.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-185
ASAS (Non-Linear) User Manual                                                                              Loading Data



                  EL TEMPE



                  U                      temp                               elno

                  FIN


                  E                        elno

                  FIN

                  T                      temp                            nodes

                  FIN

                  END




Parameters

EL TEMPE          : compulsory header to denote the start of element temperature data.

U                 : keyword to define data as uniform element temperature.

E                 : keyword to define data as element definition.

T                 : keyword to define data as nodal temperature values.

FIN               : keyword to denote the end of a block of U data, E data, or T data.

END               : compulsory keyword to denote the end of the element temperature data block.


5.4.7.3 UNIFORM Element Temperature Data

To define values of the uniform temperature and the elements to which they apply.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-186
ASAS (Non-Linear) User Manual                                                                               Loading Data




              U                   temp                   //elno//


              RP                  nrep                     ielno

              RRP                 nrrep                    iielno

              FIN




Parameters

U              : keyword to define uniform temperature data.

temp           : value of the uniform temperature. (Real)

elno           : list of user element numbers to which the uniform temperature is applied. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

ielno          : user element number increment to be added each time the data is generated by the RP command.
                  (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iielno         : user element number increment to be added each time the data is generated by the RRP command.
                  (Integer)

FIN            : keyword to denote the end of the uniform temperature data block.



5.4.7.4 NON-UNIFORM Element Temperature Data

To define non-uniform temperature on elements. An element can have a different value of temperature at each
node. The data required is a set of element (E) definitions followed by a set of nodal temperature values (T).
Mid-side temperatures are always linearly interpolated between the adjacent corner nodes.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-187
ASAS (Non-Linear) User Manual                                                                               Loading Data



ELEMENT Data

To define the elements to which non-uniform temperature is to be applied. This data must be followed by a list
of nodal temperature values.


             E                 //elno//


             RP                  nrep                      ielno

             RRP                 nrrep                     iielno

             FIN




Parameters

E              : keyword to define element data.

elno           : list of user element numbers to which the non-uniform temperature is applied. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

ielno          : user element number increment to be added each time the data is generated by the RP command.
                 (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iielno         : user element number increment to be added each time the data is generated by the RRP command.
                 (Integer)

FIN            : keyword to denote the end of set of element definitions.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-188
ASAS (Non-Linear) User Manual                                                                               Loading Data



TEMPERATURE Data

To define the nodal temperature values which are to be applied to the previously defined set of elements.


             T                    temp                   //nodes//


             RP                  nrep                      inode

             RRP                 nrrep                     iinode

             FIN




Parameters

T              : keyword to denote nodal temperature data

temp           : value of the temperature at the nodes. (Real)

nodes          : the nodes to which the temperature is applied. These nodes must exist on the elements defined by
                 the preceding set of element definitions. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment. (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment. (Integer)

FIN            : keyword to denote the end of a nodal temperature block.

Notes


1.      To define a region of non-uniform element temperature, a set of one or more elements is defined. The set
        of element data is terminated by a FIN keyword. This is immediately followed by a set of nodal
        temperature values which must be sufficient to completely define the temperature field over the selected
        elements. The nodal temperature data is also terminated by a FIN keyword, unless it is the final set in
        which case it is terminated by an END keyword.

2.      Regions of uniform element temperature and non-uniform element temperature may be mixed in any
        order.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-189
ASAS (Non-Linear) User Manual                                                                                        Loading Data


3.        Unspecified corner node temperatures are taken as the reference temperature.

4.        Mid-side node temperatures, whether specified or not, are always linearly interpolated between adjacent
          corner nodes. For elements without mid-side nodes, the average element temperature is taken to calculate
          the thermal strain.

5.        Loading due to element temperature and element face temperature are additive.

6.        If temperature is defined more than once on an element the loadings will be additive.

7.        Nodal and element temperature data must not be present in the same load set.

8.        If the material properties are temperature dependent, temperature load, if specified, must be present in all
          of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
          temperature should be specified in the data.

Example


In this example 5 BM3D elements are given element temperature values. Elements 11 and 12 have a constant
temperature of 50°, element 13 varies from 50° to 75°, element 14 varies from 75° to 100° and element 15 varies
from 50° to 25°.

                                                                                                             100
                                                                                     75
                                                                                                                 50
     T=50                      50                         50


                                                                                                                               25

                  11                        12                         13                         14

      1                          2                         3                          4                      5                  6



     EL TEMPE
     /
     U       50.0   1
     RP       2   1
     FIN
     /
     E       13
     RP       2        1
     FIN
     T       50.0          3
     T       75.0          4
     T      100.0          5
     FIN
     E   15
     FIN




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-190
ASAS (Non-Linear) User Manual                                                                               Loading Data


     T      50.0         5
     T      25.0         6
     END




5.4.8        FACE TEMPERATURE Data


5.4.8.1 Nodal Face Temperature

To define temperature gradients through plate and shell elements in terms of face temperatures at node points
throughout the structure.
                   FACE TEM


                   GROU                  grpno


                                         temp1               temp2                     //nodes//

                   RP                    nrep                inode

                   RRP                   nrrep               iinode

                   END



Parameters

FACE TEM           : compulsory header to denote the start of nodal face temperature data

GROU               : keyword to indicate that the following face temperature data applies to a single group

grpno              : group number to which face temperature data applies. (Integer)

temp1              : temperature value on face 1. (Real)

temp2              : temperature value on face 2. (Real)

nodes              : list of nodes at which the face temperatures apply. (Integer)

RP                 : keyword to indicate data generation from the previous / symbol

nrep               : number of times the data is to be generated. (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-191
ASAS (Non-Linear) User Manual                                                                               Loading Data


inode              : node increment to be added each time the data is generated by the RP command. (Integer)

RRP                : keyword to indicate data generation from the previous // symbol

nrrep              : number of times the data is to be generated. (Integer)

iinode             : node increment to be added each time the data is generated by the RRP command. (Integer)

END                : compulsory keyword to denote the end of the face temperature data block

Notes


1.      The position of Face 1 and Face 2 for each element is defined in the element description sheets in
        Appendix -A.

2.      Since face temperatures are applied to all elements attached to the given nodes within the specified group,
        care must be taken to ensure the consistent use of local axes on adjacent elements.

3.      Loading due to temperature and face temperature are additive.

4.      Nodal and element face temperature data must not be present in the same load set

5.      Notes for temperature data also apply here.

6.      If the material properties are temperature dependent, temperature load, if specified, must be present in all
        of the runs (i.e. initial and restarts). If any run does not have face temperature load, then the reference
        temperature should be specified as the top and bottom surface temperatures in the data.


5.4.8.2 ELEMENT FACE TEMPERATURE Data

To define uniform or varying face temperatures on elements. See Section 5.4.8.3 for details of uniform element
face temperature data and Section 5.4.8.4 for non-uniform element face temperature data.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-192
ASAS (Non-Linear) User Manual                                                                              Loading Data



                   EL FACET



                   U                    temp1                temp2                    elno


                   FIN



                   E                    elno


                   FIN

                   T                    temp1                temp2                    nodes

                   FIN

                   END




Parameters

EL FACET          : compulsory header to denote the start of element face temperature data.

U                 : keyword to define data as uniform face temperature.

E                 : keyword to define data as element definition.

T                 : keyword to define data as nodal face temperature values.

FIN               : keyword to denote the end of a block of U data, E data, or T data.

END               : compulsory keyword to denote the end of the element face temperature data block.


5.4.8.3 UNIFORM Element Face Temperature Data

To define values of the uniform face temperatures and the element faces to which they are applied.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-193
ASAS (Non-Linear) User Manual                                                                               Loading Data




              U                   temp1                    temp2                 //elno//


              RP                  nrep                                             ielno

              RRP                 nrrep                                            iielno

              FIN




Parameters

U              : keyword to define uniform face temperature data.

temp1          : temperature value on face 1. (Real)

temp2          : temperature value on face 2. (Real)

elno           : list of user element numbers to which the uniform face temperature is applied. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

ielno          : user element number increment to be added each time the data is generated by the RP command.
                  (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iielno         : user element number increment to be added each time the data is generated by the RRP command.
                  (Integer).

FIN            : keyword to denote the end of the uniform face temperature data block.



5.4.8.4 NON-UNIFORM Element Face Temperature Data

To define non-uniform face temperature on elements. An element can have a different value of face temperature
at each node. The data required is a set of element (E) definitions followed by a set of nodal temperature values
(T) on element faces. Mid-side face temperatures are always linearly interpolated between adjacent corner
nodes.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-194
ASAS (Non-Linear) User Manual                                                                               Loading Data



ELEMENT Data

To define the element faces to which non-uniform face temperature is to be applied. This data must be followed
by a list of nodal face temperature values.


             E                  //elno//


             RP                   nrep                                             ielno

             RRP                  nrrep                                            iielno

             FIN




Parameters

E              : keyword to define element data.

elno           : list of user element numbers to which the non-uniform face temperature is applied. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

ielno          : user element number increment to be added each time the data is generated by the RP command.
                 (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iielno         : user element number increment to be added each time the data is generated by the RRP command.
                 (Integer)

FIN            : keyword to denote the end of set of element definitions.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-195
ASAS (Non-Linear) User Manual                                                                               Loading Data



FACE TEMPERATURE Data

To define the nodal face temperature values which are to be applied to the previously defined set of elements.


              T                   temp1                 temp2                    //nodes//


              RP                  nrep                                             inode

              RRP                 nrrep                                            iinode

              FIN




Parameters

T              : keyword to denote nodal face temperature data.

temp1          : temperature value on face 1. (Real)

temp2          : temperature value on face 2. (Real)

nodes          : the nodes to which the face temperature is applied. These nodes must exist on the elements
                  defined by the preceding set of element definitions. (Integer)

RP             : keyword to indicate data generation from the previous / symbol.

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment. (Integer)

RRP            : keyword to indicate data generation from the previous // symbol.

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment. (Integer)

FIN            : keyword to denote the end of a nodal face temperature block.

Notes


1.      To define a region of non-uniform face temperature, a set of one or more elements is defined. The set of
        element data is terminated by a FIN keyword. This is immediately followed by a set of nodal face
        temperature values which must be sufficient to completely define the temperature field over the selected
        elements. The nodal face temperature data is also terminated by a FIN keyword, unless it is the final set
        in which case it is terminated by an END keyword.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-196
ASAS (Non-Linear) User Manual                                                                                  Loading Data


2.        Regions of uniform and non-uniform face temperature may be mixed in any order.

3.        The position of Face 1 and Face 2 for each element is defined in the element description sheets in
          Appendix A.

4.        Care must be taken to ensure the consistent use of local axes on adjacent elements because the definitions
          of Face 1 and Face 2 are local axes dependent.

5.        Unspecified values for element corner nodes are taken as the reference temperature. Mid-side node
          temperatures, whether specified or not, are always linearly interpolated between adjacent corner nodes.
          For elements without mid-side nodes, the average temperature on each face is taken to calculate the
          thermal strain.

6.        Loading due to temperatures and face temperatures are additive.

7.        If face temperature is defined more than once on an element, the loading will be additive.

8.        Nodal face temperature and element face temperature data must not be present in the same load set.

9.        If the material properties are temperature dependent, temperature load, if specified, must be present in all
          of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
          temperature should be specified as the top and bottom surface temperatures in the data.

Example


Uniform Element Face Temperature on 4 elements




                    1                 2                3                 4                temperature on face 1 = 100.0
                                                                                          temperature on face 2 = 50.0




     EL FACET
     /
     U      100.0           50.0          1
     RP      4    1
     END




5.4.9        BODY FORCE Data

To define forces due to linear acceleration of the structure, arising from the mass of the elements and added
masses. Only one body force loading may be defined per load set.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-197
ASAS (Non-Linear) User Manual                                                                               Loading Data




           BODY FOR

                               x-acc                y-acc              z-acc

           END




Parameters

BODY FOR : compulsory header keyword to denote the start of body force data

x-acc              : values of acceleration in the direction of the three global axes. (Real)
y-acc
z-acc

END                : compulsory keyword to denote the end of the body force data block

Notes


1.      A +ve acceleration produces +ve forces along the corresponding axis. Thus if the vertical global axis is
        positive upwards, a negative value of ‘g’ is required to generate self weight.

2.      Non-zero values of density must be included for any materials used for elements whose mass is to be
        included in the calculation of the body forces.

3.      Accelerations must be input in units (Length/Time2) consistent with those used for length and density.

Example


An example of a body force load set.

        BODY        FOR
        0.0       10.5       32.2
        END




5.4.10       CENTRIFUGAL Loads Data

To define forces due to uniform rotation about a given point, arising from the mass of the elements and added
mass. Only one centrifugal loading may be defined per load set.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-198
ASAS (Non-Linear) User Manual                                                                                       Loading Data




           CENTRIFU

                               xc            yc            zc            x-vel              y-vel            z-vel

           END




Parameters

CENTRIFU           : compulsory header keyword to denote the start of the centrifugal load data

xc                 : global coordinates of the centre of rotation of the structure. (Real)
yc
zc

x-vel              : values of angular velocity in radians/sec about the the three global axes. (Real)
y-vel
z-vel

END                : compulsory keyword to denote the end of the centrifugal load data block

Note


Non-zero values of density must be included for any materials used for elements whose mass is to be included in
the calculation of the centrifugal forces.

Example


An example of a centrifugal load case.

        CENTRIFU
        17.3        103.0        96.5       0.134         0.53       0.05
        END




5.4.11       ANGULAR ACCELERATION Loads Data

To define forces due to angular velocity and angular acceleration about a given point, arising from the mass of
the elements and added masses. Only one angular acceleration loading may be defined per load set.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-199
ASAS (Non-Linear) User Manual                                                                                   Loading Data




       ANG ACCE

                        xc        yc       zc        x-acc          y-acc        z-acc           (x-vel      y-vel   z-vel)

        END




Parameters

ANG ACCE : compulsory header keyword to denote the start of the angular acceleration data

xc,yc,zc           : global coordinates of the centre of rotation of the structure. (Real)

x-acc              : values of angular acceleration in radians/sec2 about the three global axes. (Real)
y-acc
z-acc

x-vel              : values of angular velocity in radians/sec about the three global axes. If omitted zero is
y-vel                 assumed. (Real)
z-vel

END                : compulsory keyword to denote the end of the angular acceleration data block

Notes


1.      Non-zero values of density must be included for any materials used for elements whose mass is to be
        included in the calculation of angular acceleration forces.

2.      Element forces due to angular accelerations are based on the total mass of an element subject to the
        velocities and accelerations pertaining at the centroid of that element. Therefore large elements
        positioned close to the centre of rotation can produce significant discretisation errors.

3.      The sign convention for angular accelerations is such that input of a positive clockwise acceleration will
        produce element forces acting in a counter-clockwise direction. Note, this convention is different to the
        body force convention where a positive input value produces element forces in the positive direction.

Example


An example of an angular acceleration load case.

        ANG       ACCE
        15.9        0.0      -17.6        0.16        0.02       0.0      0.23        -0.07        0.0
        END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-200
ASAS (Non-Linear) User Manual                                                                                Loading Data


5.4.12        NODAL FLUX Data

To define the application of nodal fluxes to the structure. This load type may only be specified in a HEAT
analysis.

            NODAL FL

            dof                                     load                //nodelist//


            RP               nrep             inode

            RRP              nrrep            iinode

            END




Parameters

NODAL FL            : compulsory header keyword to denote the start of nodal flux data

dof                 : freedom name. Must be T

load                : value of nodal load. (Real)

nodelist            : list of the node numbers which are being loaded. (Integer)

RP                  : keyword to indicate the generation of data from the previous / symbol

nrep                : the number of times the data is to be generated. (Integer)

inode               : node number increment to be added each time the data is generated by the RP command.
                       (Integer)

RRP                 : keyword to indicate the generation of data from the previous // symbol

nrrep               : the number of times the data is to be generated. (Integer)

iinode              : node number increment to be added each time the data is generated by the RRP command.
                       (Integer)

END                 : compulsory keyword to denote the end of the nodal load data for this load case

Note


If the same node and freedom are loaded more than once in the nodal flux data for a load case, the fluxes are
additive.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-201
ASAS (Non-Linear) User Manual                                                                                Loading Data


Example


An example of a single load set consisting only of nodal fluxes. A point flux of 25.0 is applied at all nodes from
1 to 150.

     LOAD       1
     SET   100                1.0          ’TO GENERATE 150 NODAL FLUXES’
     NODAL FL
     //
     /
     T       25.0 1
     RP       10 1
     RRP        15      10
     END




5.4.13        PRESCRIBED Field Variable Data

To define the field variable values to be applied in this load case to those freedoms declared as prescribed
freedoms in the Boundary Condition data (see Section 5.3.4).

              PRESCRIB

                dof                                  prv al                 //nodelist//


              RP               nrep             inode

              RRP              nrrep            iinode

              END




Parameters

PRESCRIB             : compulsory header keyword to denote the start of prescribed freedoms data

dof                  : freedom name. Must be T

prval                : value of prescribed field variable. (Real)

nodelist             : list of the node numbers to which the prescribed field variable is to be applied. (Integer)

RP                   : keyword to indicate the generation of data from the previous / symbol

nrep                 : the number of times the data is to be generated. (Integer)




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-202
ASAS (Non-Linear) User Manual                                                                               Loading Data


inode              : node number increment to be added each time the data is generated by the RP command.
                      (Integer)

RRP                : keyword to indicate the generation of data from the previous // symbol

nrrep              : the number of times the data is to be generated. (Integer)

iinode             : node number increment to be added each time the data is generated by the RRP command.
                      (Integer)

END                : compulsory keyword to denote the end of prescribed freedoms data



Notes


1.      All freedoms used in the prescribed field variables data must have been defined in the prescribed
        freedoms data (see Section 5.3.4).

2.      In any load case, a prescribed field variables is set to zero if it is not assigned a value and in this case a
        suppression is assumed for this freedom.

Examples


An example of prescribed field variable data for two loadcases. In case 1, both nodes are given equal values. In
case 2, node 15 is given a value of zero.

     LOAD 2
     SET     1     1.0       ’EQUAL TEMPERATURE OF 5’
     PRESCRIB
     T 5.0 10
     T 5.0         15
     END
     SET     2     2.0       ’NODE 10 = 5 DEG, NODE 15 = ZERO’
     PRESCRIB
     T 5.0 10
     T 0.0         15
     END
     STOP




5.4.14       FLUX DENSITY Data

To define uniform or varying flux density applied to the faces of panel or solid elements, or generated within an
element. This load type may only be specified in a HEAT analysis.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-203
ASAS (Non-Linear) User Manual                                                                                          Loading Data




                   FLUX DEN


                   V                                                      fden                          //nodes//

                   FIN



                   E                    //nodes//



                   FIN

                   D                                                      fden                              //nodes//


                   FIN


                   END




Parameters

FLUX DEN          : compulsory header keyword to denote the start of pressure load data

V                 : keyword to define data as uniform flux density

E                 : keyword to define data as face or element definition

D                 : keyword to define data as nodal flux density values

FIN               : keyword to denote the end of a block of V data, E data or D data

END               : compulsory keyword to denote the end of the pressure load data block


5.4.14.1.1 UNIFORM Flux Density Data

To define values of the uniform flux density and the elements or element faces to which they are applied.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-204
ASAS (Non-Linear) User Manual                                                                                 Loading Data




              V                                                      fden                          //nodes//


              RP                    nrep                             inode

              RRP                   nrrep                            iinode

              FIN




Parameters

V              : keyword to define uniform flux density data

fden           : value of the uniform flux density. (Real)

nodes          : the elements or element faces to which the uniform flux density is applied. An element is defined
                  by up to 4 corner nodes. A face of an element is defined by up to 3 corner nodes. (Integer)

RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment to be added each time the data is generated by the RP command.
                  (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment to be added each time the data is generated by the RRP command.
                  (Integer)

FIN            : keyword to denote the end of the uniform flux density data block

Notes


1.      For surface flux, a face of a brick is defined by any 3 corner nodes on the face. For TMT6, QMT8, TXT6
        and QXT8, a face is an edge defined by the 3 nodes forming the loaded edge. For TMT3, QMT4, TXT3
        and QXT4, a face is an edge defined by the two nodes forming the loaded edge. Here flux density is
        defined as flux per unit area.

2.      For internal flux, a brick element is defined by any 4 corner nodes on the element. The nodes must not all
        lie on one face. For membrane or axisymmetric solid field elements, an element is defined by any 3




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-205
ASAS (Non-Linear) User Manual                                                                               Loading Data


         corner nodes on it. The nodes must not all lie on one edge, however. Here flux density is defined as flux
         per unit volume.

3.       If both surface and internal fluxes are present, they must be defined in separate data blocks.


5.4.14.1.2 NON-UNIFORM Flux Density Data

To define non-uniform flux density on elements or element faces. An element or a face can have a different
value of flux density at each node. The data required is a set of element or face (E) definitions followed by a set
of flux density values (D). Unspecified mid-side node flux densities are interpolated between adjacent corner
nodes.

ELEMENT/FACE Data

To define the elements or element faces to which non-uniform flux density is to be applied. This data must be
followed by a list of nodal flux density values.


              E                   //nodes//


              RP                     nrep                            inode

              RRP                    nrrep                           iinode

              FIN




Parameters

E              : keyword to define element/face data

nodes          : the elements or element faces to which the non-uniform pressure is applied. An element is defined
                  by up to 4 corner nodes. A face is defined by up to 3 corner nodes (see Notes 3 and 4 in Flux
                  Density Data). (Integer)

RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment to be added each time the data is generated by the RP command.
                  (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-206
ASAS (Non-Linear) User Manual                                                                             Loading Data


iinode       : node number increment to be added each time the data is generated by the RRP command.
               (Integer)

FIN          : keyword to denote the end of set of element/face definitions




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-207
ASAS (Non-Linear) User Manual                                                                                 Loading Data



FLUX DENSITY Data

To define the nodal flux density values which are to be applied to the previously defined set of elements or
element faces.


              D                                                      fden                          //nodes//


              RP                     nrep                            inode

              RRP                    nrrep                           iinode

              FIN




Parameters

D              : keyword to denote nodal flux density data

fden           : value of the flux density at the nodes. (Real)

nodes          : the nodes to which the flux density is applied. These nodes must exist on the elements/faces
                  defined by the preceding set of element/face definitions. (Integer)

RP             : keyword to indicate the generation of data from the previous / symbol

nrep           : the number of times the data is to be generated. (Integer)

inode          : node number increment. (Integer)

RRP            : keyword to indicate the generation of data from the previous // symbol

nrrep          : the number of times the data is to be generated. (Integer)

iinode         : node number increment. (Integer)

FIN            : keyword to denote the end of a nodal flux density block

Notes


1.      To define a region of non-uniform pressure, a set of one or more elements or element faces is defined.
        The set of element/face data is terminated by a FIN keyword. This is immediately followed by a set of
        nodal flux density values which must be sufficient to completely define the flux density field over the
        selected elements/faces. The nodal flux density data is also terminated by a FIN keyword, unless it is the
        final set in which case it is terminated by an END keyword.

2.      Regions of uniform flux density and non-uniform flux density may be mixed in any order.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-208
ASAS (Non-Linear) User Manual                                                                               Loading Data


3.      For surface flux, a face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For
        TXT6 and QXT8 a face is defined by the 3 nodes forming the loaded edge. For TXT3 and QXT4 a face
        is defined by the two nodes forming the loaded edge and any other node on the element. Here, the flux
        density has unit flux per unit area.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-209
ASAS (Non-Linear) User Manual                                                                                     Loading Data



4.      For internal flux, a brick element is defined by any 4 corner nodes on the element. The nodes must not all
        lie on one face. For membrane or axisymmetric solid field elements, an element is defined by any 3
        corner nodes on it. The nodes must not all lie on one edge, however. Here the flux density has unit flux
        per unit volume.

