Patran 2008 R1 Interface To Abaqus Preference Guide
This document was uploaded by user and they confirmed that they have the permission to share it. If you are author or own the copyright of this book, please report to us by using this DMCA report form. Report DMCA
Overview
Download & View Patran 2008 R1 Interface To Abaqus Preference Guide as PDF for free.
More details
- Words: 77,358
- Pages: 484
Patran 2008 r1 Interface To ABAQUS Preference Guide
Main Index
Corporate
Europe
Asia Pacific
MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 USA Telephone: (800) 345-2078 Fax: (714) 784-4056
MSC.Software GmbH Am Moosfeld 13 81829 Munich, Germany Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6
MSC.Software Japan Ltd. Shinjuku First West 8F 23-7 Nishi Shinjuku 1-Chome, Shinjuku-Ku Tokyo 160-0023, JAPAN Telephone: (81) (3)-6911-1200 Fax: (81) (3)-6911-1201
Worldwide Web www.mscsoftware.com
Disclaimer This documentation, as well as the software described in it, is furnished under license and may be used only in accordance with the terms of such license. MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. The concepts, methods, and examples presented in this text are for illustrative and educational purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem or design. MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. User Documentation: Copyright ©2008 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved. This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of MSC.Software Corporation is prohibited. The software described herein may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. Contains IBM XL Fortran for AIX V8.1, Runtime Modules, (c) Copyright IBM Corporation 1990-2002, All Rights Reserved. MSC, MSC/, MSC Nastran, MD Nastran, MSC Fatigue, Marc, Patran, Dytran, and Laminate Modeler are trademarks or registered trademarks of MSC.Software Corporation in the United States and/or other countries. NASTRAN is a registered trademark of NASA. PAM-CRASH is a trademark or registered trademark of ESI Group. SAMCEF is a trademark or registered trademark of Samtech SA. LS-DYNA is a trademark or registered trademark of Livermore Software Technology Corporation. ANSYS is a registered trademark of SAS IP, Inc., a wholly owned subsidiary of ANSYS Inc. ACIS is a registered trademark of Spatial Technology, Inc. ABAQUS, and CATIA are registered trademark of Dassault Systemes, SA. EUCLID is a registered trademark of Matra Datavision Corporation. FLEXlm is a registered trademark of Macrovision Corporation. HPGL is a trademark of Hewlett Packard. PostScript is a registered trademark of Adobe Systems, Inc. PTC, CADDS and Pro/ENGINEER are trademarks or registered trademarks of Parametric Technology Corporation or its subsidiaries in the United States and/or other countries. Unigraphics, Parasolid and I-DEAS are registered trademarks of UGS Corp. a Siemens Group Company. All other brand names, product names or trademarks belong to their respective owners.
P3*2008R1*Z*ABAQUS*Z* DC-USR
Main Index
Contents Patran Interface to ABAQUS Preference Guide
1
Overview Purpose
2
ABAQUS Product Information
3
What is Included with this Product?
4
Patran ABAQUS Integration with Patran Configuring the ABAQUS Submit File
2
Building A Model Introduction to Building a Model Coordinate Frames
22
Finite Elements 23 Nodes 23 Elements 25 Multi-Point Constraints Material Library Materials Form
10
27
51 52
Element Properties 90 Element Properties Form 90 Loads and Boundary Conditions Loads & Boundary Conditions Form Load Cases Group
3
351
352
Running an Analysis Review of the Analysis Form
Main Index
354
332 332
5 7
ii Patran Interface to ABAQUS Preference Guide
Analysis Form
355
Translation Parameters Restart Parameters Optional Controls Direct Text Input
357 358
359 360
Step Creation 361 Select Load Cases 362 Output Requests 362 Direct Text Input 363 Solution Types 364 Step Selection
432
Read Input File
433
ABAQUS Input File Reader 435 Input Deck Formats 435 ABAQUS ELSET and NSET Entries
4
435
Read Results Review of the Read Results Form 454 Upgrading ABAQUS ODB Results Files 454 Read Results Form 455 Flat File Results 456 Translation Parameters 457 Attach Method 457 Translate and Control File Methods
457
Select Results File 458 Results Created in Patran 458 Data Translated from the Analysis Code Results File Key Differences between Attach and Translate Methods 464 Result Type Naming Conventions 464 Vector vs. Scalar Moment and Rotational Results Reaction Forces 465 Delete Result Attachment Form
Main Index
466
464
463
CONTENTS iii
5
Files Files
6
468
Errors/Warnings Errors/Warnings
Main Index
470
iv Patran Interface to ABAQUS Preference Guide
Main Index
Chapter 1: Overview Patran Interface to ABAQUS Preference Guide
1
Main Index
Overview
Purpose
ABAQUS Product Information
What is Included with this Product?
Patran ABAQUS Integration with Patran
Configuring the ABAQUS Submit File
2 3 4 5 7
2 Patran Interface to ABAQUS Preference Guide Purpose
Purpose Patran comprises a suite of products written and maintained by MSC.Software Corporation. The core of the product suite is a finite element analysis pre and postprocessor. The Patran system also includes several optional products such as advanced postprocessing programs, tightly coupled solvers, and interfaces to third party solvers. This document describes one of these interfaces. See the Patran User Manual for more information. The Patran ABAQUS Application Preference Guide provides a communication link between Patran and ABAQUS. It also provides customization of certain features that can be activated simply by selecting ABAQUS as the analysis code preference in Patran. Patran ABAQUS is integrated into Patran. The casual user will never need to be aware that separate programs are being used. For the expert user, there are three main components of Patran ABAQUS: several PCL files to provide the customization of Patran for ABAQUS, PAT3ABA to convert model data from the Patran database into the analysis code input file, and ABAPAT3 to translate results and⁄or model data from the analysis code results file into the Patran database. Selecting ABAQUS as the analysis code under the “Analysis Preference” menu customizes Patran in five main areas: 1. MPCs 2. Material Library 3. Element Library 4. Loads and Boundary Conditions 5. Analysis forms PAT3ABA translates model data directly from the .Patran database into the analysis code-specific input file format. This translation must have direct access to the originating Patran database. The program name indicates the direction of translation: from Patran to ABAQUS. ABAPAT3 translates results and⁄or model data from the analysis code-specific results file into the Patran database. This program can be run such that the data is loaded directly into the Patran database, or if incompatible computer platforms are being used, an intermediate file can be created. The program name indicates the direction of translation: from ABAQUS to Patran.
Main Index
Chapter 1: Overview 3 ABAQUS Product Information
ABAQUS Product Information ABAQUS is a general-purpose finite element computer program for structural and thermal analyses. It is developed, supported, and maintained by Hibbitt, Karlsson, and Sorensen, Inc., 1080 Main Street, Pawtucket, Rhode Island 02860, (401) 727-4200. See the ABAQUS User’s Manual for a general description of ABAQUS’ capabilities.
Main Index
4 Patran Interface to ABAQUS Preference Guide What is Included with this Product?
What is Included with this Product? The Patran ABAQUS product includes all of the following items: 1. A PCL library file, abaqus.plb, contains Patran ABAQUS-specific definitions. 2. The executable programs pat3aba and abapat3 which perform the forward and results translation of data. Although these programs are separate executables, they are run from within Patran, and are transparent to the user. 3. Script files are also included to drive the programs in item 2. These script files are started by Patran and control the running of the programs in Patran ABAQUS. 4. This Application Preference User’s Manual is included as part of the product. An on-line version is also provided to allow you direct access to this information from within Patran.
Main Index
Chapter 1: Overview 5 Patran ABAQUS Integration with Patran
Patran ABAQUS Integration with Patran Two diagrams are shown below to indicate how these files and programs fit into the Patran environment. In some cases, site customization of some of these files is indicated. Please see the Patran Installation and Operations Guide for more information on this topic. Figure 1-1 shows the process of running an analysis. The abaqus.plb library defines the various
Translation Parameter, Solution Type, Solution Parameter, and Output Request forms called by the Analysis form. When the Apply button is selected on the Analyze form, a.jba file is created, and the script AbaqusSubmit is started. This script may need to be modified for your site installation. The script, in turn, starts the PAT3ABA forward translation. Patran operation is suspended at this time. PAT3ABA reads data from the database and creates the ABAQUS input deck. A message file is also created to record any translation messages. If PAT3ABA finishes successfully, and you have requested it, the script will then start ABAQUS.
Figure 1-1
Forward Translation
Figure 1-2 shows the process of reading information from an analysis results file. When the Apply button is selected on the Read Results form, a .jbr file is created, depending on whether model or results data is to be read. The ResultsSubmit script is also started. This script may need to be modified for
Main Index
6 Patran Interface to ABAQUS Preference Guide Patran ABAQUS Integration with Patran
your site installation. The script, in turn, starts the ABAPAT3 results translation. The Patran database is closed while this translation occurs. A message file is created to record any translation messages. ABAPAT3 reads the data from the ABAQUS results file. If ABAPAT3 can find the desired database, the results will be loaded directly into it. If, however, it cannot find the database (for example, if you are running on several incompatible platforms), ABAPAT3 will write all the data into a flat file. This flat file can be taken to wherever the database is and read in using the read file selections.
Figure 1-2
Main Index
Results Translation
Chapter 1: Overview 7 Configuring the ABAQUS Submit File
Configuring the ABAQUS Submit File The AbaqusSubmit script file controls the execution of the PAT3ABA translator and the ABAQUS analysis code. It is located in the Patran directory called/patran/patran3/bin/exe/ The information that AbaqusSubmit uses to perform its operations can be categorized as specific to the job and the site. The job specific information is automatically supplied by Patran as command line arguments at run time. The site specific information is set within the script file at the time of installation. Host=LOCAL Scratchdir=” Acommand=’abaqus’ The Host parameter defines the machine that is used to perform the ABAQUS analysis. When this parameter is set to LOCAL, the analysis is performed on the same machine as the Patran session (PAT3ABA translations are always performed on the same machine as the Patran session.) The Scratchdir parameter defines the directory on the host machine that temporarily holds the analysis files as they are created. The advantage of having a scratch directory is that the contents of the analysis scratch files are never transferred across the network. This benefit is not achieved when the Host parameter is set to LOCAL, so the Scratchdir parameter is ignored for this condition. The Acommand is the ABAQUS analysis code executable. If the Host is not LOCAL then the executable should include the complete pathname.
Main Index
8 Patran Interface to ABAQUS Preference Guide Configuring the ABAQUS Submit File
Main Index
Chapter 2: Building A Model Patran Interface to ABAQUS Preference Guide
2
Main Index
Building A Model
Introduction to Building a Model
Coordinate Frames
Finite Elements
23
Material Library
51
Element Properties
Loads and Boundary Conditions
Load Cases
Group
352
351
10
22
90 332
10 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Introduction to Building a Model There are many aspects to building a finite element analysis model. In several cases, the forms used to create the finite element data are dependent on the selected analysis type. Other parts of the model are created using standard forms. Under Preferences on the Patran main form is a selection for Analysis Settings. Analysis Settings defines the intended analysis code which is to be used for this mode.
The specified code may be changed at any time during model creation. As much data as possible will be converted if the analysis code is changed after the modeling process has already begun. The setting of this option defines what will be presented in several areas during the subsequent modeling steps. These areas include the material and element libraries (including multi-point constraints), the applicable loads and boundary conditions, and the analysis forms. The selected Analysis Type may also affect the allowable selections in these same areas. For more details, see Analysis Codes (p. 426) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 11 Introduction to Building a Model
Supported ABAQUS Commands The following tables summarize all the ABAQUS commands supported by the Patran ABAQUS Preference Guide. The tables indicate where in this guide you can find more information on how the commands are supported Table 2-1
Supported ABAQUS Model Definition Options
History Definition Options
ABAQUS/ Standard Section #
Initial Options
∗HEADING
• p. 334
7.2.1
Node Definition
∗NODE
• p. 18
7.3.6
∗NSET
• p. 18
7.3.8
∗TRANSFORM
• p. 16
7.3.11
∗ELEMENT
• p. 19
7.4.2
∗ELSET
• p. 328
7.4.2
∗RIGID SURFACE
• p. 154,
∗SLIDE LINE
• p. 147
∗BEAM GENERAL SECTION
• p. 106,
p. 113,
∗BEAM SECTION
• p. 108,
p. 115 to p. 119,
*CENTROID
• p. 114
Element Definition
Property Definition
Main Index
Command
Patran Interface to ABAQUS Preference Guide Page No.
p. 155,
p. 156
p. 261
7.4.7 7.4.8
p. 121
7.5.2 7.5.3 7.5.2
12 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-1 History Definition Options
Property Definition (continued)
Supported ABAQUS Model Definition Options (continued)
Command
Patran Interface to ABAQUS Preference Guide Page No.
∗DASHPOT
• p. 100,
∗FRICTION
• p. 102 to p. 104,
p. 132,
• p. 136 to p. 145,
p. 148 to p. 152
• p. 255 to p. 259,
p. 289
• p. 132,
p. 133,
p. 294,
∗GAP
p. 101,
ABAQUS/ Standard Section #
p. 128 to p. 131
7.5.5
p. 133,
7.5.7
p. 298
7.5.8
7.5.13
• p. 300
*GAP CONDUCTANCE *GAP RADIATION
• p. 294,
p. 298,
p. 300
∗HOURGLASS STIFFNESS
• p. 232,
p. 235,
p. 238,
p. 241,
• p. 244,
p. 246,
p. 248,
p. 251,
• p. 252,
p. 254,
p. 287
• p. 102,
p. 104,
p. 136,
p. 138,
• p. 140,
p. 142,
p. 145,
p. 148,
• p. 150,
p. 152,
p. 255,
p. 257,
• p. 259,
p. 289,
p. 294,
p. 298,
∗INTERFACE
7.5.14
• p. 300
∗MASS
• p. 96
7.5.17
∗ROTARY INERTIA
• p. 97
7.5.18
∗SHELL GENERAL SECTION
• p. 238,
p. 241,
p. 246
∗SHELL SECTION
• p. 80,
p. 134,
p. 135,
p. 232,
• p. 234,
p. 235,
p. 237,
p. 244,
• p. 292,
p. 293,
p. 295,
p. 296
• p. 123,
p. 248,
p. 251,
p. 252,
• p. 254,
p. 287,
p. 291,
p. 297,
∗SOLID SECTION
7.5.19 7.5.20
7.5.21
• p. 299
Main Index
∗SPRING
• p. 98,
p. 99,
p. 124 to p. 127
∗SURFACE CONTACT
• p. 103,
p. 136,
p. 255,
• p. 259,
p. 289
p. 257,
7.5.26
Chapter 2: Building A Model 13 Introduction to Building a Model
Table 2-1 History Definition Options
Supported ABAQUS Model Definition Options (continued)
Command ∗TRANSVERSE SHEAR STIFFNESS
Material Definition
Material Definition (continued)
Main Index
Patran Interface to ABAQUS Preference Guide Page No. • p. 107,
p. 108,
p. 110,
p. 113,
• p. 115,
p. 119,
p. 121,
p. 232,
• p. 234,
p. 235,
p. 237,
p. 238,
• p. 241,
p. 244,
p. 246
ABAQUS/ Standard Section # 7.5.27
∗MATERIAL
• p. 44
7.6.2
∗CAP HARDENING
• p. 69
7.6.4
∗COMBINED TEST DATA
• p. 69
∗CAP PLASTICITY
• p. 69
∗CONDUCTIVITY
• p. 77,
p. 78,
∗CREEP
• p. 70,
p. 71
7.6.9
∗DAMPING
• p. 49,
p. 72 to p. 75
7.6.11
∗DEFORMATION PLASTICITY
• p. 64
∗DENSITY
p. 49 to p. 59,
∗DRUCKER-PRAGER
• p. 69
∗ELASTIC
• p. 49,
7.6.5 7.6.8
p. 79
7.6.12 p. 72 to p. 79
7.6.13 7.6.16
p. 72,
p. 73,
p. 74,
7.6.17
• p. 75
∗EXPANSION
p. 49 to p. 59,
∗HYPERELASTIC
p. 51 to p. 56
∗HYPERFOAM
• p. 57,
p. 59
7.6.23
∗LATENT HEAT
• p. 57,
p. 59
7.6.27
∗NO COMPRESSION
• p. 57,
p. 59
7.6.29
∗NO TENSION
• p. 57,
p. 59
7.6.30
∗PLANAR TEST DATA
• p. 69
∗PLASTIC
• p. 65,
∗POTENTIAL
• p. 65 to p. 67,
∗RATE DEPENDENT
• p. 65 to p. 68
∗SHEAR TEST DATA
• p. 69
p. 72 to p. 79
7.6.18 7.6.22
p. 66,
p. 67 p. 70,
7.6.34 p. 71
7.6.37
14 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-1
Supported ABAQUS Model Definition Options (continued)
History Definition Options
Command
Patran Interface to ABAQUS Preference Guide Page No.
∗SIMPLE SHEAR TEST DATA
• p. 69
∗SPECIFIC HEAT
• p. 77,
∗UNIAXIAL TEST DATA
• p. 69
∗VISCOELASTIC
• p. 60,
p. 78,
p. 79
p. 61,
p. 62,
ABAQUS/ Standard Section #
7.6.40
p. 63
7.6.43
∗VOLUMETRIC TEST • p. 69 DATA • p. 68
∗ORIENTATION
• p. 80,
7.6.44 p. 232,
p. 234,
p. 235,
p. 237,
p. 238,
p. 241,
p. 244,
p. 246,
p. 248,
p. 251,
p. 287,
p. 295,
p. 296,
p. 297,
p. 299
∗BOUNDARY
• p. 313,
p. 317,
p. 318
∗EQUATION
• p. 24
7.8.3
∗MPC
• p. 25 to p. 42
7.8.4
Initial Conditions
∗INITIAL CONDITIONS
• p. 316,
7.9.1
Restart Options
∗RESTART
• p. 332
7.10.1
Miscellaneous Model Options
∗AMPLITUDE
• p. 346
7.11.1
∗PSD-DEFINITION
• p. 378
7.11.3
∗SPECTRUM
• p. 374
7.11.5
∗WAVEFRONT MINIMIZATION
• p. 334
7.11.9
Material Orientation
Kinematic Constraints
Main Index
*YIELD
p. 326
7.7.1
9.5.1
Chapter 2: Building A Model 15 Introduction to Building a Model
The following ABAQUS History Definition options are supported. Table 2-2
Supported ABAQUS History Definition Options
History Definition Options Step Initialization/ Termination
*STEP
• p. 336, p. 390,
ABAQUS/ Standard Section No.
p. 346, p. 382, p. 386, 9.2.1 p. 394, p. 402
∗END STEP
• p. 336
9.2.2
∗BUCKLE
• p. 349
9.3.2
∗DYNAMIC
• p. 352,
p. 386
9.3.4
∗FREQUENCY
• p. 359,
p. 366, p. 374, p. 377
9.3.5
∗HEAT TRANSFER
• p. 401,
p. 402
9.3.7
∗MODAL DYNAMIC
• p. 359
9.3.8
∗RANDOM RESPONSE • p. 377
9.3.9
∗RESPONSE SPECTRUM
• p. 374
9.3.10
∗STATIC
• p. 382
9.3.12
∗STEADY STATE DYNAMICS
• p. 366,
p. 370
9.3.13
∗VISCO
• p. 390,
p. 394
9.3.15
∗BASE MOTION
• p. 359,
p. 365, p. 366
9.4.2
∗CFLUX
• p. 325
9.4.4
∗CLOAD
• p. 313
9.4.5
∗DFLUX
• p. 325
9.4.9
∗DLOAD
• p. 314,
∗FILM
• p. 324
9.4.12
∗TEMPERATURE
• p. 314
9.4.18
Prescribed Boundary Conditions
∗BOUNDARY
• p. 318
9.5.1
Miscellaneous History Options
∗CORRELATION
• p. 377
9.4.6
∗MODAL DAMPING
• p. 359 to p. 364
9.6.6
Procedure Definition
Loading Definition
Main Index
Command
Patran Interface to ABAQUS Preference Guide Page No.
p. 316
9.4.10
16 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-2
Supported ABAQUS History Definition Options (continued)
History Definition Options
Command
Print Definition
File Output Definition
ABAQUS/ Standard Section No.
Patran Interface to ABAQUS Preference Guide Page No.
∗EL PRINT
• p. 338
9.8.2
∗ENERGY PRINT
• p. 338
9.8.3
∗MODAL PRINT
• p. 338
9.8.4
∗NODE PRINT
• p. 338
9.8.6
∗PRINT
• p. 338
9.8.7
∗EL FILE
• p. 338
9.9.2
∗ELEMENT MATRIX OUTPUT
• p. 338
∗ENERGY FILE
• p. 338
9.9.3
FILE FORMAT
• p. 338
9.9.4
∗MODAL FILE
• p. 338
9.9.5
∗NODE FILE
• p. 338
9.9.6
∗PREPRINT
• p. 338
The following ABAQUS element types are supported. Table 2-3
Supported ABAQUS Element Types
Element Types
Patran ABAQUS Preference Guide Page No.
Stress-Displacement Elements Beam Elements
Main Index
Two-dimensional
B21 B21H B22
B22H B23 B23H
• p. 106,
p. 108
Three-dimensional
B31 B31H B32 B32H
B33 B33H B34
• p. 113,
p. 115,
Three-dimensional Open Section
B31OS B31OSH
B32OS B32OSH
• p. 121
p. 119
Chapter 2: Building A Model 17 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued) Patran ABAQUS Preference Guide Page No.
Element Types Stress-Displacement Elements Beam Elements
Main Index
• p. 123
One-dimensional
C1D2 C1D2H
C1D3 C1D3H
Axisymmetric
CAX3 CAX3H CAX4 CAX4H CAX4I CAX4IH
CAX4R CAX4RH CAX6 CAX6H
Axisymmetric with twist
CGAX3 CGAX3H CGAX4 CGAX4H CGAX4R CGAX4RH
CGAX6 CGAX6H CGAX8 CGAX8H CGAX8R CGAX8RH
Plane Strain
CPE3 CPE3H CPE4 CPE4H CPE4I CPE4IH
CPE4R CPE4RH CPE6 CPE6H CPE6M CPE6MH
Generalized Plane Strain
CGPE5 CGPE5H CGPE6 CGPE6H CGPE6I CGPE6IH CGPE6R
CGPE6RH CGPE8 CGPE8H CGPE10 CGPE10H CGPE10R CGPE10RH
• p. 249
Plane Stress
CPS3
CPS6
• p. 251
CPS4
CPS6M
CPS4I
CPS8
CPS4R
CPS8R
CAX8 CAX8H
• p. 252
CAX8R CAX8RH • p. 253
CPE8 CPE8H
• p. 248
CPE8R CPE8RH
18 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued) Patran ABAQUS Preference Guide Page No.
Element Types Stress-Displacement Elements Beam Elements Three-dimensional
C3D4
C3D10
C3D27
C3D4H
C3D10HC3 D10M
C3D27H
C3D6
• p. 287
C3D27R C3D10MH C3D27RH
C3D6H C3D15 C3D8 C3D15H C3D8H C3D20 C3D8I C3D20H C3D8IH C3D20R C3D8R C3D20RH C3D8RH Membrane Elements Membrane Elements
Main Index
M3D3
M3D8
M3D4
M3D8R
M3D4R
M3D9
M3D6
M3D9R
• p. 254
Chapter 2: Building A Model 19 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Stress-Displacement Elements Shell Elements Shell
S3RF
S4RF
• p. 244,
p. 246
S4R
STRI3
• p. 235,
p. 237,
p. 241
S4R5
S9R5
• p. 232,
p. 234,
p. 238
• p. 40,
p. 41,
p. 235,
S8R
p. 237, • p. 40,
S8R5
p. 241 p. 41,
p. 232,
p. 234,
p. 238
STRI35
• p. 232,
p. 234,
p. 238
STRI65
• p. 232,
p. 234,
p. 235,
p. 237,
p. 238,
p. 241
• p. 134,
p. 135
Special Elements Axisymmetric
SAX1
SAX2
Elbow Elements Elbow Elements
ELBOW31
ELBOW31C
• p. 117
ELBOW31B ELBOW32 Spring Elements Spring Elements
SPRING1
• p. 98,
p. 99
SPRING2
• p. 125,
p. 127
SPRINGA
• p. 124,
p. 126
Dashpot Elements Dashpot Elements
DASHPOT1
• p. 100
DASHPOT2
• p. 101,
p. 129,
DASHPOTA
• p. 128,
p. 130
Mass Element Mass Element
MASS
• p. 96
Rotary Inertia Element Rotary Inertia Element
Main Index
ROTARY1
• p. 97
p. 131
20 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Special Elements Gap Elements Gap Elements
GAPCYL
• p. 132
GAPSPHER
• p. 133
GAPUNI
• p. 132
Small Sliding Contact Elements Interface
• p. 136
INTER1
Axisymmetric
INTER2
INTER3
• p. 255
INTER4 INTER8
INTER9
• p. 289
INTER2A
INTER3A
• p. 257
Rigid Surface Contact Elements Rigid Surface
IRS3 IRS4
Axisymmetric
IRS9
• p. 259
IRS12
• p. 102
IRS13
• p. 104
IRS21
IRS22
• p. 148
IRS31
IRS32
• p. 152
IRS21A
IRS22A
• p. 150
Slide Line Contact Elements Two-dimensional
ISL21
ISL22
• p. 138,
p. 147
Three-dimensional
ISL31
ISL32
• p. 142,
p. 147
Axisymmetric
ISL21A
ISL22A
• p. 140,
p. 147
ISL31A
ISL32A
• p. 145,
p. 147
Heat Transfer Elements Heat Transfer Elements
Main Index
• p. 297
Axisymmetric
DCAX3 DCAX4
DCAX6 DCAX8
Axisymmetric Convection/Diffusion
DCCAX2
DCCAX2D
DCCAX4
DCCAX4D
• p. 297
One-dimensional
DC1D2
DC1D3
• p. 291
Chapter 2: Building A Model 21 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Heat Transfer Elements Heat Transfer Elements
Main Index
DC2D6 DC2D8
• p. 297
Two-dimensional
DC2D3 DC2D4
Two-dimensional Convection/Diffusion
DCC2D4 DCC2D4D
Three-dimensional
DC3D4 DC3D6 DC3D8
DC3D10 DC3D15 DC3D20
• p. 299
Three-dimensional Convection/Diffusion
DCC3D8
DCC3D8D
• p. 299
Interface Elements
DINTER1
• p. 297
• p. 294
DINTER2
DINTER3
• p. 298
DINTER4
DINTER8
• p. 300
Interface Elements, Axisymmetric
DINTER2A DINTER3A
• p. 298
Shell Elements
DS4 DS8
• p. 295,
p. 296
Shell Elements, Axisymmetric
DSAX1 DSAX2
• p. 292,
p. 293
22 Patran Interface to ABAQUS Preference Guide Coordinate Frames
Coordinate Frames Coordinate frames will generate different ABAQUS input, depending on the use of the coordinate frame. Unreferenced coordinate frames will not be translated into ABAQUS.
If a node references a coordinate frame in the Analysis Coordinate Frame field, the nodal degrees-offreedom will be rotated into that system through the use of the *TRANSFORM option. All vector type loads or boundary conditions must reference the same coordinate frame as the node. If a coordinate frame is referenced for element property orientation, the appropriate *ORIENTATION option will be created.
Main Index
Chapter 2: Building A Model 23 Finite Elements
Finite Elements Finite Elements in Patran allows the definition of basic finite element constructs, including the creation of nodes, element topology, and multi-point constraints.
Nodes The nodes form will generate the ∗klab option (see Section 7.3.6 in the ABAQUS / Standard User’s Manual). The name of the node set to which the nodes will be assigned will be based on the associated analysis coordinate frame number. For example, creating nodes in analysis coordinate frame “Coord 1" will generate the ABAQUS option ∗NSET, NSET=CID1.
Main Index
24 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 25 Finite Elements
Elements Finite elements in Patran simply assigns element topology, such as Quad⁄4, for standard finite elements. The type of element to be created is not determined until the element properties are assigned. See Element Properties Form for details concerning the ABAQUS element types. Elements can be created either discretely using the Element object, or indirectly using the Mesh object.
Main Index
26 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 27 Finite Elements
Multi-Point Constraints Multi-point constraints (MPCs) can also be created from the Finite Elements menu. These are special element types which define a rigorous behavior between several specified nodes. The forms for creating MPCs are found by selecting MPC as the Object on the Finite Elements form. The full functionality of the MPC forms are defined in Create Action (FEM Entities) (Ch. 3) in the Reference Manual - Part III .
Main Index
28 Patran Interface to ABAQUS Preference Guide Finite Elements
MPC Types To create an MPC, you must first select the type of MPC you want to create from an option menu. The types that will appear in this option menu are dependent on the current Analysis Type preference setting. The following table describes the MPC types that are supported.
MPC Type Explicit
Analysis Type Structural Thermal
Creates an ∗EQUATION option which defines an explicit MPC between a dependent degree-of-freedom and one or more independent degrees-of-freedom. The dependent term consists of a node ID and a degree-of-freedom, while an independent term consists of a coefficient, a node ID, and a degree-of-freedom. An unlimited number of independent terms and one dependent term can be specified.
Rigid (Fixed)
Structural
Creates a BEAM type MPC between one independent node and one or more dependent nodes in which all six structural degrees-of-freedom are rigidly attached to each other. An unlimited number of dependent terms and one independent term can be specified. Each term consists of a single node.
Rigid (Pinned)
Structural
Creates a LINK type MPC between one independent node and one or more dependent nodes in which only the three translational structural degrees-of-freedom are rigidly attached to each other. An unlimited number of dependent terms and one independent term can be specified. Each term consists of a single node.
Linear Surf-Surf
Structural
Creates a LINEAR type MPC between a dependent node on one linear 2D element and two independent nodes on another linear 2D element to model a continuum. One dependent and two independent terms can be specified. Each term consists of a single node.
Thermal
Linear Surf-Vol
Structural
Creates an SS LINEAR type MPC between a dependent node on a linear 2D plate element and two independent nodes on a linear 3D solid element to connect the plate element to the solid element. One dependent and two independent terms can be specified. Each term consists of a single node.
Linear Vol-Vol
Structural
Creates a BILINEAR type MPC between a dependent node on one linear 3D solid element and four independent nodes on another linear 3D solid element to model a continuum. One dependent and four independent terms can be specified. Each term consists of a single node.
Thermal
Main Index
Description
Chapter 2: Building A Model 29 Finite Elements
MPC Type
Main Index
Analysis Type
Description
Quad. Surf-Surf
Structural
Creates a QUADRATIC type MPC between a dependent node on one quadratic 2D element and three independent nodes on another quadratic 2D element to model a continuum. One dependent and three independent terms can be specified. Each term consists of a single node.
Quad. Surf-Vol
Structural
Creates an SS BILINEAR type MPC between a dependent node on a quadratic 2D plate element and three independent nodes on a quadratic 3D solid element to connect the plate element to the solid element. One dependent and three independent terms can be specified. Each term consists of a single node.
Quad. Vol-Vol
Structural
Creates a C BIQUAD type MPC between a dependent node on one quadratic 3D solid and eight independent nodes on another quadratic 3D solid element to model a continuum. One dependent and eight independent terms can be specified. Each term consists of a single node.
Slider
Structural
Creates a SLIDER type MPC between one dependent node and two independent nodes which forces the dependent node to move along the vector defined by the two independent nodes. One dependent and two independent terms can be specified. Each term consists of a single node.
Elbow
Structural
Creates an ELBOW type MPC which constrains two nodes of ELBOW31 or ELBOW32 elements together. One dependent and one independent terms can be specified. Each term consists of a single node.
Tie
Structural
Creates a TIE type MPC which makes all active degrees-offreedom equal at two nodes. One dependent and one independent terms can be specified. Each term consists of a single node.
Revolute
Structural
Creates a REVOLUTE type MPC which defines a revolute joint. One dependent and two independent terms can be specified. Each term consists of a single node.
V Local
Structural
Creates a V LOCAL type MPC which constrains the velocity components at the first node to be equal to the velocity components at the third node along local, rotating, directions. These local directions rotate according to the rotation at the second node. One dependent and two independent terms can be specified. Each term consists of a single node.
30 Patran Interface to ABAQUS Preference Guide Finite Elements
MPC Type
Analysis Type
Description
Universal
Structural
Creates a UNIVERSAL type MPC which defines a universal joint. One dependent and three independent terms can be specified. Each term consists of a single node.
SS Linear
Structural
Creates an SS LINEAR type MPC which constrains a shell node to a line of solid nodes for linear elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
SS Bilinear
Structural
Creates an SS BILINEAR type MPC which constrains a shell node to a line of solid nodes for quadratic elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
SSF Bilinear
Structural
Creates an SSF BILINEAR type MPC which constrains a mid-side shell node to a line of mid-face solid nodes for quadratic elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
Degrees-of-Freedom Whenever a list of degrees-of-freedom is expected for an MPC term, a listbox containing the valid degrees-of-freedom is displayed on the form. A degree-of-freedom is valid if: 1. It is valid for the current Analysis Type Preference. 2. It is valid for the selected MPC type. In most cases, all degrees-of-freedom which are valid for the current Analysis Type preference are valid for the MPC type. The following degrees-of-freedom are supported by the Patran ABAQUS MPCs for the various analysis types:
Degrees-of-Freedom
Main Index
Analysis Type
UX
Structural
UY
Structural
UZ
Structural
RX
Structural
RY
Structural
RZ
Structural
Temperature
Thermal
Chapter 2: Building A Model 31 Finite Elements
Note:
Care must be taken to make sure that a degree-of-freedom selected for an MPC actually exists at the nodes. For example, a node that is attached only to solid structural elements will not have any rotational degrees-of-freedom. However, Patran will allow you to select rotational degreesof-freedom at this node when defining an MPC.
Explicit MPCs
Creates an *EQUATION option. (See Section 7.8.3 in the ABAQUS/Standard User’s Manual). No constant term is allowed for this type of equation. The A1 multiplier for the dependent term will be set to -1.0 to create the desired equation.
