Asas by subrahmanian1956

VIEWS: 17 PAGES: 582

									                             ASAS (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superseded by a newer version of this guide.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.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                 ASAS (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

1.2                   1-2                     Update                   Delete reference to program COMPED

3.1                   3-1, 3-2                Update                   Amend description of preparatory process.

3.2.1                 3-2                     Update                   Delete reference to program COMPED

3.5.3                 3-19                    Update                   Delete reference to legacy program ASDIS

5.1.2                 5-4                     Update                   Delete reference to legacy program ASDIS

5.1.3                 5-5                     Update                   Delete reference to program COMPED

5.1.17.1              5-18                    Update                  Delete references to legacy programs APCA,
                                                                      FRAKAS

5.1.22                5-27                    Update                   Delete reference to legacy program ADLIB

5.1.23                5-28                    Update                  Delete references to legacy programs ADLIB,
                                                                      ASDIS,        COMPED,             FRAKAS,   PICASO,
                                                                      PRE-NL

5.3.5                 5-88                    Update                  Expand Note 6.

6.7                   6-13                    Update                  Delete reference to legacy program ASDIS

6.7                   6-13                    Update                   Delete reference to program COMPED

App A.7               A-17                    Update                   Delete reference to legacy program ADLIB

App. A.9              A-29 – A-168            Update                   Add hyperlinks to description sheets.

                                                                       Sections shown incorrectly for ANGL, CHAN,
                                                                       TEE sections


Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
App. C.5              C-7                     Update                   Delete reference to legacy program ASDIS

App. C.10             C-13                    Addition                 Add SMIX option

App F.1.1             F-3, F-5                Update                   Delete reference to legacy program ASDIS

App F.1.2             F-7                     Update                   Delete reference to legacy program ASDIS

App F.2.1             F-16                    Update                   Delete reference to legacy program ASDIS

App F.2.3             F-19                    Update                   Delete reference to legacy program ASDIS

App F.2.5             F-25                    Update                   Delete reference to legacy program ASDIS

App F.2.7             F-28                    Update                   Delete reference to legacy program ASDIS

App F.2.9             F-34                    Update                   Delete reference to legacy program ASDIS

App F.2.10            F-36                    Update                   Delete reference to legacy program ASDIS

App F.3.1             F-42                    Update                   Delete reference to legacy program ASDIS

App G.5               G-6                     Update                   Delete reference to legacy program PICASO




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


                                                  Table of Contents
1. Introduction ............................................................................................................................. 1-1
   1.1 The ASAS™ Finite Element System .............................................................................. 1-1
   1.2 ASAS Program Modules ............................................................................................... 1-1
   1.3 Facilities in ASAS ......................................................................................................... 1-4
   1.4 Using this Manual .......................................................................................................... 1-4
2. Modelling the Structure........................................................................................................... 2-1
   2.1 The Idealisation Process ................................................................................................ 2-1
   2.2 Types Of Element .......................................................................................................... 2-1
      2.2.1 Frames ..................................................................................................................... 2-2
      2.2.2 Membrane Elements ............................................................................................... 2-2
      2.2.3 Plates ....................................................................................................................... 2-3
      2.2.4 Shells....................................................................................................................... 2-4
      2.2.5 Solids ...................................................................................................................... 2-4
      2.2.6 Sandwich Elements ................................................................................................. 2-5
      2.2.7 Spring Elements ...................................................................................................... 2-6
      2.2.8 Crack Problems ....................................................................................................... 2-6
   2.3 Node Numbers and Coordinates .................................................................................... 2-6
   2.4 Global and Local Axis Systems ..................................................................................... 2-7
      2.4.1 Coordinate Local Axes ........................................................................................... 2-8
      2.4.2 Element Local Axes ................................................................................................ 2-8
      2.4.3 Skew Systems ......................................................................................................... 2-8
   2.5 Material Axes for Anisotropic Material ........................................................................ 2-9
   2.6 Data Units ...................................................................................................................... 2-9
   2.7 Structural Suppressions and Constraints ..................................................................... 2-12
      2.7.1 Special Degrees of Freedom ................................................................................. 2-12
   2.8 Loads............................................................................................................................ 2-14
      2.8.1 Nodal Loads .......................................................................................................... 2-14
      2.8.2 Prescribed Displacements ..................................................................................... 2-14
      2.8.3 Pressure Loads ...................................................................................................... 2-14
      2.8.4 Distributed Loads .................................................................................................. 2-14
      2.8.5 Temperature Loads ............................................................................................... 2-15
      2.8.6 Face Temperatures ................................................................................................ 2-15
      2.8.7 Body Forces .......................................................................................................... 2-15
      2.8.8 Centrifugal Loads ................................................................................................. 2-15
      2.8.9 Angular Accelerations .......................................................................................... 2-15
      2.8.10 Tank Loads ......................................................................................................... 2-16
   2.9 Results From ASAS ..................................................................................................... 2-16
      2.9.1 Input Data Images ................................................................................................. 2-16
      2.9.2 Expanded Data and Summaries ............................................................................ 2-16
      2.9.3 Results - Displacements and Reactions ................................................................ 2-16
      2.9.4 Results - Frequencies and Normal Modes ............................................................ 2-16
      2.9.5 Results - Stresses .................................................................................................. 2-17
      2.9.6 Analysis Summary ................................................................................................ 2-17
      2.9.7 Results - Post-Processing ...................................................................................... 2-17
   2.10     Substructured Analysis ........................................................................................... 2-17
      2.10.1 Planning a Substructured Analysis ..................................................................... 2-20


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


      2.10.2 The Choice of Master Components .................................................................... 2-25
      2.10.3 Component Link Node........................................................................................ 2-26
      2.10.4 Component Assembly ......................................................................................... 2-27
      2.10.5 Component Loading ........................................................................................... 2-27
      2.10.6 Component Recovery ......................................................................................... 2-28
3. The ASAS Analysis ................................................................................................................ 3-1
   3.1 Preparing for the Analysis ............................................................................................. 3-1
   3.2 Description of Each Data Block .................................................................................... 3-2
      3.2.1 Preliminary Data - see Section 5.1.......................................................................... 3-2
      3.2.2 Structural Description Data - see Section 5.2 ......................................................... 3-3
      3.2.3 Boundary Condition Data - see Section 0 ............................................................... 3-6
      3.2.4 Loading Data - see Section 5.4 ............................................................................... 3-8
      3.2.5 Additional Mass Data - see Section 5.5 .................................................................. 3-8
      3.2.6 Component Recovery Data - see Section 5.6 ......................................................... 3-9
      3.2.7 Combined Loading Data - see Section 5.8 ............................................................. 3-9
   3.3 Controlling The Run ...................................................................................................... 3-9
   3.4 Linear Stress Analysis ................................................................................................. 3-10
      3.4.1 Types of Problem .................................................................................................. 3-10
      3.4.2 The Idealisation of Linear Stress Analysis Problems ........................................... 3-10
      3.4.3 The Data for Linear Stress Analysis ..................................................................... 3-10
   3.5 Natural Frequency Analysis ........................................................................................ 3-15
      3.5.1 Types of Problem .................................................................................................. 3-15
      3.5.2 The Idealisation of Natural Frequency Problems ................................................. 3-15
      3.5.3 The Data for Natural Frequency Analysis ............................................................ 3-18
   3.6 Steady State Heat Conduction Analysis ...................................................................... 3-21
      3.6.1 Types of Problem .................................................................................................. 3-21
      3.6.2 The Idealisation of Heat Conduction Problems .................................................... 3-21
      3.6.3 The Data for Heat Conduction Analysis ............................................................... 3-22
   3.7 Substructured Linear Stress or Natural Frequency Analysis ....................................... 3-24
      3.7.1 Types of Problem .................................................................................................. 3-24
      3.7.2 The Idealisation of a Substructured Problem ........................................................ 3-25
         3.7.2.1 The Data for a Master Component Creation Analysis using COMP
         or COMD ..................................................................................................................... 3-26
         3.7.2.2 The Data for a Master Component Creation Analysis using JOB
         type STIF ..................................................................................................................... 3-29
      3.7.3 The Data for a Global Structure Analysis (linear stress or natural
      frequency) ......................................................................................................................... 3-30
      3.7.4 The Data for a Component Recovery Analysis .................................................... 3-32
   3.8 Gap Analysis ................................................................................................................ 3-32
      3.8.1 Types of problem .................................................................................................. 3-32
      3.8.2 The idealisation of Gap problems ......................................................................... 3-33
      3.8.3 The data for a Gap analysis................................................................................... 3-33
   3.9 Solution Methods and Bandwidth ............................................................................... 3-35
4. Input Data Syntax .................................................................................................................... 4-1
   4.1 General Principles .......................................................................................................... 4-1
   4.2 Special Symbols............................................................................................................. 4-3
   4.3 Data Generation Facilities ............................................................................................. 4-5
      4.3.1 Repeat Facilities ...................................................................................................... 4-5


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


      4.3.2 Re-Repeat Facilities ................................................................................................ 4-7
5. Data Formats ........................................................................................................................... 5-1
   5.1 The Preliminary Data ..................................................................................................... 5-1
      5.1.1 SYSTEM Command ............................................................................................... 5-4
      5.1.2 PROJECT Command .............................................................................................. 5-4
      5.1.3 JOB Command........................................................................................................ 5-5
      5.1.4 STRUCTURE Command ....................................................................................... 5-6
      5.1.5 COMPONENT Command ...................................................................................... 5-6
      5.1.6 FILES Command .................................................................................................... 5-7
      5.1.7 TITLE Command.................................................................................................... 5-8
      5.1.8 TEXT Command..................................................................................................... 5-8
      5.1.9 OPTIONS Command .............................................................................................. 5-9
      5.1.10 PASS Command ................................................................................................... 5-9
      5.1.11 START Command .............................................................................................. 5-10
      5.1.12 RESTART Command ......................................................................................... 5-11
      5.1.13 GOTP Command ................................................................................................ 5-12
      5.1.14 EQMA Command ............................................................................................... 5-12
      5.1.15 PARA Command ................................................................................................ 5-14
      5.1.16 FREQUENCY Command ................................................................................... 5-14
      5.1.17 SAVE FILES Command..................................................................................... 5-16
         5.1.17.1 Files for Numerical Processing ................................................................... 5-16
         5.1.17.2 Interface Files for Plotting Programs .......................................................... 5-17
      5.1.18 COPY Command ................................................................................................ 5-19
      5.1.19 RESU command ................................................................................................. 5-20
      5.1.20 WARN Command............................................................................................... 5-20
      5.1.21 UNITS Command ............................................................................................... 5-21
         5.1.21.1 Global UNITS Definition............................................................................ 5-22
         5.1.21.2 Results UNITS Command .......................................................................... 5-23
      5.1.22 LIBRARY Command ......................................................................................... 5-24
      5.1.23 INFO Command ................................................................................................. 5-25
      5.1.24 END Command................................................................................................... 5-26
   5.2 PHYSICAL Property Data .......................................................................................... 5-27
      5.2.1 UNITS Command ................................................................................................. 5-27
      5.2.2 COORDINATE Data ............................................................................................ 5-29
         5.2.2.1 Local Coordinate System Header ................................................................. 5-31
         5.2.2.2 Local Coordinate System Orientation ........................................................... 5-31
         5.2.2.3 Node Coordinates .......................................................................................... 5-34
         5.2.2.4 Coordinate Imperfection Data ....................................................................... 5-36
      5.2.3 Element Topology Data ........................................................................................ 5-39
      5.2.4 Material Properties Data ....................................................................................... 5-42
         5.2.4.1 Isotropic Material Properties ......................................................................... 5-43
         5.2.4.2 Anisotropic Material Properties .................................................................... 5-44
         5.2.4.3 Orthotropic Material Data ............................................................................. 5-45
         5.2.4.4 Laminated Material Properties ...................................................................... 5-45
         5.2.4.5 Isotropic Material Properties - Temperature Dependent............................... 5-46
      5.2.5 Geometric Properties Data .................................................................................... 5-48
         5.2.5.1 General format for the explicit definition of geometric properties ............... 5-48
         5.2.5.2 Definition of geometric properties for composite shells ............................... 5-49


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


           5.2.5.3 Definition of geometric properties for thick shell elements QUS4,
           TCS6 and TCS8 ........................................................................................................... 5-50
           5.2.5.4 Definition of geometric properties for beam elements having local
           axes definition and/or rigid offsets .............................................................................. 5-51
           5.2.5.5 Definition of Geometric Properties for Stiffened Panels .............................. 5-58
        5.2.6 Section Data .......................................................................................................... 5-62
           5.2.6.1 Section Types and Dimensions ..................................................................... 5-65
           5.2.6.2 Fabricated Plate Sections .............................................................................. 5-70
        5.2.7 Skew System Data ................................................................................................ 5-72
           5.2.7.1 Skew Systems - Direction Cosines ............................................................... 5-72
           5.2.7.2 Skew Systems - Nodal Definition ................................................................. 5-74
        5.2.8 Sets Data ............................................................................................................... 5-75
        5.2.9 Component Topology Data................................................................................... 5-76
           5.2.9.1 TRANSLATION Data .................................................................................. 5-77
           5.2.9.2 ROTATION Data .......................................................................................... 5-78
           5.2.9.3 MIRROR Data .............................................................................................. 5-79
           5.2.9.4 TOPOLOGY Data......................................................................................... 5-81
     5.3 BOUNDARY Conditions Data.................................................................................... 5-82
        5.3.1 UNITS Command ................................................................................................. 5-82
        5.3.2 Freedom RELEASE Data ..................................................................................... 5-83
        5.3.3 SUPPRESSED Freedoms Data............................................................................. 5-87
        5.3.4 DISPLACED Freedom Data................................................................................. 5-89
        5.3.5 CONSTRAINT Equation Data ............................................................................. 5-91
        5.3.6 LINK Freedom Data ............................................................................................. 5-96
        5.3.7 MASTER Freedoms Data ..................................................................................... 5-98
        5.3.8 RIGID Constraints Data...................................................................................... 5-100
        5.3.9 SPECIAL Freedom Direction Data .................................................................... 5-104
        5.3.10 GAP Data .......................................................................................................... 5-105
     5.4 LOAD Data ................................................................................................................ 5-107
        5.4.1 UNITS Command ............................................................................................... 5-108
        5.4.2 LOADING Data .................................................................................................. 5-110
        5.4.3 NODAL LOADS Data........................................................................................ 5-111
        5.4.4 PRESCRIBED Displacements Data ................................................................... 5-113
        5.4.5 PRESSURE Load Data ....................................................................................... 5-115
           5.4.5.1 UNIFORM Pressure Load Data .................................................................. 5-117
           5.4.5.2 NON-UNIFORM Pressure Load Data ........................................................ 5-119
        5.4.6 DISTRIBUTED Load Data ................................................................................ 5-123
           5.4.6.1 Local Beam Distributed Loads ................................................................... 5-126
           5.4.6.2 Global Beam Distributed Loads .................................................................. 5-136
           5.4.6.3 Panel Edge Distributed Loads ..................................................................... 5-148
           5.4.6.4 Panel Point Loads........................................................................................ 5-151
           5.4.6.5 Curved Beam Distributed Loads ................................................................. 5-153
        5.4.7 TEMPERATURE LOAD Data ........................................................................... 5-155
           5.4.7.1 Nodal Temperature ..................................................................................... 5-155
           5.4.7.2 ELEMENT TEMPERATURE Data ........................................................... 5-157
           5.4.7.3 UNIFORM Element Temperature Data ...................................................... 5-158
           5.4.7.4 NON-UNIFORM Element Temperature Data ............................................ 5-159
        5.4.8 FACE TEMPERATURE Data............................................................................ 5-162


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


         5.4.8.1 Nodal Face Temperature ............................................................................. 5-162
         5.4.8.2 ELEMENT FACE TEMPERATURE Data ................................................ 5-164
         5.4.8.3 UNIFORM Element Face Temperature Data ............................................. 5-165
         5.4.8.4 NON-UNIFORM Element Face Temperature Data ................................... 5-166
      5.4.9 BODY FORCE Data ........................................................................................... 5-169
      5.4.10 CENTRIFUGAL LOADS Data ........................................................................ 5-171
      5.4.11 ANGULAR ACCELERATION LOADS Data ................................................ 5-173
      5.4.12 COMPONENT LOADS Data........................................................................... 5-175
      5.4.13 TANK LOAD data............................................................................................ 5-177
   5.5 DIRECT MASS Input Data ....................................................................................... 5-179
      5.5.1 UNITS command ................................................................................................ 5-180
      5.5.2 LUMP ADDED MASS Data .............................................................................. 5-181
      5.5.3 CONSISTENT ADDED MASS Data................................................................. 5-183
   5.6 COMPONENT RECOVERY Data ........................................................................... 5-184
      5.6.1 COMPONENT SELECTION Data for Component Recovery........................... 5-185
      5.6.2 LOADCASE SELECTION Data for Component Recovery .............................. 5-187
   5.7 Stiffness and Mass Matrix Input Data ....................................................................... 5-189
      5.7.1 STIFFNESS Matrix Data .................................................................................... 5-189
      5.7.2 MASS Matrix Data ............................................................................................. 5-190
   5.8 COMBINED LOADCASE Data ............................................................................... 5-191
   5.9 STOP Command ........................................................................................................ 5-193
6. Running Instructions ............................................................................................................... 6-1
   6.1 General ........................................................................................................................... 6-1
   6.2 How to Run ASAS......................................................................................................... 6-1
   6.3 ASAS Initialisation File ................................................................................................. 6-4
   6.4 Extended Syntax in Data Files ....................................................................................... 6-5
      6.4.1 IF/THEN/ELSE ...................................................................................................... 6-5
      6.4.2 DATA REPLACEMENT ....................................................................................... 6-7
      6.4.3 The DEFINE Command ......................................................................................... 6-8
      6.4.4 Automatic JOB Type and Program Name Recognition.......................................... 6-9
   6.5 Secondary Data Files within ASAS Data .................................................................... 6-11
      6.5.1 Use of @filename command ................................................................................ 6-11
      6.5.2 Notes about the @ Command ............................................................................... 6-12
   6.6 Estimating Job Size...................................................................................................... 6-13
   6.7 Disk File Handling....................................................................................................... 6-13
      6.7.1 Disk Files Required for Substructures .................................................................. 6-13
      6.7.2 Using ASAS Backing Files on Separate Directories ............................................ 6-14
   6.8 Error and Warning Messages....................................................................................... 6-15
      6.8.1 Warning Messages ................................................................................................ 6-15
      6.8.2 Error Messages ..................................................................................................... 6-15
Appendix - A Description of Each Type of Finite Element in ASAS ..................................... A-1
   A.1      Element Type Related Loading Data ....................................................................... A-2
   A.2      Element Axes Systems ............................................................................................. A-3
   A.3      Beam Offsets .......................................................................................................... A-10
   A.4      Stepped Beams ....................................................................................................... A-14
   A.5      Shell Offsets ........................................................................................................... A-15
   A.6      Laminated Shells .................................................................................................... A-16
   A.7      Section Libraries .................................................................................................... A-18


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


  A.8      Beam Stresses ........................................................................................................ A-19
  A.9      Finite Element Description Sheets ......................................................................... A-30
Appendix - B Consistent Units................................................................................................. B-1
Appendix - C Options .............................................................................................................. C-1
  C.1 General Options ............................................................................................................ C-2
  C.2 Options to Control the Printing of the Data Input ........................................................ C-3
  C.3 Options which Control the Printing of the Expanded Data Lists ................................. C-5
  C.4 Options Associated with Data Checking ...................................................................... C-6
  C.5 Options which affect how results are Saved on File..................................................... C-7
  C.6 Options which Invoke Bandwidth Reduction Schemes................................................ C-7
  C.7 Options which Control the Printing of Results ............................................................. C-8
  C.8 Solution Control Options ............................................................................................ C-10
  C.9 Solution Control Options (Continued)........................................................................ C-11
  C.10     Miscellaneous Options ........................................................................................... C-11
Appendix - D Restarts .............................................................................................................. D-1
  D.1      Restart Stages For Linear Stress Analysis - JOB LINE ........................................... D-2
  D.2      Restart Stages For Natural Frequency Analysis- JOB FREQ .................................. D-3
  D.3      Restart Stages For Heat Conduction Analysis- JOB HEAT .................................... D-4
  D.4      Restart Stages for Re-run of Linear Stress Analysis - JOB LINE with
  COPY ADLD FILES ............................................................................................................. D-4
  D.5      Restart Stages For Re-run Natural Frequency Analysis - JOB FREQ with
  COPY ADMS FILES ............................................................................................................. D-5
  D.6      Restart Stages for Linear Static Stress Component Creation Analysis -
  JOB COMP ............................................................................................................................ D-5
  D.7      Restart Stages for Linear Static Stress Global Structure Analysis- JOB
  LINE D-6
  D.8      Restart Stages for Linear Static Stress Recovery- JOB RECO .............................. D-6
  D.9      Restart Stages for Natural Frequency Component Creation Analysis- JOB
  COMD D-7
  D.10     Restart Stages For Natural Frequency Global Structure Analysis- JOB
  FREQ D-7
  D.11     Restart Stages For Stiffness Input Component Creation Analysis- JOB
  STIF D-8
  D.12     Restart Stages For Gap Analysis- JOB GAPD ........................................................ D-8
Appendix - E List of Freedom Names ...................................................................................... E-1
Appendix - F Examples ............................................................................................................. F-1
  F.1 The Idealisation of Example 1 ....................................................................................... F-2
  F.2 The Idealisation of Example 2 ..................................................................................... F-14
  F.3 A Natural Frequency Analysis..................................................................................... F-38
Appendix - G Extended Facilities in the Preliminary Data ...................................................... G-1
  G.1      SAVE COMP FILES Command.............................................................................. G-1
  G.2      SAVE COMMAND ................................................................................................. G-3
  G.3      COPY Command ..................................................................................................... G-4
  G.4      USER Command ...................................................................................................... G-5
  G.5      MONITOR Command ............................................................................................. G-6
  G.6      DEBUG Command .................................................................................................. G-8
  G.7      SYSTEM Command ................................................................................................ G-9
Appendix - H Joint Flexibility ................................................................................................. H-1


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


     H.1    Introduction .............................................................................................................. H-2
     H.2    Modelling ................................................................................................................. H-3
     H.3    The Analysis .......................................................................................................... H-10
     H.4    Joint Information Data Formats ............................................................................. H-12
     H.5    Options ................................................................................................................... H-24
     H.6    Restart Stages For Linear Stress Flexible Joint Rerun Analysis - COPY
     FLEX FILE .......................................................................................................................... H-25




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



ASAS
General Finite Element Program for
Static and Dynamic Linear Structural Analysis


1.     Introduction

1.1    The ASAS™ Finite Element System

The ASAS™ System for Finite Element Analysis consists of a number of program modules surrounding the
main general purpose solution module, ASAS. It is designed not simply to provide a stiffness solution but also
to give the engineer the results he or she needs. The system is shown as a simplified flowchart in Figure 1.1. At
the top, the finite element model generation shows the program FEMGEN™, an interactive graphical pre-
processor for the creation of the structure geometry, boundary conditions and load data.                Also shown is
           ®
PATRAN , a similar program, which will also interface to ASAS. The results of the pre-processing is a
standard ASAS formatted datafile which could equally have been input directly using a character file editor or
word processor.

The main general purpose solver module is ASAS. This is described in detail in the later chapters of this
manual.

Below this comes a number of post-processing modules intended to perform numerical calculations and provide
the engineer with engineering results. These results can either be printed out for examination or may be written
to an interface file for later display in graphical form using FEMVIEW or PATRAN.

1.2    ASAS Program Modules


ASAS             -    the main general purpose finite element solution module for static and dynamic problems.

LOCO             -    a program to read the results from the ASAS database and produce new loadcases by factoring
                      and combining the existing loadcases.

RESPONSE -            to calculate the dynamic response of a structure from the mode shapes calculated by ASAS,
                      using a number of different time-varying load input systems.

BEAMST           -    a post-processor for Beam type finite elements. This program will report forces, moments and
                      stresses and also perform code checks to a number of international codes of practice.

POST             -    a post-processor for various families of finite element, including plates and shells, bricks,
                      axisymmetric solids and sandwich elements.

XTRACT           -    a small program to extract and print results for specific nodes or elements from the ASAS
                      results database.




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


MAXMIN           -    to summarise a number of loadcases and list the cases giving the highest and lowest values.

FEMGEN           -    a general purpose interactive model generation program. The majority of the ASAS data can
                      be generated including model geometry, boundary conditions and loading data.            When
                      complete the data is output as a standard data file for input to ASAS.

FEMVIEW          -    a general purpose graphical display program for all the major results produced by ASAS and
                      the post-processors.




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




                                        Figure 1.1 The ASAS Finite Element System




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


1.3    Facilities in ASAS

ASAS incorporates facilities for linear static stress analysis, natural frequency analysis and heat conduction
analysis. The program is based on the finite element method, and its extensive library of element types allows
the analysis of most engineering structures.                The element library covers frames and grillages, membrane
structures, plane strain problems, plates, thick and thin shells, general solids, axi-symmetric solids and fracture
mechanics problems. Several types of element may be combined to represent the different parts of a structure.
There are no restrictions on the number of nodes, elements, supports, or loadcases, or any other size limit other
than those imposed by the computer hardware. Problems involving linear stress analysis may also be solved
using a substructure technique, in which the whole structure is subdivided into parts and analysed separately.

The effect of foundations, support from adjacent structure or symmetrical boundaries can be represented by
fixing nodes in the required direction, or giving them specified displacements. Other structural effects, such as
sliding faces, hinges, pin joints, rigid connections and contact problems can be accommodated by constraint
equations. The load types available are similarly wide-ranging. For linear stress analysis, they cover most
mechanical and thermal load situations, including point loads, temperature loads, line loads on edges, pressures
on faces, centrifugal loads and body forces due to self weight or acceleration. For heat conduction analysis, the
thermal loading may consist of point sources or sinks, and prescribed temperature fields.

Great emphasis has been placed on making ASAS easy to use; the engineering user needs very little knowledge
of computing or programming. The data formats are clear and concise and arranged as a series of blocks with
descriptive titles. Each block contains one set of information such as material properties or coordinates. Many
blocks incorporate a facility for the concise generation of data for regular regions of the structure.

A series of exacting data checks is built into the program. In addition to checking for errors in format and
consistency, many checks are made on the actual values to see if they make sense in engineering terms. The
diagnostic messages are grouped into errors for serious problems and warnings for informative items.

For straightforward analyses, the control of the program is entirely automatic. The management of computer
resources is contained entirely within the program and there is no need for intervention by the user. To give
flexibility, however, the program contains a comprehensive set of control commands which are available if
required. Typically, these commands can be used to control the scope of the results, initiate the Restart facility
or save the backing files for post-processing.

1.4    Using this Manual

This document performs the dual function of being a reference manual for the experienced ASAS user and also
an introductory manual for the engineer who has not previously used ASAS. No attempt is made to teach the
theory of finite elements, as there are several standard textbooks, such as the following:

The Finite Element Method, Zienkiewicz and Taylor, McGraw - Hill, Fourth Edition, 1988.

Concepts and Application of Finite Element Analysis, Robert D. Cook, John Wiley, 1974.

A Finite Element Primer, NAFEMS, 1986.




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


Section 2                is an introduction to the types of analysis. It contains guidance on the selection of element
                         types and provides background information on the key features such as node numbering,
                         local axis systems, consistent units, supports, loading and output control. This section also
                         introduces the ASAS terminology which is used in later sections.

Section 3                describes the data that is needed for each type of analysis.

Section 4                describes the various data formats used by the program, as well as the powerful facilities
                         for data generation provided in ASAS.

Section 5                describes each of the ASAS data blocks in detail, and gives examples of their use.

Section 6                provides the information needed to run the program on specific computers. It also contains
                         simple information regarding the estimating of job size and file handling.

Appendix -A              contains the element specific information for each element in the ASAS library. The
                         element description sheets are a key feature of ASAS documentation.

Appendix -B              gives a summary of various sets of consistent units.

Appendix -C              describes the Options which can be used to control the run, arranged according to their
                         function.

Appendix -D              describes the use of the Restart facility and provides a list of the stages for each type of
                         analysis.

Appendix -E              gives a list of the names of the freedoms which can apply at a node.

Appendix -F              illustrates some sample problems. This Appendix shows every stage in a simple analysis,
                         from the initial thinking process, through the data forms to the printed results.

Appendix -G              describes extended facilities in the Preliminary data.




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



2.       Modelling the Structure

2.1      The Idealisation Process

The art of finite element analysis lies in the representation of a real structure or component and its loading by a
mathematical model which can be analysed by a program such as ASAS.                                      This process is known as
‘idealisation’. It involves the modelling of the structure by a number of elements of finite size (finite elements),
which are connected together only at specified points which are called ‘nodes’. Each node is free to move or
rotate in a limited number of directions, known as ‘freedoms’. Which freedoms apply to a given node is
determined by the element types attached to that node. The behaviour of the idealised model ultimately depends
on the deformations at every node. In heat conduction analysis, the freedom at each node is the temperature
value at the node.

Before proceeding with the idealisation process, the analyst must first examine his problem in general terms and
decide the scope of the analysis and the type of behaviour that is to be modelled. This produces a limited choice
of elements which will approximate the behaviour of the structure to the accuracy required. The majority of
elements in ASAS are based on assumptions which reproduce the distribution of displacement or strain within
the element. The exceptions are the force-equilibrium family of elements which are based on stress assumptions,
and the BEAM family of elements which are as ‘exact’ as the engineering theory of bending. The analyst should
be aware of the approximations inherent in a given finite element and should refine the idealisation accordingly.
Thus, if an element is only capable of reproducing a constant strain distribution, then several will be needed for
modelling an area of rapidly varying strain.

The idealisation process has three phases which are reflected in the data for ASAS:

What is the shape and composition of the structure?

How is the structure supported?

How is the structure loaded?

2.2      Types Of Element

ASAS has a large library of finite elements which are capable of modelling two-dimensional and three-
dimensional structures such as frames, plates, shells or solids. There is no restriction on the number of element
types in an analysis, but few problems need more than four different types.

Each type of element is identified by a distinctive four-character name, which indicates its form and number of
nodes:

         (e.g.       GCS8              =               Generally Curved Shell with 8 nodes

                     TRM3              =               Triangular Membrane with 3 nodes)


Many elements can have isotropic or anisotropic material properties. In the following sections, the elements are
grouped according to their structural form and use. Full details of each element type are given in Appendix -A.




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


2.2.1       Frames

A range of beam and pin-ended elements is available for structures that can be idealised by line members. These
find application in building frames, transmission towers, steel offshore platforms, floors, grillages, etc. For the
BEAM, BM3D, BM2D, GRIL and TUBE elements, properties may be defined explicitly or by way of section
profiles which provides information about the physical shape of the beam (see Section 5.2.6.1 and Appendix
A.7).

BEAM              : 2 node three-dimensional Beam element, transmitting both axial forces and bending moments
                     and suitable for most three-dimensional frames. Includes stepped sections and rigid offsets.

BMGN              : 2 node three-dimensional version of the BEAM element which allows for tapered cross-
                     section, arbitrary local axes and rigid offsets.

BM3D              : 2 node general version of BEAM which allows for the effect of shear deformation, arbitrary
                     local axes, stepped sections and rigid offsets.

BM2D              : 2 node two-dimensional Beam for plane frames subject to in-plane loading, allows for stepped
                     sections and rigid offsets.

GRIL              : 2 node two-dimensional Beam for plane frames subject to out-of-plane loading only, for
                     example, floor grillages. Includes stepped sections and rigid offsets.

CURB              : 2 node three-dimensional Beam curved in a circular arc.

FLA2              : 2 node three-dimensional pin-ended element, suitable for axially-loaded members, stiffeners in
                     membrane idealisation or scalar springs.

TUBE              : 2 node three-dimensional Beam with hollow circular cross-section which allows for arbitrary
                     local axes, stepped sections and rigid offsets.




2.2.2       Membrane Elements

Membrane idealisations are relevant to structures where local out-of-plane bending and shear are insignificant.
Global analyses of box girders, ship hulls and aerospace structures are typical applications. The ASAS library
includes elements based on displacement assumptions and on stress assumptions. The latter include force-
equilibrium elements.

Displacement elements:

TRM3              : 3 node triangle.

TRM6              : 6 node triangle with mid-side nodes allowing curved edges.

QUM4              : 4 node quadrilateral.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 2-2
ASAS (Linear) User Manual                                                                              Modelling the Structure


QUM8              : 8 node quadrilateral with mid-side nodes allowing curved edges.

MEM4              : 4 node two-dimensional rectangle designed for shear walls.

FLA2              : 2 node three-dimensional pin-ended element, suitable for axially-loaded members, stiffeners in
                     membrane idealisation or scalar springs.

FLA3              : 3 node three-dimensional pin-ended element which can be curved, suitable for stiffeners on
                     TRM6 and QUM8 idealisation.

TRM3, TRM6, QUM4 and QUM8 are isoparametric elements designed for three-dimensional analyses. They
can also be used for two-dimensional plane stress and plane strain analyses, but the freedoms in the third
dimension must be suppressed. TRM3, QUM4 and the compatible stiffener FLA2 (see Section 2.2.1) may be
mixed freely. The same is true for TRM6, QUM8 and the compatible stiffener FLA3.

Stress elements:

MOQ4              : 4 node quadrilateral semi-monocoque element incorporating stiffeners.

TSP6              : 6 node triangular shear panel.

WAP8              : 8 node warped quadrilateral shear panel.

WAPT              : 10 node quadrilateral shear panel for transition regions of the mesh.

SQM4              : 4 node quadrilateral membrane panel.

STM6              : 6 node triangular membrane panel.

SQM8              : 8 node quadrilateral membrane panel.

FAX3              : 3 node axial element for use with WAP8, TSP6, STM6 and SQM8.

BAX3              : 3 node combination of FAX3 and BMGN.

As a general rule, quadrilateral elements are to be preferred to triangles. For the equivalent total number of
nodes, the higher-order elements with mid-side nodes are better than the lower-order elements. The structural
details of a particular model may modify these rules, however.




2.2.3       Plates

In two-dimensional structures where in-plane membrane behaviour is insignificant and only out-of-plane
bending is important, the ASAS plate bending elements are applicable. Bridge decks, floor slabs and flat panels
under pressure can be analysed using such elements. There is an important difference between thin plates and
thick plates : the latter allow for the effect of transverse shear deformation and the former do not.




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


TRB3              : 3 node triangular thin plate. The element is only suitable for uniform unstiffened plates of
                     constant thickness. Thin shell formulation only.

SLB8              : 8 node quadrilateral plate, suitable for stiffened and unstiffened plates of variable thickness.
                     Available for thick and thin shell models.




2.2.4       Shells

The ASAS shell elements are those which are capable of modelling both the in-plane membrane behaviour and
out-of-plane bending. They are applied not only to curvilinear shell structures such as pressure vessels, cooling
towers and pipe intersections, but also to faceted structures such as folded plate roofs. Shell elements may be
used for structures where the stresses normal to a surface are to be ignored, and where bending strains vary
linearly through the thickness. There is an important distinction between thin shells and thick shells; the latter
allow for the effect of transverse shear deformation.

ASH2              : 2 node shell element for the analysis of axisymmetric shell structures.

AHH2              : 2 node shell element for the analysis of axisymmetric shell structures under harmonic loading.

TBC3              : 3 node triangular thin shell, combining constant membrane strain and linear bending strain.
                     Beam elements may be used as stiffeners.

QUS4              : 4 node quadrilateral shell element for the analysis of thick or thin shell structures.

GCS6              : Thin shell elements, curved in plan and elevation with 6 (triangular) and 8 (quadrilateral)
                     GCS8 nodes respectively. These elements usually perform well and are recommended for
                     most thin shell structures.

TCS6              : Thick shell elements, curved in plan and elevation, with 6 (triangular) and 8 (quadrilateral)
                     TCS8 nodes respectively. These elements are recommended for thick shell models, but may
                     also be used for thin shell applications.

GCB3              : 3 node Beam element for stiffeners on GCS6 and GCS8.

TCBM              : 3 node Beam element for stiffeners on TCS6 and TCS8.




2.2.5       Solids

A family of solid brick-like elements is available for analysing three-dimensional models of mass concrete
structures, mechanical components, irregular thick structures with local stress concentrations, etc.

BRK6              : 6 node wedge-shaped element.

BRK8              : 8 node cube-shaped element.




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


BR15              : 15 node wedge-shaped element, with curved sides.

BR20              : 20 node cube-shaped element, with curved sides.

BR32              : 32 node cube-shaped element, with curved sides.

TET4              : 4 node tetrahedral element.

TE10              : 10 node tetrahedral element, with curved sides.

BR15 and BR20 are generally to be preferred to BRK6 and BRK8 because of their superior performance and
versatile shape. The BR32 element is capable of even better accuracy, but this is seldom warranted in practice.
The tetrahedral elements, TET4 and TE10, are particularly useful when using free meshing generation facilities
as often found in CAD and solid modelling systems.

For three-dimensional structures or components with axisymmetric shape and axisymmetric loading,
axisymmetric elements are more appropriate.

TRX3              : 3 node axisymmetric element with triangular cross-section.

TRX6              : 6 node axisymmetric element with triangular cross-section, with curved sides.

QUX4              : 4 node axisymmetric element with quadrilateral cross-section.

QUX8              : 8 node axisymmetric element with quadrilateral cross-section, curved sides.

For three-dimensional structures or components with axisymmetric shape and non-axisymmetric loading an
harmonic axisymmetric element is appropriate.

THX3              : 3 node axisymmetric element with triangular cross-section under harmonic loading.

THX6              : 6 node axisymmetric element, triangular cross-section with curved sides, under harmonic
                     loading.

QHX4              : 4 node axisymmetric element with quadrilateral cross-section under harmonic loading.

QHX8              : 8 node axisymmetric element, quadrilateral cross-section with curved sides, under harmonic
                     loading.




2.2.6       Sandwich Elements

A family of sandwich elements is available for analysing plates and shells of sandwich construction. The faces
are modelled by membranes, whilst the core may be viewed as a solid material whose macroscopic properties
differ from those of the face material. Typical applications are the analysis of structures which are made from
honeycomb, or other weak shear core material often used in aircraft and other lightweight structures.

SND6              : 6 node triangular sandwich element




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


SND8              : 8 node quadrilateral sandwich element

SN12              : 12 node triangular sandwich element with curved sides allowed

SN16              : 16 node quadrilateral sandwich element with curved sides allowed

SN12 and SN16 are to be preferred to SND6 and SND8 because of their superior performance and versatile
shape.




2.2.7       Spring Elements

Two simple spring element are included, one to represent simple translation spring stiffnesses and the other
rotational spring stiffnesses. These elements may be used to model elastic foundations and local flexibilities
within the structure which are not modelled directly by the other elements. Local directions other than the global
axes may be specified.

SPR1              : 2 node translational spring

SPR2              : 2 node rotational spring




2.2.8       Crack Problems

The ASAS element library contains a number of special elements for modelling cracked structures. These
elements are used around the tip of the crack and are formulated to represent the singularity at that point.

CK11              : 11 node quadrilateral membrane containing the crack tip. Stress output is in the form of stress
                     intensity factors.

SCK7              : 7 node quadrilateral membrane for problems where the crack lies in a plane of symmetry.

CTM6              : 6 node triangular isoparametric membrane used to model the structure around the crack tip.

CB15              : 15 node wedge-shaped isoparametric solid used to model the structure around the crack tip.

CTX6              : 6 node triangular isoparametric axisymmetric solid used to model the structure around the
                     crack tip.

2.3      Node Numbers and Coordinates

Each node point in the 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 position of these nodes.

If the structure has N nodes, the node numbers need not necessarily be within the range 1 to N; gaps in the
numbering are allowed, and are often helpful to the user. For example, a regularity can be imposed on the




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 2-6
ASAS (Linear) User Manual                                                                              Modelling the Structure


numbers on a line or plane, making it possible to generate the data more economically using the in-build data
generation. In general, it is a sensible precaution to leave gaps in the node numbering so that the idealisation can
be modified to include extra nodes if required, without the need to renumber a large number of nodes to retain a
reasonable ‘bandwidth’.

It is essential to number the nodes in such a way that the maximum ‘node-number-difference’ is kept as small as
possible. The ‘node-number-difference’ for any element is the largest difference between any two node numbers
on the element. Unused node numbers do not count. The maximum node-number-difference affects the
bandwidth of the equations and hence the time to solve the problem. The usual way of minimising the node-
number-difference is by starting to number the nodes in the direction of the fewest nodes.

If no attention has been paid to the node number sequence, the analysis option BAND can be selected which will
invoke the bandwidth reduction scheme. The BAND option is often most efficient when used to reduce the out-
of-core bandwidth. The algorithm employed for out-of-core band reduction is CUTHILL-MCKEE, and its
operation is transparent to the user. This method, together with the IN option may be used to optimise the incore
bandwidth also. However, four other methods KING, LEVY, PINA and SLOAN are available for incore
bandwidth optimisation but, apart from SLOAN, they do take significantly more time to do the optimising, an
order of magnitude or more per pass compared with CUTHILL-MCKEE. This increase can be offset by use of
the START node facility to reduce the number of passes used, see Section 5.1.11. The user may perform data
checks first without the BAND option in order to determine if the data is correct and to discover the size of the
bandwidth. If the bandwidth is unreasonably large then the BAND option should be used for the analysis. Care
should be exercised when using the BAND option on a dynamic analysis as it can have an adverse affect on the
bandwidth, see Section 3.5.2(c). If the analysis is to run in-core the revised element ordering can be done
without renumbering the nodes by adding the IN option to the PASS command.

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, some ASAS elements (e.g. QUM8,
GCS8) have mid-side nodes whose coordinates do not always need defining. If a mid-side node is not defined,
the side is assumed to be straight and the mid-side node is positioned by the program. If the coordinates of a
mid-side node are given, the program defines the shape of the side by a curved line through the nodes. The mid-
side node must lie within one tenth of the side length away from the true mid-side, and the curvature must not be
excessive.

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.

2.4    Global and Local Axis Systems

Regardless of the systems used to define coordinates, the displacement freedoms within ASAS are usually
referred to the global axis system. This is a right-handed rectangular cartesian (X,Y,Z) system, except for the
axi-symmetric elements which use the 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 2-7
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.4.1       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.