5.      If both surface and internal fluxes are present, they must be defined in separate data blocks.

Examples


Two Uniform Flux Densities are to be applied, a surface flux density of 10 over edge 1-2-3, and an internal flux
density of 20 over volume covered by 3-4-5-10-9-8. The following lines will generate the data.
                                                     8                 9                  10
                                   7
                   6


                                                                               dv = 20               dv = 20




                     1                          2                         3                  4                 5

                                           ds = 10




        FLUX DEN
        * SURFACE FLUXES
        V     10.0        1    2
        V     10.0 2 3
        *     FIN TO SEPARATE SURFACE AND VOLUME FLUX DATA
              FIN
        *     EXAMPLE OF GENERATING FLUXES ON SEVERAL FACES
        *     INTERNAL GENERATED FLUXES
        /
        V     20.0        3    4     9
        RP 2          1
        END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-210
ASAS (Non-Linear) User Manual                                                                                              Loading Data


Example of a non-uniform flux density on an element. The program will assign a flux density of 7.5 to node 2
and 11.0 to node 4 by interpolation between the adjacent corner nodes.
                                                                                                       6                               5
       FLUX DEN                                                                7                                        d = 12
                                                                                    d=5               d = 10
       E 1        5    7
       FIN
       D     5.0       1       7    8                                                                                             4
                                                                             8 d=5
       D    10.0       3       6
       D 12.0          5
       END                                                                          d=5                        d = 10
                                                                                1                 2                     3

Example of a complete block of flux density data for uniform and non-uniform volume flux densities
                        dd = 20               20
                                                                                                        15
                                                                10                  10
                                                                                                                              5



                               13                 14               15                    16                    17                 18


                               7                  8                  9                   10                    11                 12




                           1                  2                  3                   4                     5                  6




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                               Page 5-211
ASAS (Non-Linear) User Manual                                                                               Loading Data


        FLUX DEN
        V 20.0 1                  2        8
        V 20.0            7       8       14
        FIN
        //
        /
        E       2     3       9
        RP 2          6
        RRP 3         1
        FIN
        D 20.0            2           8    14
        D     10.0        3           9    15   4   10     16
        D 15.0            5       11       17
        FIN
        /
        V       5.0       5           6    12
        RP      2     6
        END




5.4.15       WAVE LOAD Data


             WAVE LOA


             data


             END




Parameters

WAVE LOA : compulsory keyword to denote start of the wave data

data                : wave load data (see Appendix -M for detailed descriptions)

END                 : compulsory keyword to denote end of the wave data

Notes


1.      Wave load data should not be defined more than once in the entire load deck. The loading specified will
        be applied to all load sets.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-212
ASAS (Non-Linear) User Manual                                                                                      Loading Data


2.      The wave loading generated cannot be scaled using any of the load history types. The LFUN command
        in the wave load data should be used instead to associate the loading with a load function.

3.      SOLU procedure cannot be used when wave load is present.

4.      If modification of wave environment is required during an analysis, this can be achieved by restart with
        modified wave data supplied.




5.4.16       TANK LOAD data

To define pressure loading on the tank walls due to action of the fluid inside a tank. The specified tank load data
will be converted to pressure loads by the programe internally.

                TANK LOAD

                ACCN             xtrans          ytrans           ztrans            xrot        yrot         zrot

               setname              elno            inface            elev         denfl


                END




Parameters

TANK LOAD             :        compulsory header to denote the start of tank load data

ACCN               : command keyword to denote the start of tank acceleratio data. The accelerations will apply to
                      all following sets until antoher ACCN command is encountered.

xtrans             : Translational acceleration in global X direction (Real)

ytrans             : Translational acceleration in global Y direction (Real)

ztrans             : Translational acceleration in global Z direction (Real)

xrot               : Rotational acceleration about the global X axis (Real)

yrot               : Rotational acceleration about the global Y axis (Real)

zrot               : Rotational acceleration about the global Z axis (Real)

setname            : ASAS set name containing elements forming the tank (up to 8 characters)

elno               : User element number of an element in tank with known internal surface (Integer)




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-213
ASAS (Non-Linear) User Manual                                                                                Loading Data


inface              : Internal fact indicator for element elno (Integer)
                       1        +ve local z side is internal
                       -1       -ve local z side is internal

elev                : Z elevation of fluid surface in tank (Real)

denfl               : fluid density (Real)

END                 : compulsory keyword to denote the end of the tank load data block

Notes


1.       Both pressure and tank load data can appear in the same load case.

2.       Accelerations of the tank structure are required in the ACCN data and these are equal and opposite to
         those experienced by the fluid. It is assumed that the accelerations for the whole tank are uniform and
         given by the accelerations at the centre of gravity position of the fluid in the tank.

3.       The accelerations specified in an ACCN data will apply to all sets that follow the command until another
         ACCN command is encountered.

4.       A positive gravitational acceleration must be added to the Z acceleration data (ztrans) in order to include
         the effect of gravity. It is assumed that gravity always acts in the global Z direction.

5.       Fluid surface is assumed to remain still, i.e. sloshing effect is ignored.

6.       Tank load can only be applied to shell and membrane elements as stated in Appendix A. All other
         element types in the set will be ignored.

7.       Tank pressure loads will only be calculated for the wetted nodes (i.e. nodes that are on or below the fluid
         surface elevation elev).

8.       A warning will be given if the element set does not form a proper tank shape. Pressure loads will still be
         calculated for the elements and this will enable the application of tank loading to other modelling
         situations, e.g. applying hydostatic pressure to a wall.

9.       Each tank should only contain elements that form the surface of the tank (i.e. those that will be subjected
         to internal pressure). Any stiffeners modelled by shell elements must be excluded from the tank set or
         else pressure will be incorrectly applied to them. An error will be reported if a branched surface is
         encountered.

10.      The tank surface must be continuous. A warning will be given if a discontinuity is encountered and only
         the part containing the first element will have pressure loading applied.

Example


Tank load on set ABCD, hydrostatic pressure only.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-214
ASAS (Non-Linear) User Manual                                                                                    Loading Data


         TANK LOAD
         ACCN       0.0      0.0      9.81 0.0          0.0       0.0
         ABCD       100      1 20.0 1025.0
         END




5.4.17     LOAD Functions

The load functions must follow all other other loading data.

Load functions provide a method for applying non-proportional loads. Two basic types are available; piecewise
linear and continuous. The piecewise linear type is defined as a series of ‘time-factor’ pairs. The value of the
load at time ‘time’ is the reference load multiplied by the value of ‘factor’. The continuous load function types
are defined in terms of mathematical functions. The value of the load at time ‘time’ is the reference load
multiplied by the value of the function. Load functions must not be used if pseudo-times have been used in
specifying the loading.
                 LOAD-FUN


                  lfunno                 time              factor



                                         SINU              A            w         p         (t1)       (t2)


                  lfunno                 EXPO              a            b                   (t1)       (t2)


                                         POLY              c            d         e          f             (t1)   (t2)

                                         RAOS              (t1)         (t2)
                  END




Parameters

LOAD-FUN         : compulsory header keyword to denote the start of the load function data

lfunno           : load function number. This corresponds to the load set number specified in the loading data.
                   (Integer)

time             : time. (Real)

factor           : multiplying factor for load at time time. (Real)

SINU             : keyword to denote continuous sinusoidal load function

A,w,p            : constants in the expression Asin(wt + p) where t is time. (Real). Note: (wt + p) is in radians




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-215
ASAS (Non-Linear) User Manual                                                                                Loading Data


t1                  : time to start ramping up the load function (Real)

t2                  : time to finish ramping up the load function (Real)

EXPO                : keyword to denote continuous exponential load function

a,b                 : constants in the expression ae-bt where e is the base of the natural logarithm and t is time. (Real)

POLY                : keyword to denote continuous polynomial load function

c,d,e,f             : constants in the expression ct2 + dt3 + et4 + ft5 where t is time. (Real)

RAOS                : keyword to denote a RAO load function

END                 : compulsory keyword to denote the end of the load function data

Notes


1.       Times must be in ascending order within each load function definition.

2.       Any number of lines may be used to identify a load function defined by time-factor pairs.

3.       The times in the list time do not have to be identical to the list of times specified with the SOLV
         command. In such cases linear interpolation is used to calculate load multipliers corresponding to each
         time specified with the SOLV command.

4.       Non-proportional loading cannot be used in conjunction with special solution techniques as defined by
         the SOLU command.

5.       All constants (except the optional parameters t1 and t2) must be specified when using the continuous load
         function types SINU, EXPO and POLY.

6.       For the special load function types, the load factor applied will be scaled by a ramping factor R. This
         factor takes the following value:

         R = 0.0                    if t < t1
         R = (t-t1) / (t2-t1) if t1 ≤ t ≤ t2
         R = 1.0                    if t > t2
         R = 1.0 if both t1 and t2 are not specified




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 5-216
ASAS (Non-Linear) User Manual                                                                          Additional Mass Data



5.5     DIRECT Mass Input Data

To define mass on the structure in addition to that implied by the elements. The direct mass data consists of one
Direct Mass input header, followed by the mass data. The data consists of an input type header followed by the
appropriate data.


            DIRE


            LUMP                 ADDED MA

            (mtype)                mass                   dof                nodes

             END




Parameters

DIRE          : compulsory header keyword to denote the start of the Direct Mass data

LUMP          : keyword for lumped added mass input

END           : compulsory keyword to denote the end of each block of Direct Mass data




5.5.1       UNITS command

If global units have been defined using the UNITS command in the Preliminary Data (see Section 5.1.42), it is
possible to override the input units locally by the inclusion of UNITS command. The local units are only
operational for the data block concerned and will return to the default global units when the next END command
is encountered.

One or more UNITS commands may appear in a data block thus permitting the greatest flexibility in data input.
The form of the command is similar to that used in the Preliminary Data.

          UNITS                        unitnm




Parameters

UNITS         : keyword

unitnm        : name of unit to be utilised (see below)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-217
ASAS (Non-Linear) User Manual                                                                          Additional Mass Data


Notes


1.      The mass unit is not defined explicitly, but is derived from the force and length unit currently defined. In
        order to determine the consistent mass unit the force and length terms must both be either metric or
        imperial. Valid combinations are shown in Table 3.1.

2.      Force, length, and angular unit may be specified. Only those terms which are required to be modified
        need to be specified, undefined terms will default to those supplied on the global units definition unless
        previously overwritten in the current data block.

3.      For a list of valid unit names see Section 5.1.42.1.




5.5.2       LUMP ADDED MASS Data

To define the lumped mass input.

            LUMP                   ADDED MA

            (mtype)                 mass                  dof                //nodes//

            RP                     nrep               inode

            RRP                    nrrep              iinode

            END




Parameters

LUMP              : compulsory header keyword to denote the start of lumped mass data

ADDED MA             :        keyword to define that the following mass terms are to be added to any element mass

mtype             : optional keyword defining the mass usage
                     L        -        mass for load calculation only
                     M        -        mass for mass calculation only
                     If omitted (default), the mass will be included in all calculations.

mass              : value of the lumped mass. (Real)

dof               : freedom name to define the direction in which the mass is active. See Appendix -F

nodes             : list of node numbers to which the mass is applied. (Integer)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-218
ASAS (Non-Linear) User Manual                                                                          Additional Mass Data


RP                : keyword to indicate the generation of data from the previous / symbol

nrep              : number of times the data is to be generated. (Integer)

inode             : node increment to be added each time the data is generated by the RP command. (Integer)

RRP               : keyword to indicate the generation of data from the previous // symbol

nrrep             : number of times the data is to be generated. (Integer)

iinode            : node increment to be added each time the data is generated by the RRP command. (Integer)

END               : compulsory keyword to denote the end of the lumped mass data block

Notes


1.      Whether or not the mass of any particular element is included depends on the setting of the mass flag in
        the element topology data.

2.      Freedom name TRA may be used to assign the mass to the X, Y, Z freedoms at the nodes. Freedom
        name ROT may be used to assign the mass to the RX, RY, RZ freedoms.

3.      If a node is skewed in Boundary Condition data, any added lumped mass terms input for that node are
        assumed to be in the skewed directions.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-219
ASAS (Non-Linear) User Manual                                                                              Initial Conditions Data



5.6     Initial Conditions Data

These data blocks allow the user to define the initial residual stress state of the elements and the initial nodal
displacements and velocities for a transient dynamic analysis. This data is optional.

The following data blocks are available

                         Residual initial stresses ............ ................ ................ see Section 5.6.2

                         Residual initial stresses for stiffeners ........ ................ see Section 5.6.3

                         Initial conditions ...... ................ ................ ................ see Section 5.6.4




5.6.1       UNITS Command

If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally by the inclusion of a UNITS command. The local units are only
operational for the data block concerned and will return to the default global units when the next END command
is encountered.

In general, one or more UNITS commands may appear in a data block thus permitting the greatest flexibility in
data input. The form of the command is similar to that used in the Preliminary data.
         UNITS                          unitnm




Parameters

UNITS         : keyword

unitnm        : name of unit to be utilised (see below)

Notes


1.      Force, length and angular unit may be specified. Only those terms which are required to be modified
        need to be specified, undefined terms will default to those supplied on the global units definition unless
        previously overwritten in the current data block.

2.      The default angular unit for all load types is radians

3.      Valid unit names are as defined in Section 5.1.42.1.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 5-220
ASAS (Non-Linear) User Manual                                                                          Initial Conditions Data


5.6.2       RESIDUAL Initial Stresses

This data defines a residual stress state from which the analysis is initiated. Optional.

              RESI

                      ALL
                                                  rstv al                  //elno//
                     inptno


              RP               nrep               ielem

              RRP              nrrep              iielem

              END




Parameters

RESI          : compulsory header keyword to denote the start of the residual initial stress data

ALL           : keyword to indicate that all integration points for element elno have the same residual initial
                stress values

inptno        : integration point number to which the following residual initial stresses apply. (Integer)

rstval        : residual initial stress values, the number of which depend upon the element type. See table below.
                (Real)

elno          : element number to which the residual initial stress values apply. (Integer)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : number of times the data is to be generated. (Integer)

ielem         : element number increment to be added each time the data is generated by the RP command.
                (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : number of times the data is to be generated. (Integer)

iielem        : element number increment to be added each time the data is generated by the RRP command.
                (Integer)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-221
ASAS (Non-Linear) User Manual                                                                          Initial Conditions Data


END           : compulsory keyword to denote the end of the residual initial stress data

Notes

1.      The number of stress components (NST) for different element types and their orders are given in the
        following table:


                                                    Location in vector
        Element type                    NST
                                                    1              2              3              4           5        6
        Uniaxial                        1           XX             -              -              -           -        -
        Plane Stress                    3           XX             YY             XY             -           -        -
        Plane Strain                    4           XX             YY             XY             ZZ          -        -
        Axisymmetric                    4           RR             ZZ             HH             RZ          -        -
        3-D solids                      6           XX             YY             ZZ             XY          YZ       ZX
        Thick beams, STF4               3           XX             XY(XT)*        XZ(-)*         -           -        -
        Shells                          5           XX             YY             XY             XZ          YZ


        * for tube or box sections, XT is the tangential shear stress component


2.      The stresses are defined in the stress output axis system as specified in Appendix -A.




5.6.3       RESIDUAL Initial Stresses for Stiffeners WST4 and SST4

This data defines the residual axial stress for stiffener elements. Optional.

The residual stress is read in for two end nodes of the element and all median points of the cross-section. For
details of median points see Geometric Property Data, see Section 5.2.5.1.

Stresses are interpolated from element end nodes to Gauss points and from median points to segment integration
points. A linear interpolation is used in both cases.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-222
ASAS (Non-Linear) User Manual                                                                          Initial Conditions Data




              RESD

                    ND1
                    ND2                      rstv al                       //elno//
                    ALL

              RP               nrep               ielem

              RRP              nrrep              iielem

              END




Parameters

RESD          : compulsory header keyword to denote the start of the residual initial stress data for stiffeners
                WST4 and SST4

ND1           : keyword to indicate that the following residual stress values refer to node one

ND2           : keyword to indicate that the following residual stress values refer to node two

ALL           : keyword to indicate that the following residual stress values refer to both node one and node two

rstval        : list of residual initial axial stress values for each median point. (Real)

elno          : element number to which the residual initial axial stress values apply. (Integer)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : number of times the data is to be generated. (Integer)

ielem         : element number increment to be added each time the data is generated by the RP command.
                (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : number of times the data is to be generated. (Integer)

iielem        : element number increment to be added each time the data is generated by the RRP command.
                (Integer)

END           : compulsory keyword to denote the end of the residual initial stress data for stiffeners WST4 and
                SST4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-223
ASAS (Non-Linear) User Manual                                                                          Initial Conditions Data


Notes


1.      The RESD data block must follow the RESI data block if both are present.

2.      If the same elements appear in both the RESD and the RESI data then the residual stress is the sum of
        stress from both sets of data.

3.      Values of residual axial stress are assigned to cross-sectional median points in increasing number order.
        The number of values should not exceed the number of median points for the element cross section.
        Median points which are not assigned a stress value are assumed to have zero residual axial stress.

4.      Free format continuations (:) may be used but, if they are used, the keywords ND1, ND2 and ALL should
        appear at the start of each new line.

5.      For any particular element, the residual axial stress values required for both ends and for all median
        points must be defined at one point.




5.6.4       Initial Conditions

This data defines the initial conditions of the structure at the start of a transient dynamic or heat analysis.
Optional.

             INIT


             dof                    disp               v elo                     //node//

               T                    temp                        //node//

             RP               nrep                inode

             RRP              nrrep               iinode

             END




Parameters

INIT          : compulsory header keyword to define the start of the initial condition data for a transient dynamics
                analysis

dof           : a freedom code. See Appendix -F

disp          : an initial displacement. (Real)

velo          : an initial velocity. (Real)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-224
ASAS (Non-Linear) User Manual                                                                          Initial Conditions Data


T             : freedom code for temperature (heat analysis only)

temp          : initial temperature

node          : list of node numbers at which the initial condition is applied. (Integer, 1-99999)

RP            : keyword to indicate the generation of data from the previous / symbol

nrep          : number of times the data is to be generated. (Integer)

inode         : node number increment to be added each time the data is generated by the RP command.
                (Integer)

RRP           : keyword to indicate the generation of data from the previous // symbol

nrrep         : number of times the data is to be generated. (Integer)

iinode        : node number increment to be added each time the data is generated by the RRP command.
                (Integer)

END           : compulsory word to define the end of the initial conditions

Notes


1.      If a node is skewed in the Boundary Condition data, any initial conditions specified will be assumed to be
        in the skewed direction.

2.      If non-zero initial conditions are given, the first solution time must be time 0.0 for a new analysis and the
        last static solution time if it is restarted from a static job.

3.      In a restart, the initial conditions specified may be total values or in addition to the previous solution. By
        default, total values are assumed and Option DTRS should be set if incremental values are specified.

Example


This example gives the X freedom of nodes 1,2,3,4 an initial displacement of 0.0 and an initial velocity of 1.0.

        INIT
        /
        X 0.0 1.0               1     2
        RP 2 2
        END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-225
ASAS (Non-Linear) User Manual                                                                                STOP Data



5.7    STOP Command

To define the termination of the input data for this run.


          STOP




Parameter

STOP          : compulsory keyword




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 5-226
ASAS (Non-Linear) User Manual                                                                             STOP Data




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 5-227
ASAS (Non-Linear) User Manual                                                                          Running Instructions



6.     Running Instructions

6.1    DATA AREA Requirement

The amount of workspace or DATA AREA specified with the SYSTEM command depends mainly on the
number of elements and nodes in the model. An analysis will abort if insufficient workspace is allocated. Some
of the data area (dependent on system parameters) is always reserved for the data-manager, (see next section).
The default value for DATA AREA is 1000000 but a higher value may be required for very large problems. The
size of the data area is defined in terms of Integer words (ie 1 word = 4 bytes). Note, the word freestore is often
used in place of data area, but both terms have the same meaning.

6.2    Data-Manager Parameters

Parameters that control the operation and efficiency of the data-manager are set by default. They are normally
adequate for most analyses, but may be insufficient for large analyses. In this case a re-analysis must be
performed and default system parameters re-set using the Preliminary Data SYSPAR command. Default values
for the system parameters are given in Table 6.1.

A certain amount of the workspace (LPGSIZ*MINPAG) is always reserved for the data-manager from the data
area allocation defined with the SYSTEM command. Both parameters MINPAG and LPGSIZ may be increased
to reduce the amount of ‘paging’ by the data-manager. This, however, will increase the demand of data area
required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-1
ASAS (Non-Linear) User Manual                                                                            Running Instructions



        System                                                                                     Default Size
                                           Description
       Parameter                                                                SMALL                   MEDIUM      LARGE

     LPGSIZ                 Data-manager pagesize                                  256                    512        1024

     MINPAG                 Minimum page reserve for data-                           10                    10          10
                            manager

     MANREC                 Default length of sub-index                            335                    335         335

     LTPAGE                 Maximum length of page directory                    65535                   65535       65535

     NOPAG                  Solution Blocking Factor                               10 1                   10 1        10 1



1.      NOPAG will be automatically reduced if there is insufficient freestore available.

                                                  Table 6.1 System Parameters




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 6-2
ASAS (Non-Linear) User Manual                                                                          Running Instructions


         Default Name                     Type                         Description                            Can Name be
                                                                                                              Overwritten?
   ZZZOARCH                              External         Old Archive file                              Yes
   ZZZNARCH                              External         New Archive file                              Yes
   ZZZOSTIF                              External         Old Stiffness file                            Yes
   ZZZNSTIF                              External         New Stiffness file                            Yes
   ZZZPORTF                              External         Porthole file                                 Yes
   ZZZMODEL                              External         PATRAN/FEMVIEW Neutral                        Yes
                                                          file
   pnamJF**                              External         Project journal file                          No
   INCRJF                                External         Analysis journal file                         No


      Default Name             Default Status           Default Attribute                 Deleted on               May be
                                                                                          Successful             Overwritten?
                                                                                         Completion?
   ZZZOARCH                      Unset                         Append                          No                    Yes*
   ZZZNARCH                      New                           Append                          No                     No
   ZZZOSTIF                      Old                           Append                          No                    Yes*
   ZZZNSTIF                      New                           Append                          No                     No
   ZZZPORTF                      New                           Append                          No                     No
   ZZZMODEL                      New                           Append                          No                     No
   pnamJF**                      Old                           Append                          No                    No
   INCRJF                        Old                           Append                          No*                   No



* Upon request by user

** pnam is the project name

Note


First three letters of each file name may vary from installation to installation.

                                                     Table 6.2 External Files

6.3     File Status

The names, types and contents and default attributes of all internal and external files are given in Table 6.2.

The user is cautioned that conflicts can arise if default names are used, due to files with the same name
remaining from previous runs. It is recommended that files are explicitly named.

The types, names and dispositions of all files used in an analysis are listed in the output files under the heading
FILE STATUS. Table 6.3 contains a list of possible dispositions.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 6-3
ASAS (Non-Linear) User Manual                                                                          Running Instructions



                                        Mnemonic                                       Action

                              DEL                                          Deleted

                              OPEN                                         Open

                              CLSE                                         Closed, but not deleted



                                  Table 6.3 Dispositions of Internal and External Files

6.4    Warnings and Errors

Errors resulting in unsuccessful analyses may result for a variety of reasons:

       Data Errors
       Insufficient Data Area Allocated to the Program
       Backing Files Not Open Correctly
       System Parameters Insufficient for Analysis


Most errors result in a controlled exit, a system abort message, a sub-routine traceback indicating the subroutine
in which the program halted and a message describing the error.

Data problems with the user may result in either error or warning messages. An error message indicates a
problem that prevents satisfactory execution of the analysis. In this case, the job will terminate after the stage
where errors are reported. Warnings indicate problems or inconsistencies with the data, but which can still allow
successful analysis. In this case the analysis will terminate before the main analysis unless the option GOON is
given with the preliminary data OPTION command.

Messages such as:

        ERROR FOR UNIT 8 NAME ZZZOARCH, MODE 3, DISPOSITON 1, STATUS 0

indicate an error in opening a file (ZZZOARCH for example). Table 6.4 indicates the various possible values
for Mode, Disposition and Status.