Main Index
32 Patran Interface to ABAQUS Preference Guide Finite Elements
Rigid (Fixed) MPCs
Creates an *MPC option of type BEAM for each dependent node (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes.
Main Index
Chapter 2: Building A Model 33 Finite Elements
Rigid (Pinned) MPCs
Creates an *MPC of type LINK for each dependent node (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This provides a pinned rigid link between two nodes in order to keep the distance between the two nodes constant. The displacements of the first node are modified to enforce this constraint. The rotations at the nodes, if any, are not involved in this constraint.
Main Index
34 Patran Interface to ABAQUS Preference Guide Finite Elements
Linear Surf-Surf MPCs
Creates an *MPC option of type LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is the standard method for mesh refinement of first-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated linearly from the corresponding degrees-of-freedom at the independent nodes .
Note:
Main Index
Linear Surf-Surf and Linear Surf-Vol MPCs both generate the ABAQUS ∗MPC type LINEAR.
Chapter 2: Building A Model 35 Finite Elements
Linear Surf-Vol MPCs
Creates an *MPC option of type SS LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is the standard method for mesh refinement of first-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated linearly from the corresponding degrees-offreedom at the independent nodes.
Note:
Main Index
Linear Surf-Surf and Linear Surf-Vol MPCs both generate the ABAQUS ∗MPC type SS LINEAR.
36 Patran Interface to ABAQUS Preference Guide Finite Elements
Linear Vol-Vol MPCs
Creates an *MPC option of type BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of first-order solid elements in three dimensions. This MPC constrains each degree-of-freedom at the dependent node to be interpolated bilinearly from the corresponding degrees-of-freedom at the independent nodes.
Main Index
Chapter 2: Building A Model 37 Finite Elements
Quad. Surf-Surf MPCs
Creates an *MPC option of type QUADRATIC (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated quadratically from the corresponding degrees-of-freedom at the independent nodes.
Note:
Main Index
Quad Surf-Surf and Quad Surf-Vol MPCs both generate the ABAQUS *MPC type QUADRATIC
38 Patran Interface to ABAQUS Preference Guide Finite Elements
Quad. Surf-Vol MPCs
Creates an *MPC option of type SS BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated quadratically from the corresponding degrees-of-freedom at the independent nodes.
Note:
Main Index
Quad Surf-Surf and Quad Surf-Vol MPCs both generate the ABAQUS ∗MPC type SS BILINEAR.
Chapter 2: Building A Model 39 Finite Elements
Quad. Vol-Vol MPCs
Creates an *MPC option of type C BIQUAD (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order solid elements in three dimensions. This MPC constrains each degree-of-freedom at the dependent node to be interpolated by a constrained biquadratic from the corresponding degrees-of-freedom at the eight independent nodes.
Main Index
40 Patran Interface to ABAQUS Preference Guide Finite Elements
Slider MPCs
Creates an *MPC option of type SLIDER (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC will keep a node on a straight line defined by two other nodes, but allows the possibility of moving along the line, and the line to change length.
Main Index
Chapter 2: Building A Model 41 Finite Elements
Main Index
42 Patran Interface to ABAQUS Preference Guide Finite Elements
Elbow MPCs
Creates an *MPC option of type ELBOW (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC constrains two ELBOW31 or ELBOW32 elements together, where the cross-sectional direction changes.
Main Index
Chapter 2: Building A Model 43 Finite Elements
Pin MPCs
Creates an *MPC option of type PIN (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC provides a pinned joint between two nodes. This makes the displacements equal, but leaves the rotations, if they exist, independent of each other.
Tie MPCs
Creates an *MPC option of type TIE (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC makes all active degrees-of-freedom equal at two nodes. If there are different degrees-of-freedom active at the two nodes, only those in common will be constrained. It is usually used to join two parts of a mesh when corresponding nodes on the two parts are to be fully connected.
Main Index
44 Patran Interface to ABAQUS Preference Guide Finite Elements
Revolute MPCs
Creates an *MPC option of type REVOLUTE (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
Main Index
Chapter 2: Building A Model 45 Finite Elements
Main Index
46 Patran Interface to ABAQUS Preference Guide Finite Elements
V Local MPCs
Creates an *MPC option of type V LOCAL (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
Main Index
Chapter 2: Building A Model 47 Finite Elements
Universal MPCs
Creates an *MPC option of type UNIVERSAL (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
SS Linear MPCs
Creates an *MPC option of type SS LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a shell node to a solid node line for linear elements (S4R or S4R5; C3D8, C3D8R; SAX1; CAX4; etc.) or for midside lines on quadratic elements (S8R, S8R5; C3D20, C3D20R; etc.). This MPC is only valid for small rotations.
Main Index
48 Patran Interface to ABAQUS Preference Guide Finite Elements
SS Bilinear MPCs
Creates an *MPC option of type SS BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC is only valid for small rotations.
Main Index
Chapter 2: Building A Model 49 Finite Elements
SSF Bilinear MPCs
Creates an *MPC option of type SSF BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC is only valid for small rotations.
Main Index
50 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 51 Material Library
Patran Interface to ABAQUS Preference Guide
Material Library Selecting Materials from this Patran window displays the main form for the creation of materials. The following sections provide an introduction to the Materials form, followed by the details of all the material property definitions supported by the Patran ABAQUS Application Interface.
Main Index
52 Patran Interface to ABAQUS Preference Guide Materials Form
Materials Form The Materials form shown below provides the following options for the purpose of creating ABAQUS materials.
Change Material Status The approach to defining material properties in Patran is similar to that in ABAQUS; the complete material model is defined by individually defining the necessary constitutive models. For example, to define a material for a plasticity analysis, one would first define the elastic properties and select Apply. Then the plastic properties are defined by selecting Plastic as Option 1, the yield criteria as Option 2, the hardening law as Option 3, entering the appropriate data and pushing Apply.
Main Index
Chapter 2: Building A Model 53 Materials Form
Not all constitutive model options are valid for a particular material in a particular ABAQUS analysis. For example, it is not permissible to have both elastic and hyperelastic properties defined for the same ABAQUS material. Patran, however, allows these different constitutive models to be defined and then “deactivated” for a given ABAQUS analysis. This is done on the form displayed when the Change Material Status button is selected on the main Materials form. For example, if a user defines both Elastic and Hyperelastic properties for a given material, one of these constitutive options must be deactivated on the Change Material Status form before initiating the ABAQUS analysis. Temperature Dependence ABAQUS allows most material properties to be functions of temperature. The ABAQUS interface in Patran generally supports this as well. The first step in defining a temperature dependent material property is to define a temperature dependent material field in the Fields application. This field can then be selected from a listbox on the Materials, Input Options form. When the databox for a material property that may be temperature dependent is selected, the fields listbox appears. The following table shows the allowable selections for all options when the Action is set to Create and the Analysis Type in the Analysis Preference form is set to Structural. The various options have different names, depending on previous selections.
Object Isotropic
Option 1
Option 2
• Elastic
Material Failure Theory
Hyperelastic
Incompressible
Option 3 Test Data • Ogden • Polynomial
Coefficients • Ogden • Mooney Rivlin • Neo Hookean • Polynomial
Slightly Compressible
Test Data • Ogden • Polynomial Coefficients • Ogden • Polynomial
Main Index
54 Patran Interface to ABAQUS Preference Guide Materials Form
Object
Option 1
Option 2 Compressible
Option 3 Test Data • Ogden
Coefficients • Ogden
Viscoelastic
Frequency
• Formula • Tabular
Time
• Prony • Creep Test Data • Combined Creep Test Data • Relaxation Test Data • Combined Relax Test Data
• Deformation
Plasticity Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
Cap Hardening
• Time • Strain • Hyperbolic
2D Orthotropic (Lamina)
• Elastic
Material Failure Theory
Viscoelastic
Frequency
• Formula
Tabular Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Main Index
Chapter 2: Building A Model 55 Materials Form
Object
Option 1 Plastic
Option 2 Mises/Hill
Option 3 • Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
Cap Hardening
• Time • Strain • Hyperbolic
3D Orthotropic
• Elastic
Engineering Constants
Material Failure Theory
• [D] Matrix
Viscoelastic
Frequency
• Formula Tabular
Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
• Time • Strain • Hyperbolic
Main Index
Cap Hardening
56 Patran Interface to ABAQUS Preference Guide Materials Form
Object 3D Anisotropic
Option 1
Option 2
Option 3
• Elastic
[D] Matrix
Material Failure Theory
Viscoelastic
Frequency
• Formula Tabular
Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
• Time • Strain • Hyperbolic
Composite
• Laminate
Rule of Mixtures HAL Cont. Fiber HAL Disc. Fiber HAL Cont. Ribbon HAL Disc. Ribbon HAL Particulate Short Fiber 1D Short Fiber 2D
Main Index
Cap Hardening
Chapter 2: Building A Model 57 Materials Form
The following table shows the allowable selections for all options when the Action is set to Create and the Analysis Type is set to Thermal in the Analysis Preference form. The various options have different names, depending on previous selections.
Object
Option 1
Isotropic
Thermal
3D Orthotropic
Thermal
3D Anisotropic
Composite
Laminate
Rule of Mixtures HAL Cont. Fiber HAL Disc. Fiber HAL Cont. Ribbon HAL Disc. Ribbon HAL Particulate Short Fiber 1D Short Fiber 2D
Main Index
58 Patran Interface to ABAQUS Preference Guide Materials Form
Isotropic Elastic
Main Index
Object
Option 1
Option 2
Isotropic
Elastic
Material Failure Theory
Chapter 2: Building A Model 59 Materials Form
More data input is available for defining the Elastic properties for the Isotropic materials. Listed below are the descriptions for the remaining material properties.
Main Index
Property Name
Description
Reference Temperature
This is the reference value of temperature for the coefficient of thermal expansion. The thermal strain in the material is based on the difference between the current temperature and this reference value (default is 0.0).
Thermal Expansion Coeff
Coefficient of thermal expansion for the isotropic material.
Fraction Critical Damping
Set this parameter equal to the fraction of critical damping to be used with this material in calculating composite damping factors for the modes (for use in modal dynamics). The default is 0.0. The value is ignored in direct integration dynamics.
Mass Propornl Damping
Factor for mass proportional damping in direct integration dynamics (default = 0.0). This value is ignored in modal dynamics.
Stiffness Propornl Damping
Factor for stiffness proportional damping in direct integration dynamics (default = 0.0). This value is ignored in modal dynamics.
60 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Test Data Ogden Polynomial
Chapter 2: Building A Model 61 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Coefficients - Ogden
62 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Coefficients Moony Rivlin Neo Hookean Polynomial
Chapter 2: Building A Model 63 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Test Data Ogden Polynomial
64 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Coefficients - Ogden
Chapter 2: Building A Model 65 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Coefficients - Polynomial
66 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Object Isotropic
Main Index
Option 1 Hyperelastic
Option 2 Compressible
Option 3 Test Data - Ogden
Chapter 2: Building A Model 67 Materials Form
More data input is available for defining the Hyperelastic properties. Listed below are the descriptions for the remaining material properties.
Main Index
Property Name
Description
Volumetric Pressure
Material field defining volume ratio (current volume/original volume) as a function of pressure. This field appears on the *VOLUMETRIC TEST DATA sub option.
Poisson’s Ratio
Effective Poisson’s ratio of the material which will be equal to all ν i . This is the value of the POISSON parameter on the *HYPERFOAM option. If no value is given, the lateral strains should be entered.
Density
Defines the material mass density. This quantity appears on the *DENSITY option.
Thermal Expansion Coeff
Coefficient of thermal expansion for the isotropic material. This parameter appears as a on the *EXPANSION option.
68 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Compressible
Coefficients - Ogden
Chapter 2: Building A Model 69 Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Frequency
Tabular
3D Orthotropic or 3D Anisotropic
Main Index
Formula
70 Patran Interface to ABAQUS Preference Guide Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Prony
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 71 Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Creep Test Data
3D Orthotropic or 3D Anisotropic
Main Index
Combined Creep Test Data
72 Patran Interface to ABAQUS Preference Guide Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Relaxation Test Data
3D Orthotropic or 3D Anisotropic
Main Index
Combined Relax Test Data
Chapter 2: Building A Model 73 Materials Form
Deformation Plasticity
Main Index
Object
Option 1
Isotropic
Deformation Plasticity
74 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Mises/Hill
Perfect Plasticity
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 75 Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2DOrthotropic,
Plastic
Mises/Hill
Isotropic
3DOrthotropic or 3D Anisotropic
Main Index
76 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Mises/Hill
Kinematic
3DOrthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 77 Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Drucker-Prager
Compression
3D Orthotropic or 3D Anisotropic
Tension Shear
Main Index
78 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Modified D-Prager/Cap
Cap Hardening
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 79 Materials Form
CrÉep Object
Option 1
Option 2
Isotropic, 2D Orthotropic,
Creep
Time
3D Orthotropic or 3D Anisotropic
Main Index
Strain
80 Patran Interface to ABAQUS Preference Guide Materials Form
Creep
Object
Option 1
Option 2
Isotropic, 2D Orthotropic,
Creep
Hyperbolic
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 81 Materials Form
2D Orthotropic (Lamina) Elastic
Main Index
Option 1
Option 2
Elastic
Material Failure Theory
82 Patran Interface to ABAQUS Preference Guide Materials Form
3D Orthotropic Elastic
Option 1 Elastic
Main Index
Option 2 Engineering Constants
Option 3 Material Failure Theory
Chapter 2: Building A Model 83 Materials Form
Elastic
Object 3D Orthotropic
Main Index
Option 1 Elastic
Option 2 [D] Matrix
Option 3 Material Failure Theory
84 Patran Interface to ABAQUS Preference Guide Materials Form
3D Anisotropic Elastic
Option 1 Elastic
Main Index
Option 2 [D] Matrix
Chapter 2: Building A Model 85 Materials Form
More data input is available for defining the Elastic properties for the 3D Anisotropic materials. Listed below are the descriptions for the remaining material properties.
Property Name
Desciption
D1212 (C34)
Coefficients in the 6 x 6 stress-strain matrix for the 3D anisotropic material.
D1212 (C44) D1113 (C15) D2213 (C25) D3313 (C35) D1213 (C45) D1313 (C55) D1123 (C16) D2223 (C26) D3323 (C36) D1223 (C46) D1323 (C56) D2323 (C66) Density
Main Index
Defines the material mass density.
86 Patran Interface to ABAQUS Preference Guide Materials Form
Isotropic (Thermal)
Main Index
Chapter 2: Building A Model 87 Materials Form
3D Orthotropic (Thermal)
Main Index
88 Patran Interface to ABAQUS Preference Guide Materials Form
3D Anisotropic (Thermal)
Composite The Composite forms allow existing materials to be combined to create new materials. All of the composite materials, with the exception of the laminated composites, can be assigned to elements like any homogeneous material through the element property forms. For the laminated composites, the section thickness is entered indirectly through the definition of the stack, and the Homogeneous option on the Element Properties Form for shells, plates and beam must be changed to Laminate to avoid reentry of this information.
Main Index
Chapter 2: Building A Model 89 Materials Form
For details on how to use these forms, refer to the Composite Materials Construction (p. 116) in the Patran Reference Manual. Laminate
Main Index
90 Patran Interface to ABAQUS Preference Guide Element Properties
Patran I nterface to ABAQU S Preference Gu ide
Element Properties By choosing the Element Properties item, located on the application switch for Patran, an element properties form will appear. When creating element properties, several option menus are available. The selections made in these option menus will determine which element property form is presented, and ultimately, which ABAQUS element will be created. The following pages give an introduction to the Element Properties form, followed by the details of all the element property definitions supported by the Patran ABAQUS Application Preference.
Element Properties Form When Element Properties is selected on the main menu, this is the form which will be displayed. Four option menus on this form are used to determine which ABAQUS element types are to be created, and which property forms are to be displayed. The individual property forms are documented later in this section. For more details, see the Element Properties Forms (p. 67) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 91 Element Properties
Main Index
92 Patran Interface to ABAQUS Preference Guide Element Properties
The following table shows the allowable selections for all option menus when Analysis Type is set to Structural.
Dimension 0D
Type
Option 2
MASS
• Rotary Inertia
ROTARYI
Grounded Damper
IRS (single node)
Beam in XY Plane
• Linear
SPRING1
• Nonlinear
SPRING2
• Linear
DASHPOT1
• Nonlinear
DASHPOT2
• Planar
Elastic Slip Soft Contact IRS12 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Spatial
Elastic Slip Soft Contact IRS13 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• General Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Box Section
Standard Formulation
B21, B22 B21H, B22H B23 B23H
Hybrid Cubic Interpolation Cubic Hybrid • Circular Beam (Solid)
Main Index
Name
• Mass Grounded Spring
1D
Option 1
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
Chapter 2: Building A Model 93 Element Properties
Dimension
Type
Beam in Space
Main Index
Option 1
Option 2
Name
• Hexagonal Beam
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• I Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Pipe Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Rectangular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Trapezoid Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• General Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Arbitrary Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Box Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Circular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Curved w/Pipe Section
Standard Formulation Ovalization Only Ovalization Only with Approximated Fourier
ELBOW31, ELBOW32 ELBOW31B ELBOW31C
• Hexagonal Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
94 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension
Type
Option 2
Name
• I Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• L Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Open Section
Standard Formulation Hybrid
B31OS, B32OS B31OSH, B32OSH
• Pipe Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Rectangular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Trapezoidal Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Truss
Standard Formulation Hybrid
Spring
Linear
• Standard Formulation SPRINGA SPRING2 Fixed Direction
Nonlinear
• Standard Formulation Fixed Direction
Linear
• Standard Formulation DASHPOTA DASHPOT2 Fixed Direction
Nonlinear
• Standard Formulation Fixed Direction
Damper
Main Index
Option 1
CID2, CID3 CID2H, CID3H
Chapter 2: Building A Model 95 Element Properties
Dimension 1D
Type Gap
Option 1
True Distance GAPCYL Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Spherical
True Distance Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Uniaxial
True Distance GAPUNI Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Homogeneous • Laminate
Main Index
Name
• Cylindrical
(continued)
Axisym Shell
Option 2
GAPSPHER
SAX1, SAX2
96 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 1D
Type
Option 1
Option 2
• 1D Interface
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
ISL (in plane)
• Planar
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Axisymmetric
Elastic Slip Soft Contact ISL21A, Elastic Slip Hard Contact ISL22A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Parallel
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation
(continued)
ISL (in space)
INTER1
Lagrange Vis Damping Lagrange Vis Damping No Separation
Main Index
Name
ISL21, ISL22
ISL31, ISL32 ISL31, ISL32
Chapter 2: Building A Model 97 Element Properties
Dimension 1D
Type ISL (in space) (continued)
Option 1 • Radial
(continued)
• Slide Line
• Axisymmetric
Main Index
Name
Elastic Slip Soft Contact ISL31A, Elastic Slip Hard Contact ISL32A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation --
IRS (planar/axisym) • Planar
• IRS (beam/pipe)
Option 2
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Elastic Slip Soft Contact IRS21, IRS22 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation Elastic Slip Soft Contact IRS21A, Elastic Slip Hard Contact IRS22A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation1D (cont.) IRS31, IRS32
98 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 1D (continued)
Type
Option 1
• Rigid Surf (Seg)
Option 2
Name ---
• Rigid Surf (Cyl)
--
• Rigid Surf (Axi)
--
• Rigid Surf (Bz2D)
R2D2, RAX2
• Rigid Line (Lbc) • Rebar
Axisymmetric
SFMAX1, SFMAX2
General Axisymmetric
SFMGAX1, SFMGAX2
• Mech Joint (2D Model) ALIGN AXIAL BEAM CARTESIAN JOIN JOINTC LINK ROTATION SLOT TRANSLATOR WELD • Mech Joint (3D Model) ALIGN AXIAL BEAM CARDAN CARTESIAN CONSTANT VELOCITY CVJOINT CYLINDRICAL EULER FLEXION-TORSION
Main Index
Chapter 2: Building A Model 99 Element Properties
Dimension
Type
Option 1
Option 2
Name
HINGE JOIN JOINTC LINK PLANAR RADIAL-THRUST REVOLUTE ROTATION SLIDE-PLANE SLOT TRANSLATOR UJOINT UNIVERSAL WELD • 1D Gasket
Axisymmetric Link
3D Link
2D Link
Main Index
Gasket Behavior Model
GKAX2
Thickness Behavior Only
GKAX2N
Built-in Material
GKAX2
Gasket Behavior Model
GK3D2
Thickness Behavior Only
GK3D2N
Built-in Material
GK3D2
Gasket Behavior Model
GK2D2
Thickness Behavior Only
GK2D2N
Built-in Material
GK2D2
100 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 2D
Type Shell
Option 1 Thin
Option 2 • Homogeneous Laminate
Thick
Homogeneous
Name STRI35, S4R5, STRI65, S8R5, S9R5 S3R, S4R, STRI65, S8R
Laminate • General Thin
Homogeneous Laminate
• General Thick
Homogeneous
STRI35, S4R5, STRI65, S8R5, S9R5 S3R, S4R, STRI65, S8R
Laminate • Large Strain • General Large Strain 2D Solid
• Plane Strain
• Plane Stress
Main Index
S3R, S4R, S8R Standard Formulation
CPE3, CPE4, CPE6, CPE8
Hybrid
CPE3H, CPE4H, CPE6H, CPE8H
Hybrid / Reduced Integration
CPE4RH, CPE8RH
Reduced Integration Incompatible Modes Hybrid/Incompatible Modes Modified Modified/Hybrid
CPE4R, CPE8R CPE4I CPE4IH CPE6M, CPE6MH
Standard Formulation Reduced Integration Incompatible Modes Modified Modified/Hybrid
CPS3, CPS4, CPS6, CPS8 CPS4R, CPS8R CPS4I CPS6M, CPS6MH
Chapter 2: Building A Model 101 Element Properties
Dimension 2D
Type 2D Solid (continued)
Option 1 • Axisymmetric
(continued)
• Axisymmetric with Twist
• Membrane
2D Interface
Main Index
Option 2
Name
Standard Formulation
CAX3, CAX4, CAX6, CAX8
Hybrid
CAX3H, CAX4H, CAX6H, CAX8H
Hybrid/Reduced Integration
CAX4RH, CAX8RH
Reduced Integration
CAX4R, CAX8R
Incompatible Modes
CAX4I
Hybrid/Incompatible Modes
CAX4IH
Modified
CAX6M
Modified/Hybrid
CAX6MH
Standard Formulation
CGAX3, CGAX4, CGAX6, CGAX8
Hybrid
CGAX3H, CGAX4H, CGAX6H, CGAX8H
Hybrid/Reduced Integration
CGAX4RH, CGAX8RH
Reduced Integration
CGAX4R, CGAX8R
Standard Formulation
M3D3, M3D4, M3D6, M3D8, M3D9
Reduced Integration
M3D4R, M3D8R, M3D9R
• Planar
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
INTER2, INTER3
102 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 2D
Type
Option 1
2D Solid (continued)
• Axisymmetric
IRS (shell/solid)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
(continued)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Name INTER2A, INTER3A
IRS3, IRS4, IRS9
• Rigid Surf (Bz3D)
--
• Rigid Surface(Lbc)
R3D3, R3D4
• 2D Rebar
Cylindrical General
• 2D Gasket
Plane Strain Plane Stress
Axisymmetric
Main Index
Option 2
SFMCL9 Standard Formulation
SFM3D3, SFM3D4, SFM3D6, SFM3D8
Reduced Integration
SFM3D4R, SFM3D8R
Gasket Behavior Model
GKPE4
Built-in Material
GKPE4
Gasket Behavior Model
GKPS4
Thickness Behavior Only
GKPS4N
Built-in Material
GKPS4
Gasket Behavior Model
GKAX4
Thickness Behavior Only
GKAX4N
Built-in Material
GKAX4
Chapter 2: Building A Model 103 Element Properties
Dimension
Type
Option 1 Line
3D
• Solid
Standard Formulation Laminate Hybrid
Option 2
Name
Gasket Behavior Mode
GK3D4L
Thickness Behavior Only
GK3D4LN
Built-in Material
GK3D4L C3D4, C3D6, C3D8, C3D10, C3D15, C3D20
Laminate
C3D4H, C3D6H, C3D8H, C3D10H, C3D15H, C3D20H
Hybrid/Red Integration Laminate
C3D8RH, C3D20RH
Reduced Integration Laminate
C3D8R, C3D20R
Incompatible Modes Laminate
C3D8I
Hybrid/Incomp Modes
C3D8IH
Laminate
Main Index
Modified
C3D10M
Modified/Hybrid
C3D1OH
• 3D Interface
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
INTER4, INTER8, INTER9
• Gasket
Gasket Behavior Model
GK3D8, GK3D6
Thickness Behavior Only
GK3D8N, GK3D6N
Built-in Material
GK3D8, GK3D6
104 Patran Interface to ABAQUS Preference Guide Element Properties
The following table shows the allowable selections for all option menus when Analysis Type is set to Thermal.
Dimension 1D
Type
Option 1
Option 2
• Link
Axisymmetric Shell
DCID2, DCID3 • Homogeneous
DSAX1, DSAX2
• Laminate
• 1D Interface
2D
Shell
Name
DINTER1 • Homogeneous
DS4, DS8
• Laminate
2D Solid
• Planar
Standard Formulation
DC2D2, DC2D4, DC2D6, DC2D8 DCC2D4
Convection/Diffusion DCC2D4D Convection/Diffusion with Dispersion/Control • Axisymmetric
• 2D Interface
Main Index
Standard Formulation
DCAX3, DCAX4, DCAS6, DCAX8
Convection/Diffusion
DCCAX4
Convection/Diffusion with Dispersion/Control
DCCAX4D
Planar
DINTER2, DINTER3
Axisymmetric
DINTER2A, DINTER3A
Chapter 2: Building A Model 105 Element Properties
Dimension 3D
Type • Solid
• 3D Interface
Main Index
Option 1
Option 2
Name
Standard Formulation
DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20
Convection/Diffusion
DCC3D8
Convection/Diffusion with Dispersion Control
DCC3D8D
DINTER4, DINTER8
106 Patran Interface to ABAQUS Preference Guide Element Properties
Point Mass Analysis Type Structural
Dimension 0D
Type Mass
Option 1
Option 2
Topologies Point/1
Options above create MASS elements with ∗MASS properties.This creates a concentrated mass at a point. The mass is associated with the translational degrees-of-freedom at a node.
Main Index
Chapter 2: Building A Model 107 Element Properties
Rotary Inertia Analysis Type Structural
Dimension 0D
Type Rotary Inertia
Option 1
Option 2
Topologies Point/1
Options above createROTARI elements with ∗ROT ARY INERTIA properties. This element allows the rotary inertia of a rigid body to be included at a node. An ∗ORIENTATION option may also be created, as required.
Main Index
108 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Spring (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Spring
Option 1 Linear
Option 2
Topologies Point/1
Options above create SPRING1 elements with ∗SPRING properties. This element defines a linear spring between a node and ground. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 109 Element Properties
Nonlinear Spring (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Spring
Option 1
Option 2
Nonlinear
Topologies Point/1
Options above create SPRING1 elements with ∗SPRING properties. This element defines a nonlinear spring between a node and ground. An ∗ORIENTATION option may also be created, as required.
Linear Damper (Grounded) Analysis Type Structural
Main Index
Dimension 0D
Type Grounded Damper
Option 1 Linear
Option 2
Topologies Point/1
110 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create DASHPOT1 elements with ∗DASHPOT properties. This element defines a linear damper between a node and ground. An ∗ORIENTATION option may also be created, as required.
Nonlinear Damper (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Damper
Option 1 Nonlinear
Option 2
Topologies Point/1
Options above create DASHPOT1 elements with ∗DASHPOT properties. This element defines a nonlinear dashpot between a node and ground. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 111 Element Properties
Main Index
112 Patran Interface to ABAQUS Preference Guide Element Properties
IRS (Single Node, Planar) Analysis Type
Dimension
Structural
0D
Type IRS (single node)
Option 1 Planar
Option 2 Elastic Slip Soft Contact
Topologies Point/1
Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS12 elements with ∗INTERFACE and ∗FRICTION properties. This element defines an interface between a node on a planar model and a rigid surface.
Main Index
Chapter 2: Building A Model 113 Element Properties
More=data input is available for creating IRS (single node, planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option definition.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
114 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure
Main Index
No Sliding Contact
Chooses the Lagrange multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 115 Element Properties
IRS (Single Node, Spatial) Analysis Type Dimension Structural
0D
Type IRS (single node)
Option 1 Spatial
Option 2 Elastic Slip Soft Contact
Topologies Point/1
Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS13 elements with ∗INTERFACE and ∗FRICTION properties. This element defines an interface between a node on a spatial model and a rigid surface.
Main Index
116 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (single node, spatial) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Chapter 2: Building A Model 117 Element Properties
Property Name
Description
Stiffness in Stick
This is currently not used.
Maximum Friction
Defines the equivalent shear stress limit of the gap element. This is the equivalent shear stress limit value on the second card of the *FRICTION option.
Stress
Clearance Zero-Pressure Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant. Pressure Zero Clearance Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant. Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
General Beam in Plane Analysis Type
Dimension
Structural
1D
Type
Option 1
Beam in XY General Plane Section
Option 2
Topologies
Standard Formulation Bar/2, Bar/3 Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements, depending on the specified options and topology. ∗BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. This defines a general section beam which is restricted to remain in the XY plane.
Main Index
118 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating General Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam.
Chapter 2: Building A Model 119 Element Properties
Box Beam in Plane/Space Analysis Type Structural
Dimension 1D
Type
Option 1
Beam in Box Section XY Plane
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements in a plane, or B31, B32, B33, B34, B31H, B32H or B33H elements in space, depending on the specified options and topology. ∗BEAM SECTION, SECTION=BOX properties are also created. The planar box section beam is restricted to remain in the XY-plane. For the spatial beam, ∗TRANSVERSE SHEAR STIFFNESS is also created, as required.
Main Index
120 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 121 Element Properties
More data input is available for creating Box Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name Thickness_RHS Thickness_TOP Thickness_LHS
Description Defines the wall thickness of the element cross section. These are for the right-hand side, top, left-hand side, and bottom, respectively. These are four of the data values on the second card of the *BEAM SECTION option. These can be either real constants or references to existing field definitions. These properties are required.
Thickness_BOT Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam.
Definition of XY Plane (for beams in space only)
Defines the orientation of the XY-plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the *BEAM SECTION option. All of the Patran tools are available via the select menu to define this vector.
Beam Shape Display in Plane/Space All of the beam shapes can be displayed in their proper orientation on the 3D model. To activate the display, go to Display/Load/BC/Elem. Props... and set the "Beam Display" option. These options are discribed in detail in Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual. The beam display is shown on beam elements only, not geometry.
Main Index
122 Patran Interface to ABAQUS Preference Guide Element Properties
Additional Beam Shapes in Plane/Space Additional commonly used beam cross-sectional shapes are defined by forms analogous to that for box beams. The planar option defines a beam which is restricted to remain in the XY plane. For the spatial beam, *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS is also created, as required. CIRCULAR BEAM (SOLID) This property will have the SECTION=CIRC parameter. All that is required for the definition of the cross section is the radius. The integration schemes for planar analysis (left) and spatial analysis(right) are shown below.
HEXAGONAL BEAM This property will have the SECTION=HEX parameter. All that is required for the definition of the cross section is the circumscribing radius and the wall thickness. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
Main Index
Chapter 2: Building A Model 123 Element Properties
I-SECTION This property will have the SECTION=I parameter. The height of section, flange widths, and associated thicknesses are required. In addition, the height of the centroid, depicted as “l” is also required. This allows placement of the origin of the local cross-section axis anywhere on the symmetry line. Note also that judicious specification of the flange widths and thicknesses will allow modelling of a T-section. See p. 3.5.2-11 of the ABAQUS User’s Manual for details. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
PIPE BEAM This property will have the SECTION=PIPE parameter. The pipe thickness and outside radius define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
Main Index
124 Patran Interface to ABAQUS Preference Guide Element Properties
RECTANGULAR BEAM (SOLID) This property will have the SECTION=RECT parameter. The section width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
TRAPEZOID BEAM (SOLID) This property will have the SECTION=TRAP parameter. The top and bottom width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
General Beam in Space Analysis Type Structural
Main Index
Dimension 1D
Type Beam in Space
Option 1 General Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Cubic Initially Straight
Bar/2
Chapter 2: Building A Model 125 Element Properties
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. *BEAM GENERAL SECTION properties are also created. This property will have the SECTION=GENERAL parameter. *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS options are also created, as required. This defines a general section beam.
More data input is available for creating General Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
126 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Definition of XY Plane
Defines the orientation of the XY plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the ∗BEAM GENERAL SECTION option. All of the Patran tools are available via the select menu to define this vector.
Centroid Coord 1
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Centroid Coord 2
Shear Centroid Coord 1 Shear Centroid Coord 2
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Section Point Coord 1
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the *SECTION POINTS suboption of the *BEAM GENERAL SECTION option.
Section Point Coord 2
Main Index
Defines the location of the shear centroid of the cross section with respect to the nodal locations. These values are measured in the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the *SHEAR CENTER suboption on the *BEAM GENERAL SECTION option.
Chapter 2: Building A Model 127 Element Properties
Arbitrary Beam in Space Analysis Type Dimension Structural
1D
Type Beam in Space
Option 1 Arbitrary Section
Option 2 Standard Formulation
Topologies Bar/2, Bar/3 Bar/2, Bar/3
Hybrid Bar/2 Cubic Interpolation Bar/2 Cubic Hybrid Bar/2 Cubic Initially Straight Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=ARBITRARY properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an arbitrary section beam.
Main Index
128 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Arbitrary Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu
Main Index
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a righthand rule. This is the data on the second card of the ∗BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Chapter 2: Building A Model 129 Element Properties
Main Index
Property Name
Description
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
130 Patran Interface to ABAQUS Preference Guide Element Properties
Curved Pipe in Space Analysis Type
Dimension
Structural
1D
Type Beam in Space
Option 1 Curved w/Pipe Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Ovalization Only
Bar/2
Ovaliz Only w/ Approx Fourier
Bar/2
Options above create ELBOW31, ELBOW32, ELBOW31B, or C elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=ELBOW properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an elbow element.