2.4.2       Element Local Axes

Many types of element have their own local axes. These are used for the definition of anisotropic properties
(with the exception of shell elements), element loads and stress results. For a few elements, the local axis system
also governs the direction and orientation of special freedoms. The direction of the element local axes is usually
defined by the order of the nodes on the elements. Full details are given in the relevant element description
sheets in Appendix -A.




2.4.3       Skew Systems

Skew systems, can be used for three purposes

(i)     To specify suppressions, prescribed displacements, constrained freedoms (see Section 3.2.3) or master
        freedoms (see Section 3.2.3), in directions other than those of the global axis system. All output of
        displacements (including normal modes) 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 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 used 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 2-8
ASAS (Linear) User Manual                                                                              Modelling the Structure


        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 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 but by specifying a skew integer on the
        material property data line it is possible to input material data in an alternative direction.


2.5     Material Axes for Anisotropic Material

Unlike isotropic material, the coefficients of the material matrix required to define an anisotropic material are
strongly dependent on the choice of material reference axis system. The specification of material coefficients
that are consistent with the definition of material axis system are important to ensure the correct modelling of the
material behaviour.

By default, the material axis system coincides with the stress output axis system defined in Appendix -A. The
only exception is for shell elements where the default material Xm–axis is defined as the projection of global
Xonto the shell surface with Ym lying on the tangent plane of the shell and orthogonal to Xm. For certain
element types the user can override this default by specifying a material skew integer in the material properties
data. In this case, the material constants should be provided with respect to the skew system. For bricks,
displacement based membranes and axisymmetric solids, the skew axis system should be defined relative to the
output axis system, ie the direction cosines are those between the skew axes and the output axes. For shells,
however, a different definition of the skew system is adopted. The skew system is defined relative to the global
axis system instead, and Xm will become the projection of the skew X-axis onto the shell surface. Since the
procedure for defining the default material axis system will fail when the shell surface is normal to the global X,
a skewed material system must be specified in this situation.

Prior to ASAS version H11.2/2032, the material axis definition for shell elements was related to the element
local axis system. For compatibility this definition can still be obtained using option OAIS.

2.6     Data Units

The user is free to choose any system of units for his data. The units for the analysis can be defined explicitly.
These can be locally overridden or changed within each data block if required.

The basic global units to be employed are defined in the Preliminary data using the UNITS command (see
Section 5.1.21) 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.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 2-9
ASAS (Linear) User Manual                                                                              Modelling the Structure


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 PRIME DATA AREA 50000
PROJECT ASAS
FILES ASAS
JOB NEW LINE
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 2-10
ASAS (Linear) User Manual                                                                              Modelling the Structure



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 5.1.21.
        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 does 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. Appendix -B 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).

In substructure analyses it is important that all components and structures have the same global units definition
otherwise assembly of the stiffness matrices and load vectors will not be possible. The program does not assume
that all structures/components created under one project will use the same units, this must be defined explicitly
by the user.

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. The user
can optionally override the results units for displacements and/or stresses to be different from those supplied for
the global definitions. For further details see Section 5.1.21.2.

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.
SI Units :Force in Newtons, length in metres, mass in kilograms, time in seconds, acceleration in metres/sec2
Imperial Units :Force in pounds, length in feet, mass in slugs, time in seconds, acceleration in feet/sec2
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 Appendix -B.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-11
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.7     Structural Suppressions and Constraints

The movement of a node in any direction may start to zero applying ‘suppressions’, or may be 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 this purpose. The freedoms at a node are
determined by the elements meeting at the node. ASAS 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 and rigid constraints.

In a real structure, support is afforded by the foundations or adjacent structure. In the idealised model, such
support can be represented by suppressions, prescribed displacements, constraint equations and sometimes,
loads. For linear stress and heat conduction analysis, it is essential to ensure that there are sufficient restraints on
the idealised model to prevent any possibility of its behaving as a mechanism. In particular, the model or any
part of it must be prevented from moving or rotating freely as a rigid body.

This means:

(i)     The reactions associated with the restraints must be capable of maintaining equilibrium under any loading
        - not necessarily the actual loading.

(ii)    The freedoms at a node must all be restrained or have a finite stiffness associated with them. For
        example, a membrane element has three freedoms at each node, but only has stiffness in the two in-plane
        directions. Stiffness in the out-of-plane direction must be provided by other elements, by suppressing the
        freedom, or by making it dependent on other freedoms by means of a constraint equation. Similar
        situations occur with some shell elements used as plate elements, where the rotation about the out-of-
        plane normal needs to be restrained or provided with stiffness from adjacent elements.


It is important to note that a freedom which is restrained in one loadcase will be restrained in all. Thus, a
freedom labelled as suppressed or constrained is treated as such in all loadcases, and a freedom displaced in one
loadcase must be given a prescribed displacement in all cases, although the value may vary. A prescribed
displacement of zero is equivalent to a suppression, so a freedom can, in practice, be suppressed and prescribed
in different loadcases.

Suppressions are also used to impose the conditions which represent a line or plane of symmetry. This is needed
whenever a symmetrical problem has been halved for economy.




2.7.1       Special Degrees of Freedom

A particular feature of ASAS is the presence of special degrees of freedom in certain of the elements. The
GCS6, GCS8 and GCB3 elements have R1 and R2 degrees of freedom, and the BAX3, FAX3, TSP6, WAP8,
WAPT, STM6 and SQM8 elements have the S degree of freedom. These special freedoms are always associated
with element mid-side nodes and are always dependent on the node numbering of the individual elements. The
R1 and R2 freedoms are rotations about the edge, being positive in the sense of a right hand screw about the




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-12
ASAS (Linear) User Manual                                                                              Modelling the Structure


edge from the lower numbered corner node to the higher numbered corner node. The S degree of freedom is
similarly arranged along the element edge in the direction from the lower numbered corner to the higher.

In normal situations, ie. where there is full connectivity between elements, these degrees of freedom will always
be compatible between adjacent elements, see Figure 2.1(a). If however there are any unusual modelings, where
there is no longer a full connection between elements, for some reason, it is possible that the implied directions
no longer match. This can lead to erroneous answers and should always be guarded against. See Figures 2.1(b)
and 2.1(c)
      1                    4                     6            9                    11
                            s                                     s

                                                                                               Normal inter-element
                                                                                               connection. Freedom
    2         s                          s   7       s                      s      12          directions all correct, note
                                                                                               node 7.

                            s                                     s

        3                  5                     8            10                   13
        1                  4                     6            10                   12

                            s                                     s


                                                                                               Abnormal element connection.
    2         s                          s   7       s                      s      13          Because nodes 8 and 9 are both
                                                                                               greater than node 6, the S freedoms
                                                                                               at node 7 both go in the same
                                                                                               direction.
                            s                                     s

        3                  5                 8 9              11                   14
        1                  5                     8            10                   11
                            s                                     s
                                                                                               Abnormal element connection.
                                                                                               The S freedoms at node 7 are
                                             7                                                 incompatible due to node 4
    2         s                          s           s                      s      12
                                                                                               being less than node 8 on the left
                                                                                               element and node 9 being greater
                                                                                               than node 8 on the right element.
                            s                                     s

    3                      6                 4 9              13                   14


                                    Figure 2.1 Examples of the use of special freedoms




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 2-13
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.8      Loads

The word ‘load’ has a general meaning within ASAS. It signifies any externally imposed influence and includes
prescribed displacement and temperature variation as well as forces and moments. ASAS permits any number of
different loading types to be combined in a single loadcase, and any number of loadcases within a single
analysis. Moreover, a facility is available to apply a new set of loads after an initial analysis, without repeating
all the calculations (see Section 3.3). The individual types of loading are described below.




2.8.1       Nodal Loads

A nodal load can be a force, moment or other generalised force associated with a freedom at a node. This is the
most basic form of loading. Nodal loads may be applied in skew directions by linking them with appropriate
skew systems (see Section 2.4.3). Nodal loads applied to axisymmetric elements are defined on a per radian
basis.




2.8.2       Prescribed Displacements

Prescribed displacements are used to impose fixed values for specific freedoms at a node. The user specifies
which freedoms are to be prescribed and then quotes the displacements for every loadcase in turn. Prescribed
displacements can be applied in skew directions (see Section 2.4.3). The ASAS results include the calculated
reactions at each displaced node.




2.8.3       Pressure Loads

A constant or 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 face. The default direction in which the pressure acts depends
on the type of element and its local axis system as described in Appendix -A. Pressure can also be applied in a
specific direction.




2.8.4       Distributed Loads

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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-14
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.8.5       Temperature Loads

ASAS can determine the effect of thermal straining due to a given distribution of temperature. The distribution
can be defined at the nodes or on elements. The ambient temperature of the structure is assumed to be zero. The
temperature loads only apply to the stated nodes or elements. Mid-side nodes are interpolated between adjacent
corner nodes and all other undefined nodes or elements are assumed to be at zero degrees.




2.8.6       Face Temperatures

For some elements used in plate and shell structures, the effects due to a difference of temperature through the
thickness of the 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.
Unspecified values at element corner nodes are assumed to be zero but values at mid-side nodes are always
linearly interpolated from the values at the adjacent corner nodes.




2.8.7       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 resulting inertia 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 2.6).




2.8.8       Centrifugal Loads

Centrifugal loading is available for some element types. 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 2.6).




2.8.9       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 2.6).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-15
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.8.10      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 these tanks. By specifying the tank geometries together with
the internal fluid levels and densities, ASAS can automatically calculate the pressure loads on the tank walls.

2.9     Results From ASAS

During the data input, ASAS produces sorted lists of the various types of data and also outputs summaries and
other useful information. Following the solution stage ASAS will list out the displacements, reactions, stresses
and other results. All of this output may be controlled by various Options (see Appendix -C).




2.9.1       Input Data Images

ASAS normally prints the image of each line of data as it is read. However, by setting the appropriate control
options, this printing can be suppressed for all except specified data blocks. Data which are found to be in error
are printed with an appropriate error message.




2.9.2       Expanded Data and Summaries

ASAS normally prints a complete list of expanded and cross referenced data. By setting the appropriate control
option, only selected summaries are printed.




2.9.3       Results - Displacements and Reactions

For linear stress analysis, the values of the displacements and reactions are listed at every node for all loadcases.
For heat transfer analysis, the ‘displacements’ and ‘reactions’ are the values of the temperatures at the node and
the heat sources or sinks. Up to five loadcases of results are printed side by side on a page; further sets of results
follow immediately after the first set.

The reactions are the forces exerted by the restraints on the idealised model. For heat conduction analysis, a
positive thermal reaction indicates a heat input to the model. If a restraint has been applied at a node in a skew
direction, then the displacements and forces at that node are in the skew direction.




2.9.4       Results - Frequencies and Normal Modes

For natural frequency analysis, the frequencies in cycles/second (e.g. hertz) and the associated normal modes are
printed side by side across the page. The normal modes are described by the master freedoms only, and




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-16
ASAS (Linear) User Manual                                                                              Modelling the Structure


normalised such that the maximum value is one. If a skewed node exists, then the master freedoms at the node
are in the skew directions. By request, the modes may be scaled to give the Euclidean norm. The components of
each normal mode corresponding to non-master freedoms are printed separately.




2.9.5       Results - Stresses

Stresses are determined in linear stress analysis. They are listed for one loadcase at a time, and within each
loadcase the stresses are listed in the order of the group numbers. Within each group the stresses are printed by
element type, and within each element type in order of the user element numbers. These element numbers are
defined by the program unless the user defines his own element numbers in the element topology data (see
Section 3.2.2).




2.9.6       Analysis Summary

At the end of the ASAS run, a summary of the analysis details is given. This is a useful check on the number of
elements, nodes, etc., especially after a data checking run.




2.9.7       Results - Post-Processing

ASAS allows for the results of an analysis to be accessed by other post-processing programs. The model data
and its results in terms of displacements and stresses, natural frequencies and mode shapes can be saved on file
and further calculations carried out or the results presented in various graphical forms.

2.10 Substructured Analysis

In a simple one-step analysis the program reads the data for the entire structure and forms a set of simultaneous
equations describing the relationship between force and displacement at each node in the structure. These
equations are solved as a single process for the whole structure, followed by the formation of stresses in all the
elements. In a substructured analysis only part of the structure is analysed in each run and the complete solution
is a three-step process. Firstly, each part (or component) is solved up to its boundaries with other components.
Secondly, the boundaries of a series of components are assembled together to form the whole structure and
solved. Finally, the boundary displacements are passed back into each component in turn and combined with the
initial partial solution to form the total displacements and element stresses.

In the ASAS multilevel substructure technique, steps one and two may be repeated using both elements and
lower level components to form more and more complex assemblies.

An example of the use of components to model a box girder bridge deck is shown below. Many of the facilities
available in ASAS substructure analysis are illustrated.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-17
ASAS (Linear) User Manual                                                                              Modelling the Structure


Initially five master components are created from quadrilateral plate elements. These components, named
SUB1-SUB5, represent the top, bottom, side, centre and end plates of a single box from which the whole of the
bridge is constructed.

Four components, SUB1, SUB2, SUB3 and SUB5 are assembled to form a another master component SUB6.
Two copies of SUB6 are assembled to form master component SUB7.

Master component SUB8 is formed from 2 copies of SUB4, SUB7 and SUB7 mirrored about the centre-line of
the bridge.

Finally, the whole bridge deck is constructed from six copies of SUB8, translated to join end to end, and two
further copies of SUB3 to complete the end plate.

Displacements and stresses for part or all of the structure may be extracted by one or more stress recovery runs.

If the bridge deck were to be analysed as a single structure, over 3,600 elements would have been required. By
using substructuring, data for only 5 small components consisting of a total of 160 elements are required. The
saving in data preparation costs alone are obviously very substantial.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-18
ASAS (Linear) User Manual                                                                              Modelling the Structure


                                                                              SUB2

  SUB1




    SUB3


           SUB4
                                                                                                                    SUB5




        SUB6


                                                                                                                      SUB7




                                                                                                DECK


                               Figure 2.2 Example of a Multilevel Substructure Analysis




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-19
ASAS (Linear) User Manual                                                                              Modelling the Structure


2.10.1       Planning a Substructured Analysis

The idealisation process for substructured analysis is basically the same as that laid down in Sections 2.1 to 2.9.
However, if the process is to be applied successfully, thorough planning of the subdivision of the structure, its
assembly and its loading is necessary before any detailed ASAS data is prepared. Three extra data blocks will
also be required, namely LINK freedoms to define the component boundaries, component TOPOlogy to describe
the assembly of components or substructures together and COMPonent LOADS to describe the assembly of the
load data.

Following an initial study of the total structure and the definition of the aims of the analysis, the next step is to
plan the subdivision of the total structure into components. The lowest level components may be joined together
to form sub-assemblies or directly into the global structure. Once the global structure has been solved, the results
for each individual component may then be calculated as required.

The choice of suitable components and boundaries is discussed below but once the choice has been made, a tree
diagram should be drawn and the various names assigned to the components, files, etc. Even the simplest
substructure analysis will require several computer runs and a logical choice of names will greatly assist in the
easy solution of the task.



Project Name

All computer runs associated with a particular substructure analysis must be carried out under a common Project
Name. This four character identifier is used to set up a project file, in which details of every run carried out in
this project are stored. Thus every component creation run, global structure run, stress recovery run and post-
processing runs will make reference to this project file.



Master Component Name

A Master Component is a substructure formed by the assembly of finite elements and other components already
stored within the project file. The lowest level substructures consist only of finite elements.                        A Master
Component creation run assigns a four character Master Component Name to the component being created. This
name is used whenever the Master Component is used in a higher level assembly. (It is equivalent to an element
name such as BM3D or GCS8).

Within one project, every Master Component Name must be unique from all other Master Component Names or
Structure Names.



Assembled Component Name

Any Master Component may be used to assemble higher level components or global structures. A given Master
Component may be used in more than one assembly and may be used more than once in any given assembly by
using translation, rotation or mirroring. In order that every part of the structure may be uniquely referenced,




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-20
ASAS (Linear) User Manual                                                                              Modelling the Structure


each time a master component is assembled at a higher level it is given a different unique four character
Assembled Component Name. (This is equivalent to the user element number.)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-21
ASAS (Linear) User Manual                                                                              Modelling the Structure



Global Structure Name

The final assembly of components and elements represents the whole structure. This is given a four character
Global Structure Name which must be unique from all other Structure or Master Component Names.

Figure 2.3 illustrates the use of master component names and assembled component names in the assembly of
one quarter of a plate with three holes along the centre line. Figure 2.4 shows the corresponding tree diagram.
After assembly of the global structure, any part of the structure may be uniquely referenced by specifying the
assembled component name at every level in the branch in which it occurs.

For example              STRC A401 A301 A202

                         STRC A402 A306

Although these two examples both refer back to the same Master Component (C002), they refer to different parts
of the global structure.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-22
ASAS (Linear) User Manual                                                                              Modelling the Structure




                                                                                                                 Level 1
               C001                                  C002                              C003                      Elements only




                                                                                                 A307     C006   Level 2
                                                                                                 A306
                                                                                                                 Components
    C004            A201
                                 A202                                                   A305
                                                                                A304




                                     A302                A303

    C005                                                                                                         Level 3
                                                                                                                 Components
                    A301




                                                       A401

                                                                                                                 Global Structure
                      STRC                                                                A402                   Components




                                                                                MASTER COMPONENT NAME C004
                                                                             ASSEMBLED COMPONENT NAME A301

                                          Figure 2.3 Typical Substructure Assembly




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page 2-23
                                                                                                                                                                                                                                                          ASAS (Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.




                                                                                                        C001          C002     C001           C002         C001           C002          C002        C002          C002           C003

                                                                                                        A201          A202     A201           A202         A201           A202          A304        A305          A306           A307



                                                                                                                                                                                                                                 Level 1


                                                                                                               C004                    C004                        C004                                    C006

                                                                                                               A301                    A302                        A303                                    A402


                                                                                                                                                                                                                                 Level 2


                                                                                                                                       C005

                                                                                                                                       A401


                                                                                                                                                                                                                                 Level 3




                                                                                                                                                                                                                                            Modelling the Structure
                                                                                                                                                                       STRC                                              Global Structure



                                                                                                                 MASTER COMPONENT NAME         C004            COMPONENTS GENERATED FROM               C001
                                                                                                                                                               ORIGINAL MASTER COMPONENT
                                                                                                               ASSEMBLED COMPONENT NAME        A301            BY SHIFT, MIRROR OR ROTATION            A201
Page 2-24




                                                                                                                             Figure 2.4 Example of a Tree Diagram for the substructure assembly in Figure 2.3
       ASAS (Linear) User Manual                                                                       Modelling the Structure




2.10.2      The Choice of Master Components

In concept, substructuring may be applied to any linear stress analysis, but there are a number of areas where it is
particularly appropriate. Some examples are described below and, in each case, they indicate a natural choice of
master components and their associated boundaries.

Whether or not natural subdivisions are present, two general principles should be considered. Choosing short
boundaries reduces the cost of the master component creation run. It is also more efficient if the boundary can
be confined to a local area of the component for example one end of a tube rather than both ends.



Repetitive Symmetry

A large number of structures contain some degree of symmetry or have common areas which are repeated
several times. Such a region of the structure may be solved as a component and several copies assembled
together using the translation, rotation or mirroring facilities to form the whole structure. Since the component is
created only once but used several times savings in man time and computer time can be made.



Sub-Division of Large Structure

For very large structures it may be inconvenient or even impossible to carry out the analysis in a single pass.

The computer time to solve a large problem may be unacceptably long even using the restart facilities in ASAS.
By sub-dividing into components each run is reduced to a more convenient length and this can have benefits in
various other ways.

The task of data preparation and data checking may be shared more easily between several people.

In the event of errors being found in the data or runs exceeding computer resource limits, it is only necessary to
repeat the calculations for the component involved.

The total computer costs for the analysis by components may be significantly less than the cost of a single shot
analysis of the whole structure. (However, this is not always the case).

Disc memory may limit the size of problem which can be solved. By use of substructuring, unwanted data at any
stage may be off-loaded from the disc onto magnetic tape and copied back when next required.



Re-analysis of Part of a Structure

It may be required to analyse part of a large structure in detail and later modify and re-analyse that part. By
isolating the area concerned as a component, it will only be necessary to re-analyse a small part and reassemble
the global structure using other existing unchanged components. Since it is possible to use elements at any level
of a substructured analysis, an alternative to the above procedure would be to include the area of interest as




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-25
       ASAS (Linear) User Manual                                                                       Modelling the Structure


elements at the global structure stage. Results in terms of displacements and stresses would be immediately
available and modification could be incorporated into a single re-run of the global structure.



Identification with Manufacturing Components

Many structures consist of an assembly of separately manufactured parts or components. These parts may have
been designed in different departments, different companies or even different countries.                       It is sometimes
convenient to identify the sub-division of the analysis with the design component.



Common Components

Several variants of a product may be manufactured using common components. These common components
may be modelled separately as ASAS components and stored under a common project name. Later these
components may be assembled together to represent each variant and any future variants if required.



Stiffness Input Components

When a component creation run has been performed on a different machine or even a different program, the
resulting data including the stiffness matrix, loading or mass data may be input to form the data required to
include the component in a higher level run of the current substructure analysis (see Section 3.7.2.2). Master
components created in this way can be subsequently used in the same way as those created by the more normal
methods except that, when stress recovery is performed for each occurrence of these master components, only
the displacement values for the link freedoms will be output.




2.10.3      Component Link Node

Components are joined to other components only along predefined boundaries. A component boundary is
defined at the time of the master component creation run by listing the nodes and freedoms which form the
boundary in the LINK freedom data. The following points should be noted:

1.     A component can only have one boundary. Therefore all nodes points which will ever be used to link to
       other components should be included in the LINK data.

2.     Any or all of the freedoms present at a node may be chosen as link freedoms. Only those freedoms
       chosen will be available when the master component is used at a higher level.

3.     Nodes chosen as link nodes do not necessarily have to link with other components at a higher level. It
       may, for instance, be desirable to include the nodes on a plane of symmetry so that boundary conditions
       may be varied at the global structure stage.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-26
       ASAS (Linear) User Manual                                                                       Modelling the Structure


4.     It is necessary to define sufficient freedoms at a link node to fully describe the required structural action
       between the components meeting at a boundary. It may be correct to leave out a bending freedom if it
       were intended to model a hinge at the boundary.

5.     In general all nodes along a boundary should match with those on the component to which it is to be
       assembled. For example, it is incorrect to match elements with mid-side nodes to elements without mid-
       side nodes. In this case continuity is violated at the mid-side node.

6.     Link freedoms may be loaded at the master component creation stage or may be loaded when the
       component is assembled at a higher level. Care must be taken not to include loads on boundaries twice.

7.     Link freedoms may not be skewed, supported or displaced at the master component creation stage.




2.10.4      Component Assembly

First level Master Components consist of finite elements only. Higher level Master Components may be
assembled from elements and components. The location of each assembled component is defined in the
component topology data. The following points should be noted:

1.     A master component may be used several times in any assembly.

2.     Each assembled component must be given a unique Assembled Component Name.

3.     A component may be translated, or rotated, or mirrored before assembly. A sensible choice of the
       coordinate system for a master component creation run may simplify the problem of positioning the
       component in a higher level assembly.

4.     As a consequence of 2. and 3. above, each assembled component is described individually in the topology
       data. Generation of several components using the repeat facility is not permitted.

5.     The choice of node numbers in a master component or global structure run is unconnected with the node
       numbering in any other run. However the order of the nodes in a LINK node data when the master
       component is created must correspond with the order of the nodes in a TOPO data, when that component
       is assembled.

6.     In any higher level assembly it should only be necessary to define coordinates for nodes to which only
       elements and not components are attached. The position of all other nodes is implied by the positioning
       of the components.




2.10.5      Component Loading

Loading can be applied at each level of component creation and at the global structure stage.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-27
       ASAS (Linear) User Manual                                                                       Modelling the Structure


Loading can be in the form of nodal loads, element loads or by reference to component loadcases which have
been previously solved during the creation of master components.



Nodal Loads

During component creation runs and global structure runs, nodal loads and prescribed displacements may be
applied to any node and freedom that actually exists at that stage. However nodal loads and prescribed
displacements cannot be applied to nodes or freedoms which have been eliminated at a lower level component
creation stage.



Element loads

Element loads can be applied to any elements which actually exist during any component creation or global
structure run. Element loads include pressure, temperature, face temperatures, distributed loads, body and
acceleration loads. However, element loads may be not be applied to any elements which have been eliminated
at a lower level master component creation stage.



Component loads

Loadcases which have been applied during a particular master component creation stage can be referenced at the
time that the component is assembled in a higher level assembly to include those loads at that point. This is done
by use of the COMP LOAD data. If a loadcase is not referenced in this way, that loadcase is not automatically
included in the assembly. Component loadcases included in this way, may be factored and combined together
during assembly with other component cases, with nodal load and with elements loads to form new loadcases as
appropriate.



Global Structure Loads

The final loadcases formed at the Global Structure stage from component loads, nodal loads and element loads
are the only loadcases relating to the whole structure and therefore are the only cases for which results,
displacements and stresses, can be obtained.




2.10.6      Component Recovery

The results obtained from the Global Structure run are for the nodes, freedoms and elements which were
assembled at that stage. To obtain results for the other nodes and elements which were used in each of the
components we must use a process which is the reverse of the assembly process. The results from the global
structure form the boundary conditions for each component assembled into it. The entire displacements and
stresses for each of these components may then be obtained and the boundary conditions for the next lower level




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-28
       ASAS (Linear) User Manual                                                                       Modelling the Structure


of components extracted. This process may be continued until the results for all components have been obtained.
The following points should be noted:

1.      An assembled component is uniquely identified by the list of assembled component names at each level
        from the global structure down to that component.

2.      Where a master component has been used several times in a structure, there will be a different set of
        results for each assembled occurrence of that master component.

3.      It is not necessary to recover all the cases for all the components. The user may select which cases to
        obtain and for which components.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-29
       ASAS (Linear) User Manual                                                                        The ASAS Analysis



3.      The ASAS Analysis

3.1     Preparing for the Analysis

ASAS can be used for seven types of problem:

i.      Linear static stress analysis (see Section 3.4).

ii.     Natural frequency analysis (see Section 3.5).

iii.    Steady state heat conduction analysis (see Section 3.6).

iv.     Substructured linear static stress analysis (see Section 3.7).

v.      Substructured natural frequency analysis (see Section 3.7).

vi.     Gap analysis (see Section 3.8).

vii.    Substructure creation from an external stiffness matrix (see Section 3.7.2.2).


The details of each type of analysis are described in the following sections, but the preparatory process always
takes the following form:

1.      Identify what is expected of the analysis.

2.      Decide whether or not to substructure the problem. If so, thoroughly plan the whole analysis paying
        particular attention to the interfaces between each component that the structure is divided into.

3.      Select the appropriate types of finite element, loading, boundary conditions.

4.      Create the finite element model for ASAS.

5.      Check the results with a visualisation program.

If substructuring has been used

6.      Repeat items 3-5 for each component.

7.      Assemble the components together to form higher order components or the total structure.

8.      Select loadcases for each assembled component.

9.      Solve for each assembly until the solution for the total structure has been achieved.

10.     Using the displacements for the total structure calculate the displacements and stresses for each
        component.




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


3.2     Description of Each Data Block

The data for ASAS is prepared as a series of blocks of information, each specifying a particular feature of the
data. The details of the data required for each type of analysis are given in the appropriate section, although
there is much commonality. The data formats are described in Section 5 Extensive data generation facilities are
provided for the rapid creation of regular data (see Section 4 and Section 5).




3.2.1       Preliminary Data - see Section 5.1

The Preliminary Data is the first block of the ASAS data. This data defines the job type (eg whether statics or
dynamics), the identity of the project and the structure/component to be processed within the project, options
which affect the course of the run, the amount of printing produced and the files saved for further processing. It
also allows the memory size to be defined for runs requiring larger amounts of memory.

The Preliminary Data must terminate with an END command but the other commands may in general be in any
order. However it is recommended that the user follows the order in Section 5.1.

The SYSTEM command is optional and specifies the computer resources which are required by this run. In
particular, it defines the amount of working space in memory to be used by this run. See Section 5.1.1.

The project name is specified using the PROJECT command.                              This name links together any number of
individual runs which may be considered to be part of the same project. For the first run in any project, the word
NEW appears on the JOB command and a new project file is created. All subsequent runs within the same
project must have this project file available to them and each run will add information to the file. Hence, a job
may only access files created by other runs if they were run under the same project. See Section 5.1.2.

The JOB command indicates the type of analysis to be performed. The job type specifies one of nine possible
analysis types: single-step (non-substructured) linear stress (LINE), single-step natural frequency (FREQ),
steady state heat conduction (HEAT), substructured linear stress - component creation (COMP), global structure
assembly (LINE), recovery of component displacements and stresses (RECO), substructured natural frequency -
component creation (COMD), global structure (FREQ) or substructured component creation from a set of
formatted stiffness input data (STIF). See Section 5.1.3.

A STRUCTURE command is used to define a 4 character name used to identify the structure being analysed and
to identify the results saved in the project database.

For substructure analyses, when a master component is being created, a COMPONENT command must be used.
This contains the four character name which will be used to identify this component in future runs. When all
components have been assembled and the global structure is being solved, a STRUCTURE command must be
used to identify the assembled structure. See Sections 5.1.4 and 5.1.5.

The STRUCTURE command is also required for a stress recovery run when the displacements and stresses for
the individual components in a substructure analysis are being formed.

A backing file prefix name can be specified using the FILES command. This name identifies any files created
during this run. If omitted the files are identified by the STRUCTURE name. See Section 5.1.6.




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


A TITLE command is included in the Preliminary Data. The title specified using this line is printed at the top of
every page of output from this run. See Section 5.1.7.

The TEXT command is optional but any text specified on these lines is printed at the start of the run. Thus full
descriptive text may be included on the output. See Section 5.1.8.

For beam type elements, BM2D, BM3D, BEAM, GRIL and TUBE the geometric properties may be supplied by
way of defining the shape and cross-section details in lieu of explicit stiffness property information. The cross-
section details may be conveniently stored in an external section library file which can be standardised for
particular projects/applications (see Appendix A.7). The library file is referenced by including the LIBRARY
command which specifies the external physical file name that contains the section information to be referenced
by the program. See Section 5.1.22.

One or more OPTIONS command may be included, containing four-character control options (see Section 5.1.9
and Appendix-C). If the BAND option is specified then the bandwidth reduction facility will be invoked. The
OPTIONS command can be followed by a PASS command (see Section 5.1.10) defining the type of
optimisation and the number of attempts to reduce the bandwidth.

The user may choose to run the program in stages. In this case a RESTART command is used to define the
stages at which the program will start and finish in this run. See Section 5.1.12.

During the data checking, the program will calculate the sum of the applied loads in each direction for each
loadcase. It will also calculate the moment of the applied loading about the origin point. This point may be
redefined using the GOTP command. See Section 5.1.13.

For natural frequency analysis, the FREQUENCY command must be included, which contains several control
parameters for defining the number of frequencies, type of eigenvalue solution, etc. See Section 5.1.16.

A SAVE FILES command may be included to save files or sets of files for use in subsequent ASAS runs and/or
post-processors. The subsequent ASAS run may require a COPY FILES command to retrieve the required files
or sets of files. See Sections 5.1.17 and 5.1.18.

A RESU command may be included to save the run results permamently. See Section 5.1.19.

For extended facilities in the Preliminary Data refer to Appendix -G.

Examples of Preliminary Data are given in Sections 3.4, 3.5 and 3.6. See also Appendix -F.




3.2.2       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)      Coordinate 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 transforms




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


       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)

       This data defines the location of each of the elements by reference to its node numbers. 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 integer numbers which refer to the Geometric Property Data. Each
       line also contains a flag which indicates whether the element mass matrix is to be lumped, consistent or
       not used at all. This flag should be ignored for linear stress and heat conduction analyses. If it is omitted
       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 and also a ‘group number’ to a set
       of elements. These numbers control the order in which the results are printed and are also used by pre-
       and post-processing programs to aid element selection.

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. All elements have homogeneous properties which can be either isotropic,
       orthotropic, anisotropic or laminate. For isotropic material, the modulus of elasticity, Poisson’s ratio,
       coefficient of linear expansion and density may all be required. For orthotropic material, the density, the
       three local values of Youngs modulus, shear modulus, Poissons Ratio and expansion coefficient are
       required. For anisotropic material, the density, coefficients of the symmetric stress-strain relationship and
       the coefficients of linear expansion must be provided. The detailed needs of each element are given in
       Appendix -A. The anisotropy facility can be used to describe plane strain behaviour in membrane
       elements, and also orthotropy where appropriate.

       In heat conduction analysis, the material properties are the thermal conductivities.                For 2-D panel
       elements, two conductivity coefficients Kx, Ky are required. For solid 3-D elements the coefficients Kx,
       Ky, Kz are required. For isotropic material behaviour, Kx = Ky = Kz, but all values must be specified. If
       the material behaviour is anisotropic, Kx, Ky, Kz are referred to the element local axes.                For heat
       conduction analysis both isotropic and anisotropic material behaviour is represented by the isotropic
       material definition.

       The unit of conductivity in heat/(degree x length3 x time) must be consistent with those of length,
        temperature and nodal heat vector (see Section 2.6).

d)     Geometric Properties Data (see Section 5.2.5)




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


       This data defines the geometric properties of the element, such as thickness or cross-sectional area. The
       solid elements such as the Brick family have no geometric properties.

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

e)     Section Data (see Section 5.2.6)

       This data is used as an alternative means to define properties for beam element types BM2D, BM3D,
       GRIL, BEAM and TUBE. In order to generate the flexural properties required by ASAS 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.

       Section data can alternatively be input by way of an external library file. See Appendix A.7.

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 may be defined either in terms of direction cosines or by 3 node points. Skew
       systems are not used in heat conduction analysis and are not always needed for linear stress or natural
       frequency analysis.

g)     Component Topology Data (see Section 5.2.9)

       This data is only used in substructure analyses. It is used to define the assembly of existing master
       components to form a higher level master component or the global structure assembly. Each component
       is described using up to four types of command.

       The position of each component is defined with three commands by giving translation, rotation and
       mirroring information. Any or all of these commands may be omitted if appropriate.

       The final command type defines the component names and node numbers. Two four-character names are
       used.     The first name is the name given on the COMPONENT command at the time this master
       component was created. Since one master component may be used several times in an assembly, a
       second name is assigned, the assembled component name, to separately identify each occurrence of a
       master component. Each assembled component name must be unique. Also on this command the node
       numbers must be listed. This node list must correspond exactly to the order defined in the LINK data
       during the creation run of this master component (see Section 3.2.3(d)).




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


3.2.3         Boundary Condition Data - see Section 5.3

The Boundary Condition Data defines how the idealisation is restrained or constrained. It cannot be varied from
loadcase to loadcase. In a natural frequency analysis, if the restraints are not sufficient to prevent all rigid body
movements, including mechanisms, then care must be taken when using the SPIT method of frequency
extraction.

(a)     Suppressions 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 a global axis, then Skew Systems Data is also required (see Section 2.4.3). This data has
        no significance for heat conduction analysis.

(b)     Displaced Freedoms Data (see Section 5.3.4)

        All freedoms which are to be given a known value of displacement are listed in this data. Freedoms may
        be displaced in skew directions by reference to a skew system. The actual values of displacement are
        listed separately, loadcase by loadcase in the Prescribed Displacements Load Data. This data has no
        significance for natural frequency analysis. For heat conduction analysis, this data together with the
        Prescribed Displacements Data defines the fixed temperatures of the nodes.

(c)     Constraint Equation Data (see Section 5.3.5)

        This data defines any required linear dependence between freedoms. The dependent freedom on the left
        hand side on 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)     Link Freedom Data (see Section 5.3.6)

        This data can only appear in a master component creation analysis. It defines the nodes and freedom that
        will be used to describe how this master component is assembled to other components in any higher level
        of assembly. In general, therefore, these nodes will be on the boundary of the component.

        It is important to note that the order in which the node numbers are first encountered in this link data
        defines the order in which they must be listed when this master component is used in a subsequent
        assembly run. All other nodes and freedoms not mentioned in this data will be treated as internal to the
        master component. Any local mechanisms or singularities associated with these internal freedoms must
        be removed by suitable suppressions or prescribed displacements applied in the master component
        creation run.

        It should also be noted that freedoms designated as link freedoms cannot appear in the suppressions or
        Displaced Freedom Data, or as dependent freedoms in constraint equations in the creation run. Restraint
        applied to a link freedom must be applied at a higher assembly when the corresponding freedom becomes



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


       an internal freedom. Any restraint applied to internal freedoms of a master component will, of course,
       also become restraints to the assembled structure.

       Link freedoms may be skewed by reference to a skew system.

(e)    Dynamic Master Freedom Data (see Section 5.3.7)

       This data can only appear in a natural frequency analysis. It lists all the freedoms which are to be retained
       as master dynamic degrees of freedom. Any freedom not listed is treated as a ‘slave’ or internal freedom
       and is automatically eliminated from the eigenvalue extraction process. A suppressed freedom or a
       dependent freedom in a constraint equation is treated as a slave and must not appear in this data.

       Master freedoms may be skewed by reference to a skew system.

       If the suppressed freedoms are not sufficient to remove all rigid body modes and local mechanisms, then
       the chosen master freedoms must be sufficient to describe the remainder. A master freedom must not be
       made dependent on slave freedoms.

       If this data is not present, all freedoms are treated as master freedoms, except for suppressed freedoms
       and dependent freedoms in constraint equations.

(f)    Rigid Constraint Data (see Section 5.3.8)

       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.

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

(g)    Freedom Release Data (see Section 5.3.2)

       This data block defines freedoms which are to be disconnected on specified elements at specified nodes.
       To distinguish a released freedom from the conventional degrees of freedom in the output, a unique user
       defined freedom code must be given. 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.

       For beam elements, a release may be provided in the beam local axis system 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.

(h) Gaps Data (see Section 5.3.10)




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


        This data can only appear in a Gap analysis. It lists pairs of nodes which are separated by gaps. Gaps are
        used to model areas of the structure where, according to the loading on the structure, two nodes may or
        may not be in contact.

        It should be noted that every node listed in the Gaps Data will have a skew system associate with it. For
        each gap the first node listed will become the dependent node and the second node will become the
        independent node for an internally generated constraint equation.




3.2.4       Loading Data - see Section 5.4

The Loading Data describe how the model is loaded by external forces and other influences. It is only required
in linear stress, heat conduction and component analyses. The data is prefixed by the Load Header command.
There is no limit to the number of loadcases.

Each loadcase is prefixed by a Loadcase Header Command, defining the user loadcase number and case title.
The loadcase number has no significance except for identification, but should be unique from all other loadcase
numbers. It is printed at the head of all displacement and stress output and is used to reference the results when
stored in the database.

For linear stress analysis, each loadcase may contain any number of load types but only one data block of any
given type is permitted within the same loadcase (see Section 2.8).

Heat conduction analysis only uses the counterparts of nodal loads and prescribed displacements. The ‘nodal
loads’ are the values of the heat sources or sinks, with a +ve value if heat is input into the body. A distributed
heat flux can be represented by a set of nodal loads.                      The ‘prescribed displacements’ are the values of
temperature at the nodes which are listed in the Displaced Freedoms Data.

For substructured analyses a component load data block may be required. In any run when components are being
assembled to form a higher level master component or global structure, it is possible to include loading data
defined at the time when the lower level components were created.

The component load commands contain the assembled component name, a loadcase number and a factor by
which the loads are to be multiplied. A new loadcase may, therefore, be built up from the loadcases previously
applied to the master components.

Note that the loads selected from the master component are transformed (within the program) to the current axis
system before being added to the new loadcase being formed.




3.2.5       Additional Mass Data - see Section 5.5

Direct Mass Data

This data lists the freedoms and associated lumped mass (inertia) values which are to be added to the finite
element model. For a natural frequency analysis, the mass matrix so described can either replace the mass



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


matrix assembled from each element (FULL MASS) or it can augment the finite element mass (ADDED
MASS). If FULL MASS is specified, the matrix should correspond to the freedoms listed in the Master
Freedom Data and have a positive non-zero value for each master freedom. If the SPIT method of eigenvalue
extraction is used, a zero mass value is permitted but the number of non-zero mass values must be equal to or
greater than the subspace size. See Section 5.1.16. Each lumped mass must only be associated with the
freedoms present on the elements generated by the Element Topology Data.

For statics analysis 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.




3.2.6       Component Recovery Data - see Section 5.6

This data is only used for a component recovery analysis.

For a substructure stress recovery run it is necessary to identify which components and which loadcases are
required. The COMPONENT command defines the branch containing the assembled components for which
stress recovery is required, followed by the SELECT LOADS command to define a subset of loadcases.
COMPONENT commands followed by SELECT LOADS commands may be repeated as often as necessary to
fully identify the parts of the structure for which results are required. However, to resolve conflicts in this data it
may be necessary for the program to recover more loadcases than the user actually asks for. Therefore the user
is recommended to subdivide his stress recoveries into a number of separate runs if different load selection is
required for different parts of the structure.




3.2.7       Combined Loading Data - see Section 5.8

The basic loading information is defined as described previously (see Section 3.2.4). These loadcases can
subsequently be combined and factored to create other loadcases using the COMBINE data. If combined data is
supplied only the combined cases are solved. If combined data is omitted, then all the basic loadcases are
solved.

3.3     Controlling The Run

In the absence of any special Options, an analysis normally proceeds automatically from start to finish and the
user requires no knowledge of the internal organisation of the program. If the run stops before completion,
however, then the user can make use of the Restart facility which is described in Appendix -D.

If it is thought likely that another analysis of the same structure but with different loading data will be required,
the SAVE ADLD command should be specified in the initial run. This will cause the necessary files to be saved.
The new run with new loads requires only new Preliminary Data and new loading data (and the Additional Mass
Data if added mass has been used). In the Preliminary Data, the appropriate COPY ADLD FILES command
must appear.



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


For large jobs such repeat runs are usually very efficient because they avoid the relatively expensive stages of
the analysis in which stiffness matrices are formed and decomposed. However the files saved can be large and
use should be made of the option FL41.

It should be noted that if the restraints on a structure are changed, there is no alternative to a complete re-
analysis.

In natural frequency analysis, a facility is available which allows repeat runs with a changed direct mass matrix,
without the need to repeat all the stages of the analysis. This is especially advantageous if the changed mass is in
FULL MASS form. SAVE ADMS must be used in the initial run to save the necessary files. The new run with
the changed mass matrix requires only the new Preliminary Data and the Additional Mass Data, together with a
STOP command.            In the Preliminary Data, the appropriate COPY ADMS FILE command must appear,
indicating a changed mass matrix.