Occasionally large analyses may fail because the default system parameters are insufficient for the analysis (see
Section 6.2).

                       Parameter                       Value                            Description

                MODE                                      1             Existing File
                                                          3             New File

                DISPOSITION                               1
                                                          2
                                                          3

                STATUS                                various           Machine dependent error code.
                                                                        See specific machine documentation




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-4
ASAS (Non-Linear) User Manual                                                                          Running Instructions


                                      Table 6.4 Mode, Disposition and Status of Files


If a premature exit is made from ASAS-NL, then there will be an internal file called pnamJF (pnam is the project
name), created which indicates the stage the program had reached when the exit was made. The different stages
are given in Table 6.5.


                 Stage Number                                           Description

                          1                  Read and echo data. Preliminary checking

                          2                  Check and print data

                          3                  Determine the parameters for solution process

                          4                  Main analysis



                                           Table 6.5 Stage Numbers for ASAS-NL


If a premature exit is made within the main analysis (i.e. stage 4), a journal file called INCRJF will also be saved
indicating the current increment and iteration being analysed when the exit was made.

6.5    Running Instructions

The program ASAS-NL is required to run an ASAS-NL analysis. In addition, if a restart is attempted, the data-
manager oldarchive file and stiffness matrix oldarchive file must be present in the default directory (these files
are named with the FILE commands).

The instructions to run ASAS-NL have been kept to a minimum with all file assignments being initiated from
within the program as the run proceeds.

The PC version of ASAS-NL is run as a Windows process. The program is issued with an accompanying icon
which may be displayed on the main Windows desktop. There are three ways in which a program may be run

1. Click on the Program Icon

By clicking on the program icon, the following form will be displayed:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-5
ASAS (Non-Linear) User Manual                                                                          Running Instructions




The data file name may be identified by clicking on the Browse button. A file structure will be displayed from
which the data file may be identified. Double clicking on the file will place it in the Data File Name display box.
Alternatively, the data file name and its path may be typed in the display box. By default, the analysis will be run
in the directory defined by the path to the data file.

Command line parameters can be defined in this display box. The following parameters may be used to define
the location of files:



/DATA=          will define the name of the data file and, optionally, its location. By default .dat will be appended
                if no file extension is given.

/OUT=           will define the name of the results file and, optionally, its location. By default this will be set to the
                data file prefix appended with .out, e.g. for an input file of hull.dat the results file will be hull.out.

/PATH=          will define the path to the data and results file.
                This will be used if there is no path defined on /DATA= or /OUT=

/BACK=          will define the directory in which the analysis is to be run.
                This may be different from the location of the data and results files.

/CLEAR          will clear the dialog window. The default is for it to remain in position at the end of the run.

/LOCK           will write a lock file. This may be interrogated with the WAITLOCK process to determine when
                the process has completed. See note below.

/EXPAND         will expand all @ files, resolves all IF/THEN/ELSE references, and carries out all data
                replacements (see below). This generates a new data file with a .exp extension. Note that the use of
                /EXPAND does not run the program itself, rather it is a pre-processor for generating expanded
                data.

Parameters must be separated by a space on the command line.

To start the analysis, click on the OK button. This will display a dialog window similar to that shown below:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-6
ASAS (Non-Linear) User Manual                                                                          Running Instructions




At the end of the run a message is displayed that the analysis has completed and requests an Exit confirmation.
Clicking on ”Yes” or pressing the enter key on the keyboard will close the dialog window. Clicking on ”No” will
allow the window to be processed according to the command buttons. Note that the use of /CLEAR
automatically closes the dialog window when the analysis has completed.

2. Drag and Drop

Using Windows Explorer, a data file may be dragged and dropped on the program icon. This will automatically
initiate the analysis in the directory of the data file. To run ASASNL, drop the data file onto the ASASNL icon.

3. Using a Windows Command Prompt

The program can be run in a Windows Command Prompt using a command of the form:


            asanl DataFileName
or
            asasnl /DATA=DataFileName /OUT=ResultsFileName [/parameter]


assuming the directory where the program is installed (e.g. c:\asash) in on the path correctly. The optional
/parameter equates to any of the valid command line parameters given above e.g. /CLEAR, /PATH=c:\asash\test.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-7
ASAS (Non-Linear) User Manual                                                                          Running Instructions




Typing the program name on its own is equivalent to clicking on the program icon as described above.

It is not now possible on the PC to use the redirect symbols < and > to define data and results files.

Running ASAS-NL from batch files on PCs

As ASAS-NL now runs as a process, it may not be possible for a number of jobs to be run consecutively. This is
because when a command is issued to start an ASAS-NL run, the process begins and control may return
immediately to the DOS shell or the .BAT file. So, if a .BAT file is being used, as each process begins, control is
returned to the file and the next command is executed.

This has been overcome in the ASAS suite of programs with the use of a LOCK file. If the /LOCK parameter
(see above) is used, a file called $_$_LOCK is created. A program WAITLOCK has been written that can then
be run following an ASAS program. This program will wait until the LOCK file has been deleted, which occurs
when the preceding ASAS run completes. When the LOCK file has been deleted, WAITLOCK itself completes
and allows the next command to be executed.

Example Batch File

ASASNL        hull /LOCK
WAITLOCK



6.6    ASAS Initialisation File

The ASAS initialisation file allows the user to define the default file extensions to be used. The file is called
asas.ini. There are three locations in which the file may be stored. These are searched in the following order:

1.          In the current directory

2.          In a directory pointed to with the environmental variable ASAS_INI.

3.          In a directory pointed to with the environmental variable ASAS_SEC.

Currently, the following data items may be defined in the asas.ini file.

The first line must be [General] starting in column 1.

The next lines may be one or more of the following, all starting in column 1:

Default_input_extension=ext                                      where ext is the user’s preferred extension for the input file.
                                                                 Default is .dat

Default_output_extension=ext                                     where ext is the user’s preferred extension for the output
                                                                 file.
                                                                 Default is .out




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-8
ASAS (Non-Linear) User Manual                                                                             Running Instructions


Noclobber=on (or ON or On)                                       prevents the output file from being overwritten if it already
                                                                 exists in the current directory.

The two default extensions will only be used if no extension is given for either input or output files on the
command line, eg

             asasnl.exe               hull

The output default extension will also be used if the input file name is specified with an extension and no output
file is specified on the command line, eg

             asasnl.exe               hull.dat

6.7     Extended Syntax in Data Files



6.7.1        IF/THEN/ELSE

ASASNL data is often very similar for several runs. Differences can occur when data is used for linear and
dynamic analysis, when two similar components are being created or different loading is required in a series of
runs. These similarities will vary for each different user.

The IF/THEN/ELSE feature allows the user to create a path through a data file conditional upon one or more
pieces of key data on the command line or embedded within the data.

This feature is best described with an example of a linear and a natural frequency run.

The three columns below describe the two separate sets of data, and then how they can be merged together.

  Static Data                                 Transient Data                                Merged Data
  job stat                                    job tran                                      if static then
                                                                                              job stat
                                                                                            else
                                                                                              job tran
                                                                                            endif
  project test                                project test                                  project test
  options nobl                                options nobl                                  options nobl
                                              save new 1. 2. 3. 4.                          if static then


                                                                                            else
                                                                                              save new 1. 2. 3. 4.
                                                                                            endif
  coor, elem, mate, geom                      coor, elem, mate, geom                        coor, elem, mate, geom
  supp, disp, load                            supp, disp, load                              supp, disp
                                              resi                                          if static then




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 6-9
ASAS (Non-Linear) User Manual                                                                          Running Instructions




                                                                                            else
                                                                                              resi
                                                                                            endif
  stop                                         stop                                         stop


Note: In this example, coor, elem, load, etc represent complete sets of data.

The command line to run this data would be either:

                     asasnl.exe            hull /static for a static run


or

                     asasnl.exe            hull /#static                      for a transient run


Thus any parameter after a /, except the reserved parameters listed in section 6.5, is treated as a logical
parameter. This takes the value true if on its own, or false if preceded by #.

This has been extended to allow for testing against a value, as in the following example:

 Static Data                        Transient Data                     Merged Data
  job stat                          job tran                           if save#tran then
                                                                         job stat
                                                                       else
                                                                         job tran
                                                                       endif
  project test                      project test                       project test
  options nobl                      options nobl                       options nobl
                                    save new 1. 2. 3. 4.               if save=tran then
                                                                         save new 1. 2. 3. 4.
                                                                       else


                                                                       endif
  etc                               etc                                etc


The command line to run this data would be either:

             asasnl.exe hull                /save=tran for a transient run

or

             asasnl.exe hull                                       for a static run

Thus the parameter following / may be of the form:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-10
ASAS (Non-Linear) User Manual                                                                          Running Instructions


            /param                     param is true when encountered in the data

            /#param                    param is false when encountered in the data

            /param=value               param is true in the data if it equals value

            /param#value               param is false in the data if it does not equal value

Any parameters not defined on the command line are assumed to be false.

Then in the data, the test following IF and ELSEIF is

            IF param THEN                           the lines of data following are used if param is true

            IF #param THEN                          the lines of data following are used if param is false

            IF param=value THEN                     the lines of data following are used if param equals value

            IF param#value THEN                     the lines of data following are used if param does not equal value

The full sequence of possible IF/THEN/ELSE statements is:

IF logical1 THEN

 these lines are used if logical1 is true

ELSEIF logical2 THEN

 these lines are used if logical2 is true

ELSEIF logical3 THEN

 these lines are used if logical3 is true

ELSE

 these lines are used if none of the above is true

ENDIF

The ELSE command is not mandatory, but if it is omitted, then there could be situations when none of the lines
is used between the IF and ENDIF.

There is no limit to the number of ELSEIF statements. Nesting up to five levels may be used.

Note that it is important that there must be no embedded spaces in the parameter test.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-11
ASAS (Non-Linear) User Manual                                                                          Running Instructions


6.7.2       DATA REPLACEMENT

Specified character strings in the data may be replaced with values defined on the command line.

Consider the following data file:

          job stat
          project %proj
          options nobl
          end
          coor, elem, mate, geom, supp, disp decks
          load 1
          case 1 Point load of %load
          nodal lo
          z %load 200
          end
          stop

Then the command line would be, for example:

          asasnl.exe hull %proj=a001 %load=5000

When interpreting the data, each time %proj was encountered, it would be replaced by the characters a001, and
%load replaced by the characters 5000.

To maintain compatibility between UNIX and the PC, the $ may be used instead of %. The two characters are
completely interchangeable and the existence of one implies also the existence of the other. Thus the command
line could be:
         asasnl.exe hull $proj=a001 $load=5000

It should be noted that if any of the replacement strings is not satisfied in a data file a warning will occur for
each one. Processing will continue, but there will probably be errors in the data where the unsatisfied
replacement strings are being interpreted.




6.7.3       The DEFINE Command

The command line data may be embedded within the data file itself by using a DEFINE command. This has the
same effect as setting logical values on the command, but they can change during the processing of the file. For
example:

            define %proj=a001
            define %load=5000
            job stat
            project %proj
            options nobl




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-12
ASAS (Non-Linear) User Manual                                                                          Running Instructions


            end
            etc

When the data is interpreted, the replacement strings would take the values as on the define lines. However, they
may be overridden by a different value on the command line. The command line value takes precedence if a
string replacement is used on a command line and also on a DEFINE command. Thus, if the command line had
been:

            asasnl.exe hull %proj=a002

then the project would have been interpreted as project a002 instead.

The DEFINE commands do not have to be placed at the start of the data file. They may occur anywhere prior to
the first use of the parameter.

6.8     Secondary Data Files within ASAS-NL Data

The command @filename may appear anywhere in a data file. When such a command is encountered, the
input of data switches to the file filename and data continues to be read from that file until either the end-of-
file is reached or an @ command is encountered in the secondary file.

When the end of the secondary file is reached, that file is closed and input switches back to the previous data
file. If, however, an @ command is found in the secondary file, input switches to yet another file. This process
can continue until a maximum of 5 secondary files are open simultaneously.




6.8.1       Use of @filename command

There are many ways in which such a facility can be used, some examples of which are listed below.

(a)     The user may prepare each data block in a separate file and these files may then be referenced by a simple
        main datafile which consists of @ commands only.

        For example, hull.dat may contain the lines


                @prelim.dat
                @phase1.dat
                @phase2.dat
                @load.dat

        phase1.dat may then contain


                @coor.dat
                @elem.dat
                @mate.dat
                @geom.dat




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-13
ASAS (Non-Linear) User Manual                                                                          Running Instructions


        Finally,     coor.dat contains the coordinate data
                     elem.dat contains the element data
                     etc.

(b)     The user may prepare his data as in example (a) above but may have a number of variants of some of the
        data blocks, for example, geometry data, support data and load data.

        A number of small data files containing @ commands can be prepared to pull together the various data
        blocks in whatever combinations may be required.

(c)     The user may have a block of data, such as some loading data which he needs to repeat in a number of
        different loadcases. If these data are stored in a file, for example pressure.dat, they may be read at
        any point by including a command @pressure.dat.

(d)     On some computers, the file editors may not handle very long files conveniently. In such cases the data
        file may be split into convenient sections for editing without the need to recombine into one file before
        the analysis run.




6.8.2         Notes about the @ Command

1.      The filename on the @ command line may be up to 79 characters long . This name may include the path
        name to the directory as well as the filename.

        Examples of the @ command

        (a)     @coor.dat                           -        switch to file coor.dat

        (b)     @    coor.dat                       - spaces are allowed between @ and filename

        (c)     @/asasdata/coor.dat - an absolute path (/asasdata) is included

        (d)     @bridge/coor                        -        reference to a subdirectory (bridge) is included

        (e)     @h:\data\coor                       -        reference to a different drive and directory on a PC

        (f)     @..\data\coor                       -        reference to a directory relative to the current directory

2.      @ may be nested to a depth of 5 secondary files open at any one time in addition to the main data file.

3.      A secondary file is closed when the end-of-file is reached whereupon control returns to the line following
        the @ command in the higher level data file.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-14
ASAS (Non-Linear) User Manual                                                                          Running Instructions


4.     Any one file may be opened several times in one run using @ commands, provided that it has been closed
       before being accessed for a second time.
       Conversely, no file may be opened more than once within a given nesting of @ commands. (Recursion is
       not allowed).

5.     A secondary file which contains all or part of the preliminary data must not also contain any other data,
       such as coordinates or elements. Such a secondary file must terminate at or before the END command for
       the preliminary data.

6.9    Soft Halt Facility

There may be occasions when it is desirable to halt an analysis before all increments have been completed. This
may be achieved by creating a file named ZZZSHALT in the directory in which the program is running. At the
completion of each increment, ASASNL checks for the existence of this file and terminates accordingly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-15
ASAS (Non-Linear) User Manual                                                                          Running Instructions




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-16
ASAS (Non-Linear) User Manual                                                                          Appendix A




Appendix - A                      Element Description Sheets


A.1         Facilities Available for each Element Type

This Appendix contains a detailed description of each of the finite element types within ASAS-NL, arranged in
alphabetical order. They can be grouped as follows:


Stress/structural elements

       Uniaxial                                              FLA2

       Plane Strain/Plane Stress                             TRM3, QUM4, TRM6, QUM8

       Axisymmetric Solid                                    TRX3, QUX4, TRX6, QUX8

       3-D Solid                                             BRK6, BRK8, BR15, BR20

       3-D Laminated Solid                                   LB15, LB20

       Shell/Plate                                           QUS4, TCS6, TCS8, TCS9

       Beam/Stiffener                                        STF4, BEAM, BM2D, BM3D, TUBE

       Beam/Stiffener of arbitrary                           SST4, WST4
       (open) cross-section

       Gap                                                   GAP2, GAPX, GAPR

       Spring/Dashpot                                        SPR1, SPR2

       Rigid surface interface                               RGX3, RGX4, RG23, RG24

       Linespring                                            LSP3, LSP6


Field elements

       Uniaxial                                              FAT2, FAT3

       2-D Plane                                             TMT3, QMT4, TMT6, QMT8

       Axisymmetric Solid                                    TXT3, QXT4, TXT6, QXT8

       3-D Solid                                             BRT6, BRT8, BT15, BT20




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-1
ASAS (Non-Linear) User Manual                                                                          Appendix A



The following chart summarises the facilities available to each element.

Following the chart is a description of rigid offsets for beams.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-2
ASAS (Non-Linear) User Manual                                                                          Appendix A




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-3
 ASAS (Non-Linear) User Manual
                                                                                                 Material Models                                                                     Tangent
                                                                                                                                                                                     Stiffness
                                                        Elastic                                                  Plastic                             Fail   Creep
                                  Elem.                                                                                                                             Large                                 Mass     Skew       Default
                                  Type    Iso.   Hype   Aniso/    Lami.   Field   von      Tresca      Tension   Ivanov    Spring   Coul.    Kine.          von     Disp.   Geom.      Cent.     Press.   Matrix    Sys.     Int. Rule
                                                  .     Orth/                     Mises   Mohr/Dru                                  Frict.   Hard.          Mises            Stiff     Stiff      Stiff
                                                                                                       Cut-off
                                                        Wove                                 c
                                                          n
                                  BEAM    ♦                                                                          ♦                                               ♦        ♦                             ♦       ♦
                                  BM2D    ♦                                                                          ♦                                               ♦        ♦                             ♦       ♦
                                  BM3D    ♦                                                                          ♦                                               ♦        ♦                             ♦       ♦
                                  BRK6    ♦       ♦       ♦                        ♦         ♦           ♦                                    ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦          1x1x2
                                  BRK8    ♦       ♦       ♦                        ♦         ♦           ♦                                    ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦          2x2x2
                                  BRT6                                     ♦                                                                                                                                                   1x1x2
                                  BRT8                                     ♦                                                                                                                                                   2x2x2
                                  BR15    ♦       ♦       ♦                        ♦         ♦           ♦                                    ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦          1x3x2
                                  BR20    ♦       ♦       ♦                        ♦         ♦           ♦                                    ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦          2x2x2
                                  BT15                                     ♦                                                                                                                                                   1x3x2
                                  BT20                                     ♦                                                                                                                                                   2x2x2
                                  FAT2                                     ♦                                                                                                                                                   1x1x1
                                  FAT3                                     ♦                                                                                                                                                   2x1x1
                                  FLA2    ♦       ♦                                ♦         ♦           ♦                                    ♦              ♦       ♦        ♦         ♦                   ♦       ♦
                                  GAP2    ♦                                                                                                                                                                         ♦
                                  GAPR    ♦                                                                                                                                                                         ♦
                                  GAPX    ♦                                                                                                                                                                         ♦
                                  LB15                             ♦                                                                                  ♦                       ♦         ♦          ♦        ♦       ♦      1x3x1 per layer
                                  LB20                             ♦                                                                                  ♦                       ♦         ♦          ♦        ♦       ♦      2x2x1 per layer
                                  LSP3    ♦                                        ♦                                                                                                                                           3x1x1
                                  LSP6    ♦                                        ♦                                                                                                                                           3x1x1
                                  QMT4                                     ♦                                                                                                                                                    2x2
                                  QMT8                                     ♦                                                                                                                                                    2x2
                                  QUM4    ♦       ♦       ♦                        ♦         ♦                                                ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦           2x2
                                  QUM8    ♦       ♦       ♦                        ♦         ♦                                                ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦           2x2
                                  QUS4    ♦               ♦        ♦               ♦         ♦                       ♦                        ♦       ♦      ♦       ♦        ♦         ♦          ♦        ♦       ♦          1x1x3
Page A-4




                                  QUX4    ♦       ♦       ♦                        ♦         ♦                                                ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦           2x2
                                  QUX8    ♦       ♦       ♦                        ♦         ♦                                                ♦              ♦       ♦        ♦         ♦          ♦        ♦       ♦           2x2




                                                                                                     Table A.1 Facilities available to each element type
 ASAS (Non-Linear) User Manual                                                          Load Types
                                  Elem.
                                  Type    Nodal   Presc.   Press.   Dist.   Temp    Face   Cent.   Body    Ang.    Tank    Nodal   Presc.   Flux
                                          Loads   D,V,A    Loads    Loads     .     Temp   Loads   Force   Acce.   Loads   Flux    Field    Dens.
                                                                            Loads     .              s
                                  BEAM     ♦        ♦                ♦       ♦               ♦        ♦     ♦
                                  BM2D     ♦        ♦                ♦       ♦               ♦        ♦     ♦
                                  BM3D     ♦        ♦                ♦       ♦               ♦        ♦     ♦
                                  BRK6     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  BRK8     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  BRT6                                                                                      ♦        ♦       ♦
                                  BRT8                                                                                      ♦        ♦       ♦
                                  BR15     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  BR20     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  BT15                                                                                      ♦        ♦       ♦
                                  BT20                                                                                      ♦        ♦       ♦
                                  FAT2                                                                                      ♦        ♦
                                  FAT3                                                                                      ♦        ♦
                                  FLA2     ♦        ♦                        ♦               ♦        ♦     ♦
                                  GAP2     ♦        ♦
                                  GAPR     ♦        ♦
                                  GAPX     ♦        ♦
                                  LB15     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  LB20     ♦        ♦        ♦               ♦               ♦        ♦     ♦
                                  LSP3     ♦        ♦
                                  LSP6     ♦        ♦
                                  QMT4                                                                                      ♦        ♦       ♦
                                  QMT8                                                                                      ♦        ♦       ♦
                                  QUM4     ♦        ♦        ♦       ♦       ♦               ♦        ♦     ♦       ♦
                                  QUM8     ♦        ♦        ♦       ♦       ♦               ♦        ♦     ♦       ♦
                                  QUS4     ♦        ♦        ♦       ♦       ♦       ♦       ♦        ♦     ♦       ♦
Page A-5




                                  QUX4     ♦        ♦        ♦       ♦       ♦               ♦        ♦
                                  QUX8     ♦        ♦        ♦       ♦       ♦               ♦        ♦




                                                           Table A.1 Facilities available to each element type (cont.)
 ASAS (Non-Linear) User Manual                                                           Material Models                                                                   Tangent
                                                                                                                                                                            Stiffness
                                                        Elastic                                         Plastic                             Fail   Creep
                                  Elem.                                                                                                                    Large                                Mass     Skew     Default
                                  Type    Iso.   Hype   Aniso/    Lami.   Field   von        Tresca    Ivano      Spring   Coul.    Kine.          von     Disp.   Geom.      Cent.     Press   Matrix    Sys.   Int. Rule
                                                  .     Orth/                     Mises     Mohr/Dru     v                 Frict.   Hard.          Mises            Stiff     Stiff     Stiff
                                                        Wove                                   c
                                                          n
                                  QXT4                                     ♦                                                                                                                                        2x2
                                  QXT8                                     ♦                                                                                                                                        2x2
                                  RGX3    ♦                                                                                  ♦                              ♦                                             ♦        2x1x1
                                  RGX4    ♦                                                                                  ♦                              ♦                                             ♦        3x1x1
                                  RG23    ♦                                                                                  ♦                              ♦                                             ♦        2x1x1
                                  RG24    ♦                                                                                  ♦                              ♦                                             ♦        3x1x1
                                  SPR1    ♦                                                                         ♦                                                                                     ♦
                                  SPR2    ♦                                                                         ♦                                                                                     ♦
                                  SST4    ♦                                        ♦                                                                        ♦        ♦         ♦                  ♦       ♦
                                                                                                                                                                                                                 2x3x3 Rect
                                                                                                                                                                                                                 2x8x1 Tube
                                  STF4    ♦                                        ♦           ♦                                     ♦              ♦       ♦        ♦         ♦                  ♦       ♦
                                                                                                                                                                                                                   2x12x1
                                                                                                                                                                                                                    Box
                                  TCS6    ♦               ♦        ♦               ♦           ♦        ♦                            ♦       ♦      ♦       ♦        ♦         ♦         ♦        ♦       ♦        1x3x3
                                  TCS8    ♦               ♦        ♦               ♦           ♦        ♦                            ♦       ♦      ♦       ♦        ♦         ♦         ♦        ♦       ♦        2x3x3
                                  TCS9    ♦               ♦        ♦               ♦           ♦        ♦                            ♦       ♦      ♦       ♦        ♦         ♦         ♦        ♦       ♦        2x3x3
                                  TMT3                                     ♦                                                                                                                                        1x1
                                  TMT6                                     ♦                                                                                                                                        1x3
                                  TRM3    ♦       ♦       ♦                        ♦           ♦                                     ♦              ♦       ♦        ♦         ♦         ♦        ♦       ♦         1x1
                                  TRM6    ♦       ♦       ♦                        ♦           ♦                                     ♦              ♦       ♦        ♦         ♦         ♦        ♦       ♦         1x3
                                  TRX3    ♦       ♦       ♦                        ♦           ♦                                     ♦              ♦       ♦        ♦         ♦         ♦        ♦       ♦         1x1
                                  TRX6    ♦       ♦       ♦                        ♦           ♦                                     ♦              ♦       ♦        ♦         ♦         ♦        ♦       ♦         1x3
                                  TUBE    ♦                                                             ♦                                                   ♦                                     ♦       ♦
                                  TXT3                                     ♦                                                                                                                                        1x1
                                  TXT6                                     ♦                                                                                                                                        1x3
                                  WST4    ♦                                        ♦                                                                        ♦        ♦         ♦                  ♦       ♦
Page A-6