Main Index
Chapter 2: Building A Model 131 Element Properties
More data input is available for creating Curved Pipe in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Torus Radius
Defines the radius of the elbow bend. This is one of the data values on the second card of the *BEAM SECTION option. This is either a real constant or a reference to an existing field definition. This property is required.
Integ Points around Pi
Defines the number of integration points to be used around the pipe cross section. This is the second value on the fourth card of the *BEAM SECTION option. This is an integer value. This property is required.
132 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Point Tangents Inters
Defines the orientation of the XY plane of the element coordinate system. This is the data on the second card of the *BEAM SECTION option. This is a Node ID. This property is required.
Integ Points thru Thick
Defines the number of integration points to be used through the pipe wall thickness. This is the first value on the fourth card of the *BEAM SECTION option. This is an integer value.
# Ovalization Modes
Defines the number of ovalization modes to be included in the shape functions of this element. This is the third value of the fourth card of the *BEAM SECTION option. This is an integer value.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
L-Section Beam in Space Analysis Type Dimension Structural
1D
Type Beam in Space
Option 1 L-Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Cubic Initially Straight
Bar/2
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=L properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an L-section beam.
Main Index
Chapter 2: Building A Model 133 Element Properties
More data input is available for creating L-Section Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
134 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Shear Factor
The product of this factor, the beam cross sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Open Beam in Space Analysis Type Structural
Dimension 1D
Type Beam in Space
Option 1 Open Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Options above create B31OS, B32OS, B31OSH, or B32OSH elements depending on the specified options and topology. ∗BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an open section beam.
Main Index
Chapter 2: Building A Model 135 Element Properties
More data input is available for creating Open Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
136 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Definition of XY Plane Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM GENERAL SECTION option. This is a real vector. This property is required. 1st. Sectorial Moment
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Warping Constant
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Centroid Coord 1
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Centroid Coord 2
Shear Center Coord 1 Defines the location of the shear centroid of the cross section with respect to the local cross section coordinate system. These values are either real Shear Center Coord 2 constants or references to existing field definitions. These are the values on the ∗SHEAR CENTER suboption of the ∗BEAM GENERAL SECTION option. Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Section Point Coord 1
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the ∗SECTION POINTS suboption of the ∗BEAM GENERAL SECTION option.
Section Point Coord 2
Truss Analysis Type Structural
Dimension 1D
Type Truss
Option 1 Standard Formulation
Option 2
Topologies Bar/2. Bar/3 Bar/2. Bar/3
Hybrid
Main Index
Chapter 2: Building A Model 137 Element Properties
Options above create T3D2, T3D2H, T3D3, or T3D3H elements depending on the specified options and topology. *SOLID SECTION properties are also created. The cross sectional area is included on the *SOLID SECTION option.
Linear Spring (Axial) Analysis Type Dimension Structural
1D
Type Spring
Option 1 Linear
Option 2 Standard Formulation
Topologies Bar/2
Options above create SPRINGA elements with *SPRING properties. This element defines a linear spring between two nodes whose line of action is the line joining the two nodes.
Main Index
138 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Spring (Fixed Direction) Analysis Type
Dimension
Structural
1D
Type Spring
Option 1 Linear
Option 2
Topologies
Fixed Direction Bar/2
Options above create SPRING2 elements with *SPRING properties.This element defines a linear spring between specified degrees-of-freedoms at two nodes. An *ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 139 Element Properties
Nonlinear Spring (Axial) Analysis Type Structural
Dimension 1D
Type Spring
Option 1 Nonlinear
Option 2 Standard Formulation
Topologies Bar/2
Options above create SPRINGA elements with *SPRING properties.This element defines a nonlinear spring between two nodes whose line of action is the line joining the two nodes.
Main Index
140 Patran Interface to ABAQUS Preference Guide Element Properties
Nonlinear Spring (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Spring
Option 1 Nonlinear
Option 2
Topologies
Fixed Direction Bar/2
Options above create SPRING2 elements with ∗SPRING properties. This element type defines a nonlinear spring between two nodes, acting in a fixed direction. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 141 Element Properties
Linear Damper (Axial) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Linear
Option 2 Standard Formulation
Topologies Bar/2
Options above create DASHPOTA elements with ∗DASHPOT properties. This element type defines a linear damper between two nodes whose line of action is the line joining the two nodes.
Main Index
142 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Damper (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Linear
Option 2 Fixed Direction
Topologies Bar/2
Options above create DASHPOT2 elements with ∗DASHPOT properties. This element type defines a linear damper between two nodes, acting in a fixed direction. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 143 Element Properties
Nonlinear Damper (Axial) Analysis Type
Dimension
Structural
1D
Type Damper
Option 1 Nonlinear
Option 2 Standard Formulation
Topologies Bar/2
Options above create DASHPOTA elements with ∗DASHPOT properties. This element type defines a nonlinear damper between two nodes whose line of action is the line joining the two nodes.
Main Index
144 Patran Interface to ABAQUS Preference Guide Element Properties
Nonlinear Damper (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Nonlinear
Option 2
Topologies
Fixed Direction Bar/2
Options above create DASHPOT2 elements with ∗a^pemlq properties. This element type defines a nonlinear damper between two specified nodes, acting in a fixed direction. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 145 Element Properties
Gap (Uniaxial), Gap (Cylindrical) Analysis Type Structural
Dimension 1D
Type Gap
Option 1
Cylindrical True Distance Uniaxial
Main Index
Option 2
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2
146 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create GAPUNI or GAPCYL elements with *GAP properties. The ∗FRICTION option is created, as required.
Main Index
Chapter 2: Building A Model 147 Element Properties
Gap (Spherical) Analysis Type Dimension Structural
1D
Type Gap
Option 1 Spherical
Option 2 True Distance Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2
Options above create GAPSPHER elements with *GAP properties. The *FRICTION option is created, as required.
Main Index
148 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Shell Analysis Type Structural
Dimension 1D
Type Axisymmetric Shell
Option 1 Homogeneous
Option 2
Topologies Bar/2 Bar/3
Options above create SAX1 or SAX2 elements, depending on the specified topology, with *SHELL SECTION properties.
Main Index
Chapter 2: Building A Model 149 Element Properties
Axisymmetric Shell (Laminate) Analysis Type Dimension Structural
1D
Type Axisymmetric Shell
Option 1 Laminate
Option 2
Topologies Bar/2
Options above create SAX1 or SAX2 elements, depending on the specified topology, with ∗SHELL SECTION, COMPOSITE properties.
Main Index
150 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 151 Element Properties
1D Interface Analysis Type Dimension Structural
1D
Type 1D Interface
Option 1 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2 Topologies Bar/2
Options above create INTER1 elements with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
Main Index
152 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating 1D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Chapter 2: Building A Model 153 Element Properties
Property Name
Description
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Planar ISL (In Plane)
Main Index
Analysis Type
Dimensio n
Structural
1D
Type ISL (in plane)
Option 1 Planar
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
154 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create ISL21 or ISL22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on a planar model and another part of the model.
More data input is available for creating Planar ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Chapter 2: Building A Model 155 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure
Main Index
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
156 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric ISL (In Plane) Analysis Type
Dimension
Structural
1D
Type ISL (in plane)
Option 1
Option 2
Axisymmetric Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2, Bar/3
Options above create ISL21A or ISL22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on an axisymmetric model and another part of the model.
Main Index
Chapter 2: Building A Model 157 Element Properties
More data input is available for creating Axisymmetric ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
158 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Parallel ISL (In Space) Analysis Type Dimension Structural
Main Index
1D
Type ISL (in space)
Option 1 Parallel
Option 2
Topologies
Bar/2, Bar/3 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Dampin Lagrange Vis Damping No Separation
Chapter 2: Building A Model 159 Element Properties
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of an element and another part of the model.
More data input is available for creating Parallel ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Vector
Main Index
Defines the normal to the plane in which sliding contact occurs. This is the second card of the *INTERFACE option. This value is a global vector. This property is required.
160 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping Clearance at which the damping coefficient is zero. Damping Zero Clearance Damping coefficient at zero clearance. Frac Clearance Const Damping
Main Index
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 161 Element Properties
Radial ISL (In Space) Analysis Type Structural
Dimension 1D
Type
Option 1
ISL (in space) Radial
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element and another part of the model.
Main Index
162 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Radial ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Vector
Defines the normal to the plane in which sliding contact occurs. This is the second card of the ∗INTERFACE option. This value is a global vector. This property is required.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Chapter 2: Building A Model 163 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Slide Line
Analysis Type
Dimensio n
Structural
1D
Type Slide Line
Option 1
Option 2
Topologies Bar/2, Bar/3
Options above create Slide Lines for the ISL elements. These elements must be equivalenced and continuous.
Main Index
164 Patran Interface to ABAQUS Preference Guide Element Properties
IRS (Planar) Analysis Type Structural
Main Index
Dimension 1D
Type IRS (plane/axisym)
Option 1 Planar
Option 2
Topologies
Bar/2, Bar/3 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Chapter 2: Building A Model 165 Element Properties
Options above create IRS21 or IRS22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on a planar model and a rigid surface.
More data input is available for creating IRS (planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
166 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 167 Element Properties
IRS (Axisymmetric) Analysis Type Structural
Dimensio n 1D
Type
Option 1
IRS Axisymmetric (plane/axisym)
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS21A or IRS22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on an axisymmetric model and a rigid surface.
Main Index
168 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (axisymmetric) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Chapter 2: Building A Model 169 Element Properties
Property Name
Description
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Beam/Pipe)
Main Index
Analysis Type
Dimension
Structural
1D
Type
Option 1
IRS (beam/pipe)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologies Bar/2, Bar/3
170 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create IRS31 or IRS32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between a beam or pipe element on a spatial model and a rigid surface.
More data input is available for creating IRS (beam/pipe) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Elastic Slip
Main Index
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Chapter 2: Building A Model 171 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Defines the ROUGH parameter on the *FRICTION option. This property is only used for the Lagrange option.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Rigid Surface (Segments) Analysis Type Dimension Structural
1D
Type Rigid Surf (Seg)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE=SEGMENTS option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The start Point (Node ID) defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Main Index
172 Patran Interface to ABAQUS Preference Guide Element Properties
Rigid Surface (Cylindrical) Analysis Type Dimension Structural
1D
Type Rigid Surf (Cyl)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE = CYLINDRICAL option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is first defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The rigid surface’s +x direction is defined from the start point (node ID) along the line of the rigid surface. The +y direction is away from the object the rigid surface will be in contact with. The +z direction (the surface generation vector) is defined by using right-hand rule, crossing the rigid surface’s +x axis with the +y axis.
Main Index
Chapter 2: Building A Model 173 Element Properties
Rigid Surface (Axisymmetric) Analysis Type
Dimension
Structural
1D
Type Rigid Surf (Axi)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE=AXISYMMETRIC option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
Main Index
174 Patran Interface to ABAQUS Preference Guide Element Properties
The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Surface (Bezier 2D)
Main Index
Analysis Type
Dimension
Structural
1D
Type Rigid Surf (Bz2D)
Option 1
Option 2
Topologies Bar/2
Chapter 2: Building A Model 175 Element Properties
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in two-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Line (LBC) Analysis Type Structural
Main Index
Dimension 1D
Type Rigid Line(LBC)
Option 1
Option 2
Topologies Bar/2
176 Patran Interface to ABAQUS Preference Guide Element Properties
This property set is created when the Rigid-Deform contact LBC is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R2D2 and RAX2 elements.
Rebar Analysis Type Structural
Dimension 1D
Type Rebar
Option 1 Axisymmetric General Axisymmetric
Option 2
Topologies Bar/2, Bar/3
The options above create SFMAX1, SFMAX2, SFMGAX1 and SFMGAX2 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
Main Index
Chapter 2: Building A Model 177 Element Properties
Main Index
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
178 Patran Interface to ABAQUS Preference Guide Element Properties
Rebar Orient. Angle
Defines the angular orientation of the rebar from the meridional plane in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Mech Joint (2D Model) - ALIGN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 ALIGN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 179 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
180 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - AXIAL Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 AXIAL
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 181 Element Properties
Main Index
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock, Min Disp
This property value defines the lower bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
182 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - BEAM Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 BEAM
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 183 Element Properties
Mech Joint (2D Model) - CARTESIAN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 CARTESIAN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Y Axis
Main Index
184 Patran Interface to ABAQUS Preference Guide Element Properties
Zero Force Ref Len
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (2D Model) - JOIN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 JOIN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 185 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - JOINTC Analysis Type Dimension Structural
1D
Type Mech Joint (2D Model)
Option 1 JOINTC
Option 2
Topologies Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
Main Index
186 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Y Axis
Main Index
Chapter 2: Building A Model 187 Element Properties
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis
Rot Damping, Z Axis
Main Index
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
188 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - LINK Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 LINK
Option 2 Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 189 Element Properties
Mech Joint (2D Model) - ROTATION Analysis Type
Dimension
Type
Option 1
Structural
1D
Mech Joint (2D Model)
ROTATION
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
190 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, Z Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Chapter 2: Building A Model 191 Element Properties
jÉÅÜ=gçáåí=EOa=jçÇÉäF=J=pilq Analysis Type
Dimension
Structural
1D
Type Mech Joint (2D Model)
Option 1 SLOT
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
Main Index
192 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Chapter 2: Building A Model 193 Element Properties
Mech Joint (2D Model) - TRANSLATOR Analysis Type
Dimension
Structural
1D
Type
Option 1
Mech Joint TRANSLATOR (2D Model)
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
194 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - WELD Analysis Type Structural
Dimension 1D
Type
Option 1
Mech Joint WELD (2D Model)
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to WELD on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 195 Element Properties
Mech Joint (3D Model) - ALIGN Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 ALIGN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
196 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - AXIAL Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 AXIAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
Main Index
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Chapter 2: Building A Model 197 Element Properties
Main Index
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock Min Disp
This property value defines the upper bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
198 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - BEAM Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 BEAM
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 199 Element Properties
Mech Joint (3D Model) - CARDAN Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 CARDAN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CARDAN on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
200 Patran Interface to ABAQUS Preference Guide Element Properties
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n onspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Mom/Rot about Y Axis Mom/Rot about Z Axis
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
jÉÅÜ=gçáåí=EPa=jçÇÉäF=J=`^oqbpf^k Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 CARTESIAN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 201 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, YAxis Force/Disp, Z Axis
Main Index
202 Patran Interface to ABAQUS Preference Guide Element Properties
Zero Force Ref Len
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis Damping, Z Axis
Mech Joint (3D Model) - CONSTANT VELOCITY Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 CONSTANT VELOCITY
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CONSTANT VELOCITY on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 203 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - CVJOINT Analysis Type Structural
Dimension 1D
Type
Option 1
Mech Joint CVJOINT (3D Model)
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CVJOINT on the *CONNECTOR SECTION option.
Main Index
204 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 205 Element Properties
Mech Joint (3D Model) - CYLINDRICAL Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 CYLINDRICAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CYLINDRICAL on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
206 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - EULER Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 EULER
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to EULER on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 207 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
208 Patran Interface to ABAQUS Preference Guide Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - FLEXION-TORSION Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 FLEXION-TORSION
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to FLEXION-TORSION on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 209 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
210 Patran Interface to ABAQUS Preference Guide Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - HINGE Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 HINGE
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to HINGE on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 211 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
212 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - JOIN Analysis Type
Dimension
Type
Option 1 Option 2 Topologies
Structural
1D
Mech Joint (3D Model)
JOIN
Bar/2
This option creates CONN3D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
Node A Analysis CID
Main Index
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 213 Element Properties
Mech Joint (3D Model) - JOINTC Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 JOINTC
Option 2
Topologies Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
214 Patran Interface to ABAQUS Preference Guide Element Properties
Force/Disp, X Axis Force/Disp, Y Axis Force/Disp, Z Axis
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
Main Index
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable. This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Chapter 2: Building A Model 215 Element Properties
Mech Joint (3D Model) - LINK Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 LINK
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
216 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - PLANAR Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 PLANAR
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to PLANAR on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 217 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - RADIAL-THRUST Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 RADIAL-THRUST
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to RADIAL-THRUST on the *CONNECTOR SECTION option.
Main Index
218 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, ZAxis
Zero Force Ref Len
Main Index
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Chapter 2: Building A Model 219 Element Properties
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, X Axis Damping, Z Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - REVOLUTE Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 REVOLUTE
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to REVOLUTE on the *CONNECTOR SECTION option.
Main Index
220 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Chapter 2: Building A Model 221 Element Properties
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Mech Joint (3D Model) - ROTATION Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 ROTATION
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
Main Index
222 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Chapter 2: Building A Model 223 Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - SLIDE-PLANE Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 SLIDE-PLANE
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to SLIDE-PLANE on the *CONNECTOR SECTION option.
Main Index
224 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, Y Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Z Axis
Zero Force Ref Len
Main Index
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Chapter 2: Building A Model 225 Element Properties
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis Damping, Z Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - SLOT Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 SLOT
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
Main Index
226 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Chapter 2: Building A Model 227 Element Properties
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Mech Joint (3D Model) - TRANSLATOR Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 TRANSLATOR
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
Main Index
228 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - UJOINT Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 UJOINT
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to UJOINT on the *CONNECTOR
Main Index
Chapter 2: Building A Model 229 Element Properties
SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
230 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - UNIVERSAL Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 UNIVERSAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to UNIVERSAL on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 231 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n onspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Mom/Rot about Z Axis
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Rot Damping, Z Axis
Mech Joint (3D Model) - WELD
Analysis Type
Dimensio n
Structural
1D
Type Mech Joint (3D Model)
Option 1 WELD
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to WELD on the *CONNECTOR
Main Index
232 Patran Interface to ABAQUS Preference Guide Element Properties
SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 233 Element Properties
Axisym Link Gasket Analysis Type Structural
Dimension 1D
Type
Option 1
Option 2
Topologies
1D Gasket Axisymmetric Gasket Bar2 Link Behavior Model
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the membrane and transverse shear behaviors.
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
234 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Chapter 2: Building A Model 235 Element Properties
Axisym Link Gasket (Thick only) Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket Axisymmetric Link
Option 2 Thickness Behavior Only
Topologies Bar2
These options create GKAX2N elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
236 Patran Interface to ABAQUS Preference Guide Element Properties
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisym Link Gasket (Material)
Main Index
Chapter 2: Building A Model 237 Element Properties
Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket Axisymmetric Link
Option 2 Built-in Material
Topologies Bar2
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
238 Patran Interface to ABAQUS Preference Guide Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket 3D Link
Option 2 Gasket Behavior Model
Topologies Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
Chapter 2: Building A Model 239 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
240 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Chapter 2: Building A Model 241 Element Properties
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket (Thick only) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 3D Link
Option 2
Topologies
Thickness Behavior Only
Bar2
These options create GK3D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
242 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 243 Element Properties
Main Index
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
244 Patran Interface to ABAQUS Preference Guide Element Properties
3D Link Gasket (Material) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 3D Link
Option 2
Topologies
Built-in Material
Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 245 Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
246 Patran Interface to ABAQUS Preference Guide Element Properties
2D Link Gasket Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Gasket Behavior Model
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
Chapter 2: Building A Model 247 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
248 Patran Interface to ABAQUS Preference Guide Element Properties
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
2D Link Gasket (Thick only) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Thickness Behavior Only
Bar2
These options create GK2D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 249 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
250 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Chapter 2: Building A Model 251 Element Properties
2D Link Gasket (Material) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Built-in Material
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
252 Patran Interface to ABAQUS Preference Guide Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Thin Shell Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thin Shell
Option 2 Homogeneous
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This element defines a standard thin shell element.
Main Index
Chapter 2: Building A Model 253 Element Properties
More data input is available for creating Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
254 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Normal Hourglass Stiffness Bending Hourglass Stiffness
Thin Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thin Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
Main Index
Chapter 2: Building A Model 255 Element Properties
Thick Shell Analysis Type
Dimension
Structural
2D
Type Shell
Option 1
Option 2
Topologies
Thick Shell
Homogeneous
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS and *HOURGLASS STIFFNESS options may also be created, as required. This defines a homogeneous thick shell element.
Main Index
256 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name Orientation System
Main Index
Description Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Chapter 2: Building A Model 257 Element Properties
Property Name
Description Defines the transverse shear stIffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K13 Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stIffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Thick Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thick Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
Main Index
258 Patran Interface to ABAQUS Preference Guide Element Properties
General Thin Analysis Type Structural
Dimension 2D
Type Shell
Option 1
Option 2
Topologies
General Thin Shell
Homogenous
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thin shell element.
Main Index
Chapter 2: Building A Model 259 Element Properties
More data input is available for creating General Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
260 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Define the temperature effects on the *SHELL GENERAL SECTION Temperature Scaling Thermal Expansion Scaling option. These are lists of real values. Each list must have the same Temperature Values number of values. These values are optional.
Main Index
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Chapter 2: Building A Model 261 Element Properties
General Thin Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Thin Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI3, STRI65, S4R5, S8R5 or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
Main Index
262 Patran Interface to ABAQUS Preference Guide Element Properties
General Thick Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Thick Shell
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thick shell element.
More data input is available for creating General Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Chapter 2: Building A Model 263 Element Properties
Property Name Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling Thermal Expansion Scaling Temperature Values
Define the temperature effects on the *SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Shear Stiffness K13
Defines the transverse shear stiffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Main Index
Description
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
264 Patran Interface to ABAQUS Preference Guide Element Properties
General Thick Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1
Option 2
General Thick Laminate Shell
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
Main Index
Chapter 2: Building A Model 265 Element Properties
Large Strain Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Large Strain Shell
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, S4R, or S8R elements with ∗SHELL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a large strain element.
Main Index
266 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu .
Property Name
Description
Membrane Hourglass Stiff
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Normal Hourglass Stiff Bending Hourglass Stiff
General Large Strain Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Large Strain Shell
Option 2
Topologies Tri/3, Quad/4
Options above create S3R, S4R, or S8R elements with ∗SHELL GENERAL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a general large strain element.
Main Index
Chapter 2: Building A Model 267 Element Properties
More data input is available for creating General Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
268 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Property Name
Description
Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the ∗SHELL GENERAL SECTION option. These properties are required.
Force Vector F1...F6
Defines the 6 values of the {F} vector on the ∗SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling D Thermal Expansion Scaling Temperature Values
Define the temperature effects on the ∗SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the ∗ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the ∗SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit surface area for the shell element. This is the DENSITY parameter on the ∗SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *SHELL GENERAL SECTION option.
Chapter 2: Building A Model 269 Element Properties
Property Name
Description
Shear Stiffness K13
Defines the transverse shear stiffness. These are the values on the ∗TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Plane Strain Analysis Type Structural
Dimension 2D
Type 2D Solid
Option 1 Plane Strain
Option 2
Topologies
Standard Formulation
Tri/3, Quad/4, Tri/6, Quad/8
Hybrid Hybrid/Reduced Integration Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Tri/6 Tri/6
Modified Formulation Modified/Hybrid Options above create CPE3, CPE4, CPE4R, CPE6, CPE6M, CPE8, CPE8R, CPE3H, CPE4H, CPE4RH, CPE6H, CPE6MH, CPE8H, or CPE8RH (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular element are found where reduced integration is requested, standard integration elements will be used
Main Index
270 Patran Interface to ABAQUS Preference Guide Element Properties
.
Generalized Plane Strain Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Solid General Plane Strain
Option 2
Topologies
Standard Formulation
Tri/3, Quad/4
Hybrid
Tri/6, Quad/8
Hybrid/Reduced Integration Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Main Index
Chapter 2: Building A Model 271 Element Properties
These options create CGPE5, CGPE5H, CGPE6, CGPE6H, CGPE6I, CGPE6IH, CGPE6R, CGPE6RH, CGPE8, CGPE8H, CGPE10, CGPE10H, CGPE10R or CGPE10RH elements with *SOLID SECTION properties when writing an ABAQUS V5.X or V4.X input file. Otherwise, they create CPEG3, CPEG3H, CPEG4, CPEG4H, CPEG4I, CPEG4IH, CPEG4R, CPEG4RH, CPEG6, CPEG6H, CPEG8, CPEG8H, CPEG8R or CPEG8RH elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
272 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
[Reference Node] V6.X+
Defines the REF NODE parameter on the *SOLID SECTION option. The third degree of freedom of this node defines the change in length between the bounding planes. The fourth and fifth degrees of freedom of this node define the relative rotations of one bounding plane with respect to the other. This property is required when generating an ABAQUS version 6 or greater input file.
[Node A: DOF] V5.X
This property is required when generating an ABAQUS version 4 or 5 input file.
[Node B: DOF
This property is required when generating an ABAQUS version 4 or 5 input file.
Plane Stress Analysis Type Dimension Structural
2D
Type 2D Solid
Option 1 Plane Stress
Option 2 Standard Formulation
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Reduced Integration Incompatible Modes Tri/6 Modified Formulation Options above create CPS3, CPS4, CPS4R, CPS6, CPS6M, CPS8, or CPS8R (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option will be included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
Chapter 2: Building A Model 273 Element Properties
Axisymmetric Solid Analysis Type Structural
Dimension 2D
Type
Option 1
2D Solid
Axisymmetric
Option 2
Topologies
Standard Formulation Tri/3, Quad/4, Tri/6, Quad/8 Reduced Integration Incompatible Modes Hybrid Tri/6 Modified Formulation Modified/Hybrid
Main Index
Tri/6
274 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create CAX3, CAX4, CAX4R, CAX6, CAX6M, CAX8, CAX8R, CAX3H, CAX4H, CAX4RH, CAX6H, CAX6MH, CAX8H, or CAX8RH elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. *ORIENTATION and ∗HOURGLASS STIFFNESS option may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Axisymmetric Solid with Twist (General) Analysis Type Structural
Dimension 2D
Type 2D Solid
Option 1
Option 2
General Standard Formulation Axisymmetric Hybrid
Topologies Tri/3, Quad/4, Tri/6, Quad/8 Quad/4, Quad/8
Reduced Integration Hybrid/Reduced Integration Options above create CGAX3, CGAX4, CGAX4R, CGAX6, CGAX8, CGAX8R, CGAX3H, CGAX4H, CGAX4RH, CGAX6H, CGAX8H, or CGAX8RH elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. *ORIENTATION and ∗HOURGLASS STIFFNESS
Main Index
Chapter 2: Building A Model 275 Element Properties
options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Membrane Analysis Type
Dimension
Structural
2D
Type
Option 1
Membrane Standard Formulation
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Reduced Integration Options above create M3D3, M3D4, M3D4R, M3D6, M3D8, M3D8R, M3D9 or M3D9R elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. The thickness value on the ∗plifa=pb`qflk option is included. ∗lofbkq^qflk and ∗elrodi^pp= pqfcckbpp options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
276 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 277 Element Properties
Planar 2D Interface Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Interface Planar
Option 2
Topologies
Quad/4, Elastic Slip Soft Contact Quad/8 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create INTER2 or INTER3 elements (depending on the selected topology) with ∗fkqboc^`b, ∗cof`qflk, and ∗proc^`b=`lkq^`q properties. The SOFTENED parameter on the ∗proc^`b=`lkq^`q option may be included, depending on the selected option. This element defines an interface region between two portions of a planar model. These elements must be created from one contact surface to the other.
Main Index
278 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Planar 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Main Index
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Press
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 279 Element Properties
Axisymmetric 2D Interface Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Interface Axisymmetric
Option 2
Topologies
Elastic Slip Soft Contact Quad/4, Quad/8 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create INTER2A or INTER3A elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element
Main Index
280 Patran Interface to ABAQUS Preference Guide Element Properties
defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
More data input is available for creating Axisymmetric 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Main Index
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Chapter 2: Building A Model 281 Element Properties
Property Name
Description
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Shell/Solid) Analysis Type Structural
Dimensio n 2D
Type
Option 1
IRS (shell/solid)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologie s Quad/4
Options above create IRS3, IRS4, and IRS9 elements (depending on the selected topology) with ∗INTERFACE, ∗FRICTION and ∗SURFACE CONTACT properties. The SOFTENED parameter on the ∗SURFACE CONTACT option may be included, depending on the selected option. This defines a rigid surface element for use with solid or shell elements.
Main Index
282 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (shell/solid) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Reference Node
Reference node common to the IRS elements and the rigid surface.
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Chapter 2: Building A Model 283 Element Properties
Property Name
Description
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Rigid Surface (Bezier 3D) Analysis Type Dimension Structural
2D
Type Rigid Surf (Bz3D)
Option 1
Option 2
Topologies Quad 4
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in three-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s manual). All trias forming up the rigid surface must have the normals pointing towards the contacting surface. Trias must all be connected.
Main Index
284 Patran Interface to ABAQUS Preference Guide Element Properties
Rigid Surface (LBC) Analysis Type
Dimension
Structural
2D
Type Rigid Surface(LBC)
Option 1
Option 2
Topologies Quad4, Tria3
This property set is created when the Rigid-Deform contact lbc is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R3D3 and R3D4 elements.
Main Index
Chapter 2: Building A Model 285 Element Properties
2D Rebar Analysis Type Structural
Dimension 2D
Type Rebar
Option 1 Cylindrical
Option 2 Standard Formulation
General Reduced Integration
Topologies Quad/9 Tri/3, Tri/6, Quad/4, Quad/8 Quad/4, Quad/8
The options above create SFM3D3, SFM3D4, SFM3D4R, SFM3D6, SFM3D8, SFM3D8R and SFMCL9 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
Main Index
286 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Chapter 2: Building A Model 287 Element Properties
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
Rebar Orient. Angle
Defines the angular orientation of the rebar from the local 1-direction in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Orientation System
Defines a local coordinate system for orienting the rebars. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create an *ORIENTATION option. The orientation name is then used for the ORIENTATION parameter on the *REBAR LAYER option. This property is not required.
Orientation Axis
Defines the axis of rotation on the “Orientation System” to use for the additional rotation specified by the “Orientation Angle”. The axis should have a nonzero component in the direction of the normal to the surface. An integer value between 1 and 3 may be specified. The local 1-direction is the default value. This property is not required.
Orientation Angle
Defines the additional rotation in degrees about the “Orientation Axis” of the “Orientation System”. Either a real scalar or a reference to an existing field definition may be specified. The default value is zero. This property is not required.
Plane Strain Gasket Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Strain
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
288 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 289 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Strain Gasket (Material) Analysis Type Structural
Main Index
Dimension 2D
Type
Option 1
2D Gasket Plane Strain
Option 2 Built-in Material
Topologies Quad4
290 Patran Interface to ABAQUS Preference Guide Element Properties
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Chapter 2: Building A Model 291 Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Stress
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
292 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 293 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Thick only) Analysis Type Structural
Main Index
Dimension 2D
Type
Option 1
Option 2
2D Gasket Plane Stress
Thickness Behavior Only
Topologies Quad4
294 Patran Interface to ABAQUS Preference Guide Element Properties
These options create GKPS4N elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 295 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Material) Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Stress
Option 2 Built-in Material
Topologies Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
296 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Chapter 2: Building A Model 297 Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisymmetric Gasket Analysis Type
Dimension
Structural
2D
Type 2D Gasket
Option 1
Option 2
Axisymmetric Gasket Behavior Model
Topologies Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
298 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 299 Element Properties
Main Index
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
300 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Gasket (Thick only) Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Axisymmetric
Option 2 Thickness Behavior Only
Topologies Quad4
These options create GKAX4N elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 301 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
302 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Gasket (Material)
Analysis Type Structural
Dimensio n 2D
Type
Option 1
2D Gasket Axisymmetri c
Option 2 Built-in Material
Topologies Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 303 Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gaske t
Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
304 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 305 Element Properties
F/L vs. Closure (Unloading) This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Main Index
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
306 Patran Interface to ABAQUS Preference Guide Element Properties
3D Line Gasket (Thick only) Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Thickness Behavior Only
Topologies Quad4
These options create GK3D4LN elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 307 Element Properties
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading) This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Main Index
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
308 Patran Interface to ABAQUS Preference Guide Element Properties
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gasket (Material) Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Built-in Material
Topologies Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 309 Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Main Index
310 Patran Interface to ABAQUS Preference Guide Element Properties
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Analysis Type Structural
Dimension
Type
3D
Solid
Option 1 Standard Formulation Hybrid Hybrid/Reduced Integration
Option 2
Topologies
Laminate
Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20, Hex/27
Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Tet/10 Tet/10
Modified Formulation Modified/Hybrid Options above create C3D4, C3D6, C3D8, C3D8R, C3D10, C3D10M, C3D15, C3D20, C3D20R, C3D4H, C3D6H, C3D8H, C3D8RH, C3D10H, C3D10MH, C3D15H, C3D20H, C3D20RH, C3D27, C3D27R, C3D27H, or C3D27RH elements (depending on the selected options and topologies) with ∗SOLID SECTION properties. ∗ORIENTATION and ∗HOURGLASS STIFFNESS options may also be created, as required. If tetrahedral or wedge elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
Chapter 2: Building A Model 311 Element Properties
Material Name
Defines the material to be used. When entering data, a list of all materials in the database is displayed. You can either pick one from the list with the mouse or type the name in. This identifies the material which will be referenced on the *SOLID SECTION option. This property is required.
Orientation Axis This property defines the the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option. Stack Direction
Main Index
This property defines the direction in which the material layers are stacked. This is the STACK DIRECTION parameter on the *SOLID SECTION option. An integer value of 1, 2 or 3 may be entered. Please see the section on defining composite solid elements in the ABAQUS Standard User’s Manual to determine the correct stack direction. This property is not required. The default value is 3.
312 Patran Interface to ABAQUS Preference Guide Element Properties
3D Interface Analysis Type Structural
Dimension 3D
Type
Option 1
3D Interface Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologies Hex/8, Hex/20, Hex/27
Options above create INTER4, INTER8 or INTER9 elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of a spatial model. These elements must be created from one contact surface to the other.