For substructure analysis, each run, except the first run in a new project requires the project file to be available
on disk. Any run involving the assembly or stress recovery of components will also require the files associated
with the master component in use to be on disk.

3.4     Linear Stress Analysis



3.4.1       Types of Problem

Linear stress analysis is intended for structures and parts of structures which obey the assumptions of static or
quasi-static loading and a linear relationship between load and deformation. The results obtained from the
analysis are displacements, reactions and stresses or forces.




3.4.2       The Idealisation of Linear Stress Analysis Problems

For linear stress analysis, the idealisation process follows the standard form described in Section 3.1.




3.4.3       The Data for Linear Stress Analysis

The data for linear stress analysis is organised into five groups, each of which contains several data blocks. See
Table 3.1 . Section 3.2 describes the functions of each block and Section 5 describes their formats in detail.

Apart from the data blocks shown in Table 3.1 , no other data blocks are relevant. The groups of data must be
entered in order, but within each group the order of data blocks can be varied, although the user is advised to
adopt the order shown here. Figure 3.1 shows the appearance of a typical data file for linear stress analysis.

The Preliminary Data is compulsory and all the data blocks in the structural description must appear except for
the geometric property and Skew System Data which are not always needed. At least one data block from the
boundary conditions must be present, and there will be one or more data blocks in each loadcase.



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


The following examples of Preliminary Data for linear stress analysis are appropriate for typical problems.
Examples of other data blocks are given in Section 5 and Appendix -F shows the data for a complete linear stress
analysis.

(i)      Example of the Preliminary Data for a straightforward linear stress analysis data-checking run:

         JOB NEW LINE
         TITLE A SIMPLE PROBLEM
         OPTIONS DATA
         END

This is suitable for a single analysis. The project name has been omitted because the user is running only one
ASAS problem and there is no chance of confusing the files with those remaining from a previous run.

(ii)     Example of the Preliminary Data for a complete run of a simple linear stress analysis:

         JOB NEW LINE
         TITLE A SIMPLE PROBLEM
         END

This is identical with the first example, except that the Options have been changed to allow a complete run.

(iii)    Example of the Preliminary Data for a more advanced problem:

         SYSTEM DATA AREA 500000
         PROJECT PN02
         JOB OLD LINE
         STRUCTURE AVPR
         TITLE AN ADVANCED PROBLEM
         OPTIONS PRNO NODL COOR ELEM
         RESTART 17 21
         END

The user has specified a project name on the PROJECT command to identify which project database is to be
accessed. JOB OLD indicates that the project database already exists. The structure within this project is
identified by the name AVPR and all files relating to this structure will have the prefix AVPR in the filenames.
This analysis is being restarted at the start of Stage 17 and is being allowed to run to completion, the end of
Stage21.

If the SAVE ADLD FILES command is used during a linear stress run, the relevant files are saved to enable
further analyses to be carried out with new loading data. In these further analyses, the user needs to provide only
the Preliminary Data which includes a COPY ADLD FILES command, Phase 3 data (and Phase 4 data if added
mass has been used) and a STOP command.

(iv)     Example of Preliminary Data blocks for an additional loads analysis

(a) Original Run

         SYSTEM DATA AREA 300000
         PROJECT TEST
         JOB NEW LINE
         STRUCTURE RUN1



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


       TITLE ORIGINAL LOADS RUN
       SAVE ADLD FILES
       END

(b) Additional Loads Run

        SYSTEM DATA AREA 300000
        PROJECT TEST
        JOB OLD LINE
        STRUCTURE RUN2
        TITLE RERUN WITH ADDITIONAL LOADS
        COPY ADLD FILES FROM STRUCTURE RUN1
        END




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



       Data Block Contents                                                                                                      Section

       Preliminary Data
                              Run 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 ............. ................................................................... 5.3.8
                              Freedom Releases ............ ................................................................... 5.3.2

       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
                              Tank Loads ...................... ................................................................. 5.4.13

       Additional Mass
                              Lumped Mass Values ...... ................................................................... 5.5.2

       Load Combinations
                              Combined Loadcase Data ....................................................................... 5.8

       End of File
                              STOP Command .............. ...................................................................... 5.9


                                            Table 3.1 Data for Linear Static Analysis




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



                * PRELIMINARY DATA
                SYSTEM DATA AREA 500000
                PROJECT WING
                JOB NEW LINE
                STRUCTURE STBD
                TITLE STARBOARD WING - VERSION 3
                OPTIONS DATA GOON ASDS
                SAVE LOCO FILES
                END

                          * COORDINATES
                          COOR
                          CART
                          1 0.0 0.0 10.3
                          2 0.0 3.7 10.8
                          3 0.0 5.9 11.2

                                 * ELEMENTS
                                 ELEM
                                 MATP 1
                                 GROUP 1
                                 /
                                 QUM8 1 2 3 17 26 25 24 15 1001
                                 RP 6 2
                                 FLA3 1 2 3 2001

                                          * MATERIAL PROPERTIES
                                          MATE
                                          1 ISO 2.1E5 0.3 1E-5 7.85E-9
                                          END

                                                * GEOMETRIC PROPERTIES
                                                GEOM
                                                1001 QUM8 1.1
                                                1002 QUM8 1.21
                                                2001 FLA3 2.73
                                                       * SUPPRESSIONS
                                                       SUPP
                                                       X Z 1 13 24 36
                                                       ALL 15 27
                                                       END
                                                            * LOADCASES
                                                            LOAD
                                                            CASE 100 UNDERCARRIAGE LOADS
                                                            NODAL LOADS
                                                            Z 1530 216
                                                            Z 1325 221
                                                            Y 169 221
                                                            END
                                                            .
                                                            CASE 200 STALLED PRESSURE DISTRIBUTION

                              Figure 3.1 Typical layout for linear stress data file




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


3.5      Natural Frequency Analysis



3.5.1       Types of Problem

There are two intended uses for natural frequency analysis in ASAS.

(i)      To calculate the natural frequencies and associated mode shapes of dynamically sensitive structures.

(ii)     As a pre-processor for other programs, for example RESPONSE, which calculate dynamic response.


The results of the analysis consist of a specified number of natural frequencies and normal modes, together with
mass and stiffness matrices if requested with the SAVE DYPO FILES command.




3.5.2       The Idealisation of Natural Frequency Problems

The type of idealisation created for a linear stress analysis is not always suitable for natural frequency analysis,
although the general principles of Section 3.1 still apply. In addition to ensuring that the overall stiffness
characteristics are adequately represented, care is also necessary in modelling the inertia (mass) correctly.

(a) Mass matrices

         The inertia properties of a structure or component are described by its global mass matrix. ASAS permits
         three basic forms:

(i)      The program assembles the mass matrix from the mass of each element lumped at its nodes - the Lumped
         mass matrix for the element.

(ii)     The program assembles the mass matrix from the actual distribution of mass within each element - the
         Consistent mass matrix for the element.

(iii)    User specified lumped mass values at appropriate nodes to produce a Direct Input mass matrix.

         The three forms can be mixed if required. For example, a Direct Input mass matrix may be used as the
         only mass in the analysis (FULL MAS command) or it may be used to augment the Lumped or Consistent
         element mass matrices (ADDED MA command).                            The type of element mass matrix (Lumped or
         Consistent) is indicated individually for each element in the Element Topology Data (see Section 5.2.3).
         The mass of selected elements can also be omitted by flagging the appropriate Element Topology Data.
         If no mass type is selected specifically, the type of element mass matrix defaults to that given on the
         element description sheets in Appendix -A.

         There are no easy rules governing the choice of the mass type. In general, the idealisation of inertia
         characteristics can be far coarser than the idealisation of stiffness, but the degree of refinement necessary




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


       for any problem can only be established by experience. Lumped mass is always preferable on grounds of
       computational efficiency, and Consistent mass matrices are seldom justified if condensation to a reduced
       number of master freedoms is used. The analyst should also recognise the profound influence that non-
       structural mass may have on the frequencies.


(b) Condensation

       Finite element idealisations of dynamic problems often have more freedoms than are necessary to
       describe the essential dynamic characteristics. For economy, the number of freedoms can be reduced by
       ‘condensation’, otherwise knows as ‘eigenvalue economisation’ or ‘Guyan reduction’. From a total of n
       freedoms, the user selects a set of m master freedoms that are to be retained; the n-m ‘slave’ freedoms are
       eliminated automatically. Condensation is normally worthwhile if m <n/10. ASAS condenses both the
       mass matrix and the stiffness matrix, except that where the global mass matrix is defined only by Direct
       Input (FULL MAS command), then only the stiffness matrix is condensed.

       Experience shows that condensation has a very small effect on the accuracy of the first few frequencies;
       thereafter, there is a progressive deterioration. However, some judgement is necessary in selecting the
       master freedoms. In general, it is best to remove those freedoms where the inertia effects are small,
       because they do not contribute much to the total kinetic energy. For example, in-plane translational
       freedoms should be condensed out rather than out-of-plane translations, and rotations should be removed
       in preference to translations. Freedoms near to suppressed points usually have little effect and can be
       condensed out. The master freedoms must be capable of describing all potential mechanisms of the
       parent structure, including rigid body modes which have not been removed by suppressions.


(c) Suppressions and constraints

       Suppressions are used to represent supports and to remove rigid body movements. Note, however, that
       ASAS does not require a model for natural frequency analysis to be supported. For such ‘free-free’
       structures, the mode shapes are computed correctly for the number of rigid body movements present, and
       their associated frequencies are presented as zero. Free-free structures should be used with discretion
       however, and it is usually better to remove any potential local mechanisms by applying restraints. Where
       suppressions are used to remove such modelling problem, due account must be taken of the fact that some
       mass will no longer be participating in the solution. A suppressed freedom may not also be listed as a
       master freedom. SPIT should not be used for an analysis in which rigid body movement is possible.
       However if the structure is totally unsupported SPIT may be used and the program will apply a frequency
       shift technique to obtain a solution.

       Prescribed displacements have no significance in natural frequency analysis; a freedom specified as such
       is treated as a suppression.




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


       When running SPIT the supported nodes should have the lowest node numbers to minimise the
       bandwidth. The remainder of the nodes should then be ordered moving away from the supports across
       the structure.

       The BAND options for bandwidth reduction should be used with caution for frequency analysis.

(d) Selection of method for natural frequency analysis


ASAS offers four methods for determining eigenvalues (natural frequencies). They are identified by four-
character names:

        JACO :           Jacobi method.

       HOSS :            Householder reduction to tri-diagonal form followed by a bisection technique using Sturm
                         Sequences to obtain eigenvalues.                Eigenvectors (normal modes) are then obtained by
                         inverse iteration.

       HOQL :            Householder reduction to tri-diagonal form followed by the Q-L iteration method for
                         eigenvalues and eigenvectors.

       SPIT :            Subspace iteration.


No one method is best for all problems, and the user should be aware of the fundamental characteristics of each
method before choosing the one he wants.

The JACO, HOSS, HOQL methods are most efficient when all necessary matrices fit into the main memory.
There is thus a limit to the size of problem which can be treated by these methods and the user must ensure that
the number of master freedoms is less than the limit imposed by the user defined Data Area on the System
command.

The JACO method determines all the natural frequencies and normal modes of the model as defined by the
master freedoms. It is best suited to small problems with small bandwidths, but is not normally suitable for
problems where condensation is required.

The HOQL and HOSS methods are most efficient for problems with large bandwidths or with full matrices, such
as after condensation. If the user requires relatively few (say less than 25%) of the frequencies and the normal
modes, then HOSS should be chosen. If only the frequencies are to be calculated, then HOSS is better up to
approximately 40% of the frequency spectrum; otherwise HOQL is to be preferred.

The SPIT method is most efficient for large problems where only a few frequencies are required. It cannot be
used with condensation and therefore a MASTER’s data block should not be used in a SPIT run.

The mass matrix can be represented in ASAS either as a diagonal matrix or as a banded matrix similar to the
stiffness.

A diagonal matrix is formed when

(i)    All the elements and added mass are represented as lumped mass



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


(ii)     Mass is input as DIRECT mass and is used as FULL MASS


In all other situations the mass matrix is banded. The user should be aware that when the mass matrix is banded
the solution times are much longer and the disk storage requirements are much greater.

In all methods, the eigenvectors (normal modes) can be normalised in three ways:

(i)      The eigenvector is scaled such that the largest component is one

(ii)     The Euclidean norm is set to one - i.e. for an eigenvector x, xT.x = 1.0

(iii)    No normalisation




3.5.3       The Data for Natural Frequency Analysis

The data for natural frequency analysis is organised into three groups, each of which contains several data
blocks. Section 3.2 describes the function of each data block and Section 5 describes their formats in detail.
Much of this data is common to other forms of analysis.




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




             Data Block Contents                                                                                                   Section

             Preliminary Data
                                   Run 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

             Kinematic Boundary Conditions
                                   Suppressions.................... .................................................................... 5.3.3
                                   Constraint Equations ....... .................................................................... 5.3.5
                                   Master Freedoms ............. .................................................................... 5.3.7
                                   Rigid Constraints............. .................................................................... 5.3.8
                                   Freedom Releases ........... .................................................................... 5.3.2

             Additional Mass
                                   Lumped Mass Values ...... .................................................................... 5.5.2
                                   Consistent Mass Values ............................................................... 5.5.35.5.3

             End of File
                                   STOP Command ............. ....................................................................... 5.9



                                    Table 3.2 Data for Natural Frequency Analysis



Apart from the data blocks shown in Table 3.2, no other data blocks are relevant. The Preliminary Data and
rjhxg98sr structural description are compulsory, except for the geometric property and Skew System Data blocks
which are not always needed. The Master Freedom Data must not be used with the SPIT method of eigenvalue
determination. The Boundary Conditions and Additional Mass Data blocks are not always needed. A STOP
command must always appear as the last item in the data.

The user can select Options which allow some of the standard stages to be bypassed. If reflation of the
eigenvectors to uncondensed form is not required, then NORF should be set. The printed eigenvectors do not
then include slave freedoms. The option NOSL prevents the printing of the slave freedom components of each
eigenvector.

The following examples of Preliminary Data for natural frequency analyses are typical. The examples for other
data blocks are given in Section 5




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


(i)      Example of Preliminary Data for a straightforward natural frequency analysis:


       JOB NEW FREQ
       TITLE SIMPLE NATURAL FREQUENCY PROBLEM
       FREQUENCY HOQL
       END

(ii)     Example of Preliminary Data for a more advanced problem:


       SYSTEM DATA AREA 400000
       PROJECT ASAS
       JOB OLD FREQ
       STRUCTURE COLM
       TITLE ADVANCED NATURAL FREQUENCY PROBLEM
       OPTIONS NOBL DYFS
       SAVE DYPO FILES
       RESTART 13 19
       FREQUENCY HOSS 0                0     1    10
       END

If further post-processing is required, excluding the plotting of mode shapes, the SAVE DYPO FILES command
must be used. (The SAVE LOCO FILES command is not a valid option in dynamics and should not be used.)

If the SAVE ADMS FILES command is used during a natural frequency run, the relevant files are saved to
enable further analyses to be carried out with new direct mass input data. In these further analyses, the user
needs to provide only the Preliminary Data, the Additional Mass Data and a STOP command, together with an
appropriate COPY ADMS command.

During a natural frequency run using SPIT, the SAVE ADFQ FILES command can be used to save files for
further analyses if additional frequencies are required. In the reruns, the user needs only to provide the
Preliminary Data which includes a COPY ADFQ FILES command. The direct mass input data block may also
be included but it has to be used with caution (see Notes (iii) and (iv)). Finally, a STOP command must be
provided as well. The following are some restrictions for the SAVE ADFQ and COPY ADFQ runs:

(i)      SAVE ADFQ FILES and COPY ADFQ FILES option are only available with SPIT.

(ii)     An additional 50% eigenvalues can be computed in the COPY ADFQ FILES run, but an upper limit of
         25 extra eigenvalues has been set. However, the user defined subspace size will overwrite the default
         value and thus determine the total number of frequencies that can be evaluated.

(iii)    The reruns use the eigenvectors calculated in the original run as the starting vectors and these may not be
         good estimates if the mass characteristics of the structure has changed significantly.

(iv)     Added mass is not allowed for the rerun of a free-free structure since the computed frequency shift will
         become invalid.

(v)      Sturm sequence check is not available for the rerun.




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


Example of Preliminary Data blocks for an additional frequency analysis

(i)     Original Run


        SYSTEM DATA AREA 300000
        PROJECT TEST
        JOB NEW FREQ
        STRUCTURE RUN1
        TITLE FIRST FREQUENCY RUN
        SAVE ADFQ FILES
        FREQUENCY SPIT                0    0     1     6
        END

(ii)    Additional Frequency Run


        SYSTEM DATA AREA 300000
        PROJECT TEST
        JOB OLD FREQ
        STRUCTURE RUN2
        TITLE RERUN FOR ADDITIONAL FREQUENCIES
        COPY ADFQ FILES FROM STRUCTURE RUN1
        FREQUENCY SPIT                0    0     1     8
        END

3.6     Steady State Heat Conduction Analysis



3.6.1       Types of Problem

Heat conduction analysis is intended for steady state problems of heat diffusion in two and three-dimensional
solids. This form of analysis is limited to problems where the dominant heat transfer mechanism is conduction
within the body. The result from the analysis is the temperature distribution within the body.




3.6.2       The Idealisation of Heat Conduction Problems

The boundary conditions can either be specified in terms of prescribed temperatures or in terms of heat flux
across a surface. Where more complex boundary conditions such as convection or radiation are required, the user
is referred to the associated heat transfer analysis system, ASASHEAT.

In using the heat analysis facility, the user needs to grasp the analogy between the heat conduction equations and
the stiffness equations of structural mechanics.                 This manual is written in the terminology of structural
mechanics and the following analogies should be applied when using heat conduction analysis:

Stiffness matrix              : Thermal stiffness or conductivity matrix




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


Material properties           : Thermal properties (conductivity coefficients)

Modulus of elasticity         : Conductivity coefficient

Freedom                       : Temperature

Reaction                      : Thermal reaction or equivalent heat source/sink

Load                          : Thermal load or heat vector

Similar analogies can be made with other field problems. The facility can be used, for example, for analysing
problems in electric potential and seepage.

Temperature is treated as a special type of freedom in ASAS - the T freedom - and all nodes have this single
freedom, regardless of the type of element. Heat conduction analysis can use all the types of elements which
exhibit thermal straining. However, bending elements such as the beams, plates and shells, are only treated as
line or sheet elements which conduct heat in an axial or membrane sense with a uniform temperature distribution
through the thickness.




3.6.3       The Data for Heat Conduction Analysis

Heat conduction analysis is organised into three groups, each of which contains several data blocks. Section 3.2
describes the function of each data block and Section 5 describes their formats in detail.

Apart from the data blocks listed in Table 3.3, no other data blocks are relevant. The Preliminary Data and the
three groups of data are all necessary but data blocks, geometric properties, displaced freedoms and nodal loads
are not always needed.




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




            Data Block Contents                                                                                                   Section

            Preliminary Data
                                  Run Parameters ............... ....................................................................... 5.1

            Structural Description - Shape and Properties of the Model
                                  Coordinates ..................... .................................................................... 5.2.2
                                  Element Topology ........... .................................................................... 5.2.3
                                  Thermal Properties (Material Properties) ............................................. 5.2.4
                                  Geometric Properties....... .................................................................... 5.2.5
                                  Section Information......... .................................................................... 5.2.6

            Boundary Conditions
                                  Prescribed Temperature Freedoms (Displaced Freedoms) ................... 5.3.4
                                  Constraint Equations ....... .................................................................... 5.3.5

            Thermal Loading
                                  Thermal Loads (Nodal Loads) ............................................................. 5.4.3
                                  Prescribed Temperatures (Prescribed Displacements) ......................... 5.4.4

            End of File
                                  STOP Command ............. ....................................................................... 5.9




                                     Table 3.3 Data for Heat Conduction Analysis




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


The following examples of Preliminary Data for heat conduction analysis are typical.

(i)      Example of Preliminary Data for a simple heat conduction analysis data-checking run:


       JOB NEW HEAT
       TITLE DATA CHECK FOR THERMAL ANALYSIS
       OPTIONS DATA
       END

The PROJECT command has been omitted because the user is running only one ASAS problem and there is no
chance of confusing the files.

(ii)     Example of Preliminary Data for restarting a heat conduction analysis:


       PROJECT THRZ
       JOB HEAT
       TITLE RESTART OF A THERMAL ANALYSIS
       RESTART 10 17
       END

This data block will allow the problem to restart at the beginning of Stage 10 and finish at the end of Stage 17 -
the end of the analysis. The project name THRZ is needed to identify which project database is to be accessed.
The structure name has been omitted therefore the structure name also defaults to THRZ.

3.7      Substructured Linear Stress or Natural Frequency Analysis



3.7.1        Types of Problem

Substructured analysis may be applied to structures which may be assumed to have static loading and obey a
linear relationship between load and displacement.

The main feature of a substructured analysis is that the structure is sub-divided into several parts each of which
may be partially analysed separately. These master components, as they are called, are later assembled together
to form either higher level, more complex, components or the global structure.

Subsequent processing after the global structure has been formed enables displacements, reactions and stresses to
be recovered for each separate component as and when required. An exception to this is when a component has
been created from a set of stiffness input data. In this case stress recovery of the component will only give
displacements for the link nodes, all reactions will be zero and no stresses will be given.




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


3.7.2       The Idealisation of a Substructured Problem

The basic principles outlined in Section 3.4 apply to the structure whether it is analysed in a single run or
substructured and the behaviour of the total structure will be unaffected providing identical idealisation has been
used throughout.

(a)     Component boundaries

        The definition of link nodes and freedoms describes the points at which one component may be attached
        to another. The geometry of the boundaries of two components which are to be joined must be identical.
        The node numbering on a master component is independent of the node numbering on any other master
        component to which it may subsequently be attached. Translation, rotation or mirroring can be used to
        align components during assembly.

        The formation of the reduced component stiffness during a master component creation run is more
        efficient if the link nodes on the boundary are assigned the highest node numbers, and nodes furthest
        away from the boundaries are assigned the lowest node numbers.


(b)     Link Freedoms

        Only the nodes and freedom directions required to describe the structure action across a boundary
        between two components need be defined as link freedoms. All other freedoms will move independently
        even if they are physically located on the boundary. For example, a component consisting of flat area of
        membrane elements in the xy-plane may only require X and Y link freedoms.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 3-25
      ASAS (Linear) User Manual                                                                        The ASAS Analysis



(c)    Loading (Linear stress analysis only)

       Loading may be applied to the internal nodes and freedoms of a component at the master component
       creation stage. Loading on the link freedoms may be provided at the master component creation stage or
       at the higher level assembly stage when that component is being used, but not both.

       Loadcases applied to a component at the creation stage can be referenced at a higher level in the
       Component Load Data. It is possible to select, factor or combine the component cases to form the new
       cases.

       If a component is being assembled several times the load data applicable to each occurrence must have
       been included in the component creation analysis and selected, as appropriate, in the higher level
       Component Load Data.


(d)     Mass Input

        Mass input may be applied to any nodes and/or elements of a component at the master component
        creation stage. Note that if FULL MAS is used it must be applied to all link freedoms. Note, however,
        that ADDED MASS at the next higher level will achieve the same effect.


(e)     Calculation of Eigenvalues

        If the substructure analysis is to be used to calculate Eigenvalues (frequencies), only those degrees of
        freedom which exist in the global structure assembly run will be used in the eigenvalue calculations.
        Both stiffness and mass will have been condensed down during the substructure creation stages to the link
        freedoms in a similar manner to the Guyan reduction used when MASTER freedoms are defined.
        Therefore the user may wish to retain some freedoms, other than those at the boundary, as link freedoms
        in order that the distribution of the freedoms in the global structure run better suited for the eigenvalue
       analysis.



       3.7.2.1 The Data for a Master Component Creation Analysis using COMP or COMD

This data is similar to that required for a linear stress analysis but with the following possible additions.

The Preliminary Data will require the addition of a COMPONENT command to define the name of the master
component being created (see Sections 2.10.1 and 5.1.5).

For master components formed from other lower level components, it is necessary to include component
topology data in the Structural Description Data (see Section 5.2.9). A LINK freedom data block is required in
the Boundary Description Data (see Section 5.3.6). For master components formed from other lower level
components, it may be necessary to include Component Load Data (see Section 5.4.12).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 3-26
     ASAS (Linear) User Manual                                                                         The ASAS Analysis


Apart from the data blocks listed in Table 3.4, no other data blocks are relevant. Preliminary Data must appear.
In the Structural Description Data, either element topology or component topology must appear. All other
Structural Description Data are optional.

In the Boundary Description Data, Link Freedom Data must appear but all other data are optional. Loading Data
may only be used for linear stress analysis and all data here are optional. If Element Topology Data is absent,
only nodal load, Prescribed Displacement and Component Load Data are permitted. The consistent added mass
may only be used for natural frequency analysis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 3-27
     ASAS (Linear) User Manual                                                                                                The ASAS Analysis



         Data Block Contents                                                                                                   Section
         Preliminary Data
                                 Run 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 Systems .................. ................................................................... 5.2.7
                           Component Topology ...... ................................................................... 5.2.9

         Boundary Conditions - Restraints on the Model
                         Suppressions ................... ................................................................... 5.3.3
                         Displaced Freedoms ........ ................................................................... 5.3.4
                         Constraint Equations ....... ................................................................... 5.3.5
                         Link Freedoms ................. ................................................................... 5.3.6
                         Rigid Constraints ............. ................................................................... 5.3.8
                         Freedom Releases ............ ................................................................... 5.3.2

         Loading Applied to the Model (Linear stress analysis only)
                         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
                         Component Loads ........... ................................................................. 5.4.12
                         Tank Loads ...................... ................................................................. 5.4.13

         Additional Mass
                                 Lumped Mass Values ..... ................................................................... 5.5.2
                                 Consistent Mass Values ...................................................................... 5.5.3
                                 (Natural frequency analysis only)

         Load Combinations
                        Combined Loadcase Data ....................................................................... 5.8

         End of File
                                 STOP Command ............. ...................................................................... 5.9


            Table 3.4 Data for a Master Component Creation Analysis using COMP or COMD




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                        Page 3-28
     ASAS (Linear) User Manual                                                                                                          The ASAS Analysis


       3.7.2.2 The Data for a Master Component Creation Analysis using JOB type STIF

The Preliminary Data will be similar to that required for a linear stress analysis except that the JOB type is STIF.
A COMPONENT command will be required to define the name of this master component (see Sections 2.10.1
and 5.1.5). Also the use of the BAND option or PASS or START commands will be ignored.

Apart from the data blocks in Table 3.5, no other data blocks are relevant. Preliminary Data must appear. In the
Structural Description Data, the Coordinate Data must appear and must contain data for all the link nodes. In the
Boundary Condition Data, the link freedoms data must appear and if it includes special freedoms (see Section
2.7.1), the special freedom directions data must also appear. In the Loading Data, the nodal load data is optional.
In the Stiffness Data, the stiffness matrix data must appear and for a dynamic analysis, the mass matrix data must
also appear.

Note, by adding a Preliminary Data block to the start of the formatted output file created with the SAVE COMP
FILES command, an input data file for stiffness input component creation run is formed.




         Data Block Contents                                                                                                           Section

         Preliminary Data
         Run Parameters ......................................... ...................................................................... 5.1

         Structural Description
         Coordinates              ......................................... ................................................................... 5.2.2

         Boundary Conditions
         Link Freedoms            ......................................... ................................................................... 5.3.6
         Special Freedom Directions ......................... ................................................................... 5.3.9

         Loading Applied to the Component (Linear stress analysis only)
         Nodal loads              ......................................... ................................................................... 5.4.3

         Stiffness and Mass Data (Mass data for dynamic analysis only)
         Stiffness Matrix ......................................... ................................................................... 5.7.1
         Mass Matrix              ......................................... ................................................................... 5.7.2

         End of File
         STOP Command ......................................... ...................................................................... 5.9




               Table 3.5 Data for a Master Component Creation Analysis using JOB type STIF




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                                   Page 3-29
     ASAS (Linear) User Manual                                                                         The ASAS Analysis


3.7.3       The Data for a Global Structure Analysis (linear stress or natural frequency)

This data is similar to a linear stress analysis but with the following additions. The Preliminary Data will require
a STRUCTURE command to define the name of the global structure being formed (see Sections 2.10.1 and
5.1.4). A Component Topology Data block is required in the Structural Description Data (see Section 5.2.9). A
Component Load Data block may be required in the Loading Data (see Section 5.4.12).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 3-30
     ASAS (Linear) User Manual                                                                                                   The ASAS Analysis




           Data Block Contents                                                                                                      Section

           Preliminary Data
           Run 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 Systems ......................................... ....................................................................5.2.7
           Component Topology .................................. ....................................................................5.2.9
           Boundary Conditions - Restraints on the Model
           Suppression       ......................................... ....................................................................5.3.3
           Displaced Freedoms .................................... ....................................................................5.3.4
           Constraint Equations ................................... ....................................................................5.3.5
           Master Freedoms (dynamics only) .............. ....................................................................5.3.7
           Rigid Constraints ......................................... ....................................................................5.3.8
           Freedom Releases ........................................ ....................................................................5.3.2
           Loading applied to the Model (static stress analysis only)
           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 Temperature ........................................ ....................................................................5.4.8
           Body Forces      ......................................... ....................................................................5.4.9
           Centrifugal Loads ........................................ ..................................................................5.4.10
           Angular Accelerations ................................. ..................................................................5.4.11
           Component Loads........................................ ..................................................................5.4.12
           Tank Loads       ......................................... .................................................................. 5.4.13
           Additional Mass
           Lumped Mass Values .................................. ....................................................................5.5.2
           Consistent Mass Values (dynamics only) .... ....................................................................5.5.3
           Load Combinations
           Combined Loadcase Data ............................ .......................................................................5.8
           End of File
           STOP Command ......................................... .......................................................................5.9




                                        Table 3.6 Data for a Global Structure Analysis




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                         Page 3-31
      ASAS (Linear) User Manual                                                                                                 The ASAS Analysis


Apart from the data blocks shown in Table 3.6, no other data blocks are relevant. Preliminary Data must appear.
In the Structural Description Data, a Component Topology Data block must appear. All other data blocks are
optional but if element topology is present then Material Property Data must appear.

In the Boundary Condition Data, all data are optional. Loading data must only appear in a linear stress analysis.
At least one load data block must appear for each loadcase but data blocks 3.3 to 3.9 can only appear if element
topology is present in the Structural Description Data.




3.7.4       The Data for a Component Recovery Analysis

The Preliminary Data is the same as that required for a global structure analysis, in that a STRUCTURE
command is necessary to define the name of the structure containing the components to be recovered.

After the Preliminary Data, COMPONENT commands are required to define which components are to be
recovered and the type of output required for each. Loadcases may be selected for specific components by using
SELECT LOADS commands (see Section 5.6).

No other data blocks are relevant.


         Data Block Contents                                                                                                     Section

         Preliminary Data
         Run Parameters ......................................... ...................................................................... 5.1

         Component Recovery Selection Data
         COMPONENT Commands ............................................................................................. 5.6.1
         SELECT LOADS Commands ......................................................................................... 5.6.2

         End of File
         STOP Commands ........................................ ...................................................................... 5.9




                                     Table 3.7 Data for Component Recovery Analysis


3.8     Gap Analysis



3.8.1       Types of problem

Gap analysis is intended for use with structures where the basic behaviour of the structure makes it suitable for
linear stress analysis, but in which there are parts of the structure which, under the influence of the loading, may
or may not come into contact with each other. The presence of an unknown contact area necessitates the use of
an iterative solution technique. The parts of the structure which may or may not come into contact with each



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                          Page 3-32
     ASAS (Linear) User Manual                                                                         The ASAS Analysis


other are represented by GAP Data, each GAP defined in terms of a pair of nodes, a gap direction and an initial
gap. The two nodes in the pair will be assumed to move independently of each other until the relative movement
of node1 towards node2 in the defined direction is greater than the initial gap. The nodes will then be
constrained to move together in this direction (while remaining independent of each other in directions at right
angles) until such time as the force holding them together becomes a tensile force. The nodes are then released
and allowed to move independently.




3.8.2       The idealisation of Gap problems

For a Gap analysis, the idealisation process follows the standard form described in Section 3.1.




3.8.3       The data for a Gap analysis

A Gap analysis is most efficiently organised as a substructured analysis. All nodes not involved in the gapping
process are consigned to master components and those nodes needed for the Gap analysis are retained as link
nodes. The Gap analysis then replaces the global assembly run (see Section 3.7.3).

The data for a Gap analysis is organised into five groups, each of which contains several data blocks. Section
3.2 describes the functions of each data block and Section 5 describes their formats in detail.

Apart from the data blocks shown in Table 3.8, no other data blocks are relevant.

Preliminary Data is compulsory. All the data blocks in the structural description must appear except for the
Geometric Property and Skew System Data blocks which are not always needed. At least one data block from
the boundary conditions must be present and there will be one or more data blocks in each loadcase in the
loading data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 3-33
     ASAS (Linear) User Manual                                                                                                   The ASAS Analysis



         Data Block Contents                                                                                                      Section
         Preliminary Data
                                Run 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 Systems .................. ................................................................... 5.2.7
                                Component Topology ...... ................................................................... 5.2.9

         Boundary Conditions - Restraints on the Model
                                Suppressions .................... ................................................................... 5.3.3
                                Displaced Freedoms ........ ................................................................... 5.3.4
                                Constraint Equations ....... ................................................................... 5.3.5
                                Rigid Constraints ............. ................................................................... 5.3.8
                                Freedom Releases ............ ................................................................... 5.3.2
                                Gaps................................. ................................................................. 5.3.10

         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
                                Component Loads............ ................................................................. 5.4.12
                                Tank Loads ...................... ................................................................. 5.4.13

         Additional Mass
                                Lumped Mass Values ...... ................................................................... 5.5.2

         Load Combinations
                                Combined Loadcase Data ....................................................................... 5.8

         End of File
                                STOP Command.............. ...................................................................... 5.9



                                               Table 3.8 Data for a Gap Analysis



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                            Page 3-34
      ASAS (Linear) User Manual                                                                                    The ASAS Analysis


3.9    Solution Methods and Bandwidth

ASAS incorporates two solution techniques, the partitioned (out-of-core) hypermatrix solution and the frontal
(in-core) solution. For linear static and global structure runs and natural frequency analyses using the Subspace
Iteration technique (SPIT), an optimised frontal solution is also available that can greatly reduce the solution
time and storage requirements in medium to large problems. For dynamic (natural frequency) analyses not using
SPIT the partitioned solution is always used. Constraint equations also default the program to the partitioned
solution unless the optimised frontal solution is in use. For linear statics or substructure creation runs the frontal
and partitioned solution methods techniques are alternatives. ASAS will use the frontal solver if there is
adequate memory space as defined by the DATA AREA or system limits, but will otherwise use the partitioned
solver (note: the switch to partitioned solver is not automatic with the optimised frontal solver). Options ISOL
and OSOL can be used in some situations to direct the program to use the frontal (ISOL) or partitioned (OSOL)
solution method.

The partitioned bandwidth is given by the maximum element freedom difference in the job and as such is purely
a function of the element node numbering. The frontal bandwidth (more strictly the ‘frontwidth’), is a function
of the number of degrees of freedom needed to be held in memory at any stage during the frontal elimination.
ASAS generally allocates system element numbers on the basis of least node number order. Elements are then
assembled into the front in this order.

It is possible to request ASAS to assemble elements in a specific order for the frontal solution only, by assigning
user element numbers on the Element Topology Data and setting the MYEL option or by using the input element
order by setting the INEL option. Using this technique it is sometimes possible to reduce the frontwidth (and
hence cost of an analysis) significantly.

As an illustration of this consider the simple linear structure in the figure below, which is not a representative
way of numbering structures.

        Node                                1        7        5        3        9        4        8         6       2


        System element no.                       1       7        3        4        5        6          8       2

        User element no.                        1        2        3        4        5        6          7       8




Partitioned bandwidth (nodes) = (max. node difference on an element) = (7-1) = 6 nodes

Frontwidth, based on least node number order from the system element numbers = 5 nodes

Frontwidth, based on user element numbers = 2 nodes

Other methods of reducing the bandwidth of the stiffness equations are available using the BAND option and the
PASS and START commands in the Preliminary Data. See Sections 5.1.10, 5.1.11 and Appendix -C.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 3-35
      ASAS (Linear) User Manual                                                                         Input Data Syntax


4. Input Data Syntax

4.1     General Principles

The input data for ASAS 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 command 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 alphanumeric strings (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.

A single line of data must not be longer than 80 characters.

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

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

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




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


Exponent 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)


                       keyw ord                           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.

                       real                               integer




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


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 will give details of any default value to be 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 4.2).

                     KEYWORD                           integer




4.2     Special Symbols

The following is a list of characters which have a special significance to the ASAS 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 4-3
     ASAS (Linear) User Manual                                                                         Input Data Syntax


,      A comma or one or more consecutive blanks 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                     is the same as             5     0       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 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 five secondary files are open simultaneously.

        For example

                @prelim.dat
                @phase1.dat
                @phase2.dat
                @load.dat

        phase1.dat might then contain the lines




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


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

            finally

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


4.3        Data Generation Facilities



4.3.1           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




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

KEYWORD                : items notenclosed within slashes will be repeatedwithout any increment for generated
                            real           data

/integer/              : an item enclosed by / characters indicates data which can be modified using the repeat facility.
                            The / characters 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 certain data items for the second and subsequent generated blocks.
                            (The first block corresponds to the original data)




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


For example, suppose the data format is specified as

                   KEYWORD                                     /integer/




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

              ALL       1          6          11         16        21         26         31        36   41     46




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


     or

               ALL        1
               ALL        6
               ALL        11
               .
               .
               .
               ALL        46

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

     (i)       /
               ALL        1
               RP         10        5


     (ii)      /
               ALL        1         6
               RP         5         10


     (iii)     /
               ALL        1
               ALL        6
               RP         5         10




4.3.2        Re-Repeat Facilities

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

                     //

                     /

                     KEYWORD                             real                       //integer//

                     RP                                  nrep                        incr1


                     RRP                                 nrrep                       incr2




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




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


/                     : identifies the start of the data to be repeated

KEYWORD               : items not enclosed within 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 // characters 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)




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


For example, taking the previous example in Section 4.3.1, if the data syntax was specified as

                  KEYWORD                                     //integer//




then the data could be

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

Note that the order of the numbers generated by this example in Section 4.3.1 using RP and in Section 4.3.2
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 or the order of LINK nodes for assembly at a
higher level.




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



5.       Data Formats

ASAS 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

                        Component Recovery Data ..... ................ ................ Section 5.6

                        Stiffness and Mass Matrix Input Data ....... ................ Section 5.7

                        Combined Loadcase Data ......... ................ ................ Section 5.8

                        STOP Data .............. ................ ................ ................ Section 5.9



     5.1    The Preliminary Data

     The preliminary data is the first block of the ASAS 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




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

The preliminary data must contain a JOB command and terminate with END. A UNITS command is
highly recommended because postprocessors often need to know the units being used. Within these
bounds the other commands may be in any order, however the user is recommended to follow the order
given below.

Different commands are required for the various analysis types and these are indicated in Table 5.1.

The following commands are available within the Preliminary data:

               SYSTEM                     -            memory requirement
               PROJECT                    -            name of project
               JOB                        -            type of analysis
               STRUCTURE                  -            name of structure
               COMPONENT                  -            name of component
               FILES                      -            name of backing files written in current run
               TITLE                      -            title for current run
               TEXT                       -            descriptive text
               OPTIONS                    -            control options
               PASS                       -            requests node number resequencing
               START                      -            node list for start of node number resequencing
               RESTART                    -            select restart stages
               GOTP                       -            origin for load resultants
               EQMA                       -            output mass values equivalent to the loading
               PARA                       -            defines problem parameters
               FREQUENCY                  -            natural frequency parameters
               SAVE                       -            select files to be saved
               COPY                       -            copy files from run to run
               RESU                       -            save results of run
               WARN                       -            suppress excessive numbers of warning messages
               UNITS                      -            defines the units to be used in the analysis
               LIBRARY                    -            external file name containing section library information
               INFO                       -            to read and print site dependent information
               USER                       -            user-defined list of restart stages
               MONITOR                    -            monitor file transfers and other system operations
               DEBUG                      -            optional subroutine monitoring
               END                        -            terminate preliminary data

These commands are described in Sections 5.1.1 to 5.1.24 except for USER, MONITOR and DEBUG
which are described in Appendix -G.




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 5-2
   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.




                                                                                                                                                                                                                                         ASAS (Linear) User Manual
                                                                                                                                                                                  INPUT LINES
                                                                                                                 ANALYSIS                                                                                                 JOB TYPE




                                                                                                                                                                   COMPONENT




                                                                                                                                                                   FREQUENCY
                                                                                                                                                                                                                          IDENTIFIERS




                                                                                                                                                                   STRUCTURE




                                                                                                                                                                   MONITOR*
                                                                                                                                                                   RESTART
                                                                                                                                                                   OPTIONS
                                                                                                                                                                   PROJECT




                                                                                                                                                                   LIBRARY
                                                                                                                                                                   SYSTEM




                                                                                                                                                                   DEBUG*
                                                                                                                                                                   START




                                                                                                                                                                   USER*
                                                                                                                                                                   EQMA
                                                                                                                                                                   TITLE




                                                                                                                                                                   UNITS
                                                                                                                                                                   WARN
                                                                                                                                                                   FILES




                                                                                                                                                                   GOTP
                                                                                                                                                                   TEXT




                                                                                                                                                                   SAVE
                                                                                                                                                                   PARA


                                                                                                                                                                   COPY
                                                                                                                                                                   PASS




                                                                                                                                                                   RESU



                                                                                                                                                                   INFO




                                                                                                                                                                                                                    END
                                                                                                                                                                   JOB
                                                                                                             Non-substructured:
                                                                                                                   linear static stress:
                                                                                                                           initial run                               C RX     R                  X           R       C
                                                                                                                                                                     C C X    R                  X   C                       LINE
                                                                                                                           further loads rerun                                                               R       C
                                                                                                                                                                                                                             LINE

                                                                                                             linear natural frequency:
                                                                                                                     initial run                                     C RX     R              X   C           R       C
                                                                                                                                                                     C C X    R              X   C   C                       FREQ
                                                                                                                     further masses rerun                                                                    R       C
                                                                                                                                                                                                                             FREQ

                                                                                                             steady-state heat conduction                            C RX     R              X       X               C        HEAT

                                                                                                             Substructured:
                                                                                                                    linear static stress:
                                                                                                                            master component creation                C XC   R                    X       X   R       C       COMP
                                                                                                                            global structure                         C C X  R                    X           R       C
                                                                                                                                                                     C C XR R        X XX    X   X                           LINE
                                                                                                                            component recovery                                                               R       C
                                                                                                                                                                                                                             RECO

                                                                                                                    linear natural frequency:
                                                                                                                            master component creation                C XC     R              X   X       XX R        C
                                                                                                                                                                     C C X    R              X   C          R        C       COMD
                                                                                                                            global structure                                                                                 FREQ

                                                                                                                    stiffness input master                           C XC     R      X X X   X   X X XX XR           C        STIF
                                                                                                                            component creation

                                                                                                           KEY      X - invalid                  R - recommended         C   - compulsory        blank - optional
                                                                                                                   * - commands documented in Appendix -G




                                                                                                                                                                                                                                        Data Formats
                                                                                                                                                  Table 5.1 Preliminary Data Requirements for Each Problem Type
Page 5-3
      ASAS (Linear) User Manual                                                                         Preliminary Data




5.1.1        SYSTEM Command

To define the amount of memory used for data by this run. Optional.