                                                                                  Table A.1 Facilities available to each element type (cont.)
 ASAS (Non-Linear) User Manual                                                                             Load Types
                                                     Elem.
                                                     Type    Nodal   Presc.   Press.   Dist.   Temp.    Face   Cent.   Body     Ang.    Tank    Nodal   Presc.   Flux
                                                             Loads   D,V,A    Loads    Loads   Loads   Temp.   Loads   Forces   Acce.   Loads   Flux    Field    Dens.
                                                     QXT4                                                                                        ♦        ♦       ♦
                                                     QXT8                                                                                        ♦        ♦       ♦
                                                     RGX3     ♦        ♦
                                                     RGX4     ♦        ♦
                                                     RG23     ♦        ♦
                                                     RG24     ♦        ♦
                                                     SPR1     ♦        ♦
                                                     SPR2     ♦        ♦
                                                     SST4     ♦        ♦                                        ♦        ♦       ♦
                                                     STF4     ♦        ♦                ♦       ♦               ♦        ♦       ♦
                                                     TCS6     ♦        ♦        ♦       ♦       ♦       ♦       ♦        ♦       ♦       ♦
                                                     TCS8     ♦        ♦        ♦       ♦       ♦       ♦       ♦        ♦       ♦       ♦
                                                     TCS9     ♦        ♦        ♦       ♦       ♦       ♦       ♦        ♦       ♦       ♦
                                                     TMT3                                                                                        ♦        ♦       ♦
                                                     TMT6                                                                                        ♦        ♦       ♦
                                                     TRM3     ♦        ♦        ♦       ♦       ♦               ♦        ♦       ♦       ♦
                                                     TRM6     ♦        ♦        ♦       ♦       ♦               ♦        ♦       ♦       ♦
                                                     TRX3     ♦        ♦        ♦       ♦       ♦               ♦        ♦
                                                     TRX6     ♦        ♦        ♦       ♦       ♦               ♦        ♦
                                                     TUBE     ♦        ♦                ♦       ♦               ♦        ♦       ♦
                                                     TXT3                                                                                        ♦        ♦       ♦
                                                     TXT6                                                                                        ♦        ♦       ♦
                                                     WST4     ♦        ♦                                        ♦        ♦       ♦



                                  Notes
Page A-7




                                  1.      Elastic material data must be supplied.

                                  2.      The geometric stiffness is invoked by directive LARGe with the Problem or Group Title commands. The centrifugal stiffness is included by default if the
                                          structure is spinning. Symmetrized load stiffness is included by default if the structure is subject to pressure loading.


                                                                              Table A.1 Facilities available to each element type (cont.)
ASAS (Non-Linear) User Manual                                                                          Appendix A




A.2         Element Axes Systems

All elements have some form of local element axes system associated with them. These are used for the purpose
of defining material axes and element related loading and also for the calculation and display of stress results. For
some elements the global axes system is used as the element local axis system. All other elements have a local
system (as defined in the element description sheets which follow) normally based on the order in which the
element nodes are specified in the element topology data. The general rules used for defining the local axes for
elements of certain types are outlined in the following sections.

It must be noted that adjacent elements not using the global axes system can have a completely different
orientation of local axes system. For this reason the nodal stress/force results on adjacent elements may not be
averaged directly but must be re-orientated into a consistent axes system first. This type of re-orientation may be
conducted for the shell elements by the post processor POSTNL.

A.2.1 Local Axes on Beam Elements
The beam elements have the local X direction along the axis of the beam from the first node towards the last node.
The local Y and Z axes are normal to the beam axis and defined according to element specific rules (as described
in the individual element description sheets). For beam element types BM3D and TUBE the local Y and Z
directions may be explicitly defined in the geometric property data for the element by specifying the plane
containing the local Y or Z direction. For a TUBE element, the local axis definition may be omitted, in which
case a default local axis system is used. See TUBE element description sheets.

The planes of the local Y and Z axes may be defined by one of the following methods:

COOR command (Default)
        This gives the coordinates of a point in the local XY plane with the local Y axis positive towards this point
        from end 1 of the element. If command XZ is also present, the point defines the local XZ plane with local
        Z positive towards the point.


NODE command
        This works in the same way as for COOR except that the node number of a point with the required
        coordinates is given.


BETA command
        This gives an angle through which the default local Y and Z axes are to be rotated about the element local
        X axis. The default axes for BM3D assume the coordinate point in the local XY plane (XZ plane if
        command XZ is present) to be the origin, and for the TUBE are as given when the coordinate point is
        omitted.


GPOS, GNEG commands
        This gives an axis X,Y or Z which will be taken as a vector lying in the required local XY plane. The
        GPOS or GNEG keyword gives the positive or negative global direction as defining the positive direction
        for the local Y axis so defined. If command XZ is also present, then the vector lies in the required local XZ
        plane and the GPOS or GNEG defines the direction for the positive local Z axis.

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page A-8
ASAS (Non-Linear) User Manual                                                                          Appendix A


SPOS, SNEG commands
       This gives a skewed X,Y or Z axis, which will be taken as a vector lying in the required local XY plane.
       The SPOS or SNEG keyword and the skew system integer gives the positive or negative skewed global
       direction as defining the positive direction for the local Y axis so defined. If command XZ is also present,
       then the vector lies in the required local XZ plane and the SPOS or SNEG defines the direction for the
       positive local Z axis.


VECT command
       This gives the coordinates of a point defining a vector from the origin, lying in the required local XY plane
       with the local Y axis positive in the direction of the vector. If command XZ is also present, then the vector
       defines the required local XZ plane with the local Z axis positive in the direction of the vector.


These are shown diagrammatically in the following table.

For a further description of data formats see Section 5.2.5.5.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page A-9
ASAS (Non-Linear) User Manual                                                                                                  Appendix A


                                                             X'                                                                   X'
                                                           node2                                                                node2
                                                                                          Y'


        node1                                           (10,20,0)              node1                                         (10,20,0)
                      Z'                         Y'                                                                   Z'

                                                 COOR 10 20 0 [XY]                                                         COOR 10 20 0 XZ


                             501                                                                Z'         501
                Y'
                                                            X'                                                                       X'
                                                        node2                                                                    node2

        node1                                                                        Y'
                                                                                   node1
                             Z'
                                                      NODE 501 [XY]                                                           NODE 501 XZ

                                                                                     Y'               default Y'
                                                              X'                                                                     X'
                                     Y'                   node2                                                                  node2
                                                                                                               Z'
            node1                                                                    node1
                             β=35°                                                                        β=35°

                         β         default Y'                                                               default Z'
     default Z'               Z'                         BETA 35 [XY]                                                           BETA 35 XZ
        Y                                                                      Y
                                                                                                     Y'
                                                                                                                                       X'
                     X        Y'                                     X'                   X
                                                                                                                                   node2
                                                                 node2
    Z                                                                     Z
                                                                                          node1
                     node1
                                                                                                            Y'
                                       Z'
                                                        GP OS Y [XY]                                 Z'                         GNEG Y XZ

            Y                                                                      Y
   Ys                 Xs                                                  Ys                   Xs
                      X                                                                        X
                                                                     X'                                                                 X'
        Z                    Y'                                  node2         Z                     Y'                             node2
                 Zs                         Z'                                            Zs
                                                                                                                 Z'

                     node1                                                                node1
                                                        SNEG 1 Z [SY]                                                           SP OS 1 X XZ


                                                                X'                                                                 X'
                                   Y' |5,4,3|                                                        Z'   |5,4,3|
                                                            node2                                                              node2
                                                                               Y'

             node1                                                             node1
                                     Z'
                                                      VECT 5 4 3 [XY]                                                        VECT 5 4 3 XZ




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                             Page A-10
ASAS (Non-Linear) User Manual                                                                                          Appendix A


A.3         Beam Offsets

The element types BEAM, BM2D, BM3D, and TUBE can have rigid offsets defined at each node.

It is normally assumed that a beam member has its centroidal axes lying along the line joining the two end nodes
and that it is flexible throughout its length. Often, however, this is not the case. Sometimes the centroidal axis is
offset from this line. It may also be appropriate when modelling the intersection of two beams at a node to
consider the end portion of one of the beams to be rigid.

Rigid offsets may be defined by the OFFG, OFFS, OFSK or OFCO command in the Geometric Properties Data
(Section 5.2.5). The offset command for an element occurs after the Geometric Properties commands for that
element.

One command is required for each set of geometric property data which describes a member with offsets


An offset beam element has two local axis systems. Local X’,Y’,Z’ refer to the node points used to define the
element and X”,Y”,Z” refer to the physical ends of the element centroidal axis after the offsets have been taken
into account. If the member has no offsets then X’,Y’,Z’ and X”,Y”,Z” are coincident.
                                                   Y'
                                                          Y”



                                                                                       Node2
                                          Node1                                                                    X'

                                                End1
                                     Z'                                                         End 2
                                                                                                        X”

                                              Z”



                                       Figure A.1 Local Axes for a Beam with Offsets

A.3.1 OFFS Command
For the OFFS command, the local offsets are defined as the distances from the physical ends of the member
centroidal axes to the nodes, measured in the local X’,Y’,Z’ axes system.

Positive values of the local offsets ex, ey, ez, are as shown:
                     Y'                                                                                       Y'
                                  Y”



                           Node1                                   Node 2                                      Node 1
                                                                                      X'                           Z'
                                                                                                        ey
                                ey
                           ex
                                                                      ey                                 ez

                                                                           ex

                                                                                           X”




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page A-11
ASAS (Non-Linear) User Manual                                                                                            Appendix A


                                        Figure A.2 Beam Offsets Defined using OFFS

Notes


1.      ex at node 2 is measured in the negative x’ direction such that a shortening at either end of the beam is
        given by a positive ex value.

2.      The command has the keyword OFFS and the six offset values ex, ey, ez values for node 1 followed by ex,
        ey, ez values for node 2.

3.      For BM2D element, 4 values of offset are required, ex, ey values for node 1 followed by ex ey for node 2

Example


Example of an Offset BM3D

        175      BM3D       17.5        145.0            97.3          5.7
        :                     0.0       225.0        1107.0                  0.0       0.0
        :        OFFS       12.7           4.3            0.0          0.0   4.3       0.0

A.3.2 OFFG and OFSK Commands
For the OFFG and OFSK commands, the offsets are defined as the distances from the nodes to the physical ends
of the member centroidal axis, measured in the global or skewed global axes system.
        Y




                                                            ex (-ve)

                                                          ey
                 ex                                                                                     Y
                                                                 Node 2
                                                                                                             ez
                       ey
                                                                                                                     ey
             Node1
                                                                                                            Node 1
                                                                       X                                                    Z




                                 Figure A.3 Beam Offsets Defined using OFFG or OFSK

Notes


(i)     The OFFG command has the keyword OFFG and the six offset values ex, ey, ez values for node 1 followed
        by ex, ey, ez values for node 2.

(ii)    The OFSK command has the keyword OFSK followed by a skew system integer to identify the skewed
        global axes system. This is then followed by 6 offset values as above.

(iii)   For BM2D element, 4 values of offset are required, ex, ey, values for node 1 followed by ex, ey for node 2.


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      Page A-12
ASAS (Non-Linear) User Manual                                                                                  Appendix A


Example


Example of offset beam elements.

        175      BM3D         17.5         145.0               97.3    5.7
        :                         0.0           225.0          1107.0                0.0       0.0
        :       OFFG          -5.0         0.0    2.0 0.0                 -8.0          6.0
        1       BEAM          64.2         1208.0 497.0                   23.0
        :       OFSK          6        1.0          0.0          0.0           -1.0         0.0           5.0

A.3.3 OFCO Command
For the OFCO command, the global coordinates of the physical ends of member centroidal axes are required.
                        Y




                                                                                    (x2,y2 ,z2 )



                                                                                          Node 2
                                                (x1 ,y1 z1 )

                                      Node1

                                                                                             X




                                       Figure A.4 Beam Offsets Defined using OFCO

Notes


1.      The command has the keyword OFCO and the 6 coordinate values x,y,z for end 1 followed by x,y,z for
        end2.

2.      For BM2D element, 4 values of coordinates are required, x,y for end 1 followed by x,y for end 2.

Example of offset BM3D

        175      BM3D         17.5         145.0               97.3    5.7
        :                         0.0           225.0          1107.0                0.0       0.0
        :       OFCO          10.0         5.0                 8.0        12.0          3.0             20.0




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-13
ASAS (Non-Linear) User Manual                                                                                  Appendix A



A.3.4 Finite Element Description Sheets

                                                                                                             Beams/Bars
BEAM 2 node beam with constant cross section and rigid offset and special orientations for three
     dimensional structures
BM3D 2 node beam with constant cross section and rigid offsets for three dimensional structures.
BM2D 2 node beam with constant cross section and rigid offsets for two dimensional structures.
FLA2     2 node axial element with varying cross section.
TUBE     2 node circular tube element with constant cross section and rigid offsets.




                                                                                                          Solid Elements
BRK6     6 node straight edged wedge.
BRK8     8 node straight edged brick.
BR15     15 node wedge.
BR20     20 node brick.
LB15     15 node laminate wedge.
LB20     20 node laminate brick.



                                                                                                Axisymmetric Elements
QUX4     Axisymmetric quadrilateral solid with straight or curved edges.
QUX8
TRX3      Axisymmetric triangular solid with straight or curved edges.
TRX6




                                                                                                        Membrane Elements
QUM4 4 node quadrilateral membrane with varying thickness and plane strain options.
QUM8 8 node isoparametric quadrilateral membrane with varying thickness and plane strain options.
TRM3 3 node triangular membrane with varying thickness and plane strain options.
TRM6 6 node isoparametric triangular membrane with varying thickness and plane strain options.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-14
ASAS (Non-Linear) User Manual                                                                               Appendix A


A.3.4         Finite Element Description Sheets

                                                                                                          Gap Elements
 GAP2                  2D/3D node-to-node interface/gap element.
 GAPX                  axisymmetric node-to-node interface/gap element.
 GAPR                  node-to-node radial interface/gap element




                                                                                                Beam/Stiffener Elements
 SST4       curved beam/stiffener element with thin-walled open section.
 STF4       curved beam/stiffener with solid rectangular, tube and box section.
 WST4       curved beam/stiffener element with thin-walled open section including warping.




                                                                                 Rigid Surface Interface Elements
 RGX3       rigid surface interface for use with axisymmetric elements TRX3 and QUX4.
 RGX4       rigid surface interface for use with axisymmetric elements TRX6 and QUX8.
 RG23       rigid surface interface for use with plane elements TRM3 and QUM4.
 RG24       rigid surface interface for use with plane elements TRM6 and QUM8.




                                                                                                          Shell Elements
 TCS6       6 node triangular element for modelling thick and thin shell applications.
 TCS8       8 node quadrilateral element for modelling thick and thin shell applications.
 TCS9       9 node quadrilateral element for modelling thick and thin shell applications.
 QUS4       4 node quadrilateral shell element for modelling thick and thin shell applications.

 Note all elements can have laminated composite material properties




                                                                                                        Special Elements
 SPR1       Translational spring element between 2 nodes with damper.
 SPR2       Rotational spring element between 2 nodes with damper.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-15
ASAS (Non-Linear) User Manual                                                                                  Appendix A


A.3.4         Finite Element Description Sheets

                                                                                                        Linespring Elements
LSP3     elasto-plastic line-spring element for use with high order shell elements for
         modelling surface flaws, symmetric boundary.
LSP6     elasto-plastic line-spring element for use with high order shell elements for
         modelling surface flaws.




                                                                                                  Uniaxial Field Elements
FAT2     2 node uniaxial field element with varying cross-section.
FAT3     3 node curved uniaxial field element with varying cross-section.




                                                                                                 3-D Solid Field Elements
BRT6     6 node straight edged wedge.
BRT8     8 node straight edged brick.
BT15     15 node wedge.
BT20     20 node brick.




                                                                                        Axisymmetric Field Elements
QXT4     Axisymmetric quadrilateral solid with straight or curved edges.
QXT8
TXT3     Axisymmetric triangular solid with straight or curved edges.
TXT6




                                                                                                2-D Plane Field Elements
QMT4 4 node quadrilateral membrane with varying thickness.
QMT8 8 node isoparametric quadrilateral membrane with varying thickness.
TMT3 3 node triangular membrane with varying thickness.
TMT6 6 node isoparametric triangular membrane with varying thickness.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-16
BEAM
ASAS (Non-Linear) User Manual                                                                               Appendix A



BEAM

    Three-dimensional Beam Bending Element with Uniform Cross-section and Special
                                               Orientation of the Local Axes

                                                                                                        1
NUMBER OF NODES                            2
                                                                                                                       2
NODAL COORDINATES                          x, y, z



DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node

GEOMETRIC PROPERTIES                       A             Cross-sectional area (≥ 0.0)
            (uniform)                      Iz”z”         Principal moment of inertia about the local Z” axis (≥ 0.0)
                                           Iy”y”         Principal moment of inertia about the local Y” axis (≥ 0.0)
                                           J             Torsion constant (≥ 0.0)


OFFSETS                                    The OFFG, OFFS, OFSK, OFCO commands can be used to define rigid offsets
                                           at each end. For further details see Section 5.2.5.5 and Appendix A.3.

MATERIAL MODEL                             ELASTIC           -   Isotropic

                                           PLASTIC           -   Stress resultant model based on generalised plastic hinge
                                                                 theory. Note that hinges can only form at nodes.
                                                                 See Appendix -B for details.

                                           Material properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Temperature loads
                                           Distributed load patterns               BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
                                                                                   GL1, GL4, GL5, GL6, GL7
                                                                                   GP1, GP4, GP6, GP7
                                           Body Forces
                                           Centrifugal Loads
                                           Angular Acceleration
                                           Wave load


MASS MODELLING                             Consistent Mass
                                           Lumped Mass (used by default)

FORCE OUTPUT                               The forces are exerted by the nodes on the element and related to the centroidal
                                           local axes.
                                           Axial Force X”X” at each end
                                           Transverse shears QY” and QZ” at each end
                                           Torque X”X” at each end
                                           Bending Moments Y”Y” and Z”Z” at each end

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-17
BEAM
ASAS (Non-Linear) User Manual                                                                          Appendix A


INTEGRATION RULES                          There are no integration points for the element, all the necessary element
                                           matrices being formed explicitly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-18
BEAM
ASAS (Non-Linear) User Manual                                                                                         Appendix A


LOCAL AXES                                 A beam element has two local axes systems. The X’Y’Z’ local axes are
                                           associated with end nodes of the element. The X”Y”Z” local axes are
                                           associated with the end points of the centroidal axis of the element, taking
                                           account of any non-zero rigid offsets.


                                           If all offsets are zero, X’Y’Z’ and X”Y”Z” are coincident.
                                           Geometric properties, distributed loads and output forces are all referred to the
                                           X”Y”Z” local axes.
                                           Local X” lies along the centroidal axis from end 1 towards end 2. Local Z”
                                           must lie in the global XY plane with +ve local Y” on the +ve side of the global
                                           XY plane. In the special case where local Y” is also in the global XY plane,
                                           local Y” must lie in the global Y direction. BM3D should be used for a beam
                                           with general orientation of local Z”.

                                           See also Section 5.2.5.5 and Appendix A.2.1.

SIGN CONVENTIONS                           Axial force                          positive for tension
                                           Shear force                          positive for end 2 sagging relative to end 1
                                           Torque                               positive for clockwise rotation of end 2
                                                                                relative to end 1, looking from end 1
                                                                                towards end 2
                                           Bending moment                       Positive for sagging
                                           Shear QY”      +ve                              Shear QZ”             +ve
                                           Moment Z”Z”                +ve                   Moment Y”Y”          +ve
                                               Y''                                           Z''

                                                        1                   2                           1              2
                                                                                    X''                                     X''




LIMITATIONS                                Length must be >0.0

REFERENCE                                  A.1

DATA EXAMPLES                              ELEM
                                           MATP             1
                                           BEAM             9    10     3
                                           BEAM         10       11     2
                                           END
                                           GEOM
                                           2         BEAM       27.1    1469.7         1614.1           2766.9
                                           3         BEAM       39.2    2006.3         1987.0           3124.8
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page A-19
BM2D
ASAS (Non-Linear) User Manual                                                                              Appendix A


              Two-dimensional Beam Bending Element with Uniform Cross-section,
                                Lying in the Global XY Plane

                                                                                                        Y

                                                                                                                     2
NUMBER OF NODES                            2


NODAL COORDINATES                          x, y
                                                                                                        1
                                           Option TWOD must be specified                                              X


DEGREES OF FREEDOM                         X, Y, RZ at each node


GEOMETRIC PROPERTIES                       A         Cross-sectional area (> 0.0)
                                           (uniform) Iz”z”
                                           Principal moment of inertia about the local Z” axis (> 0.0) Asy”Effective shear
                                           area (shear strain is neglected if Asy” is blank)

OFFSETS                                    The OFFG, OFFS, OFSK, OFCO commands may be used to define rigid
                                           offsets at each end. For further details see Appendix A.3 and Section 5.2.5.

MATERIAL MODEL                             ELASTIC           -   Isotropic

                                           PLASTIC           -   Stress resultant model based on generalised plastic hinge
                                                                 theory. Note that hinges can only form at nodes.
                                                                 See Appendix -B for details.

                                           Material properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Temperature loads
                                           Distributed load patterns               BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
                                                                                   GL1, GL4, GL5, GL6, GL7
                                                                                   GP1, GP4, GP6, GP7
                                           Body Forces
                                           Centrifugal Loads
                                           Angular Acceleration

MASS MODELLING                             Consistent Mass
                                           Lumped Mass (used by default)

FORCE OUTPUT                               The forces are exerted by the nodes on the element, and related to the local
                                           axes. Note that for an offset beam the forces output are related to the member
                                           centroidal axes.

INTEGRATION RULES                          There are no integration points for the element, all the necessary element
                                           matrices being formed explicitly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-20
BM2D
ASAS (Non-Linear) User Manual                                                                                   Appendix A


LOCAL AXES                                 The X’Y’ local axes are associated with the end nodes of the member. The
                                           X”Y” local axes are associated with the physical ends of the centroid of the
                                           member after taking account of any non-zero rigid offsets. If the offsets are all
                                           zero then X’Y’ and X”Y” are coincident.


                                           Local X’ (X”) lies along the element from node 1 (end1) towards node 2
                                           (end2). Local Z’ (Z”) must lie in the global Z direction. Local Y” forms a
                                           right handed set with local X” and local Z”

                                           The geometric properties Iz”z” and Asy” are related to X”Y” system. Distributed
                                           loads are also in the X”Y” system.