Main Index
Chapter 2: Building A Model 313 Element Properties
More data input is available for creating 3D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
314 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping Fraction of the clearance interval over which the damping coefficient is constant. Thermal Link Analysis Type Dimension Thermal
Main Index
1D
Type Link
Option 1
Option 2
Topologies Bar/2, Bar/3
Chapter 2: Building A Model 315 Element Properties
Options above create DC1D2 or DC1D3 elements, depending on the specified topology with *SOLID SECTION properties. The cross-sectional area value on the *SOLID SECTION option is included.
Thermal Axisymmetric Shell Analysis Type
Dimension
Thermal
1D
Type Axisymmetric Shell
Option 1 Homogeneous
Option 2
Topologies Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with *SHELL SECTION properties.
Main Index
316 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Axisymmetric Shell (Laminated) Analysis Type Thermal
Dimension 1D
Type Axisymmetric Shell
Option 1 Laminate
Option 2
Topologies Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with ∗pebii= pb`qflk, COMPOSITE properties.
Main Index
Chapter 2: Building A Model 317 Element Properties
Thermal 1D Interface Analysis Type Dimension Thermal
1D
Type 1D Interface
Option 1
Option 2
Topologies Bar/2
Options above create DINTER1 elements with ∗fkqboc^`b properties. These elements must be created from one contact surface to the other. ∗GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Main Index
318 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Shell Analysis Type Dimension Thermal
2D
Type Shell
Option 1 Homogeneous
Option 2
Topologies Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION properties. An *ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 319 Element Properties
Thermal Shell (Laminated) Analysis Type
Dimension
Type
Option 1
Thermal
2D
Shell
Laminate
Option 2
Topologies Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION, COMPOSITE properties. An *ORIENTATION option may also be created, as required.
Main Index
320 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Planar Solid Analysis Type Thermal
Dimension 2D
Type 2D Solid
Option 1
Option 2
Planar
Standard Formulation
Axisymmetric
Convection/Diffusion Convection/Diffusion w/Dispersion Control
Topologies Tri/3, Quad/4, Quad/8 Quad/4 Quad/4
Options above create DC2D3, DC2D4, DC2D6, DC2D8, DCC2D4, DCC2D4D, DCAX3, DCAX4, DCAX6, DCAX8,DCCAX4, or DCCAX4D elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. The thickness value on the ∗plifa=pb`qflk option is included. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 321 Element Properties
Thermal Preference (Planar) Analysis Type Dimension Thermal
2D
Type 2D Interface
Option 1 Planar
Option 2
Topologies Quad/4, Quad/8
Axisymmetric Options above create DINTER2, DINTER3, DINTER2A, or DINTER3A elements (depending on the selected option and topology) with *INTERFACE properties. These elements must be created from one
Main Index
322 Patran Interface to ABAQUS Preference Guide Element Properties
contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are created, as required.
Main Index
Chapter 2: Building A Model 323 Element Properties
Thermal Solid Analysis Type
Dimension
Thermal
3D
Type Solid
Option 1 Standard Formulation
Topologies Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20
Convection/Diffusion Hex/8 Convection/Diffusion w/ Dispersion Control Options above create DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20, DCC3D8, or DCC3D8D (depending on the selected options and topologies) elements with *SOLID SECTION properties. An *ORIENTATION option may also be created, as required.
Main Index
324 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Preference (Solid) Analysis Type Dimension Thermal
3D
Type 3D Interface
Option 1
Option 2
Topologies Hex/8, Hex/20
Options above create DINTER4 or DINTER8 elements (depending on the selected) with *INTERFACE properties. These elements must be created from one contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Main Index
Chapter 2: Building A Model 325 Element Properties
Solid Gasket Analysis Type Structural
Dimension 3D
Type
Option 1
Gasket
Gasket Behavior Model
Option 2
Topologies Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
326 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Chapter 2: Building A Model 327 Element Properties
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Thick only) Analysis Type Structural
Dimension 3D
Type Gasket
Option 1 Thickness Behavior Only
Option 2
Topologies Wedge6, Hex8
These options create GK3D8N or GK3D6N elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
328 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 329 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Material) Analysis Type Structural
Dimension 3D
Type Gasket
Option 1 Built-in Material
Option 2
Topologies Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
330 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Chapter 2: Building A Model 331 Element Properties
Main Index
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
332 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Patran I nterface to ABAQU S Preference Gu ide
Loads and Boundary Conditions When choosing the Loads/BCs toggle, the Loads and Boundary Conditions form will appear. The selections made will determine which loads and boundary form is presented, and ultimately, which ABAQUS loads and boundaries will be created. The following pages give an introduction to the Loads and Boundary Conditions form, followed by the details of all the loads and boundary conditions supported by the Patran ABAQUS Application Preference.
Loads & Boundary Conditions Form The Loads & Boundary Conditions form shown below provides the following options for the purpose of creating ABAQUS loads and boundaries. The full functionality of the form is defined in Loads and Boundary Conditions Form (p. 27) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 333 Loads and Boundary Conditions
The following table shows the allowable selections for all options when the Analysis Type is set to Structural.
Main Index
334 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Analysis Type Structural
Object
Type
• Displacement
Nodal
• Force
Nodal
• Pressure
Element Uniform
• Temperature
Nodal Element Uniform Element Variable
• Inertial Load
Element Uniform
• Initial Velocity
Nodal
• Velocity
Nodal
• Acceleration
Nodal
• Contact (Deform-Deform)
Element Uniform
• Contact (Rigid-Deform)
Element Uniform
• Pre-Tension
Element Uniform
The following table shows the allowable selections for all options when the Analysis Code is set to Thermal.
Analysis Type Thermal
Object
Type
• Temperature (Thermal)
Nodal
• Convection
Element Uniform
• Heat Flux
Element Uniform
• Heat Source
Nodal Element Uniform
• Initial Temperature
Nodal
Input Data Clicking on the Input Data button generates either a Static or Transient Input Data form, depending on the current Load Case Type. Static
This subordinate form appears whenever Load Case Type is set to Static and the Input Data button is clicked. The information contained on this form will vary according to the Object that has been selected. Information that remains standard to this form is defined below.
Main Index
Chapter 2: Building A Model 335 Loads and Boundary Conditions
Transient
This subordinate form appears whenever Load Case Type is set to Transient and the Input Data button is clicked. The information contained on this form will vary according to the Object that has been selected. Information that remains standard to this form is defined below.
Main Index
336 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Object Tables On the static and transient input data forms are areas where the load data values are defined. The data fields presented depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. These Object Tables list and define the various input data that pertains strictly to a specific selected object:
Main Index
Chapter 2: Building A Model 337 Loads and Boundary Conditions
Displacement
Object
Type
Type
Displacement
Nodal
Structural
Creates *BOUNDARY TYPE=DISPLACEMENT options.
Input Data
Description
Translations (T1,T2,T3)
Defines the enforced translational displacement values. These are in model length units.
Rotations (R1,R2,R3)
Defines the enforced rotational displacement values. These are in radians.
Force
Object
Type
Type
Force
Nodal
Structural
Creates *CLOAD options.
Input Data
Description
Force (F1,F2,F3)
Defines the applied forces in the translation degrees-of-freedom.
Moment (M1,M2,M3)
Defines the applied moments in the rotational degrees-of-freedom.
Pressure
Object
Type
Type
Pressure
Element Uniform Structural
Dimension 2D
Creates *DLOAD options.
Input Data Top Surf Pressure
Main Index
Description Defines the magnitude of the pressure in the direction of the negative normal to the shell.
338 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Input Data
Description
Bot Surf Pressure
Defines the magnitude of the pressure in the direction of the positive normal to the shell.
Edge Pressure
Defines the edge pressure value on axisymmetric, plane strain,and plane stress elements.
Object
Type
Type
Pressure
Element Uniform Structural
Dimension 3D
Creates *DLOAD options.
Input Data
Description
Pressure
Defines the face pressure value on solid elements.
Temperature
Object
Type
Type
Temperature
Nodal
Structural
Creates *TEMPERATURE options.
Input Data
Description
Temperature
Defines the nodal temperature value.
Object
Type
Type
Dimension
Temperature
Element Uniform
Structural
1D 2D 3D
Creates *TEMPERATURE options.
Input Data Temperature
Main Index
Description Defines the temperature on elements.
Chapter 2: Building A Model 339 Loads and Boundary Conditions
Object
Type
Type
Dimension
Temperature
Element Variable
Structural
1D 2D 3D
Creates *TEMPERATURE options.
Input Data
Description
Centroid Temp (1D)
Defines the temperature at the centroid of the beam.
Axis-1 Gradient (1D)
Defines the temperature gradient along the axis-1 of the beam section.
Axis-2 Gradient (1D)S
Defines the temperature gradient along the axis-2 of the beam section.
Top Surf Temp (2D)
Defines the temperature at the top of the shell element.
Bot Surf Temp (2D)
Defines the temperature at the bottom of the shell element.
Temperature (3D)
Defines the temperature in the solid element.
Inertial Load
Object
Type
Type
Inertial Load
Element Uniform
Structural
Creates *DLOAD options with the load type set to GRAV, CENT, or CORIO as appropriate.
Input Data
Description
Trans Accel (A1,A2,A3)
Defines the magnitude and direction of the gravity vector. This must be assigned to all elements which are to have gravity loads.
Rot Velocity (w1,w2,w3)
Defines the centrifugal and Coriolis forces to be applied to the elements.
Rot Accel (a1,a2,a3)
These load terms are not currently supported by Patran ABAQUS.
Initial Velocity
Main Index
Object
Type
Type
Initial Velocity
Nodal
Structural
340 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *INITIAL CONDITIONS TYPE=VELOCITY options.
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the initial velocity values for the translational degrees-offreedom.
Rot Veloc (w1,w2,w3)
Defines the initial velocity values for the rotational degrees-offreedom.
Velocity
Object
Type
Type
Velocity
Nodal
Structural
Creates *Boundary, Type=Velocity options.
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the velocity values for the translational degrees-of-freedom.
Rot Veloc (w1, w2, w3)
Defines the velocity values for the rotational degrees-of-freedom.
Acceleration
Object
Type
Type
Acceleration
Nodal
Structural
Creates *Boundary, Type=Acceleration options.
Input Data
Main Index
Description
Trans Accel (A1, A2, A3)
Defines the acceleration values for the translational degrees-of-freedom.
Rot Accel (a1, a2, a3)
Defines the acceleration values for the rotational degrees-of-freedom.
Chapter 2: Building A Model 341 Loads and Boundary Conditions
Contact (Deform-Deform)
Object
Type
Type
Contact
Element Uniform
Structural
Defines the contact between two deformable structural bodies and creates the following ABAQUS input cards: *Surface Definition: Master and Slave surface definitions. *Contact Pair: Pairing of the Master and Slave Surfaces. *Tie: Tying of the Master and Slave Surfaces (version 6 and greater). *Surface Interaction: Contact Interaction properties between Master and Slave. *Contact Controls: Set the Automatic Tolerances parameter *Contact Inerference: Set the Shrink parameter
Main Index
342 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Defines the Master and Slave surface interaction properties.
The contact type can be General (contacting surfaces move relative to each other) or Tied (contacting surfaces remain fixed with respect to each other usually used in mesh refinement). The sliding between the contacting surfaces can be Large or Small. For contact in 3D space the sliding is limited to Small sliding. Four types of contact surface behavior options are available, Hard, Softened, Modified Softened, and No Separation. The surfaces do not separate after contact in the case when No Separation option is used. Three types of friction formulations are available, Penalty, Lagrange, and No Slip. In the case of No Slip option there is no relative motion between the contacting surfaces after contact. The Penetration Type can be One Sided (Only the slave nodes are checked against the master surface) or Symmetric (Both the slave and master nodes are checked against each other by swapping the master and slave surfaces). The Contact Control can be turned On to activate the *Contact Control, Automatic Tolerances parameter. Use this parameter to have ABAQUS automatically compute an overclosure tolerance and a separation pressure tolerance to prevent chattering in contact. Shrink Fit can be turned On to activate the *Contact Interference, Shrink parameter. Use this parameter to invoke the automatic shrink fit capability. This capability can be used only in the first step of an analysis. When this parameter is invoked, no data are required other than the contact pairs to which the option is applied. The application region form is used to pick the master and slave surfaces.
Main Index
Chapter 2: Building A Model 343 Loads and Boundary Conditions
Application Region: Defines the Master and Slave contacting surfaces.
Contact (Rigid-Deform)
Object
Type
Type
Contact
Element Uniform
Structural
Defines the contact between the rigid surface and deformable structural body and creates the following ABAQUS input cards: *Surface Definition: Master and Slave surface definitions. *Contact Pair: Pairing of the Master and Slave Surfaces.
Main Index
344 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
*Surface Interaction: Contact Interaction properties between Master and Slave. *Contact Controls: Set the Automatic Tolerances parameter *Contact Inerference: Set the Shrink parameter Defines the Master and Slave surface interaction properties.
The sliding between the contacting surfaces can be Large or Small. Four types of contact surface behavior options are available, Hard, Softened, Modified Softened, and No Separation. The surfaces do not separate after contact in the case when No Separation option is used. Three types of friction formulations are available, Penalty, Lagrange, and No Slip. In the case of No Slip option there is no relative motion between the contacting surfaces after contact. The Contact Control can be turned On to activate the *Contact Control, Automatic Tolerances parameter. Use this parameter to have ABAQUS automatically compute an overclosure tolerance and a separation pressure tolerance to prevent chattering
Main Index
Chapter 2: Building A Model 345 Loads and Boundary Conditions
in contact. Shrink Fit can be turned On to activate the *Contact Interference, Shrink parameter. Use this parameter to invoke the automatic shrink fit capability. This capability can be used only in the first step of an analysis. When this parameter is invoked, no data are required other than the contact pairs to which the option is applied. A vector pointing from the rigid line to the slave surface must be defined. This vector is used to calculate the order of rigid bar elements. The vector should be defined such that the most of the vector markers point away from the rigid line. The application region form is used to pick the master and slave surfaces. Application Region: Defines the Master and Slave contacting surfaces.
Main Index
346 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Application Region: Defines the Master and Slave contacting surfaces. This form appears when Contact Type: is Rigid Geom. and Master: is Rigid Surface.
Main Index
Chapter 2: Building A Model 347 Loads and Boundary Conditions
Pre-tension
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Displacement
Structural
1D
Creates *BOUNDARY and *PRE-TENSION SECTION options.
Input Data
Description
Relative Displacement Defines the relative displacement to apply to the length of the elements.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Displacement
Structural
2D, 3D
Creates *BOUNDARY, *SURFACE and *PRE-TENSION SECTION options.
Input Data Relative Displacement
Description Defines the relative displacement to apply to the underlying elements in the direction of the section's normal.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Force
Structural
1D
Creates *CLOAD and *PRE-TENSION SECTION options.
Input Data
Description
Force
Main Index
Defines the pre-tension force to apply to the elements.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Force
Structural
2D, 3D
348 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *CLOAD, *SURFACE and *PRE-TENSION SECTION options.
Input Data Force
Description Defines the pre-tension force to apply to the underlying elements in the direction of the section's normal.
Temperature (Thermal)
Object
Type
Type
Temp (Thermal)
Nodal
Thermal
Creates *BOUNDARY options.
Input Data
Description
Temperature
Defines the nodal temperature value.
Convection
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
2D
Creates *FILM options.
Input Data
Main Index
Description
Top Surf Convection
Defines the convection coefficient for the top surface of a shell element.
Bot Surf Convection
Defines the convection coefficient for the bottom surface of a shell element.
Edge Convection
Defines the convection coefficient for the edges of axisymmetric, plane strain, and plane stress type elements.
Ambient Temp
Defines the ambient temperature.
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
3D
Chapter 2: Building A Model 349 Loads and Boundary Conditions
Creates *FILM options.
Input Data
Description
Convection
Defines the convection coefficient for the face of a solid element.
Ambient Temp
Defines the ambient temperature.
Heat Flux
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
2D
Creates *DFLUX options.
Input Data
Description
Top Surf Heat Flux
Defines the heat flux for the top surface of a shell element.
Bot Surf Heat Flux
Defines the heat flux for the bottom surface of a shell element.
Edge Heat Flux
Defines the heat flux for the edges of axisymmetric, plane strain, and plane stress type elements.
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
3D
Creates *DFLUX options.
Input Data Heat Flux
Description Defines the heat flux for the face of a solid element.
Heat Source
Main Index
Object
Type
Type
Heat Source
Nodal
Thermal
350 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *CFLUX options.
Input Data Heat Source
Description Defines the reference magnitude for flux (units
Object
Type
Type
Heat Source
Element Uniform
Thermal
J T Ó 1 ).
Creates *DFLUX options.
Input Data Heat Source
Description Defines the reference magnitude for flux (units
J T Ó 1 ).
Initial Temperature
Object
Type
Type
Initial Temperature
Nodal
Thermal
Creates *INITIAL CONDITIONS TYPE=TEMPERATURE options
Input Data Temperature
Main Index
Description Defines the initial temperature for a specified node.
Chapter 2: Building A Model 351 Load Cases
Load Cases Load Cases in Patran ABAQUS are used to group a series of Load sets into one load environment for the model. A load case is selected when preparing an analysis, not load sets. The individual load sets are translated into the input options described in the Object Tables of the section on Loads and Boundary Conditions form.
Main Index
352 Patran Interface to ABAQUS Preference Guide Group
Group Groups in Patran ABAQUS are used to create groups of nodes (*NSET) and groups of elements (*ELSET). All the groups created in Patran will be translated as *NSETs and *ELSETs except for the “default_group” which always exists in the database, and group names which do not begin with an alphabetic character (a-z, A-Z).d
Main Index
Chapter 3 : Running Analysis Patran Interface to ABAQUS Preference Guide
3
Main Index
Running an Analysis
Review of the Analysis Form
Translation Parameters
Restart Parameters
Optional Controls
Direct Text Input
Step Creation
Step Selection
Read Input File
ABAQUS Input File Reader
354
357
358 359 360
361 432 433 435
354 Patran Interface to ABAQUS Preference Guide Review of the Analysis Form
Review of the Analysis Form The Analysis toggle located on the main form for Patran brings up The Analysis Form (p. 8) in the MSC.Patran Reference Manual. This form is used to request an analysis of the model with the ABAQUS finite element program. It can also be used to incorporate the contents of an ABAQUS results file into the database. See Read Results. The following page gives an introduction to the Analysis form used to prepare an ABAQUS analysis. This is followed by detailed descriptions of the subordinate forms that can be displayed from the Analysis form.
Main Index
Chapter 3 : Running Analysis 355 Review of the Analysis Form
Analysis Form Setting the Action option menu on the Analysis Form to Analyze indicates that an analysis run is being prepared.
The Object indicates which part of the model is to be analyzed. It can be set to either Entire Model or Current Group. If the whole model is to be analyzed, select Entire Model. If only a part of the model is
Main Index
356 Patran Interface to ABAQUS Preference Guide Review of the Analysis Form
to be analyzed, create a group of that part, set that as the current group, then select Current Group as the Object. The Method indicates how far the translation is to be taken. Currently only Analysis Deck is supported. The method generates an ABAQUS input deck.
Main Index
Chapter 3 : Running Analysis 357 Translation Parameters
Translation Parameters This subordinate form appears whenever the Translation Parameters button is selected. The parameters controlling the translation of the ABAQUS input deck are defined on this form.
Note:
Main Index
The spatially varying field property values are compared within the band of +half of field properties tolerance and -half of field properties tolerance to group the elements. The property values for this group of elements are added and divided by the number of elements in this group to get the average property value to be used.
358 Patran Interface to ABAQUS Preference Guide Restart Parameters
Restart Parameters This subordinate form appears whenever the Restart Parameters button is selected. This form creates a *RESTART option (see Section 7.10.1 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 359 Optional Controls
Optional Controls This subordinate form appears whenever the Restart Parameters button is selected.
Main Index
360 Patran Interface to ABAQUS Preference Guide Direct Text Input
Direct Text Input This subordinate form appears whenever the Direct Text Input button is selectedK This widget is to facilitate the input of the ABAQUS input data that cannot be created using the functionality available in Patran. All data input here will be appended to the ABAQUS model data before the step history block.
Note:
There is no checking available for invalid input.
Note:
The font for the text input may vary from one system to another. A default font is specified in app_defaults/Patran file: Patran*fixedFont: -misc-fixed-bold-r-normal--13-100-100-100-c-70-iso8859-1 For any problems with the text on a particular system, change the font specifications in the Patran file which should reside in your ~home directory. Use xfontsel, or xlxfonts commands to get the list of available fonts on a given system.
Main Index
Chapter 3 : Running Analysis 361 Step Creation
Step Creation This subordinate form appears whenever the Step Creation button is selected on the Analysis form. A step is defined by associating the load cases created and stored on the database, with the ABAQUS analysis procedure that best addresses that load case, and the relevant associated parameters that guide the solution path for the chosen analysis procedure. There is no importance to the order in which the Job Steps are created on this form--they will be ordered for the job in the Step Selection form.
Main Index
362 Patran Interface to ABAQUS Preference Guide Step Creation
Select Load Cases This subordinate form appears whenever the Select Load Cases button is selected on the Step Creation form.
Output Requests This subordinate form appears whenever the Output Requests button is selected on the Step Create form. It is used for specifying the specific variables to be included in the output from ABAQUS options such as: ∗EL PRINT, ∗ENERGY PRINT, ∗MODAL PRINT, ∗NODE PRINT, ∗PRINT, ∗EL FILE, ∗ENERGY FILE, ∗FILE FORMAT, ∗MODAL FILE, and ∗NODE FILE *ELEMENT MATRIX OUTPUT. An explanation of the output variables that can be requested is included in the Output Requests description for each solution type.
Main Index
Chapter 3 : Running Analysis 363 Step Creation
Direct Text Input This subordinate form appears whenever the Direct Text Input button is selectedK This widget is to facilitate the input of the ABAQUS input data that cannot be created using the functionality available in Patran menus. All data input here will be appended to the ABAQUS step history being created.
Note:
There is no checking available for invalid data. The font for the text input may vary from one system to another. A default font is specified in app_defaults/Patran file:
Main Index
364 Patran Interface to ABAQUS Preference Guide Step Creation
Patran*fixedFont: -misc-fixed-bold-r-normal--13-100-100-100-c-70-iso8859-1 For any problems with the text on a particular system, change the font specifications in the Patran file which should reside in your ~home directory. Use xfontsel, or xlxfonts commands to get the list of available fonts on a given system.
Solution Types Each step has an associated Solution type, and the information that is requested on the Solution Parameters and Output Requests forms varies based on this selection. ABAQUS calls these analysis procedures, and the full explanations of these procedures can be found in Chapter 2 “Procedures Library” of the ABAQUS/Standard User’s Manual.
Main Index
Parameter Type
Description
Linear Static
Static stress analysis is used when inertia effects can be neglected. During a linear static step, the model’s response is defined by the linear elastic stiffness at the base state, the state of deformation and stress at the beginning of the step. For ∗HYPERELASTIC and ∗HYPERFOAM materials, the tangent elastic moduli in the base state is used. Contact conditions cannot change during the step--they remain as they are defined in the base state.
Natural Frequency
This solution type uses eigenvalue techniques to extract the frequencies of the current system. The stiffness determined at the end of the previous step is used as the basis for the extraction, so that small vibrations of a preloaded structure can be modeled.
Chapter 3 : Running Analysis 365 Step Creation
Parameter Type
Description
Bifurcation Buckling
Eigenvalue buckling estimates are obtained. Classical eigenvalue buckling analysis (e.g., “Euler” buckling) is often used to estimate the critical (buckling) load of “stiff” structures. “Stiff” structures are those that carry their design loads primarily by axial or membrane action, rather than by bending action. Their response usually involves very little deformation prior to buckling.
Direct Linear Transient
This solution procedure integrates all of the equations of motion through time, and is significantly more expensive than modal methods for finding dynamic response for linear systems. For linear systems, the dynamic method, using the Hilber-Hughes-Taylor operator, is unconditionally stable, meaning there is no mathematical limit on the size of the time increment that can be used to integrate a linear system. Since the procedure uses a fixed time increment, the HAFTOL parameter on the *DYNAMIC card is not required.
Direct Steady State Dynamics Calculates steady state response for the given range of frequencies. The damping may be created by dashpots, by “Rayleigh” damping associated with materials, and by viscoelasticity included in the material definitions. Modal Linear Transient
This solution type gives the response of the model as a function of time, based on a given time dependent loading. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.The number of modes extracted must be sufficient to model the dynamic response of the system adequately. This is a matter of judgment on the part of the user. The modal amplitudes are integrated through time and the response synthesized from these modal responses.
Modal Steady State Dynamics This solution type provides the response of the system when it is excited by harmonic loading at a given frequency. This procedure is usually preceded by extraction of the natural modes using the NATURAL FREQUENCY solution type, although ABAQUS also allows the response to be calculated directly from the system matrices for use in those cases where the eigenvalues cannot be extracted, such as a nonsymmetric stiffness case, or models in which the behavior is itself a function of frequency, such as frequency dependent material damping.
Main Index
366 Patran Interface to ABAQUS Preference Guide Step Creation
Main Index
Parameter Type
Description
Response Spectrum
This solution type provides an estimate of the peak response of a structure to steady-state dynamic motion of its fixed points (“base motion”). The method is typically used when an approximate estimate of such peak response is required for design purposes. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.
Random Vibration
This solution type predicts the response of a system which is subjected to a nondeterministic continuous excitation that is expressed in a statistical sense using a power spectral density function. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.
Nonlinear Static
Nonlinear static analysis requires the solution of nonlinear equilibrium equations, for which ABAQUS uses Newton’s method. Many problems involve history dependent response, so that the solution is usually obtained as a series of increments, with iteration within each increment to obtain equilibrium. For most cases, the automatic incrementation provided by ABAQUS is preferred, although direct user control is also provided for those cases where the user has experience with a particular problem.
Chapter 3 : Running Analysis 367 Step Creation
Main Index
Parameter Type
Description
Nonlinear Transient Dynamic
This solution type is used when nonlinear dynamic response is being studied. Because all of the equations of motion of the system must be integrated through time, direct integration methods are generally significantly more expensive than modal methods. For most cases, the automatic incrementation provided by ABAQUS is preferred, although direct user control is also provided for those cases where the user has experience with a particular problem.
Creep
This analysis procedure performs a transient, static, stress⁄displacement analysis. It is especially provided for the analysis of materials which are described by the ∗CREEP material form.
Viscoelastic (Time Domain)
This is especially provided for the time domain analysis of materials which are described by the ∗VISCOELASTIC, TIME material option. The dissipative part of the material behavior is defined through a Prony series representation of the normalized shear and bulk relaxation moduli, either specified directly on the ∗VISCOELASTIC, TIME material option, determined from user input creep test data, or determined from user input relaxation test data.
Viscoelastic (Frequency Domain)
This is especially provided for the frequency domain analysis of materials which are described by the ∗VISCOELASTIC, FREQUENCY material option, which is activated by a ∗STEADY STATE DYNAMICS, DIRECT procedure.The dissipative part of the material behavior is defined by the real and imaginary parts of the Fourier transforms of the nondimensional shear viscoelasticity parameter g and, for compressible materials, of the bulk viscoelasticity parameter k.
Steady State Heat Transfer
This solution type is for pure heat transfer problems for which the ∗HEAT TRANSFER option is used and where the temperature field can be found without knowledge of stress and deformation of the bodies being studied.
Transient Heat Transfer
This solution type is for pure transient heat transfer problems for which the ∗HEAT TRANSFER option is used and where the temperature field can be found without knowledge of stress and deformation of the bodies being studied. For all transient heat transfer cases, the time increments may be specified directly, or will be selected automatically based on a user prescribed maximum nodal temperature change in a step. Automatic time incrementation is generally preferred.
368 Patran Interface to ABAQUS Preference Guide Step Creation
Linear Static
Read Temperature File= This option is used to specify temperatures via the results file which has been generated from a previous heat transfer analysis. Only one temperature results file is allowed in an analysis but the same file can be referenced by many steps.
Main Index
Chapter 3 : Running Analysis 369 Step Creation
Linear Static If the selected solution type is Linear Static then the following parameters may be defined on the Output Requests form.
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. S11, S22, S33, For example, the truss element outputs the axial stress (S11) only, S12, S13, S23 while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
SINV The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The strain E components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Elem Energy Densities
The strain energy per unit volume of each element. Plastic, creep, and viscous dissipative energy densities should not be affected by linear static analysis.
ENER
Elem Energy Magnitudes
The strain energy of each element. Plastic, creep, and viscous dissipative energy densities should not be affected by linear static analysis.
ELEN
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the axial SF force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
370 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N). Displacements
Displacements are output at nodes and are referred to as follows:
STH U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degreeof-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist RF changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Chapter 3 : Running Analysis 371 Step Creation
Parameter Name
Description
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Element Mass Matrix
Mass matrices output.
Output Variable Identifier ALLEN
Element Stiffness matrices output. Stiffness Matrix Natural Frequency This subordinate form appears whenever the Solution Parameters button is selected and the solution types is Natural Frequency. This generates ∗FREQUENCY procedures (see Section 9.3.5 of the ABAQUS/Standard User’s Manual). The optional NLGEOM parameter on the ∗STEP option may be included, as defined below. None of the other optional parameters on the ∗pqbm option (AMPLITUDE, INC, or MONOTONIC) are used.
Natural Frequency
If the selected Solution Type is Natural Frequency, then the following parameters may be defined on the Output Requests form. A complete discussion of the ABAQUS results file can be found in Chapter 6 of the ABAQUS/Standard User’s Manual. Note that the Natural Frequency solution type extracts the frequency and corresponding mode shapes (eigenvalues and eigenmodes), usually for use in a later analysis (e.g., Response Spectrum). The stresses and strains corresponding to the mode shapes can be
Main Index
372 Patran Interface to ABAQUS Preference Guide Step Creation
output, but are usually of limited direct value except as a possible means for guiding mode limitations for future analyses.
Parameter Name
Output Variable Identifier
Description
S11, S22, S33, S12, S13, S23
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, First principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system.
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
SE
Chapter 3 : Running Analysis 373 Step Creation
Parameter Name
Output Variable Identifier
Description
Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time. Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
RF
Bifurcation Buckling This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Bifurcation Buckling. This form defines the data required for a *BUCKLE command (see Section 9.3.2 of the ABAQUS/Standard User’s Manual). This step may be included either as the first step or when the structure has already been preloaded. If the structure has been preloaded, the buckle sensitivity around the preloaded state is calculated. The problem is a classical eigenvalue problem, with the
Main Index
374 Patran Interface to ABAQUS Preference Guide Step Creation
eigenvalues defined as the load multipliers of the load pattern for which buckling sensitivity is being investigated.
Bifurcation Buckling
If the selected Solution Type is Bifurcation Buckling then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
The stress components output depend on the elements analyzed. S11, S22, S33, S12, For example, the truss element outputs the axial stress (S11) S13, S23 only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Chapter 3 : Running Analysis 375 Step Creation
Parameter Name
Output Variable Identifier
Description E
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Section Forces
SF Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Sectiono 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
376 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Description Displacements are output at nodes and are referred to as follows:
Output Variable Identifier U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time. Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
RF
Direct Linear Transient This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Direct Linear Transient. This generates a *DYNAMIC procedure, with the optional DIRECT parameter included (see Section 9.3.4 of the ABAQUS/Standard User’s Manual). Note that modal methods are usually more economical for linear dynamic analysis. Many of the parameters described in the ABAQUS/Standard User’s Manual for the *DYNAMIC option are not used for this option.
Main Index
Chapter 3 : Running Analysis 377 Step Creation
Direct Linear Transient
If the selected Solution Type is Direct Linear Transient then the following parameters may be defined on this form.
Parameter Name
Description
Stress Components The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual. Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Main Index
Output Variable Identifier S11, S22, S33, S12, S13, S23
SINV
E
378 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Output Variable Identifier
Elem Energy Densities
The strain energy per unit volume of each element.
ENER
Elem Energy Magnitudes
The strain energy of each element.
ELEN
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, SE these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 379 Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
380 Patran Interface to ABAQUS Preference Guide Step Creation
Direct Steady State Dynamics This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Direct Steady State Dynamics. This generates a ∗STEADY STATE DYNAMIC procedure.
Direct Steady State Dynamics
If the selected solution type is Direct Steady State Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Ph Angle Stress Components
The phase angle shift of the stress components.
PHS
Chapter 3 : Running Analysis 381 Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Ph Angle Strain Components
The phase angle shift of the strain components.
PHE
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
382 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Phase Angle Rel. Displacements
The phase angle shift of the relative displacement components.
PU
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
The phase angle shift of the reaction force components.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 383 Step Creation
Modal Linear Transient This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Modal Linear Transient. This generates a *FREQUENCY procedure (see Section 9.3.5 of the ABAQUS/Standard User’s Manual) followed by a ∗MODAL DYNAMIC procedure (see Section 9.3.8 of the ABAQUS/Standard User’s Manual). A ∗MODAL DAMPING option will also be generated, as required. Only one load case may be selected.
Main Index
384 Patran Interface to ABAQUS Preference Guide Step Creation
Modal Linear Transient
This subordinate form appears whenever the Output Request button is selected on the Step Create form, and the Solution Type is Modal Linear Transient.
Parameter Name
Description
Stress Components
S11, S22, The stress components output depend on the elements S33, S12, analyzed. For example, the truss element outputs the axial S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal tress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
Chapter 3 : Running Analysis 385 Step Creation
Parameter Name Section Strains
Description
Output Variable Identifier
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N)
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Acceleration
Nodal accelerations, following the same convention as for displacements.
A
386 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Total Displacements
The summation of all individual modal components of displacement. The output follows the same convention as for the individual modal components.
TU
Total Velocities
The summation of all individual modal components of velocity. The output follows the same convention as for the individual modal components.
TV
Total Accelerations
The summation of all individual modal components of acceleration. The output follows the same convention as for the individual modal components.
TA
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads, (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration.
GA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix Mass matrices output. Element Stiffness Matrix
Main Index
Output Variable Identifier
Stiffness matrices output.