          SYSTEM                    DATA AREA                        memory




Parameters

SYSTEM             : keyword

DATA AREA             :        keyword

memory             : amount of memory (in integer words) to be used by this run. Typical values are between
                      30000 and 1000000. If omitted a default value 1000000 is used. See Section 6 (Integer)

Example


        SYSTEM            DATA     AREA       300000




5.1.2        PROJECT Command

To define the project name for the current run. Optional.

                          PROJECT                          pname




Parameters

PROJECT            : keyword

pname              : project name for current run. (Alphanumeric, 4 characters, first character must be alphabetic)

Notes


i.      All runs with the same project name access the same data base. 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.

ii.     If the PROJECT command is omitted or pname is omitted then pname defaults to the name ASAS.




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


Example


        PROJECT HIJK




5.1.3       JOB Command

To define the type of analysis being performed and whether to create a new project data base or to update an
existing one. Compulsory.

             JOB                 (status)                  jobtype




Parameters

JOB               : keyword

status            : NEW         - defines that this run will create a new project data base
                     OLD - this run will add to an existing project data base.
                     REPL - this run will replace a previous run of the same structure/component on the
                                           project database
                     Optional, if omitted it defaults to OLD

jobtype           : define the type of analysis to be performed in this run. See Table 5.1.
                     LINE       - linear static stress analysis
                     FREQ - natural frequency analysis
                     COMP - static component creation analysis
                     COMD - dynamic component creation analysis
                     RECO - component recovery analysis
                     HEAT - heat conduction analysis
                     GAPS - gap analysis
                     STIF - component creation analysis by direct stiffness input

Notes


1.      JOB REPL cannot be used to replace a lower level component in a sub-structured analysis.

Examples

(i)     To define a natural frequency analysis and a new project data base.


        PROJECT         FRED
        JOB      NEW      FREQ




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


(ii)     To add a static stress analysis to the existing project FRED, and to define that the structure name for this
         run will be BILL. Status has been allowed to default to OLD.


         PROJECT FRED
         JOB LINE
         STRUCTURE BILL




5.1.4       STRUCTURE Command

To define the structure name for the curent run. Recommended. See Table 5.1

                STRUCTURE                            sname




Parameters

STRUCTURE :                   keyword

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

(i)      This command must not be used for a component creation run.

(ii)     If the FILES command is omitted, sname is also used as the file name prefix fname.

(iii)    If both the STRUCTURE and the FILES commands are omitted then the project name pname is used
         in place of sname and fname

Example


         STRUCTURE SHIP




5.1.5       COMPONENT Command

To define the component name for a component creation run. Compulsory for component creation runs.

                COMPONENT                            cname



Parameters




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



COMPONENT               : keyword

cname              : component name for the master component being created by this run. The name must be
                         unique from all other structure and master component names in this project.
                         (Alphanumeric, 4 characters, the first character must be alphabetic)

Notes


(i)      The name must not be an element name (eg BR20, BEAM) or the words DCOS, MIRR or ORIG

(ii)     If the FILES command is omitted , caname is also used as the file name prefix fname.

Example


         COMPONENT          LEFT




5.1.6       FILES Command

To define the prefix name to be used for the backing files created in this run. Optional.

              FILES                     fname




Parameters

FILES             : keyword

fname             : prefix name for any backing files created by the current run. (Alphanumeric, 4 characters, first
                     character must be alphabetic)

Notes


(i)      fname is used as a prefix for all files created during the current run. The four characters are appended
         with two digits in the range 12 to 35 to create each individual file.

(ii)     If the FILES command is omitted, the structure name sname or component name cname is used in
         place of fname.

(iii)    If both the STRUCTURE and the FILES commands are omitted then the project name pname is used
         in place of fname.

Example


         FILES       BILL




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


5.1.7       TITLE Command

To define a title for this run. Recommended.

              TITLE                   title




Parameters

TITLE         : keyword

title         : this line of text will be printed out at the top of each page of ASAS output. (Alphanumeric, up to
                74 characters)

Examples


         TITLE       THIS IS AN EXAMPLE OF A TITLE LINE




5.1.8       TEXT Command

To define a line of text to be printed once near 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          : keyword

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.




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


5.1.9       OPTIONS Command

To define the control options for this run. Optional.

                OPTIONS                              option




Parameters

OPTIONS           : keyword

option            : 4 character option name, or list of option names. See Appendix -C for details of the options
                    available.

Examples


        OPTIONS         DATA        GOON       NODL




5.1.10      PASS Command

To define the parameters for node number reordering in order to reduce computation time. Optional.

                                                            (IN)
           PASS           (method)                                                  ( npass )
                                                           (OUT)




Parameters

PASS              : keyword

method            : optional word KING, LEVY, PINA or SLOAN to indicate method of optimising. These 4
                     methods will automatically set type to IN. If blank, CUTHILL-MCKEE is assumed. However
                     when the optimised frontal solver is adopted, the default method is SLOAN.

IN/OUT            : optional word IN or OUT to indicate type of optimisation required. This is only required if
                     CUTHILL-MCKEE method is selected and if blank, OUT is assumed.

npass             : number of attempts to reduce the bandwidth. For most structures little is gained after the first
                     7-15 passes. If omitted, defaults to 2 for SLOAN and 10 for other methods. Only 1 pass is
                     allowed in a component creation run.




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


Notes


1.      The parameter IN or OUT refers to the type of equation solution method being used. IN indicates an
        incore or frontal solution method and OUT indicates an out-of-core or partitioned solution.

2.      The value of npass must not be greater than the actual number of nodes referenced on the element and
        component data, ie the number of nodes on the structure.

3.      For a component creation run, renumbering is carried out such that the boundary or link nodes are the
        highest node numbers on the structure.

4.      Dynamic analyses, including COMD component runs, always solve using out-of-core methods and
        therefore the IN parameter should not be specified.

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

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

Example


        PASS         10
        PASS         KING IN 3
        PASS         IN




5.1.11      START Command

To define lists of node numbers as starting vectors for any renumbering attempted using the PASS command.
This command is optional and is only applicable if a PASS command is present. If absent the renumbering will
commence from a point chosen by the program. The START command is not valid for component creation
(COMP or COMD) analyses.

                START               nodelist




Parameters

START         : keyword

nodelist      : list of nodes as starting vector

Note


1.      Up to 3 START commands may be used to define 3 start vectors. Each start vector can have up to 10
        nodes defined.




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



2.       START will have no effect on the Sloan method and, thus, is not required when adopting this method.

Examples

(i)      A single start vector consisting of 3 nodes


         START 15 29 36

(ii)     3 start vectors with 5, 5 and 7 nodes respectively


         START       15     29      36     39      42
         START       1064 1072 1073                     1075 1096
         START       15 65 110 207                      501 701 1064




5.1.12      RESTART Command

To define the restart stages to be executed for this run. Optional.



             RESTART                          first                 (last)




Parameters

RESTART           : keyword

first             : number of the first restart stage to be computed by this run.

last              : number of the last restart stage to be computed by this run.
                     Optional, if omitted defaults to last valid stage for this run.

Notes


1.       Appendix -D contains a list of valid restart stages for each type of analysis.

2.       All valid restart stages from first to last inclusive for the current analysis will be executed. Only valid
         restart stage numbers must be defined for first and last.

3.       first must be the next valid stage after the previous completed restart stage for the current analysis.

4.       If a restart stage is not completed when a run stops, that restart stage number should be used as first on a
         subsequent restart run.

Example




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



An example to request that the current statics run should execute all valid stages between element stiffness
calculation (Stage 3) and stiffness decomposition (Stage 10)

        RESTART           3       10




5.1.13      GOTP Command

Defines the point about which the resultant moments of the applied loads are calculated.
(The Global OverTurning Point). Optional.

           GOTP                   xcoord                   ycoord                      zcoord




Parameters

GOTP          : keyword

xcoord        : the coordinates of the point about which the resultant moments of the applied loads are
                ycoord                     calculated. (Real)
                zcoord

Note


If the GOTP command is omitted then the global origin (0,0,0) is used to calculate the moment resultants.

Example


        GOTP         27.6         0.0        15.9




5.1.14      EQMA Command

To compute and output equivalent nodal mass for each element from the applied loading.

                                       (RES)
           EQMA                                                 (grav ity)
                                        VEC




Parameters




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



EQMA              : keyword

RES/VEC           : optional word RES or VEC to indicate method being used for computing the equivalent nodal
                     masses, see note 2 If blank, RES is assumed.

gravity           : optional value of gravitational acceleration for mass computation (Real) (see note 3)

Notes


1.      Only translational terms are considered for nodal mass generation.

2.      In translating the applied loading into masses, it is assumed that F = mg, where F is the resultant force
        acting on an element, m is the total element mass and g is gravity. Option RES uses the load resultant to
        generate a single translational mass at a node, preserving the magnitude of the element resultant load
        vector. Option VEC generates a mass vector at a node, preserving the relative magnitude of the element
        resultant load component.

3.      The gravity term should normally be specified and this may only be omitted if units are supplied. If
        omitted, a default gravity of 9.81 m/s2 is assumed and this will be automatically converted to the
        corresponding value in the analysis units adopted. If gravity is specified, it must be supplied in units
        consistent to the analysis units as no conversion will be made in this case.

4.      The equivalent nodal masses for each element are reported as lump added mass data in ASAS input
        format. A FILEEM file (FILE is the name on the FILES command) is created which uses the @ facility
        to reference the mass data corresponding to each loadcase. The names of these mass data files are
        FILEnnnn.MAS, where the range of nnnn is from 0001 to the number of loadcases (e.g. 0008 for 8
        loadcases).

5.      The equivalent nodal masses calculated will not be the same as those obtained from nodal mass lumping
        procedure if normal pressure or body type loadings are being applied to higher order membrane, plate,
        shell or brick elements. In spite of this, the total element mass is always preserved.

6.      Distributed loading on engineering beams can produce moments as well as forces. Because rotational
        terms are being ignored, the equivalent nodal masses calculated in this situation may be deficient in some
        respect.

7.      Prescribed displacement alone will not produce any equivalent load and therefore the nodal mass is
        always zero.

8.      The nodal masses resulting from thermal effect may be meaningless as this is not a mechanical load type.

9.      Body force, centrifugal load and angular acceleration are forces arising from inertia of the structural
        elements and thus the nodal masses obtained from these loadings will reflect the structural mass content.
        Care should be taken therefore not to duplicate the structural masses in the subsequent dynamic analysis.

Example




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



       EQMA RES           9.81
       EQMA VEC             (a UNITS command must be supplied in this case)




5.1.15      PARA Command

To enable the values of certain problem parameters to be set.


         PARA                   ident            pv al




Parameters

PARA          : keyword
                ident             alphanumeric identifier. See table below. (Real)
                pval              value of parameter ident (Real). See table below


       Identifier                 Description


        GACCEL                gravitational acceleration for equivalent mass
                              computation. See also the EQMA command. (default 9.81m/s2
                              applied only if units are supplied)
       DRILF                  Fictitious stiffness multiplier for shell element drilling
                              freedoms (default 1.0E-08)




5.1.16      FREQUENCY Command

To define the solution method and other parameters required for a natural frequency analysis. See Section
3.5.20. Compulsory for natural frequency analyses.
                           HOQL

                                   HOSS
    FREQUENCY                                          norm         modes           (lmode)             (hmode)
                                   JAC0

                                   SPIT



                                                               (subspace)                 (cutoff)           (shift)




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



Parameters

FREQUENCY              : keyword

HOQL                   : keyword for Householder QL solution

HOSS                   : keyword for Householder - Sturm Sequence solution

JACO                   : keyword for Jacobi solution

SPIT                   : keyword for Subspace Iteration solution

norm                   : normalisation of Eigenvectors. (Integer)
                                  Values:           0 - Maximum component is 1.0
                                                    1 - Euclidean norm
                                                    3 - No normalisation

modes                  : to request frequencies or mode shapes for printing. (Integer)
                                  Values:           0 - frequency and mode shapes
                                                    1 - frequency only

lmode                  : lowest mode number required. (Integer)

hmode                  : the highest mode number required. Compulsory for SPIT, defaults to all frequencies if
                         blank. (Integer)

subspace               : size of subspace (the number of frequencies to iterate over). For SPIT only. (Integer)

cutoff                 : upper limit to the calculated frequencies (Hertz). For SPIT only. (Real)

shift                  : frequency shift (Hertz). For SPIT only (Real). See Notes below.

Notes


1.       If HOSS is selected and the number of frequencies is greater than 25% of the number of dynamic
         freedoms (or 40% if no modes are requested), then HOQL is substituted.

2.       If subspace is omitted, it defaults to the lesser of 2n or n+8 where n is the number of frequencies
         requested.

3.       If SPIT and no suppression data is supplied in the run, the shift is applied to prevent failure (occurs if the
         stiffness matrix is singular (I.e. when the structure is not properly supported)). If no shift is supplied, the
         program calculates a suitable value. If the run is a substructure assembly and all suppressions are in the
         substructures, a very small value for shift must be supplied to prevent the program from calculating an
         unsuitable value. The effect of the shift means that a shifted stiffness matrix (Ks) will be utilised. This
         can be detailed mathematically as:




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




         K s = Kpluss.M



         where s = (2 π f )         2




        f is the frequency shift specified

Examples

(i)     A simple frequency command using HOSS to select all frequencies. Mode shapes are normalised to a
        maximum value of 1.0, frequencies and mode shapes are to be printed.


        FREQUENCY           HOSS        0    0

(ii)    A frequency command using SPIT requesting 8 frequencies, a subspace of 14 and a cutoff of 100 Hertz.


        FREQUENCY           SPIT        0    0     1     8    14      100.0




5.1.17      SAVE FILES Command

To define which files or sets of files are to be saved for subsequent runs. Two types of files may be saved, those
for further numeric processing and those for interfacing to graphical results display programs such as
FEMVIEW.


        5.1.17.1 Files for Numerical Processing

            SAVE                            set               (FILES)




Parameters

SAVE          : keyword

set           : keywords to define sets of files to be saved for subsequent processing. See also Section 3.3.

                Name                    Subsequent run/processing




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



                ADLD            -      job type LINE, to rerun with further loads
                ADMS            -      job type FREQ, to rerun with further masses
                ADFQ            -      job type FREQ (SPIT), to rerun with additional frequencies
                COMP            -      job type COMP or COMD, to save component data in a single formatted file
                                                                                   for transfer to another analysis on a different

                                                                                   machine and/or program
                COMF            -      as for COMP except matrices will be output in full form instead of packed
                                       symmetric form
                DYPO            -      for dynamics response calculations using RESPONSE
                LOCO            -      for loadcase factoring using LOCO

FILES           :               keyword

Note


The SAVE command may be used to save explicit files using a list of file numbers. See Appendix -G.

Example

(i)      To save files necessary for subsequent loadcase factoring and combination

         SAVE       LOCO      FILES

(ii)     To save files for both loadcase factoring and for subsequent reanalysis with the application of new
         loadcases.

         SAVE       LOCO      FILES
         SAVE       ADLD      FILES

(iii)    The above example can be specified using a single SAVE FILES command.

         SAVE       LOCO      ADLD       FILES


         5.1.17.2 Interface Files for Plotting Programs


        SAVE        FEMM            FEMD           FEMS           (FILES)          CREATE               (name)   (FILE    filenm)

                                                                                   APPEND
                    PATM

                    PATD
                                             (FILES)
                    PTDC




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



Parameters

SAVE          : keyword

FEMM          : keyword to denote model data to be added to FEMVIEW file

FEMD          : keyword to denote displacements to be added to FEMVIEW file

FEMS          : keyword to denote stresses to be added to FEMVIEW file

FILES         : keyword (Optional)

CREATE : keyword to indicate that model data must be added to FEMVIEW file

APPEND : keyword to indicate model data not to be added to FEMVIEW file

name          : model name for FEMVIEW (defaults to structure name)

FILE          : keyword to indicate file name follows

filenm        : name of file to contain FEMVIEW data

PATM          : keyword to denote model data to be added to neutral PATRAN file

PATD          : keyword to denote displacements to be added to binary PATRAN file

PTDC          : keyword to denote displacements to be added to ascii PATRAN file

Notes


1.      If SAVE FEMM/FEMD/FEMS is used in a component recovery run any explicit file name (filenm) will
        be ignored. The name of each recovered component being processed is used to generate the Femview
        file(s) required (one for each recovered component).

2.      The PATM mnemonic may only be used at Restart Stage 1 to read an ASAS data file and produce a
        PATRAN model neutral file. ASAS does not continue beyond Stage 1.




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



Examples

(i)     To save files necessary for viewing results in FEMVIEW


        SAVE       FEMM       FEMD         FEMS      FILES        APPEND         TANKER         FILE    TANKER.FVI

(ii)    To save files necessary for viewing displacements in PATRAN


        SAVE       PATD       FILES




5.1.18      COPY Command

To copy a set of files from a previous analysis in the current project into the current run.

       COPY        set       FILES         (FROM)               COMPONENT                    name

                                                                STRUCTURE                    name

                                                                STRUCTURE                    name       RECO      comp




Parameters

COPY                   : keyword

set                    : keywords to define the set of files required. See also Section 3.3.

                         Name              Job type

                         ADLD          -   LINE, additional loads rerun
                         ADMS          -   FREQ, additional masses rerun
                         ADFQ          -   FREQ (SPIT), additional frequencies rerun

FILES                  : compulsory keyword

FROM                   : keyword

COMPONENT              : keyword

STRUCTURE              : keyword

name                   : name of an existing component or structure from which the file set is to be copied.
                         (4 character, Alphanumeric)

RECO                   : keyword to indicate that the files are to be copied from a recovered component




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


comp                   : number of the recovered component from which the set of files is to be copied. (Integer)

Note


The COPY command may be used to copy explicit files using a list of file numbers. See Appendix -G.

Examples


This run is being performed with new loadcase data using the files saved from a previous structure run named
SHIP.

        COPY ADLD FILES FROM STRUCTURE SHIP




5.1.19      RESU command

To specify saving of results. For static job, the displacements and stresses will be saved. For natural frequency
job, the frequencies and mode shapes will be saved.

            RESU



Parameters

RESU          : keyword

Example


            RESU

Notes


1.      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.

2.      RESU command is not valid for a component creation job and this will be ignored if specified.
        Initialisation of the database must therefore be made in the global structure run for a sub-structured
        analysis.




5.1.20      WARN Command

This command may be used to suppress excessive numbers of what the user may feel are irrelevant warning
messages. Only certain warnings fall into this category and these are listed below. At the end of the data




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



checking stage of ASAS, a summary of the suppressed messages is output. If the command is absent all warning
messages are output. Optional.

          WARN                     nnnn

Parameters

WARN          : keyword

nnnn          : maximum number of warning messages to be printed of each type, if zero or blank 10 is assumed.
                (Integer)

Note


Current suppressible messages are:

1.      FAX3 Element: Area exceeds half length squared

2.      Shell and Membrane elements: Thickness exceeds radius of inscribed circle

3.      Higher order elements: Midside node temperature not linear between corner node values (This is
        recommended if ASASHEAT has been used with the FULL option to generate the data for ASAS)

4.      Prescribed Displacement not assigned although node/freedom appears in Displaced Freedom data.
        Suppression assumed

5.      Non-existent node referenced in SUPP or DISP data

6.      Non-existent freedom referenced in SUPP or DISP data

7.      Zero Spring Stiffness

8.      Undefined value of pressure on a face. Zero assumed

9.      Distributed load on non-unique BEAM/TUBE element

Example


In this example the user only wants to see the first 5 occurrences of each of the suppressible messages.

        WARN       5




5.1.21      UNITS Command

Recommended. Some postprocessors require to know which units are being used.




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



This command allows the user to define the units to be employed in the analysis and the default units for the
input data. Facilities exist to specify the results units for output if they are required to be different from those
supplied for input (see Section 5.1.21.2). 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 2.6).

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 and 5.5.1 for further details.


5.1.21.1        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)


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 Appendix -B.

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




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



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

Note


In substructure analyses, all components to be assembled together must use the same global units definition.
Similarly, the resulting structure must also use the same global units. If parts of the overall structure are required
to be modelled using a different set of units, the local UNITS commands within the main data should be
employed. See Sections 5.2.1, 5.3.1, 5.4.1 and 5.5.1.


5.1.21.2        Results UNITS Command

This permits the displacements and/or stresses to be reported in different units from those supplied for the input
data. This can only be used if a global units definition has been supplied.

                 UNITS                  resultnm                     unitnm




Parameters

UNITS             : keyword

resultnm          : keyword to identify results units to be modified. The following keywords are available

                     DISP         displacement printing
                     STRE         stress or force printing

unitnm            : name of unit to be utilised. See 5.1.21.1 for valid names.

Notes


1.      For the results units, the angular term may be specified. (Default is radians).
        Valid names are




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


                     RADIAN(S)                  RAD
                     DEGREE(S)                  DEG


2.     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. For example:

                     UNITS N M
                     UNITS STRE            MM

            will provide stresses in terms of N/mm2

Examples


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.


2.      The S.I. system is to be used for input, but the displacements are to be printed in mm and the stresses in
        KN/mm2

       UNITS           N            M
       UNITS           DISP         MM
       UNITS           STRE         KN       MILLIMETRES

       Note that the reactions printed in the displacement report will be in Newtons and Millimetres.

       The derived consistent unit of mass will be 1 kg.




5.1.22      LIBRARY Command

This command is used to provide the name of an external file which contains beam section information for use in
the geometric property data. The library file may be standard steel section library, as supplied with the software,
or may contain user supplied sections generated using program SECTIONS. Only one such command line may
appear in the preliminary data. See Appendix A.7.

                LIBRARY                     filenm




Parameters

LIBRARY           : keyword




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



filenm            : up to 6 character name of an external (physical) file which contains section library information
                     for beam type elements. The file must either be one of the standard section libraries supplied
                     with the software (listed below) or user generated usingprogram SECTIONS.

Standard Libraries


AISCLB       AISC wide flange (I/H) sections




5.1.23      INFO Command

This command may be used to read and print a file of site dependent information.

             INFO                                 ALL

                                                  name




Parameters

INFO          : keyword

ALL           : keyword to indicate all information in the file is to be printed

name          : name of an information block which is to be printed

Notes


1.      This command will always print the general information block on the file and any information relevant to
        the program currently running, even if no parameters are included.

2.      Program information relating to other programs may be obtained by using one or more of the following
        abbreviations:
                ASAS          -            ASAS                       LOCO         -             LOCO
                RESP          -            RESPONSE                   POST         -             POST
                WAVE          -            WAVE                       MASS         -             MASS
                FATJ          -            FATJACK                    BEAM         -             BEAMST
                PATT          -            PATTA                      XTRA         -             XTRACT
                SPLI          -            SPLINTER                   MAXN         -             MAXMIN
                ASNL          -            ASAS-NL                    PSNL         -             POST-NL


For other site dependent names, users should contact their local site representative.




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


5.1.24      END Command

To terminate the preliminary data. Compulsory.


             END




Parameters

END           : compulsory keyword




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



5.2     PHYSICAL Property Data

These data blocks define the physical properties and shape of the structure.

The following data blocks may be input here.

                         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

                         Sets Data................ .................. ................ see Section 5.2.8

                         Component Topology............... ................ see Section 5.2.9




5.2.1       UNITS Command

If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.21), 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



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


       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 5.1.21.1.

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 Appendix -B. 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 2.6.

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.
        SECT                           -   Section data - UNITS command may appear anywhere.
        SKEW and NSKW                  -   Skew systems - UNITS not applicable.
        TOPO                           -   Component topology data - UNITS command may appear anywhere.




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


Example


   Data                                                               Operational Units                    Notes

   SYSTEM DATA AREA 50000
   PROJECT ASAS
   JOB NEW LINE
   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




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. The last system of coordinate data is terminated by an END keyword.



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



                    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   z-inc
                                                    x                                                    i
                                                                  SIN                 hleng1              SIN         hleng2
                    IMPE           ampl             y
                                                                  COS                 harno1             COS          hleng2
                                                    z


                    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.

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 5-30
       ASAS (Linear) User Manual                                                                       Boundary Conditions 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 to be used. Optional, if omitted CART is assumed.
                CART           (name)

                  CYLI                                    DEG

                  SPHE               name                  RAD

Parameters

CART          : keyword to denote a cartesian system, global or local

CYLI          : keyword to denote a cylindrical polar system

SHPE          : keyword to denote a 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. (Alphanumeric, 4 character, 1st character must be
                alphabetic.)

DEG           : keyword used to define the angular unit as degrees for θ and φ. If both DEG and RAD are
                omitted, degrees are assumed

RAD           : keyword used to define the angular unit as 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 commands define the origin and direction of the local axis system.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-31
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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 direction 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 5-32
       ASAS (Linear) User Manual                                                                        Boundary Conditions 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.

2 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.

                                                                        2 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’).

                                                                        ø 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 5-33
        ASAS (Linear) User Manual                                                                      Boundary Conditions Data


5.2.2.3         Node Coordinates

     //node//                        // x //                     // y //                   // z //

                                     // r //                     // θ //                   // z //

                                     // r //                     // θ //                   // φ //

     RP            nrep            inode                x-inc                    y-inc                   z-inc

                                                         r-inc                   θ-inc                   z-inc

                                                         r-inc                   θ-inc                   ø-inc


     RRP           nrrep           iinode               x-inc                    y-inc                   z-inc

                                                         r-inc                   θ-inc                   z-inc

                                                         r-inc                   θ-inc                   φ-inc


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)
θ-inc
φ-inc



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

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
   ****     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
   ****     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



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

     /
     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 commands 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
                                                 X             SIN                hlengy                SIN        hlengz
                 IMPE            ampl            Y                                hlengz                           hlengx
                                                 Z             COS                hlengx                COS        hlengy




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 5-36
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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 local z direction

A radial variation data will be generated of the form:




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


Spherical Systems



                                                               SIN                                      SIN
                 IMPE                  ampl                                       harno1                          harno2
                                                               COS                                      COS




Parameters

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


A radial variation data will be generated of the form:




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

5.2.3       Element Topology Data

To define each element which makes up the structure.

                ELEM


                MATP                      material



                GROU                      group



                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)

GROU          : keyword to define the group to which all following elements are assigned until another GROU
                line is used

group         : group number. (Integer, 1-9999.) If 9999 is used, results for elements in this group will not be
                printed. This is useful if dummy elements have been used with Rigid Constraints (see Section
                5.3.8)

eltype        : element type. (Alphanumeric, 4 characters.) For a full list of elements available, see Appendix -A.

mtype         : type of mass matrix for this element (natural frequency runs only). 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, 1-999999)




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

geom          : geometric property integer. (Integer, 1-999999.) 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 3.2.2). (Integer, 1-999999)

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)

END           : compulsory keyword 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

(i)      An example of a simple element topology data block.

       ELEM
       MATP    1
       BEAM    8       9         1
       BEAM    9      10         2
       BEAM    8      10         1
       BEAM   10      11         1
       END

(ii)     An example of element topology data using data generation.

       ELEM
       MATP    1
       GROU   10
       /
       BEAM     1     21     3
       BEAM     1     41     2



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-40
        ASAS (Linear) User Manual                                                                      Boundary Conditions Data

    BEAM 41 21               2
    RP   10,1
    END

(iii)    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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-41
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.4       Material Properties Data

To define the material properties for each material type used in the analysis. The material may be isotropic,
anisotropic, orthotropic, laminated or temperature dependent isotropic.




                     MATE


                     mat            ISO               elas              poisson             (expansion)            (density)



                     mat            (skew )           AISO              density             properties



                     mat            (skew )           ORTH              density             properties



                     mat            (skew )           LAMI              (density)



                     mat            TISO           elas         poisson            expansion             density        temp



                     END


Parameters

MATE          : compulsory header keyword to denote the start of the material properties data.

ISO           : keyword to define an isotropic material.

AISO          : keyword to define an anisotropic material.

ORTH          : keyword to define an orthotropic material

LAMI          : keyword to define a laminated material

TISO          : keyword to define a temperature dependent isotropic material.

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 to 5.2.4.5.

2.      Every material referenced in the element topology data and laminated geometry data must be fully
        defined in this data block.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-42
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.2.4.1          Isotropic Material Properties

To define the properties for an isotropic material.

           mat          ISO            elas            poisson                (expansion)                (density)


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)

expansion           : linear coefficient of thermal expansion. Optional. (Real)

density             : density, mass per unit volume. Optional. (Real)

Notes


1.        The expansion coefficient is optional and is only required if temperatures or face temperatures are to be
          included in any of the loading applied to the structure. If present, the TEMP option may be used for more
          complete data checking.

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 analysis is being performed. If present, the
          BODY option may be used for more complete data checking. See Appendix -B.

3.        For a steady state heat conduction analysis (JOB HEAT) the only material properties required are the
          thermal conductivity coefficients. Two conductivity coefficients in the element local X and Y directions,
          are required for 1-D and 2-D elements. For BRICK elements, three coefficients in the global X,Y and Z
          directions are required.

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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-43
         ASAS (Linear) User Manual                                                                     Boundary Conditions Data

5.2.4.2          Anisotropic Material Properties

To define the properties for an anisotropic material. See Appendix -A.

           mat              (skew )                AISO                   density

             :                       properties


Parameters

mat               : material property integer. (Integer, 1-9999)

skew              : skew system integer. (Integer, 1-9999)

AISO              : keyword to define the material as anisotropic.

density           : density, mass per unit volume. (Real)

properties        : coefficients of the anisotropic stress-strain matrix, 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 analysis is being performed. If present, the
          BODY option may be used for more complete data checking. If present, the value of density must be on
          the same line as AISO.

2.        The anisotropic stress-strain properties must start on the first continuation line and may then spread onto
          further continuation lines as required.

Example


An example of an anisotropic material for a GCS8 element.

     MATE
     11      AISO         0.290
     :      0.42E8          0.18E8           0.39E8          0.18E8           0.16E8
     :      0.42E8          0.0              0.0             0.0              0.13E8
     :      0.0             0.0              0.0             0.0              0.12E8
     :      0.0             0.0              0.0             0.0              0.0
     :      0.11E8
     :   0.1094E-4                0.0910E-4             0.1412E-4
     END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-44
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.4.3         Orthotropic Material Data

To define the properties for an orthotropic material. See Appendix -A.

          mat           (skew )             ORTH             (density)


          :             e11                 e22              e33                 g12               g23         g31

          :             v 12                v 23             v 31                a11               a22         a33




Parameters

mat               : material integer. (Integer, 1-9999)

skew              : skew integer defining orientation of material axis. (Integer, 1-9999)

ORTH              : keyword

density           : material density. (Real)

e11-e33           : Young’s modulus in local 1, 2 and 3 directions. (Real)

g12-g31           : shear modulii in local 12, 23 and 31 planes. (Real)

v12-v31           : Poisson’s ratio in local 12, 23 and 31 planes. (Real)

a11-a33           : coefficients of thermal expansion in local 1, 2 and 3 directions. (Real)

Notes


1.      The orthotropic material properties must start on a new continuation line and may then spread onto
        further continuation lines if necessary.

2.      This material type may be used for either laminate layer definition or for the whole of an element for
        which this material type may be used.


        5.2.4.4 Laminated Material Properties

To define the properties for a laminated material.

          mat           (skew)              LAMI             (density)




Parameters

mat               : material integer. (Integer, 1-9999)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-45
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


skew               : skew integer defining orientation of material axis. (Integer, 1-9999)

LAMI               : keyword

density            : material density. (Real)

Notes


1.      A material integer and LAMI must be given even if both skew and density are omitted.

2.      This material type may only be used for elements having a laminate capability and which have laminate
        geometric properties.

3.      Different lami material properties may be used for elements having the same lamina geometric property
        but elements with the same lami material property must have the same geometric property.

4.      In addition to the material for the element as a whole it is also necessary to define the material for the
        individual laminates in the material data block. These may be ISO, AISO or ORTH material types only.

5.      For further details see Appendix A.6.


        5.2.4.5 Isotropic Material Properties - Temperature Dependent

Defines the properties for a temperature dependent isotropic material.

          mat          TISO          elas        poisson            expansion               density         temp

               :      elas            poisson            expansion               density            temp




Parameters

mat                : property integer. (Integer, 1-9999)

TISO               : keyword to define the material as temperature dependent isotropic.

elas               : modulus of elasticity. (Real)

poisson            : Poisson’s ratio. (Real, 0.0≤poisson<0.5)

expansion          : linear coefficient of thermal expansion. (Real)

density            : density. (Real)

temp               : temperature at which these properties apply. Properties should be supplied in the order of
                     increasing temperature.            The properties for each temperature must be on a separate
                     continuation line. (Real)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-46
         ASAS (Linear) User Manual                                                                     Boundary Conditions Data

Notes


1.        The material properties used in the analysis for each element are based on the average nodal temperature
          for the element as defined by the temperatures in the first user loadcase. The material properties are
          linearly interpolated between the values defined in the input table. If an element’s average temperature is
          below or above the temperatures referred to in the material property input no extrapolation is carried out,
          that is, the properties are assumed constant below the lowest and above the highest specified
          temperatures, having the respective extreme values.

2.        Because the first loadcase defines the material properties it may be necessary to make this a dummy
          loadcase which specifies the average temperature for various real loadcases which follow. For
          circumstances where the temperatures are widely different between real loadcases it may be necessary to
          run each loadcase as a separate analysis.

Example


An example of a single temperature dependent material with properties defined at 0°, 200°, 350°, 500° and
600°.

     MATE
     17     TISO         2.07E11           0.32          1.47E-6          0.284            0.0
     :                   2.01E11           0.31          1.57E-6          0.284         200.0
     :                   1.87E11           0.30          1.72E-6          0.284         350.0
     :                   1.73E11           0.30          1.92E-6          0.284         500.0
     :                   1.69E11           0.30          2.08E-6          0.284         600.0
     END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-47
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

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. The general format for the geometric properties data is described in Section 5.2.5.1 below. Section
5.2.5.2 describes the specific data required for composite shells. Section 5.2.5.3 describes the specific data
required for thick shell elements for which offsets may be defined. Section 5.2.5.4 describes the specific data
required for the beam elements for which local axes orientation and/or offsets may be defined.


5.2.5.1         General format for the explicit definition of geometric properties

                GEOM


                geom                         eltype                     properties



                END




Parameters

GEOM              : compulsory header keyword to denote the start of the geometric property data.

geom              : identifying number for the geometric property. This number must be unique, a separate
                     number being used for every different element type as well as for each different geometric
                     definition. (Integer)

eltype            : element type. This must correspond to the element type defined in the element topology
                     referencing this geometric property.

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)

END               : keyword to denote the end of the geometric properties data block.

Examples


A simple example of geometric properties.

            GEOM
            1            CURB                   1208.0                23.0                  497.0           0.0   0.0
                10.0       64.2
            2            CURB                   1402.0                29.0                  571.0           0.0   0.0
              10.0   75.7
            101    FLA2                         50.1
            END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-48
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.2.5.2         Definition of geometric properties for composite shells

The general format used to define the laminates of a composite shell element is given below. A full description
of laminated shell properties is given in Appendix A.6.

               geom                   eltype                  thick


               :                      LAMI                    nlay                    (sym)


               :                      mat                      thick                    theta




Parameters

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)

eltype             : element type. This must correspond to the element type defined in the element topology
                     referencing this geometry property.

thick              : thickness of the element at each node point in order of nodes in the element topology. If the
                     element is constant thickness then only one value is required. (Real)

LAMI               : keyword to denote start of lamina data.

nlay               : number of layers in the laminate. (Integer)

sym                : symmetry flag (1 = symmetric layup). (Integer)

mat                : material integer for layer. (Integer)

thick              : layer thickness. (Real)

theta              : angle between material X axis and layer primary direction. (Real)

Notes


1.      The LAMI keyword must start on a new continuation line. The layer definition line is repeated for each
        of the nlay layers.

2.      If a symmetric layup is defined (sym = 1) then nlay is half the number of layers.

3.      The material integer may be for materials type ISO, AISO and ORTH only.

4.      Layer materials may be used repeatedly within the same laminate or for different laminates.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-49
        ASAS (Linear) User Manual                                                                      Boundary Conditions Data

5.2.5.3         Definition of geometric properties for thick shell elements QUS4, TCS6 and TCS8

The general format used to define the geometric properties of a thick shell element is given below. Further
details relating to rigid offsets are given in Appendix A.5.

               geom                   eltype                  thick


               :                      OFFS                   zloff




Parameters

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)

eltype             : element type. This must correspond to the element type defined in the element topology
                     referencing this geometry property. Valid types are: QUS4, TCS6 and TCS8.

thick              : thickness of the element at each node point in order of nodes in the element topology. If the
                     element has constant thickness then only one value is required. (Real)

OFFS               : keyword to denote start of rigid offset data.

zloff              : local z offset at each node point in order of nodes in the element topology. If the element has
                     constant offset then only one value is required. (Real)

Note


The OFFS keyword, if present, must start on a new continuation line.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-50
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.5.4         Definition of geometric properties for beam elements having local axes definition
                and/or rigid offsets

There are eight 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 5.2.5.1 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                                             ( (SLEN)        length)
                                                               a     iz    iy     j

                                       OFFG             glboff

                                       OFFS             locoff
                    :
                                       OFSK             skew                    skw off
                                       OFCO             coords

                    :    STEP            a    iz iy j               (length)
                                              sectid




b) BM2D

                                                                    sectid
                        geom             BM2D                                                  ( (SLEN)       length)
                                                                a    iz    ay

                                     OFFG             glboff

                                     OFFS             locoff
                :
                                     OFSK             skew                  skw off
                                     OFCO             coords

                :       STEP            a     iz ay                (length)
                                             sectid



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 5-51
      ASAS (Linear) User Manual                                                                          Boundary Conditions Data


c) BM3D
                                                     BETA         angle

                                                     NODE         nodeno

                                     sectid                                             (XY)
                                                     (COOR)       pcoor
            geom       BM3D                                                                      (SHAR)*      ay   az   ((SLEN)   length)
                                    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

              :       STEP          a     iz    iy    j    ay    az         (length)
                                                  sectid




d) TUBE
                                                     BETA         angle

                                                     NODE         nodeno

                                     sectid                                             (XY)
                                                     (COOR)       pcoor
            geom       TUBE                                                                             ( (SLEN)    length)
                                    dia thick        GPOS                               XZ

                                                     GNEG

                                                     SPOS                    axis
                                                                  skew
                                                     SNEG

                                                     VECT         vcoor


                                    OFFG             glboff

                                    OFFS             locoff
              :
                                    OFSK             skew                  skwoff

                                    OFCO             coords

              :       STEP           dia     thick              (length)
                                        sectid




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 5-52
       ASAS (Linear) User Manual                                                                                           Boundary Conditions Data


e) BAX3
                                                                          BETA      angle

                                                                          NODE      nodeno
                                                                                                                (XY)
                                                                          (COOR)    pcoor
            geom      BAX3      a1        iz1     iy1         j1                                                              (SHAR)           ay1         az1
                                                                          GPOS                                  XZ

                                                                          GNEG

                                                                          SPOS                    axis
                                                                                    skew
                                                                          SNEG

                                                                          VECT        vcoor

              :       a2       iz2              iy2                j2       ay2     az2           inty          intz         intj

                                     OFFG                          glboff

                                     OFFS                          locoff
              :
                                     OFSK                          skew                skwoff

                                     OFCO                          coords




Note


Data on continuation line (starting a2) may be appended to end of first line.

f) BMGN
                                                                             BETA         angle

                                                                             NODE         nodeno
                                                                                                                     (XY)
                                                                             (COOR)       pcoor
            geom       BMGN          a1     iz1         iy1        j1                                                                 (SHAR)         ay1         az1
                                                                             GPOS                                      XZ

                                                                             GNEG

                                                                             SPOS                        axis
                                                                                          skew
                                                                             SNEG

                                                                             VECT         vcoor


              :         a2       iz2              iy2               j2       ay2       az2         inty              intz      intj


                                     OFFG                          glboff

                                     OFFS                          locoff
              :
                                     OFSK                          skew                skwoff

                                     OFCO                          coords




Note


Data on continuation line (starting a2) may be appended to end of first line.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                           Page 5-53
       ASAS (Linear) User Manual                                                                        Boundary Conditions Data


g) GRIL

                                                 sectid
              geom          GRIL                                                ( (SLEN)                  length)
                                             a    iz       iy    j



                  :             OFFS                     locoff



                  :             STEP                   a        iz iy j                    (length)
                                                                 sectid




Note


Only local offsets may be defined and these relate to local X’ and Z’ directions only.


h) TCBM



              geom             TCBM                 a1          iz1    iy2            j1     ay1        az2




              :                                     a2          iz2    iy2            j2     ay2        az2




              :                                     a3          iz3    iy3            j3     ay3        az3



                                   OFFG             glboff

                                   OFFS             locoff
              :
                                   OFSK             skew                     skwoff

                                   OFCO             coords




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-54
       ASAS (Linear) User Manual                                                                       Boundary Conditions 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.
BAX3, BMGN,
GRIL, TCBM

sectid                 : section identifier. (Alphanumeric up to 12 characters). This refers to a section either
                         predefined in an external library or input as SECTion data. See Section 5.2.6 and Appendix
                         A.7.