                                           See also section 5.2.5 and Appendix A.2.1

SIGN CONVENTIONS                           Axial force                   +ve for tension
                                           Shear force                   +ve for node 2 sagging relative to node 1
                                           Bending moment                +ve for sagging


                                                Y'

                                                                                           Shear QY”      +ve
                                                          1                  2
                                                                                      X'   Moment Z”Z”    +ve




LIMITATIONS                                Length must be >0.0

REFERENCE                                  A. 1

DATA EXAMPLE                               ELEM
                                           MATP       1
                                           BM2D       9       10     3
                                           /
                                           BM2D 10            11     2
                                           RP 6           1
                                           END
                                           GEOM
                                           2      BM2D        27.1       1469.7
                                           3      BM2D        39.2       2006.3        32.8
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page A-21
BM3D
ASAS (Non-Linear) User Manual                                                                               Appendix A


       Three-dimensional Beam Bending Element with Uniform Cross-section and any
                             Orientation of the Local Axes


                                                                                                        1
NUMBER OF NODES                            2
                                                                                                                       2
NODAL COORDINATES                          x, y, z

DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node

GEOMETRIC PROPERTIES                       A             Cross-sectional area (> 0.0)
                                                         (uniform)

                                           Iz”z”         Principal moment of inertia about the local Z” axis (> 0.0)
                                           Iy”y”         Principal amount of inertia about the local Y” axis (> 0.0)
                                           J         Torsion constant (> 0.0)
                                           Local Axis Definition - see Section 5.2.5.5 and Appendix A.2.1.
                                           Asy”          Effective shear area for forces in Y” direction
                                                         (Y” shear strain is neglected if Asy” is blank)
                                           Asz”          Effective shear area for forces in Z” direction
                                                         (Z” shear strain is neglected if Asz” is blank)

OFFSETS                                    The OFFG, OFFS, OFSK, OFCO commands may be used to define rigid
                                           offsets at each end. For further details see Appendix A.3 and Section 5.2.5.

MATERIAL MODEL                             ELASTIC           -   Isotropic

                                           PLASTIC           -   Stress resultant model based on generalised plastic hinge
                                                                 theory. Note that hinges can only form at nodes.
                                                                 See Appendix -B for details.

                                           Material properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Temperature loads
                                           Distributed load patterns               BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
                                                                                   GL1, GL4, GL5, GL6, GL7
                                                                                   GP1, GP4, GP6, GP7
                                           Body Forces
                                           Centrifugal Loads
                                           Angular Acceleration
                                           Wave load

MASS MODELLING                             Consistent Mass
                                           Lumped Mass (used by default)

FORCE OUTPUT                               The forces are exerted by the nodes on the element, and related to the local
                                           axes. Note that for an offset beam the forces output are related to the element
                                           centroidal axes.

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-22
BM3D
ASAS (Non-Linear) User Manual                                                                          Appendix A


INTEGRATION RULES                          There are no integration points for the element, all the necessary element
                                           matrices being formed explicitly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-23
BM3D
ASAS (Non-Linear) User Manual                                                                                        Appendix A


LOCAL AXES                                 The X’Y’Z’ local axes are associated with the end nodes of the member. The
                                           X”Y”Z” local axes are associated with the physical ends of the centroid of the
                                           member after taking account of any non-zero rigid offsets. If the offsets are all
                                           zero then X’Y’Z’ and X”Y”Z” are coincident.


                                           Local X’ (X”) lies from node 1 (end1) towards node 2 (end2). Local Y’ (Y”)
                                           lies in the plane defined by the two nodes (ends) and a third point defined in
                                           the Geometric Properties list. This third point must not lie on the X’ or X”
                                           axes. Local Y’ (Y”) lies from node 1 (end1) and is +ve towards the third point.
                                           Local Z’ (Z”) forms a right-handed set with local X’ (X”) and local Y’ (Y”).

                                           The geometric properties A, Iy”y”, Iz”z”, Asy”, Asz” and J all refer to the X”Y”Z”
                                           system. Distributed loads are also in the X”Y”Z” system.

                                           If a local axis definition is not supplied, a 3rd point with coordinates of 0.0,
                                           0.0, 0.0 is assumed.

                                           See also Section 5.2.5.5 and Appendix A.2.1

SIGN CONVENTIONS                           Axial force                                     +ve for tension
                                           Shear force                                     +ve for node 2 sagging relative to node 1
                                           Torque                                          +ve for anti-clockwise rotation at node
                                                                                           1 and clockwise rotation at node 2
                                                                                                 looking from node 1 towards node 2
                                           Bending moment                                  +ve for sagging

                                           Shear QY”              +ve                      Shear QZ”         +ve
                                           Moment Z”Z”            +ve                      Moment Y”Y”       +ve
                                            Y''                                                Z''

                                                       1                   2                            1                 2
                                                                                     X''                                            X''




LIMITATIONS                                Length must be >0.0

REFERENCE                                  A. 1

DATA EXAMPLE                               ELEM
                                           MATP 1
                                           BM3D            9     10   3
                                           /
                                           BM3D 10               11   2
                                           RP 6 1
                                           END
                                           GEOM
                                           3 BM3D              39.2   2006.3         1987.0          3124.8        -1.4       2.3
                                           :               -18.1          32.8             13.7
                                           END


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-24
BRK6
ASAS (Non-Linear) User Manual                                                                                                     Appendix A


                   Isoparametric Brick Element with Quasi-linear Strain Variation

                                                                                                         1
                                                                                                                                        2
NUMBER OF NODES                            6

NODAL COORDINATES                          x, y, z
                                                                                                                         3

DEGREES OF FREEDOM                         X, Y, Z at each node
                                                                                                     4
                                                                                                                                            5
GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            ELASTIC           -    Isotropic                                              6

                                                             -    Orthotropic
                                                             -    Woven
                                                             -    Anisotropic

                                                                  Anisotropic matrix (C or C-1) - referred to axis system
                                                                  selected for output (global by default)

                                                                 σxx                C1 C2       C4           C7    C11       C16            εxx
                                                                 σyy                . C3        C5           C8    C12       C17            εyy
                                                                 σzz                .   .       C6           C9    C13       C18            εzz
                                                                          =
                                                                 σxy                .   .        .           C10   C14       C19            εxy
                                                                 σyz                .   .        .            .    C15       C20            εyz
                                                                 σzx                .   .        .            .     .        C21            εzx


                                                                  6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
                                                                  referred to axis system selected for output.

                                                             -    Hyperelastic

                                           PLASTIC           -    von Mises, Tresca, Mohr-Coulomb, Drucker-Prager, Tension
                                                                  cut, yield criteria.
                                                                  Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                  Hardening.
                                           CREEP             -    von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                               Page A-25
BRK6
ASAS (Non-Linear) User Manual                                                                              Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to either global or
                                           local axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face

INTEGRATION RULES                          1x1x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ coincides with the (straight) line L1=0 +ve in the
                                           direction 1, 2. Local Y’ lies in the triangular plane L1L2L3 +ve towards node 3.
                                           Local Z’ forms a right-handed set with local X’ and local Y’. See Appendix -
                                           G for explanation of curvilinear axes.
SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz     +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-26
BRK8
ASAS (Non-Linear) User Manual                                                                                              Appendix A


                                           Isoparametric Brick Element with
                                             Quasi-linear Strain Variation

                                                                                                                                      2
                                                                                                        1
NUMBER OF NODES                            8
                                                                                                                        4                 3

NODAL COORDINATES                          x, y, z

DEGREES OF FREEDOM                         X, Y, Z at each node
                                                                                                                                  6
                                                                                                        5
GEOMETRIC PROPERTIES                       None

                                                                                                                  8                       7
MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic

                                                                 Anisotropic matrix (C or C-1) - referred to axis system
                                                                 selected for output (global by default)

                                                                  σxx                 C1 C2        C4       C7    C11       C16           εxx
                                                                  σyy                 . C3         C5       C8    C12       C17           εyy
                                                                  σzz        =        .   .        C6       C9    C13       C18           εzz
                                                                  σxy                 .   .         .       C10   C14       C19           εxy
                                                                  σyz                 .   .         .        .    C15       C20           εyz
                                                                  σzx                 .   .         .        .     .        C21           εzx


                                                                 6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
                                                                 referred to axis system selected for output.

                                                             -   Hyperelastic

                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 Tension cut, yield criteria.
                                                                 Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                 Hardening.
                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                         Page A-27
BRK8
ASAS (Non-Linear) User Manual                                                                              Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to either global or
                                           local axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face

INTEGRATION RULES                          2x2x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is coincident with curvilinear ξ. Local Y’ lies in the
                                           curvilinear ξη plane, +ve in the +ve η direction. Local Z’ forms a right-
                                           handed set with local X’ and local Y’. See Appendix -G for explanation of
                                           curvilinear axes.
SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz             +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-28
BR15
ASAS (Non-Linear) User Manual                                                                                           Appendix A


                Isoparametric Brick Element with Quasi-quadratic Strain Variation



NUMBER OF NODES                            15 (6 corner, 9 mid-side)

NODAL COORDINATES                          x, y, z
                                           (may be omitted for mid-side nodes on
                                           straight edges). The position of each
                                           mid-side node has a tolerance of side-
                                           length/10      about the        true     mid-side
                                           position.

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic

                                                                 Anisotropic matrix (C or C-1) - referred to axis system
                                                                 selected for output (global by default)


                                                                     σxx                 C1 C2          C4   C7    C11   C16      εxx
                                                                     σyy                 . C3           C5   C8    C12   C17      εyy
                                                                     σzz        =        .   .          C6   C9    C13   C18      εzz
                                                                     σxy                 .   .           .   C10   C14   C19      εxy
                                                                     σyz                 .   .           .    .    C15   C20      εyz
                                                                     σzx                 .   .           .    .     .    C21      εzx

                                                                 6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
                                                                 referred to axis system selected for output.

                                                             -   Hyperelastic

                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager Tension
                                                                 cut, yield criteria
                                                                 Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                 Hardening.
                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-29
BR15
ASAS (Non-Linear) User Manual                                                                              Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to either global or
                                           local axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face at a corner node

INTEGRATION RULES                          1x3x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is tangential to curvilinear L1 = constant +ve in the
                                           direction 1 to 2. Local Y’ is tangential to the curvilinear L1L2L3 surface, +ve
                                           towards node 5. Local Z’ forms a right-handed set with local X’ and local Y’.
                                           See Appendix -G for explanation of curvilinear axes.
SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz  +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-30
BR20
ASAS (Non-Linear) User Manual                                                                                           Appendix A


                Isoparametric Brick Element with Quasi-quadratic Strain Variation



NUMBER OF NODES                            20 (8 corner, 12 mid-side)

NODAL COORDINATES                          x, y, z
                                           (may be omitted for mid-side nodes on
                                           straight edges). The position of each
                                           mid-side node has a tolerance of side-
                                           length/10      about the        true    mid-side
                                           position.

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic

                                                                 Anisotropic matrix (C or C-1) - referred to axis system
                                                                 selected for output (global by default)


                                                                   σxx                  C1 C2           C4   C7    C11   C16        εxx
                                                                   σyy                  . C3            C5   C8    C12   C17        εyy
                                                                   σzz        =         .   .           C6   C9    C13   C18        εzz
                                                                   σxy                  .   .            .   C10   C14   C19        εxy
                                                                   σyz                  .   .            .    .    C15   C20        εyz
                                                                   σzx                  .   .            .    .     .    C21        εzx

                                                                 6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
                                                                 referred to axis system selected for output.

                                                             -   Hyperelastic

                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb,                         Drucker-Prager
                                                                 Tension cut, yield criteria.
                                                                 Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                 Hardening.
                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-31
BR20
ASAS (Non-Linear) User Manual                                                                              Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to either global or
                                           local axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
                                           corner node

INTEGRATION RULES                          2x2x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is tangential to and in the direction of curvilinear ξ.
                                           Local Y’ is tangential to the curvilinear ξη surface, +ve in the +ve η direction.
                                           Local Z’ forms a right-handed set with local X’ and local Y’.
                                           See Appendix -G for explanation of curvilinear axes.
SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz  +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-32
BRT6
ASAS (Non-Linear) User Manual                                                                              Appendix A


                    Isoparametric Field Brick Element with Quasi-linear Variation
                                          of Field Variable

                                                                                                  1
                                                                                                                2
NUMBER OF NODES                            6

NODAL COORDINATES                          x, y, z
                                                                                                        3

DEGREES OF FREEDOM                         T at each node
                                                                                              4
                                                                                                                    5
GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD                                                        6


                                           PIER

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal value related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradient
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face

INTEGRATION RULES                          1x1x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ coincides with the (straight) line L1=0 +ve in the
                                           direction 1, 2. Local Y’ lies in the triangular plane L1L2L3 +ve towards node 3.
                                           Local Z’ forms a right-handed set with local X’ and local Y’. See Appendix -
                                           G for explanation of curvilinear axes.

SIGN CONVENTIONS                           Fluxes and gradients positive when in the positive axis direction.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-33
BRT6
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4A. 4A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-34
BRT8
ASAS (Non-Linear) User Manual                                                                              Appendix A


                    Isoparametric Field Brick Element with Quasi-linear Variation
                                           of Field Variable



NUMBER OF NODES                            8

NODAL COORDINATES                          x, y, z

DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal values related to the field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at the integration points related to either the
                                           local or global axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
                                           corner node

INTEGRATION RULES                          2x2x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is coincident with curvilinear ξ. Local Y’ lies in the
                                           curvilinear ξη plane, +ve in the +ve η direction. Local Z’ forms a right-
                                           handed set with local X’ and local Y’. See Appendix -G for explanation of
                                           curvilinear axes.

SIGN CONVENTIONS                           Fluxes and gradients are positive when in the positive axis direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-35
BRT8
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-36
BT15
ASAS (Non-Linear) User Manual                                                                              Appendix A


                 Isoparametric Field Brick Element with Quasi-quadratic Variation
                                         of Field Variable



NUMBER OF NODES                            15 (6 corner, 9 mid-side)

NODAL COORDINATES                          x, y, z
                                           (may be omitted for mid-side nodes on
                                           straight edges). The position of each
                                           mid-side node has a tolerance of side-
                                           length/10 about the true mid-side
                                           position.

DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal values related to the field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at the integration points related to either the
                                           local or global axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face at a corner node

INTEGRATION RULES                          1x3x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is tangential to curvilinear L1 = constant +ve in the
                                           direction 1 to 2. Local Y’ is tangential to the curvilinear L1L2L3 surface, +ve
                                           towards node 5. Local Z’ forms a right-handed set with local X’ and local Y’.
                                           See Appendix -G for explanation of curvilinear axes.

SIGN CONVENTIONS                           Fluxes and gradients are positive when in the positive axis direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-37
BT15
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-38
BT20
ASAS (Non-Linear) User Manual                                                                              Appendix A


                 Isoparametric Field Brick Element with Quasi-quadratic Variation
                                         of Field Variable



NUMBER OF NODES                            20 (8 corner, 12 mid-side)

NODAL COORDINATES                          x, y, z
                                           (may be omitted for mid-side nodes on
                                           straight edges). The position of each
                                           mid-side node has a tolerance of side-
                                           length/10 about the true mid-side
                                           position.

DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal values related to the field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at the integration points related to either the
                                           local or global axes (global by default)

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
                                           corner node

INTEGRATION RULES                          2x2x2 Gauss quadrature by default. Higher order rules by request.
                                           Appendix -G gives positions of integration points.

LOCAL AXES                                 At any point local X’ is tangential to and in the direction of curvilinear ξ.
                                           Local Y’ is tangential to the curvilinear ξη surface, +ve in the +ve η direction.
                                           Local Z’ forms a right-handed set with local X’ and local Y’.
                                           See Appendix -G for explanation of curvilinear axes.

SIGN CONVENTIONS                           Fluxes and gradients positive when in the positive axis direction.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-39
BT20
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-40
FAT2
ASAS (Non-Linear) User Manual                                                                              Appendix A


                              Straight Field Axial Element with Linear Variation
                                               of Field Variable

                                                                                                                   2
NUMBER OF NODES                            2
                                                                                                        1
NODAL COORDINATES                          x, y, z
                                           z should be omitted for 2D problems

DEGREES OF FREEDOM                         T at each node.

GEOMETRIC PROPERTIES                       A1            Cross-sectional area at node 1
                                           A2            Cross-sectional area at node 2
                                                     (The cross-sectional area varies linearly between node 1 and node 2.
                                           The value A2 may be omitted for an element with uniform area A1).

MATERIAL MODELS                            FIELD

                                           PIER

                                           CVEC

                                           RADI

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal values related to the field variable type
                                           Prescribed field variable
                                           Temperature

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at the integration points related to the local
                                           axes

INTEGRATION RULE                           Not appropriate, explicit integration assuming constant field variable is used.

LOCAL AXES                                 Local X’ lies along the element from node 1 towards node 2.

SIGN CONVENTIONS                           Fluxes and gradients positive when in the positive axis direction.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-41
FAT2
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details

4.     For heat conduction analysis, this element may be used to model convection by specifying directive FLNS
       in the PROB/TITL or GROUP commands. In this case, the first material property specified will have the
       meaning of a heat transfer (or film) coefficient and the length of an element will not enter into the heat flow
       calculations. All FAT2 elements in the same group are so treated.

5.     The convective and radiant heat transfer can be modelled directly using the CVEC and RADI material
       models, respectively. The length of an element will not enter into the calculations with these 2 models.

6.     The area required for the RADI model is the direct interchange area. This is defined to the product of the
       geometric view factor and the emitting surface area.


REFERENCE                                  A. 1, A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-42
FAT3
ASAS (Non-Linear) User Manual                                                                                  Appendix A


                           Curved Axial Field Element with Quadratic Variation
                                             of Field Variable



NUMBER OF NODES                            3                                                                2        3

NODAL COORDINATES                          x, y, z
                                                                                                        1
                                           z should be omitted for 2D problems

DEGREES OF FREEDOM                         T at each node.

GEOMETRIC PROPERTIES                       A1            Cross-sectional area at node 1
                                           A2            Cross-sectional area at node 2
                                           A3            Cross-sectional area at node 3
                                                         (The cross-sectional area varies quadratically between node 1,
                                                         node 2 and node 3. The values A2 and A3 may be omitted for an
                                                         element with uniform area A1).

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material properties can be temperature dependent if required

LOAD TYPES                                 Nodal values related to the field variable type
                                           Prescribed field variable
                                           Temperature

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at the integration points related to the local
                                           axes

INTEGRATION RULE                           2 point integration assuming linear variation of the field variable

LOCAL AXES                                 Local X’ lies along the element axis from node 1 towards node 3.

SIGN CONVENTIONS                           Fluxes and gradients positive when in the positive axis direction.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-43
FAT3
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 1, A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-44
FLA2
ASAS (Non-Linear) User Manual                                                                              Appendix A


                                   Straight Axial Element with Constant Strain



NUMBER OF NODES                            2                                                                              2

NODAL COORDINATES                          x, y, z                                                      1
                                           z should be omitted
                                           2D problems

DEGREES OF FREEDOM                         X, Y, (Z) at each node.
                                           Option TWOD converts to 2-D form, freedoms X, Y only.

GEOMETRIC PROPERTIES                       There are two types of geometric properties available:

                                           (a)       Cross-sectional areas at nodes 1 and 2, no keyword required with
                                           geometric property data

                                                         A1 Cross-sectional area at node 1
                                                         A2 Cross-sectional area at node 2
                                                         (The cross-sectional area varies linearly between node 1 and
                                                              node 2. The value A2 may be omitted for an element with
                                                              uniform area A1).

                                           (b)           Cross-sectional areas at nodes 1 and 2 plus keyword CABL on
                                                         a continuation line to invoke the conversion to a tension only
                                                              (cable formulation)

                                                         A1 Cross-sectional area at node 1
                                                         A2 Cross-sectional area at node 2
                                                         (The cross-sectional area varies linearly between node 1 and
                                                              node 2. The value A2 may be omitted for an element with
                                                              uniform area A1).

                                                         The geometric property data required following the keyword CABL
                                           are:

                                                         Te     -   erection tension
                                                         m      -   mass unit per length
                                                         g      -   acceleration due to gravity
                                                         Cd     -   coefficient of drag
                                                         ρa     -   mass per unit volume for air
                                                         d      -   cable diameter
                                                         V      -   magnitude of wind velocity
                                                         α      -   bearing of V from the global XZ plane
                                                         β      -   bearing of V from the global XY plane
                                                         a      -   load stiffness




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-45
FLA2
ASAS (Non-Linear) User Manual                                                                                Appendix A


MATERIAL MODELS                            ELASTIC           -        Isotropic
                                                             -        Hyperelastic
                                           PLASTIC           -        von Mises, Tresca, Mohr-Coulomb, Drucker-Prager,
                                                                      Tension cut, yield criteria
                                                                      Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                      Hardening.
                                           CREEP             -        von Mises.


                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Temperature loads (Not valid with CABL properties)
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations

MASS MODELLING                             Lumped mass (used by default)
                                           Consistent mass

OUTPUT                                     Stresses and strains are available for the centre of the element
                                           (in local axes).

INTEGRATION RULE                           Not appropriate, explicit integration assuming constant stress is used.

LOCAL AXES                                 Local X’ lies along the element from node 1 towards node 2.

SIGN CONVENTION                            Axial stress +ve for tension.

NOTES

1.     Any group containing FLA2 elements must contain only FLA2 elements.

2.     The stiffness E(A1 + A2)/2L of the element can be set to E(A1 + A2)/2, thereby allowing the elastic (natural)
       stiffness to be unchanged by large deformations. This is accomplished by directive FLNS using the
       PROB/TITL or GROUP commands. All FLA2 elements in the same group are so treated.


REFERENCE                                  A. 1, A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-46
GAP2
ASAS (Non-Linear) User Manual                                                                               Appendix A


                                   Interface/Gap Element with Sliding Capacity

                                                                                                         2
NUMBER OF NODES                            2

NODAL COORDINATES                          x, y, z
                                           z should be omitted for 2D problems                                            1


DEGREES OF FREEDOM                         X, Y, (Z) at each node.
                                           Option TWOD converts to 2-D form, freedoms X, Y only.

GEOMETRIC PROPERTIES                       GAP           The initial size of the gap. (GAP ≤ 0.0 assumes an initial
                                                         gap closed condition and GAP will be reset to zero internally)
                                           MUY           Coefficient of friction in local Y’-direction
                                           MUZ           Coefficient of friction in local Z’-direction, zero for TWOD
                                           XG            X component of vector defining the gap reference axis
                                           YG            Y component of vector defining the gap reference axis
                                           ZG            Z component of vector defining the gap reference axis
                                           KN            Normal contact stiffness factor (see note 4)
                                           KT            Tangential stick stiffness factor (see note 5)
                                           KR            Gap residual stiffness factor (see note 6)
                                           C             Damping coefficient

MATERIAL MODELS                            Elastic only. K - the effective contact stiffness is given in the material
                                                             property data (see note 3)

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP, in the X’-direction and sliding displacements SLIDE-Y
                                           and SLIDE-Z are related to local axes. Force across the gap, Fx’x’, and
                                           frictional forces Fy’y’ and Fz’z’ are related to the local axes. STATUS refers to
                                           the status of the element at the last iteration.
                                           Both STRS and STRN should be specified using the corresponding BLOC
                                           command to obtain gap output.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-47
GAP2
ASAS (Non-Linear) User Manual                                                                              Appendix A


LOCAL AXES                                 Local X’ lies along the gap reference axis (see note 1). Local Y’ lies in the
                                           global xy plane, perpendicular to local X’. (If local X’ is parallel to global z,
                                           then local Y’ lies in the global xy plane in the negative x direction). Local Z’
                                           forms a right-handed set with local X’ and local Y’.


SIGN CONVENTIONS                           Force Fx’x’ tending to open gap is positive.
                                           GAP is positive if gap is open.