Chapter 3 : Running Analysis 387 Step Creation
Define Damping Direct When the type of Modal Damping selected is Direct, this subordinate form appears whenever Define Damping is selected. The data is used to define the *MODAL DAMPING option (see Section 9.6.6 of the ABAQUS/Standard User’s Manual) with the MODAL parameter set to DIRECT.
Main Index
388 Patran Interface to ABAQUS Preference Guide Step Creation
Define Damping Rayleigh When the type of Modal Damping selected is Rayleigh, this subordinate form appears whenever Define Damping is selected. This form defines the data required for the *MODAL DAMPING, RAYLEIGH option (see Section 9.6.6 of the ABAQUS/Standard User’s Manual).
Base Motion This subordinate form appears whenever Define Base Motion is selected from the Modal Linear Transient, Steady State Dynamics, or Viscoelasticity Frequency Domain Solution Parameter forms. It defines the values on the ∗BASE MOTION option (see Section 9.4.2 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 389 Step Creation
Steady State Dynamics This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Steady State Dynamics. This generates a *STEADY STATE DYNAMICS procedure (see Section 9.3.13 of the ABAQUS/Standard User’s Manual). A *FREQUENCY procedure may also be created prior to the *STEADY STATE DYNAMICS procedure, if required.
Main Index
390 Patran Interface to ABAQUS Preference Guide Step Creation
Steady State Dynamics
If the selected solution type is Steady State Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Ph Angle Stress Component
The phase angle shift of the stress components.
PHS
Chapter 3 : Running Analysis 391 Step Creation
Parameter Name
Output Variable Identifier
Description
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Ph Angle Strain Component
The phase angle shift of the strain components.
PHE
Element Energy Magnitudes
A scalar value for the energy content of the element.
ELEN
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
392 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for A displacements.
Total Displacements
The summation of all individual modal components of displacement. The output follows the same convention as for the individual modal components.
TU
Total Velocities
The summation of all individual modal components of velocity. The output follows the same convention as for the individual modal components.
TV
Total Accelerations
The summation of all individual modal components of acceleration. The output follows the same convention as for the individual modal components.
TA
Phase Angle Rel. Displacements
All components of the phase angle of the displacements at the node.
PU
Phase Angle Total Displacements
All components of the phase angle of the total displacements at the node.
PTU
Chapter 3 : Running Analysis 393 Step Creation
Parameter Name
Main Index
Output Variable Identifier
Description
Reaction Forces
The forces at the nodes which are constrained and so, therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
All components of the phase angle of the reaction forces at the node.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads, (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration. GA
Phase Angle Generalized Displacements
The phase angle of displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
Phase Angle Generalized Velocities
The phase angle of velocities associated with the modes of PGV vibration.
Phase Angle Generalized Accelerations
The phase angle of accelerations associated with the modes of vibration.
PGA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration). BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, ALLEN recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
PGU
394 Patran Interface to ABAQUS Preference Guide Step Creation
Define Frequencies The data on this form is used to define the input for the *STEADY STATE DYNAMICS option (see Section 9.3.13 of the ABAQUS/Standard User’s Manual).
Response Spectrum This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Response Spectrum. This generates a *FREQUENCY procedure, and a *RESPONSE SPECTRUM procedure (see Sections 9.3.5 and 9.3.10, respectively, of the ABAQUS/Standard User’s Manual). A ∗SPECTRUM option is also created (see Section 7.11.5 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 395 Step Creation
Define Response Spectra (Response Spectrum) This subordinate form appears whenever the Define Response Spectra button is selected on the Response Spectrum Solution Parameter form.
Main Index
396 Patran Interface to ABAQUS Preference Guide Step Creation
Define Spectrum (Response Spectrum) This form appears whenever the Define Spectrum button is selected on the Response Spectra form, which is itself subordinate to the Response Spectrum Solution Parameter Form. Similar forms are used for the second and third directions.The data on this form will define the *SPECTRUM option (see Section 7.11.5 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 397 Step Creation
Response Spectrum
If the selected solution type is Response Spectrum, then the following parameters may be defined on the Output Requests form.
Main Index
398 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
SF
Chapter 3 : Running Analysis 399 Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
400 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Main Index
Description
Output Variable Identifier
Reaction Forces
The forces at the nodes which are constrained and therefore, RF resist changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Chapter 3 : Running Analysis 401 Step Creation
Parameter Name
Description
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration.
GA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Main Index
Output Variable Identifier
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
ALLEN
402 Patran Interface to ABAQUS Preference Guide Step Creation
Random Vibration This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Random Vibration. This generates a *FREQUENCY procedure and a *RANDOM RESPONSE procedure (see Sections 9.3.5 and 9.3.9 of the ABAQUS⁄Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 403 Step Creation
Define Spectrum (Random Vibration) The Spectrum Data Table form is used to define the power spectral density function data for the ∗PSDDEFINITION option (see Section 7.11.3 of the ABAQUS/Standard User’s Manual).
Main Index
404 Patran Interface to ABAQUS Preference Guide Step Creation
Random Vibration
If the selected solution type is Random Vibration, then the following parameters may be defined on the Output Requests form.
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
R.M.S. Stress Components
The root mean square value of the stress components.
RA
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
R.M.S. Strain Components
The root mean square value of the strain components.
RE
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
Chapter 3 : Running Analysis 405 Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
R.M.S. Relative Displacement
The root mean square value of the displacement components relative to the base motion.
RU
406 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
R.M.S. Relative Velocities
The root mean square value of the velocity components relative to the base motion.
RV
R.M.S. Relative Acceleration
The root mean square value of the acceleration components relative to the base motion.
RA
Total Displacements The total displacement (including base motion) of the nodes.
Main Index
Output Variable Identifier
TU
Total Velocities
The total velocity (including base motion) of the nodes.
TV
Total Acceleration
The total acceleration (including base motion) of the nodes.
TA
R.M.S. Total Displacements
The root mean square value of the displacement components including the base motion.
RTU
R.M.S. Total Velocities
The root mean square value of the velocity components including the base motion.
RTV
R.M.S. Total Accelerations
The root mean square value of the acceleration components including the base motion.
RTA
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
R.M.S. Reaction Forces
The root mean square value of the modal component of the reaction forces.
RRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibrations, each of GV which have a shape (eigenmode) and associated frequency (eigenvalue).
Generalized Accelerations
The accelerations associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GA
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Chapter 3 : Running Analysis 407 Step Creation
Parameter Name
Description
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier
Nonlinear Static This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Nonlinear Static. This generates a *STATIC procedure with the associated *STEP option. The NLGEOM parameter on the *STEP command is included. The NLGEOM parameter is included on the *STEP option.
More data input is available for defining the Nonlinear Static Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu if the Riks method is not selected.
Main Index
408 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Max No of Increments
Defines the maximum number of increments that can be used within a single step. This is a positive integer value. This is the optional INC parameter on the ∗STEP option.
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Listed below are the remaining parameters contained in this menu if the Riks method is selected.
Main Index
Parameter Name
Description
Initial Load Fraction
Defines the initial load fraction to be applied to the model. This is a real constant. This is the initial time increment data value on the ∗STATIC command.
Minimum Load Fraction
Defines the minimum load fraction which will be added during any increment. These are real constants.
Maximum Load Fraction
Defines the maximum load fraction which will be added during any increment. These are real constants.
Stopping Condition
Indicates which stopping condition is to be used. This can be set to “Max. no. increments”, “Max. load multiplier”, or “Monitor a Node.” This indicates which stopping condition data values are to be defined on the ∗STATIC option.
Max. Load Multiplier
This defines the maximum load multiplier allowed before the iteration will be stopped. This is only used if “Max. load multiplier,” or “Monitor a Node” are selected.
Node Number
Indicates the node ID to be monitored. This is only used if “Monitor a Node” is selected.
Chapter 3 : Running Analysis 409 Step Creation
Parameter Name
Description
Limit Value
Defines the limiting displacement at the node being monitored. This is only used if “Monitor a Node” is selected.
DOF Number
Indicates which degree-of-freedom at this node is to be monitored. This is only used if “Monitor a Node” is selected.
Nonlinear Static
If the selected solution type is Nonlinear Static, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier S11, S22, S33, S12, S13, S23
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
410 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Output Variable Identifier
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, creep, and viscous dissipative energy densities are reported.
ENER
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, plastic, creep, and ELEN viscous dissipative energies are reported.
Internal Stress Forces
The forces that are found at each node by summing the element NFORC stress contributions at the nodes.
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 411 Step Creation
Parameter Name Displacement
Description Displacements are output at nodes and are referred to as follows:
Output Variable Identifier U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
412 Patran Interface to ABAQUS Preference Guide Step Creation
Nonlinear Transient Dynamic This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Nonlinear Transient Dynamic. This generates a ∗DYNAMIC procedure, with the associated ∗STEP option. The DIRECT and HAFTOL parameters are available on the ∗DYNAMIC option.
Main Index
Chapter 3 : Running Analysis 413 Step Creation
More data input is available for defining the Nonlinear Transient Dynamic Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Main Index
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Max Error in Mid Increment Residual
This is the HAFTOL parameter on the ∗DYNAMIC option. See Section 9.3.4 of the ABAQUS/Standard User’s Manual and Section 5.2.1 of the ABAQUS/Standard Example Problems.
414 Patran Interface to ABAQUS Preference Guide Step Creation
Nonlinear Transient Dynamic
If the selected solution type is Nonlinear Transient Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Output Variable Identifier
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Chapter 3 : Running Analysis 415 Step Creation
Parameter Name Section Forces
Description Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
Output Variable Identifier SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SW
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, STH SAX2, SAXA1N, SAXA2N).
416 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads CF (e.g., the force at a node resulting from pressure distributions on adjacent elements).
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
ALLEN
Chapter 3 : Running Analysis 417 Step Creation
Creep This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Creep. This generates a ∗VISCO procedure, with the associated ∗STEP option.
More data input is available for defining the Creep Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Main Index
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
418 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Admissable Error in Strain Increment
This is the CETOL parameter on the ∗VISCO option. See Section 9.3.15 of the ABAQUS/Standard User’s Manual.
Creep
The strain components output depend on the elements analyzed, analogous to the stress components. In addition, the total strain component can be separated into its contributory parts (e.g., elastic strain, plastic strains, etc.) and these are reported separately.
Main Index
Output Variable Identifier
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Chapter 3 : Running Analysis 419 Step Creation
Parameter Name
Output Variable Identifier
Description
Elastic Strains
The elastic strain component of the total strain. Note that the EE elastic strain component is the component from which the stress is computed.
Inelastic Strains
The total strain minus the elastic strain component.
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
IE
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
420 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, RF resist changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 421 Step Creation
Viscoelastic (Time Domain) This subordinate form appears whenever Solution Parameters is selected and the Solution Type is Viscoelastic (Time Domain). This generates a ∗VISCO procedure, with the associated ∗STEP command.
Main Index
422 Patran Interface to ABAQUS Preference Guide Step Creation
More data input is available for defining the Viscoelastic (Time Domain) Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Viscoelastic (Time Domain)
If the selected Solution Type is Viscoelastic (Time Domain), then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
SINV The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Chapter 3 : Running Analysis 423 Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
424 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 425 Step Creation
Viscoelastic (Frequency Domain) This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Viscoelastic (Frequency Domain). This generates a *STEADY STATE DYNAMIC procedure.
Viscoelastic (Frequency Domain)
If the selected solution type is Viscoelastic (Frequency Domain), then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Ph Angle Stress Components
The phase angle shift of the stress components.
PHS
426 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Ph Angle Strain Components
The phase angle shift of the strain components.
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
PHE
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 427 Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Phase Angle Rel. Displacements
The phase angle shift of the relative displacement components.
PU
Reaction Forces
The forces at the nodes which are constrained and so, therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
The phase angle shift of the reaction force components.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
428 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier
Steady State Heat Transfer This subordinate form appears whenever Solution Parameters is selected and the solution type is Steady State Heat Transfer. This generates a ∗HEAT TRANSFER, STEADY STATE procedure.
Steady State Heat Transfer
If the selected solution type is Steady State Heat Transfer, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Element Temperature
Temperature.
TEMP
Heat Flux
Current magnitude and components of the heat flux vector. The integration of points for these values are located at the Gauss points.
HFL
Nodal Temperatures
NT All temperature values at a node. These will be the temperatures defined as degrees-of-freedom if heat transfer elements are connected to the node, or predefined temperatures if the node is only connected to stress elements without temperature degrees-of-freedom.
Reaction Fluxes
All reaction flux values (conjugate to temperature).
RFL
Chapter 3 : Running Analysis 429 Step Creation
Parameter Name
Main Index
Description
Concentrated Fluxes
All concentrated flux values.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier CFL
430 Patran Interface to ABAQUS Preference Guide Step Creation
Transient Heat Transfer This subordinate option is Transient Heat Transfer. This generates a ∗HEAT TRANSFER procedure.
Transient Heat Transfer
If the selected solution type is Transient Heat Transfer, then the following parameters may be defined on the Output Requests form.
Main Index
Chapter 3 : Running Analysis 431 Step Creation
Parameter Name
Main Index
Description
Output Variable Identifier
Element Temperature
Temperature.
TEMP
Heat Flux
Current magnitude and components of the heat flux vector. The integration of points for these values are located at the Gauss points.
HFL
Nodal Temperatures
NT All temperature values at a node. These will be the temperatures defined as degrees-of-freedom if heat transfer elements are connected to the node, or predefined temperatures if the node is only connected to stress elements without temperature degrees-of-freedom.
Reaction Fluxes
All reaction flux values (conjugate to temperature).
RFL
Concentrated Fluxes
All concentrated flux values.
CFL
Element Stiffness Matrix
Stiffness matrices output.
432 Patran Interface to ABAQUS Preference Guide Step Selection
Step Selection This subordinate form appears whenever the Step Selection button is selected on the main Analysis form. This form is used to select and order the Job Steps that will be analyzed for the ABAQUS Job.
Main Index
Chapter 3 : Running Analysis 433 Read Input File
Read Input File It is possible to read an existing ABAQUS input file (jobname.inp) into Patran. This is not a fully supported feature and must be invoked by setting a special parameter. This is done by editing the settings.pcl file and adding the following line: pref_env_set_logical( "shareware_input_file", TRUE ) If this setting is set to TRUE, then an additional Action item will appear under the Analysis form called Read Input File. This file can exist in the installation, local or home directories.
Main Index
434 Patran Interface to ABAQUS Preference Guide Read Input File
Main Index
Chapter 3 : Running Analysis 435 ABAQUS Input File Reader
ABAQUS Input File Reader This section describes a software module that reads ABAQUS input files and writes the data to the MSC/PATRAN database in a form compatible with the MSC/PATRAN ABAQUS preference.
Input Deck Formats Both fixed format and free format entries are supported. Floating point formats with and without an “E” in the exponent are supported (e.g. 1.23E6 and 1.23+6 are both supported). Message File Informative, warning, and error messages are written to an external file with the name.msg. where is the portion of the ABAQUS input file name before the suffix and is a unique version number beginning with 01. After import, this file should be carefully examined to understand what was processed by the reader and what was not. Sometimes the error messages will indicate where minor editing of the input deck will convert an unsupported entity to one that can be handled by the reader.
ABAQUS ELSET and NSET Entries A PATRAN group is created for each ABAQUS ELSET or NSET entry. The name of the group is taken from the NAME parameter of the ELSET or NSET. Supported Element Types When the reader encounters a *ELEMENT entry, the combination of the element type and the ABAQUS property set entry are used to map the ABAQUS element type to the appropriate PATRAN element type. In some cases this is not possible because not all ABAQUS element types are currently supported in PATRAN. In these cases, the reader attempts to find the PATRAN element type that “best” matches the ABAQUS type. Thus, the ABAQUS elements retain their association to their property set. This allows the finite element mesh to be edited in PATRAN and an ABAQUS input deck output that can be easily edited to correct the property entry. Supported Keywords The table below describes the ABAQUS keywords that are supported in the current version of the product.
ABAQUS Keyword
Notes Model Section
Main Index
*AMPLITUDE
A PATRAN time- or frequency-dependent field is created.
*BEAM GENERAL SECTION
A PATRAN property set is created.
436 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
ABAQUS Keyword
Notes
*BEAM SECTION
A PATRAN property set is created.
*BOUNDARY
A PATRAN LBC set is created for each ABAQUS BOUNDARY and added to all load cases. Displacement, temperature, velocity, and acceleration boundary conditions are currently supported.
*CENTROID
Location is added to the PATRAN property set.
*CONDUCTIVITY
Value is added to the PATRAN material.
*CONTACT NODE SET
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*CONTACT PAIR
A PATRAN contact-type LBC set is created for each entry in *CONTACT PAIR.
*CORRELATION *DAMPING
Value is added to the PATRAN material or shell element property set.
*DASHPOT
A PATRAN property set is created.
*DENSITY
Value is added to the PATRAN material.
*ELASTIC
Values are added to the PATRAN material.
*ELCOPY
Element Generation Command
*ELEMENT
PATRAN elements are created. Both a PATRAN group and a property set are created with the ELSET name.
*ELGEN
PATRAN elements are created.
*ELSET
A PATRAN group is created.
*EQUATION
A PATRAN MPC is created. The use of node sets in *EQUATION entries is not currently supported.
*EXPANSION
Values are added to the PATRAN material.
*FRICTION
The *FRICTION keyword is supported within *GAP, *INTERFACE, and *SURFACE INTERACTION blocks. The friction properties are added to the appropriate property or LBC set.
*GAP
A PATRAN property set is created.
*HEADING
A PATRAN analysis job is created with this description.
*HOURGLASS STIFFNESS The values are added to the appropriate PATRAN property set.
Main Index
*INCLUDE
The referenced file is read. *INCLUDE entries may be nested to any reasonable depth.
*MASS
A PATRAN property set is created.
*MATERIAL
A PATRAN material is created.
*MEMBRANE SECTION
A PATRAN property set is created.
Chapter 3 : Running Analysis 437 ABAQUS Input File Reader
ABAQUS Keyword *MPC
Notes A PATRAN MPC is created. The use of node sets in *MPC entries is not currently supported.
*MODAL DAMPING *NCOPY
Generates additional nodes using NID and X/Y/Z offsets.
*NFILL
PATRAN nodes are created. The SINGULAR option is not currently supported.
*NGEN
PATRAN nodes are created. Nodes may be generated along a line or a circular arc (LINE=C) but not along a parabola (LINE=P).
*NODAL THICKNESS
A PATRAN nodal FEM field and property set are created.
*NODE
PATRAN nodes are created. If an NSET parameter is specified, a PATRAN group is created with this name, otherwise the nodes are added to the default group.
*NSET
A PATRAN group is created.
*ORIENTATION
Is used to define orientation for homogeneous or laminate material properties.
*PLASTIC
Only HARDENING=ISOTROPIC and HARDENING=KINEMATIC are currently supported. The RATE parameter is not currently supported; only the first set *PLASTIC entries for a material are imported.
*PSD
Main Index
*RIGID BODY
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*RIGID SURFACE
The *RIGID SURFACE keyword is currently supported in two ways by the PATRAN, ABAQUS preference. For the older style of ABAQUS contact, which required the use of IRSx type elements, *RIGID SURFACE entries were written out for “rigid surface type” element properties. For the newer style of ABAQUS contact ,which uses *CONTACT PAIR, geometric curves are selected directly in a PATRAN contact-type LBC. Only this second usage of *RIGID SURFACE is supported by the reader. When referenced in a *CONTACT PAIR entry, curves are created and references to them added to the contact-type LBC set.
*ROTARY INERTIA
A PATRAN property set is created.
*SECTION POINTS
Points are added to the PATRAN property set.
*SHEAR CENTER
Location is added to the PATRAN property set.
*SHELL GENERAL SECTION
A PATRAN property set is created.
*SHELL SECTION
A PATRAN property set is created.
438 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
ABAQUS Keyword *SOLID SECTION
Notes A PATRAN property set is created.
*SPECTRUM *SPECIFIC HEAT
Value is added to the PATRAN material.
*SPRING
A PATRAN property set is created.
*SURFACE DEFINITION
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*SURFACE INTERACTION The only keyword currently supported within this block is *FRICTION. The keyword parameters and friction data are added to the appropriate contact-type LBC set. *SYSTEM
PATRAN node locations are transformed to the coordinate system defined on this entry.
*TRANSFORM
A PATRAN coordinate frame is created and used to define the analysis system for the node.
*TRANSVERSE SHEAR STIFFNESS
The values are added to the appropriate PATRAN property set. History Section
Main Index
*BOUNDARY
A PATRAN LBC set is created for each ABAQUS BOUNDARY and added to the load case for this step. Displacement, temperature, velocity, and acceleration boundary conditions are currently supported.
*BUCKLE
The parameters associated with this entry are added to the PATRAN analysis step.
*CFLUX
A PATRAN LBC set is created for each ABAQUS CFLUX and added to the load case for this step.
*CLOAD
A PATRAN LBC set is created for each ABAQUS CLOAD and added to the load case for this step.
*DFLUX
A PATRAN LBC set is created for each ABAQUS DFLUX and added to the load case for this step.
*DLOAD
A PATRAN LBC set is created for each ABAQUS DLOAD and added to the load case for this step. The pressure DLOAD types as well as GRAV, CENT, CENTRIF, and CORIO are currently supported.
*DYNAMIC
The parameters associated with this entry are added to the PATRAN analysis step.
*FILM
A PATRAN LBC set is created for each ABAQUS FILM and added to the load case for this step.
*FREQUENCY
The parameters associated with this entry are added to the PATRAN analysis step.
Chapter 3 : Running Analysis 439 ABAQUS Input File Reader
ABAQUS Keyword
Notes
*HEAT TRANSFER
The parameters associated with this entry are added to the PATRAN analysis step.
*MODAL DYNAMIC
The parameters associated with this entry are added to the PATRAN analysis step.
*STATIC
The parameters associated with this entry are added to the PATRAN analysis step.
*STEADY STATE DYNAMICS
The parameters associated with this entry are added to the PATRAN analysis step.
*STEP
A PATRAN load case and an analysis job step are created for each ABAQUS step. The parameters on the *STEP entry are added to the analysis step
*TEMPERATURE
A PATRAN LBC set is created for each ABAQUS TEMPERATURE and added to the load case for this step.
*VISCO
The parameters associated with this entry are added to the PATRAN analysis step.
Both fixed format and free format entries are supported. The table below shows the PATRAN element property options that are created when a specific ABAQUS element type is imported. Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element
ABAQUS Element AC1D2 AC1D3 AC2D4 AC2D8 AC3D20 AC3D8 ACAX4 ACAX8 ASI1 ASI2 ASI2A ASI3
Dim 1D 1D 2D 2D 3D 3D 2D 2D 0D 1D 1D 2D
Name IRS (planar/axisym) ISL (in plane) Rigid Surface(LBC) 2D Interface Solid Solid Rigid Surface(LBC) 2D Interface IRS (single node) IRS (planar/axisym) IRS (planar/axisym) IRS (shell/solid)
ASI3A ASI4
2D 2D
Shell IRS (shell/solid)
Option1 Axisymmetric Axisymmetric
Option2 Elastic Slip Hard Contact Lagrange Soft Contact
Axisymmetric Homogeneous Homogeneous
Lagrange Vis Damping Standard Formulation Hybrid
Axisymmetric Planar Axisymmetric Axisymmetric Elastic Slip Hard Contact General Large Strain Lagrange Hard Contact
Lagrange Vis Damping Elas Slip Vis Damping Elastic Slip Hard Contact Elastic Slip Hard Contact
Homogeneous
440 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1 ABAQUS Element ASI8 B21 B21H B22 B22H B23 B23H B31 B31H B31OS B31OSH B32 B32H B32OS B32OSH B33 B33H B34 C1D2 C1D2H C1D2T C1D3 C1D3H C1D3T C3D10 C3D10E C3D10H C3D10M C3D10MH C3D15 C3D15E C3D15H C3D15V C3D15VH C3D20 C3D20E C3D20H C3D20HT C3D20P
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D
Name 2D Interface Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Truss Truss Truss Truss Truss Truss Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid
Option1 Axisymmetric General Section General Section General Section General Section General Section General Section General Section General Section Open Section Open Section General Section General Section Open Section Open Section General Section General Section General Section Standard Formulation Hybrid Hybrid Standard Formulation Hybrid Standard Formulation Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
Option2 Lagrange Vis Damping Standard Formulation Hybrid Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
Standard Formulation Homogeneous Hybrid Modified Formulation Modified/Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Standard Formulation
Chapter 3 : Running Analysis 441 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element C3D20PH C3D20R C3D20RE C3D20RH
Dim 3D 3D 3D 3D
Solid Solid Solid Solid
Option1 Homogeneous Homogeneous Homogeneous Homogeneous
C3D20RHT C3D20RP C3D20RPH C3D20RT C3D20T C3D27 C3D27H C3D27R C3D27RH
3D 3D 3D 3D 3D 3D 3D 3D 3D
Solid Solid Solid Solid Solid Solid Solid Solid Solid
Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
C3D4 C3D4E C3D4H C3D6 C3D6E C3D6H C3D8 C3D8E C3D8H C3D8HT C3D8I C3D8IH
3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D
Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid
Homogeneous Standard Formulation Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
C3D8R C3D8RH
3D 3D
Solid Solid
Homogeneous Homogeneous
C3D8T CAX3 CAX3E CAX3H CAX4 CAX4E CAX4H CAX4HT
3D 2D 2D 2D 2D 2D 2D 2D
Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Homogeneous Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Name
Option2 Standard Formulation Reduced Integration Standard Formulation Hybrid/Reduced Integration Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Hybrid Hybrid Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation
442 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CAX4I CAX4IH
Dim 2D 2D
Name 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric
CAX4P CAX4PH CAX4R CAX4RH
2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAX4T CAX6 CAX6E CAX6H CAX6M CAX6MH CAX8 CAX8E CAX8H CAX8HT CAX8P CAX8PH CAX8R CAX8RE CAX8RH
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAX8RHT CAX8RP CAX8RPH CAX8RT CAX8T CAXA41 CAXA42 CAXA43 CAXA44 CAXA4H1 CAXA4H2 CAXA4H3 CAXA4H4 CAXA4R1 CAXA4R2
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Incompatible Modes Hybrid/Incompatible Modes Standard Formulation Standard Formulation Reduced Integration Hybrid/Reduced Integration Standard Formulation Standard Formulation Axisymmetric Hybrid Modified Formulation Modified/Hybrid Standard Formulation Hybrid Hybrid Hybrid Hybrid Hybrid Reduced Integration Hybrid Hybrid/Reduced Integration Hybrid Hybrid Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Hybrid Reduced Integration Reduced Integration
Chapter 3 : Running Analysis 443 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CAXA4R3 CAXA4R4 CAXA4RH1
Dim 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric Axisymmetric
CAXA4RH2
2D
2D Solid
Axisymmetric
CAXA4RH3
2D
2D Solid
Axisymmetric
CAXA4RH4
2D
2D Solid
Axisymmetric
CAXA81 CAXA82 CAXA83 CAXA84 CAXA8H1 CAXA8H2 CAXA8H3 CAXA8H4 CAXA8P1 CAXA8P2 CAXA8P3 CAXA8P4 CAXA8R1 CAXA8R2 CAXA8R3 CAXA8R4 CAXA8RH1
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAXA8RH2
2D
2D Solid
Axisymmetric
CAXA8RH3
2D
2D Solid
Axisymmetric
CAXA8RH4
2D
2D Solid
Axisymmetric
CAXA8RP1 CAXA8RP2 CAXA8RP3 CAXA8RP4 CGAX3
2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Reduced Integration Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Reduced Integration Reduced Integration Reduced Integration Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid Hybrid Hybrid Hybrid Standard Formulation
444 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CGAX3H CGAX4 CGAX4H CGAX4I CGAX4IH
Dim 2D 2D 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CGAX4R CGAX4RH
2D 2D
2D Solid 2D Solid
Axisymmetric Axisymmetric
CGAX6 CGAX6H CGAX8 CGAX8H CGAX8R CGAX8RH
2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CGPE10 CGPE10H CGPE10R CGPE10RH
2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid
General Plane Strain General Plane Strain General Plane Strain General Plane Strain
CGPE5 CGPE5H CGPE6 CGPE6H CGPE6I CGPE6IH
2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
General Plane Strain General Plane Strain General Plane Strain General Plane Strain General Plane Strain General Plane Strain
CGPE6R CGPE6RH
2D 2D
2D Solid 2D Solid
General Plane Strain General Plane Strain
CGPE8 CGPE8H
2D 2D
2D Solid 2D Solid
General Plane Strain General Plane Strain
Option2 Hybrid Standard Formulation Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Axisymmetric Hybrid Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Standard Formulation Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid
Chapter 3 : Running Analysis 445 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CONN2D2
Dim 1D
Name Mech Joint (2D Model)
CONN3D2
1D
Mech Joint (3D Model)
CPE3 CPE3E CPE3H CPE4 CPE4E
2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Option1 ALIGN AXIAL BEAM CARTESIAN JOIN JOINTC LINK ROTATION SLOT TRANSLATOR WELD ALIGN AXIAL BEAM CARDAN CARTESIAN CONSTANT VELOCITY CVJOINT CYLINDRICAL EULER FLEXION-TORSION HINGE JOIN JOINTC LINK PLANAR RADIAL-THRUST REVOLUTE ROTATION SLIDE-PLANE SLOT TRANSLATOR UJOINT UNIVERSAL WELD Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain
Option2
Standard Formulation Plane Strain Hybrid Standard Formulation Reduced Integration
446 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CPE4H CPE4HT CPE4I CPE4IH
Dim 2D 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid
Option1 Plane Strain Plane Strain Plane Strain Plane Strain
CPE4R CPE4RH
2D 2D
2D Solid 2D Solid
Plane Strain Plane Strain
CPE4T CPE6 CPE6E CPE6H CPE8 CPE8E CPE8H CPE8HT CPE8P CPE8PH CPE8R CPE8RE CPE8RH
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain
CPE8RHT CPE8RP CPE8RPH
2D 2D 2D
2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Strain
CPE8RT CPE8T CPS3 CPS3E CPS4 CPS4E CPS4I CPS4R CPS4T CPS6 CPS6E CPS6M CPS8
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress
Option2 Hybrid Reduced Integration Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Reduced Integration Standard Formulation Standard Formulation Hybrid Standard Formulation Reduced Integration Hybrid Reduced Integration Standard Formulation Hybrid Reduced Integration Reduced Integration Hybrid/Reduced Integration Reduced Integration Reduced Integration Hybrid/Reduced Integration Reduced Integration Reduced Integration Standard Formulation Plane Stress Standard Formulation Reduced Integration Incompatible Modes Reduced Integration Reduced Integration Standard Formulation Standard Formulation Modified Formulation Standard Formulation
Chapter 3 : Running Analysis 447 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CPS8E CPS8R CPS8RE CPS8RT CPS8T DASHPOT1 DASHPOT2 DASHPOTA DC1D2 DC1D2E DC1D3 DC1D3E DC2D3 DC2D4 DC2D6 DC2D8 DC3D10 DC3D15 DC3D20 DC3D4 DC3D6 DC3D8 DCAX3 DCAX4 DCAX6 DCAX8 DCC1D2 DCC1D2D DCC2D4 DCC2D4D
Dim 2D 2D 2D 2D 2D 0D 1D 1D 1D 1D 1D 1D 2D 2D 2D 2D 3D 3D 3D 3D 3D 3D 2D 2D 2D 2D 1D 1D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid Grounded Damper Damper Damper Link Link Link Link 2D Solid 2D Solid 2D Solid 2D Solid Solid Solid Solid Solid Solid Solid 2D Solid 2D Solid 2D Solid 2D Solid IRS (planar/axisym) IRS (planar/axisym) 2D Solid 2D Solid
Option1 Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Linear Linear Linear
Option2 Standard Formulation Reduced Integration Standard Formulation Standard Formulation Standard Formulation
Planar Planar Planar Planar Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Planar Planar
Standard Formulation Standard Formulation Standard Formulation Standard Formulation
DCC3D8 DCC3D8D
3D 3D
Solid Solid
DCCAX2 DCCAX2D DCCAX4
1D 1D 2D
IRS (planar/axisym) IRS (planar/axisym) 2D Solid
Convection/Diffusion Convection/Diffusion with Dispersion Control Axisymmetric Axisymmetric Axisymmetric
Fixed Direction Standard Formulation
Standard Formulation Standard Formulation Standard Formulation Standard Formulation Elastic Slip Hard Contact Elastic Slip Hard Contact Convection/Diffusion Convection/Diffusion with Dispersion Control
Elastic Slip Hard Contact Elastic Slip Hard Contact Convection/Diffusion
448 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element DCCAX4D
Dim 2D
Name 2D Solid
DINTER1 DINTER2 DINTER2A DINTER3 DINTER3A DINTER4 DINTER8 DS4 DS8 DSAX1 DSAX2 ELBOW31
1D 2D 2D 2D 2D 3D 3D 2D 2D 1D 1D 1D
1D Interface 2D Interface 2D Interface 2D Interface 2D Interface 3D Interface 3D Interface Shell Shell Axisym Shell Axisym Shell Beam in Space
ELBOW31B
1D
Beam in Space
ELBOW31C
1D
Beam in Space
ELBOW32
1D
Beam in Space
F2D2 F3D3 F3D4 FAX2 FLINK GAPCYL GAPSPHER GAPUNI
1D 2D 2D 1D 1D 1D 1D 1D
IRS (planar/axisym) Shell Rigid Surface(LBC) IRS (planar/axisym) Link Gap Gap Gap
INTER1 INTER1P INTER1T INTER2
1D 1D 1D 2D
IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) IRS (shell/solid)
INTER2A INTER2AT INTER2T
2D 2D 2D
2D Interface 2D Interface IRS (shell/solid)
Option1 Axisymmetric
Planar Axisymmetric Planar Axisymmetric
Option2 Convection/Diffusion with Dispersion Control
Lagrange Vis Damping
Homogeneous Homogeneous Homogeneous Homogeneous Curved with Pipe Section Curved with Pipe Section Curved with Pipe Section Curved with Pipe Section Axisymmetric General Large Strain
Elastic Slip Hard Contact Homogeneous
Axisymmetric
Elastic Slip Hard Contact
Cylindrical Spherical Uniaxial
True Distance Elas Slip Vis Damping Lagrange Vis Damping No Sep Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact
Axisymmetric Axisymmetric Axisymmetric Lagrange Hard Contact Axisymmetric Axisymmetric Lagrange Hard Contact
Standard Formulation Ovalization Only Ovaliz Only with Approximated Fourier Standard Formulation
Lagrange Hard Contact Lagrange Hard Contact
Chapter 3 : Running Analysis 449 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element INTER3 INTER3A INTER3AP INTER3AT INTER3P INTER3T INTER4
Dim 2D 2D 2D 2D 2D 2D 3D
Name 2D Interface 2D Interface 2D Interface 2D Interface 2D Interface 2D Interface 3D Interface
INTER4T
3D
3D Interface
INTER8 INTER8T INTER9
3D 3D 3D
3D Interface 3D Interface 3D Interface
IRS12 IRS13 IRS21 IRS21A IRS22 IRS22A IRS3
0D 0D 1D 1D 1D 1D 2D
IRS (single node) IRS (single node) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane) IRS (shell/solid)
IRS31 IRS32 IRS4
1D 1D 2D
IRS (planar/axisym) ISL (in plane) IRS (shell/solid)
IRS9
2D
IRS (shell/solid)
ISL21 ISL21A ISL21AT ISL21T ISL22 ISL22A ISL22AT ISL31 ISL31A ISL32 ISL32A
1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D
IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane) ISL (in plane) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane)
Option1 Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Lagrange Vis Damping Lagrange Vis Damping Elas Slip Vis Damping Elas Slip Vis Damping Lagrange Vis Damping Planar Planar Axisymmetric Axisymmetric Axisymmetric Axisymmetric Elastic Slip Hard Contact Axisymmetric Axisymmetric Lagrange Hard Contact Lagrange Hard Contact Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping
Elas Slip Vis Damping Elas Slip Vis Damping Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact
Elastic Slip Hard Contact Lagrange Soft Contact
Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact Lagrange Soft Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact
450 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1 ABAQUS Element ISP1 ISP1T ISP3 ISP4 ISP4T JOINTC LS6 M3D3 M3D4 M3D4R M3D6 M3D8 M3D8R M3D9 M3D9R MASS MAX1 MAX2 MGAX1 MGAX2 PIPE21 PIPE21H PIPE22 PIPE22H PIPE31 PIPE31H PIPE32 PIPE32H R2D2 R3D3 R3D4 RAX2 RB2D2 RB3D2 ROTARYI S3 S3R S4 S4R
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 0D 0D 2D 2D 2D 1D 2D 2D 2D 2D 2D 2D 2D 2D 2D 0D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 2D 2D 1D 1D 1D 0D 2D 2D 2D 2D
Name IRS (single node) IRS (single node) Shell Shell Shell IRS (planar/axisym) Shell Membrane Membrane Membrane Membrane Membrane Membrane Membrane Membrane Mass IRS (planar/axisym) ISL (in plane) IRS (planar/axisym) ISL (in plane) Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in Space Beam in Space IRS (planar/axisym) Rigid Surface(LBC) Rigid Surface(LBC) IRS (planar/axisym) Rigid Line(LBC) Rigid Line(LBC) Rotary Inertia Shell Shell Shell Shell
Option1 Planar Planar Thick General Large Strain General Large Strain Axisymmetric Thin Standard Formulation Standard Formulation Reduced Integration Standard Formulation Standard Formulation Reduced Integration Standard Formulation Reduced Integration
Option2 Elas Slip Vis Damping Elas Slip Vis Damping Homogeneous Homogeneous Homogeneous Elastic Slip Hard Contact Homogeneous
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Axisymmetric
Elastic Slip Hard Contact Lagrange Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Elastic Slip Hard Contact
Axisymmetric
Elastic Slip Hard Contact
Thick General Large Strain General Large Strain Thick
Homogeneous Homogeneous Homogeneous Homogeneous
Chapter 3 : Running Analysis 451 ABAQUS Input File Reader
Table 3-1 ABAQUS Element S4R5 S8R S8R5 S8RT S9R5 SAX1 SAX2 SAX2T SAXA11 SAXA12 SAXA13 SAXA14 SAXA21 SAXA22 SAXA23 SAXA24 SPRING1 SPRING2 SPRINGA STRI3 STRI35 STRI65 T2D2 T2D2E T2D2H T2D2T T2D3 T2D3E T2D3H T2D3T T3D2 T3D2E T3D2H T3D2T T3D3 T3D3E T3D3H T3D3T
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 2D 2D 2D 2D 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 0D 1D 1D 2D 2D 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D
Name Shell Shell Shell Shell Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Grounded Spring Spring Spring Shell Shell Shell Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss
Option1 Thin Thick Thin Thick Thin Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Linear Linear Linear Thick Thin Thick Hybrid Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation
Option2 Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
Fixed Direction Standard Formulation Homogeneous Homogeneous Homogeneous
452 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Under some circumstances, the values of the option menus in Patran (Option 1 and Option 2) may be different than shown in the table. This is often the case when the ABAQUS element is one that is not directly supported by the Patran interface and the translator is making a “best guess” at which Patran element to choose. For many beam elements in the table, Option 1 is shown as “General Section”. Depending on the beam cross section type defined on the *BEAM SECTION or *BEAM GENERAL SECTION entry, Option 1 may be General Section, Box Section, Circular Section, Hexagonal Section, I Section, Pipe Section, Rectangular Section, or Trapezoid Section. For the 3D solid elements and shell elements in the table, Option 1 is shown as Homogeneous. Depending on the *SHELL SECTION or *SHELL GENERAL SECTION entry, Option 1 may be either Homogeneous or Laminate.