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)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-55
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

VECT                   : keyword to denote that local axis defined by vector. See Appendix A.2.

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.

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 and mid point for TCBM. (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) Step definition

SLEN                   : keyword to denote that a step length follows.

length                 : length of elemental step. (Real) See Appendix A.4.

STEP                   : keyword to denote that this beam has steps in the cross-section properties at certain points
                         along its length. See Appendix A.4.


e) Basic properties (see Appendix -A for full element specification)

a, a1, a2, a3          : cross-sectional area, constant for section or at node/end positions on the beam. (Real)

iz, iz1, iz2, iz3      : 2nd moment of area about local ZZ axis, constant for section or at node/end positions on
                         beam. (Real)

iy, iy1, iy2, iy3      : 2nd moment of area about local YY axis, constant for section or at node/end positions on
                         beam. (Real)



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-56
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

j, j1, j2, j3          : torsion constant, constant for section or at node/end positions on beam. (Real)

SHAR                   : keyword indicating that shear areas follow.

ay,ay1,ay2,ay3 : shear area in local Y, constant for section or at node/end positions on beam. (Real)

az,az1,az2,az3 : shear area in local Z, constant for section or at node/end positions on beam. (Real)

inty, intz, intj       : order of parametric interpolation of IY, IZ, J between ends of the beam. (Integer)

Notes


1.      For stepped beams, it is permissible to define some steps using sections and others using explicit property
        definition. For example

                           GEOM
                           1           BEAM              64.2                  1208              497          23.
                           :           STEP              W12X100               12.0
        is valid

2.      Non-tubular sections must not be assigned to TUBE elements.

3.      Only relevant flexural properties will be utilised for a given element type, for example

                                                              BEAM          BM2D           BM3D         TUBE        GRILL

                                                                 ♦             ♦             ♦                       ♦
                Area                          A
                                                                 ♦             ♦             ♦
                Moment of Inertia             IZ
                                                                 ♦                           ♦                       ♦
                Moment of Inertia             IY
                                                                 ♦                           ♦                       ♦
                Torsion constant              J
                                                                               ♦             ♦
                Shear Area                    AY
                                                                                             ♦                       ♦
                Shear Area                    AZ

                                                                                                          ♦
                Diameter                      D
                                                                                                          ♦
                Thickness                     T



4.      Note that the local axes convention used for sections applied to GRIL elements is the reverse to that used
        for the other element types. See Section 5.2.6.1.

5.      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 5-57
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data



5.2.5.5         Definition of Geometric Properties for Stiffened Panels

The general format used to define the geometric details of a stiffened panel is given below.

               geom              eltype            thick

               :                SSTF              nlay

               :                mat             (sectid)          space            offset           theta




Parameters

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)

eltype             : element type. They must correspond to the element type defined in the element topology
                     referencing the geometric property. Valid types are: QUS4, TCS6 and TCS8.

thick              : thickness of the element at each node point in order of nodes in the element topology. If the
                     element has constant thickness then only one value is required. (Real)

SSTF               : keyword to denote start of stiffened panel data.

nlay               : number of shell and stiffener layers to define the panel (Integer)

mat                : material integer for layer. (Integer)

sectid             : section identifier for stiffener (Alphanumeric up to 12 characters). This refers to a section
                     either predefined in an external library or input as SECTion data. For shell layer, this data may
                     be omitted or specified as SHELL.

space              : layer thickness for shell layer or spacing between stiffeners for stiffener. (Real)

offset             : offset of layer mid-surface from the reference axis for shell layer or offset of stiffener section
                     origin from the reference axis for stiffener. (Real)

theta              : angle (in degrees) between material X axis and layer principle direction. (Real)

Notes


1.       The element that has stiffened panel geometric properties must also be assigned a LAMI material
         property type.

2.       The layer properties (mat, secid, space, offset and theta) are repeated nlay times.

3.       If the layer stress resultants are computed, these will be given in ascending layer numbers from 1 to nlay.
         The layer number corresponds to the order in which the layer data are specified in the SSTF data.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-58
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


4.      If space is specified as 0.0, the layer is assumed to be inactive, i.e. it will not contribute towards the
        panel stiffness and all the stresses will be zero. It is useful to use this setting to maintain a consistent
        definition of layer number throughout the entire model if the stiffening pattern is not uniform.

5.      It is assumed that the Y axis of the stiffener section lies along the local Z axis of the shell element.

6.      If offset is specified as 0.0 in a stiffener definition, it is assumed that the stiffener section origin lies on
        the top surface of the equivalent shell element, i.e. offset is equal to t/2, where t is the average thickness
        of the element (average of thick).

7.      It is assumed that the section neutral axis position relative to the section origin is in the same direction as
        the offset data specified (i.e. offset), i.e. the section neutral axis is always further away from the shell
        reference axis than the origin offset. The following diagrams illustrate the assumed stiffened patterns
        when different section origin is specified for offset equals to 0.0 (i.e. attached to top surface). If a
        negative offset is given, the stiffeners will be upside down to the shown patterns.




        Z                                                                                               Z
                                                            Z




            ORIG YMIN 0.0                                       ORIG YMAX 0.0                                no ORIG



8.      The stiffened panel properties are computed from the specified SSTF data. Thus, the element thickness
        thick will not affect the computed panel properties except the following:

     Variable element thicknesses cause variation of material stiffness over the element. This can be seen from
            the dependency on thickness in the shell anisotropic material matrix. The conversion of stiffened
            panel properties into the equivalent anisotropic form is made based on the averaged element thickness.

     Average element thickness defines the default stiffener offset.

     The element thickness defines the thermal gradient thickness for face temperature load calculation.


9.      For face temperatures, the mean temperature is applied to the reference surface of the panel while the
        thermal curvature is the temperature difference of the two specified face values divided by thick. It is
        assumed that this temperature distribution applies to both the stiffener and panel.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 5-59
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


Example




                                                                    Os



                                         0.2                                        0.2                          0.1 0.11
   Z

          x


The stiffened panel geometry is as shown above. The section properties of the T-stiffeners are defined in the
section data with a section name BEAM01. The origin of the section is taken as the bottom of the section (point
Os in the diagram). Both the panel and the stiffeners are made from the same material with material property
integer 1. The stiffened panel elements have laminated (LAMI) material properties of material property integer
11.

The following illustrate the data required for defining the stiffened panel elements in such an analysis:

        ELEM
        //
        /
        MATP 11
        QUS4    1             22       21       1        1
        rp 5           1
        rrp 4        20
        END
        MATE
           1         ISO           205.0E9          0.3          1.0E-5            7850.0
              11     LAMI
        END
        GEOM
        * Define stiffened panel properties
        1 QUS4 0.02
        * Two layers - one shell, one stiffener
        : sstf 2
        * Shell layer
        : 1         0.02   0.01    0.0
        * Stiffener layer (reinforcement in Y)
        : 1        beam01 0.2               0.11         90.0
        END
        SECT
        * Define T section properties
        beam01 tee xsec 0.15 0.075 0.015                                       0.0075



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-60
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


       * Origin at bottom of section
       : orig ymin 0.0
       END

If the stiffened panel reference axis coincides with the shell mid-surface, then the geometric property data can be
simplified as follows:

       GEOM
       * Define stiffened panel properties
       1 QUS4 0.02
       * Two layers - one shell, one stiffener
       : sstf 2
       * Shell layer
       : 1           0.02
       * Stiffener layer (reinforcement in y)
       * Default offset means beam origin at shell top surface
       : 1 beam01    0.2       0.0          90.0
       END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-61
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


5.2.6       Section Data

To define section type, dimensions and properties for sections to be used with element types BEAM, BM2D,
BM3D, GRIL and TUBE elements.

               SECT

               sectid              type                   XSEC                    dimensions


               sectid              FAB                    ftype                   dimensions



               :                                          ftype                   dimensions




                                                            flexprops
               :                  FLEX
                                                            proptype                            property


                                                          ZMAX                 (zoff)                   YMAX            (yoff)

               :                  ORIG                    ZMIN                 (zoff)                   YMIN            (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 5-62
       ASAS (Linear) User Manual                                                                       Boundary Conditions 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

                         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.

ORIG              : keyword to denote that a new section origin is to be defined.

YMAX              : keyword to denote that the datum for local Z centre-line is the top edge of the section

YMIN              : keyword to denote that the datum for local Z centre-line is the bottom edge of the section.

ZMAX              : keyword to denote that the datum for local Y centre-line is the right hand edge of the section.

ZMIN              : keyword to denote that the datum for local Y centre-line is the left hand edge of the section.

CENT              : indicates no local Y” or Z” offsets appllied. (i.e. origin on centroidal axis)

yoff              : local Y” offset from the datum line, +ve offset is away from the section.

zoff              : local Z” offset from the datum line, +ve offset is away from the section




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-63
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

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. The section dimensions will be stored for utilisation in the stress calculations in
        the BEAMST post-processor.

        If only FLEX is defined, all property values must be supplied. The FLEX command is not valid for a
        TUBE element. If post-processing in BEAMST is required for elements associated with this section, the
        section dimensions will have to be specified in the BEAMST data file.

        If both XSEC and FLEX commands are utilised, any geometric properties explicitly defined will
        overwrite those calculated from the section dimensions. The use of XSEC and FLEX together is not
        permitted for TUBE elements. This feature permits modification to the stiffness of the section to model
        ring or web stiffeners, built up sections, etc. The section dimensions will be stored for utilisation in the
        stress calculations in the post-processor BEAMST.


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 or CURB. The
        order of these data lines are interchangeable, but a logical sequence is recommended.

4.      Positive values of origin offsets are as shown:


                                         zoff O                                         ZMIN
                                               yoff
               YMAX


                                                                                                          YMIN
                                                                                yoff
                                    ZMAX                                          O zoff




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-64
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data



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, or where post-processing in BEAMST is intended, 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. (See also Appendix A.7).

Note


The axes shown correspond to the local axes of the member for element types BEAM, BM3D, TUBE and
BM2D. Positive Y is from bottom to top and positive Z is from left to right. For GRIL elements, the axes are
reversed i.e Y becomes Z and vice versa.

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 5-65
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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      b   tf tw (b2)     (tf2)

where           d         is the beam depth
                b         is the top flange width
                tf        is the top flange thickness
                tw        is the web thickness
                b2        is the bottom flange width
                          (optional, assumed same as b)
                tf2       is the bottom flange thickness
                          (optional, assumed same as tf)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-66
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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 tf tw (tf2)

where           d        is the beam depth
                b        is the beam width
                tf       is the thickness of the ‘top’ plate
                tw       is the thickness of the ‘side’ plates
                tf2      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 5-67
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


Channel - Type CHAN

A maximum of five dimensions can be provided: the first four are obligatory. Note that this section type
cannot be code checked in BEAMST

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. Note that this section type
cannot be code checked in BEAMST.

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 5-68
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


Tee - Type TEE

A maximum of five dimensions can be provided: the first four are obligatory. Note that this section type
cannot be code checked in BEAMST.

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. Note that
this section type cannot be processed in BEAMST.




Values are d b

where           d        is the maximum depth crossing the Z axis
                b        is the maximum breadth crossing the Y axis




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-69
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data



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.

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 5-70
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


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
END

Note


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 5-71
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

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:

                    x ′ x 2 + x ′ y2 + x ′ z 2                                = 1.0 ± .001


                    y′ x 2 + y′ y2 + y′ z 2                                   = 1.0 ± .001


                 x′x* y′x+ x′y* y′y+ x ′z* y′z                                = 0.0 ± .001




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-72
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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


                                                                                                                          y'
Hence, the direction cosines for local x’ are given by:


                   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 5-73
      ASAS (Linear) User Manual                                                                        Boundary Conditions 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 orthogonal 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 be referenced in the ELEM or TOPO
        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 5-74
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data




5.2.8       Sets Data

This data describes how selected elements are grouped together to enable collective selection in subsequent post-
processing.

                   SETS

                                                         ELEM                   elno

                   setname                               GROU                    group

                                                         setname

                   END




Parameters

SETS          : compulsory header keyword to denote the start of the sets data.

setname : name of the set (up to 8 characters).

ELEM          : keyword to denote that a list of element numbers follows.

GROU          : keyword to denote that a list of group numbers follows.

END           : compulsory keyword to denote the end of the sets data block.

Notes


1.          The SETS concept differs from the ASAS GROUP concept in that an element may appear in more
            than one set and not all elements need to be in a set.

2.          The element/group lists may include the keyword TO, allowing all entries within a range to be
            selected, or the syntax e.g. 3-8 may be used.

Example


This is an example of a SETS command.

     SETS
     BRACKET ELEM 1 5 10 11 12 TO 100
     LEVER ELEM 800 801 802 803 804
     COMPLETE BRACKET LEVER
     END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-75
       ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.9       Component Topology Data

This data describes the assembly of existing master components to form a higher level master component or
structure. It is therefore only applicable to a substructured analysis.

                   TOPO



                   MIRR                nx             ny              nz            px             py         pz



                   DCOS                x'x             x'y            x'z             y'x               y'y    y'z



                   ORIG                 ox             oy              oz


                   Mname               Aname               nodelist

                   END



Parameters

TOPO          : compulsory header keyword to denote the start of the component topology data.

MIRR          : keyword to denote that this component has been mirrored.

DCOS          : keyword to denote that this component has been rotated.

ORIG          : keyword to denote that this component has been translated.

END           : compulsory keyword to denote the end of the component topology data block.

Note


Each component to be assembled is described by one or more lines of topology data, optionally preceded by:

                mirror data (MIRR)
                direction cosine data (DCOS)
                origin data (ORIG)


If these lines are not included then the coordinate system of the existing master component being assembled is
assumed to be coincident with the global coordinate system of the current run.

Regardless of the order of the MIRR, DCOS or ORIG lines, the component is always translated and rotated
first, then mirrored and finally assembled into the current assembly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 5-76
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.9.1         TRANSLATION Data

Defines the amount of translation applied to the master component before assembly. If no ORIG line is
included, then the master component’s local coordinate system coincides with the global coordinate system of
the current analysis. Optional.

          ORIG              ox           oy           oz




Parameters

ORIG          : compulsory keyword.

ox,oy,oz : coordinates of the origin of the master component’s local coordinate system referred to the global
                coordinate system of the current analysis. (Real)

Example


This example of an ORIG command defines that the component is translated along the x-axis of the current
global system by 15.6 and along the z-axis by 27.45, without any shift in the y direction before being assembled.

   ORIG         15.6         0.0         27.45




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-77
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.9.2         ROTATION Data

Defines the amount of rotation to be applied to the master component before assembly. If no DCOS line is
included then no skewing is performed. Optional.

           DCOS             x’x          x’y          x’z           y’x           y’y           y’z




Parameters

DCOS          : compulsory keyword.

x’x,x’y,      : 6 direction cosines required to define the direction of the master component local coordinate
x’z,y’x,        system in terms of the coordinate system of the current analysis. (Real)
y’y,y’z

Example


This example of a DCOS command defines that the component is rotated through -30° about the Z-axis before
being assembled.

   DCOS         0.8660            -0.5         0.0        0.5        0.8860           0.0




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-78
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

5.2.9.3         MIRROR Data

Defines the location and orientation of the mirror used to reflect the master component before assembly. If no
MIRR line is included the component is assembled without any mirroring. Optional.

          MIRR              nx           ny           nz            px            py            pz




Parameters

MIRR          : compulsory keyword.

nx,ny,nz : direction cosines of a vector normal to the plane of the mirror. (Real)

px,py,pz : coordinates of any point in the plane of the mirror referred to the master component coordinate
                system. (Real)

Example


This example of a MIRR command describes a mirror parallel to the X-Z plane through a point (0,3,0) defined in
the coordinate axes of the current analysis, not the axis system used during the creation of the lower level
component.

   MIRR         0.0         1.0        0.0        0.0        3.0         0.0




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-79
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


                                    NO TRANSFORMATIONS                                                                MIRROR




                                                                                 MIRR 1.0 0.0 0.0 20.0 0.0 0.0


                                                              MOVE                                                    ROTATE




        ORIG 30.0 0.0 0.0                                                     DCOS 0.5 0.866 0.0 -0.866 0.5 0


                                         MOVE AND ROTATE                                                     MOVE AND MIRROR




       ORIG 30.0 0.0 0.0                                                         ORIG 30.0 0.0 0.0
       DCOS 0.5 0.866 0.0 -0.866 0.5 0                                           MIRR 1.0 0.0 0.0 20.0 0.0 0.0

                                      ROTATE AND MIRROR                                     MOVE AND ROTATE AND MIRROR




                                                                                 ORIG 30.0 0.0 0.0
       DCOS 0.5 0.866 0.0 -0.866 0.5 0                                           DCOS 0.5 0.866 0.0 -0.866 0.5 0
       MIRR 1.0 0.0 0.0 20.0 0.0 0.0                                             MIRR 1.0 0.0 0.0 20.0 0.0 0.0

                            Figure 5.1 Examples of use of the ORIG, DCOS and MIRR commands




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-80
         ASAS (Linear) User Manual                                                                     Boundary Conditions Data

5.2.9.4          TOPOLOGY Data

Defines which lower level master component is to be assembled, assigns a unique name to this assembled
component and defines the nodes to which it is attached.

           Mname                Aname                 nodelist



Parameters

Mname         : master component name of the lower level master component. (Alphanumeric, 4 characters).

Aname         : assembled component name. (Alphanumeric, 4 characters)

nodelist      : a list of node numbers for this assembled component. The node numbers must be listed in an
                 order which corresponds exactly with that order specified by the LINK data of the master
                 component when it was created. Continuation lines may be used if required. (Integer)

Notes


1.        If a component is to be skewed, mirrored or to have skewed nodes, there are restrictions on the degrees of
          freedom that can be used. See notes in Section 5.3.6.

2.        Component names must not be the same as that of any of the element names in Appendix -A (e.g. BR20,
          BEAM, etc). DCOS, MIRR, ORIG are also invalid Master Component names.

Examples


This example assembles a lower level master component WALL giving it an assembled name LEFT. It has 10
link nodes.

     WALL        LEFT                    6      16        26       27        28
     :     128    127       126      116      106




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-81
       ASAS (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

                         Link Freedoms ........ ................ ................ see Section 5.3.6

                         Master Freedoms ..... ................ ................ see Section 5.3.7

                         Rigid Constraints ..... ................ ................ see Section 5.3.8

                         Special Freedom Directions ..... ................ see Section 5.3.9

                         Gaps ....... ................ ................ ................ see Section 5.3.10

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 5.1.21).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-82
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.2       Freedom RELEASE Data

To define elements which are to have particular freedoms released from being rigidly connected to the
surrounding elements. There are two types of release. All elements may have any of their global freedoms
released. Beam elements may also have freedoms released 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.
              RELE

              (skew )           dof             userfree                 //elno//            //node//

                                                                         //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 and Appendix -E.

userfree : user-defined new freedom name. This name is used to identify the freedom during the solution
                and in the subsequent output. Omit for local releases. (Alphanumeric, up to 3 characters).

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 5-83
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

Notes

1.      The following names must not be used as user defined freedom names.

                X             R            S             U1           VYY          V22           W2
                Y             R1           T             U2           VZZ          V12           W11
                Z             R2           TH            U11          VZX          WXX           W22
                RX            RTH          UYY           U22          V1           WYY           W12
                RY            RFI          UZZ           U12          V2           WXY           Y1
                RZ            RZ1          UYZ           VXX          V11          W1            F


2.      The freedom data should be the first data in the Phase 2 data to allow the released freedom names to be
        used in the input for suppressions and prescribed displacements, etc if required.

3.      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.

4.      When beam offsets are used at an element and node which is to be released, the following conditions
        apply. For Global releases, the release is applied to the element at the node position. For Local releases,
        the release is applied to the element at the offset position in the offset local axes.

5.      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.


Global Releases only

The maximum number of unique user defined freedom names in an analysis is 21. However the same user-
defined freedom name can be used at many different nodes.

At a node where freedoms have been released, nodal loads or prescribed displacements cannot be applied using
skew systems.

Local Releases only

Local releases are only available on the following element types: BEAM, BM2D, BM3D, BMGN, BAX3, GRIL
and TUBE, including stepped elements where relevant.

The data corresponds to that specified for global releases, but if no user defined freedom name is supplied, the
freedom to be released is assumed to be in the element’s local axis system.

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.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-84
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


Displacements corresponding to the local releases are not calculated or printed.

If a skew is defined, all skewable degrees of freedom at the node, including the original and user-defined
freedoms, are rotated to the new axis system, not only those defined by dof and userfree.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-85
      ASAS (Linear) User Manual                                                                         Boundary Conditions Data


Examples


1.     In this example of global freedom releases, three beam elements with User elements number 5, 7 and 10
       meet at node 20. Elements 7 and 10 have RZ renamed as RZW and RZX 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.
                                                                                               10
             RELE
             RZ         RZW       7          20
             RZ         RZX      10          20                                                          Y
                                                                  5
             END                                                                7
                                                                                                             X




       The example above could also be defined using local freedom releases as follows. However in this case
       the rotations on elements 7 and 10 cannot be obtained.


             RELE
             RZ         7       20
             RZ 10              20
             END



2.     In this example of global freedom releases two surfaces are allowed to slide in the X direction.


                                         1             2                3                 4
         Y

                                21                22              23                24                  25

                        X                5             6                7                  8




             RELE
             /
             X     X1       5    21
             X     X1       5    22
             RP     4       1        1




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-86
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

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
be assigned a value of zero displacement for all loadcases 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 notes and
                Appendix -E. (Character)

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 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 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)

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 suppressed freedom 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 freedom releases have been defined at a node, the released freedoms would also be suppressed by use
        of the word ALL.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-87
         ASAS (Linear) User Manual                                                                     Boundary Conditions Data


3.        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.

4.        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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-88
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.4       DISPLACED Freedom Data

This data defines the nodes and freedoms which will be given a prescribed value of displacement in the load
data. See also Section 5.4.3.

              DISP

              (skew )                           dof                              //nodes//


              RP                  nrep            inode

              RRP                  nrrep          iinode

              END




Parameters

DISP          : compulsory header to define the start of the displaced freedom 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 notes and Appendix
                -E. (Character)

nodes         : list of nodes at which the degrees of freedom are to be given a fixed displacement. Continuation
                lines may be used if required. (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 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)

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 displaced freedom data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-89
      ASAS (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 displaced.

2.      If freedom releases have been defined at a node, the released freedoms would also be displaced freedoms
        by use of the word ALL.

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 displacement is defined in
        the loading data. See Section 5.4.3.

5.      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


An example to define nodes 126 and 128 as having displaced freedoms in the y direction.

     DISP
     Y   126          128
     END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-90
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.5       CONSTRAINT Equation Data

This data defines degrees of freedom on the structure whose displacements are linearly dependent on one or
more other degrees of freedom in the structure.

              CONS

              (skew )          ddof         //dnode//                factor        dof        //nodes//


              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 notes and Appendix -E.

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 notes and Appendix -E.

node          : independent node number. (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 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.

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 5-91
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data

END           : compulsory keyword to define the end of the constraint equation 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 admissible 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.      The program defaults to an out-of-core solution when constraints are present and the high speed frontal
        solver is not in use. If there are no singularities present before the application of the constraints, which
        are intended to be removed by the constraints, then the solution may be forced in-core. This is done by
        using Option ISOL. Option ISOL is automatically set with the high speed frontal solver. Constraints
        may be able to remove local singularities in this case but this should be treated with caution.

        On rare occasions, the in-core solution may fail if there is a singularity in the model before applying the
        constraints. Since this solution depends on the order in which the elements are processed, option BAND
        will therefore have an effect because it will re-arrange the element processing order.

        If rigid beams/links are used to stitch two parts together, the problem can be resolved by specifying
        dummy beams/FLA2s at the positions where the rigid elements are used.

7.      If the solution is forced in-core with constraints then 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).

8.      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 neighboring point which has




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-92
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


       stiffness. A component may be assembled in a higher level assembly in such a way that it may be left
       with an unrestrained rigid body freedom. This too could be removed by the use of constraint equations.

       However, constraints cannot be used to remove a rigid body motion from a whole structure or assembly
       which is due to a lack of overall support. This can only be done with suppressed or displaced nodes.


9.     The forces associated with the constraint systems are printed out as reactions during Stage 17
       (Displacement printing). For an out-of-core solution only the force on the dependent freedom is
       calculated. However, with an in-core solution both dependent and independent forces are calculated.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-93
       ASAS (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
                                                                                                                             25
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                           88                 89
of rotation. (Some types of joint may require the constraining of one                                                        24
or two of the rotational freedoms.)

   CONS
   X       89           1.0       X        24                                                                                23
   Y       89           1.0       Y        24
   Z       89           1.0       Z        24
   END

A Rigid Edge
                                                                                                        4                1
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                                     5                2
related by the equation:                                                                                                       0.2

X2 = 0.2 = (X1 + X3) /2                                                                                 6                3

giving:

X2 = 0.2 (a prescribed displacement)

X3 = 0.4 - X1

   CONS
   X       3      0.4         -1.0              X     1
   END

This example is only valid using an in-core solution (see Note 7 above).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                        Page 5-94
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


Construction Mismatch

This example shows how a gap in the construction of a structure
which causes built in stresses as the two parts are pulled together can
                                                                                              2          4
be modelled.
                                                                                                             0.1
The following constraint equation will cause nodes 2 and 4 to be
coincident in the x-direction after an initial gap of 0.1 units. (Note,                       1          3
this will only work for an in-core solution.)

   CONS
   X       2      .1        1.0        X      4




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-95
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.6       LINK Freedom Data

Defines the nodes and freedoms which are to be used as link freedoms for the master component being created
by the current analysis. Only applicable to component creation analysis.

                LINK

                (skew )                     dof                        //nodes//


                RP               nrep             inode

                RRP              nrrep            iinode

                END



Parameters

LINK          : compulsory header to define the start of the link freedom data.

skew          : optional skew system identifier. See Section 5.2.7. (Integer)

dof           : names of the freedoms to be used as link freedoms. Up to 5 freedoms may be defined. See notes
                and Appendix -E.

nodes         : list of nodes at which the degrees of freedom are to be used as links at a higher level assembly.
                Continuation lines may be used if required. (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 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)

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 link freedom data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-96
         ASAS (Linear) User Manual                                                                     Boundary Conditions Data

Notes


1.        The order in which the nodes are generated by this data defines the order in which the nodes in the
          component topology must be defined whenever this master component is assembled at a higher level.
          The first occurrence of the node number determines the link node order for use at the next level assembly.

2.        The word ALL may be used to indicate that all freedoms at the given node or nodes are to be links. This
          may not be used with stiffness input runs, the actual freedom names must be given.

3.        If Freedom Releases are being used, a released freedom, i.e. the user generated freedom name, must not
          be used as a LINK freedom either explicitly or implicitly by using the ALL command.

4.        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.

5.        Skewed link freedoms must be used with care if they are to be connected to other components or elements
          at a higher level. In order that the stiffness matrix is correctly assembled the same skew system must be
          applied to all nodes of connecting components. In general it is not recommended that elements are
          connected directly to skewed component nodes.

6.        If the Master Component being created is to be skewed, mirrored or to have skewed nodes in a higher
          level assembly, then only the following combinations of freedoms at a node are valid. If other
          combinations of freedoms are used at a link node, that node cannot be skewed in a higher level assembly.

          X Y                           RX RY                  X Y RZ
          X Z                           RX RZ                  Z RX RY
          Y Z                           RY RZ                  Z R
          X Y Z                         RX RY RZ               X Y Z RX RY RZ
                                                               X Y Z R1 R2

Examples


A simple example of LINK data

     LINK
     X       1        2        3        4        5
     X Y         12       13       24       27
     RX           9       10       14       28       29   30
     /
     ALL          6
     RP          14       51
     END

The order of the link nodes for use in a higher level assembly is as follows

          1-5 12 13 24 27 9 10 14 28-30 6 57 108 159
          210 261 312 363 414 465 516 567 618 669




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-97
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.7       MASTER Freedoms Data

This data defines the nodes and freedoms which will be retained as dynamic degrees of freedom and used to
calculate the eigenvalues and eigenvectors. Only required for natural frequency analysis.

         MAST

         (skew )                     dof                        //nodes//


         RP               nrep             inode

         RRP              nrrep             iinode

         END



Parameters

MAST          : compulsory header to define the start of the master freedom data

skew          : optional skew system identifier. See Section 5.2.7. (Integer)

dof           : names of the freedoms to be used as masters. Up to 5 freedoms may be defined. See notes and
                Appendix -E. (Character)

nodes         : list of nodes at which the degrees of freedom are to be used as masters. Continuation lines may be
                used if required. (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 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)

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 master freedom data.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-98
        ASAS (Linear) User Manual                                                                      Boundary Conditions Data


Notes


(i)         The word ALL may be used to indicate that all freedoms at the given node or nodes are to be used as
            Masters.

(ii)        If freedom releases have been defined at a node, the released freedoms would also become a master by
            use of the word ALL.

(iii)       If a skew is defined, all skewable degrees of freedom are rotated to the new axis system, not only those
            defined by dof.

(iv)        The master freedom data must not be used for a SPIT analysis since all unsuppressed degrees of freedom
            are used as master freedoms.

(v)         If the master freedom data is omitted for a natural frequency analysis all unsuppressed degrees of freedom
            are used as master freedoms.

Example


A simple example of master freedom data.

       MAST
       X        1     2      3      4        5
       X Y     12    13     24     27
       R2        9   10     14     28      29     30
       /
       ALL      6
       RP      14    51
       END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-99
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data

5.3.8       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.

          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: RLNK, RBM2, RBM3, RLSY, RBSY

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 5-100
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


Note


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


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 coordinates               X,Y,Z         X,Y           X,Y,Z           X,Y,Z           X,Y,Z          X,Y,Z          X,Y,Z



Degrees of Freedom              X,Y,Z       X,Y,RZ          X,Y,Z           X,Y,Z           X,Y,Z          X,Y,Z          X,Y,Z
linked by the element                                    RX,RY,RZ                        RX,RY,RZ            for            for
(Minimum)                                                                                                 dependent      dependent


                                                                                                           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 5-101
      ASAS (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.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-102
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


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.     When dummy elements have been used (see Note 1) an element group number of 9999 can be specified
       in the element topology data to suppress the output of results. Otherwise misleading forces and stresses
       (which must be zero) will be printed for the appropriate element type.

3.     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.

4.     An independent freedom can be suppressed, displaced, linked or constrained and can be specified as a
       master freedom for dynamics analysis; dependent freedoms cannot.

5.     For an in-core solution the structure without the rigid elements should ideally be non-singular although
       this is not an essential requirement. See notes in Section 5.3.5.

6.     In an in-core solution there are no limitations on the number of rigid elements joining at a node or the
       number of occurrences of a dependent node.

7.     If the out-of-core solution is used there is a restriction on the number of times a node can be used as a
       dependent node. This number is different if the rigid elements/systems are co-planar or if as well as being
       co-planar they also lie in a straight line.


                Element                 No of dofs               No of                  If Co-planar         If Co-planar
                                                               Times Used                                      and In-line

               RLNK                          3                       3                          2                  1

               RLNK                          6                       3                          2                  1

               RBM2                          3                                                  1                  1

               RBM3                          6                       1                          1                  1

               RLSY                          3                       3                          2                  1

               RBSY                          6                       1                          1                  1




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 5-103
           ASAS (Linear) User Manual                                                                   Boundary Conditions Data

5.3.9          SPECIAL Freedom Direction Data

To define positive directions for special freedoms. Required only for JOB STIF.

                SPEC

                node           x            y            z

                END




Parameters

SPEC             : compulsory header to denote start of the special freedom direction data.

node             : node number of the node. (Integer, 1-5 digits)

x,y,z            : 3 values giving the components of the direction vector for positive direction of any special
                   freedoms on this node. (Real)

END              : compulsory keyword to denote the end of the special freedom direction data block.

Example


       SPEC
       1     0.0    2.0       0.0
       7 3.5        1.0 -2.7
       END

Notes


(i)         This data block is only valid in a direct stiffness input component creation (STIF) job, and is necessary if
            any link freedoms given in the LINK data (see Section 5.3.6) referred to special freedom types (see
            Section 2.7.1).

(ii)        The direction vector values may be given as direction cosines if desired but this is not essential and no
            checks will be performed on their values.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-104
       ASAS (Linear) User Manual                                                                       Boundary Conditions Data


5.3.10      GAP Data

This data defines the node numbers and initial gaps for any pairs of nodes on the structure to be linked by Gaps.

             GAPS

             node1             node2             (gap0)             (skew )


             RP               nrep               inode1             inode2

             RRP              nrrep              iinode1            iinode2

             END



Parameters

GAPS          : compulsory header to define the start of the gap data.

node1         : node number of first gap node. (Integer)

node2         : node number of second gap node. (Integer)

gap0          : initial gap between node1 and node2. (Real). Optional. See Note 1

skew          : skew system identifier. (Integer). Optional. See Notes 2, 3 and 4.

RP            : keyword to indicate data generation from the previous / symbol.

nrep          : the number of times the data is to be generated. (Integer)

inode1        : node number increment to be added to node1 each time the data is generated by the RP command.
                (Integer)

inode2        : node number increment to be added to node2 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)

iinode1       : node number increment to be added to node1 each time the data is generated by the RRP
                command. (Integer)

iinode2       : node number increment to be added to node2 each time the data is generated by the RRP
                command. (Integer)

END           : compulsory keyword to define the end of the gap data.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-105
      ASAS (Linear) User Manual                                                                        Boundary Conditions Data


Notes


1.      If the initial gap (gap0) is omitted then the initial gap will be taken as the distance between node1 and
        node2.

2.      If the skew integer (skew) is omitted then a skew system will be generated by the program as follows:

        Skew x will be taken as the direction from node1 to node2, skew z will lie in the global X-Y plane with
        skew y positive on the positive side of that plane.

        If skew y is in the global X-Y plane then skew y is taken to lie in the global Y direction. If node1 and
        node2 are coincident then the skew system will be taken to be the same as the global axis system.


3.      Program-generated skew systems will be numbered G1...Gn where n is the number of program-generated
        skew systems.

4.      If a skew system integer is specified then an initial gap (gap0) must also be specified.

5.      The gap status is determined by the relative displacement of node1 to node2 in the gap direction (skew
        x). For open gaps, if the displacement of node1 relative to node2 in the gap direction is greater than the
        specified gap then the gap is deemed to have closed. For closed gaps a tensile force between the nodes
        results in the gap opening.

6.      All freedoms at node1 must be truly free and not suppressed, displaced or otherwise restrained. If any
        freedoms at node 2 are to be suppressed or displaced then the gap data must include a user-defined skew
        sytem. this skew system must also be used in the corresponding suppression or displacement data.

7.      For the efficient solution of a problem using gaps, it is important that some care is taken in defining the
        gap data. In particular it is important that gaps are defined only in places where the gap is likely to close
        for one or more of the loadcases. Structures with large numbers of open gaps are likely to require
        relatively large amounts of computer time to solve.

8.      Because the solution of a Gap run is an iterative procedure, Component Analysis should be used to create
        a final structure run as simple as possible whilst retaining all the gaps.

9.      Because a job using gaps requires an incore solution of a structure with constraint equations, there must
        be no singularities present on the structure prior to application of the gaps and any other user-defined
        constraint equations.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-106
ASAS (Linear) User Manual                                                                                  Loading Data



5.4     LOAD 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......... ................ 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
                            a) nodal temperature ............. ................ see Section 5.4.7.1
                            b) element temperature ......... ................ see Section 5.4.7.2

                          Face temperature loads ............. ................ see Section 5.4.8
                            a) nodal face temperature ...... ................ see Section 5.4.8.1
                            b) element face temperature .. ................ see Section 5.4.8.2

                          Body Force loads..... ................ ................ see Section 5.4.9

                          Centrifugal loads ..... ................ ................ see Section 5.4.10

                          Angular Acceleration loads ...... ................ see Section 5.4.11

                          Component loads ..... ................ ................ see Section 5.4.12

                          Tank loads ............... ................ ................ see Section 5.4.13




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-107
ASAS (Linear) User Manual                                                                                           Loading Data


5.4.1          UNITS Command

If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.21), 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.
             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 5.1.21.1.

Example


Data                                                                              Operational Units          Notes

SYSTEM DATA AREA 50000
PROJECT ASAS
FILES ASAS
JOB NEW LINE
UNITS NEWTON METRE                                                                Newtons, metres,           Global definition
END                                                                               centigrade
.
.
.
LOAD 2
CASE 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




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-108
ASAS (Linear) User Manual                                                                                         Loading Data


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
Y     BL1         1.5       1.6          5   6                                                              unit to KN
END
*
CASE 2 ’DISTRIBUTED LOAD ONLY’
DISTRIBU                                                                         Newtons, metres,           New loadcase reverts
Z     BL5       1200.0           5       6                                       radians                    units to global
END
STOP




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-109
ASAS (Linear) User Manual                                                                                Loading Data


5.4.2       LOADING Data

The loading data consists of a header keyword, followed by the data for each loadcase. The data for each
loadcase begins with a loadcase header followed by the data for each type of loading.
                  LOAD                (ncase)

                  CASE                case             title

                  loadtype

                  data

                  END




Parameters

LOAD          : compulsory header keyword to denote the start of the loading data.

ncase         : number of loadcases in the current analysis. Optional. (Integer, 1-9999). If supplied, ncase
                 must equal the number of loadcases supplied.

CASE          : compulsory keyword to denote the start of the next loadcase.

case          : user loadcase number. Every loadcase number must be unique but need not form a sequence with
                 the other loadcase numbers. (Integer, 1-9999)

title         : loadcase title. (Alphanumeric, 40 characters)

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.

Example

An example of load data consisting of two separate loadcases.
                          LOAD
                          CASE 100 NODAL LOADS AND PRESSURE
                          NODAL LO
                          X 1055.6 652
                          RZ 3.64E5 652
                          END
                          PRESSURE
                          /
                          U 9.63 426 456 476
                          RP 10 50
                          END
                          CASE 200 SELF WEIGHT
                          BODY FOR
                          0.0 0.0 -981.0
                          END
                          STOP



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-110
ASAS (Linear) User Manual                                                                                Loading Data


5.4.3       NODAL LOADS Data

To define the application of nodal loads to the structure. The loads may be forces or moments.

               NODAL LO

               (skew )           dof             load               //nodelist//


               RP              nrep              inode

               RRP             nrrep             iinode

               END



Parameters

NODAL LO          : compulsory header to denote the start of nodal load data.

skew              : skew system integer. Optional. (Integer)

dof               : freedom name. See notes and Appendix -E.

load              : value of nodal load. (Real)

nodelist          : list of the node numbers to which the load 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)

inode             : node 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)

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 loadcase.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-111
ASAS (Linear) User Manual                                                                                   Loading Data



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, in the node local axis system if a skew system
           has been applied to the node in the Boundary Conditions data.

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 Conditions 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 nodal loads are applied to the same node and freedom more than once for the same loadcase, the loads
           are additive.

Example


An example of a single loadcase 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
      CASE   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 5-112
ASAS (Linear) User Manual                                                                                   Loading Data


5.4.4          PRESCRIBED Displacements Data

To define the values of displacements to be applied in this loadcase to those freedoms declared as displaced
freedoms in the Boundary Conditions Data (see Section 5.3.4).

                  PRESCRIB

                  (skew )           dof             displ              //nodelist//


                  RP               nrep             inode

                  RRP              nrrep            iinode

                  END



Parameters

PRESCRIB             : compulsory header to denote the start of prescribed displacement data.

skew                   : skew system integer. Optional. (Integer)

dof                  : freedom name. See notes and Appendix -E.

displ                : value of prescribed displacement. For rotational degrees of freedom the value is given in
                        radians. (Real)

nodelist             : list of the node numbers which are to be displaced. (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 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)

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 displacement data.

Notes


1.         All freedoms used in the prescribed displacements data must have been defined in the displaced freedoms
           data (see Section 5.3.4).




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-113
ASAS (Linear) User Manual                                                                                   Loading Data


2.         In any loadcase, a prescribed displacement is set to zero if it is not assigned a value and in such cases a
           suppression is assumed for the freedom.

3.         If a skew system has been defined in the Boundary Conditions Data for a displaced freedom node, the
           same skew integer must appear in prescribed displacement load data for that node. However unlike
           nodal loads the two skew systems are not additive.

Examples


An example of prescribed displacements for two loadcases. 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
      CASE        1    EQUAL DISPLACEMENT OF 5mm
      PRESCRIB
      Z 5.0 10
      Z 5.0           15
      END
      CASE        2    NODE 10 DISPLACED, NODE 15 FIXED
      PRESCRIB
      Z 5.0 10
      Z 0.0           15
      END
      STOP




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-114
ASAS (Linear) User Manual                                                                                  Loading Data


5.4.5         PRESSURE Load Data

To define uniform pressure or varying pressure applied to the faces of panel or solid elements.




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.
                       For Brick elements, only global directions may be specified

U                   : keyword to define data as uniform pressure.

F                   : keyword to define data as face definition.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-115
ASAS (Linear) User Manual                                                                                  Loading Data


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.

Note


(i)       The sign convention for pressure in the default direction on each element type is defined in the element
          description sheets in Appendix -A.

(ii)      Local pressure load direction is only permitted for shell elements.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-116
ASAS (Linear) User Manual                                                                                  Loading Data


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                     press                          //nodes//


               RP                    nrep                             inode

               RRP                   nrrep                            iinode

               FIN



Parameters

U               : keyword to define uniform pressure data.

press           : value of the uniform pressure. (Real)

nodes           : the element face 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 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 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)

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 pressure data block.

Notes


(i)       A face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For TRX6, THX6,
          QUX8 and QHX8 a face is defined by the 3 nodes forming the loaded edge. For TRX3, THX3, QHX4
          and QUX4 a face is defined by the two nodes forming the loaded edge and any other node on the element.
          ASH2 or AHH2 are defined by their 2 nodes.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-117
ASAS (Linear) User Manual                                                                                Loading Data


(ii)    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 element in the local element axes.