NOTES

1.     The gap reference axis defines the direction of the gap surface, which is assumed to be in a plane
       perpendicular to this axis. If this is specified as {0.0, 0.0, 0.0}, the gap reference axis will be assumed to
       lie along the element from node 1 to node 2. In this case, nodes 1 and 2 must not be coincident.

2.     GAP elements cannot be placed with other types of element in the same group.

3.     The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
       elastic modulus and A is the effective area at the contact node.

4.     When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
       specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000).

5.     When the gap is closed and stick, the tangential stick stiffness betweeen the two nodes is computed as
       KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
       command (default 1000).

6.     When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
       KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
       command (default 10-8).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.         Page A-48
GAPR
ASAS (Non-Linear) User Manual                                                                                    Appendix A


                                     Radial Gap Element with Sliding Capacity

                                                                                   GAP > 0.0                  GAP < 0.0
NUMBER OF NODES                            2



                                                                                           2                           2
NODAL COORDINATES                          x, y, z                                 1

DEGREES OF FREEDOM                         X, Y, Z

MATERIAL MODELS                            Elastic only -
                                                                                                         the effective stiffness, K
                                                                                                                      (see note 4)

GEOMETRIC PROPERTIES                       GAP           Gap parameter (see note 2)
                                           MUY           Coefficient of friction in local Y’ direction
                                           MUZ           Coefficient of friction in local Z’ direction
                                           XG            X component of vector defining the gap reference axis
                                           YG            Y component of vector defining the gap reference axis
                                           ZG            Z component of vector defining the gap reference axis
                                           KN            Normal contact stiffness factor (see note 5)
                                           KT            Tangential stick stiffness factor (see note 6)
                                           KR            Gap residual stiffness factor (see note 7)
                                           C             Damping coefficient

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP in the X’ direction and sliding displacements SLIDE-Y and
                                           SLIDE-Z are related to the local axes. Forces across the gap Fx’x’ and frictional
                                           forces Fy’y’ and Fz’z’ are related to the local axes. STATUS refers to the status
                                           of the element at the last iteration. STATUS = 1 for no contact, = 2 for contact
                                           and stick, = 5 for contact and slide. Both STRS and STRN should be specified
                                           using the corresponding BLOC command to obtain gap output.

LOCAL AXES                                 Local Z’ axis is the gap reference axis (see note 3). Local X’ lies from node 1
                                           to node 2 and on the normal plane to local Z’. Local Y’ is also on the normal
                                           plane to local Z’ and perpendicular to local X’.

SIGN CONVENTIONS                           Force Fx’x’ tending to open gap is positive. GAP is positive if gap is open.

Notes


1.      Gap elements cannot be placed with other types of element in the same group.

2.      The gap parameter is used to define the position and diameter of the tubes (plus any non-structural
        coatings, etc).

        a) Tube in Tube configuration.
        The parameter is used to define the distance (gap) between the outer diameter of the inner tube and the

Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-49
GAPR
ASAS (Non-Linear) User Manual                                                                          Appendix A


       inner diameter of the outer tube. Hence the value entered ought to equal the outer tube’s inner radius less
       the inner tube’s outer radius. Allowance will be automatically be made if the nodes are not coincident.


       b) Two separate tubes configuration.
       To indicate that this is the case, the sign of this parameter must be negative. The magnitude of the
       parameter is used to define the distance (gap) between nodes below which contact will occur. Hence the
       the value will be equal to the sum of the two outer radii.

3.     The gap reference axis defines the direction that is normal to the contact plane. If this is specified as {0.0,
       0.0, 0.0}, the gap reference axis will be assumed to be in the global Z direction (i.e. the contact plane is the
       global X-Y plane).

4.     The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
       elastic modulus and A is the effective area at the contact node.

5.     When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
       specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000).

6.     When the gap is closed and stick, the tangential stick stiffness betweeen the two nodes is computed as
       KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
       command (default 1000).

7.     When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
       KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
       command (default 10-8).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-50
GAPX
ASAS (Non-Linear) User Manual                                                                                Appendix A


                       Axisymmetric Interface/Gap Element with Sliding Capacity


                                                                                                              2
NUMBER OF NODES                            2

NODAL COORDINATES                          r, z                                                                           1
                                                                                                          Z
                                           (Note that r and z occupy the first and third
                                           fields with coordinate data using an
                                           unnamed cartesian system).
                                                                                                                    R

DEGREES OF FREEDOM                         R, Z at each node.
                                           Any skew system must be 2-D.

GEOMETRIC PROPERTIES                       GAP           The initial size of the gap. (GAP ≤ 0.0 assumes an initial
                                                         gap closed condition and GAP will be reset to zero internally)
                                           MUY           Coefficient of friction in local Y’-direction
                                           MUZ           Coefficient of friction in local Z’-direction (always ignored)
                                           XG            X component of vector defining the gap reference axis
                                           YG            Y component of vector defining the gap reference axis (always
                                                         assumed zero)
                                           ZG            Z component of vector defining the gap reference axis
                                           KN            Normal contact stiffness factor (see note 4)
                                           KT            Tangential stick stiffness factor (see note 5)
                                           KR            Gap residual stiffness factor (see note 6)
                                           C             Damping coefficient

MATERIAL MODELS                            Elastic only. K - the effective contact stiffness is given in the material property
                                           data (see note 3)

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP, in the X’-direction and sliding displacements SLIDE-Y are
                                           related to local axes. Force across the gap, Fx’x’, and frictional force Fy’y’ are
                                           related to the local axes. STATUS refers to the status of the element at the last
                                           iteration. Both STRS and STRN should be specified using the corresponding
                                           BLOC command to obtain gap output.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-51
GAPX
ASAS (Non-Linear) User Manual                                                                             Appendix A


LOCAL AXES                                 Local X’ lies along the gap reference axis (see note 1). Local Y’ lies in the
                                           global rz plane, perpendicular to local X’.


SIGN CONVENTIONS                           Force Fx’x’ tending to open gap is positive. GAP is positive if gap is open.

NOTES

1.     The gap reference axis defines the direction of the gap surface, which is assumed to be in a plane
       perpendicular to this axis. If this is specified as {0.0, 0.0, 0.0}, the gap reference axis will be assumed to
       lie along the element from node 1 to node 2. In this case, nodes 1 and 2 must not be coincident.

2.     GAP elements cannot be placed with other types of element in the same group.

3.     The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
       elastic modulus and A is the effective area at the contact node.

4.     When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
       specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000)

5.     When the gap is closed and stick, the tangential stick stiffness between the two nodes is computed as
       KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
       command (default 1000).

6.     When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
       KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
       command (default 10-8).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-52
LB15
ASAS (Non-Linear) User Manual                                                                            Appendix A


                    Isoparametric Laminated Brick Element with Quasi-quadratic
                                         Strain Variation



NUMBER OF NODES                            15 (6 corner, 9 mid-side)

NODAL COORDINATES                          x, y, z
                                           (may be omitted for mid-side nodes on
                                           straight edges). The position of each
                                           mid-side node has a tolerance of side-
                                           length/10 about the true mid-side
                                           position.

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       Lay up data. See Section 5.2.5.3.
                                           The layers are stacked from the bottom surface
                                           up. The bottom surface is defined as the first face
                                           formed by the local node numbering (the face formed
                                           by nodes 1-6 in this case).

MATERIAL MODELS                            ELASTIC           -   Laminated

                                           FAIL              -   Lamina failure law for composites.

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to the principal
                                           material axes of each layer

                                           For failure analysis, the equivalent stress at each integration point is also
                                           available. This is defined as:

                                           SEQ=10*mode+f

                                           where f is the failure function value and mode is the failure mode integer.

                                           mode         = 0, elastic
                                                        = 4, fibre failure


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-53
LB15
ASAS (Non-Linear) User Manual                                                                           Appendix A


                                                         = 5, matrix failure
                                                         = 6, lamina failure
                                                         = 7, transverse shear/normal stress failure
                                                         = 8, modes 5 and 7


NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
                                           a triangular face at a corner node

INTEGRATION RULES                          1x3x1 Gauss quadrature for each layer by default. If the element contains one
                                           single layer only, then the default is 1x3x3, where Gauss quadrature is used for
                                           the in-plane integration and Newton-Coates for through thickness integration.
                                           Other rules by request.
                                           Appendix -G gives positions of integration points.
                                           Note that the integration order specified in the preliminary data is the rule
                                           adopted for each layer.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page A-54
LB15
ASAS (Non-Linear) User Manual                                                                          Appendix A


SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz             +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-55
LB20
ASAS (Non-Linear) User Manual                                                                            Appendix A


                    Isoparametric Laminated Brick Element with Quasi-quadratic
                                         Strain Variation

NUMBER OF NODES                            20 (8 corner, 12 mid-side)

NODAL COORDINATES                          x, y, z (may be omitted for mid-
                                           side nodes on straight edges).
                                           The position of each mid-side
                                           node has a tolerance of side/10
                                           about the true mid-side position.

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       Lay up data. See Section 5.2.5.3.
                                           The layers are stacked from the bottom surface
                                           up. The bottom surface is defined as the first face
                                           formed by the local node numbering (the face formed
                                           by nodes 1-8 in this case).

MATERIAL MODELS                            ELASTIC           -   Laminated

                                           FAIL              -   Lamina failure law for composites

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (on any face, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points related to the principal
                                           material axes of each layer.

                                           For failure analysis, the equivalent stress at each integration point is also
                                           available. This is defined as:

                                           SEQ=10*mode+f

                                           where f is the failure function value and mode is the failure mode integer.

                                           mode         = 0, elastic
                                                        = 4, fibre failure
                                                        = 5, matrix failure
                                                        = 6, lamina failure


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-56
LB20
ASAS (Non-Linear) User Manual                                                                            Appendix A


                                                         = 7, transverse shear/normal stress failure
                                                         = 8, modes 5 and 7



NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
                                           corner node

INTEGRATION RULES                          2x2x1 Gauss quadrature for each layer by default. If the element contains one
                                           single layer only, then the default is 2x2x3, where Gauss quadrature is used for
                                           the in-plane integration and Newton-Coates for through thickness integration.
                                           Other rules by request.
                                           Appendix -G gives positions of integration points.
                                           Note that the integration order specified in the preliminary data is the rule
                                           adopted for each layer.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-57
LB20
ASAS (Non-Linear) User Manual                                                                          Appendix A


SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz             +ve for tension
                                           Shear stresses σxy, σyz, σzx              +ve as shown




REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-58
LSP3
ASAS (Non-Linear) User Manual                                                                                  Appendix A


                Line-Spring Element Compatible with Quadratic Shell Elements for
                       Modelling Surface Flaws with Symmetry Boundary

NUMBER OF NODES                            3

NODAL COORDINATES                          x, y, z
                                                                                                                     3
                                                                                                            2
DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ
                                                                                                        1
GEOMETRIC PROPERTIES                       d1            Crack depth at node 1
                                           t1            Shell thickness at node 1
                                           d2            Crack depth at node 2
                                           t2            Shell thickness at node 2
                                           d3            Crack depth at node 3
                                           t3            Shell thickness at node 3
                                           x1, y1, z1 Orientation node coordinates for node 1
                                           x2, y2, z2 Orientation node coordinates for node 2
                                           x3, y3, z3 Orientation node coordinates for node 3
                                           The orientation node is a node in the plane of the crack, pointing in the
                                           direction of the surface from which the crack originates.
                                           (Note - d is +ve if a flaw lies on the +ve Z’ side and vice versa)

MATERIAL MODELS                            ELASTIC           -   Isotropic only

                                           PLASTIC           -   von Mises yield criterion
                                                                 Isotropic hardening only

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements

MASS MODELLING                             No mass

OUTPUT                                     Forces and moments per unit length of flaw for fracture modes I, II and III and
                                           the associated relative displacements and rotations are available at all
                                           integration points. In addition, the mode I, II and III stress intensity factors,
                                           the plastic part of the J-integral and the total J are also printed at each
                                           integration point.

INTEGRATION RULES                          3 point Simpson’s rule along the flaw (i.e. 3x1x1) and this cannot be changed.

LOCAL AXES                                 Local X’ axis is tangential to the curvilinear ξ axis, positive in the direction of
                                           node 1 to node 3. The local Y’ axis lies in the plane through the orientation
                                           node and the local X’ axis, positive towards the orientation node. Local Z’
                                           forms a right handed set with local X’ and local Y’.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-59
LSP3
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     The element is written for small displacement analysis only, i.e. large displacement effects are not included
        and should not be specified.

2.      Thermal strain effects are not included.

3.      Plasticity is included for mode I response only, so that elasto-plastic analysis should only be carried out
       with LSP3 or with LSP6 when mode I behaviour dominates. Significant approximations have been made
       in the plasticity model and therefore this should be used with care.

4.     The amount of plastic work of the numerical model can be adjusted using the PARA command FACLSP
       (default 0.4) to provide a matching to the experiment results for an edge-cracked specimen.


REFERENCE                                  A. 6        , A. 7




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-60
LSP6
ASAS (Non-Linear) User Manual                                                                                  Appendix A


     Line-Spring Element Compatible with Quadratic Shell Elements for
                             Modelling Surface Flaws
NUMBER OF NODES                            6
                                                                                                                             6
                                                                                                                   5
NODAL COORDINATES                          x, y, z
                                                                                                                                 3
                                                                                                        4          2
DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ
                                                                                                            1
GEOMETRIC PROPERTIES                       d1            Crack depth at node 1
                                           t1            Shell thickness at node 1
                                           d2            Crack depth at node 2
                                           t2            Shell thickness at node 2
                                           d3            Crack depth at node 3
                                           t3         Shell thickness at node 3
                                           x1, y1, z1 Orientation node coordinates for node 1
                                           x2, y2, z2 Orientation node coordinates for node 2
                                           x3, y3, z3 Orientation node coordinates for node 3
                                           The orientation node is a node in the plane of the crack, pointing in the
                                           direction of the surface from which the crack originates.
                                           (Note - d is +ve if a flaw lies on the +ve Z’ side and vice versa)

MATERIAL MODELS                            ELASTIC           -   Isotropic only

                                           PLASTIC           -   von Mises yield criterion
                                                                 Isotropic hardening only

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements

MASS MODELLING                             No mass

OUTPUT                                     Forces and moments per unit length of flaw for fracture modes I, II and III and
                                           the associated relative displacements and rotations are available at all
                                           integration points. In addition, the mode I, II and III stress intensity factors,
                                           the plastic part of the J-integral and the total J are also printed at each
                                           integration point.

INTEGRATION RULES                          3 point Simpson’s rule along the flaw (i.e. 3x1x1) and this cannot be changed.

LOCAL AXES                                 Local X’ axis is tangential to the curvilinear ξ axis, positive in the direction of
                                           node 1 to node 3. The local Y’ axis lies in the plane through the orientation
                                           node and the local X’ axis, positive towards the orientation node. Local Z’
                                           forms a right handed set with local X’ and local Y’.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-61
LSP6
ASAS (Non-Linear) User Manual                                                                          Appendix A



NOTES
1.     The element is written for small displacement analysis only, i.e. large displacement effects are not included
       and should not be specified.

2.     Thermal strain effects are not included.

3.     Plasticity is included for mode I response only, so that elasto-plastic analysis should only be carried out
       with LSP3 or with LSP6 when mode I behaviour dominates. Significant approximations have been made
       in the plasticity model and therefore this should be used with care.

4.     The amount of plastic work of the numerical model can be adjusted using the PARA command FACLSP
       (default 0.4) to provide a matching to the experiment results for an edge-cracked specimen.


REFERENCE                                  A. 6        , A. 7




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-62
QMT4
ASAS (Non-Linear) User Manual                                                                                          Appendix A


                Quadrilateral Membrane Field Element with Quasi-linear Variation
                                      of Field Variable

NUMBER OF NODES                            4

NODAL COORDINATES                          x, y, (z)
                                           z should be omitted for 2-D problems.

DEGREES OF FREEDOM                         T at each node.

GEOMETRIC PROPERTIES                       ti Thickness at node i (i=1,4),
                                           t2 to t4 may be omitted for an element with
                                           uniform thickness t1.

                                           No geometric property required with PLSN option. In this case, the geometric
                                           property integer in the topology data should also be omitted.


MATERIAL MODELS                            FIELD

                                           PIER

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal values related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (local by default).

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
                                           position of integration points.
                                                                                                 Y'                 3

LOCAL AXES                                 Invariant throughout element. Local
                                           X’ lies along the straight line from            4                    σx'y'
                                           node 1 towards node 2. Local Y’ is
                                                                                                                        σx'x'
                                           in the plane of the element
                                           perpendicular to local X’ and +ve
                                           towards node 3. Local Z’ forms a                             σy'y'
                                                                                                                                    X'
                                           right-handed set with local X’ and                   1                               2
                                           local Y’.

SIGN CONVENTION                            Fluxes and gradients are positive when in the positive axis direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      Page A-63
QMT4
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-64
QMT8
ASAS (Non-Linear) User Manual                                                                                  Appendix A


 Isoparametric Quadrilateral Membrane Field Element with Quasi-quadratic Variation
                                 of Field Variable
                                                                                                                       6
NUMBER OF NODES                            8                                                            7
                                                                                                                                        5
NODAL COORDINATES                          x, y, (z)
                                           z should be omitted for 2D problems.
                                           Coordinates may be omitted for mid-                              8                       4
                                           side nodes on straight edges, but if
                                           given each node must be within side/10
                                           of the true mid-side.                                                                3
                                                                                                                1          2
DEGREES OF FREEDOM                         T at each node.

GEOMETRIC PROPERTIES                       ti Thickness at node i (i=1,8)
                                           t2 to t8 may be omitted for an element with uniform thickness t1.

                                           No geometric property required with PLSN option. In this case, the geometric
                                           property integer in the topology data should also be omitted.


MATERIAL MODELS                            FIELD

                                           PIER

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal values related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (local by default).

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
                                           position of integration points.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-65
QMT8
ASAS (Non-Linear) User Manual                                                                            Appendix A


LOCAL AXES                                 Local X’ lies on the element surface. For
                                           flat elements, it is a straight line parallel to
                                           a line through nodes 1 and 3.                     For
                                           elements curved out-of-plane, it is the
                                           intersection of the element surface with
                                           the plane containing the surface normal
                                           and the straight line through nodes 1 and
                                           3.    Local Y’ is in the surface,
                                           perpendicular to local X’ and +ve towards
                                           node 5. Local Z’ forms a right-handed set
                                           with local X’ and local Y’.



SIGN CONVENTION                            Fluxes and gradients are positive when in the positive axis direction

NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-66
QUM4
ASAS (Non-Linear) User Manual                                                                                        Appendix A


               Quadrilateral Membrane Element with Quasi-linear Strain Variation

This element can be used for both plane strain and plane stress applications in two and three dimensions.


REQUIRED OPTIONS                           PLSN       - 2-D Classical Plane Strain (εz = 0.0)
                                           EPSN       - 2-D Engineering Plane Strain (εz = const.)
                                           TWOD - 2-D Plane Stress
                                           none - 3-D Plane Stress                                            4                    3



NUMBER OF NODES                            4

NODAL COORDINATES                          x, y, (z)
                                           z should be omitted for plane strain
                                           and 2-D plane stress forms.
                                                                                                                  1         2
DEGREES OF FREEDOM                         X Y, for Plane Strain and 2-D plane
                                           stress forms.

                                           X,Y,Z for 3-D Plane stress.
                                           Deformations out-of-plane must be suppressed or restrained by adjacent
                                           elements.

GEOMETRIC PROPERTIES                       Plane strain      -   None (the geometric property integer with the element
                                                                 topology data should also be omitted)

                                           Plane stress      -   ti Thickness at node i (i=1,4),
                                                                 t2 to t4 may be omitted for an element with uniform
                                                                 thickness t1.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (or C-1) defined in axis system
                                                                 selected for output.
                                                                 σxx                C1 C2        C4     C7            εxx
                                                                 σyy        =       .  C3        C5     C8            εyy
                                                                 σxy                .   .        C6     C9            εxy
                                                                 σzz                .   .         .     C10           εzz


                                                                 4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
                                                                 referred to axis system selected for output

                                                             -   Hyperelastic




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page A-67
QUM4
ASAS (Non-Linear) User Manual                                                                             Appendix A


                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager      yield
                                                                 criteria
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.

                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal Loads
                                           Prescribed displacements
                                           Edge pressure loads (on any side, +ve towards the element centre)
                                           Normal pressure loads (+ve for +ve local z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points referred to either global
                                           or element local axes (local by default). Note global should not be used with
                                           elements in the 3-D Plane stress form.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Invariant throughout element. Local
                                           X’ lies along the straight line from
                                           node 1 towards node 2. Local Y’ is
                                           in the plane of the element
                                           perpendicular to local X’ and +ve
                                           towards node 3. Local Z’ forms a
                                           right-handed set with local X’ and
                                           local Y’.

SIGN CONVENTION                            Direct stresses σxx, σyy, σzz                +ve for tension
                                           Shear stress σxy                             +ve as shown




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-68
QUM4
ASAS (Non-Linear) User Manual                                                                          Appendix A

NOTES

1.      With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
        on the structure), is automatically added to the structure. The node has εz as its only freedom, which is
       reported in the displacement output. As this extra node is common to all elements, εz is constant for the
       entire structure.

2.     2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
       required.


REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-69
QUM8
ASAS (Non-Linear) User Manual                                                                                            Appendix A


       Isoparametric Quadrilateral Membrane with Quasi-quadratic Strain Variation

This element can be used for both plane strain and plane stress applications in two and three dimensions.

REQUIRED OPTIONS                           PLSN       - 2-D Classical Plane Strain (εz = 0.0)
                                           EPSN - 2-D Engineering Plane Strain (εz = const.)
                                           TWOD - 2-D Plane Stress
                                           none       - 3-D Plane Stress                                                   6
                                                                                                        7
NUMBER OF NODES                            8                                                                                               5

NODAL COORDINATES                          x, y, (z)
                                           z should be omitted for plane strain and                         8                          4
                                           2-D plane stress forms.
                                           Coordinates may be omitted for mid-
                                           side nodes on straight edges, but if
                                                                                                                                   3
                                           given each node must be within side/10                               1              2
                                           of the true mid-side.

DEGREES OF FREEDOM                         X, Y for Plane strain and 2-D Plane stress forms
                                           X, Y, Z for 3-D Plane stress.
                                           Deformations out-of-plane must be suppressed or restrained by adjacent
                                           elements.

GEOMETRIC PROPERTIES                       Plane strain      - None (the geometric property integer with the topology
                                                                 data should also be omitted).

                                           Plane stress      - ti Thickness at node i (i=1,8), t2 to t8 may be omitted for
                                                                 an element with uniform thickness t1.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (or C-1) defined in axis system
                                                                 selected for output

                                                           σxx                C1 C2        C4     C7                εxx
                                                           σyy        =       .  C3        C5     C8                εyy
                                                           σxy                .   .        C6     C9                εxy
                                                           σzz                .   .         .     C10               εzz




                                                                 4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
                                                                 referred to axis system selected for output.

                                                             -   Hyperelastic




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      Page A-70
QUM8
ASAS (Non-Linear) User Manual                                                                             Appendix A


                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager      yield
                                                                 criteria
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.

                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal Loads
                                           Prescribed displacements
                                           Edge pressure loads (on any side, +ve towards the element centre)
                                           Normal pressure loads (+ve for +ve local z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads
                                           Body forces
                                           Centrifugal forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points referred to either global
                                           or element local axes (local by default). Note global should not be used with
                                           elements in the 3-D Plane stress form.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Local X’ lies on the element surface.
                                           For flat elements, it is a straight line
                                           parallel to a line through nodes 1 and 3.
                                           For elements curved out-of-plane, it is
                                           the intersection of the element surface
                                           with the plane containing the surface
                                           normal and the straight line through
                                           nodes 1 and 3.           Local Y’ is in the
                                           surface, perpendicular to local X’ and
                                           +ve towards node 5. Local Z’ forms a
                                           right-handed set with local X’ and local
                                           Y’.