Main Index
Chapter 4: Read Results Patran Interface to ABAQUS preference Guide
4
Main Index
Read Results
Review of the Read Results Form
Translation Parameters
Select Results File
Data Translated from the Analysis Code Results File
Key Differences between Attach and Translate Methods
Delete Result Attachment Form
454
457
458
466
463 464
454 Patran Interface to ABAQUS preference Guide Review of the Read Results Form
Review of the Read Results Form By choosing the Analysis toggle located on the Patran main form, an Analysis form will appear.
Selecting Read Results as the Action on the Analysis form allows you to read results data into the Patran database from a text (“jobname”.fin) or binary (“jobname”.fil) ABAQUS results file, or to access ABAQUS results directly from an ABAQUS results output database (“jobname”.odb). Other forms that are accessible from here are used to define translation parameters and select the ABAQUS results file. These forms are described on the following pages.
Upgrading ABAQUS ODB Results Files Since the ABAQUS DRA in Patran is integrated with the ABAQUS 6.3-1 libraries, you must make sure your ODB results files have been upgraded to 6.3 before attempting to attach to them from within Patran. This can be done in one of two ways: Manually Upgrade ODB Files The procedure for upgrading ODB files is part of ABAQUS: abaqus upgrade job=job-name odb=old-odb-file-name Automatic Upgrade of ODB Files If you want to automatically upgrade your older ODB results files, you can set the following environment variable: Setenv ABAQUS_DRA_UPGRADE_ODB=YES By setting this variable, Patran will make a copy of the ODB results file and upgrade the copy to the current version of ABAQUS.
Main Index
Chapter 4: Read Results 455 Review of the Read Results Form
Read Results Form Read Results defines the type of data to be read from the analysis code results file into Patran. The Object box may only be set to Results Entities.
Main Index
456 Patran Interface to ABAQUS preference Guide Review of the Read Results Form
Flat File Results In some cases, the translation will not be able to write the data directly into the Patran database. In those cases, a text file will be created containing all the instructions as to how this data is to be loaded into the database. This file can be transferred between computers if necessary, then read into the proper database using the File Import functionality. The full functionality of this form is described in Working with Files (p. 45) in the Patran Reference Manual.
Main Index
Chapter 4: Read Results 457 Translation Parameters
Translation Parameters The Translation Parameters form is used to define filters for the data being accessed.
Attach Method There is only one filter control for the Attach method, which indicates whether or not to allow access to the results invariants, as calculated by Abaqus.
Translate and Control File Methods Translation parameters for the Translate and Control File methods include the results filtering options based on the step number and the increment number. If none of the options are specified, then all the results will be translated. If only step is specified, then all the increments in that step will be translated. If only increment is specified, then that increment for the first step will be translated. If both step and increment are specified, then only the increment for that step will be translated.
Main Index
458 Patran Interface to ABAQUS preference Guide Select Results File
Select Results File The Select file form allows you to select a file to be read. There are several features available. This form is brought up when you select the Select Results File button on the Read Results form. The default file filters will change depending on the Current analysis code in the Preferences menu.
Results Created in Patran For direct ODB access (Attach method), no results are created in Patran, and all result types represented within the field output data in the ODB file are available for postprocessing. The following table indicates all the possible results quantities which can be loaded into the Patran database during results translation (Translate method) from ABAQUS. The Primary and Secondary Labels are the items you select from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor. This determines which postprocessing techniques will be available to view this results quantity. Post Codes indicates which ABAQUS element post codes the data comes from. The Description gives a brief discussion about the results quantity. The Output Requests forms use the actual
Main Index
Chapter 4: Read Results 459 Select Results File
primary and secondary labels that will appear in the results. For example, if “Strain, Elastic” is selected on the Element Output Requests form, the “Strain, Elastic” is created for postprocessing. Table 4-1
Results Quantities Loaded into Patran During Translation
Primary Label Acceleration
Base Motion Change in Length Concentrated Flux (Nodal) Concentrated Deformation Displacements Elastic Strain Energy Density
Energy in Element
Total Energy
Force and Shear Force
Main Index
Secondary Label Generalized Rotational Generalized Translational Rotational Translational Rotational Translational Components Layer or Section Points Load Moment Displacements Rotations Generalized Displacements Generalized Rotations Components Artificial Strain Energy Creep Dissipation Plastic Dissipation Strain Energy Viscous Dissipation Artificial Strain Energy Creep Dissipation Kinetic Energy Plastic Dissipation Strain Energy Viscous Dissipation Total Artificial Strain Energy Total Creep Dissipation Total Energy Loss at Impact Total External Work Total Kinetic Total Plastic Dissipation Total Strain Total Viscous Dissipation Components
Type Vector Vector Vector Vector Vector Vector Tensor Scalar Vector Vector Vector Vector Vector Vector Tensor Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Tensor
Results Key 303 303 103 103 304 304 21 206 106 106 101 101 301 301 25 14 14 14 14 14 19 19 19 19 19 19 1999 1999 1999 1999 1999 1999 1999 1999 11
460 Patran Interface to ABAQUS preference Guide Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Force Frequency Heat Flux (Nodal) Heat Flux Inelastic Strain Internal Flux (Nodal) Internal Forces Mass Flux Modal
Mag-Phase Strain Mag-Phase Stress Phase Angle
Mag-Phase Reaction Mag-Phase Reaction Mag-Phase Displacements Mag-Phase Acceleration Mag-Phase Velocity Mag-Phase Displacements Mag-Phase Velocity Mag-Phase Total Displacement Mag-Phase Total Acceleration Mag-Phase Total Velocity Mag-Phase Total Displacement Mag-Phase Total Acceleration
Main Index
Secondary Label Components Steady State Dynamics Components Components Magnitude Components Layer or Section Points Components at Element Node Components Magnitude Composite Damping Effective Mass Eigen Values Generalized Mass Participation Factor Components Components Generalized Displacements Generalized Rotational Acceleration Generalized Rotational Velocities Generalized Rotations Generalized Translational Accelerations Generalized Translational Velocities Force Moment Displacements Rotational Rotational Rotations Translational Translational
Type Tensor Scalar Vector Vector Scalar Tensor Scalar Vector Vector Scalar Scalar Scalar Scalar Scalar Scalar Tensor Tensor Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector
Results Key 11 2000 10 28 28 24 214 15 39 39 1980 1980 1980 1980 1980 65 62 305 307 306 305 307 306 135 135 111 137 136 111 136 112
Rotational
Vector
140
Rotational Rotational
Vector Vector
139 112
Translational
Vector
140
Chapter 4: Read Results 461 Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Mag-Phase Total Velocity Mag-Phase Acceleration Plastic Strain
Pressure and Shear Stresses RMS Strain RMS Stress Reaction Relative Displacements and Shear Slips Rel. Normal & Tangential Displacements Residual Flux (Nodal) Root Mean Square
Strain
Main Index
Secondary Label Translational Translational Components Equivalent Magnitude Yield Flag Components
Type Vector Vector Tensor Scalar Scalar Scalar Tensor
Results Key 139 137 22 22 22 22 11
Components Components Force Moment Components
Tensor Tensor Vector Vector Tensor
66 63 104 104 21
Components
Tensor
21
Layer and Section Points Reaction Forces Reaction Moments Relative Displacements Relative Rotational Accelerations Relative Rotational Velocities Relative Rotations Relative Translational Velocities Total Displacements Total Rotational Accelerations Total Rotational Velocities Total Rotations Total Translational Accelerations Total Translational Velocities Relative Translational Accelerations Components
Scalar Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Tensor
204 134 134 123 131 127 123 127 124 132 128 124 132 128 131 21
462 Patran Interface to ABAQUS preference Guide Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Stress
Temperature (Nodal) Temperature Total Acceleration Total Displacement Total Velocity Total
Velocity
Creep Strain
Main Index
Secondary Label 1st Principal 2nd Principal 3rd Principal 3rd Stress Invariant Components Hydrostatic Pressure Maximum Stress in Section Mises Tresca Layer or Section Points Element Centroidal Temperature Rotational Translational Rotational Translational Rotational Translational Creep Time Dynamic Time Heat Transfer Time Soils Time Time Generalized Rotational Generalized Translational Rotational Translational Components Equivalent Magnitude Yield Flag
Type Scalar Scalar Scalar Scalar Tensor Scalar Scalar Scalar Scalar Scalar Scalar Vector Vector Vector Vector Vector Vector Scalar Scalar Scalar Scalar Scalar Vector Vector Vector Vector Tensor Scalar Scalar Scalar
Results Key 12 12 12 12 11 12 16 12 12 201 2 115 115 113 113 114 114 2000 2000 2000 2000 2000 302 302 102 102 23 23 23 23
Chapter 4: Read Results 463 Data Translated from the Analysis Code Results File
Data Translated from the Analysis Code Results File When reading model data from an ABAQUS results file, the following table defines all the data which will be created. No other model data is extracted from the results file. This data should be sufficient for evaluating any results values.
Item Nodes
Results Key 1901
Description Node ID Nodal Coordinates
Elements
1900
Element ID Nodal Connectivity
Groups
n/a, ODB access only
Group name Node and Element references Groups are generated for each part instance, as well as for each node and element set.
Main Index
464 Patran Interface to ABAQUS preference Guide Key Differences between Attach and Translate Methods
Key Differences between Attach and Translate Methods The most obvious difference between direct ODB access (Attach method) and results translation (Translate method) is that the results are not imported into the Patran database in the case of the former, while they are for the latter. Direct access avoids redundancy and saves disk space, while Translation uses more disk space, but takes less time to retrieve results for postprocessing. The following sections describe other differences that users should be aware of, before deciding which method to use.
Result Type Naming Conventions The names used for the result types within an ODB attachment come directly from the field output description fields of the ODB database. Using the “direct access” philosophy of bringing the data in asis, there is no attempt to map those names to the same names used by the Translate method (listed in Table 4-1). Therefore, direct ODB access will use Abaqus terminology exclusively in generating the result type names. The primary name is equal to the field output description field, while the secondary name is the field output key. For example, the stress tensor result type is “Stress components, S”, where “Stress components” is the field output description, and “S” is the field output key.
Vector vs. Scalar Moment and Rotational Results For results such as reaction moments or rotational displacements, the ODB database saves space by only storing results for the non-zero component, whenever possible. So, if non-zero values for moments only occur in the Z component, then the ODB database stores it as a scalar result (e.g. key RM3). However, the Translate method will import the results as vector results, with the X and Y values always being zero. This difference may cause confusion when comparing translated results against direct ODB access via the quick or fringe plot operations, where reaction moments and rotational displacements are concerned. The default “invariant” for fringe plots of vector data is “Magnitude”, which is always a positive value. If the magnitude of the translated vector data is compared against the ODB scalar data, then they will not always match (all negative data from the ODB access will be flipped positive in the translated plot). To compare “apples with apples”, one must display the appropriate component (Z from our example) from the translated case, and compare that against the scalar (key RM3) from the direct ODB access case.
Main Index
Chapter 4: Read Results 465 Key Differences between Attach and Translate Methods
Reaction Forces During translation, only non-zero reaction force data is imported. Direct ODB access, on the other hand, returns zero vectors for any nodes that do not have any reaction forces. This makes no difference for the display of reaction force vectors; however, if one displays a fringe plot distribution of the reaction forces, the fringe plots vary between translation and direct ODB access dramatically. The translation plot is all black, with only the min/max values displayed on a hidden line plot; while the ODB fringe plot shows a color distribution from the zero values (white over most of the model) to the non-zero values. For the latter, the contours only vary over elements with nodes having non-zero reaction forces.
Main Index
466 Patran Interface to ABAQUS preference Guide Delete Result Attachment Form
Delete Result Attachment Form The following form may be used to remove a results attachment, created via the Attach method, from the database.
Main Index
Chapter 5 : Files Patran Interface to ABAQUS Preference Guide
5
Files
Main Index
Files
468
468 Patran Interface to ABAQUS Preference Guide Files
Files There are several files associated which are either used or created by the Patran ABAQUS Application Preference. The following table describes each file and how it is used. In the definition of the file names, any occurrence of “jobname” would be replaced with the jobname the user assigns.
File Name
Main Index
Description
jobname.db
This is the Patran database from which the model data is read during an analyze pass, and into which model and⁄or results data is written during a Read Results pass.
jobname.jbm jobname.jbr
These are small files used to pass certain information between Patran and the Application Preference during translation. You should never have need to do anything directly with these files.
jobname.inp
This is the ABAQUS input file created by the interface.
jobname.fil
This is the ABAQUS results file which is read by the Read Results pass.
jobname.flat
This file may be generated during a Read Results pass. If the results translation cannot, for any reason, write data directly into the jobname.db Patran database, it will create this jobname.flat file.
jobname.msg
These message files contain any diagnostic output from the translation, either forward or reverse.
AbaqusExecute
This is a UNIX script file which is called on to submit both the forward PAT3ABA translation program, as well as to submit ABAQUS after translation is complete. This file should be customized for your particular site installation.
ResultsSubmit
This is another UNIX script which is called on to submit the reverse, ABAPAT3 translation program. This file should also be customized for your particular site.
load_abaqus.ses
This file is only used when creating a new Patran template database. This file loads in all the element, material, MPCs and loads and boundary condition tables for the Patran ABAQUS product.
Chapter 6 : Errors/Warnings Patran Intreface to ABAQUS Preference Guide
6
Errors/Warnings
Main Index
Errors/Warnings
470
470 Patran Intreface to ABAQUS Preference Guide Errors/Warnings
Errors/Warnings There are several error or warning messages which may be generated by the Patran ABAQUS Application Preference.
Message
Main Index
Description
Fatal
This error stops the translation and exits the Preference.
Warning
Some expected action did not execute. Translation continues. Check the .msg file.
Information
General Messages about the translation.
jp`Kc~íáÖìÉ=nìáÅâ=pí~êí=dìáÇÉ
Index Patran Interface to ABAQUS Preference Guide få Ç É ñ= Index
Numerics 1D interface, 96, 104, 151 2D interface, 101, 104 2D orthotropic, 81 2D orthotropic lamina, 54 2D solid, 100, 104 3D anisotropic, 56, 84 3D anisotropic thermal, 88 3D interface, 103, 105, 312 3D orthotropic, 55, 82 3D orthotropic thermal, 87
A abapat3, 4 ABAQUS, 3 abaqus.plb, 4, 5 AbaqusExecute, 468 AbaqusSubmit, 5, 7 acceleration, 334, 340 Acommand, 7 amplitude, 14 analysis, 354 arbitrary beam, 127 area moment I12, 126 average shear stiffness, 254 axisymmetric 2D interface, 279 axisymmetric ISL, 156 axisymmetric shell, 95, 104, 148 laminate, 149 axisymmetric solid, 273
B base motion, 15, 388
Main Index
beam, 28, 32 circular, 122 cross-sectional shape, 122 elements, 16, 17, 18 general section, 11, 117, 125 hexagonal, 122 in space, 93 in XY plane, 92 section, 11 bifurcation buckling, 365, 373, 374 bilinear, 28, 36 boundary, 14, 15 box beam, 119 buckle, 15
C C biquad, 29, 39 cap hardening, 13, 78 plasticity, 13 centrifugal force, 339 centroid, 11 centroid coordinate, 126 CETOL, 418 CFLUX, 15 change material status, 52 circular beam, 122 solid, 122 clearance zero damping, 114, 117, 153 clearance zero-pressure, 114, 117, 153 CLOAD, 15 combined creep test data, 71 combined test data, 13 composite, 56, 88, 319 conductivity, 13 constitutive models, 52 control, 104 convection, 104, 334, 348 convection/diffusion, 320, 323
472 Patran Interface to ABAQUS Preference Guide
coordinate frames, 22 Coriolis force, 339 correlation, 15 creep, 13, 54, 55, 56, 79, 80, 367, 417, 418 creep test data, 71 cubic hybrid, 92, 93 cubic initially straight, 93 cubic interpolation, 92, 93 curved pipe, 130
D damper, 94 damping, 13 direct, 387 Rayleigh, 388 zero clearance, 114, 117, 153 dashpot, 12 elements, 19 DASHPOT1, 110 DASHPOT2, 142, 144 DASHPOTA, 141, 143 deformation plasticity, 13, 54, 73 degree-of-freedom, 30 density, 13, 67, 88 DFLUX, 15 diffusion, 104 direct linear transient, 365, 376, 377 direct steady state dynamics, 365, 380 direct text input, 360, 363 dispersion, 104 displacement, 334, 337 DLOAD, 15 Drucker-Prager, 13, 77 dynamic, 15
E eigenvalue, 364 eigenvalue buckling, 365 EL file, 16, 362 print, 16, 362 elastic, 13, 53, 54, 55, 56, 58, 81, 82, 83 elastic slip, 113, 116, 152, 154, 157, 160, 162,
Main Index
165, 168, 170, 278, 280, 282, 314 hard contact, 92 no separation, 92 soft contact, 92 vis damping, 92 vis damping no separation, 92 elbow, 29, 42 elements, 19 MPC, 42 ELBOW31, 42, 130 ELBOW31B, 130 ELBOW32, 42, 130 element, 11, 25 definition, 11 matrix output, 16, 362 properties, 90 elements beam, 16, 17, 18 dashpot, 19 elbow, 19 gap, 20 heat transfer, 20, 21 mass, 19 membrane, 18 rigid surface contact, 20 rotary inertia, 19 shell, 19 slide line contact, 20 small sliding contact, 20 spring, 19 ELSET, 11, 352 end step, 15 energy file, 16, 362 print, 16, 362 engineering constants, 82 equation, 14, 28, 31 expansion, 13, 67 explicit, 28
F fatal, 470
INDEX
file EL, 16, 362 energy, 16, 362 format, 16, 362 modal, 16, 362 node, 16, 362 output definition, 16 film, 15 finite elements, 23 flat file results, 456 force, 334, 337 Frac Clearance Const Damping, 114, 117, 153 fraction of critical damping, 59 frequency, 15, 394 friction, 12, 112 Friction in Dir_1, 113, 116 Friction in Dir_2, 116
G gap, 12, 95 conductance, 12, 317, 324 cylindrical, 145 elements, 20 radiation, 12, 317, 324 spherical, 147 uniaxial, 145 GAPCYL, 146 GAPSPHER, 147 GAPUNI, 146 general beam, 117, 124 general large strain, 266 general thick, 262 general thick shell laminated, 264 general thin, 258 general thin shell laminated, 261 gravity loads, 339 grounded damper, 92 grounded spring, 92 group, 352
H HAFTOL, 412, 413 hard contact, 114, 117, 153, 155, 158, 160, 163,
Main Index
166, 169, 171, 278, 281, 283, 314 harmonic loading, 365 heat flux, 334, 349 heat source, 334, 349 heat transfer, 15 elements, 20, 21 hexagonal beam, 122 Hilber-Hughes-Taylor operator, 365 host, 7 hourglass stiffness, 12, 255 bending, 254, 257, 260, 263, 266, 269 membrane, 254, 257, 260, 263, 266, 269 normal, 254, 257, 260, 263, 266, 269 hybrid, 92, 93, 100, 269, 310 integration, 100 modes, 100 hyperbolic, 80 hyperelastic, 13, 53, 60, 61, 62, 63, 64, 65, 66, 68 hyperfoam, 13, 67
I import input file, 433 incompatible modes, 100, 269, 270, 272, 273, 274, 310 inertia rotary, 12 inertial load, 334, 339 information, 470 initial conditions, 14 initial temperature, 334, 350 initial velocity, 334, 339 input data, 334 interface, 12, 112 IRS, 97, 102, 112, 115 axisymmetric, 167 beam/pipe, 169 planar, 164 shell/solid, 281 single node, 92 IRS12, 112 IRS13, 115 I-section, 123 ISL, 96, 97
473
474 Patran Interface to ABAQUS Preference Guide
isotropic, 53, 58, 75 thermal, 86
J jobname.db, 468
K kinematic, 76 constraints, 14
L Lagrange hard contact, 92 no separation, 92 soft contact, 92 vis damping, 92 vis damping no separation, 92 Lamina, 81 laminate, 56, 89 large strain, 265 latent heat, 13 linear, 28, 34 linear damper, 109, 141, 142 grounded, 109 linear spring, 108, 137, 138 grounded, 108 linear static, 364, 368, 369 linear surf-surf, 28 linear surf-surf MPC, 34 linear surf-vol, 28 linear surf-vol MPC, 34, 35 linear vol-vol, 28 linear vol-vol MPC, 36 link, 28, 33, 104 load cases, 351, 362 loading definition, 15 loads and boundary conditions, 332 L-section beam, 132
M mass, 12, 92, 106 elements, 19 mass proportional damping, 59
material, 13 change status, 52 definition, 13 orientation, 14 temperature dependent, 53 materials, 51 form, 52 maximum friction stress, 114, 117, 152 maximum negative pressure, 114, 117, 153 maximum overclosure, 114, 117, 153 membrane, 101, 275 elements, 18 Mises/Hill, 74, 75, 76 modal damping, 15 dynamic, 15 file, 16, 362 print, 16, 362 steady state dynamics, 365 modal linear transient, 365, 383, 384 modified Drucker-Prager/Cap, 78 Moony Rivlin, 62 MPC, 14 elbow, 42 explicit, 31 linear surf-surf, 34 linear surf-vol, 34, 35 linear vol-vol, 36 pin, 43 quad surf-surf, 37 quad surf-vol, 37, 38 quad vol-vol, 39 revolute, 44 rigid fixed, 32 rigid pinned, 33 slider, 40 SS bilinear, 48 SS linear, 47 SSF bilinear, 49 tie, 43 universal, 47 V Local, 46 multi-point constraints, 27
N natural frequency, 364, 371
Main Index
INDEX
Neo Hookean, 62 Newton’s method, 366 no compression, 13 no sliding contact, 114, 117, 153 no tension, 13 node, 11, 23 definition, 11 file, 16, 362 print, 16, 362 nondeterministic continuous excitation, 366 nonlinear damper, 110, 143, 144 grounded, 110 nonlinear spring, 109, 139, 140 grounded, 109 nonlinear static, 366, 407, 409 nonlinear transient dynamic, 367, 412, 414 NSET, 11, 23, 352
O object tables, 336 Ogden, 60, 61, 63, 64, 66, 68 open beam, 134 optional controls, 359 orientation, 14, 22, 89 system, 253 output requests, 362
P parallel ISL, 158 pat3aba, 4 peak response, 366 perfect plasticity, 74 pin, 43 pin MPC, 43 pipe beam, 123 planar 2D interface, 277 ISL, 153 test data, 13 plane strain, 269, 270 plane stress, 272 plastic, 13, 54, 55, 56, 74, 75, 76, 77, 78 point mass, 106 Poisson parameter, 118, 121, 126, 128, 133, 136
Main Index
Poisson’s ratio, 67 polynomial, 60, 62, 63, 65 potential, 13 power spectral density, 403 preferences, 10 analysis, 10 preprint, 16 prescribed boundary conditions, 15 pressure, 334, 337 pressure zero clearance, 114, 117, 153 pre-tension, 347 print, 16, 362 definition, 16 EL, 16, 362 energy, 16, 362 modal, 16, 362 node, 16, 362 procedure definition, 15 Prony, 70, 367 property definition, 11 PSD-Definition, 14
Q quad surf-surf, 29 quad surf-surf MPC, 37 quad surf-vol, 29 quad surf-vol MPC, 37, 38 quad vol-vol, 29 quad vol-vol MPC, 39 quadratic, 29, 37
R radial ISL, 161 random response, 15 random vibration, 366, 402, 403, 404 rate dependent, 13 read input file, 433 read results, 454, 455 read temperature file, 368 rebar 2D, 285 rectangular beam, 124 reduced integration, 100, 269, 270, 272, 273, 274, 275, 310 reference temperature, 59 relaxation test data, 72
475
476 Patran Interface to ABAQUS Preference Guide
response spectrum, 15, 366, 394, 395, 396, 397 restart, 14 restart parameters, 358 results file select, 458 ResultsSubmit, 5, 468 revolute, 29, 44 revolute MPC, 44 rigid fixed, 28 pinned, 28 rigid fixed MPC, 32 rigid line, 98 LBC, 175 rigid pinned MPC, 33 rigid surf, 98, 102 rigid surface, 11, 112, 115, 165, 167, 170, 171, 172, 174, 175, 281, 283 axisymmetric, 173 Bezier 2D, 174 Bezier 3D, 283 cylindrical, 172 LBC, 284 segments, 171 rigid surface contact elements, 20 ROTARI, 107 rotary inertia, 12, 92, 107 elements, 19 rough (no slip) friction, 114, 117, 153, 155, 158, 160, 163, 166, 169, 278, 281, 283, 314 rough parameter, 171
S Scratchdir, 7 section point coordinate, 126 shear centroid coordinate, 126 shear factor, 118, 121, 126, 129, 134, 136 shear test data, 13 shell, 100, 104 elements, 19 general section, 12, 262 section, 12, 255 simple shear test data, 14 slide line, 11, 97, 163
Main Index
slide line contact elements, 20 slider, 29, 40 slider MPC, 40 sliding friction, 113, 154, 157, 159, 162, 165, 168, 170, 282 slip tolerance, 113, 116, 152 small sliding contact elements, 20 soft contact, 114, 117, 153, 155, 158, 160, 163, 166, 169, 171, 278, 280, 283, 314 solid, 103, 105, 310 solid section, 12 solution types, 364 specific heat, 14, 88 spectrum, 14 spring, 12, 94 elements, 19 SPRING1, 108, 109 SPRING2, 138, 140 SPRINGA, 137, 139 SS bilinear, 29, 30, 38, 48 SS bilinear MPC, 48 SS linear, 28, 30, 35, 47 SS linear MPC, 47 SSF bilinear, 30, 49 SSF bilinear MPC, 49 standard formulation, 92, 93, 100, 104 static, 15, 334 steady state dynamics, 15, 389, 390 steady state heat transfer, 367, 428 steady state response, 365 step, 15 creation, 361 initialization, 15 selection, 432 termination, 15 stiffness hourglass, 12 transverse shear, 13 stiffness in stick, 113, 117, 152 stiffness proportional damping, 59 strain, 79 surface contact, 12, 279
INDEX
T tabular formula, 69 tangent elastic moduli, 364 TAUMAX, 152, 155, 158, 160, 163, 166, 169, 171, 278, 280, 283, 314 temperature, 15, 334, 338 thermal, 334, 348 temperature dependent material, 53 test data combined, 13 creep, 71 creep combined, 71 Ogden, 66 planar, 13 relaxation, 72 shear, 13 simple shear, 14 uniaxial, 14 volumetric, 14 thermal 1D interface, 317 thermal axisymmetric shell, 315 laminated, 316 thermal expansion coefficient, 59, 67 thermal interface planar, 321 solid, 324 thermal link, 314 thermal planar solid, 320 thermal shell, 318 laminated, 319 thermal solid, 323 thermal strain, 59 thick shell, 255 laminated, 257 thin shell, 252 laminated, 254 tie, 29, 43 tie MPC, 43 time, 79 time dependent loading, 365 torsional constant, 126, 135 transform, 11, 22 transient, 335 transient heat transfer, 367, 430 translation parameters, 357, 457
Main Index
transverse shear stiffness, 13, 122, 125, 127 trapezoid beam, 124 true distance, 95 truss, 94, 136
U uniaxial test data, 14 universal, 30, 47 universal MPC, 47
V V Local, 29, 46 V Local MPC, 46 velocity, 334, 340 VISCO, 15, 417 viscoelastic, 14, 54, 55, 56, 69, 70, 71, 72 frequency domain, 367, 425 time domain, 367, 421, 422 volumetric pressure, 67 volumetric test data, 14, 67
W warning, 470 warping constant, 136 wavefront minimization, 14
X XY plane definition, 126, 128
Y yield, 14
477
478 Patran Interface to ABAQUS Preference Guide
Main Index
Main Index
Corporate
Europe
Asia Pacific
MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 USA Telephone: (800) 345-2078 Fax: (714) 784-4056
MSC.Software GmbH Am Moosfeld 13 81829 Munich, Germany Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6
MSC.Software Japan Ltd. Shinjuku First West 8F 23-7 Nishi Shinjuku 1-Chome, Shinjuku-Ku Tokyo 160-0023, JAPAN Telephone: (81) (3)-6911-1200 Fax: (81) (3)-6911-1201
Worldwide Web www.mscsoftware.com
Disclaimer This documentation, as well as the software described in it, is furnished under license and may be used only in accordance with the terms of such license. MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. The concepts, methods, and examples presented in this text are for illustrative and educational purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem or design. MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. User Documentation: Copyright ©2008 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved. This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of MSC.Software Corporation is prohibited. The software described herein may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. Contains IBM XL Fortran for AIX V8.1, Runtime Modules, (c) Copyright IBM Corporation 1990-2002, All Rights Reserved. MSC, MSC/, MSC Nastran, MD Nastran, MSC Fatigue, Marc, Patran, Dytran, and Laminate Modeler are trademarks or registered trademarks of MSC.Software Corporation in the United States and/or other countries. NASTRAN is a registered trademark of NASA. PAM-CRASH is a trademark or registered trademark of ESI Group. SAMCEF is a trademark or registered trademark of Samtech SA. LS-DYNA is a trademark or registered trademark of Livermore Software Technology Corporation. ANSYS is a registered trademark of SAS IP, Inc., a wholly owned subsidiary of ANSYS Inc. ACIS is a registered trademark of Spatial Technology, Inc. ABAQUS, and CATIA are registered trademark of Dassault Systemes, SA. EUCLID is a registered trademark of Matra Datavision Corporation. FLEXlm is a registered trademark of Macrovision Corporation. HPGL is a trademark of Hewlett Packard. PostScript is a registered trademark of Adobe Systems, Inc. PTC, CADDS and Pro/ENGINEER are trademarks or registered trademarks of Parametric Technology Corporation or its subsidiaries in the United States and/or other countries. Unigraphics, Parasolid and I-DEAS are registered trademarks of UGS Corp. a Siemens Group Company. All other brand names, product names or trademarks belong to their respective owners.