(iii)   For coincident 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 element number. The direction of the pressure load will be
        determined by this element’s local axis system.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-118
ASAS (Linear) User Manual                                                                                  Loading Data


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 linearly 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 face to which the non-uniform pressure is to be applied. A face is defined by up to 3
                   corner nodes. See notes. (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 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)

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 5-119
ASAS (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                      press                         //nodes//

                RP                     nrep                            inode

                RRP                    nrrep                           iinode

                FIN




Parameters
P          : keyword to denote nodal pressure data

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 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 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)

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 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. Corner nodes
           with undefined pressure are assumed to have zero pressure. Mid-side nodes with undefined pressure are
           interpolated from adjacent corner node values. 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.
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, THX6,
           QUX8 and QHX8 elements, a face is defined by the 3 nodes forming the loaded edge. For TRX3, THX3,
           QUX4 and QHX4 elements, a face is defined by the 2 nodes forming the loaded edge on any other node
           on the element. ASH2 and AHH2 elements are defined by their 2 nodes.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-120
ASAS (Linear) User Manual                                                                                        Loading Data


4.         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 element in the local element axes.

Examples

(i)        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

(ii)       Non-uniform Pressure on one face. Mid-side nodes 2 and 4 are undefined and therefore will be given
           values of 7.5 and 11.0 respectively by interpolation.
                                                                                                   5
                                                                         6
                                              7                                          p = 12
                                                                     p = 10
                                                  p=5


                                                                                               4
                                          8       p=5



                                                  p=5                         p = 10
                                              1                  2                   3

                    PRESSURE
                    F 1 5            7
                    FIN
                    P   5.0          1    7       8
                    P 10.0           3    6
                    P 12.0           5
                    END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-121
ASAS (Linear) User Manual                                                                                         Loading Data


(iii)   Example of a Complete Pressure Data block 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
                 * TWO FACES WITH UNIFORM PRESSURE=20.0
                 U 20.0 1 2      8
                 U 20.0 7 8 14
                 FIN
                 * GENERATE 6 FACES FOR NON-UNIFORM PRESSURE
                 //
                 /
                 F   2 3 9
                 RP 2 6
                 RRP 3 1
                 FIN
                 * APPLY NODAL PRESSURES TO THE FACES ABOVE
                 P 20.0 2     8 14
                 P 10.0 3     9 15 4 10 16
                 P 15.0 5 11 17
                 FIN
                 /
                 * TWO FACES WITH UNIFORM PRESSURE=5.0
                 U   5.0 5    6 12
                 RP 2 6
                 END




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-122
ASAS (Linear) User Manual                                                                                Loading Data


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 loadcase.

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

ML3      -       Varying transverse shear load on the edge of membrane and shell elements

TB1      -       Intermediate normal point load on TRB3

CB1       -      Varying distributed load on GCB3, TCBM




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-123
ASAS (Linear) User Manual                                                                                       Loading Data


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)

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 5-124
ASAS (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
           DISTRIBU
           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 5-125
ASAS (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.
                         DISTRIBUTED LOAD PATTERNS BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
                                       on BEAM, BM2D, BM3D, GRIL, 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 5-126
ASAS (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 5-127
ASAS (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”
   BM2D              Y”                       RZ”                              1                     2

   BM3D              Y”      Z”     RY”       RZ”                    Y”
                                                                                                          Bending
   GRIL                      Z”     RY”
                                                                           1                                   X”
   TUBE              Y”      Z”     RY”       RZ”                                                    2




Distributed Load Pattern BL2 - Linearly varying axial load or torque

   Element         Valid freedom directions
                                                                     Y”

   BEAM              X”      RX”                                                                     Axial
   BM2D              X”                                                                                        X”
                                                                           1                        2
   BM3D              X”      RX”                                     Y”
   GRIL                      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 5-128
ASAS (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”
   GRIL                       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 5-129
ASAS (Linear) User Manual                                                                                                Loading Data


Notes


1.         The nodes must be listed in the same order as the element topology data.

2.         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
                                                                                   Y”
                                                                                                                  Normal
      Element          Valid freedom directions                                                                             X”
                                                                                        1                     2
                                                                                   Y”
      BEAM               X”      Y”     Z”      RX”      RY”       RZ”
                                                                                                                  Axial
      BM2D               X”      Y”                                RZ”                                                      X”
                                                                                        1                     2
      BM3D               X”      Y”     Z”      RX”      RY”       RZ”
                                                                                   Y”
      GRIL                              Z”      RX”      RY”                                                      Bending
      TUBE               X”      Y”     Z”      RX”      RY”       RZ”                                                      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)

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




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                       Page 5-130
ASAS (Linear) User Manual                                                                                              Loading Data


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
                                                                              Y”
   Element          Valid freedom directions                                                                  Normal
                                                                                                                        X”
                                                                                   1                         2
   BEAM               X”      Y”     Z”      RX”      RY”       RZ”           Y”
   BM2D               X”      Y”                                RZ”                                           Axial
   BM3D               X”      Y”     Z”      RX”      RY”       RZ”                                                     X”
                                                                                   1                         2
   GRIL                              Z”      RX”      RY”                     Y”

   TUBE               X”      Y”     Z”      RX”      RY”       RZ”                                           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.

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




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      Page 5-131
ASAS (Linear) User Manual                                                                                               Loading Data


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

   Element          Valid freedom directions                                     Y”
                                                                                                                     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”
   GRIL                              Z”      RX”      RY”                             1                          2
                                                                                 Y”
   TUBE               X”      Y”     Z”      RX”      RY”       RZ”                                                  Bending
                                                                                                                               X”
                                                                                      1                          2
                                                                                 Y”
                                                                                                                     Torsion
                                                                                                                               X”
                                                                                      1                          2


Data Line
                                                                                                          //node1//          //node2//
       dof         BL6          force1           force2          dist1          dist2
                                                                                                          ELEM               //elno//



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)




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                         Page 5-132
ASAS (Linear) User Manual                                                                                            Loading Data


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”
   Element          Valid freedom directions                                                                     Normal
                                                                                                                           X”
                                                                                         1                       2
   BEAM               X”      Y”     Z”      RX”      RY”       RZ”
                                                                                    Y”
   BM2D               X”      Y”                                RZ”                                              Axial
   BM3D               X”      Y”     Z”      RX”      RY”       RZ”                                                        X”
                                                                                         1                       2
   GRIL                              Z”      RX”      RY”                           Y”
   TUBE               X”      Y”     Z”      RX”      RY”       RZ”                                              Bending
                                                                                                                           X”
                                                                                         1                       2
                                                                                    Y”
                                                                                                                 Torsion
                                                                                                                           X”
                                                                                         1                       2


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)




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page 5-133
ASAS (Linear) User Manual                                                                                              Loading Data


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
                                                                            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
   GRIL                              Z”      RX”      RY”                   Y”
                                                                                                              Bending
   TUBE               X”      Y”     Z”      RX”      RY”       RZ”
                                                                               1                                      X”
                                                                                                                  2
                                                                            Y”
                                                                                                              Torsion

                                                                                 1                                    X”
                                                                                                                  2


Data Line
                                                                    //node1//          //node2//
         dof              BL8               force
                                                                     ELEM              //elno//




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 5-134
ASAS (Linear) User Manual                                                                                Loading Data


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




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-135
ASAS (Linear) User Manual                                                                                         Loading Data


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.

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, GRIL, 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 5-136
ASAS (Linear) User Manual                                                                                    Loading Data


                               DISTRIBUTED LOAD PATTERNS GL1, GP1, GL4, GP4, GL5, GL6, GP6,
                                       GL7, and GP7 on BEAM, BM2D, BM3D, GRIL, 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 5-137
ASAS (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




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-138
ASAS (Linear) User Manual                                                                                          Loading Data


5.4.6.2.1       GL1 and GP1 Load Patterns

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



                                                                                               1             GL1 - Global Z
                                                                                                                               X”
                                                                                          Y”                          2
   Element         Valid freedom directions

   BEAM              X       Y      Z       RX       RY        RZ             X                1
   BM2D              X       Y                                 RZ                                             GP1 - Global X
                                                                                     Z
   BM3D              X       Y      Z       RX       RY        RZ
   GRIL                             Z       RX       RY                                                                        X”
                                                                                          Y”                          2
   TUBE              X       Y      Z       RX       RY        RZ

                                                                                               1
                                                                                                              GP1 - Global Z

                                                                                                                               X”
                                                                                          Y”                          2



                                                                                               1
Data Line
                          GL1                                                            //node1//       //node2//
         dof                              force1                force2
                          GP1                                                            ELEM            //elno//

Parameters

dof          : global freedom code for direction of loading. See list above.

GL1          : load pattern types.
GP1
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 5-139
ASAS (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




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-140
ASAS (Linear) User Manual                                                                                       Loading Data


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”
                                                                                           Y”
                                                                                                                  2
   Element         Valid freedom directions
                                                                                                 1                GL4 - Global RZ
   BEAM              X     Y    Z     RX      RY     RZ                                                                  X”
   BM2D              X     Y                         RZ                                     Y”                    2
   BM3D              X     Y    Z     RX      RY     RZ                   X
                                                                                                 1
   GRIL                         Z     RX      RY                                                                  GP4 - Global X
                                                                                 Z                                       X”
   TUBE              X     Y    Z     RX      RY     RZ                                    Y”
                                                                                                                  2

                                                                                                 1                GP4 - Global RZ
                                                                                                                         X”
                                                                                            Y”                     2

                                                                                                 1
Data Line

                          GL4                                                                        //node1//   //node2//
         dof                               force              dist1            dist2
                          GP4                                                                        ELEM        //elno//



Parameters

dof          : local freedom code for direction of loading. See list above.

GL4          : load pattern type.

GP4

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        : 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 5-141
ASAS (Linear) User Manual                                                                                Loading Data


Note

The nodes must be listed in the same order as the element topology data.

Example

See Section 5.4.6.2




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-142
ASAS (Linear) User Manual                                                                                        Loading Data


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
   BEAM               X     Y    Z     RX      RY     RZ
                                                                                             1                   Global Z
   BM2D               X     Y                         RZ
                                                                                                                         X”
   BM3D               X     Y    Z     RX      RY     RZ
                                                                                       Y”                        2
   GRIL                          Z     RX      RY                   X
   TUBE               X     Y    Z     RX      RY     RZ                                     1
                                                                                                                 Global RY
                                                                            Z                                            X”
                                                                                      Y”
                                                                                                                 2

                                                                                             1                   Global RZ
                                                                                                                         X”
                                                                                       Y”                        2

                                                                                             1

Data Line
                                                                                   //node1//         //node2//
         dof               GL5              force             dist
                                                                                   ELEM             //elno//


Parameters

dof           : local freedom code for direction of loading. See list above.

GL5           : 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 5-1365.4.6.2




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-143
ASAS (Linear) User Manual                                                                                      Loading Data


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
                                                                                                                      GL6 - Global X
                                  over part of the element                                                                   X”
                                                                                             Y”
                                                                                                                      2
   Element         Valid freedom directions
                                                                                                    1                 GL6 - Global RY
   BEAM              X     Y    Z     RX      RY     RZ                                                                      X”

   BM2D              X     Y                         RZ                                       Y”                      2
                                                                           X
   BM3D              X     Y    Z     RX      RY     RZ                                             1
                                                                                                                      GP6 - Global X
   GRIL                         Z     RX      RY                                   Z                                         X”
                                                                                             Y”
   TUBE              X     Y    Z     RX      RY     RZ                                                               2

                                                                                                    1                 GP6 - Global RY
                                                                                                                             X”
                                                                                               Y”                     2


Data Line                                                                                           1

                 GL6                                                                                //node1//   //node2//
      dof                        force1         force2          dist1          dist2
                GP6                                                                                 ELEM        //elno//



Parameters

dof          : local freedom code for direction of loading. See above list.

GL6          : load pattern type.
GP6

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)




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-144
ASAS (Linear) User Manual                                                                                Loading Data


Note

The nodes must be listed in the same order as the element topology data.

Example

See Section 5.4.6.2




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-145
ASAS (Linear) User Manual                                                                                           Loading Data


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

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
   BEAM              X     Y    Z     RX      RY     RZ                                    1                    GL7 - Global RY
   BM2D              X     Y                         RZ                                                                X”
                                                                                    Y”
   BM3D              X     Y    Z     RX      RY     RZ                                                         2
                                                                  X
   GRIL                         Z     RX      RY
                                                                                          1
   TUBE              X     Y    Z     RX      RY     RZ                                                         GP7 - Global X
                                                                          Z                                            X”
                                                                                    Y”
                                                                                                                2

                                                                                           1                    GP7 - Global RY
                                                                                                                       X”
                                                                                    Y”
                                                                                                                2

Data Line                                                                                  1
                GL7                                                                                      //node1//     //node2//
      dof                      force1        force2        force3        dist1       dist2
               GP7                                                                                       ELEM          //elno//


Parameters

dof          : local freedom code for direction of loading. See list above.

GL7          : load pattern type.
GP7

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)




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 5-146
ASAS (Linear) User Manual                                                                                Loading Data


Note


The nodes must be listed in the same order as the element topology data.

Example


See Section 5.4.6.2




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-147
ASAS (Linear) User Manual                                                                                Loading Data


5.4.6.3         Panel Edge Distributed Loads

Distributed Load Patterns ML1, ML2 and ML3 can be applied on element types CTM6, GCS6, GCS8, QUM4,
QUM8, QUS4, SLB8, SQM4, TCS6, TCS8, TRB3, TRM3, TRM6.

Note - ML1 and ML2 not available on SLB8 and TRB3.



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 CTM6,
QUM8, TCS6, TCS8, TRM6, GCS6, GCS8, a quadratic variation of the load is allowed, so linear variation and
uniform loading are also acceptable. For QUS4, QUM4, SQM4, 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 CTM6, QUM8, TCS6, TCS8, TRM6,
GCS6, GCS8, a quadratic variation of load is allowed, so linear variation and uniform loading are also
acceptable. For QUM4, TRM3, SQM4, 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 5-148
ASAS (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 CTM6, GCS6, GCS8, QUM8, SLB8, TCS6, TCS8 and TRM6 a quadratic variation of load is allowed, so
linear variation and uniform loading are also acceptable. For QUM4, QUS4, SQM4, TRB3 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

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)

force3        : value of the load/unit length at the mid-side node for CTM6, GCS6, GCS8, QUM8, SLB8, TCS6,
                 TCS8, TRM6. This mid-side value must be calculated and given. (Real)




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-149
ASAS (Linear) User Manual                                                                                   Loading Data


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)

Note

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




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




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-150
ASAS (Linear) User Manual                                                                                           Loading Data


5.4.6.4         Panel Point Loads



Distributed Load Pattern TB1 on Element TRB3 - Intermediate normal point load

The loads are always in the global Z direction, normal to the global XY plane in which the element lies. A +ve
load acts in the direction of the +ve global Z axis.




Data Line

                                                                                        //nodes//
        dof          TB1           force          dist1           dist2
                                                                                        ELEM              //elno//


Parameters

dof           : freedom code for the direction of loading. Only Z is available.

TB1           : load pattern type.

force         : value of the point load. (Real)

dist1         : global X coordinate of the load point. (Real)

dist2         : global Y coordinate of the load point. (Real)

nodes         : node number list. (Integer)

ELEM          : keyword to indicate following data is an element number.

elno          : element number to define the loaded element. (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 5-151
ASAS (Linear) User Manual                                                                               Loading Data



Example of Distributed Load Data for Pattern TB1




Data

  DISTRIBU
  Z       TB1        -500.0           20.0         27.0         18        19       94
  Z       TB1        -500.0           30.0         20.0         18        19       94
  Z       TB1        -500.0           60.0         27.0         19        20       95
  Z   TB1            -500.0           70.0         20.0         19        20       95
  END




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-152
ASAS (Linear) User Manual                                                                                       Loading Data



5.4.6.5         Curved Beam Distributed Loads



Distributed Load Pattern CB1 on elements GCB3 and TCBM

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.

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         : node number 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 5-153
ASAS (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




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-154
ASAS (Linear) User Manual                                                                                             Loading Data


5.4.7          TEMPERATURE LOAD Data


5.4.7.1            Nodal Temperature

To define the temperature values at node points throughout the structure.
                TEMPERAT


                      GROU                   grpno


                                             temp                           //nodes//


                      RP                     nrep                  inode

                      RRP                    nrrep                 iinode
                      GRES                   sname                 (lc)       isub         (node1)           (node2)

                      END




Parameters
TEMPERAT : compulsory header 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 data generation 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 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)

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 5-155
ASAS (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.         TEMP option should be used on the OPTIONS command.

2.         Unspecified corner node temperatures are assumed to be zero.

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 are additive at common nodes.

5.         Nodal and element temperature data must not be present in the same loadcase. The program LOCO can
           be used to produce a combined loadcase if required.

6.         The following points concern 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 in 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.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-156
ASAS (Linear) User Manual                                                                                  Loading Data


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.
                    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.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-157
ASAS (Linear) User Manual                                                                                  Loading Data


5.4.7.3            UNIFORM Element Temperature Data

To define values of the uniform temperature and the elements to which they apply.


               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.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-158
ASAS (Linear) User Manual                                                                                  Loading Data


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.



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 5-159
ASAS (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 5-160
ASAS (Linear) User Manual                                                                                   Loading Data


3.         TEMP option should be used on the OPTIONS command.

4.         Unspecified corner node temperatures are assumed to be zero.

5.         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.

6.         Loading due to element temperature and element face temperature are additive.

7.         If temperature is defined more than once on an element the loadings will be additive.

8.         Nodal and element temperature data must not be present in the same loadcase.

Example


In this example 5 BEAM 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°.




      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
      T       50.0         5




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-161
ASAS (Linear) User Manual                                                                                Loading Data


     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.
                TEMPERAT

                  GROU                      grpno


                temp                             //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 temperature data applies to a single group.

grpno             : group number to which 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)

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)




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-162
ASAS (Linear) User Manual                                                                                   Loading Data


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, care must be taken to
           ensure the consistent use of local axes on adjacent elements.

3.         If necessary, because of the complexity of the modelling, adjacent elements can be separated by using
           different node numbers for the application of face temperatures and subsequently joined together using
           constraint equations. Alternatively element face temperatures may be used (see Section 5.4.8.2).

4.         Unspecified values for element corner nodes are assumed to be zero. 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.

5.         Face temperature and temperature loading is additive at common nodes.

6.         Nodal and element face temperature data must not be present in the same loadcase. The program LOCO
           can be used to produce a combined loadcase if required.

Examples


A simple constant face temperature loadcase.

      CASE           100 ’PEAK TEMP GRADIENT ACROSS VESSEL WALL’
      FACE TEM
      //
      /
      27.3           162.9         1
      RP        10       2
      RRP        7       100
      END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-163
ASAS (Linear) User Manual                                                                                  Loading 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.
                     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.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-164
ASAS (Linear) User Manual                                                                                  Loading Data




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.


               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.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-165
ASAS (Linear) User Manual                                                                                  Loading Data


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.



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 5-166
ASAS (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 5-167
ASAS (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 assumed to be zero. 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 loadcase.

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




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-168
ASAS (Linear) User Manual                                                                                Loading Data


5.4.9       BODY FORCE Data

To define a linear acceleration of the structure. The forces arising from the mass of the elements and added
masses are calculated automatically by the program. Only one body force loading may be defined per loadcase.
             BODY FOR

            x-acc                y-acc              z-acc
                       ELEM
                                                      // list //
                       GROU
             RP                  nrep                ilist

             RRP                 nrrep               iilist

             END




Parameters

BODY FOR : compulsory header 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

ELEM              : keyword to denote selection by element numbers.

GROU              : keyword to denote selection by group numbers.

list              : list of element or group numbers where body force 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)

ilist             : element/group 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)

iilist            : element/group number increment. (Integer)

END               : compulsory keyword to denote the end of the body force data block.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-169
ASAS (Linear) User Manual                                                                                   Loading Data



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.

4.         If ELEM/GROU command is omitted, then all elements will be assumed.

5.         Added mass effect will only be included if the added mass is attached to an element which is loaded with
           body forces.

6.         Only one set of acceleration values can be applied per loadcase. If different values are required on
           different parts of the structure, this loading can be generated using the combined loadcase facility. See
           Section 5.8.

7.         If an element is repeatedly selected for body force loading within a given loadcase, either explicitly or by
           way of using its associated group number, the element is loaded only once.

Example


An example of a body force loadcase.

      CASE        56     SIMULTANEOUS Y and Z ACCELERATION
      BODY        FOR
      0.0       10.5         32.2
      END

An example of a body force on elements 51 to 60 and group 3.

      CASE        57     GRAVITY LOADING
      BODY FOR
      0.0 0.0 -9.81
      /
      ELEM              51
      RP   10            1
      GROU               3
      END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-170
ASAS (Linear) User Manual                                                                                Loading Data


5.4.10      CENTRIFUGAL LOADS Data

To define a uniform rotation of the structure about a given point. The radial forces arising from the mass of the
elements and added mass are calculated automatically by the program. Only one centrifugal loading may be
defined per loadcase.

             CENTRIFU
             xc            yc           zc            x-vel              y-vel              z-vel
                        ELEM
                                                       // list //
                        GROU
             RP                   nrep               ilist

             RRP                  nrrep              iilist

             END



Parameters

CENTRIFU          : compulsory header 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 three global directions. (Real)
y-vel
z-vel

ELEM              : keyword to denote selection by element numbers.

GROU              : keyword to denote selection by group numbers.

list              : list of element or group numbers where centrifugal loading 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)

ilist             : element/group 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)

iilist            : element/group number increment. (Integer)

END               : compulsory keyword to denote the end of the centrifugal load data block.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-171
ASAS (Linear) User Manual                                                                                   Loading Data



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 the centrifugal forces.

2.         If ELEM/GROU command is omitted, then all elements will be assumed.

3.         Added mass effect will only be included if the added mass is attached to an element which is loaded with
           centrifugal load.

4.         Only one set of angular velocity values can be applied per loadcase. If different values are required on
           different parts of the structure, this loading can be generated using the combined loadcase facility. See
           Section 5.8.

5.         If an element is repeatedly selected for centrifugal loading within a given loadcase, either explicitly or by
           way of using its associated group number, the element is loaded only once.

Example


An example of a centrifugal loadcase.

      CASE 1 A GENERAL ROTATION ABOUT ALL AXES
      CENTRIFU
      17.3        103.0        96.5       0.134        0.53        0.05
      END

An example of centrifugal loading on elements 51 to 60 and group 3.

      CASE        57     PARTIAL CENTRIFUGAL LOADING
      CENTRIFUGAL
      5.0       15.7         0.0    0.0       1.6      0.0
      /
      ELEM             51
      RP   10           1
      GROU               3
      END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-172
ASAS (Linear) User Manual                                                                                        Loading Data


5.4.11      ANGULAR ACCELERATION LOADS Data

To define angular velocity and angular acceleration of the structure about a given point. The forces arising from
the mass of the elements and added masses are calculated automatically by the program. Only one angular
acceleration loading may be defined per loadcase.
         ANG ACCE
         xc          yc           zc         x-acc           y-acc           z-acc            (x-vel      y-vel      z-vel)
                       ELEM
                                                      // list //
                       GROU
             RP                  nrep               ilist

             RRP                 nrrep              iilist

            END



Parameters

ANG ACCE : compulsory header 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 directions. (Real)
y-acc
z-acc

x-vel             : values of angular velocity in radians/sec about the three global directions. If omitted zero is
y-vel               assumed. (Real)
z-vel

ELEM              : keyword to denote selection by element numbers.

GROU              : keyword to denote selection by group numbers.

list              : list of element or group numbers where angular acceleration 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)

ilist             : element/group 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)

iilist            : element/group number increment. (Integer)

END               : compulsory keyword to denote the end of the angular acceleration data block.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-173
ASAS (Linear) User Manual                                                                                   Loading Data



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 this load type 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 differs from the
           body force convention where a positive input value produces element forces in the positive direction.

4.         If ELEM/GROU command is omitted, then all elements will be assumed.

5.         Added mass effect will only be included if the added mass is attached to an element which is loaded with
           angular accelerations.

6.         Only one set of acceleration values can be applied per loadcase. If different values are required on
           different parts of the structure, this loading can be generated using the combined loadcase facility. See
           Section 5.8.

7.         If an element is repeatedly selected for angular acceleration loading within a given loadcase, either
           explicitly or by way of using its associated group number, the element is loaded only once.

Example


An example of an angular acceleration loadcase.


      CASE        6    CONTAINER ON DECK OF SHIP
      ANG ACCE
      15.9 0.0               -17.6      0.16       0.02        0.0      0.23        -0.07        0.0
      END

An example of angular acceleration loading on elements 51 to 60 and group 3.

      CASE        57     PARTIAL ANGULAR ACC. LOADING
      ANG ACCELERATION
      5.0       15.7         0.0    0.74        0.0      0.0
      /
      ELEM             51
      RP   10            1
      GROU               3
      END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-174
ASAS (Linear) User Manual                                                                                Loading Data


5.4.12      COMPONENT LOADS Data

To define which loadcases from lower level master components are to be included in the loading data for this
component creation or global structure run. Only those component loadcases which are selected will be used in
forming the loadcases for this component creation or structure. Applicable to substructure analyses only.

            COMP LOA

            Aname                      case                        (factor)

            END



Parameters

COMP LOA : compulsory header to denote the start of the component load data.

Aname               : name of the assembled component to which the selected component loadcase is to be applied.
                      (Alphanumeric, 4 characters)

case                : user loadcase number of a loadcase from the master component corresponding to Aname.
                      (Integer)

factor              : factor by which this master component loadcase is to be multiplied. If omitted 1.0 is assumed.
                      (Real)

END                 : compulsory keyword to denote the end of the component load data block.

Note

Only loadcases generated when the lower level master components currently being assembled were created can
be selected.

Example

In this example of component loadcase selection, loadcase 20 is created by selecting user loadcase 7 from the
lower level master component WALL, multiplying it by 2.50 and applying it to the assemble component LEFT.

   CASE        20     LOADS APPLIED TO COMPONENT LEFT
   COMP        LOA
   LEFT         7     2.50
   END

A more general example combining loadcases and several components.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-175
ASAS (Linear) User Manual                                                                               Loading Data


  CASE        21     LOADS APPLIED TO COMPONENT LEFT AND RIGHT
  COMP LOA
  LEFT        10       1.0
  LEFT        11       1.5
  RIGH        10     -1.0
  RIGH        11     -1.0
  END




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-176
ASAS (Linear) User Manual                                                                                       Loading Data


5.4.13      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 program 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 acceleration 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)

inface            : Internal face 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




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-177
ASAS (Linear) User Manual                                                                                   Loading Data


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.

           TANK LOAD
           ACCN         0.0      0.0 9.81 0.0 0.0                    0.0
           ABCD         100      1 20.0 1025.0
           END




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 5-178
      ASAS (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 a data block for one or more of the mass types. Each block consists of a
mass type header followed by the appropriate data. Only one block of each type is permitted for the structure.
                  DIRE

                  LUMP                   ADDED MA
                                         FULL MAS

                   (mtype)               mass              dof                 nodes

                  RP                     nrep              inode

                  RRP                    nrrep             iinode

                  END


                  CONS                ADDED MA


                  x-mass                 y-mass                 z-mass                  nodes

                   RP                    nrep               inode

                  RRP                    nrrep              increment

                  END


Parameters
DIRE          : compulsory header to denote the start of the Direct Mass Input data.

LUMP          : keyword for lumped added mass input.

CONS          : keyword for consistent added mass input.

END           : compulsory keyword to denote the end of each block of Direct Mass Input data.

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 equal mass to the X, Y, Z freedoms at a node. Freedom name
        ROT may be used to assign equal mass to the RX, RY, RZ freedoms at a node.
3.      FULL MAS is only valid for dynamic analyses. The mass values must only be supplied at master
        freedoms and all master freedoms must be provided with a non-zero mass. If no master freedom data is
        supplied all unsuppressed freedoms are considered to be masters.
4.      If a node is skewed in the Boundary Conditions Data, any added lumped mass terms input for that node
        are assumed to be in the skewed directions.
5.      The direct input mass data must be re-specified in an additional load or frequency run.



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-179
     ASAS (Linear) User Manual                                                                         Additional Mass Data


5.5.1       UNITS command

If global units have been defined using the UNITS command in the Preliminary Data (see Section 5.1.21), 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)

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 Appendix -B.

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 5.1.21.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-180
       ASAS (Linear) User Manual                                                                       Additional Mass Data


5.5.2       LUMP ADDED MASS Data

To define the values for lumped added mass.

With the FULL MAS option, the mass values supplied in this data replace any mass implied by the elements.
With the ADDED MA option, the mass values supplied are in addition to the mass of the elements.

            LUMP                   ADDED MA
                                   FULL MAS


             (mtype)                mass                  dof                //nodes//

            RP                     nrep               inode

            RRP                    nrrep              iinode

            END



Parameters

LUMP              : compulsory header 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.

FULL MAS          : keyword to define the following mass terms are to replace all other mass from the elements.

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 notes and Appendix -E.

nodes             : list of node numbers to which the mass is applied. (Integer).

RP                : keyword to indicate data generation 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 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)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-181
      ASAS (Linear) User Manual                                                                        Additional Mass Data


END               : compulsory keyword to denote the end of the lumped mass data block.

Notes


4.      Freedom name TRA may be used to assign equal mass to the X, Y, Z freedoms at a node. Freedom name
        ROT may be used to assign equal mass to the RX, RY, RZ freedoms at a node.

5.      Mass type L is not allowed with FULL MAS.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 5-182
        ASAS (Linear) User Manual                                                                           Additional Mass Data


5.5.3       CONSISTENT ADDED MASS Data

To define added consistent mass data. Direct input of consistent mass is given in terms of an additional material
density for each of the three local axes. It is only applicable to the elements BEAM, BM2D, BM3D, TUBE,
GRIL. Any elements with added consistent mass must also have consistent mass type in the Element Topology
data.

            CONS                 ADDED MA


            x-mass                 y-mass                 z-mass                //node1//               //node2//

            RP                     nrep               inode

            RRP                    nrrep               increment

            END



Parameters

CONS              : compulsory header keywords to denote the start of consistent mass data.

ADDED MA : keyword to define that the following mass values are to be added to any element mass.

x-mass            : value of additional density in local x-direction. (Real)

y-mass            : value of additional density in local y-direction. (Real)

z-mass            : value of additional density in local z-direction. (Real)

node1             : a pair of node numbers to define the element. (Integer)
node2

RP                : keyword to indicate data generation 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 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 consistent mass data block.

Note


Consistent added mass data may only be used in a natural frequency analysis.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-183
      ASAS (Linear) User Manual                                                                        Component Recovery Data



5.6    COMPONENT RECOVERY Data

These data blocks allow the user to select the output from each component in a stress recovery run.

The following data blocks are available:

                         Component selection ................ ................ see Section 5.6.1

                         Loadcase selection... ................ ................ see Section 5.6.2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-184
     ASAS (Linear) User Manual                                                                         Component Recovery Data


5.6.1       COMPONENT SELECTION Data for Component Recovery

To define which assembled components are to have their internal displacements and element stresses calculated
and printed.


         COMPONENT                          Sname                  Aname(option)



Parameters

COMPONENT : keyword to define the path to a lower level assembled component.

Sname             : global structure name for this entire assembly. For dynamic stress recovery, the global
                      structure name is the NEWSTRUCTURE name specified in RESPONSE run.

Aname             : assembled component name for each level of assembly from the global structure level down to
                        the point at which recovery is to cease.

(option)          : a print option, enclosed in brackets. See Note 4 below.

Notes


1.      The user may identify the part, or branch of the structure for which he requires to recover results by
        specifying the Global Structure Name followed by a list of Assembled Component Names for each level
        of the assembled structure in order to identify the required branch.

2.      Each main branch of the structure must start on a new component line starting with the Global Structure
        Name.

3.      The word ALL may be used at any point in place of an assembled component name, including following
        the Global Structure Name, to indicate that all lower level components from that point in the tree structure
        are required to be recovered.

4.      Each Assembled Component Name (including the word ALL) may be followed by a print option enclosed
        in brackets. Options available are:

                (D)                        : print displacements and reactions only
                (S)                        : print stresses for elements only
                (DS) or (SD)               : print displacements, reactions and stresses
                blank                      : do not print displacements, reactions or stresses


5.      Continuation lines may be used if required to complete a branch.

6.      Each branch is processed from the highest level down in order. Partial processing of a branch down to an
        intermediate level is permitted.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-185
     ASAS (Linear) User Manual                                                                         Component Recovery Data


7.     Processing of a previously partially processed branch may be completed by re-specifying the branch from
       the Global Structure Name but extended to include the required extra components.

       Results for Components which have already been recovered are not recalculated during this process but
       may be reprinted, if required, by use of the appropriate print options.

Example


This example requests that all components forming the left side of a structure ROOF are recovered but only one
branch on the right side. Full printing of displacements and stresses for all components is specified.

       COMPONENT            ROOF        LEFT(DS)          ALL(DS)
       COMPONENT            ROOF        RIGH(DS)          TOPP(DS)           TRUS(DS)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-186
     ASAS (Linear) User Manual                                                                         Component Recovery Data


5.6.2       LOADCASE SELECTION Data for Component Recovery

To define a subset of loadcases for the selected components from the total set of loadcases solved at the global
structure stage.

          SELECT LOADS                         Aname                     cases



Parameters

SELECT LOADS : keywords to define the loadcases required by the component Aname.

Aname         : assembled component name to which this subset of loadcases applies.

cases         : list of global structure loadcase numbers required for this component.                        For dynamic stress
                recovery, loadcase numbers are those defined in the RESPONSE run. (Integer)

Notes


1.      A SELECT LOADS command applies to an Assembled Component in a given branch of the assembled
        structure and, therefore, must follow the corresponding COMPONENT selection.

2.      A SELECT LOADS command defines a subset of the loadcases existing (or previously selected) for the
        component at the next higher level in the branch. It also implies that the selected subset will apply to all
        lower level components in the branch, unless the load set for these components are further reduced by
        other SELECT LOADS commands.

3.      SELECT LOADS commands are cumulative for the current run. Output for a given assembled
        component will consist of all the cases specified by all the SELECT LOADS commands which apply to
        that component from all branches.

4.      If no SELECT LOADS command is present for a particular branch, than all loadcases from the Global
        Structure will be assumed.

5.      SELECT LOADS commands must not be defined for Components implied by the optional ALL and not
        specifically named by a COMPONENT selection line.

6.      Continuation lines are not allowed, but more than one SELECT LOADS line may be used if necessary to
        define all the loadcases required.

7.      If, due to an unwise choice of Assembled Component Names, the same name appears more than once in
        any branch, the SELECT LOADS commands are assumed to apply to the higher level component.

8.      SELECT LOADS commands can only select the loadcases and the loadcase numbers of the global
        structure. Loadcases applied during the master component creation phase cannot be selected because
        factoring and combining of these cases may not have taken place during assembly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 5-187
     ASAS (Linear) User Manual                                                                         Component Recovery Data


9.     If a subset of the loadcases is selected for a given component it is not possible to recover any of the
       remaining loadcases in a subsequent recovery run. It is advisable, therefore, to ensure that all loadcases
       for which results are required are included in the initial recovery run.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 5-188
       ASAS (Linear) User Manual                                                     Stiffness and Mass Matrix Input Data


5.7     Stiffness and Mass Matrix Input Data


5.7.1       STIFFNESS Matrix Data

This data defines the component stiffness matrix. Job type STIF only.
            STIF
                                         (FULL)
            TYPE
                                         (PACKED)
             stiffness


             END


Parameters

STIF          : compulsory header to denote start of the stiffness matrix data.

TYPE          : keyword to define the matrix type.

FULL          : keyword to denote full matrix form will be given. (N*N values, where N is number of link
                freedoms)

PACKED          :        keyword to denote packed symmetric matrix form will be given. (N*(N+1)/2 values, where
                N is number of link freedoms)

stiffness : stiffness values (continuation characters : should not be used). (Real)

END           : compulsory keyword to denote the end of stiffness matrix data block.

Notes

1.      Stiffness values must be given to cover all link freedoms and                                   1   2   3   4    5    6
                                                                                                        1   2   4   7    11   16   1
        must be ordered to reflect ascending user node numbers and
        ascending ASAS freedom number order (see Appendix -E).                                              3   5   8    12   17   2

                                                                                                                6   9    13   18   3
2.      If the TYPE command is omitted, the packed symmetric form
        of matrix input is assumed.                                                                                 10   14   19   4

3.      This data is only valid in a direct stiffness input component                                                    15   20   5
        creation job (JOB STIF).
                                                                                                                              21   6

4.      The order of the packed symmetric matrix form is shown by
        means of the following example of a 6 freedom matrix.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 5-189
      ASAS (Linear) User Manual                                                      Stiffness and Mass Matrix Input Data


5.7.2       MASS Matrix Data

This data defines the component mass matrix.

             MASS

                                         (FULL)
            TYPE
                                         (PACKED)

             mass


             END



Parameters

MASS          : compulsory header to denote start of the mass matrix data.

TYPE          : keyword to define matrix type.

FULL          : keyword to denote full matrix form will be given. (N*N values, where N is the number of link
                freedoms).

PACKED : keyword to denote packed symmetric matrix form will be given. (N*(N+1)/2 values where N is
                the number of link freedoms).

mass          : mass values (continuation characters : should not be used). (Real)

END           : compulsory keyword to denote end of mass matrix data block.

Notes


1.      A component mass matrix must be supplied if the component is to be used in a natural frequency analysis.

2.      Mass values must be given all link freedoms and must be ordered to reflect ascending user node numbers
        and ascending ASAS freedom number order. (See Appendix -E).

3.      If the TYPE command is omitted, the packed symmetric form of matrix input is assumed.

4.      This data is only valid in a direct stiffness input component creation (JOB STIF) run when a dynamic
        component is being created.

5.      For the order of the terms in the packed symmetric form, see example in Section 5.7.1.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 5-190
        ASAS (Linear) User Manual                                                                      Combined Loadcase Data



5.8      COMBINED LOADCASE Data

The basic loadcase data is defined in Section 5.4 together with all the input syntax.

The user may specify combined loadcase data which must follow the basic load data and any direct input mass
data.

If there is no combined loadcase data then ASAS will analyze the cases defined in the basic loadcase data. If
combined loadcase data is present then only the combined cases will be analysed. If the user wishes to analyse
some or all of the basic cases with the combinations, it is necessary to specify a combination case as a unit factor
on the basic loadcase for each basic loadcase required.
                  COMB                      ( ncombs )

                  SELE                         new case               `title'



                  CASE                         case                   factor



                  NEWCASE                      case                   factor



                  END




Parameters

COMB              : compulsory header to denote the start of the combined loadcase data

ncombs            : number of combined cases to be analysed. Optional. (Integer, 1-9999). If supplied, ncombs
                     must equal the number of combined loadcases defined.

SELE              : compulsory keyword to denote the start of the data for the next combined case.

newcase           : combined loadcase number. (Integer, 1-9999.) Every combined case number must be unique,
                     but need not form a sequence with the other combined loadcase numbers. The combined
                     loadcases numbers are independent of the basic loadcase numbers.

title             : combined loadcase title. (Alphanumeric string enclosed in quotes, 40 characters)

CASE              : keyword to indicate the basic case to be added into the current combined case.

NEWCASE           : keyword to indicate that a preceding combined case to be added into the current combined
                     case.

case              : basic loadcase number. (Integer)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-191
       ASAS (Linear) User Manual                                                                       Combined Loadcase Data


factor                : factor by which basic loadcase is to be multiplied before addition to current combined case.
                        (Real)

END                   : compulsory keyword to denote the end of the data for each combined loadcase.


Example


An example showing the creation of 2 combined cases from several basic cases.

   COMB
   SELE                17           ’SELF WEIGHT, WIND AND PRESSURE LOADS’
   CASE       2             1.0
   CASE       4             1.7
   CASE       5             1.0
   END
   SELE       18            ’REVERSE THRUST, SELF WEIGHT, BRAKING’
   CASE           2          1.0
   CASE           1         -2.36
   CASE           3         1.0
   END

Note


Depending on the load combination facilities required it may be more economical or necessary to use the
program LOCO.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page 5-192
ASAS (Linear) User Manual                                                                                    STOP Data



5.9     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 5-193
ASAS (Linear) User Manual                                                                                General Instructions


6.      Running Instructions

6.1     General

Every attempt has been made to create a program which, in spite of its broad scope of application, is easy to
handle on any given machine. The commands to run the program have been kept to a minimum and all file
assignments are handled automatically from within the program.

This chapter contains some general instructions for running the program. Exact details depend on the computer
type and model number and also on the way the program has been installed. Users should contact their local
ASAS representative for further information if any problems are encountered.

6.2     How to Run ASAS

The instructions to run ASAS 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 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 6-1
ASAS (Linear) User Manual                                                                                General 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:

/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 ASAS 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.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-2
ASAS (Linear) User Manual                                                                                   General Instructions

To start the analysis, click on the OK button. This will display a dialog window similar to that shown below:




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.

3. Using a DOS Shell

The program can be run in a DOS Shell using a command of the form:


               asas DataFileName
or
               asas /DATA=DataFileName /OUT=ResultsFileName [/parameter]


assuming the directory where the program is installed (e.g. c:\Program Files\ANSYS Inc\v120\asas\win32) is 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 6-3
ASAS (Linear) User Manual                                                                                   General 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 from batch files on PCs

As ASAS 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 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

ASAS hull /LOCK
WAITLOCK
copy hulljf hulljf.save
LOCO13 hulla

6.3        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

Default_prenl_output_extension=ext                                   where ext is the user’s preferred extension for the output
                                                                     file for prenl
                                                                     Default is .pno




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

Default_asasnl_output_extension=ext where ext is the user’s preferred extension for the output
                                                                  file for asasnl
                                                                  Default is .ano

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

             asas.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

             asas.exe              hull.dat

6.4     Extended Syntax in Data Files



6.4.1        IF/THEN/ELSE

ASAS 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.