SIGN CONVENTION                            Direct stresses σxx, σyy, σzz                +ve for tension
                                           Shear stress σxy                             +ve as shown




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-71
QUM8
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
       on the structure), is automatically added to the structure. The node has εz as its only freedom, which is
       reported in the displacement output. As this extra node is common to all elements, εz is constant for the
       entire structure.

2.     2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
       required.

REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-72
QUS4
ASAS (Non-Linear) User Manual                                                                                     Appendix A


                          Quadrilateral Element with Linearly Varying Thickness
                                    for Modelling Thin or Thick Shells

NUMBER OF NODES                            4
                                                                                                          4                            3
NODAL COORDINATES                          x, y, z
DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node.

GEOMETRIC PROPERTIES                       ti Thickness at node i (i = 1,4),
                                           t2 to t4 may be omitted for an element with
                                           uniform thickness t1. Additional lay-up data is
                                           required for laminated material option.
                                                                                                               1               2
                                           See Section 5.2.5.3 for the LAMI command.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (not C-1) defined in element
                                                                 material axes. (see Appendix B.1.2)
                                                                 Coefficients C1-C24 required. Note that they do not
                                                                 contain the thickness.



                                               Nx’x’             C1t C2t C4t       C7t2    C11t2   C16t2 0   0         εx’x’
                                               Νy’y’             .   C3t C5t       C8t2    C12t2   C17t2 0   0         εy’y’
                                               Νx’y’             .    . C6t        C9t2    C13t2   C18t2 0   0         εx’y’
                                               Mx’x’     =       .    .   .        C10t3   C14t3       3
                                                                                                   C19t 0    0         yx’x’
                                               My’y’             .    .   .          .     C15t3   C20t3 0   0         yy’y’
                                               Mx’y’             .    .   .          .       .     C21t3 0   0         yx’y’
                                               Qx’z’             .    .   .          .       .       . C22t C23t       εx’z’
                                               Qy’z’             .    .   .          .       .       .   . C24t        εy’z’




                                                                 3 coefficients of thermal expansion αxx, αyy, αxy referred to
                                                                 local axes.
                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager               yield
                                                                 criteria.
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.
                                                                 Ivanov yield criterion with Isotropic hardening.
                                           CREEP             -   von Mises
                                           FAIL              -   lamina failure law for composites
                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-73
QUS4
ASAS (Non-Linear) User Manual                                                                           Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Pressure loads (+ve for +ve local Z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads
                                           Face temperature loads (Face 1 is on the -ve local Z’ side)
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page A-74
QUS4
ASAS (Non-Linear) User Manual                                                                                  Appendix A


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses, strains and stress resultants are available at all integration points
                                           referred to element local axes. For Ivanov (full section) models only stress and
                                           strain resultants are available. In addition, the stress indicators are printed for
                                           plastic points.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          1 point Gaussian integration in the plane and 3 point Newton-Cotes through
                                           thickness by default. 2x2 Gauss rule in the plane by request. Other in-plane
                                           rules not recommended. See Appendix -G for positions of integration points.

LOCAL AXES                                 Local X’,Y’,Z’ form a right- handed
                                           orthogonal system which, in general,
                                           varies in orientation from point to
                                           point within the element. At any
                                           point P in the element, X’ and Y’ lie
                                           in the tangent plane at P. The
                                           tangent plane is the plane containing
                                           the vectors PR and PS which are
                                           vectors tangent to the curvilinear ξ
                                           and η directions respectively. X’
                                           and Y’ are positioned in the tangent
                                           plane such that the angle between
                                           PR and X’ equals the angle between
                                           PS and Y’.
SIGN CONVENTIONS                           Direct forces/unit width Νx’x’, Νy’y’, Νx’y’                 +ve as shown.
                                           Bending moments/unit width Μx’x’, Μy’y’, Μx’y’               +ve as shown.
                                           Shear forces/unit width Qx’z’, Qy’z’                         +ve as shown.




REFERENCE                                  A. 3




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-75
QUX4
ASAS (Non-Linear) User Manual                                                                                     Appendix A


                         Axisymmetric Quadrilateral Element With Straight Sides
                                                                                                                    Z
NUMBER OF NODES                            4

NODAL COORDINATES                          r, z                                                                         4
                                           (Note that r and z occupy the first and                                              3
                                           third fields with coordinate data using                                      1
                                                                                                                            2
                                           an unnamed cartesian system)


DEGREES OF FREEDOM                         R, Z at each node
                                           (Any skew system must be 2-D. Of the six direction cosines R’R, R’θ, R’Z,
                                           Z’R, Z’θ, Z’Z, the values R’θ and Z’θ must be zero).

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (or C-1) - referred to axis system
                                                                 selected for output (global by default)

                                                                      σrr                C1 C2          C4   C7      εrr
                                                                      σzz                .  C3          C5   C8      εzz
                                                                                =
                                                                      σθθ                .   .          C6   C9      εθθ
                                                                      σrz                .   .           .   C10     εrz


                                                                 4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
                                                                 referred to axis system selected for output

                                                             -   Hyperelastic

                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                 Hardening.

                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-76
QUX4
ASAS (Non-Linear) User Manual                                                                                Appendix A


LOAD TYPES                                 Nodal Loads (must be defined per radian)
                                           Prescribed displacements
                                           Pressure loads (on any side, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points in global or local element
                                           axes (global by default)

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.


INTEGRATION RULES                          2x2 rule used by default. Higher order rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Invariant throughout the element. Local R’ lies along the line from node 1 to
                                           node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
                                           counter clockwise from R’.

SIGN CONVENTIONS                           Direct stresses σrr, σzz, σθθ                +ve for tension
                                                                                                          z
                                           Shear stress σrz                             +ve as shown




                                                                                                                          r

NOTE                                       Global stress output must be used if fracture mechanics processing in POSTNL
                                           is required.

REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-77
QUX8
ASAS (Non-Linear) User Manual                                                                                     Appendix A


                             Axisymmetric Isoparametric Quadrilateral Element

                                                                                                                    Z
NUMBER OF NODES                            8

NODAL COORDINATES                          r, z
                                           (may be omitted for mid-side nodes                                               7   6
                                                                                                                                         5
                                           on a straight edge). Note that r and z                                       8
                                                                                                                                        4
                                           occupy the first and third fields with                                       1       2   3
                                           coordinate data using an unnamed
                                           cartesian system.

DEGREES OF FREEDOM                         R, Z at each node
                                           (Any skew system must be 2-D. Of the six direction cosines R’R, R’θ, R’Z,
                                           Z’R, Z’θ, Z’Z, the values R’θ and Z’θ must be zero)

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (or C-1) - referred to axis system
                                                                 selected for output (global by default)

                                                                      σrr                C1 C2          C4   C7     εrr
                                                                      σzz        =
                                                                                         .  C3          C5   C8     εzz
                                                                      σθθ                .   .          C6   C9     εθθ
                                                                      σrz                .   .           .   C10    εrz


                                                                 4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
                                                                 referred to axis system selected for output

                                                             -   Hyperelastic

                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Prager or Ziegler) or Combined
                                                                 Hardening.

                                           CREEP             -   von Mises.

                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-78
QUX8
ASAS (Non-Linear) User Manual                                                                                Appendix A


LOAD TYPES                                 Nodal Loads (must be defined per radian)
                                           Prescribed displacements
                                           Pressure loads (on any side, +ve towards the element centre)
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses and strains are available at integration points in global or local element
                                           axes (global by default)

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          2x2 rule used by default. Higher order rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Invariant throughout the element. Local R’ lies along the line from node 1 to
                                           node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
                                           counter clockwise from R’.

SIGN CONVENTIONS                           Direct stresses σrr, σzz, σhh                +ve for tension
                                                                                                          z
                                           Shear stress σrz                             +ve as shown




                                                                                                                          r

NOTE                                       Global stress output must be used if fracture mechanics processing in POSTNL
                                           is required.

REFERENCE                                  A. 2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-79
QXT4
ASAS (Non-Linear) User Manual                                                                             Appendix A


             Axisymmetric Quadrilateral Field Element with Quasi-linear Variation
                                      of Field Variable

NUMBER OF NODES                            4                                                                  Z

NODAL COORDINATES                          r, z
                                           (Note that r and z occupy the first and                                 4
                                                                                                                             3
                                           third fields with coordinate data using
                                                                                                                   1
                                           an unnamed cartesian system)                                                  2



DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal values related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (global by default).

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          2x2 rule used by default. Higher order rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Invariant throughout the element. Local R’ lies along the line from node 1 to
                                           node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
                                           counter clockwise from R’.

SIGN CONVENTION                            Fluxes and gradients are positive when in the positive axis direction

NOTES

1.      Temperature loading does not produce thermal loading and does not imply prescribed temperature but
        simply allows temperature dependent material properties to be specified. This is not required for heat
        conduction analysis.

2.      The element allows linear analysis only except for heat conduction analysis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-80
ASAS (Non-Linear) User Manual                                                                          Appendix A

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-81
QXT8
ASAS (Non-Linear) User Manual                                                                             Appendix A


       Axisymmetric Isoparametric Quadrilateral Field Element with Quasi-quadratic
                              Variation of Field Variable
                                                                                                            Z
NUMBER OF NODES                            8

NODAL COORDINATES                          r, z
                                                                                                                    7   6
                                           (may be omitted for mid-side nodes                                                    5
                                                                                                                8
                                                                                                                                4
                                           on a straight edge). Note that r and z                               1       2   3
                                           occupy the first and third fields with
                                           coordinate data using an unnamed
                                           cartesian system.

DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       None

MATERIAL MODELS                            FIELD

                                           PIER

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal values related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (global by default).

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          2x2 rule used by default. Higher order rules by request. Appendix -G gives
                                           position of integration points.

LOCAL AXES                                 Invariant throughout the element. Local R’ lies along the line from node 1 to
                                           node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
                                           counter clockwise from R’.

SIGN CONVENTION                            Fluxes and gradients are positive when in the positive axis direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-82
QXT8
ASAS (Non-Linear) User Manual                                                                          Appendix A


NOTES

1.     Temperature loading does not produce thermal loading and does not imply prescribed temperature but
       simply allows temperature dependent material properties to be specified. This is not required for heat
       conduction analysis.

2.     The element allows linear analysis only except for heat conduction analysis.

3.     Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
       electrical conduction.
       See Reference A. 4, Chapter 7 for full details


REFERENCE                                  A. 2, A. 4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-83
RGX3
ASAS (Non-Linear) User Manual                                                                                   Appendix A


                            Linear Axisymmetric Rigid Surface Contact Element

                                                                                                                           2
NUMBER OF NODES                            3
                                                                                                         1
NODAL COORDINATES                          r, z

DEGREES OF FREEDOM                         R, Z
                                                                                                                    3



GEOMETRIC PROPERTIES                       No basic geometric property.
                                           RIGS required to define the geometry of rigid surface.
                                           (See Section 5.2.5.4)

MATERIAL MODELS                            ELASTIC            -   K is the normal contact stiffness (stress/penetration)
                                           PLASTIC            -   Coulomb friction

                                           Frictionless surface is assumed if no plastic material data.

LOAD TYPES                                 Nodal loads,
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
                                           related to local axes. Stress across the gap, STRESS-XX and frictional stress,
                                           STRESS-YY are related to the local axes.

INTEGRATION RULES                          2 point Newton-Cotes (Trapezoidal rule) along the interface at nodes 1 and 2
                                           (i.e. 2x1x1)
LOCAL AXES                                 Local X’ lies normal to the rigid surface and passes through the integration
                                           point. Local Y’ lies in the global rz plane, perpendicular to local X’ (ie
                                           tangential to the rigid surface).

                                                                  2


                                               1
                                                   X'
                                                        Y'              +ve direction of
                                                                        rigid surface



SIGN CONVENTIONS                           σx’x’          is positive when compressive.
                                           σy’y’    is positive when it acts in negative y’ direction
                                           GAP is positive when penetrated
                                           SLIDE-            Yis positive when sliding in the +ve Y’ direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-84
RGX3
ASAS (Non-Linear) User Manual                                                                          Appendix A



NOTES
1.     Node 3 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1 and
       2 should be on the deforming body.

2.     It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
       and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
       not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
       singularity. These boundary conditions can then be removed once the contact condition with the rigid
       surface is established.

3.     If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
       during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
       analysis further.

4.     Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
       required, MXAUGM, in the PARA command. See also Appendix C.6.


REFERENCE                                  A. 8




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-85
RGX4
ASAS (Non-Linear) User Manual                                                                                   Appendix A


                         Quadratic Axisymmetric Rigid Surface Contact Element

NUMBER OF NODES                            4                                                                     2         3


NODAL COORDINATES                          r, z
                                                                                                          1
DEGREES OF FREEDOM                         R, Z
                                                                                                                      4


GEOMETRIC PROPERTIES                       No basic geometric property.
                                           RIGS required to define the geometry of rigid surface.
                                           (See Section 5.2.5.4)

MATERIAL MODELS                            ELASTIC            -   K is the normal contact stiffness (stress/penetration)
                                           PLASTIC            -   Coulomb friction

                                           Frictionless surface is assumed if no plastic material data

LOAD TYPES                                 Nodal loads,
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
                                           related to local axes. Stress across the gap, STRESS-XX and frictional stress,
                                           STRESS-YY are related to the local axes.

INTEGRATION RULES                          3 point Newton-Cotes (Simpson’s rule) along the interface at nodes 1, 2 and 3
                                           (i.e. 3x1x1)
LOCAL AXES                                 Local X’ lies normal to the rigid surface and passes through the integration
                                           point. Local Y’ lies in the global rz plane, perpendicular to local X’ (ie
                                           tangential to the rigid surface).

                                                    2              3



                                             1
                                                   X'
                                                        Y'              +ve direction of
                                                                        rigid surface



SIGN CONVENTIONS                           σx’x’             is positive when compressive.
                                           σy’y’             is positive when it acts in negative y’ direction
                                           GAP               is positive when penetrated
                                           SLIDE-Y           is positive when sliding in the +ve Y’ direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page A-86
RGX4
ASAS (Non-Linear) User Manual                                                                          Appendix A



NOTES
1.     Node 4 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1, 2
       and 3 should be on the deforming body.

2.     It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
       and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
       not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
       singularity. These boundary conditions can then be removed once the contact condition with the rigid
       surface is established.

3.     If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
       during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
       analysis further.

4.     Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
       required, MXAUGM, in the PARA command. See also Appendix C.6.


REFERENCE                                  A. 8




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-87
RG23
ASAS (Non-Linear) User Manual                                                                                   Appendix A


                                    Linear 2-D Rigid Surface Contact Element

                                                                                                                           2
NUMBER OF NODES                            3
                                                                                                         1
NODAL COORDINATES                          x, y
                                           Option TWOD must be specified

DEGREES OF FREEDOM                         X, Y                                                                    3




GEOMETRIC PROPERTIES                       (i)     Basic Properties
                                                   Plane stress -       ti thickness at node i (i=1,2) (>0.0)
                                                                        t2 may be omitted for an element with uniform
                                                                        thickness t1.
                                                   Plane strain -       no basic geometric property

                                           (ii)    RIGS required to define the geometry of the rigid surface
                                                   (see Section 5.2.5.4)

MATERIAL MODELS                            ELASTIC            -   K is the normal contact stiffness (stress/penetration)
                                           PLASTIC            -   Coulomb friction

                                           Frictionless surface is assumed if no plastic material data

LOAD TYPES                                 Nodal loads,
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
                                           related to local axes. Stress across the gap, STRESS-XX and frictional stress,
                                           STRESS-YY are related to the local axes.

INTEGRATION RULES                          2 point Newton-Cotes (Trapezoidal rule) along the interface at nodes 1 and 2
                                           (i.e. 2x1x1)
LOCAL AXES                                 Local X’ lies normal to the rigid surface and passes through the integration
                                           point. Local Y’ lies in the global xy plane, perpendicular to local X’ (ie
                                           tangential to the rigid surface).

                                                                  2


                                               1
                                                   X'
                                                        Y'              +ve direction of
                                                                        rigid surface



SIGN CONVENTIONS                           σx’x’             is positive when compressive.
                                           σy’y’             is positive when it acts in negative Y’ direction
                                           GAP               is positive when penetrated
                                           SLIDE-Y           is positive when sliding in the +ve Y’ direction



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-88
RG23
ASAS (Non-Linear) User Manual                                                                          Appendix A



NOTES
1.     Node 3 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1 and
       2 should be on the deforming body.

2.     It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
       and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
       not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
       singularity. These boundary conditions can then be removed once the contact condition with the rigid
       surface is established.

3.     If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
       during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
       analysis further.

4.     Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
       required, MXAUGM, in the PARA command. See also Appendix C.6.


REFERENCE                                  A. 8




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-89
RG24
ASAS (Non-Linear) User Manual                                                                                       Appendix A


                                  Quadratic 2-D Rigid Surface Contact Element

NUMBER OF NODES                            4                                                                2
                                                                                                                        3


NODAL COORDINATES                          x, y
                                                                                                        1
                                           Option TWOD must be specified

DEGREES OF FREEDOM                         X, Y
                                                                                                                 4



GEOMETRIC PROPERTIES                       (i)     Basic Properties
                                                   Plane stress -       ti thickness at node i (i=1,3) (>0.0)
                                                                        t2 and t3 may be be omitted for an element with
                                                                           uniform thickness t1.
                                                   Plane strain -       no basic geometric property

                                           (ii)    RIGS required to define the geometry of the rigid surface
                                                   (see Section 5.2.5.4)

MATERIAL MODELS                            ELASTIC            -   K is the normal contact stiffness (stress/penetration)
                                           PLASTIC            -   Coulomb friction

                                           Frictionless surface is assumed if no plastic material data

LOAD TYPES                                 Nodal loads,
                                           Prescribed displacements

OUTPUT                                     The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
                                           related to local axes. Stress across the gap, STRESS-XX and frictional stress,
                                           STRESS-YY are related to the local axes.

INTEGRATION RULES                          3 point Newton-Cotes (Simpson’s rule) along the interface at nodes 1, 2 and 3
                                           (i.e. 3x1x1)
LOCAL AXES                                 Local X’ lies normal to the rigid surface and passes through the integration
                                           point. Local Y’ lies in the global xy plane, perpendicular to local X’ (ie
                                           tangential to the rigid surface).

                                                                   3
                                                   2


                                             1
                                                   X'
                                                        Y'              +ve direction of
                                                                        rigid surface



SIGN CONVENTIONS                           σx’x’             is positive when compressive.
                                           σy’y’             is positive when it acts in negative Y’ direction
                                           GAP               is positive when penetrated
                                           SLIDE-Y           is positive when sliding in the +ve Y’ direction



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page A-90
RG24
ASAS (Non-Linear) User Manual                                                                          Appendix A



NOTES
1.     Node 4 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1, 2
       and 3 should be on the deforming body.

2.     It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
       and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
       not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
       singularity. These boundary conditions can then be removed once the contact condition with the rigid
       surface is established.

3.     If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
       during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
       analysis further.

4.     Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
       required, MXAUGM, in the PARA command. See also Appendix C.6.


REFERENCE                                  A. 8




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-91
SPR1
ASAS (Non-Linear) User Manual                                                                              Appendix A


                                        Translational Spring/Dashpot Element

                                                                                                                        2
NUMBER OF NODES                            2

NODAL COORDINATES                          x, y, (z)                                                              C
                                           z should be omitted for TWOD option
                                                                                                             K
                                                                                                        1
DEGREES OF FREEDOM                         X, Y, (Z), at each node

GEOMETRIC PROPERTIES                       (i)      Global coordinates of a point defining line of action of spring
                                           (ii)     Linear stiffness K or tabulated values of displacement and force
                                           (iii)    Linear damping factor C or tabulated values of velocity and force

MATERIAL PROPERTIES                        ELASTIC - Isotropic (Not used but material integer must be specified.)
                                           PLASTIC - Inelastic spring, SPRG

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements.

MASS MODELLING                             No mass (use added mass).

OUTPUT                                     Spring force, relative displacement, damping force and relative velocity in
                                           spring direction.

LOCAL AXES                                 If the global coordinates P specified in the geometric properties data are all
                                           zero, local X’ lies along the element from node 1 to node 2. For other cases,
                                           local X’ is defined by the position vector OP, where O is the origin of the
                                           global axes.

SIGN CONVENTIONS                           Forces are positive in tension.
                                           Displacements are positive when node 2 moves positively relative to node1.

NOTES

1.     If the coordinates of P are all zero, nodes 1 and 2 must not be coincident.

2.     Elastic behaviour is always assumed for damping.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-92
SPR2
ASAS (Non-Linear) User Manual                                                                             Appendix A


                                          Rotational Spring/Dashpot Element



NUMBER OF NODES                            2


NODAL COORDINATES                          x, y, z


DEGREES OF FREEDOM                         RX, RY, RZ, at each node



GEOMETRIC PROPERTIES                       (i)       Global coordinates of a point, P, defining line of action of spring
                                           (ii)      Linear rotational stiffness K or tabulated values of moment and rotation
                                           and moment.
                                           (iii)     Linear damping factor C or tabulated values of moment and
                                                     angular velocity and moment.

MATERIAL PROPERTIES                        ELASTIC - Isotropic (Not used but material integer must be specified.)
                                           PLASTIC - Inelastic spring, SPRG.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements.

MASS MODELLING                             No mass (use added mass).

OUTPUT                                     Spring moment, relative rotation, damping moment and relative angular
                                           velocity.

LOCAL AXES                                 If the global coordinates P specified in the geometric properties data are all
                                           zero, local X’ lies along the element from node 1 to node 2. For other cases,
                                           local X’ is defined by the position vector OP, where O is the origin of the
                                           global axes.

SIGN CONVENTIONS                           Rotations are positive when node 2 rotates positively relative to node 1.

NOTES

1.     If the coordinates of P are all zero, nodes 1 and 2 must not be coincident.

2.     Elastic behaviour is always assumed for damping.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-93
SST4
ASAS (Non-Linear) User Manual                                                                                        Appendix A


                        Isoparametric Beam/Stiffener Element having Thin-walled
                           Open Cross-sections of Arbitrary Shape (no warping)



NUMBER OF NODES                            4 (2 end, 1 mid-length and 1 auxiliary node).
                                                                                                                                 2
NODAL COORDINATES                          X, Y, Z (may be omitted for mid-length                             4
                                                                                                                         3
                                           node on a straight element). The mid-
                                           length node has tolerance of length/10
                                           about the true mid-length. The auxiliary
                                           node is only used to define the local axes                                        s
                                           (see below).                                                           1

                                                                                                        r     t
DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ.


GEOMETRIC PROPERTIES                       The element can have any open thin-walled cross-section made up of straight
                                           sided segments, connected at median points.                      The element has special
                                           geometric properties (see Geometric Property Section 5.2.5.1).

                                           RMUL              -   Rigidity multiplier (= 1.0 - to represent full
                                                                 cross-section, or = 0.5 to represent half symmetric
                                                             cross-section).
                                           s,t               - Local coordinates to define median points in plane of
                                                             cross-section.
                                           IA,IB             -   Local connectivity.

                 Repeat this               NSTAT             -   Number of integration stations along the segment.
                 for each
                 segment                   NLAY              -   Number of integration layers through segment thickness.
                                           T                 -   Segment thickness.

                                           The cross-section of the element is assumed constant along the length
                                           (Geometric Properties at nodes 2 and 3 need not be supplied).

MATERIAL MODEL                             ELASTIC           -   Isotropic
                                           PLASTIC           -   von-Mises
                                                                 Isotropic Hardening

                                           Material properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page A-94
SST4
ASAS (Non-Linear) User Manual                                                                                 Appendix A


LOAD TYPES                                 Nodal loads
                                           Prescribed displacements.
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Direct stress σrr, shear stress σrm, (referred to segment axes) and stress
                                           resultants (in element local axes) are available as follows.