P3*2008R1*Z*ABAQUS*Z* DC-USR
Main Index
Contents Patran Interface to ABAQUS Preference Guide
1
Overview Purpose
2
ABAQUS Product Information
3
What is Included with this Product?
4
Patran ABAQUS Integration with Patran Configuring the ABAQUS Submit File
2
Building A Model Introduction to Building a Model Coordinate Frames
22
Finite Elements 23 Nodes 23 Elements 25 Multi-Point Constraints Material Library Materials Form
10
27
51 52
Element Properties 90 Element Properties Form 90 Loads and Boundary Conditions Loads & Boundary Conditions Form Load Cases Group
3
351
352
Running an Analysis Review of the Analysis Form
Main Index
354
332 332
5 7
ii Patran Interface to ABAQUS Preference Guide
Analysis Form
355
Translation Parameters Restart Parameters Optional Controls Direct Text Input
357 358
359 360
Step Creation 361 Select Load Cases 362 Output Requests 362 Direct Text Input 363 Solution Types 364 Step Selection
432
Read Input File
433
ABAQUS Input File Reader 435 Input Deck Formats 435 ABAQUS ELSET and NSET Entries
4
435
Read Results Review of the Read Results Form 454 Upgrading ABAQUS ODB Results Files 454 Read Results Form 455 Flat File Results 456 Translation Parameters 457 Attach Method 457 Translate and Control File Methods
457
Select Results File 458 Results Created in Patran 458 Data Translated from the Analysis Code Results File Key Differences between Attach and Translate Methods 464 Result Type Naming Conventions 464 Vector vs. Scalar Moment and Rotational Results Reaction Forces 465 Delete Result Attachment Form
Main Index
466
464
463
CONTENTS iii
5
Files Files
6
468
Errors/Warnings Errors/Warnings
Main Index
470
iv Patran Interface to ABAQUS Preference Guide
Main Index
Chapter 1: Overview Patran Interface to ABAQUS Preference Guide
1
Main Index
Overview
Purpose
ABAQUS Product Information
What is Included with this Product?
Patran ABAQUS Integration with Patran
Configuring the ABAQUS Submit File
2 3 4 5 7
2 Patran Interface to ABAQUS Preference Guide Purpose
Purpose Patran comprises a suite of products written and maintained by MSC.Software Corporation. The core of the product suite is a finite element analysis pre and postprocessor. The Patran system also includes several optional products such as advanced postprocessing programs, tightly coupled solvers, and interfaces to third party solvers. This document describes one of these interfaces. See the Patran User Manual for more information. The Patran ABAQUS Application Preference Guide provides a communication link between Patran and ABAQUS. It also provides customization of certain features that can be activated simply by selecting ABAQUS as the analysis code preference in Patran. Patran ABAQUS is integrated into Patran. The casual user will never need to be aware that separate programs are being used. For the expert user, there are three main components of Patran ABAQUS: several PCL files to provide the customization of Patran for ABAQUS, PAT3ABA to convert model data from the Patran database into the analysis code input file, and ABAPAT3 to translate results and⁄or model data from the analysis code results file into the Patran database. Selecting ABAQUS as the analysis code under the “Analysis Preference” menu customizes Patran in five main areas: 1. MPCs 2. Material Library 3. Element Library 4. Loads and Boundary Conditions 5. Analysis forms PAT3ABA translates model data directly from the .Patran database into the analysis code-specific input file format. This translation must have direct access to the originating Patran database. The program name indicates the direction of translation: from Patran to ABAQUS. ABAPAT3 translates results and⁄or model data from the analysis code-specific results file into the Patran database. This program can be run such that the data is loaded directly into the Patran database, or if incompatible computer platforms are being used, an intermediate file can be created. The program name indicates the direction of translation: from ABAQUS to Patran.
Main Index
Chapter 1: Overview 3 ABAQUS Product Information
ABAQUS Product Information ABAQUS is a general-purpose finite element computer program for structural and thermal analyses. It is developed, supported, and maintained by Hibbitt, Karlsson, and Sorensen, Inc., 1080 Main Street, Pawtucket, Rhode Island 02860, (401) 727-4200. See the ABAQUS User’s Manual for a general description of ABAQUS’ capabilities.
Main Index
4 Patran Interface to ABAQUS Preference Guide What is Included with this Product?
What is Included with this Product? The Patran ABAQUS product includes all of the following items: 1. A PCL library file, abaqus.plb, contains Patran ABAQUS-specific definitions. 2. The executable programs pat3aba and abapat3 which perform the forward and results translation of data. Although these programs are separate executables, they are run from within Patran, and are transparent to the user. 3. Script files are also included to drive the programs in item 2. These script files are started by Patran and control the running of the programs in Patran ABAQUS. 4. This Application Preference User’s Manual is included as part of the product. An on-line version is also provided to allow you direct access to this information from within Patran.
Main Index
Chapter 1: Overview 5 Patran ABAQUS Integration with Patran
Patran ABAQUS Integration with Patran Two diagrams are shown below to indicate how these files and programs fit into the Patran environment. In some cases, site customization of some of these files is indicated. Please see the Patran Installation and Operations Guide for more information on this topic. Figure 1-1 shows the process of running an analysis. The abaqus.plb library defines the various
Translation Parameter, Solution Type, Solution Parameter, and Output Request forms called by the Analysis form. When the Apply button is selected on the Analyze form, a.jba file is created, and the script AbaqusSubmit is started. This script may need to be modified for your site installation. The script, in turn, starts the PAT3ABA forward translation. Patran operation is suspended at this time. PAT3ABA reads data from the database and creates the ABAQUS input deck. A message file is also created to record any translation messages. If PAT3ABA finishes successfully, and you have requested it, the script will then start ABAQUS.
Figure 1-1
Forward Translation
Figure 1-2 shows the process of reading information from an analysis results file. When the Apply button is selected on the Read Results form, a .jbr file is created, depending on whether model or results data is to be read. The ResultsSubmit script is also started. This script may need to be modified for
Main Index
6 Patran Interface to ABAQUS Preference Guide Patran ABAQUS Integration with Patran
your site installation. The script, in turn, starts the ABAPAT3 results translation. The Patran database is closed while this translation occurs. A message file is created to record any translation messages. ABAPAT3 reads the data from the ABAQUS results file. If ABAPAT3 can find the desired database, the results will be loaded directly into it. If, however, it cannot find the database (for example, if you are running on several incompatible platforms), ABAPAT3 will write all the data into a flat file. This flat file can be taken to wherever the database is and read in using the read file selections.
Figure 1-2
Main Index
Results Translation
Chapter 1: Overview 7 Configuring the ABAQUS Submit File
Configuring the ABAQUS Submit File The AbaqusSubmit script file controls the execution of the PAT3ABA translator and the ABAQUS analysis code. It is located in the Patran directory called
Main Index
8 Patran Interface to ABAQUS Preference Guide Configuring the ABAQUS Submit File
Main Index
Chapter 2: Building A Model Patran Interface to ABAQUS Preference Guide
2
Main Index
Building A Model
Introduction to Building a Model
Coordinate Frames
Finite Elements
23
Material Library
51
Element Properties
Loads and Boundary Conditions
Load Cases
Group
352
351
10
22
90 332
10 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Introduction to Building a Model There are many aspects to building a finite element analysis model. In several cases, the forms used to create the finite element data are dependent on the selected analysis type. Other parts of the model are created using standard forms. Under Preferences on the Patran main form is a selection for Analysis Settings. Analysis Settings defines the intended analysis code which is to be used for this mode.
The specified code may be changed at any time during model creation. As much data as possible will be converted if the analysis code is changed after the modeling process has already begun. The setting of this option defines what will be presented in several areas during the subsequent modeling steps. These areas include the material and element libraries (including multi-point constraints), the applicable loads and boundary conditions, and the analysis forms. The selected Analysis Type may also affect the allowable selections in these same areas. For more details, see Analysis Codes (p. 426) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 11 Introduction to Building a Model
Supported ABAQUS Commands The following tables summarize all the ABAQUS commands supported by the Patran ABAQUS Preference Guide. The tables indicate where in this guide you can find more information on how the commands are supported Table 2-1
Supported ABAQUS Model Definition Options
History Definition Options
ABAQUS/ Standard Section #
Initial Options
∗HEADING
• p. 334
7.2.1
Node Definition
∗NODE
• p. 18
7.3.6
∗NSET
• p. 18
7.3.8
∗TRANSFORM
• p. 16
7.3.11
∗ELEMENT
• p. 19
7.4.2
∗ELSET
• p. 328
7.4.2
∗RIGID SURFACE
• p. 154,
∗SLIDE LINE
• p. 147
∗BEAM GENERAL SECTION
• p. 106,
p. 113,
∗BEAM SECTION
• p. 108,
p. 115 to p. 119,
*CENTROID
• p. 114
Element Definition
Property Definition
Main Index
Command
Patran Interface to ABAQUS Preference Guide Page No.
p. 155,
p. 156
p. 261
7.4.7 7.4.8
p. 121
7.5.2 7.5.3 7.5.2
12 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-1 History Definition Options
Property Definition (continued)
Supported ABAQUS Model Definition Options (continued)
Command
Patran Interface to ABAQUS Preference Guide Page No.
∗DASHPOT
• p. 100,
∗FRICTION
• p. 102 to p. 104,
p. 132,
• p. 136 to p. 145,
p. 148 to p. 152
• p. 255 to p. 259,
p. 289
• p. 132,
p. 133,
p. 294,
∗GAP
p. 101,
ABAQUS/ Standard Section #
p. 128 to p. 131
7.5.5
p. 133,
7.5.7
p. 298
7.5.8
7.5.13
• p. 300
*GAP CONDUCTANCE *GAP RADIATION
• p. 294,
p. 298,
p. 300
∗HOURGLASS STIFFNESS
• p. 232,
p. 235,
p. 238,
p. 241,
• p. 244,
p. 246,
p. 248,
p. 251,
• p. 252,
p. 254,
p. 287
• p. 102,
p. 104,
p. 136,
p. 138,
• p. 140,
p. 142,
p. 145,
p. 148,
• p. 150,
p. 152,
p. 255,
p. 257,
• p. 259,
p. 289,
p. 294,
p. 298,
∗INTERFACE
7.5.14
• p. 300
∗MASS
• p. 96
7.5.17
∗ROTARY INERTIA
• p. 97
7.5.18
∗SHELL GENERAL SECTION
• p. 238,
p. 241,
p. 246
∗SHELL SECTION
• p. 80,
p. 134,
p. 135,
p. 232,
• p. 234,
p. 235,
p. 237,
p. 244,
• p. 292,
p. 293,
p. 295,
p. 296
• p. 123,
p. 248,
p. 251,
p. 252,
• p. 254,
p. 287,
p. 291,
p. 297,
∗SOLID SECTION
7.5.19 7.5.20
7.5.21
• p. 299
Main Index
∗SPRING
• p. 98,
p. 99,
p. 124 to p. 127
∗SURFACE CONTACT
• p. 103,
p. 136,
p. 255,
• p. 259,
p. 289
p. 257,
7.5.26
Chapter 2: Building A Model 13 Introduction to Building a Model
Table 2-1 History Definition Options
Supported ABAQUS Model Definition Options (continued)
Command ∗TRANSVERSE SHEAR STIFFNESS
Material Definition
Material Definition (continued)
Main Index
Patran Interface to ABAQUS Preference Guide Page No. • p. 107,
p. 108,
p. 110,
p. 113,
• p. 115,
p. 119,
p. 121,
p. 232,
• p. 234,
p. 235,
p. 237,
p. 238,
• p. 241,
p. 244,
p. 246
ABAQUS/ Standard Section # 7.5.27
∗MATERIAL
• p. 44
7.6.2
∗CAP HARDENING
• p. 69
7.6.4
∗COMBINED TEST DATA
• p. 69
∗CAP PLASTICITY
• p. 69
∗CONDUCTIVITY
• p. 77,
p. 78,
∗CREEP
• p. 70,
p. 71
7.6.9
∗DAMPING
• p. 49,
p. 72 to p. 75
7.6.11
∗DEFORMATION PLASTICITY
• p. 64
∗DENSITY
p. 49 to p. 59,
∗DRUCKER-PRAGER
• p. 69
∗ELASTIC
• p. 49,
7.6.5 7.6.8
p. 79
7.6.12 p. 72 to p. 79
7.6.13 7.6.16
p. 72,
p. 73,
p. 74,
7.6.17
• p. 75
∗EXPANSION
p. 49 to p. 59,
∗HYPERELASTIC
p. 51 to p. 56
∗HYPERFOAM
• p. 57,
p. 59
7.6.23
∗LATENT HEAT
• p. 57,
p. 59
7.6.27
∗NO COMPRESSION
• p. 57,
p. 59
7.6.29
∗NO TENSION
• p. 57,
p. 59
7.6.30
∗PLANAR TEST DATA
• p. 69
∗PLASTIC
• p. 65,
∗POTENTIAL
• p. 65 to p. 67,
∗RATE DEPENDENT
• p. 65 to p. 68
∗SHEAR TEST DATA
• p. 69
p. 72 to p. 79
7.6.18 7.6.22
p. 66,
p. 67 p. 70,
7.6.34 p. 71
7.6.37
14 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-1
Supported ABAQUS Model Definition Options (continued)
History Definition Options
Command
Patran Interface to ABAQUS Preference Guide Page No.
∗SIMPLE SHEAR TEST DATA
• p. 69
∗SPECIFIC HEAT
• p. 77,
∗UNIAXIAL TEST DATA
• p. 69
∗VISCOELASTIC
• p. 60,
p. 78,
p. 79
p. 61,
p. 62,
ABAQUS/ Standard Section #
7.6.40
p. 63
7.6.43
∗VOLUMETRIC TEST • p. 69 DATA • p. 68
∗ORIENTATION
• p. 80,
7.6.44 p. 232,
p. 234,
p. 235,
p. 237,
p. 238,
p. 241,
p. 244,
p. 246,
p. 248,
p. 251,
p. 287,
p. 295,
p. 296,
p. 297,
p. 299
∗BOUNDARY
• p. 313,
p. 317,
p. 318
∗EQUATION
• p. 24
7.8.3
∗MPC
• p. 25 to p. 42
7.8.4
Initial Conditions
∗INITIAL CONDITIONS
• p. 316,
7.9.1
Restart Options
∗RESTART
• p. 332
7.10.1
Miscellaneous Model Options
∗AMPLITUDE
• p. 346
7.11.1
∗PSD-DEFINITION
• p. 378
7.11.3
∗SPECTRUM
• p. 374
7.11.5
∗WAVEFRONT MINIMIZATION
• p. 334
7.11.9
Material Orientation
Kinematic Constraints
Main Index
*YIELD
p. 326
7.7.1
9.5.1
Chapter 2: Building A Model 15 Introduction to Building a Model
The following ABAQUS History Definition options are supported. Table 2-2
Supported ABAQUS History Definition Options
History Definition Options Step Initialization/ Termination
*STEP
• p. 336, p. 390,
ABAQUS/ Standard Section No.
p. 346, p. 382, p. 386, 9.2.1 p. 394, p. 402
∗END STEP
• p. 336
9.2.2
∗BUCKLE
• p. 349
9.3.2
∗DYNAMIC
• p. 352,
p. 386
9.3.4
∗FREQUENCY
• p. 359,
p. 366, p. 374, p. 377
9.3.5
∗HEAT TRANSFER
• p. 401,
p. 402
9.3.7
∗MODAL DYNAMIC
• p. 359
9.3.8
∗RANDOM RESPONSE • p. 377
9.3.9
∗RESPONSE SPECTRUM
• p. 374
9.3.10
∗STATIC
• p. 382
9.3.12
∗STEADY STATE DYNAMICS
• p. 366,
p. 370
9.3.13
∗VISCO
• p. 390,
p. 394
9.3.15
∗BASE MOTION
• p. 359,
p. 365, p. 366
9.4.2
∗CFLUX
• p. 325
9.4.4
∗CLOAD
• p. 313
9.4.5
∗DFLUX
• p. 325
9.4.9
∗DLOAD
• p. 314,
∗FILM
• p. 324
9.4.12
∗TEMPERATURE
• p. 314
9.4.18
Prescribed Boundary Conditions
∗BOUNDARY
• p. 318
9.5.1
Miscellaneous History Options
∗CORRELATION
• p. 377
9.4.6
∗MODAL DAMPING
• p. 359 to p. 364
9.6.6
Procedure Definition
Loading Definition
Main Index
Command
Patran Interface to ABAQUS Preference Guide Page No.
p. 316
9.4.10
16 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-2
Supported ABAQUS History Definition Options (continued)
History Definition Options
Command
Print Definition
File Output Definition
ABAQUS/ Standard Section No.
Patran Interface to ABAQUS Preference Guide Page No.
∗EL PRINT
• p. 338
9.8.2
∗ENERGY PRINT
• p. 338
9.8.3
∗MODAL PRINT
• p. 338
9.8.4
∗NODE PRINT
• p. 338
9.8.6
• p. 338
9.8.7
∗EL FILE
• p. 338
9.9.2
∗ELEMENT MATRIX OUTPUT
• p. 338
∗ENERGY FILE
• p. 338
9.9.3
FILE FORMAT
• p. 338
9.9.4
∗MODAL FILE
• p. 338
9.9.5
∗NODE FILE
• p. 338
9.9.6
∗PREPRINT
• p. 338
The following ABAQUS element types are supported. Table 2-3
Supported ABAQUS Element Types
Element Types
Patran ABAQUS Preference Guide Page No.
Stress-Displacement Elements Beam Elements
Main Index
Two-dimensional
B21 B21H B22
B22H B23 B23H
• p. 106,
p. 108
Three-dimensional
B31 B31H B32 B32H
B33 B33H B34
• p. 113,
p. 115,
Three-dimensional Open Section
B31OS B31OSH
B32OS B32OSH
• p. 121
p. 119
Chapter 2: Building A Model 17 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued) Patran ABAQUS Preference Guide Page No.
Element Types Stress-Displacement Elements Beam Elements
Main Index
• p. 123
One-dimensional
C1D2 C1D2H
C1D3 C1D3H
Axisymmetric
CAX3 CAX3H CAX4 CAX4H CAX4I CAX4IH
CAX4R CAX4RH CAX6 CAX6H
Axisymmetric with twist
CGAX3 CGAX3H CGAX4 CGAX4H CGAX4R CGAX4RH
CGAX6 CGAX6H CGAX8 CGAX8H CGAX8R CGAX8RH
Plane Strain
CPE3 CPE3H CPE4 CPE4H CPE4I CPE4IH
CPE4R CPE4RH CPE6 CPE6H CPE6M CPE6MH
Generalized Plane Strain
CGPE5 CGPE5H CGPE6 CGPE6H CGPE6I CGPE6IH CGPE6R
CGPE6RH CGPE8 CGPE8H CGPE10 CGPE10H CGPE10R CGPE10RH
• p. 249
Plane Stress
CPS3
CPS6
• p. 251
CPS4
CPS6M
CPS4I
CPS8
CPS4R
CPS8R
CAX8 CAX8H
• p. 252
CAX8R CAX8RH • p. 253
CPE8 CPE8H
• p. 248
CPE8R CPE8RH
18 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued) Patran ABAQUS Preference Guide Page No.
Element Types Stress-Displacement Elements Beam Elements Three-dimensional
C3D4
C3D10
C3D27
C3D4H
C3D10HC3 D10M
C3D27H
C3D6
• p. 287
C3D27R C3D10MH C3D27RH
C3D6H C3D15 C3D8 C3D15H C3D8H C3D20 C3D8I C3D20H C3D8IH C3D20R C3D8R C3D20RH C3D8RH Membrane Elements Membrane Elements
Main Index
M3D3
M3D8
M3D4
M3D8R
M3D4R
M3D9
M3D6
M3D9R
• p. 254
Chapter 2: Building A Model 19 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Stress-Displacement Elements Shell Elements Shell
S3RF
S4RF
• p. 244,
p. 246
S4R
STRI3
• p. 235,
p. 237,
p. 241
S4R5
S9R5
• p. 232,
p. 234,
p. 238
• p. 40,
p. 41,
p. 235,
S8R
p. 237, • p. 40,
S8R5
p. 241 p. 41,
p. 232,
p. 234,
p. 238
STRI35
• p. 232,
p. 234,
p. 238
STRI65
• p. 232,
p. 234,
p. 235,
p. 237,
p. 238,
p. 241
• p. 134,
p. 135
Special Elements Axisymmetric
SAX1
SAX2
Elbow Elements Elbow Elements
ELBOW31
ELBOW31C
• p. 117
ELBOW31B ELBOW32 Spring Elements Spring Elements
SPRING1
• p. 98,
p. 99
SPRING2
• p. 125,
p. 127
SPRINGA
• p. 124,
p. 126
Dashpot Elements Dashpot Elements
DASHPOT1
• p. 100
DASHPOT2
• p. 101,
p. 129,
DASHPOTA
• p. 128,
p. 130
Mass Element Mass Element
MASS
• p. 96
Rotary Inertia Element Rotary Inertia Element
Main Index
ROTARY1
• p. 97
p. 131
20 Patran Interface to ABAQUS Preference Guide Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Special Elements Gap Elements Gap Elements
GAPCYL
• p. 132
GAPSPHER
• p. 133
GAPUNI
• p. 132
Small Sliding Contact Elements Interface
• p. 136
INTER1
Axisymmetric
INTER2
INTER3
• p. 255
INTER4 INTER8
INTER9
• p. 289
INTER2A
INTER3A
• p. 257
Rigid Surface Contact Elements Rigid Surface
IRS3 IRS4
Axisymmetric
IRS9
• p. 259
IRS12
• p. 102
IRS13
• p. 104
IRS21
IRS22
• p. 148
IRS31
IRS32
• p. 152
IRS21A
IRS22A
• p. 150
Slide Line Contact Elements Two-dimensional
ISL21
ISL22
• p. 138,
p. 147
Three-dimensional
ISL31
ISL32
• p. 142,
p. 147
Axisymmetric
ISL21A
ISL22A
• p. 140,
p. 147
ISL31A
ISL32A
• p. 145,
p. 147
Heat Transfer Elements Heat Transfer Elements
Main Index
• p. 297
Axisymmetric
DCAX3 DCAX4
DCAX6 DCAX8
Axisymmetric Convection/Diffusion
DCCAX2
DCCAX2D
DCCAX4
DCCAX4D
• p. 297
One-dimensional
DC1D2
DC1D3
• p. 291
Chapter 2: Building A Model 21 Introduction to Building a Model
Table 2-3
Supported ABAQUS Element Types (continued)
Element Types
Patran ABAQUS Preference Guide Page No.
Heat Transfer Elements Heat Transfer Elements
Main Index
DC2D6 DC2D8
• p. 297
Two-dimensional
DC2D3 DC2D4
Two-dimensional Convection/Diffusion
DCC2D4 DCC2D4D
Three-dimensional
DC3D4 DC3D6 DC3D8
DC3D10 DC3D15 DC3D20
• p. 299
Three-dimensional Convection/Diffusion
DCC3D8
DCC3D8D
• p. 299
Interface Elements
DINTER1
• p. 297
• p. 294
DINTER2
DINTER3
• p. 298
DINTER4
DINTER8
• p. 300
Interface Elements, Axisymmetric
DINTER2A DINTER3A
• p. 298
Shell Elements
DS4 DS8
• p. 295,
p. 296
Shell Elements, Axisymmetric
DSAX1 DSAX2
• p. 292,
p. 293
22 Patran Interface to ABAQUS Preference Guide Coordinate Frames
Coordinate Frames Coordinate frames will generate different ABAQUS input, depending on the use of the coordinate frame. Unreferenced coordinate frames will not be translated into ABAQUS.
If a node references a coordinate frame in the Analysis Coordinate Frame field, the nodal degrees-offreedom will be rotated into that system through the use of the *TRANSFORM option. All vector type loads or boundary conditions must reference the same coordinate frame as the node. If a coordinate frame is referenced for element property orientation, the appropriate *ORIENTATION option will be created.
Main Index
Chapter 2: Building A Model 23 Finite Elements
Finite Elements Finite Elements in Patran allows the definition of basic finite element constructs, including the creation of nodes, element topology, and multi-point constraints.
Nodes The nodes form will generate the ∗klab option (see Section 7.3.6 in the ABAQUS / Standard User’s Manual). The name of the node set to which the nodes will be assigned will be based on the associated analysis coordinate frame number. For example, creating nodes in analysis coordinate frame “Coord 1" will generate the ABAQUS option ∗NSET, NSET=CID1.
Main Index
24 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 25 Finite Elements
Elements Finite elements in Patran simply assigns element topology, such as Quad⁄4, for standard finite elements. The type of element to be created is not determined until the element properties are assigned. See Element Properties Form for details concerning the ABAQUS element types. Elements can be created either discretely using the Element object, or indirectly using the Mesh object.
Main Index
26 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 27 Finite Elements
Multi-Point Constraints Multi-point constraints (MPCs) can also be created from the Finite Elements menu. These are special element types which define a rigorous behavior between several specified nodes. The forms for creating MPCs are found by selecting MPC as the Object on the Finite Elements form. The full functionality of the MPC forms are defined in Create Action (FEM Entities) (Ch. 3) in the Reference Manual - Part III .
Main Index
28 Patran Interface to ABAQUS Preference Guide Finite Elements
MPC Types To create an MPC, you must first select the type of MPC you want to create from an option menu. The types that will appear in this option menu are dependent on the current Analysis Type preference setting. The following table describes the MPC types that are supported.
MPC Type Explicit
Analysis Type Structural Thermal
Creates an ∗EQUATION option which defines an explicit MPC between a dependent degree-of-freedom and one or more independent degrees-of-freedom. The dependent term consists of a node ID and a degree-of-freedom, while an independent term consists of a coefficient, a node ID, and a degree-of-freedom. An unlimited number of independent terms and one dependent term can be specified.
Rigid (Fixed)
Structural
Creates a BEAM type MPC between one independent node and one or more dependent nodes in which all six structural degrees-of-freedom are rigidly attached to each other. An unlimited number of dependent terms and one independent term can be specified. Each term consists of a single node.
Rigid (Pinned)
Structural
Creates a LINK type MPC between one independent node and one or more dependent nodes in which only the three translational structural degrees-of-freedom are rigidly attached to each other. An unlimited number of dependent terms and one independent term can be specified. Each term consists of a single node.
Linear Surf-Surf
Structural
Creates a LINEAR type MPC between a dependent node on one linear 2D element and two independent nodes on another linear 2D element to model a continuum. One dependent and two independent terms can be specified. Each term consists of a single node.
Thermal
Linear Surf-Vol
Structural
Creates an SS LINEAR type MPC between a dependent node on a linear 2D plate element and two independent nodes on a linear 3D solid element to connect the plate element to the solid element. One dependent and two independent terms can be specified. Each term consists of a single node.
Linear Vol-Vol
Structural
Creates a BILINEAR type MPC between a dependent node on one linear 3D solid element and four independent nodes on another linear 3D solid element to model a continuum. One dependent and four independent terms can be specified. Each term consists of a single node.
Thermal
Main Index
Description
Chapter 2: Building A Model 29 Finite Elements
MPC Type
Main Index
Analysis Type
Description
Quad. Surf-Surf
Structural
Creates a QUADRATIC type MPC between a dependent node on one quadratic 2D element and three independent nodes on another quadratic 2D element to model a continuum. One dependent and three independent terms can be specified. Each term consists of a single node.
Quad. Surf-Vol
Structural
Creates an SS BILINEAR type MPC between a dependent node on a quadratic 2D plate element and three independent nodes on a quadratic 3D solid element to connect the plate element to the solid element. One dependent and three independent terms can be specified. Each term consists of a single node.
Quad. Vol-Vol
Structural
Creates a C BIQUAD type MPC between a dependent node on one quadratic 3D solid and eight independent nodes on another quadratic 3D solid element to model a continuum. One dependent and eight independent terms can be specified. Each term consists of a single node.
Slider
Structural
Creates a SLIDER type MPC between one dependent node and two independent nodes which forces the dependent node to move along the vector defined by the two independent nodes. One dependent and two independent terms can be specified. Each term consists of a single node.
Elbow
Structural
Creates an ELBOW type MPC which constrains two nodes of ELBOW31 or ELBOW32 elements together. One dependent and one independent terms can be specified. Each term consists of a single node.
Tie
Structural
Creates a TIE type MPC which makes all active degrees-offreedom equal at two nodes. One dependent and one independent terms can be specified. Each term consists of a single node.
Revolute
Structural
Creates a REVOLUTE type MPC which defines a revolute joint. One dependent and two independent terms can be specified. Each term consists of a single node.
V Local
Structural
Creates a V LOCAL type MPC which constrains the velocity components at the first node to be equal to the velocity components at the third node along local, rotating, directions. These local directions rotate according to the rotation at the second node. One dependent and two independent terms can be specified. Each term consists of a single node.
30 Patran Interface to ABAQUS Preference Guide Finite Elements
MPC Type
Analysis Type
Description
Universal
Structural
Creates a UNIVERSAL type MPC which defines a universal joint. One dependent and three independent terms can be specified. Each term consists of a single node.
SS Linear
Structural
Creates an SS LINEAR type MPC which constrains a shell node to a line of solid nodes for linear elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
SS Bilinear
Structural
Creates an SS BILINEAR type MPC which constrains a shell node to a line of solid nodes for quadratic elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
SSF Bilinear
Structural
Creates an SSF BILINEAR type MPC which constrains a mid-side shell node to a line of mid-face solid nodes for quadratic elements. One dependent and an unlimited number of independent terms can be specified. Each term consists of a single node.
Degrees-of-Freedom Whenever a list of degrees-of-freedom is expected for an MPC term, a listbox containing the valid degrees-of-freedom is displayed on the form. A degree-of-freedom is valid if: 1. It is valid for the current Analysis Type Preference. 2. It is valid for the selected MPC type. In most cases, all degrees-of-freedom which are valid for the current Analysis Type preference are valid for the MPC type. The following degrees-of-freedom are supported by the Patran ABAQUS MPCs for the various analysis types:
Degrees-of-Freedom
Main Index
Analysis Type
UX
Structural
UY
Structural
UZ
Structural
RX
Structural
RY
Structural
RZ
Structural
Temperature
Thermal
Chapter 2: Building A Model 31 Finite Elements
Note:
Care must be taken to make sure that a degree-of-freedom selected for an MPC actually exists at the nodes. For example, a node that is attached only to solid structural elements will not have any rotational degrees-of-freedom. However, Patran will allow you to select rotational degreesof-freedom at this node when defining an MPC.
Explicit MPCs
Creates an *EQUATION option. (See Section 7.8.3 in the ABAQUS/Standard User’s Manual). No constant term is allowed for this type of equation. The A1 multiplier for the dependent term will be set to -1.0 to create the desired equation.
Main Index
32 Patran Interface to ABAQUS Preference Guide Finite Elements
Rigid (Fixed) MPCs
Creates an *MPC option of type BEAM for each dependent node (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes.
Main Index
Chapter 2: Building A Model 33 Finite Elements
Rigid (Pinned) MPCs
Creates an *MPC of type LINK for each dependent node (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This provides a pinned rigid link between two nodes in order to keep the distance between the two nodes constant. The displacements of the first node are modified to enforce this constraint. The rotations at the nodes, if any, are not involved in this constraint.
Main Index
34 Patran Interface to ABAQUS Preference Guide Finite Elements
Linear Surf-Surf MPCs
Creates an *MPC option of type LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is the standard method for mesh refinement of first-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated linearly from the corresponding degrees-of-freedom at the independent nodes .
Note:
Main Index
Linear Surf-Surf and Linear Surf-Vol MPCs both generate the ABAQUS ∗MPC type LINEAR.
Chapter 2: Building A Model 35 Finite Elements
Linear Surf-Vol MPCs
Creates an *MPC option of type SS LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is the standard method for mesh refinement of first-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated linearly from the corresponding degrees-offreedom at the independent nodes.
Note:
Main Index
Linear Surf-Surf and Linear Surf-Vol MPCs both generate the ABAQUS ∗MPC type SS LINEAR.
36 Patran Interface to ABAQUS Preference Guide Finite Elements
Linear Vol-Vol MPCs
Creates an *MPC option of type BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of first-order solid elements in three dimensions. This MPC constrains each degree-of-freedom at the dependent node to be interpolated bilinearly from the corresponding degrees-of-freedom at the independent nodes.