  Linear Data                                 Frequency Data                                Merged Data
  job line                                    job freq                                      if linear then
                                                                                              job line
                                                                                            else
                                                                                              job freq
                                                                                            endif
  project test                                project test                                  project test
  options nobl                                options nobl                                  options nobl
  save loco files                             save dypo files                               if linear then
                                                                                              save loco files
                                                                                            else
                                                                                              save dypo files
                                                                                            endif
  coor, elem, mate, geom                      coor, elem, mate, geom                        coor, elem, mate, geom
  supp, disp                                  supp, disp                                    supp, disp



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

  load                                            dire                                         if linear then
                                                                                                 load
                                                                                               else
                                                                                                 dire
                                                                                               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:

                        asas.exe           hull /linear               for a linear run

or
                        asas.exe           hull /#linear for a dynamics run


Thus any parameter after a /, except the reserved parameters listed in section 6.2, 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:

  Linear Data                          Frequency Data                      Merged Data
  job line                             job freq                            if save#dypo then
                                                                            job line
                                                                           else
                                                                            job freq
                                                                           endif
  project test                         project test                        project test
  options nobl                         options nobl                        options nobl
  save femm files                      save dypo files                     if save=femv then
  save femd files                                                           save femm files
  save fems files                                                           save femd files
                                                                            save fems files
                                                                           elseif save=dypo then
                                                                            save dypo files
                                                                           else
                                                                            save loco files
                                                                           endif
  end                                  end                                 end
  etc                                  etc                                 etc


The command line to run this data would be either:

               asas.exe hull                 /save=femv                            for a linear run

or

               asas.exe hull                 /save=dypo                            for a dynamics run



     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 6-6
ASAS (Linear) User Manual                                                                                General Instructions

Thus the parameter following / may be of the form:

            /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
are 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.




6.4.2       DATA REPLACEMENT

Specified character strings in the data may be replaced with values defined on the command line.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-7
ASAS (Linear) User Manual                                                                                General Instructions

Consider the following data file:

          job line
          project test
          options nobl
          save %save files
          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:

          asas.exe hull %save=fatjack %load=5000

When interpreting the data, each time %save was encountered, it would be replaced by the characters
fatjack, 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:
         asas.exe hull $save=fatjack $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.




6.4.3       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 %save=fatjack
            define %load=5000
            job line
            project test
            options nobl
            save %save files
            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



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-8
ASAS (Linear) User Manual                                                                                General Instructions

string replacement is used on a command line and also on a DEFINE command. Thus, if the command line had
been:

            asas.exe hull %save=loco

then the save command would have been interpreted as ”save loco files” 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.




6.4.4       Automatic JOB Type and Program Name Recognition

As the JOB command is an important part of the definition of the job type, this may be used automatically within
the data. Thus, for example, in the data file:

job line
project test
options nobl
if job=line then
   save loco files
elseif job=freq
   save dypo file
endif
end
etc

the save commands would automatically be used according to the job command. Hence, for job line, save
loco files would be used, and if the job command was job freq, then save dypo files would be
used. If any other job type was used, then neither of the save commands would be used.

The name of the program being executed is also available during the interpretation of the data. This is
recognised with the key word prog. Thus, a number of data files can be combined using a prog test. For
example:

if prog=asas then
            ASAS data
elseif prog=loco then
            LOCO data
elseif prog=beamst then
            BEAMST data
else
            STOP
endif

A condition does not need to encompass a complete data file. The tests may surround blocks of data that are
program dependent, for example:




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-9
ASAS (Linear) User Manual                                                                               General Instructions

job freq
project test
options nobl end
end
coor, elem, mate, geom, supp, disp data
load 1
wave loa
if prog=wave then
           WAVE data
elseif prog=mass then
           MASS data
end
stop




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-10
ASAS (Linear) User Manual                                                                                 General Instructions

In this example, the relevant WAVE or MASS data would be used accordingly.

The available program names are as follows:

ASAS                        LOCO                    RESPONSE                   POST                       WAVE

MASS                        FATJACK                 BEAMST                     XTRACT                     SPLINTER

WINDSPEC                    MAXMIN                  ASASLINK

6.5     Secondary Data Files within ASAS 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.




6.5.1       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

        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.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 6-11
ASAS (Linear) User Manual                                                                                   General Instructions

           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.




6.5.2           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.

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.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-12
ASAS (Linear) User Manual                                                                                General Instructions

6.6     Estimating Job Size

For the latest information about estimating memory, disk space and run-time resources please refer to the ASAS
web site.

6.7     Disk File Handling

The creation, deletion and assigning of disk files is largely automatic and carried out from within the program as
the run proceeds.

A separate database is created for each PROJECT. This database consists of a number of disk files, each of
which is referenced through an index file (the “10 file”).

Whenever the word NEW is used on the JOB command, a new database is started. Should a database already
exist, the files associated with this database will be renamed with the extension .bak. An index file is created
with a name consisting of the number 10 appended to the project name, the “10 file”. As the run proceeds other
files are created using the file name on the FILES command, in this case with numbers in the range 12 to 45
appended. Various data blocks are written to these files such as element data, stiffness matrices, stresses, etc,
and the information to say what data is stored on each file is kept in the index file.

During the run a temporary copy of the “10 file” is made. This is the “11 file”. At the end of a successful run
the “11 file” will be deleted by the program. However if the run aborts and does not conclude with a tidy
closedown, this file may be left on disk. It is of no use and may safely be deleted once the run has finished.

Normally most disk files created during a run will be deleted before the end of the run. However, if the user
requires that some information is to be saved such as by use of “SAVE FILES” command, or automatically
saved as in the case of a component analysis, the relevant information will be written to the “35 file” and will not
be deleted at the end of the run. Subsequent runs of ASAS or other programs will then be able to use this data as
appropriate.

If saving of results is requested using the RESU command, the information will be written to the “45 file” and
will not be deleted at the end of the run.

Further runs of ASAS using the same project name without NEW on the JOB command will add to that database
for that project and therefore the “10 file” must be on disk at the start of each run.

Remember, the “10 file” is the only way to access a database. Do not delete this file unless the entire database is
to be deleted. For security, it is important to ensure that a copy of this file is taken from time to time just in case
it is accidentally damaged or lost.




6.7.1       Disk Files Required for Substructures

At the various stages of a substructured analysis, files will be needed from previous runs in order that the
required information is available.

For any component creation run and for the global structure run, the disk files (“35 files”) relating to all the
master components which are being assembled in that run must be on disk and accessible by ASAS.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-13
ASAS (Linear) User Manual                                                                                General Instructions

To carry out the stress recovery for a component ASAS needs to access the “35 files” for (a) the master
component creation run for this component, (b) the global structure run and (c) the previously recovered higher
level component.

To illustrate these requirements consider the structure defined by the tree diagram in Figure 2.4 in Section 2 To
create master component C006 it is necessary to have on disk the “35 files” for the master components C002 and
C003.

To create the global structure STRC it is necessary to have the “35 files” for C005 and C006.

To recover the displacements and stresses for assembled component A402 it is necessary to have on disk the “35
files” for master component C006 and the global structure STRC.

To recover the displacements and stresses for assembled component A202 which is part of A302 (in the centre of
the diagram) it is necessary to have on disk the “35 files” for master component C002, the global structure STRC
and the higher level assembled component A302. A302 must have already been recovered.




6.7.2       Using ASAS Backing Files on Separate Directories

Under normal circumstances ASAS creates its backing files on the local directory. There are some
circumstances, however, when it would be desirable or advantageous to distribute the files to different directories
or different disk drives. This may be necessary if there is little free space on the current disk or where a very
large job has to be run and the space on several disk drives is required.

A facility exists to allow most backing files to be located elsewhere from the local area. This is achieved using a
PATH file.

Each time an ASAS program runs, it examines the local directory for an ASCII file called proj.PTH, where proj
is the project name for the current run. This file can contain up to 20 entries, each of which is a revised location
for one of the backing files. Note, proj10 and proj11 must always be on the local directory and cannot be
relocated by this means.

Even when files are distributed, it is still a requirement that each ASAS backing file is located in one single
directory. It is not possible to split a single file between directories or disk drives.

The format of each of the lines of the file proj.PTH is:

        cols 1-6          name of the backing file (eg ABCD21, XXXX35)

        col 7             blank

        cols 8-48         path for the location of the file. The format for this varies according to system. See below.


                                   Machine                    Example Path Name

                                   UNIX                       /usr/auto/ford

                                   PC                         H:\SEA\REGION




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-14
ASAS (Linear) User Manual                                                                                   General Instructions

Thus a complete line might be:

                    ABCD21           /usr/auto/ford                      for a UNIX System
                    XXXX35           H:\SEA\REGION                       for a PC


If subsequent post-processing is carried out, the program will know where any relevant backing files are stored.
It is also possible to copy an existing backing file to a different location and then create a path file to indicate its
new location. Care should be taken that the correct file access controls have been applied to the file and
directory in its new location. The user may not have permission to read or write at that location.

6.8        Error and Warning Messages

Diagnostic messages divide broadly into two groups, Errors and Warnings. In most cases Errors and Warnings
are accompanied on the printout by an explanation of the cause.

The user must be aware that the program can only check for syntax problems and data which are logically
incorrect or inconsistent. The program cannot necessarily check the description of the structure or the physical
data values used.




6.8.1          Warning Messages

Warning messages are issued when the program detects an unusual condition or a data item which does not
match the rest of the data, but the program can still proceed. For example an option may be specified which is
not applicable to the type of analysis being performed and can be safely ignored. Again the user may have
defined a material type but never referenced it in the element data.

In the case of a run with Warnings, the run will terminate at the end of the data check unless the option GOON
has been supplied. In this way the user has the opportunity to check the data and, if acceptable, proceed without
having to make major changes.




6.8.2          Error Messages

Error messages are issued when the program detects a condition which makes it unreasonable or impossible for
the run to continue. For example, a material type has been referenced in the element data but that material has
not been defined in the material data. Again, an error message will be issued and the program will stop if a
singularity is detected during the equation solution. Errors fall logically into a number of groups which are
described in general terms below.

1.         Errors discovered by the data checks

           As data is read in, checks are performed on the syntax of the commands and the data items they contain.
           Any errors detected here will be indicated with an explanatory message.

           Once the whole data has been read, cross checks are made on the consistency of the data and again errors
           detected are accompanied by a suitable message.



     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-15
ASAS (Linear) User Manual                                                                                   General Instructions

2.         Data errors not discovered by the data checks.

           It is not possible to detect all errors at the checking stage and it is possible that an undetected error in the
           data may cause problems later in the run.

           These errors can manifest themselves in a number of ways.

           (i)     A later calculation may detect a problem but be unable to give a clear explanation as to its cause
                   and the error message may not be very helpful.

           (ii)    The computer system may detect the problem and issue a message such as ‘divide by zero’ or
                   ‘square root of negative number’ detected.

           (iii)   Very occasionally the program may decide it cannot continue and abort the run with no
                   explanation.

           Where the program finds it necessary to stop the run immediately, a message of the form


                    ABORT IN ROUTINE abcdef

           is issued followed by a subroutine traceback. This is a list of FORTRAN subroutine names which can be
           of assistance to the ASAS support team in diagnosing what the cause might be if the user cannot resolve
           the problem.


3.         System related errors

           A number of the error messages might loosely be described as system related. These might arise from
           hardware or software causes or the interaction of both. Usually they are related to memory requirements
           or disk storage.

          (i)      Data Area related problems

           The manipulation of data in ASAS takes place largely in an area of the memory which is referred to as the
           Data Area or Freestore. The length of this region of memory is user defined on the SYSTEM command.
           For most analysis, ASAS is able to make use of the space provided, assuming that the space allocated is
           reasonable compared to the size of the run. See the ASAS Web site for further information on run size.
           However, two types of errors related to Data Area memory allocation may appear. Firstly, an error
           message of the form


                      *** ERROR *** ATTEMPT TO CLAIM SPACE OF
                                                LENGTH nnn FROM DATA AREA IN
                                                ROUTINE abcd ON CALL NO. j

           The value of nnn is zero or negative and this is usually caused by errors in the data either where the error
           has gone undetected or where the error was detected and the program has tried to continue to check other
           data. The user should initially remove all known errors from the data and rerun.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-16
ASAS (Linear) User Manual                                                                                   General Instructions

           The second data area related message is of the form


                    *** ERROR *** DATA AREA FULL.                              PROBLEM TOO LARGE
                                               SPACE OF nnn CLAIMED IN
                                               ROUTINE abcd ON CALL NO. j
                                               SPACE OF mmm AVAILABLE
                                               TOTAL DATA AREA REQUESTED ppp

           This may be caused by data errors but is most likely to be caused by insufficient space being requested on
           the SYSTEM command. The user should (a) correct all known errors in the data (b) increase the size of
           the Data Area allocation on the System Command and (c) rerun. If the problem persists the user should
           contact the ASAS support team.

          (ii)     Disk File Related Problems

           A group of error messages which may arise are of the form


                    **** FILES PACKAGE ERROR NO nn IN ROUTINE abcd ****

           followed by a simple message.

           The two most common causes of these messages are either that the files required from a previous run are
           not available on the disk in the current directory or that the previous runs did not complete successfully.
           The user should check the preliminary data for the correct use of project names, file names and structure
           names and that all previous runs were successful.

           Messages of the form


                      ERROR nn WRITING UNIT mm KEY ppp
                      ABORT IN ROUTINE WTBUFF

           or


                      ERROR nn READING UNIT mm KEY ppp
                      ABORT IN ROUTINE RDBUFF

           are related to the writing and reading of blocks of data to and from the disk. The causes are most likely to
           be that the user has filled up the disk or that there is a disk hardware failure.


4.         ASAS Support

           If the user has problems interpreting an error message he should contact the ASAS support team. When
           doing so it is extremely helpful to have available the exact wording of the error message, the details of the
           subroutine traceback and the two tailsheet tables relating to the files and the run parameters. Details of
           any previous errors and warning within the run would also be useful. The version number of the program
           being used will also be required.




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 6-17
ASAS (Linear) User Manual                                                                                  Appendix A


Appendix - A                      Description of Each Type of Finite Element in ASAS

This Appendix contains details of all element related data used within ASAS. The first sections describe general
element data applicable to all or groups of element types. This is followed by a quick reference table giving an
overview of all the elements and finally detailed description sheets for each ASAS element arranged in
alphabetical order.

The following sections are included:

                         Element Related Loading ......... ................ ................A.1

                         Element Axes Systems ............. ................ ................A.2

                         Beam Offsets ........... ................ ................ ................A.3

                         Stepped Beams ........ ................ ................ ................A.4

                         Shell Offsets ............ ................ ................ ................A.5

                         Laminated Shells ..... ................ ................ ................A.6

                         Section Libraries ..... ................ ................ ................A.7

                         Beam Stresses.......... ................ ........................ ........A.8

                         ASAS Element Description Sheets ............................ A.9

                         Overview of ASAS Elements .................... ......Table A.1




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


A.1 Element Type Related Loading Data
Details of all the ASAS load types are given in Section 2.8. These load types may be divided into two groups:

            Element Specific Load Types

            Standard Load Types

The Element Specific Load Types consist of the element applied mechanical loads (eg Pressure and Distributed
loading) and thermal loading of all types. These are covered on an element by element basis in the ASAS
element description sheets.

The Standard Load Types are applicable to models of any element type and consist of nodally applied
mechanical loading (eg Nodal Loads and Prescribed Displacements) and mass loading (eg Body Force,
Centrifugal and Angular Acceleration Loads). The one exception is that Angular Acceleration cannot be applied
to 2-D and Axi-symmetric elements.

For nodal loads and prescribed displacements the freedom that is loaded must exist on at least one element
attached to the loaded node.




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

A.2 Element Axes Systems
All ASAS 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 is
conducted by the post processor ASASPOST.

A.2.1 Local Axes on Beam Elements

ASAS 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, BMGN, TUBE and
BAX3 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-3
ASAS (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 5.2.5.4.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page A-4
ASAS (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
                                                                                                     default Y'
                                                              X'                     Y'                                              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




                                            Figure A.1 Examples of Beam Local Axes Definitions




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


A.2.2 Local Axes on Shell/Plate Elements

ASAS shell and plate elements all use local element axis systems (with the exception of the MEM4, SLB8 and
TRB3 elements which use the global axis system). The definition of these local axes systems is consistent
between all the shell and plate element types. The local X axis is in the direction from the first corner node to
the second corner node. The local Y axis is perpendicular to the local X axis, positive towards the third corner
node. Local Z axis forms a right handed orthogonal axis system with the local X and Y axes. Local Z is always
normal to the surface of the element and defines the positive normal used for pressure loading and face
temperature loading.

For curved elements the local axes are curvilinear, the local X axis follows the surface of the element and is
defined by the intersection of the surface with the plane containing the surface normal and a line parallel to the
straight line between the first and second corner nodes. The local Y axis also follows the surface of the element
and positive towards the third corner node.

For shell elements, anisotropic, orthotropic and laminated material properties are defined with respect to the
material axes. The material Xm axis is defined as the projection of the global X axis (or skew X axis if a skew
system is specified in the material data) onto the shell surface, with Ym lying on the tangent plane of the shell
and orthogonal to Xm. Since this definition will break down if the projection does not exist, the user must ensure
that the control vector (global X axis or skew X axis) is not normal to the shell surface. Further consideration of
the material axis is given in Appendix A.6.

The direction of pressure and face temperature loading is dependant on the direction of the element local Z
direction. For this reason it is extremely important that adjacent elements have a consistent local Z direction.
This is achieved by ensuring that the element nodes are ordered in the same sense in the element topology data,
ie all defined clockwise or all defined anti-clockwise order. This is illustrated in Figure A.2 below.
                         4                      5                    6
              Z'
                          Y'                                                                 QUS4       1 2 5 4 1 1
                                                        X'
                                                                                             QUS4       2 5 6 3 1 2
                           X'
                                                        Y'                              gives conflicting local Z direction
      1                            2                              3
                                                                 Z'
                                           Z'
                               4                             5                     6
               Z'                                                      Y'
                          Y'                                                                 QUS4       1 2 5 4 1 1
                                                   X'                                        QUS4       5 2 3 6 1 2
                           X'
                                                                                       gives consistent local Z direction
      1                            2                              3                    (but conflicting local X and Y directions)



                                    Figure A.2 Defining Consistent Local Z Direction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page A-6
ASAS (Linear) User Manual                                                                                   Appendix A

By default all element stress results are printed in the elements local axes systems. For this reason it is
preferable to get local X, Y and Z consistent on adjacent elements where possible. For certain plate type
elements it is possible to request the results in the global axes system using the GLST option.

A.2.3 Local Axes on Brick Elements

By default, brick elements use the global axes system for both definition of material axes and presentation of
stress results. Local element axes may be requested using the LSTS option in the preliminary data. The element
local axes will then be used for both defining the material axes (if anisotropic materials are used) and for the
presentation of stress results.

The local axes are defined in the following manner. The Local X’ direction is parallel to the first edge defined
for the element. Local Y’ is orthogonal to local X’ and lies in the first surface defined for the element. Local Z’
is orthogonal to local X’ and Y’.
                                                                 7
                                                                                   6
                                               8
                                                                                                        5
                                                   Z'
                                                             Y'                                         11
                                   1
                                                         X'                              4              17
                                       9
                                                             2
                                  13                                      3                  16
                                                        14                     10


                                                                              15

                                       Figure A.3 Local Axes for a Rectangular Brick

For non-rectangular elements, the local axes follow the taper or curvature of the element as shown in the
diagrams. For example, for a BR20, local X’ is always parallel to edges 1-2-3, 7-6-5, 13-14-15, 19-18-17 and
local Y’ always lies in the surfaces 1-2-3-4-5-6-7-8 and 13-14-15-16-17-18-19-20. Note, X’Y’Z’ always form
an orthogonal set of axes at any point on an element.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-7
ASAS (Linear) User Manual                                                                              Appendix A




                                   Figure A.4 Local Axes for a Non-rectangular Brick

Warning - Care must be taken if the user intends to use the post-processor POST. If the stresses are all global
(i.e. LSTS is not set) then the average stresses and principal stresses will be correct. If the LSTS option is set
then care must be taken that the local axes of adjacent elements, within an ASAS group, are consistent, i.e. the
local axis set for the common node is identical for all elements at that node.

A.2.4 Local Axes on Axisymmetric Elements

Axisymmetric shell elements use the local axes system as defined in the element description sheets.

Axisymmetric brick elements use the global axes by default. Like the brick elements above, local axes may be
requested using the LSTS option in the preliminary data.

The local axis definition is given by the way the element is numbered on the topology data. The first side
defines the local r' direction. Local Z' lies 90° counter clockwise from r', in the plane of the section, as defined
below. This local set is used at all nodes on the element and, unlike the bricks, it does not vary if the element
edges are tapered or curved.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page A-8
ASAS (Linear) User Manual                                                                              Appendix A



                     Z
                                                                                     5
                                                 Z∋
                                                            6

                                    7


                                    8                                        4



                                    1
                                                      2
                                                                     3               r∋

                                                                                                        R




                               Figure A.5 Local Axes for an Axisymmetric Solid Element

Local axes may be used for two purposes. Firstly for anisotropic material to define the orientation of the
material relative to the global axes, and secondly to specify output axes for stresses.

Warning - Care must be taken if the user intends to use the post-processor, POST. If the stresses are all global,
(i.e. option LSTS is not set) then POST will produce correct global average and principal stresses. If the LSTS
be set then care must be taken that the local axes of adjacent elements in an ASAS group be consistent, i.e. the
local axis set for all elements at common nodes are identical.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-9
ASAS (Linear) User Manual                                                                                        Appendix A

A.3 Beam Offsets
The element types BAX3, BEAM, BMGN, BM2D, BM3D, GRIL, TCBM 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.

Note


GRIL element may only use the OFFS command.


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.6 Local Axes for a Beam with Offsets




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page A-10
ASAS (Linear) User Manual                                                                              Appendix A


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:




                                       Figure A.7 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 TCBM elements 9 values of offset are required, ex, ey, ez for nodes 1, 2 and 3. The ex value for the
        middle node must be zero.

4.      For BM2D and GRIL elements 4 values of offset are required, ex, ey, values for node 1 followed by ex, ey,
        for node 2 for BM2D, ex, ez for node 1 followed by ex, ez for node 2 for GRIL.

5.      For BAX3 elements only the offsets at the end nodes may be defined and the ey values at each end of the
        beam must be equal as must the ez values.

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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-11
ASAS (Linear) User Manual                                                                                    Appendix A


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.




                                Figure A.8 Beam Offsets Defined using OFFG or OFSK

Notes


1.      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.

2.      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.

3.      For TCBM elements 9 values of offset are required, ex, ey, ez for nodes 1, 2 and 3. The offsets for the
        middle node must equate to a local ex of zero.

4.      For BM2D elements, 4 values of offset are required, ex, ey, values for node 1 followed by ex, ey for node
        2.

5.      For BAX3 elements only the offsets at the end nodes may be defined and the ey values at each end of the
        beam must be equal as must the ez values.

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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-12
ASAS (Linear) User Manual                                                                              Appendix A

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.9 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 TCBM elements 9 values of offset are required, ex, ey, ez for nodes 1, 2 and 3. The offsets for the
        middle node must equate to a local ex of zero.

3.      For BM2D elements 4 values of coordinates are required, x,y for end 1 followed by x,y for end2.

4.      For BM2D elements, 4 values of offset are required, ex, ey, values for node 1 followed by ex, ey for node
        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 (Linear) User Manual                                                                              Appendix A

A.4 Stepped Beams
The element types BEAM, BM2D, BM3D, GRIL and TUBE can have stepped changes in the geometric
properties along the length of a member. Each set of properties define one constant prismatic section of the
beam.

Stepped beam properties are defined by an optional STEP command in the Geometric Properties Data (Section
5.2.5). STEP commands for a beam occur immediately following the Geometric Properties data for that beam.

For a stepped beam the local axes apply to the whole element and are defined by the position of the two end
points and, in the case of BM3D and TUBE, by additional data in the geometric properties for the first section.

Each stepped section must be defined in order starting with the section adjacent to node 1. There is no restriction
on the number of sections which can be defined for a member. The length of the first section is defined at the
end of the basic set of geometric properties. For example, the 5 geometric properties required for a tube are
increased to 6. Each subsequent section is defined by a STEP command with the new properties for that section
and the section length.

For TUBE and BM3D the data defining the local axes should be omitted from the STEP command. Therefore,
BEAM, BM2D, BM3D, GRIL and TUBE require 5, 4, 7, 5 and 3 properties respectively for each step.

The length of one section (including the first) may be omitted. The length of this section will then be calculated
by the program from the coordinates of the end nodes and any specified offsets.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-14
ASAS (Linear) User Manual                                                                              Appendix A

A.5 Shell Offsets
The element types QUS4, TCS6 and TCS8 can have rigid offsets defined at each node.

It is normally assumed that the nodal coordinates of a shell element define the mid-surface geometry.
Sometimes, however, the mid-surface is offset from this plane and rigid offsets may be used to model this
situation.

Rigid offsets may be defined by the OFFS 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 shell with offsets.

An offset shell 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 position of the element mid-surface after the offsets have been taken
into account. If the member has no offsets then X’,Y’,Z’ and X”,Y”,Z” are coincident.

The local offsets are defined as the distances from the physical position of the shell mid-surface to the nodes,
measured in the local Z’ axis system.

Positive value of the local offset ez is as shown:



                         Z'
                                                  nodal surface


                                Node i

                    i
                  ez      Z''

                                                  physical shell
                                                  mid-surface


                                         Figure A.10 Sign Conventions for Shell Offsets

Note


The command has the keyword OFFS followed by ez value for each node. If the element has constant offset then
only one value is required.

Example


Example of a QUS4 with uniform thickness and offset

       175       QUS4           0.2
       :         OFFS           0.5




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-15
ASAS (Linear) User Manual                                                                              Appendix A

A.6 Laminated Shells
Composite shells may be modelled using the special laminate facility of the QUS4, TCS6 and TCS8 elements.
The composite is specified by defining the material properties, thickness and fibre orientation of each individual
lamina through the thickness of the composite. ASAS then calculates equivalent properties for the whole
composite section.

The material properties for each lamina are defined in the material data block. The laminae may be defined as
isotropic, anisotropic or orthotropic. For anisotropic laminae the out-of-plane coefficients of the stiffness matrix
will be ignored since it is assumed that each lamina acts as a membrane. The bending stiffness of the composite
section is derived when ASAS integrates the membrane properties of each layer over the section as a whole. The
materials used for laminae should not use a skew integer, instead the orientation should be defined by the fibre
angle.

In addition to defining the material for each individual laminae, a LAMI material must be assigned to the
element. This material defines the density of the section as a whole (the density of individual laminae is not
used), and also the direction of the material axis if a skew integer is specified. The equivalent material data
calculated by ASAS is also stored under the material integer of the element.

If an element is laminated, it must have both LAMI material and LAMI geometry data assigned to it. Elements
having the same LAMI material definition must also have the same LAMI geometry definition. However
elements with the same LAMI geometry definition may use different LAMI material definitions to allow for
differing material skews that may be specified for the same laminate.

The layup of a composite element is defined as part of the geometry definition for the element following the
nodal thicknesses. For a symmetric composite it is only necessary to define half of the layup. The material,
thickness and fibre orientation is defined for each layer in turn working from the bottom surface (on the elements
negative Z face) towards the top. The thicknesses of the laminae will be scaled to give the total nodal
thicknesses as defined in the geometry definition. Thus if a variable thickness element is defined then the
individual constituent laminae will also vary in thickness accordingly. The fibre orientation angle is defined
with respect to the material axes, which in turn is related to the projection of the global X axis, or the skew X
axis, defined on the elements LAMI material definition.

Both stress and strain results are calculated for QUS4, TCS6 and TCS8 elements. By default the element
stresses are printed (and written to plot files). If strains are required then the option STRN should be specified in
the OPTIONS data of the preliminary data. Processing of the stresses for individual layers of the composite is
undertaken by the POST program.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-16
ASAS (Linear) User Manual                                                                                                   Appendix A

Example

A simple mesh of TCS6 and TCS8 elements are to be modelled with a two layer lamina, the fibres of which are
oriented at ±45°. The material Xm axis is defined to coincide with the global Y axis.
                       12              13                14              15                                        16

                                                                                  Xe3
                                   Xe1
                                                                       Xe2                              Ye3
                           8                               9                 10                                        11

                                                  Ye1
                                                           60°

                               1          2        3           4 Ye2         5                    6                7
                                                Mesh showing element local axes
                    Xm
                                                                       Xm                                               Xm
                                                                        a1                                    a2


                                     Ym                                      Ym                                              Ym

                  Material Axes                                Layer 1                                      Layer 2
                                                     (positive fibre orientation)                 (negative fibre orientation)


                     Figure A.11 Example of Use of Laminated Material with Shell Elements

      ELEM
        MATP 1
        TCS8 1 8 12 13 14 9 3 2                              1
        MATP 2
        TCS6 3 9 14 10 5 4                                   2
        MATP 3
        TCS8 5 10 14 15 16 11 7 5                            1
      END
      MATE
          1    1   LAMI 0.001
          2    1   LAMI 0.001
          3    1   LAMI 0.001
        11         ORTH 0.001
      :            40.E+6 1.E+6 0.0                          0.5E+6 0.5E+6 0.5E+6 0.25 0.0 0.0
      :            1.0 1.0 1.0
      END
      GEOM
        1 TCS8 1.0
      : LAMI 2 0
      :     11   0.5    45.0
      :     11   0.5 -45.0
        2 TCS6 1.0
      : LAMI 2 0
      :     11   0.5    45.0
      :     11   0.5 -45.0
      END
      SKEW
        1    0.0     1.0 0.0    1.0                              0.0    0.0
      END
Reference:           ESR100792, “Implementation of Composite Shell Analysis in ASASH11”




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                             Page A-17
ASAS (Linear) User Manual                                                                                      Appendix A

A.7 Section Libraries
As an alternative to defining flexural properties explicitly for beam type elements BEAM, BM2D, BM3D, GRIL
and TUBE it is possible to utilise section definitions where a profile and physical dimensions are supplied. The
sections can either be defined using a SECT data block (see Section 5.2.6) or using an external Section Library
file which can contain either standard and/or user defined sections. Utilisation of section libraries makes for
more compact data files and ensures a greater degree of data validity.

Only one section library file may be used for a given analysis. This may be a standard library file supplied with
ASAS, or a library file created by the user using program SECTIONS.

A typical standard library called AISCLB is for AISC wide flange sections. It contains the following sections:

            W36X300          W36X280           W36X260          W36X245          W36X230           W36X210   W36X194
            W36X182          W36X170           W36X160          W36X150          W36X135           W33X241   W33X221
            W33X201          W33X152           W33X141          W33X130          W33X118           W30X211   W30X191
            W30X173          W30X132           W30X124          W30X116          W30X108           W30X99    W27X178
            W27X161          W27X146           W27X114          W27X102          W27X94            W27X84    W24X162
            W24X146          W24X131           W24X117          W24X104          W24X94            W24X84    W24X76
            W24X68           W24X62            W24X55           W21X147          W21X132           W21X122   W21X111
            W21X101          W21X93            W21X83           W21X73           W21X68            W21X62    W21X57
            W21X50           W21X44            W18X119          W18X106          W18X97            W18X86    W18X76
            W18X71           W18X65            W18X60           W18X55           W18X50            W18X46    W18X40
            W18X35           W16X100           W16X89           W16X77           W16X67            W16X57    W16X50
            W16X45           W16X40            W16X36           W16X31           W16X26            W14X730   W14X665
            W14X605          W14X550           W14X500          W14X455          W14X426           W14X398   W14X370
            W14X342          W14X311           W14X283          W14X257          W14X233           W14X211   W14X193
            W14X176          W14X159           W14X145          W14X132          W14X120           W14X109   W14X99
            W14X90           W14X82            W14X74           W14X68           W14X61            W14X53    W14X48
            W14X43           W14X38            W14X34           W14X30           W14X26            W14X22    W12X336
            W12X305          W12X279           W12X252          W12X230          W12X210           W12X190   W12X170
            W12X152          W12X136           W12X120          W12X106          W12X96            W12X87    W12X79
            W12X72           W12X65            W12X58           W12X53           W12X50            W12X45    W12X40
            W12X35           W12X30            W12X26           W12X22           W12X19            W12X16    W12X14
            W10X112          W10X100           W10X88           W10X77           W10X68            W10X60    W10X54
            W10X49           W10X45            W10X39           W10X33           W10X30            W10X26    W10X22
            W10X19           W10X17            W10X15           W10X12           W8X67             W8X58     W8X48
            W8X40            W8X35             W8X31            W8X28            W8X24             W8X21     W8X18
            W8X15            W8X13             W8X10            W6X25            W6X20             W6X15     W6X16
            W6X12            W6X9              W5X19            W5X16            W4X13             M14X18    M12X11.8
            M10X9            M8X6.5            M6X20            M6X4.4           M5X18.9           M4X13     S24X121
            S24X106          S24X100           S24X90           S24X80           S20X96            S20X86    S20X75
            S20X66           S18X70            S18X54.7         S15X50           S15X42.9          S12X50    S12X40.8
            S12X35           S12X31.8          S10X35           S10X25.4         S8X23             S8X18.4   S7X20
            S7X15.3          S6X17.25          S6X12.5          S5X14.75         S5X10             S4X9.5    S4X7.7
            S3X7.5           S3X5.7




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-18
ASAS (Linear) User Manual                                                                              Appendix A

A.8 Beam Stresses
For beam element types BEAM, BM2D, BM3D, GRIL and TUBE, the stresses at the nodes of a member may be
requested in addition to forces and moments. In order to activate the beam stress calculation, the RESU
command must be specified together with either OPTION CBST (for no printing) or PBST (if printing required).
Note that beam stresses will only be computed and stored for members with section dimensions defined at both
ends of the member. The section definition may be specified either through the XSEC section data or an
external section library.

Beam stress results are saved to the database as result type ’ASAS BEAM STRESS’. There are 12 result
components at each element node for all beam and section types. These are:

SAX             Axial stress
SVY             Shear stress in Y
SVZ             Shear stress in Z
SVT             Maximum torsion shear stress
SBY_C           Maximum compressive bending stress about YY
SBZ_C           Maximum compressive bending stress about ZZ
SBY_T           Maximum tensile bending stress about YY
SBZ_T           Maximum tensile bending stress about ZZ
SXX.A           Combined stresses at point A
SXX.B           Combined stresses at point B
SXX.C           Combined stresses at point C
SXX.D           Combined stresses at point D

The following sections give details of the dimensional data required to define each section type and the equations
used to calculate the flexural properties and member stresses. The nomenclature used is defined as follows:

Dimensional:
            d            =                 section depth (in local Y direction)

            b            =                 section width (in local Z direction)

            t,tw,tf      =                 thickness; wall, web, flange

            D, ID, Dn =                    tube diameters; outer, inner, nominal

            ry, rz, rt   =                 radii of gyration; bending Y, bending Z, torsional


Flexural:
            Ax, Ay, Az =                   section area; cross section, Y and Z shear areas

            Ix, Iy, Iz   =                 sectional inertias; torsional, minor and major bending




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-19
ASAS (Linear) User Manual                                                                               Appendix A

Acting Forces and Stresses:
            Fx                             =           axial force

            Mx, My, Mz                     =           moments; torsion, minor (Y) bending, major (Z) bending

            Q y, Q z                       =           shear forces Y,Z

            fa                             =           computed axial stress

            fby, fbz                       =           computed bending stresses in Y/Z local bending planes

            ftx                            =           torsion shear for tubes

            fty, ftz                       =           torsion shear in web and flange plates of boxes

            fvy, fvz                       =           shear stresses Y, Z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page A-20
TUB
ASAS (Linear) User Manual                                                                                Appendix A

                                                 Tubes of Circular Section


Dimensional Properties:                D t


where       D     is the outer diameter

            t     is the wall thickness




Flexural Property Formulae:

                          π
             Ax =              (D2 - ID2)                        where        ID = D-2t
                           4
                          3π     (D4 - ID4)
             Ay =
                          16 (D2 + ID2 + D . ID)
             Az =         Ay
                           π      4
             Ix =               (D -ID4)
                          32
             I y = Iz = I x
                        2
Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =           Fx/Ax                                           FA =       f a - f bz
                          My D
             f by =            Iy                                              FB =          f a - f by
                           2
                          Mz D
             f bz =            Iz                                              FC =          f a +f bz
                           2
                          Mx D
             f tx =            Ix                                              FD =          f a +f by
                           2
             f vy =       Qy / A y

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page A-21
FBI
ASAS (Linear) User Manual                                                                                                     Appendix A

                                                     Fabricated I-Section
                                                                                                             Y
                                                                                                         b
Dimensional Properties: d b tf tw [b2 tf2]                                               A                                       B

where       d     is the beam depth                                                                tf
                                                                                                                                      d
             b    is the top flange width                                                                                 tw
                                                                                         Z                                                Z
             t f is the top flange thickness
             t w is the web thickness                                                              tf2

            b2    is the bottom flange width
                  if omitted b2 is assumed the same as b                                D                                         C
                                                                                                                     b2
            tf2   is the bottom flange thickness
                  if omitted tf2 is assumed the same as tf                                                       Y


Flexural Property Formulae:
          Ay =     dt w
                          4
             Az =           bt f
                          3

Other flexural properties taken from ASAS data


Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
             fa =        Fx/Ax                                                 FA =          f a + f by - f bz
                          My b
             f by =                                                            FB =          f a - f by - f bz
                          2I y

                          Mz d
             f bz =                                                            FC =          f a - f by + f bz
                          2I z

             f vy =       Qy / A y                                             FD =          f a + f by + f bz

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                           Page A-22
WF
ASAS (Linear) User Manual                                                                                       Appendix A

                                             Wide Flanged Rolled I-Section


Dimensional Properties: d            b t f t w [f]


where       d     is the beam depth

             b    is the flange width

             t f is the flange thickness
             t w is the web thickness
            f     is optional fillet radius (zero if not specified)

Flexural Property Formulae:
             Ay =         dt w
                          4
             Az =           bt f
                          3

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =           Fx/Ax                                           FA =       f a + f by - f bz
                          My b
             f by =                                                            FB =          f a - f by - f bz
                          2I y

                          Mz d
             f bz =                                                            FC =          f a - f by + f bz
                          2I z

             f vy =       Qy / A y                                             FD =          f a + f by + f bz

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-23
RHS
ASAS (Linear) User Manual                                                                                                  Appendix A

                                                    Rolled Hollow Section



Dimensional Properties: d b t [f]

where       d       is the beam depth

            b       is the beam width

            t       is the thickness

            f       is the optional fillet radius (zero if not specified)


Flexural Property Formulae:
             Ay =         2 t (d- 2 t)

             Az =         2 t (b- 2 t)

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =               Fx / A x                                    FA         =      f a + f by - f bz

                             My b
             f by     =                                                        FB           =           f a - f by - f bz
                             2I y

                      =      Mz d                                                           =           f a - f by + f bz
             f bz                                                              FC
                             2I z
             f ty     =      M x / 2 t A box                                   FD           =           f a + f by + f bz
             f tz     =      M x / 2 t A box
where        A box =         2(b- t)(d- t)

             f vy     =      f ty + Q y / A y

             f vz     =      f tz + Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                        Page A-24
BOX
ASAS (Linear) User Manual                                                                                                  Appendix A

                                                        Fabricated Box Section



                                                                                                            Y         tf    B
                                                                                         A
Dimensional Properties: d b tf tw [tf2]

where       d       is the beam depth
                                                                                                    tw           tw
            b       is the beam width                                                                                            d
            tf      is the thickness of the ’top’ plate                            Z                                                 Z

            tf2     is the thickness of the ’bottom’ plate
                    if omitted tf2 is assumed the same as tf
                                                                                                                    tf2
            tw      is the thickness of the ’side’ plates
                                                                                         D                                  C
                                                                                                        b
Flexural Property Formulae:                                                                                     Y
             Ay     =       2 t w (d- t f - t f 2)

             Az =           ( t f + t f 2) (b-2 t w )

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =                Fx / A x                                   FA         =      f a + f by - f bz

                               My b
             f by       =                                                      FB            =          f a - f by - f bz
                               2I y

                        =      Mz d                                            FC            =          f a - f by + f bz
             f bz
                               2I z
             f ty       =     M x / 2 t w A box                                FD            =          f a + f by + f bz
             f tz       =     M x / 2 t f A box
where        A box =          2(b-t w )(d-t f )
             f vy =           f ty + Q y / A y                                 f vz          =          f tz + Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                           Page A-25
PRI
ASAS (Linear) User Manual                                                                                                Appendix A

                                                 Solid Rectangular Section


                                                                                                        Y
Dimensional Properties:           d b                                             A                               B

where       d     is the beam depth

            b     is the beam width                                                                                       d
                                                                                   Z                                  Z

Flexural Property Formulae:
                          2
             Ay =           bd
                          3
                                                                                  D                               C
                          2                                                                             Y
             Az   =         bd
                          3                                                                             b

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
             fa   =       Fx / A x                                             FA =          f a + f by - f bz

                          My b
             f by =                                                            FB =          f a - f by - f bz
                          2I y

                          Mz d                                                               f a - f by + f bz
             f bz =                                                            FC =
                          2I z

                          Mx / α b d
                                  2
             f ty =                                                            FD = f a + f by + f bz

                          Mx / α b d
                                        2
             f tz =

             f vy = f ty + Q y / A y

             f vz = f tz + Qz / A z

f ty and f tz maximum values in the Y and Z directions and occur on the edges of the cross section at mid-depth
and mid-width positions respectively. The value of α is approximated using the following formulae:
                                    d                 d                                                     d
            α     =       - 0.0029 ( - 1 )2 + 0.0333 ( - 1) + 0.208                        for 0.0 <          < 6.0
                                 d b                  b d                                                   b
            α     =       0.0033 + 0.279 for 6.0 < < 10.0
                                 b                       b
                          1                                  d
            α     =                          for 10.0 <        <∞
                          3                                  b




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                         Page A-26
CHAN
ASAS (Linear) User Manual                                                                                       Appendix A

                                                         Channel Section


Dimensional Properties:            d b t f t w [f]



where       d     is the beam depth

            b     is the flange width

             t f is the flange thickness
             t w is the web thickness
            f     is optional fillet radius (zero if not specified)


Flexural Property Formulae:
             Ay =         dt w
                          4
             Az =           bt f
                          3

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =            Fx / A x                                       FA =       f a + f by - f bz

                          My y
             f by =                       at locations A and D                 FB =          f a - f by - f bz
                           Iy

                                 (b- y) at locations B and C
             f by =       My                                                   FC =          f a - f by + f bz
                                   Iy
                          Mz d                                                               f a + f by + f bz
             f bz =                                                            FD =
                          2I z

             f vy =       Qy / A y

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-27
TEE
ASAS (Linear) User Manual                                                                                        Appendix A

                                                             Tee Section


Dimensional Properties:            d b tf t w [f]



where       d     is the beam depth

            b     is the flange width

            tf    is the flange thickness

             t w is the web thickness
            f     is optional fillet radius (zero if not specified)


Flexural Property Formulae:
                          2
             Ay =           dt w
                          3
                          2
             Az =           bt f
                          3

Other flexural properties taken from ASAS data or from DESI/PROF commands.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =            Fx / A x                                       FA =       f a + f by - f bz

                          Mz z
             f bz =                        at locations A and B                FB =          f a - f by - f bz
                           Iz
                          M z (d - z) at locations C and D                                   f a + f bz - f b y
             f bz =                                                            FC =
                               Iz
                          My b
             f by =                        at locations A and B                FD =          f a + f bz + f b y
                          2I y

                          My tw
             f by =                        at locations C and D
                           2I y

             f vy =       Qy / A y

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page A-28
ANGL
ASAS (Linear) User Manual                                                                                       Appendix A

                                                           Angle Section


Dimensional Properties:           d b t [f]


where       d     is the beam depth

            b     is the beam width

             t    is the thickness
            f     is optional fillet radius (zero if not specified)


Flexural Property Formulae:
                          2
             Ay =           dt
                          3
                          2
             Az =           bt
                          3

Other flexural properties taken from ASAS data.