                                           STRS:            stresses at all integration points on element
                                           SSTR:            smoothed stresses for all integration points at 2 cross-sections
                                                            corresponding to 2 point Gauss rule on length.
                                           ESTR:            smoothed stresses for top and bottom layers at end of each
                                                            segment (ie extreme fibrepoints) at 2 cross-sections
                                                            corresponding to 2 point Gauss rule on length.
                                           SRES:            stress resultants at all 4 Gauss points along the length
                                           SSRE:            smoothed stress resultants at 2 cross-sections corresponding
                                                            to 2 point Gauss rule on length
                                           Strains and strain resultants are not available
                                           For elastic analysis, only stress resultants (i.e. SRES or SSRE) are available.

INTEGRATION RULES                          4 Point Gauss Quadrature along length (invariant and independent of stress
                                           output). User defined trapezoidal rule for each segment. (NO DEFAULT) -
                                           see Geometric Properties Data. As a guide the following are suggested:

                                           Elastic - 2 stations, 1 layer
                                           Plastic - 5 stations, 4 layers

NODE NUMBERING                             Node 3 is always the MID-LENGTH node and 4 the auxiliary node.

LOCAL AXES r, s, t                         Independent of cross-sectional shape - ie s, t do not have to coincide with
                                           principal axes of the cross-section. Local r is tangential to the curvilinear
                                           nodal axis, positive in the direction node 1 to node 2. s is normal to the plane
                                           containing the r-axis and node 4. t is orthogonal to r and s and points away
                                           from node 4, ie positive t and the auxiliary node are on opposite sides of the r
                                           axis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-95
SST4
ASAS (Non-Linear) User Manual                                                                          Appendix A


SIGN CONVENTIONS                           Axial force                +ve tension
                                           Axial stress               +ve tension


                                           Generalised stress resultants, +ve as shown

                                           Fr         -        axial force
                                           Qrs        -        shear along s
                                           Qrt        -        shear along t
                                           Ms         -        moment about s
                                           Mt         -        moment about t
                                           Tsv        -        St. Venant Torque

                                                          Mt


                                                 Qrt


                                                                                          Ms
                                                  t
                                                                               Qrs
                                                                  s

                                                                  r
                                                                               Fr
                                                                                          T sv

NOTES

1.      This element requires special Geometry Property and Residual stress input data (see Sections 5.2.5.1 and
        5.6.3).

2.     Note that the element topology definition and local axes are not the same as the STF4 beam stiffener.

3.     Segment number 1 must start at free edge of the beam cross-section. Each subsequent segment must start
       from the end of any previously numbered segment.

4.     Stress and stress resultant outputs always correspond to the full cross-section.


REFERENCE                                  A. 5




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-96
STF4
ASAS (Non-Linear) User Manual                                                                                          Appendix A


                    Curved Beam Element with Transverse Shear and Offset Nodes
                        for use with the TCS Family of Thick Shell Elements



NUMBER OF NODES                            4 (2 end, 1 mid-length and 1
                                           auxiliary node, see Note).
                                                                                                         Y'         4                         3

NODAL COORDINATES                          x, y, z (may be omitted for mid-                                                         2
                                           length node on a straight element).
                                           The mid-length node has a tolerance
                                                                                                         1               Z'
                                           of length/10 about the true mid-
                                           length. The auxiliary node defines                       X'
                                           the local axes.

DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at nodes 1, 2, 3.

GEOMETRIC PROPERTIES                       There are three types of cross sections available:

                                           (a) Solid rectangular cross-section RECT (or blank) with the
                                               geometric property data
                                                                                                                              Y'
                                           For nodes 1, 2 and 3, in turn:
                                                aY’ cross-sectional dimension of
                                                     local Y’ direction                                       aY'
                                                                                                                                         Z'
                                                 aZ’     cross-sectional dimension of
                                                         local Z’ direction
                                                 eX’     nodal offset in local X’ direction                                   aZ'
                                                 eY’     nodal offset in local Y’ direction
                                                                                                                    X' axis into paper
                                                 eZ’     nodal offset in local Z’ direction


                                           (b) Thin tubular cross-section TUBE - with the geometric
                                               property data

                                                 For nodes 1, 2 and 3, in turn:
                                                 ro   outer radius
                                                 t       wall thickness (ro/t should be ≥ 10)
                                                 eX’     nodal offset in local X’ direction
                                                 eY’     nodal offset in local Y’ direction
                                                 eZ’     nodal offset in local Z’ direction


                                                 Note that +ve θ is the rotation from local Y’ towards local Z’.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-97
STF4
ASAS (Non-Linear) User Manual                                                                                      Appendix A


                                           (c) Thin hollow rectangular cross-section (Box-section) BOX - with                           the
                                           geometric property data.


                                                                                                                         Y'
                                                 For nodes 1, 2 and 3, in turn:
                                                 ao outer dimension of box in                                        1
                                                                                                                    t1         t2
                                                      local Y’ axis.                                            4
                                                                                                        ao                          2
                                                 bo      outer dimension of box in                                  t4        t3              Z'
                                                                                                                         3
                                                         local Z’ axis.
                                                 t1      thickness of segment 1
                                                 t2      thickness of segment 2                                          bo
                                                 t3      thickness of segment 3                              X' axis into paper
                                                 t4      thickness of segment 4
                                                 eX’     nodal offset in local X’ direction
                                                 eY’     nodal offset in local Y’ direction
                                                 eZ’     nodal offset in local Z’ direction

                                           In this case again thin section assumption is made, ao/(t2 or t4)>10 and
                                           bo/(t1 or t3)>10. The hollow section is divided into four segments for
                                           integration purposes. Numbering of segments is shown above. Segment 1 is
                                           numbered where positive Y’ axis crosses the segment and segment 3 is
                                           numbered where the negative Y’ axis crosses. Similarly segments 2 and 4 are
                                           numbered where +ve and -ve Z’ axis crosses respectively.

MATERIAL MODEL                             ELASTIC           -   Isotropic
                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.
                                           CREEP             -   von Mises

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal loads
                                           Prescribed displacements
                                           Distributed load pattern CB1
                                           Temperature loads
                                           Body forces
                                           Centrifugal loads
                                           Angular acceleration

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass

OUTPUT                                     Stresses, strains and stress resultants are available at integration points referred
                                           to element local axes. Stress point indicators for plastic points are also printed.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page A-98
STF4
ASAS (Non-Linear) User Manual                                                                                                    Appendix A


INTEGRATION RULES                          (1) Rectangular cross-section.


                                           2 point Gauss quadrature along length and 3 x 3 Newton-Cotes rules on cross-
                                           section by default (2 x 3 x 3). Other rules, by request, using the INTEgration
                                           command in Preliminary data. Newton-Cotes points are equally spaced and
                                           Appendix -G gives the positions of the Gauss integration points.
                                           Examples

                                                           Y'                      Y'                    Y'                        Y'

                                                   7           8   9                           13            14       15     25     26     27

                                                                                                                             22     23     24
                                                                                               10            11       12     19     20     21
                                                                                                                             16     17     18
                                                                           Z'             Z'       7         8        9 Z'   13     14     15   Z'
                                              4            5           6        1 2 3 4   5                                  10     11     12
                                                                                                   4         5        6      7      8       9
                                                                                                                             4      5       6

                                               1          2        3                           1         2        3          1      2       3

                                                        3x3=9                    1x5=5                 5x3=15                    9x3=27
                                                       (default)



                                           From the above examples it may be noted that the numbering of integration
                                           points always start from the negative quadrant of Y’ Z’ axis.                                  Points are
                                           numbered in the local Z’ axis direction (from -ve to +ve direction) first. Then
                                           points are numbered in the local Y’ axis direction (from -ve to +ve direction)
                                           as shown above.

                                           (2) Tube cross-section

                                           2 point Gauss quadrature along length and 8 points (Trapezoidal) equally
                                           spaced around the tube periphery by default (ie 2x8x1 = NGX*NGY*NGZ).
                                           Other rules, by request, using the INTEgration command in Preliminary data.
                                           (Note that NGZ must be given but is not used) NGY should be a multiple of 4.

                                           Examples




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                              Page A-99
STF4
ASAS (Non-Linear) User Manual                                                                                            Appendix A


                                           The numbering of the integration points always start from the negative
                                           quadrant of the Y’ Z’ axes as shown above. The points are equally spaced on
                                           the circumference.


                                           (3) Box cross-section

                                           2 point Gauss quadrature along length and 12 point Newton-Cotes on cross-
                                           section by default (2x12x1). Other orders, by request, using the INTEgration
                                           command in Preliminary data. NGY must be a multiple of 4 with a minimum
                                           of 12.

                                           Examples




                                           Take NGY = 4n ; n = number of integration points for each segment


                                                        Y'                           C
                                                                                     L                           Y'
                                                                                                            Z'
                                                    5                                                                 5
                                                                1          2             3      4       5
                                                    4                                                                 4
                                                    3                                                                 3
                                           C
                                           L                                                            C
                                                                                                        L
                                                                                    C
                                                                                    L
                                                    2                                                                 2
                                                                                                            Z'
                                                    1                                                                 1
                                                                1          2             3      4       5


                                                                          NGY = 20, n = 5

                                           For the box section, there are the two stresses at each point on the segment.
                                           These are the normal stress and the shear stress along the segment.

NODE NUMBERING                             Node 2 is always the mid-length node and node 4 is the auxiliary node.

LOCAL AXES                                 Local X’ axis is tangential to the curvilinear centroidal axis, positive in the
                                           direction of node 1 to node 3. The local Y’ axis lies in the plane through node



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-100
ASAS (Non-Linear) User Manual                                                                          Appendix A


                                           4 and the local X’ axis, positive towards node 4. Local Z’ forms a right-
                                           handed set with local X’ and local Y’.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-101
STF4
ASAS (Non-Linear) User Manual                                                                                   Appendix A


SIGN CONVENTIONS                           Axial force                 +ve for tension
                                           Axial stress                +ve for tension
                                           Torque                      +ve in positive direction of local axis
                                           Bending Moment              +ve for sagging
                                           Shear force                 +ve in the local axes Y’ Z’ +ve direction


OFFSETS                                    Offsets eX’, eY’, eZ’ +ve as shown. Note that the mid-length node cannot be
                                           offset in the local X’ direction.
                                                                                    4                                    4

                                         eX'                                                      eX'              eZ'   Y'
                                                                                                                         1
                                                                                                        X'                          Z'
                                                                       2
                                           1                                                       3                          eY'




NOTE                                       The auxiliary node must be a dummy node and NOT a node on the structure.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-102
TCS6
ASAS (Non-Linear) User Manual                                                                                      Appendix A


                     Generally Curved Degenerate Triangular Thick Shell Element
                      with Varying Thickness and Transverse Shear Capable of
                        Modelling Discontinuities in Curvature and Thickness


NUMBER OF NODES                            6 (3 corner, 3 mid-side)
NODAL COORDINATES                          x, y, z (may be omitted for mid-side nodes
                                           on straight edges). Each mid-side node has
                                           tolerance of side/10 about the true mid-side.

DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES                       ti Thickness at node i (i = 1,6),
                                           t2 to t6 may be omitted for an element with uniform thickness.
                                           Additional lay-up data is required for laminated material option.
                                           See Section 5.2.5.3 for the LAMI command.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Laminated
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (not C-1) defined in element
                                                                 material axes. (See Appendix B.1.2)
                                                                 Coefficients C1-C24 required. Note that they do not
                                                                 contain the thickness.

                                                Nx’x’                C1t C2t C4t       C7t2    C11t2    C16t2 0   0       εx’x’
                                                Νy’y’                .   C3t C5t       C8t2    C12t2    C17t2 0   0       εy’y’
                                                Νx’y’                .    . C6t        C9t2    C13t2    C18t2 0   0       εx’y’
                                                Mx’x’        =       .    .   .        C10t3   C14t3        3
                                                                                                        C19t 0    0       yx’x’
                                                My’y’                .    .   .          .     C15t3    C20t3 0   0       yy’y’
                                                Mx’y’                .    .   .          .       .      C21t3 0   0       yx’y’
                                                Qx’z’                .    .   .          .       .        . C22t C23t     εx’z’
                                                Qy’z’                .    .   .          .       .        .   . C24t      εy’z’
                                                                 3 coefficients of thermal expansion αxx, αyy, αxy referred to
                                                                 local axes.
                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.
                                                                 Ivanov yield criterion with Isotropic hardening.
                                           CREEP             -   von Mises
                                           FAIL              -   lamina failure law for composites
                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-103
TCS6
ASAS (Non-Linear) User Manual                                                                           Appendix A


LOAD TYPES                                 Nodal Loads
                                           Prescribed displacements
                                           Pressure loads (+ve for +ve local Z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads
                                           Face temperature loads (Face 1 is on the -ve local Z’ side)
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-104
TCS6
ASAS (Non-Linear) User Manual                                                                                  Appendix A


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass


OUTPUT                                     Stresses, strains and stress resultants are available at all integration points
                                           referred to element local axes. For Ivanov (full section) models only stress and
                                           strain resultants are available. In addition, the stress indicators are printed for
                                           plastic points.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          3 point triangular rule in plane and 3 point Newton-Cotes rule through
                                           thickness (1x3x3) by default. Other rules by request, but only the through
                                           thickness integration rule may be altered. See Appendix -G for positions of
                                           integration points.

LOCAL AXES                                 Local X’, Y’, Z’ form a right-
                                           handed orthogonal system which, in
                                           general, varies in orientation from
                                           point to point within the element.
                                           At any point P in the element, X’
                                           and Y’ lie in the tangent plane at P.
                                           The tangent plane is the plane
                                           containing the vectors PR and PS
                                           which are vectors tangent to the
                                           curvilinear ξ         and η directions
                                           respectively.         X’ and Y’ are
                                           positioned in the tangent plane such
                                           that the angle between PR and X’
                                           equals the angle between PS and Y’.

SIGN CONVENTIONS                           Direct forces/unit width Νx’x’, Νy’y’, Νx’y’                 +ve as shown.
                                           Bending moments/unit width Μx’x’, Μy’y’, Μx’y’               +ve as shown.
                                           Shear forces/unit width Qx’z’, Qy’z’                         +ve as shown.




REFERENCE                                  A. 2, A. 4, A. 5


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page A-105
TCS8
ASAS (Non-Linear) User Manual                                                                                     Appendix A


                    Generally Curved 8-Node Quadrilateral Thick Shell Element
                          with Varying Thickness and Transverse Shear,
                  Capable of Modelling Discontinuities in Curvature and Thickness


NUMBER OF NODES                            8 (4 corner, 4 mid-side).
NODAL COORDINATES                          x, y, z (may be omitted for mid-side nodes
                                           on straight edges). Each mid-side node has
                                           tolerance of side/10 about the true mid-side.

DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES                       ti Thickness at node i (i = 1,8),
                                           t2 to t8 may be omitted for an element with uniform thickness t1.
                                           Additional lay-up data is required for laminated material option.
                                           See Section 5.2.5.3 for the LAMI command.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Laminated
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (not C-1) defined in element
                                                                 material axes. (See Appendix B.1.2)
                                                                 Coefficients C1-C24 required. Note that they do not
                                                                 contain the thickness.
                                             Nx’x’               C1t C2t C4t       C7t2    C11t2   C16t2 0   0         εx’x’
                                             Νy’y’               .   C3t C5t       C8t2    C12t2   C17t2 0   0         εy’y’
                                             Νx’y’               .    . C6t        C9t2    C13t2       2
                                                                                                   C18t 0    0         εx’y’
                                             Mx’x’       =       .    .   .        C10t3   C14t3   C19t3 0   0         yx’x’
                                             My’y’               .    .   .          .     C15t3   C20t3 0   0         yy’y’
                                             Mx’y’               .    .   .          .       .     C21t3 0   0         yx’y’
                                             Qx’z’               .    .   .          .       .       . C22t C23t       εx’z’
                                             Qy’z’               .    .   .          .       .       .   . C24t        εy’z’

                                                                 3 coefficients of thermal expansion αxx, αyy, αxy referred to
                                                                 local axes.
                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.
                                                                 Ivanov yield criterion with Isotropic hardening.
                                           CREEP             -   von Mises
                                           FAIL              -   lamina failure law for composites
                                           Material Properties may be temperature dependent if required.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page A-106
TCS8
ASAS (Non-Linear) User Manual                                                                           Appendix A


LOAD TYPES                                 Nodal Loads
                                           Prescribed displacements
                                           Pressure loads (+ve for +ve local Z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads
                                           Face temperature loads (Face 1 is on the -ve local Z’ side)
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-107
TCS8
ASAS (Non-Linear) User Manual                                                                                  Appendix A


MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass


OUTPUT                                     Stresses, strains and stress resultants are available at all integration points
                                           referred to element local axes. For Ivanov (full section) models only stress and
                                           strain resultants are available. In addition, the stress indicators are printed for
                                           plastic points.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          2x2 Gauss quadrature in plane and 3 point Newton-Cotes through thickness
                                           (2x2x3) by default. Other rules by request, but only the through thickness
                                           integration rule may be altered. See Appendix -G for positions of integration
                                           points.

LOCAL AXES                                 Local X’, Y’, Z’ form a right
                                           handed orthogonal system which,
                                           in general, varies in orientation
                                           from point to point within the
                                           element. At any point P in the
                                           element, X’ and Y’ lie in the
                                           tangent plane at P. The tangent
                                           plane is the plane containing the
                                           vectors PR and PS which are
                                           vectors tangent to the curvilinear ξ
                                           and η directions respectively. X’
                                           and Y’ are positioned in the
                                           tangent plane such that the angle
                                           between PR and X’ equals the
                                           angle between PS and Y’.

SIGN CONVENTIONS                           Direct forces/unit width Νx’x’, Νy’y’, Νx’y’                 +ve as shown.
                                           Bending moments/unit width Μx’x’, Μy’y’, Μx’y’               +ve as shown.
                                           Shear forces/unit width Qx’z’, Qy’z’                         +ve as shown.




REFERENCE                                  A. 2, A. 4, A. 5




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page A-108
TCS9
ASAS (Non-Linear) User Manual                                                                                      Appendix A


                    Generally Curved 9-Node Quadrilateral Thick Shell Element
                          with Varying Thickness and Transverse Shear,
                  Capable of Modelling Discontinuities in Curvature and Thickness


NUMBER OF NODES                            9 (4 corner, 4 mid-side, 1 centre).
NODAL COORDINATES                          x, y, z (may be omitted for mid-side nodes
                                           on straight edges). Each mid-side node has
                                           tolerance of side/10 about the true mid-side.
DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES                       ti Thickness at node i (i = 1,9),
                                           t2 to t9 may be omitted for an element with uniform thickness t1.
                                           Additional lay-up data is required for laminated material option.
                                           See Section 5.2.5.3 for the LAMI command.

MATERIAL MODELS                            ELASTIC           -   Isotropic
                                                             -   Orthotropic
                                                             -   Woven
                                                             -   Laminated
                                                             -   Anisotropic
                                                                 Anisotropic matrix C (not C-1) defined in element
                                                                 material axes. (See Appendix B.1.2)
                                                                 Coefficients C1-C24 required. Note that they do not
                                                                 contain the thickness.
                                                Nx’x’               C1t C2t C4t       C7t2    C11t2     C16t2 0   0      εx’x’
                                                Νy’y’               .   C3t C5t       C8t2    C12t2     C17t2 0   0      εy’y’
                                                Νx’y’               .    . C6t        C9t2    C13t2     C18t2 0   0      εx’y’
                                                Mx’x’       =       .    .   .        C10t3   C14t3         3
                                                                                                        C19t 0    0      yx’x’
                                                My’y’               .    .   .          .     C15t3     C20t3 0   0      yy’y’
                                                Mx’y’               .    .   .          .       .       C21t3 0   0      yx’y’
                                                Qx’z’               .    .   .          .       .         . C22t C23t    εx’z’
                                                Qy’z’               .    .   .          .       .         .   . C24t     εy’z’

                                                                 3 coefficients of thermal expansion αxx, αyy, αxy referred to
                                                                 local axes.
                                           PLASTIC           -   von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
                                                                 yield criteria.
                                                                 Isotropic, Kinematic (Ziegler) or Combined Hardening.
                                                                 Ivanov yield criterion with Isotropic hardening.
                                           CREEP             -   von Mises
                                           FAIL              -   lamina failure law for composites




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-109
TCS9
ASAS (Non-Linear) User Manual                                                                                  Appendix A


                                           Material Properties may be temperature dependent if required.
LOAD TYPES                                 Nodal Loads
                                           Prescribed displacements
                                           Pressure loads (+ve for +ve local Z’ direction)
                                           Distributed load patterns ML1, ML2, ML3
                                           Temperature loads.
                                           Face temperature loads (Face 1 is on the -ve local Z’ side)
                                           Body forces
                                           Centrifugal loads
                                           Angular accelerations
                                           Tank Loads

MASS MODELLING                             Consistent mass (used by default)
                                           Lumped mass


OUTPUT                                     Stresses, strains and stress resultants are available at all integration points
                                           referred to element local axes. For Ivanov (full section) models only stress and
                                           strain resultants are available. In addition, the stress indicators are printed for
                                           plastic points.

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
                                           corner node.

INTEGRATION RULES                          2x2 Gauss quadrature in plane and 3 point Newton-Cotes through thickness
                                           (2x2x3) by default. Other in-plane rules not recommended although 3x3 rule
                                           may be adopted in special circumstances. Other through thickness rules by
                                           request. See Appendix -G for positions of integration points.

LOCAL AXES                                 Local X’, Y’, Z’ form a right
                                           handed orthogonal system which,
                                           in general, varies in orientation
                                           from point to point within the
                                           element. At any point P in the
                                           element, X’ and Y’ lie in the
                                           tangent plane at P. The tangent
                                           plane is the plane containing the
                                           vectors PR and PS which are
                                           vectors tangent to the curvilinear ξ
                                           and η directions respectively. X’
                                           and Y’ are positioned in the
                                           tangent plane such that the angle
                                           between PR and X’ equals the
                                           angle between PS and Y’.

SIGN CONVENTIONS                           Direct forces/unit width Νx’x’, Νy’y’, Νx’y’                 +ve as shown.
                                           Bending moments/unit width Μx’x’, Μy’y’, Μx’y’               +ve as shown.
                                           Shear forces/unit width Qx’z’, Qy’z’                         +ve as shown.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page A-110
TCS9
ASAS (Non-Linear) User Manual                                                                          Appendix A




REFERENCE                               A. 2, A. 4, A. 5




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-111
TMT3
ASAS (Non-Linear) User Manual                                                                                               Appendix A


                       Triangular Membrane Field Element with Linear Variation
                                         of Field Variable


NUMBER OF NODES                            3

NODAL COORDINATES                          x, y, (z)
                                           z should be omitted for 2-D problems.

DEGREES OF FREEDOM                         T at each node

GEOMETRIC PROPERTIES                       ti Thickness at node i (i=i,3)
                                           t2, t3 may be omitted for an element with
                                           uniform thickness t1

                                           No geometric property required with PLSN option. In this case, the geometric
                                           property integer in the topology data should also be omitted.


MATERIAL MODELS                            FIELD

                                           PIER

                                           Material Properties may be temperature dependent if required.

LOAD TYPES                                 Nodal values related to field variable type
                                           Prescribed field variable
                                           Temperature
                                           Flux density - surface or internal

OUTPUT                                     Fluxes per unit area (analogous to stresses) and field variable gradients
                                           (analogous to strains) are available at integration points related to either global
                                           or local axes (local by default).

NODE NUMBERING                             The nodes are listed in cyclic order, clockwise or anti-clockwise.

INTEGRATION RULES                          Single point rule by default (1x1). 3 point rule by request. Appendix -G gives
                                           position of integration points.
                                                                                                        Y'      3

LOCAL AXES                                 Local X’ lies along the straight line
                                           from node 1 towards node 2. Local
                                                                                                                    σy'y'
                                           Y’ is in the plane, perpendicular to
                                           X’ and positive towards node 3.
                                           Local Z’ forms a right-handed set                                                σx'x'
                                                                                                        σx'y'
                                           with local X’ and local Y’.                           1                                  2
                                                                                                                                          X'


SIGN CONVENTION