Stress Formulae:                                                 Combined Stresses (at positions on above diagram)
          fa =            Fx / A x                                       FA =       f a + f by - f bz

                          M z (d- z)
             f bz =                          at locations C and D              FB =          f a - f by - f bz
                              Iz
                          Mz z
             f bz =                          at locations A and B              FC =          f a + f by + f bz
                           Iz

                          My y
             f by =                          at locations A and D              FD =          f a + f by + f bz
                           Iy


                          M y (b- y)
             f by =                          at location B
                              Iy


                          M y (y − t)
             f by =                          at location C
                               Iy




             f vy =       Qy / A y

             f vz =       Qz / A z




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page A-29
ASAS (Linear) User Manual                                                                                       Appendix A

A.9 Finite Element Description Sheets

                                                                                                               Beams
BEAM     2 node beams with constant or stepped cross sections and rigid offsets for three
BM3D     dimensional structures.
BM2D     2 node frame and grillage beams with constant or stepped cross sections and rigid
GRIL     offsets for two dimensional structures.
BMGN     2 node tapered beam with arbitrary local axes and rigid offsets.
CURB     2 node beam with constant curvature and uniform cross section.
FLA2     2 node axial element with varying cross section.
FLA3     3 node axial element with varying cross section.
TUBE     2 node circular tube element with constant or stepped 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.
BR32     32 node brick.
CB15     Special 15 node solid wedge element for modelling crack tip singularities in fracture
         mechanics problems.
TET4     4 node straight edged tetrahedra.
TE10     10 node tetrahedra.


                                                                                                Axisymmetric Elements
ASH2     Axisymmetric shell with varying thickness for both axisymmetric and harmonic
AHH2     loading.
QUX4
QUX8 Axisymmetric quadrilateral solid with straight or curved edges for both
         axisymmetric
QHX4     and harmonic loading.
QHX8
TRX3
TRX6     Axisymmetric triangular solid with straight or curved edges for both axisymmetric
         and
THX3     harmonic loading.
THX6
CTX6     Axisymmetric triangular solid with stress singularity for axisymmetrically cracked
         bodies with axisymmetric loading
                                                                                                        Membrane Elements
QUM4 4 node quadrilateral membrane with varying thickness.
QUM8 8 node isoparametric quadrilateral membrane with varying thickness.
TRM3 3 node triangular membrane with constant stress.
TRM6 6 node isoparametric triangular membrane with varying thickness.
MOQ4 4 node warped semi monocoque element with optional bi-directional stiffeners.
CK11 11 node planar symmetric membrane elements for linear fracture mechanics.
SCK7 7 node planar symmetric membrane elements for linear fracture mechanics.
CTM6 Triangular membrane with stress singularity to model the crack tip in fracture
     mechanics problems.
MEM4 4 node plane rectangular membrane for in-plane shear.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page A-30
ASAS (Linear) User Manual                                                                                       Appendix A

                              Finite Element Description Sheets Continued
                                                                                                Stress-based elements
Force equilibrium elements are a special range of hybrid elements designed for analysing thin-walled structures where shear
flow is a significant characteristic. They are particularly useful in analysing stiffened panel, fabricated and monocoque
structures.
FAX3     3 node straight force equilibrium axial stiffener with linearly varying load.
SQM4     4 node straight-sided stress-based quadrilateral membrane element.
STM6     6 node straight-sided stress-based triangular membrane element.
SQM8     8 node straight-sided stress-based quadrilateral membrane element.
TSP6     6 node straight-sided force equilibrium triangular shear panel.
WAP8     8 node straight-sided force equilibrium quadrilateral shear panel.
WAPT     10 node force equilibrium transition shear panel to allow mesh densities
           to be graded.
BAX3     3 node force equilibrium straight beam element compatible with other
         force
         equilibrium elements.


                                                                                                        Shell elements
GCS6     6 node triangular semi-loof curved shell element.
GCS8     8 node quadrilateral semi-loof curved shell element.
GCB3     3 node curved beam compatible with semi-loof shell elements.
TCS6     6 node triangular element for modelling thick shell applications.
TCS8     8 node quadrilateral element for modelling thick shell applications.
TCBM     3 node beam element for modelling thick shell applications.
TBC3     3 node triangular shell element.
QUS4     4 node quadrilateral shell element.
SLB8     8 node thick plate bending element for modelling slab type structures.
TRB3     3 node triangular plate for modelling thin slab structures.
Note that the TCS6, TCS8 and QUS4 elements can have laminated composite material
        properties.


                                                                                                        Sandwich elements

The sandwich elements consist of solid core material with a membrane panel on the top
        and bottom faces.
SND6 6 node triangular wedge sandwich element.
SND8 8 node quadrilateral brick sandwich element.
SN12 12 node triangular wedge sandwich element.
SN16 16 node quadrilateral brick sandwich element.



                                                                                                          Special elements
SPR1     Translational spring element between 2 nodes
SPR2
A generalised stiffness matrix may be applied to an arbitrary set of nodes.
         See Section 5.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page A-31
            Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.




                                                                                                                                                                                                                                                                                                         ASAS (Linear) User Manual
                                                                                                                                       Analysis Types                 Material Types            Mass Modelling                                      Load Types
                                                                                                                    Element
                                                                                                                     Type     Linear       Nat       Heat                 Anisotro     Orth/   Cons     Lumped   Nodal   Prescr   Press   Distr   Temp     Face   Body     Centr   Ang   Tank
                                                                                                                                                              Isotropic
                                                                                                                              Stress       Freq     Conduct                 pic        Lami    Mass      Mass    Loads    Disp    Loads   Loads   Loads    Temp   Forces   Loads   Acc   Loads

                                                                                                                    AHH2        ♦            ♦                   ♦           ♦                   ♦         ♦               ♦       ♦       ♦                ♦       ♦       ♦
                                                                                                                    ASH2        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦        ♦       ♦       ♦
                                                                                                                    BAX3        ♦            ♦                   ♦                                         ♦      ♦        ♦                                ♦
                                                                                                                    BEAM        ♦            ♦          ♦        ♦                               ♦         ♦      ♦        ♦               ♦                ♦       ♦       ♦

                                                                                                                    BMGN        ♦            ♦                   ♦                                         ♦      ♦        ♦                                        ♦
                                                                                                                    BM2D        ♦            ♦          ♦        ♦                               ♦         ♦      ♦        ♦               ♦       ♦                ♦       ♦
                                                                                                                    BM3D        ♦            ♦          ♦        ♦                               ♦         ♦      ♦        ♦               ♦       ♦                ♦       ♦      ♦
                                                                                                                    BRK6        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦

                                                                                                                    BRK8        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                    BR15        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                    BR20        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                    BR32        ♦            ♦          ♦        ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦

                                                                                                                    CB15        ♦            ♦                   ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                    CK11        ♦            ♦                   ♦                                                ♦        ♦       ♦                                ♦              ♦
                                                                                                                    CTM6        ♦            ♦                   ♦           ♦                   ♦         ♦      ♦        ♦       ♦       ♦       ♦                ♦       ♦
                                                                                                                    CTX6        ♦            ♦                   ♦           ♦                   ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦

                                                                                                                    CURB        ♦            ♦          ♦        ♦                                         ♦      ♦        ♦                                        ♦              ♦
                                                                                                                    FAX3        ♦            ♦                   ♦                                         ♦      ♦        ♦                       ♦                ♦              ♦
                                                                                                                    FLA2        ♦            ♦          ♦        ♦                               ♦         ♦      ♦        ♦                       ♦                ♦       ♦      ♦
                                                                                                                    FLA3        ♦            ♦          ♦        ♦                               ♦         ♦      ♦        ♦                       ♦                ♦       ♦      ♦



                                                                                                                                                                                               Table A.1 Overview of ASAS Elements




                                                                                                                                                                                                                                                                                                 Appendix A
Page A-32
          Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.




                                                                                                                                                                                                                                                                                                      ASAS (Linear) User Manual
                                                                                                                                     Analysis Types                 Material Types           Mass Modelling                                      Load Types
                                                                                                                  Element
                                                                                                                   Type     Linear       Nat       Heat                 Anisotro     Orth/   Cons    Lumped   Nodal   Prescr   Press   Distr   Temp     Face   Body     Centr   Ang   Tank
                                                                                                                                                            Isotropic
                                                                                                                            Stress       Freq     Conduct                 pic        Lami    Mass     Mass    Loads    Disp    Loads   Loads   Loads    Temp   Forces   Loads   Acc   Loads

                                                                                                                  GCB3        ♦            ♦          ♦        ♦                              ♦         ♦      ♦        ♦               ♦       ♦                ♦       ♦      ♦
                                                                                                                  GCS6        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦       ♦       ♦        ♦       ♦       ♦      ♦      ♦
                                                                                                                  GCS8        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦       ♦       ♦        ♦       ♦       ♦      ♦      ♦
                                                                                                                  GRIL        ♦            ♦          ♦        ♦                              ♦         ♦      ♦        ♦               ♦                        ♦

                                                                                                                  MEM4        ♦            ♦          ♦        ♦                                        ♦      ♦        ♦                                        ♦
                                                                                                                  MOQ4        ♦            ♦                               ♦                            ♦      ♦        ♦       ♦                                ♦                     ♦
                                                                                                                  QHX4        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                  QHX8        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦

                                                                                                                  QUM4        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦       ♦       ♦                ♦       ♦      ♦      ♦
                                                                                                                  QUM8        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦       ♦       ♦                ♦       ♦      ♦      ♦
                                                                                                                  QUS4        ♦            ♦          ♦        ♦           ♦          ♦       ♦         ♦      ♦        ♦       ♦       ♦       ♦        ♦       ♦       ♦      ♦      ♦
                                                                                                                  QUX4        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦

                                                                                                                  QUX8        ♦            ♦          ♦        ♦           ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                  SCK7        ♦            ♦          ♦        ♦                                               ♦        ♦       ♦                                ♦              ♦
                                                                                                                  SLB8        ♦            ♦          ♦        ♦           ♦                  ♦                ♦        ♦       ♦       ♦                ♦       ♦
                                                                                                                  SND6        ♦            ♦                               ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦

                                                                                                                  SND8        ♦            ♦                               ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                  SN12        ♦            ♦                               ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                  SN16        ♦            ♦                               ♦                  ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                  SPR1        ♦            ♦                                                                   ♦        ♦




                                                                                                                                                                                   Table A.1 Overview of ASAS Elements ...cont.




                                                                                                                                                                                                                                                                                              Appendix A
Page 33
          Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.




                                                                                                                                                                                                                                                                                                        ASAS (Linear) User Manual
                                                                                                                                     Analysis Types                 Material Types             Mass Modelling                                      Load Types
                                                                                                                  Element
                                                                                                                   Type     Linear       Nat       Heat                 Anisotro     Orth/     Cons    Lumped   Nodal   Prescr   Press   Distr   Temp     Face   Body     Centr   Ang   Tank
                                                                                                                                                            Isotropic
                                                                                                                            Stress       Freq     Conduct                 pic        Lami      Mass     Mass    Loads    Disp    Loads   Loads   Loads    Temp   Forces   Loads   Acc   Loads

                                                                                                                  SPR2        ♦            ♦                                                                     ♦        ♦
                                                                                                                  SQM4        ♦            ♦          ♦        ♦           ♦                              ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦      ♦
                                                                                                                  SQM8        ♦            ♦                   ♦           ♦                              ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦      ♦
                                                                                                                  STM6        ♦            ♦                   ♦           ♦                              ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦      ♦
                                                                                                                  TBC3        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦              ♦      ♦

                                                                                                                  TCBM        ♦            ♦          ♦        ♦                                ♦         ♦      ♦        ♦               ♦       ♦                ♦       ♦      ♦
                                                                                                                  TCS6        ♦            ♦          ♦        ♦           ♦          ♦         ♦         ♦      ♦        ♦       ♦       ♦       ♦        ♦       ♦       ♦      ♦      ♦
                                                                                                                  TCS8        ♦            ♦          ♦        ♦           ♦          ♦         ♦         ♦      ♦        ♦       ♦       ♦       ♦        ♦       ♦       ♦      ♦      ♦
                                                                                                                  TET4        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                  TE10        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦      ♦
                                                                                                                  THX3        ♦            ♦                   ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦

                                                                                                                  THX6        ♦            ♦                   ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                  TRB3        ♦            ♦          ♦        ♦           ♦                              ♦      ♦        ♦       ♦       ♦                ♦       ♦
                                                                                                                  TRM3        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦       ♦       ♦                ♦       ♦      ♦      ♦
                                                                                                                  TRM6        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦       ♦       ♦                ♦       ♦      ♦      ♦

                                                                                                                  TRX3        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                  TRX6        ♦            ♦          ♦        ♦           ♦                    ♦         ♦      ♦        ♦       ♦               ♦                ♦       ♦
                                                                                                                  TSP6        ♦            ♦                   ♦                                          ♦      ♦        ♦       ♦               ♦                ♦              ♦
                                                                                                                  TUBE        ♦            ♦          ♦        ♦                                ♦         ♦      ♦        ♦               ♦       ♦                ♦       ♦      ♦

                                                                                                                  WAP8        ♦            ♦                   ♦                                          ♦      ♦        ♦       ♦                                ♦              ♦
                                                                                                                  WAPT        ♦            ♦                   ♦                                          ♦      ♦        ♦       ♦                                ♦              ♦




                                                                                                                                                                                                                                                                                                Appendix A
                                                                                                                                                                                             Table A.1 Overview of ASAS Elements ...cont
Page 34
AHH2                                                                                                ASAS (Linear) User Manual


Straight Axisymmetric Shell with Varying Thickness for the Analysis of Thin or Thick
                                Axisymmetric Shells under Harmonic Loading

NUMBER OF NODES                            2

NODAL COORDINATES                          r, z
                                           (Note that r and z occupy the first and
                                           third fields on the line using an
                                           unnamed cartesian system. The
                                           second field must be input as zero.)

DEGREES OF FREEDOM                         R, Z, TH, RTH, RFI at each node.
                                           (Any skew system must be defined by 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                       t1            thickness at node 1 (> 0.0)
                                           t2            thickness at node 2 (> 0.0)
                                           Harno         Harmonic Number. (Integer)
                                                         The thickness varies linearly between node 1 and node 2.

MATERIAL PROPERTIES                        E             Modulus of elasticity
            isotropic:                     υ             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           10            coefficients of the local stress-strain matrix
                                           2             linear coefficients of expansion αss, αhh
                                                         (ρ, αss and αhh are not always needed)

LOAD TYPES                                 Standard load types listed in Appendix A.1
                                           Body Forces (Parallel to Z axis and zero harmonic only)
                                           Pressure Loads (Positive pressure is in the direction of the positive
                                                                 normal and is thus dependent on the node numbering.
                                           See diagram.)
                                           Temperature
                                           Face Temperature (Face 1 is on the -ve local Z side)
                                           Centrifugal Loads (rotation about Z axis and zero harmonic only)
                                           Nodal Loads must be defined per radian
                                           (Note, all loading is harmonic with specified amplitude)

MASS MODELLING                             Consistent Mass only

STRESS OUTPUT                              Membrane stress σss, σhh, σsh
                                           Bending moments/unit length Mss, Mhh, Msh
                                           Shear forces/unit length Qr’s,Qr’h
                                           All values are calculated at the element mid-side position



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-35
AHH2                                                                                                ASAS (Linear) User Manual


                                           In addition, RESU command in the preliminary data causes the saving of
                                           local stresses and von-Mises stress on bottom, middle and top surfaces to the
                                           results database. (Bottom surface is on the -ve local Z’ side).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-36
AHH2                                                                                                ASAS (Linear) User Manual


ANISOTROPIC MATRIX                             σss                  C1 C2       0      0    0            0      0     0              εss
                                               σhh                     C3       0      0    0            0      0     0              εhh
                                               σsh                              C4     0    0            0      0     0              εsh
                                               Mss       =                            C5t3 C6t3          0      0     0              Wss
                                               Mhh                                         C7t3          0      0     0              Whh
                                               Mhs                                                      C8t3    0     0              Whs
                                               Qr’s                                                            C9t    0              γr’s
                                               Qr’h                                                                  C10t            γr’h


                                                                                                                       Z         S

                                                                                                                            2



LOCAL AXES                                 Local S axis lies along the element from
                                           node 1 to node 2.                                                                     1
                                                                                                                            R'
                                           Local R’ axis is at right angles to S axis.
                                                                                                                                            R
SIGN CONVENTIONS                           Stress resultants are positive as shown.




LIMITATIONS                                radii must be ≥ 0.0
                                           length must be > 0.0

REFERENCE                                  “A Simple and Efficient Element for Axisymmetric Shells”.
                                           Zienkiewicz et al International Journal for Numerical Methods in
                                           Engineering Vol. II pp 1545 (1977).

                                           This element is the harmonically loaded version of the ASH2 element.


DATA EXAMPLES                              ELEM
                                           MATP          1
                                           AHH2          1      2      1
                                           AHH2         11    12       2
                                           END
                                           GEOM
                                           1          AHH2    0.25         0.25      2
                                           2          AHH2    0.37         0.37      2
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                           Page A-37
ASH2                                                                                                ASAS (Linear) User Manual



Straight Axisymmetric Shell with Varying Thickness for the Analysis of Thin or Thick
                Axisymmetric Shells Under Axisymmetric Loading

NUMBER OF NODES                            2

NODAL COORDINATES                          r, z
                                           (Note that r and z occupy the first and
                                           third fields on lines using an unnamed
                                           cartesian system. The second field
                                           must be input as zero.)

DEGREES OF FREEDOM                         R, Z, RTH at each node.
                                           (Any skew system must be defined by 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                       t1            thickness at node 1 (> 0.0)
                                           t2            thickness at node 2 (> 0.0)
                                                         (The thickness varies linearly between node 1 and node 2.
                                                         The value t2 may be omitted for an element with uniform
                                                         thicknesst1)

MATERIAL PROPERTIES                        E             Modulus of elasticity
            isotropic:                     ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           7             coefficients of the local stress-strain matrix
                                           2             linear coefficients of expansion αss, αhh
                                                         (ρ, αss and αhh are not always needed)

LOAD TYPES                                 Standard load types listed in Appendix A.1
                                           Body Forces (Parallel to Z axis only)
                                           Pressure Loads (Positive pressure is in the direction of the positive
                                                                  normal and is thus dependent on the node numbering.
                                           See diagram.)
                                           Temperature
                                           Face Temperatures (Face 1 is on the -ve local z side)
                                           Centrifugal Loads (rotation about Z axis only)
                                           Nodal Loads must be defined per radian.
                                           (Note, all loading must be axisymmetric)

MASS MODELLING                             Consistent Mass only

STRESS OUTPUT                              Membrane stress σss, σhh
                                           Bending moments/unit length Mss, Mhh
                                           Shear force/unit length Qr’s



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-38
ASH2                                                                                                ASAS (Linear) User Manual


                                           All values are calculated at the element mid-side
                                           In addition, RESU command in the preliminary data causes the saving of
                                           local stresses and von-Mises stress on bottom, middle and top surfaces to the
                                           results database. (Bottom surface is on the -ve local Z’ side).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-39
ASH2                                                                                                         ASAS (Linear) User Manual


ANISOTROPIC MATRIX                            σss                             C1 C2        0    0      0             εss
                                              σhh                                C3        0    0      0             εhh
                                              Mss                                            3
                                                                                          C4t C5t3     0             Wss
                                              Mhh               =                              C6t3    0             Whh
                                              Qr’s                                                    C7t3           γr’s


                                                                                                                     Z        S

LOCAL AXES                                 Local S axis lies along the element from                                      2
                                           node 1 to node 2.
                                           Local R’ axis is at right angles to S axis.

SIGN CONVENTIONS                           Stress resultants are positive as shown.                                           1
                                                                                                                         R'

                                                                                                                                       R

                                                       S
                                                               Qr's

                                             2




                                                   1                   Qr's



                                              R'




LIMITATIONS                                radii must be ≥ 0.0
                                           length must be > 0.0

REFERENCE                                  “A Simple and Efficient Element for Axisymmetric Shells”.
                                           Zienkiewicz et al International Journal for Numerical Methods in
                                           Engineering Vol. II pp 1545 (1977).

DATA EXAMPLES                              ELEM
                                           MATP            1
                                           ASH2                16       18     3      6
                                           ASH2                18       19     4      7
                                           END
                                           GEOM
                                           3 ASH2                     1.75     1.5
                                           4 ASH2                     1.5
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                             Page A-40
BAX3                                                                                                ASAS (Linear) User Manual



     Straight Three Dimensional Beam Bending Element with Tapered Cross-section
                    Arbitrary Local Axes Direction and Rigid Offsets
                              Combined with Axial Force Equilibrium Element

NUMBER OF NODES                            3

NODAL COORDINATES                          x, y, z (end nodes only)


DEGREES OF FREEDOM                         X, Y, Z, RX, RY, RZ, at end nodes, S at mid-side.
                                           The S freedom is parallel to the element and in the
                                           directions of the end node with the higher number.
                                           Skew systems may be applied to end nodes only.

GEOMETRIC PROPERTIES                       A1                             Cross-sectional area at end 1
                                           Iz”z”1                         2nd moment of area about local z”z” axis end 1
                                           Iy”y”1                         2nd moment of area about local y”y” axis end 1
                                           J1                             Torsion constant end 1
                                           Local Axis definition          See Section 5.2.5.4 and Appendix A.2.1
                                           Asy”1                          Shear area y” at end 1
                                           Asz”1                          Shear area z” at end 1
                                           A2                             Cross-sectional area at end 2
                                           Iz”z”2                         2nd moment of area about local z”z” axis end 2
                                           Iy”y”2                         2nd moment of area about local y”y” axis end 2
                                           J2                             Torsion constant end 2
                                           Asy”2                          Shear area y” at end 2
                                           Asz”2                          Shear area z” at end 2
                                           RINDIC Iz”z”                   Order of parametric interpolation of Iz”z”
                                                                          between end 1 and end 2 (Integer)
                                           RINDIC Iy”y”                   Order of parametric interpolation of Iy”y”
                                                                          between end 1 and end 2 (Integer)
                                           RINDIC J                       Order of parametric interpolation of J
                                                                          between end 1 and end 2 (Integer)

Notes on Geometric Properties


1.     If a section property at end 2 is identical to the corresponding property at end 1, the value at end 2 may
       be omitted.

2.     The value of the parameter RINDIC governs the variation of I and J along its length and can be one of
       the following.
                                                    omitted, 0, 1 linear taper
                                                    2                    quadratic taper
                                                    3                         cubic taper

3.     The cross-section area and shear areas are always interpolated linearly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-41
BAX3                                                                                                ASAS (Linear) User Manual


OFFSETS                                    BAX3 may have rigid offsets at each end, defined on the OFFG, OFFS,
                                           OFSK or OFCO commands. If offsets are used then ey1= ey2 and ez1=ez2, i.e.
                                           they must define a lateral translation of the element. For further details see
                                           Section 5.2.5.4 and Appendix A.3.


MATERIAL PROPERTIES                        E             Modulus of elasticity
        (isotropic only)                   ν             Poisson’s Ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume)
                                                         (α and ρ are not always needed)

LOAD TYPES                                 Nodal load and prescribed displacements.
                                           Body Force Load. (Note, the equivalent fixed end loads are evaluated in
                                           terms of equivalent end forces only and do not include equivalent end
                                           moments. Thus the overall effect is approximately correct.)

MASS MODELLING                             Lumped mass only

FORCE OUTPUT                               The forces are exerted by the nodes on the element and are related to the
                                           centroidal local axes.

                                           Distributed shear force/unit length along the centroidal axis
                                           Axial force and Axial stress at each end
                                           Transverse shear forces QY”, QZ” at each end
                                           Torque X”X” at each end
                                           Moments Y”Y” and Z”Z” at each end

                                           In addition, member stresses at the nodes of the element will be computed
                                           and saved to the results database by specifying the RESU command together
                                           with OPTION CBST or PBST. For further details, See Appendix A.8 and
                                           C.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-42
BAX3                                                                                                ASAS (Linear) User Manual


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 Y”
                                           lies in the direction defined in the geometric properties for the element, with
                                           its origin at end 1. Local Z” forms a right handed set with local X” and
                                           localY”.

                                           See also Section 5.2.5.4 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 a 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'




REFERENCES                                 Element is combination of BMGN and FAX3

                                           Przemieniecki, J.S. “Theory of Matrix Structural Analysis”,
                                           McGraw Hill, 1968.

                                           Robinson, J. “Integrated Theory of Finite Element Methods”,
                                           John Wiley, 1973.

                                           Atkins Research and Development BMGN and BAX3 Reports, 1982.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page A-43
                                                                                                    ASAS (Linear) User Manual


DATA EXAMPLES                              ELEM
                                           MATP         1
                                           BAX3         324         344        364        127           29
                                           END
                                           GEOM
                                           127       BAX3        0.35        1.24       0.52        0.073    126.5   742.3
                                           :                    57.4         0.2        0.15        0.6       2.02     0.71
                                           :                      0.09       0.42       0.18        1.0       1.0       1.0
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page A-44
BEAM                                                                                                ASAS (Linear) User Manual



  Three-dimensional Beam Bending Element with Uniform Cross-section and Special
                          Orientation of the Local Axes

NUMBER OF NODES                            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)


STEPS AND OFFSETS                          The STEP and OFFG, OFFS, OFSK, OFCO commands can be used to
                                           define changes in the geometric properties along its length and rigid offsets
                                           at each end. For further details see Section 5.2.5.4 and Appendix A.3 and
                                           A.4.

MATERIAL PROPERTIES                        E             Modulus of elasticity
        (isotropic only)                   ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Temperature
                                           Distributed Load Pattern            BL1, BL2, BL3, BL4, BL5,
                                                                               BL6, BL7, BL8, GL1, GP1
                                                                               GL4, GP4, GL5, GL6, GP6
                                                                               GL7, GP7
                                           Centrifugal Loads

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

                                           In addition, member stresses at the nodes of the element will be computed
                                           and saved to the results database by specifying the RESU command together



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-45
                                                                                                    ASAS (Linear) User Manual


                                           with OPTION CBST or PBST. For further details, See Appendix A.8 and
                                           C.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-46
BEAM                                                                                                ASAS (Linear) User Manual


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 5.2.5.4 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                                  Przemieniecki J. S. “Theory of Matrix Structural Analysis”
                                           McGraw Hill 1968.

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-47
BMGN                                                                                                ASAS (Linear) User Manual



                     Three Dimensional Beam Bending Element with Tapered
                  Cross-section, Arbitrary Local Axes Direction and Rigid Offsets


                                                                                           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
                                           A1                             Cross-sectional area at end 1
                                           Iz”z”1                         2nd moment of area about local Z”Z” axis end 1
                                           Iy”y”1                         2nd moment of area about local Y”Y” axis end 1
                                           J1                             Torsion constant end 1
                                           Local Axis definition          See Section 5.2.5.4 and Appendix A.2.1
                                           Asy”1                          Shear area Y” at end 1
                                           Asz”1                          Shear area Z” at end 1
                                           A2                             Cross-sectional area at end 2
                                           Iz”z”2                         2nd moment of area about local Z”Z” axis end 2
                                           Iy”y”2                         2nd moment of area about local Y”Y” axis end 2
                                           J2                             Torsion constant end 2
                                           Asy”2                          Shear area Y” at end 2
                                           Asz”2                          Shear area Z” at end 2
                                           RINDIC Iz”z”                   Order of parametric interpolation of Iz”z”
                                                                          between end 1 and end 2 (Integer)
                                           RINDIC Iy”y”                   Order of parametric interpolation of Iy’’y’’
                                                                          between end 1 and end 2 (Integer)
                                           RINDIC J                       Order of parametric interpolation of J
                                                                          between end 1 and end 2 (Integer)

Notes on Geometric Properties


1.     If a section property at end 2 is identical to the corresponding property at end 1, the value at end 2 may
       be omitted.

2.     The value of the parameter RINDIC governs the variation of I and J along its length and can be one of
       the following.
                                           omitted, 0, 1 linear taper
                                           2                  quadratic taper
                                           3                      cubic taper

3.     The cross-section area and shear areas are always interpolated linearly.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-48
BMGN                                                                                                ASAS (Linear) User Manual


OFFSETS                                    BMGN may have rigid offsets at each end, defined on the OFFG, OFFS,
                                           OFSK or OFCO commands. If offsets are used then ey1=ey2 and ez1=ez2, i.e.
                                           they must define a lateral translation of the element. For further details see
                                           Section 5.2.5.4 and Appendix A.3.


MATERIAL PROPERTIES                        E             Modulus of elasticity
                                           ν             Poisson’s Ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume)
                                                         (α and ρ are not always needed)

LOAD TYPES                                 Nodal loads and prescribed displacements.
                                           Body Force load. (Note, the equivalent fixed end loads are evaluated in
                                           terms of equivalent end forces only and do not include equivalent end
                                           moments. Thus the overall effect is approximately correct.)

MASS MODELLING                             Lumped mass only

FORCE OUTPUT                               The forces are exerted by the nodes on the element, and are related to the
                                           centroidal local axes.

                                           Axial force X”X” at each end
                                           Transverse shear forces QY”, QZ” at each end
                                           Torque X”X” at each end
                                           Moments Y”Y” and Z”Z” at each end

                                           In addition, member stresses at the nodes of the element will be computed
                                           and saved to the results database by specifying the RESU command together
                                           with OPTION CBST or PBST. For further details, See Appendix A.8 and
                                           C.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-49
BMGN                                                                                                ASAS (Linear) User Manual


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 Y”
                                           lies in the direction defined in the geometric properties for the element, with
                                           its origin at end 1. Local Z” forms a right handed set with local X” and
                                           localY”.

                                           See also Section 5.2.5.4 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 a clockwise rotation of end 2
                                                                               relative to node 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'



REFERENCES                                 Przemieniecki, J.S. “Theory of Matrix Structural Analysis”,
                                           McGraw Hill, 1968.
                                           Robinson, J. “Integrated Theory of Finite Element Methods”,
                                           John Wiley, 1973.
                                           Atkins Research and Development “BMGN Element Report”. 1982.

DATA EXAMPLES                              ELEM
                                           MATP 1
                                           BMGN 9          10     2
                                           BMGN 10          11        2
                                           END
                                           GEOM
                                           2        BMGN     0.35         1.24       0.52       0.073       126.5    742.3
                                           :                57.4          0.2        0.15       0.6          2.02      0.71
                                           :                    0.09      0.42       0.18       1.0          1.0       1.0
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page A-50
BM2D                                                                                                ASAS (Linear) User Manual



             Two-dimensional Beam Bending Element with Uniform Cross-section,
                               Lying in the Global XY Plane
                                                                                                        Y
NUMBER OF NODES                            2
                                                                                                                    2

NODAL COORDINATES                          x, y

                                                                                                        1
DEGREES OF FREEDOM                         X, Y, RZ at each node
                                                                                                                     X


GEOMETRIC PROPERTIES                       A             Cross-sectional area (≥ 0.0)
              (uniform)                    Iz”z”         Principal moment of inertia about the local Z” axis (≥ 0.0)
                                           As            Effective shear area (Shear strain is neglected if As is blank)

STEPS AND OFFSETS                          The STEP and OFFG, OFFS, OFSK, OFCO commands can be used to
                                           define changes in the geometric properties along the length and rigid offsets
                                           at each end. For further details see Appendix A.3, A.4 and Section 5.2.5.4.

MATERIAL PROPERTIES                        E   Modulus of elasticity
          (isotropic only)                 ν   Poisson’s ratio
                                           α   Linear coefficient of expansion
                                           ρ   Density (mass/unit volume). See Appendix -B
                                               (α and ρ are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1 except Angular Accelerations
                                           Temperature
                                           Distributed Load Patterns     BL1, BL2, BL3, BL4, BL5,
                                                                                  BL6, BL7, BL8, GL1, GP1
                                                                                  GL4, GP4, GL5, GL6, GP6
                                                                                  GL7, GP7
                                           Centrifugal Loads

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 shear QY” at each end
                                           Bending Moment Z”Z” at each end


                                           In addition, member stresses at the nodes of the element will be computed
                                           and saved to the results database by specifying the RESU command together
                                           with OPTION CBST or PBST. For further details, See Appendix A.8 and
                                           C.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-51
BM2D                                                                                                ASAS (Linear) User Manual


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 the offsets are all 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 Z direction. Local Y” forms a right handed set with
                                           local X” and local Z”.

                                           See also Section 5.2.5.4 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'

                                                     1                  2                 Shear QY”          +ve
                                                                                 X'
                                                                                          Moment Z”Z”        +ve




LIMITATIONS                                Length must be >0.0

REFERENCE                                  Przemieniecki J.S. “Theory of Matrix Structural Analysis”
                                           McGraw Hill 1968

DATA EXAMPLES                              ELEM
                                           MATP          1
                                           BM2D 9            10     3
                                           BM2D 10           11     2
                                           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-52
BM3D                                                                                                ASAS (Linear) User Manual


     Three-dimensional Beam Bending Element with Uniform Cross-section and any
                           Orientation of the Local Axes

NUMBER OF NODES                            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)
                                           Local Axis definition          See Section 5.2.5.4 and Appendix A.2.1
                                           Asy”                           Effective shear area in Y” direction
                                                                          (Y” shear strain is neglected if Asy” is blank)
                                           Asz”                           Effective shear area in Z” direction
                                                                          (Z” shear strain is neglected if Asz” is blank)

STEPS AND OFFSETS                          The STEP and OFFG, OFFS, OFSK, OFCO commands can be used to
                                           define changes in the geometric properties along its length and rigid offsets
                                           at each end. For further details see Appendix A.3, A.4 and Section 5.2.5.4.

MATERIAL PROPERTIES                        E             Modulus of elasticity
        (isotropic only)                   ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Temperature
                                           Distributed Load Patterns BL1, BL2, BL3, BL4, BL5,
                                                                               BL6, BL7, BL8, GL1, GP1
                                                                               GL4, GP4, GL5, GL6, GP6
                                                                               GL7, GP7
                                           Centrifugal Loads

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-53
BM3D                                                                                                ASAS (Linear) User Manual


                                           In addition, member stresses at the nodes of the element will be computed
                                           and saved to the results database by specifying the RESU command together
                                           with OPTION CBST or PBST. For further details, See Appendix A.8 and
                                           C.7.

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 Y”
                                           lies in the direction defined in the geometric properties for the element, with
                                           its origin at end 1. Local Z” forms a right handed set with local X” and
                                           localY”.

                                           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 5.2.5.4 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 toward end 2
                                           Bending moment            positive for sagging
                                           Shear QY”                +ve                Shear QZ”              +ve
                                           Moment Z”Z”              +ve                     Moment Y”Y”       +ve




LIMITATIONS                                Length must be >0.0

REFERENCE                                  Przemieniecki J. S. “Theory of Matrix Structural Analysis”
                                           McGraw Hill 1968

DATA EXAMPLES                              ELEM
                                           MATP 1
                                           BM3D   9           10      3
                                           BM3D       10      11      2
                                           END
                                           GEOM
                                           3 BM3D          39.2       2006.3         1987.0 3124.8 -1.4             2.3 -18.1




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page A-54
                                                                                                    ASAS (Linear) User Manual


                                           :              32.8           13.7
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-55
BRK6                                                                                                ASAS (Linear) User Manual



                  Isoparametric Brick Element with Quasi-linear Stress Variation

NUMBER OF NODES                            6

NODAL COORDINATES                          x, y, z

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       None

MATERIAL PROPERTIES                        E             Modulus of elasticity
            isotropic:                     ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           21            coefficients of the global 3-D stress-strain matrix
                                           6             linear coefficients of expansion αxx, αyy, αzz, αxy, αyz, αzx
                                                         related to the global axes.
                                                         (ρ and the expansion coefficients are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Pressure Loads (on any face, +ve towards the element centre)
                                           Temperature
                                           Centrifugal Loads

MASS MODELLING                             Consistent Mass (used by default)
                                           Lumped Mass

STRESS OUTPUT                              Direct stresses σxx, σyy, σzz and shear stresses σxy, σyz, σzx at each node
                                           related to the global axes.

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting
                                           with a triangular face.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-56
BRK6                                                                                                ASAS (Linear) User Manual


ANISOTROPIC MATRIX                           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


LOCAL AXES                                 The orientation of the stress output and the input of anisotropic material data
                                           can be related to a local axis system. See Appendix A.2.3.

SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz
                                           +ve for tension

                                           Shear stresses σxy, σyz, σzx
                                           +ve as shown




LIMITATIONS                                Coincident nodes are not permitted

REFERENCE                                  Zienkiewicz O. C. “The Finite Element Method in Engineering Science”
                                           McGraw Hill 1971

DATA EXAMPLES                              ELEM
                                           MATP 1
                                           BRK6       40      41      31     20      21      11
                                           BRK6       90      91      81     70      71      81
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page A-57
BRK8                                                                                                ASAS (Linear) User Manual



                  Isoparametric Brick Element with Quasi-linear Stress Variation

NUMBER OF NODES                            8

NODAL COORDINATES                          x, y, z

DEGREES OF FREEDOM                         X, Y, Z at each node

GEOMETRIC PROPERTIES                       None


MATERIAL PROPERTIES                        E             Modulus of elasticity
                      isotropic:           ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           21            coefficients of the global 3-D stress-strain matrix
                                           6             linear coefficients of expansion αxx, αyy, αzz, αxy, αyz, αzx
                                                         related to the global axes.
                                                         (ρ and the expansion coefficients are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Pressure Loads (on any face, +ve towards the element centre)
                                           Temperature
                                           Centrifugal Loads

MASS MODELLING                             Consistent Mass (used by default)
                                           Lumped Mass

STRESS OUTPUT                              Direct stresses σxx, σyy, σzz and shear stresses σxy, σyz, σzx at each node,
                                           related to the global axes.

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at
                                           any node.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-58
BRK8                                                                                                ASAS (Linear) User Manual


ANISOTROPIC MATRIX                           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


LOCAL AXES                                 The orientation of the stress output and the input of anisotropic material data
                                           can be related to a local axis system. See Appendix A.2.3.

SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz
                                           +ve for tension

                                           Shear stresses σxy, σyz, σzx
                                           +ve as shown



LIMITATIONS                                Coincident nodes are not permitted

REFERENCE                                  Korelc, J. and Wriggers, P. “An Efficient 3D Enhanced Strain Element with
                                           Taylor Expansion of the Shape Functions”, Computational Mechanics, Vol.
                                           19, 1996, pp 30-40.

DATA EXAMPLES                              ELEM
                                           MATP 1
                                           BRK8        20        21       31        30       120        121   131    130
                                           BRK8       120       121      131       130       220        221   231    230
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page A-59
BR15                                                                                                ASAS (Linear) User Manual



               Isoparametric Brick Element with Quasi-quadratic Stress 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 PROPERTIES                        E             Modulus of elasticity
            isotropic:                     ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           21            coefficients of the global 3-D stress-strain matrix
                                           6             linear coefficients of expansion αxx, αyy, αzz, αxy, αyz, αzx
                                                         related to the global axes.
                                                         (ρ and the expansion coefficients are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Pressure Loads (on any face, +ve towards the element centre)
                                           Temperature
                                           Centrifugal Loads

MASS MODELLING                             Consistent Mass (used by default)
                                           Lumped Mass

STRESS OUTPUT                              Direct stresses σxx, σyy, σzz and shear stresses σxy, σyz, σzx at each node,
                                           related to the global axes.

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting
                                           with a triangular face at a corner node.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-60
BR15                                                                                                ASAS (Linear) User Manual


ANISOTROPIC MATRIX                           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


LOCAL AXES                                 The orientation of the stress output and the input of anisotropic material data
                                           can be related to a local axis system. See Appendix A.2.3.

SIGN CONVENTIONS                           Direct stresses σxx, σyy, σzz
                                           +ve for tension

                                           Shear stresses σxy, σyz, σzx
                                           +ve as shown



LIMITATIONS                                Coincident nodes are not permitted

REFERENCE                                  Zienkiewicz O. C. “The Finite Element Method in Engineering Science”
                                           McGraw Hill 1971

DATA EXAMPLES                              ELEM
                                           MATP 1
                                           BR15 1 2 3                  4     5     6     11      13       15    21     22     23   24
                                           :    25 26
                                           BR15 101           102      103       104      105       106        111   113     115
                                           :         121      122      123       124      125       126
                                           END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                       Page A-61
BR20                                                                                                ASAS (Linear) User Manual



               Isoparametric Brick Element with Quasi-quadratic Stress 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                       None

MATERIAL PROPERTIES                        E             Modulus of elasticity
            isotropic:                     ν             Poisson’s ratio
                                           α             Linear coefficient of expansion
                                           ρ             Density (mass/unit volume). See Appendix -B
                                                         (α and ρ are not always needed)

                   anisotropic:            ρ             Density (mass/unit volume). See Appendix -B
                                           21            coefficients of the global 3-D stress-strain matrix
                                           6             linear coefficients of expansion αxx, αyy, αzz, αxy, αyz, αzx
                                                         related to the global axes.
                                                         (ρ and the expansion coefficients are not always needed)

LOAD TYPES                                 Standard types listed in Appendix A.1
                                           Pressure Loads (on any face, +ve towards the element centre)
                                           Temperature
                                           Centrifugal Loads

MASS MODELLING                             Consistent Mass (used by default)
                                           Lumped Mass

STRESS OUTPUT                              Direct stresses σxx, σyy, σzz and shear stresses σxy, σyz, σzx at each node,
                                           related to the global axes.

NODE NUMBERING                             The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at
                                           a corner node.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page A-62
B