Main Index
Chapter 2: Building A Model 37 Finite Elements
Quad. Surf-Surf MPCs
Creates an *MPC option of type QUADRATIC (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated quadratically from the corresponding degrees-of-freedom at the independent nodes.
Note:
Main Index
Quad Surf-Surf and Quad Surf-Vol MPCs both generate the ABAQUS *MPC type QUADRATIC
38 Patran Interface to ABAQUS Preference Guide Finite Elements
Quad. Surf-Vol MPCs
Creates an *MPC option of type SS BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order elements. This MPC constrains each degree-of-freedom at the dependent node to be interpolated quadratically from the corresponding degrees-of-freedom at the independent nodes.
Note:
Main Index
Quad Surf-Surf and Quad Surf-Vol MPCs both generate the ABAQUS ∗MPC type SS BILINEAR.
Chapter 2: Building A Model 39 Finite Elements
Quad. Vol-Vol MPCs
Creates an *MPC option of type C BIQUAD (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This is a standard method for mesh refinement of second-order solid elements in three dimensions. This MPC constrains each degree-of-freedom at the dependent node to be interpolated by a constrained biquadratic from the corresponding degrees-of-freedom at the eight independent nodes.
Main Index
40 Patran Interface to ABAQUS Preference Guide Finite Elements
Slider MPCs
Creates an *MPC option of type SLIDER (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC will keep a node on a straight line defined by two other nodes, but allows the possibility of moving along the line, and the line to change length.
Main Index
Chapter 2: Building A Model 41 Finite Elements
Main Index
42 Patran Interface to ABAQUS Preference Guide Finite Elements
Elbow MPCs
Creates an *MPC option of type ELBOW (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC constrains two ELBOW31 or ELBOW32 elements together, where the cross-sectional direction changes.
Main Index
Chapter 2: Building A Model 43 Finite Elements
Pin MPCs
Creates an *MPC option of type PIN (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC provides a pinned joint between two nodes. This makes the displacements equal, but leaves the rotations, if they exist, independent of each other.
Tie MPCs
Creates an *MPC option of type TIE (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC makes all active degrees-of-freedom equal at two nodes. If there are different degrees-of-freedom active at the two nodes, only those in common will be constrained. It is usually used to join two parts of a mesh when corresponding nodes on the two parts are to be fully connected.
Main Index
44 Patran Interface to ABAQUS Preference Guide Finite Elements
Revolute MPCs
Creates an *MPC option of type REVOLUTE (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
Main Index
Chapter 2: Building A Model 45 Finite Elements
Main Index
46 Patran Interface to ABAQUS Preference Guide Finite Elements
V Local MPCs
Creates an *MPC option of type V LOCAL (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
Main Index
Chapter 2: Building A Model 47 Finite Elements
Universal MPCs
Creates an *MPC option of type UNIVERSAL (see Section 7.8.4 in the ABAQUS/Standard User’s Manual).
SS Linear MPCs
Creates an *MPC option of type SS LINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a shell node to a solid node line for linear elements (S4R or S4R5; C3D8, C3D8R; SAX1; CAX4; etc.) or for midside lines on quadratic elements (S8R, S8R5; C3D20, C3D20R; etc.). This MPC is only valid for small rotations.
Main Index
48 Patran Interface to ABAQUS Preference Guide Finite Elements
SS Bilinear MPCs
Creates an *MPC option of type SS BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC is only valid for small rotations.
Main Index
Chapter 2: Building A Model 49 Finite Elements
SSF Bilinear MPCs
Creates an *MPC option of type SSF BILINEAR (see Section 7.8.4 in the ABAQUS/Standard User’s Manual). This MPC is used to constrain a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC is only valid for small rotations.
Main Index
50 Patran Interface to ABAQUS Preference Guide Finite Elements
Main Index
Chapter 2: Building A Model 51 Material Library
Patran Interface to ABAQUS Preference Guide
Material Library Selecting Materials from this Patran window displays the main form for the creation of materials. The following sections provide an introduction to the Materials form, followed by the details of all the material property definitions supported by the Patran ABAQUS Application Interface.
Main Index
52 Patran Interface to ABAQUS Preference Guide Materials Form
Materials Form The Materials form shown below provides the following options for the purpose of creating ABAQUS materials.
Change Material Status The approach to defining material properties in Patran is similar to that in ABAQUS; the complete material model is defined by individually defining the necessary constitutive models. For example, to define a material for a plasticity analysis, one would first define the elastic properties and select Apply. Then the plastic properties are defined by selecting Plastic as Option 1, the yield criteria as Option 2, the hardening law as Option 3, entering the appropriate data and pushing Apply.
Main Index
Chapter 2: Building A Model 53 Materials Form
Not all constitutive model options are valid for a particular material in a particular ABAQUS analysis. For example, it is not permissible to have both elastic and hyperelastic properties defined for the same ABAQUS material. Patran, however, allows these different constitutive models to be defined and then “deactivated” for a given ABAQUS analysis. This is done on the form displayed when the Change Material Status button is selected on the main Materials form. For example, if a user defines both Elastic and Hyperelastic properties for a given material, one of these constitutive options must be deactivated on the Change Material Status form before initiating the ABAQUS analysis. Temperature Dependence ABAQUS allows most material properties to be functions of temperature. The ABAQUS interface in Patran generally supports this as well. The first step in defining a temperature dependent material property is to define a temperature dependent material field in the Fields application. This field can then be selected from a listbox on the Materials, Input Options form. When the databox for a material property that may be temperature dependent is selected, the fields listbox appears. The following table shows the allowable selections for all options when the Action is set to Create and the Analysis Type in the Analysis Preference form is set to Structural. The various options have different names, depending on previous selections.
Object Isotropic
Option 1
Option 2
• Elastic
Material Failure Theory
Hyperelastic
Incompressible
Option 3 Test Data • Ogden • Polynomial
Coefficients • Ogden • Mooney Rivlin • Neo Hookean • Polynomial
Slightly Compressible
Test Data • Ogden • Polynomial Coefficients • Ogden • Polynomial
Main Index
54 Patran Interface to ABAQUS Preference Guide Materials Form
Object
Option 1
Option 2 Compressible
Option 3 Test Data • Ogden
Coefficients • Ogden
Viscoelastic
Frequency
• Formula • Tabular
Time
• Prony • Creep Test Data • Combined Creep Test Data • Relaxation Test Data • Combined Relax Test Data
• Deformation
Plasticity Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
Cap Hardening
• Time • Strain • Hyperbolic
2D Orthotropic (Lamina)
• Elastic
Material Failure Theory
Viscoelastic
Frequency
• Formula
Tabular Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Main Index
Chapter 2: Building A Model 55 Materials Form
Object
Option 1 Plastic
Option 2 Mises/Hill
Option 3 • Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
Cap Hardening
• Time • Strain • Hyperbolic
3D Orthotropic
• Elastic
Engineering Constants
Material Failure Theory
• [D] Matrix
Viscoelastic
Frequency
• Formula Tabular
Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
• Time • Strain • Hyperbolic
Main Index
Cap Hardening
56 Patran Interface to ABAQUS Preference Guide Materials Form
Object 3D Anisotropic
Option 1
Option 2
Option 3
• Elastic
[D] Matrix
Material Failure Theory
Viscoelastic
Frequency
• Formula Tabular
Time
• Prony • Creep Test Data Combined Creep Test Data • Relaxation Test Data Combined Relax Test Data
Plastic
Mises/Hill
• Perfect Plasticity • Isotropic • Kinematic
• Drucker-Prager
Compression Tension Shear
Modified D-Prager/Cap Creep
• Time • Strain • Hyperbolic
Composite
• Laminate
Rule of Mixtures HAL Cont. Fiber HAL Disc. Fiber HAL Cont. Ribbon HAL Disc. Ribbon HAL Particulate Short Fiber 1D Short Fiber 2D
Main Index
Cap Hardening
Chapter 2: Building A Model 57 Materials Form
The following table shows the allowable selections for all options when the Action is set to Create and the Analysis Type is set to Thermal in the Analysis Preference form. The various options have different names, depending on previous selections.
Object
Option 1
Isotropic
Thermal
3D Orthotropic
Thermal
3D Anisotropic
Composite
Laminate
Rule of Mixtures HAL Cont. Fiber HAL Disc. Fiber HAL Cont. Ribbon HAL Disc. Ribbon HAL Particulate Short Fiber 1D Short Fiber 2D
Main Index
58 Patran Interface to ABAQUS Preference Guide Materials Form
Isotropic Elastic
Main Index
Object
Option 1
Option 2
Isotropic
Elastic
Material Failure Theory
Chapter 2: Building A Model 59 Materials Form
More data input is available for defining the Elastic properties for the Isotropic materials. Listed below are the descriptions for the remaining material properties.
Main Index
Property Name
Description
Reference Temperature
This is the reference value of temperature for the coefficient of thermal expansion. The thermal strain in the material is based on the difference between the current temperature and this reference value (default is 0.0).
Thermal Expansion Coeff
Coefficient of thermal expansion for the isotropic material.
Fraction Critical Damping
Set this parameter equal to the fraction of critical damping to be used with this material in calculating composite damping factors for the modes (for use in modal dynamics). The default is 0.0. The value is ignored in direct integration dynamics.
Mass Propornl Damping
Factor for mass proportional damping in direct integration dynamics (default = 0.0). This value is ignored in modal dynamics.
Stiffness Propornl Damping
Factor for stiffness proportional damping in direct integration dynamics (default = 0.0). This value is ignored in modal dynamics.
60 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Test Data Ogden Polynomial
Chapter 2: Building A Model 61 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Coefficients - Ogden
62 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Incompressible
Coefficients Moony Rivlin Neo Hookean Polynomial
Chapter 2: Building A Model 63 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Test Data Ogden Polynomial
64 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Coefficients - Ogden
Chapter 2: Building A Model 65 Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Slightly Compressible
Coefficients - Polynomial
66 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Object Isotropic
Main Index
Option 1 Hyperelastic
Option 2 Compressible
Option 3 Test Data - Ogden
Chapter 2: Building A Model 67 Materials Form
More data input is available for defining the Hyperelastic properties. Listed below are the descriptions for the remaining material properties.
Main Index
Property Name
Description
Volumetric Pressure
Material field defining volume ratio (current volume/original volume) as a function of pressure. This field appears on the *VOLUMETRIC TEST DATA sub option.
Poisson’s Ratio
Effective Poisson’s ratio of the material which will be equal to all ν i . This is the value of the POISSON parameter on the *HYPERFOAM option. If no value is given, the lateral strains should be entered.
Density
Defines the material mass density. This quantity appears on the *DENSITY option.
Thermal Expansion Coeff
Coefficient of thermal expansion for the isotropic material. This parameter appears as a on the *EXPANSION option.
68 Patran Interface to ABAQUS Preference Guide Materials Form
Hyperelastic
Main Index
Object
Option 1
Option 2
Option 3
Isotropic
Hyperelastic
Compressible
Coefficients - Ogden
Chapter 2: Building A Model 69 Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Frequency
Tabular
3D Orthotropic or 3D Anisotropic
Main Index
Formula
70 Patran Interface to ABAQUS Preference Guide Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Prony
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 71 Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Creep Test Data
3D Orthotropic or 3D Anisotropic
Main Index
Combined Creep Test Data
72 Patran Interface to ABAQUS Preference Guide Materials Form
Viscoelastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Viscoelastic
Time
Relaxation Test Data
3D Orthotropic or 3D Anisotropic
Main Index
Combined Relax Test Data
Chapter 2: Building A Model 73 Materials Form
Deformation Plasticity
Main Index
Object
Option 1
Isotropic
Deformation Plasticity
74 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Mises/Hill
Perfect Plasticity
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 75 Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2DOrthotropic,
Plastic
Mises/Hill
Isotropic
3DOrthotropic or 3D Anisotropic
Main Index
76 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Mises/Hill
Kinematic
3DOrthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 77 Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Drucker-Prager
Compression
3D Orthotropic or 3D Anisotropic
Tension Shear
Main Index
78 Patran Interface to ABAQUS Preference Guide Materials Form
Plastic
Object
Option 1
Option 2
Option 3
Isotropic, 2D Orthotropic,
Plastic
Modified D-Prager/Cap
Cap Hardening
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 79 Materials Form
CrÉep Object
Option 1
Option 2
Isotropic, 2D Orthotropic,
Creep
Time
3D Orthotropic or 3D Anisotropic
Main Index
Strain
80 Patran Interface to ABAQUS Preference Guide Materials Form
Creep
Object
Option 1
Option 2
Isotropic, 2D Orthotropic,
Creep
Hyperbolic
3D Orthotropic or 3D Anisotropic
Main Index
Chapter 2: Building A Model 81 Materials Form
2D Orthotropic (Lamina) Elastic
Main Index
Option 1
Option 2
Elastic
Material Failure Theory
82 Patran Interface to ABAQUS Preference Guide Materials Form
3D Orthotropic Elastic
Option 1 Elastic
Main Index
Option 2 Engineering Constants
Option 3 Material Failure Theory
Chapter 2: Building A Model 83 Materials Form
Elastic
Object 3D Orthotropic
Main Index
Option 1 Elastic
Option 2 [D] Matrix
Option 3 Material Failure Theory
84 Patran Interface to ABAQUS Preference Guide Materials Form
3D Anisotropic Elastic
Option 1 Elastic
Main Index
Option 2 [D] Matrix
Chapter 2: Building A Model 85 Materials Form
More data input is available for defining the Elastic properties for the 3D Anisotropic materials. Listed below are the descriptions for the remaining material properties.
Property Name
Desciption
D1212 (C34)
Coefficients in the 6 x 6 stress-strain matrix for the 3D anisotropic material.
D1212 (C44) D1113 (C15) D2213 (C25) D3313 (C35) D1213 (C45) D1313 (C55) D1123 (C16) D2223 (C26) D3323 (C36) D1223 (C46) D1323 (C56) D2323 (C66) Density
Main Index
Defines the material mass density.
86 Patran Interface to ABAQUS Preference Guide Materials Form
Isotropic (Thermal)
Main Index
Chapter 2: Building A Model 87 Materials Form
3D Orthotropic (Thermal)
Main Index
88 Patran Interface to ABAQUS Preference Guide Materials Form
3D Anisotropic (Thermal)
Composite The Composite forms allow existing materials to be combined to create new materials. All of the composite materials, with the exception of the laminated composites, can be assigned to elements like any homogeneous material through the element property forms. For the laminated composites, the section thickness is entered indirectly through the definition of the stack, and the Homogeneous option on the Element Properties Form for shells, plates and beam must be changed to Laminate to avoid reentry of this information.
Main Index
Chapter 2: Building A Model 89 Materials Form
For details on how to use these forms, refer to the Composite Materials Construction (p. 116) in the Patran Reference Manual. Laminate
Main Index
90 Patran Interface to ABAQUS Preference Guide Element Properties
Patran I nterface to ABAQU S Preference Gu ide
Element Properties By choosing the Element Properties item, located on the application switch for Patran, an element properties form will appear. When creating element properties, several option menus are available. The selections made in these option menus will determine which element property form is presented, and ultimately, which ABAQUS element will be created. The following pages give an introduction to the Element Properties form, followed by the details of all the element property definitions supported by the Patran ABAQUS Application Preference.
Element Properties Form When Element Properties is selected on the main menu, this is the form which will be displayed. Four option menus on this form are used to determine which ABAQUS element types are to be created, and which property forms are to be displayed. The individual property forms are documented later in this section. For more details, see the Element Properties Forms (p. 67) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 91 Element Properties
Main Index
92 Patran Interface to ABAQUS Preference Guide Element Properties
The following table shows the allowable selections for all option menus when Analysis Type is set to Structural.
Dimension 0D
Type
Option 2
MASS
• Rotary Inertia
ROTARYI
Grounded Damper
IRS (single node)
Beam in XY Plane
• Linear
SPRING1
• Nonlinear
SPRING2
• Linear
DASHPOT1
• Nonlinear
DASHPOT2
• Planar
Elastic Slip Soft Contact IRS12 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Spatial
Elastic Slip Soft Contact IRS13 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• General Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Box Section
Standard Formulation
B21, B22 B21H, B22H B23 B23H
Hybrid Cubic Interpolation Cubic Hybrid • Circular Beam (Solid)
Main Index
Name
• Mass Grounded Spring
1D
Option 1
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
Chapter 2: Building A Model 93 Element Properties
Dimension
Type
Beam in Space
Main Index
Option 1
Option 2
Name
• Hexagonal Beam
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• I Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Pipe Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Rectangular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• Trapezoid Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid
B21, B22 B21H, B22H B23 B23H
• General Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Arbitrary Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Box Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Circular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Curved w/Pipe Section
Standard Formulation Ovalization Only Ovalization Only with Approximated Fourier
ELBOW31, ELBOW32 ELBOW31B ELBOW31C
• Hexagonal Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
94 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension
Type
Option 2
Name
• I Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• L Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Open Section
Standard Formulation Hybrid
B31OS, B32OS B31OSH, B32OSH
• Pipe Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Rectangular Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Trapezoidal Section
Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
B31, B32 B31H, B32H B33 B33H B34
• Truss
Standard Formulation Hybrid
Spring
Linear
• Standard Formulation SPRINGA SPRING2 Fixed Direction
Nonlinear
• Standard Formulation Fixed Direction
Linear
• Standard Formulation DASHPOTA DASHPOT2 Fixed Direction
Nonlinear
• Standard Formulation Fixed Direction
Damper
Main Index
Option 1
CID2, CID3 CID2H, CID3H
Chapter 2: Building A Model 95 Element Properties
Dimension 1D
Type Gap
Option 1
True Distance GAPCYL Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Spherical
True Distance Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Uniaxial
True Distance GAPUNI Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Homogeneous • Laminate
Main Index
Name
• Cylindrical
(continued)
Axisym Shell
Option 2
GAPSPHER
SAX1, SAX2
96 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 1D
Type
Option 1
Option 2
• 1D Interface
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
ISL (in plane)
• Planar
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Axisymmetric
Elastic Slip Soft Contact ISL21A, Elastic Slip Hard Contact ISL22A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
• Parallel
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation
(continued)
ISL (in space)
INTER1
Lagrange Vis Damping Lagrange Vis Damping No Separation
Main Index
Name
ISL21, ISL22
ISL31, ISL32 ISL31, ISL32
Chapter 2: Building A Model 97 Element Properties
Dimension 1D
Type ISL (in space) (continued)
Option 1 • Radial
(continued)
• Slide Line
• Axisymmetric
Main Index
Name
Elastic Slip Soft Contact ISL31A, Elastic Slip Hard Contact ISL32A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation --
IRS (planar/axisym) • Planar
• IRS (beam/pipe)
Option 2
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Elastic Slip Soft Contact IRS21, IRS22 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation Elastic Slip Soft Contact IRS21A, Elastic Slip Hard Contact IRS22A Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation1D (cont.) IRS31, IRS32
98 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 1D (continued)
Type
Option 1
• Rigid Surf (Seg)
Option 2
Name ---
• Rigid Surf (Cyl)
--
• Rigid Surf (Axi)
--
• Rigid Surf (Bz2D)
R2D2, RAX2
• Rigid Line (Lbc) • Rebar
Axisymmetric
SFMAX1, SFMAX2
General Axisymmetric
SFMGAX1, SFMGAX2
• Mech Joint (2D Model) ALIGN AXIAL BEAM CARTESIAN JOIN JOINTC LINK ROTATION SLOT TRANSLATOR WELD • Mech Joint (3D Model) ALIGN AXIAL BEAM CARDAN CARTESIAN CONSTANT VELOCITY CVJOINT CYLINDRICAL EULER FLEXION-TORSION
Main Index
Chapter 2: Building A Model 99 Element Properties
Dimension
Type
Option 1
Option 2
Name
HINGE JOIN JOINTC LINK PLANAR RADIAL-THRUST REVOLUTE ROTATION SLIDE-PLANE SLOT TRANSLATOR UJOINT UNIVERSAL WELD • 1D Gasket
Axisymmetric Link
3D Link
2D Link
Main Index
Gasket Behavior Model
GKAX2
Thickness Behavior Only
GKAX2N
Built-in Material
GKAX2
Gasket Behavior Model
GK3D2
Thickness Behavior Only
GK3D2N
Built-in Material
GK3D2
Gasket Behavior Model
GK2D2
Thickness Behavior Only
GK2D2N
Built-in Material
GK2D2
100 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 2D
Type Shell
Option 1 Thin
Option 2 • Homogeneous Laminate
Thick
Homogeneous
Name STRI35, S4R5, STRI65, S8R5, S9R5 S3R, S4R, STRI65, S8R
Laminate • General Thin
Homogeneous Laminate
• General Thick
Homogeneous
STRI35, S4R5, STRI65, S8R5, S9R5 S3R, S4R, STRI65, S8R
Laminate • Large Strain • General Large Strain 2D Solid
• Plane Strain
• Plane Stress
Main Index
S3R, S4R, S8R Standard Formulation
CPE3, CPE4, CPE6, CPE8
Hybrid
CPE3H, CPE4H, CPE6H, CPE8H
Hybrid / Reduced Integration
CPE4RH, CPE8RH
Reduced Integration Incompatible Modes Hybrid/Incompatible Modes Modified Modified/Hybrid
CPE4R, CPE8R CPE4I CPE4IH CPE6M, CPE6MH
Standard Formulation Reduced Integration Incompatible Modes Modified Modified/Hybrid
CPS3, CPS4, CPS6, CPS8 CPS4R, CPS8R CPS4I CPS6M, CPS6MH
Chapter 2: Building A Model 101 Element Properties
Dimension 2D
Type 2D Solid (continued)
Option 1 • Axisymmetric
(continued)
• Axisymmetric with Twist
• Membrane
2D Interface
Main Index
Option 2
Name
Standard Formulation
CAX3, CAX4, CAX6, CAX8
Hybrid
CAX3H, CAX4H, CAX6H, CAX8H
Hybrid/Reduced Integration
CAX4RH, CAX8RH
Reduced Integration
CAX4R, CAX8R
Incompatible Modes
CAX4I
Hybrid/Incompatible Modes
CAX4IH
Modified
CAX6M
Modified/Hybrid
CAX6MH
Standard Formulation
CGAX3, CGAX4, CGAX6, CGAX8
Hybrid
CGAX3H, CGAX4H, CGAX6H, CGAX8H
Hybrid/Reduced Integration
CGAX4RH, CGAX8RH
Reduced Integration
CGAX4R, CGAX8R
Standard Formulation
M3D3, M3D4, M3D6, M3D8, M3D9
Reduced Integration
M3D4R, M3D8R, M3D9R
• Planar
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
INTER2, INTER3
102 Patran Interface to ABAQUS Preference Guide Element Properties
Dimension 2D
Type
Option 1
2D Solid (continued)
• Axisymmetric
IRS (shell/solid)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
(continued)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Name INTER2A, INTER3A
IRS3, IRS4, IRS9
• Rigid Surf (Bz3D)
--
• Rigid Surface(Lbc)
R3D3, R3D4
• 2D Rebar
Cylindrical General
• 2D Gasket
Plane Strain Plane Stress
Axisymmetric
Main Index
Option 2
SFMCL9 Standard Formulation
SFM3D3, SFM3D4, SFM3D6, SFM3D8
Reduced Integration
SFM3D4R, SFM3D8R
Gasket Behavior Model
GKPE4
Built-in Material
GKPE4
Gasket Behavior Model
GKPS4
Thickness Behavior Only
GKPS4N
Built-in Material
GKPS4
Gasket Behavior Model
GKAX4
Thickness Behavior Only
GKAX4N
Built-in Material
GKAX4
Chapter 2: Building A Model 103 Element Properties
Dimension
Type
Option 1 Line
3D
• Solid
Standard Formulation Laminate Hybrid
Option 2
Name
Gasket Behavior Mode
GK3D4L
Thickness Behavior Only
GK3D4LN
Built-in Material
GK3D4L C3D4, C3D6, C3D8, C3D10, C3D15, C3D20
Laminate
C3D4H, C3D6H, C3D8H, C3D10H, C3D15H, C3D20H
Hybrid/Red Integration Laminate
C3D8RH, C3D20RH
Reduced Integration Laminate
C3D8R, C3D20R
Incompatible Modes Laminate
C3D8I
Hybrid/Incomp Modes
C3D8IH
Laminate
Main Index
Modified
C3D10M
Modified/Hybrid
C3D1OH
• 3D Interface
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
INTER4, INTER8, INTER9
• Gasket
Gasket Behavior Model
GK3D8, GK3D6
Thickness Behavior Only
GK3D8N, GK3D6N
Built-in Material
GK3D8, GK3D6
104 Patran Interface to ABAQUS Preference Guide Element Properties
The following table shows the allowable selections for all option menus when Analysis Type is set to Thermal.
Dimension 1D
Type
Option 1
Option 2
• Link
Axisymmetric Shell
DCID2, DCID3 • Homogeneous
DSAX1, DSAX2
• Laminate
• 1D Interface
2D
Shell
Name
DINTER1 • Homogeneous
DS4, DS8
• Laminate
2D Solid
• Planar
Standard Formulation
DC2D2, DC2D4, DC2D6, DC2D8 DCC2D4
Convection/Diffusion DCC2D4D Convection/Diffusion with Dispersion/Control • Axisymmetric
• 2D Interface
Main Index
Standard Formulation
DCAX3, DCAX4, DCAS6, DCAX8
Convection/Diffusion
DCCAX4
Convection/Diffusion with Dispersion/Control
DCCAX4D
Planar
DINTER2, DINTER3
Axisymmetric
DINTER2A, DINTER3A
Chapter 2: Building A Model 105 Element Properties
Dimension 3D
Type • Solid
• 3D Interface
Main Index
Option 1
Option 2
Name
Standard Formulation
DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20
Convection/Diffusion
DCC3D8
Convection/Diffusion with Dispersion Control
DCC3D8D
DINTER4, DINTER8
106 Patran Interface to ABAQUS Preference Guide Element Properties
Point Mass Analysis Type Structural
Dimension 0D
Type Mass
Option 1
Option 2
Topologies Point/1
Options above create MASS elements with ∗MASS properties.This creates a concentrated mass at a point. The mass is associated with the translational degrees-of-freedom at a node.
Main Index
Chapter 2: Building A Model 107 Element Properties
Rotary Inertia Analysis Type Structural
Dimension 0D
Type Rotary Inertia
Option 1
Option 2
Topologies Point/1
Options above createROTARI elements with ∗ROT ARY INERTIA properties. This element allows the rotary inertia of a rigid body to be included at a node. An ∗ORIENTATION option may also be created, as required.
Main Index
108 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Spring (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Spring
Option 1 Linear
Option 2
Topologies Point/1
Options above create SPRING1 elements with ∗SPRING properties. This element defines a linear spring between a node and ground. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 109 Element Properties
Nonlinear Spring (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Spring
Option 1
Option 2
Nonlinear
Topologies Point/1
Options above create SPRING1 elements with ∗SPRING properties. This element defines a nonlinear spring between a node and ground. An ∗ORIENTATION option may also be created, as required.
Linear Damper (Grounded) Analysis Type Structural
Main Index
Dimension 0D
Type Grounded Damper
Option 1 Linear
Option 2
Topologies Point/1
110 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create DASHPOT1 elements with ∗DASHPOT properties. This element defines a linear damper between a node and ground. An ∗ORIENTATION option may also be created, as required.
Nonlinear Damper (Grounded) Analysis Type Structural
Dimension 0D
Type Grounded Damper
Option 1 Nonlinear
Option 2
Topologies Point/1
Options above create DASHPOT1 elements with ∗DASHPOT properties. This element defines a nonlinear dashpot between a node and ground. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 111 Element Properties
Main Index
112 Patran Interface to ABAQUS Preference Guide Element Properties
IRS (Single Node, Planar) Analysis Type
Dimension
Structural
0D
Type IRS (single node)
Option 1 Planar
Option 2 Elastic Slip Soft Contact
Topologies Point/1
Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS12 elements with ∗INTERFACE and ∗FRICTION properties. This element defines an interface between a node on a planar model and a rigid surface.
Main Index
Chapter 2: Building A Model 113 Element Properties
More=data input is available for creating IRS (single node, planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option definition.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
114 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure
Main Index
No Sliding Contact
Chooses the Lagrange multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 115 Element Properties
IRS (Single Node, Spatial) Analysis Type Dimension Structural
0D
Type IRS (single node)
Option 1 Spatial
Option 2 Elastic Slip Soft Contact
Topologies Point/1
Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS13 elements with ∗INTERFACE and ∗FRICTION properties. This element defines an interface between a node on a spatial model and a rigid surface.
Main Index
116 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (single node, spatial) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Chapter 2: Building A Model 117 Element Properties
Property Name
Description
Stiffness in Stick
This is currently not used.
Maximum Friction
Defines the equivalent shear stress limit of the gap element. This is the equivalent shear stress limit value on the second card of the *FRICTION option.
Stress
Clearance Zero-Pressure Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant. Pressure Zero Clearance Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant. Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
General Beam in Plane Analysis Type
Dimension
Structural
1D
Type
Option 1
Beam in XY General Plane Section
Option 2
Topologies
Standard Formulation Bar/2, Bar/3 Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements, depending on the specified options and topology. ∗BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. This defines a general section beam which is restricted to remain in the XY plane.
Main Index
118 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating General Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam.
Chapter 2: Building A Model 119 Element Properties
Box Beam in Plane/Space Analysis Type Structural
Dimension 1D
Type
Option 1
Beam in Box Section XY Plane
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements in a plane, or B31, B32, B33, B34, B31H, B32H or B33H elements in space, depending on the specified options and topology. ∗BEAM SECTION, SECTION=BOX properties are also created. The planar box section beam is restricted to remain in the XY-plane. For the spatial beam, ∗TRANSVERSE SHEAR STIFFNESS is also created, as required.
Main Index
120 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 121 Element Properties
More data input is available for creating Box Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name Thickness_RHS Thickness_TOP Thickness_LHS
Description Defines the wall thickness of the element cross section. These are for the right-hand side, top, left-hand side, and bottom, respectively. These are four of the data values on the second card of the *BEAM SECTION option. These can be either real constants or references to existing field definitions. These properties are required.
Thickness_BOT Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam.
Definition of XY Plane (for beams in space only)
Defines the orientation of the XY-plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the *BEAM SECTION option. All of the Patran tools are available via the select menu to define this vector.
Beam Shape Display in Plane/Space All of the beam shapes can be displayed in their proper orientation on the 3D model. To activate the display, go to Display/Load/BC/Elem. Props... and set the "Beam Display" option. These options are discribed in detail in Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual. The beam display is shown on beam elements only, not geometry.
Main Index
122 Patran Interface to ABAQUS Preference Guide Element Properties
Additional Beam Shapes in Plane/Space Additional commonly used beam cross-sectional shapes are defined by forms analogous to that for box beams. The planar option defines a beam which is restricted to remain in the XY plane. For the spatial beam, *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS is also created, as required. CIRCULAR BEAM (SOLID) This property will have the SECTION=CIRC parameter. All that is required for the definition of the cross section is the radius. The integration schemes for planar analysis (left) and spatial analysis(right) are shown below.
HEXAGONAL BEAM This property will have the SECTION=HEX parameter. All that is required for the definition of the cross section is the circumscribing radius and the wall thickness. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
Main Index
Chapter 2: Building A Model 123 Element Properties
I-SECTION This property will have the SECTION=I parameter. The height of section, flange widths, and associated thicknesses are required. In addition, the height of the centroid, depicted as “l” is also required. This allows placement of the origin of the local cross-section axis anywhere on the symmetry line. Note also that judicious specification of the flange widths and thicknesses will allow modelling of a T-section. See p. 3.5.2-11 of the ABAQUS User’s Manual for details. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
PIPE BEAM This property will have the SECTION=PIPE parameter. The pipe thickness and outside radius define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
Main Index
124 Patran Interface to ABAQUS Preference Guide Element Properties
RECTANGULAR BEAM (SOLID) This property will have the SECTION=RECT parameter. The section width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
TRAPEZOID BEAM (SOLID) This property will have the SECTION=TRAP parameter. The top and bottom width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
General Beam in Space Analysis Type Structural
Main Index
Dimension 1D
Type Beam in Space
Option 1 General Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Cubic Initially Straight
Bar/2
Chapter 2: Building A Model 125 Element Properties
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. *BEAM GENERAL SECTION properties are also created. This property will have the SECTION=GENERAL parameter. *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS options are also created, as required. This defines a general section beam.
More data input is available for creating General Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
126 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Definition of XY Plane
Defines the orientation of the XY plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the ∗BEAM GENERAL SECTION option. All of the Patran tools are available via the select menu to define this vector.
Centroid Coord 1
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Centroid Coord 2
Shear Centroid Coord 1 Shear Centroid Coord 2
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Section Point Coord 1
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the *SECTION POINTS suboption of the *BEAM GENERAL SECTION option.
Section Point Coord 2
Main Index
Defines the location of the shear centroid of the cross section with respect to the nodal locations. These values are measured in the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the *SHEAR CENTER suboption on the *BEAM GENERAL SECTION option.
Chapter 2: Building A Model 127 Element Properties
Arbitrary Beam in Space Analysis Type Dimension Structural
1D
Type Beam in Space
Option 1 Arbitrary Section
Option 2 Standard Formulation
Topologies Bar/2, Bar/3 Bar/2, Bar/3
Hybrid Bar/2 Cubic Interpolation Bar/2 Cubic Hybrid Bar/2 Cubic Initially Straight Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=ARBITRARY properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an arbitrary section beam.
Main Index
128 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Arbitrary Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu
Main Index
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a righthand rule. This is the data on the second card of the ∗BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Chapter 2: Building A Model 129 Element Properties
Main Index
Property Name
Description
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
130 Patran Interface to ABAQUS Preference Guide Element Properties
Curved Pipe in Space Analysis Type
Dimension
Structural
1D
Type Beam in Space
Option 1 Curved w/Pipe Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Ovalization Only
Bar/2
Ovaliz Only w/ Approx Fourier
Bar/2
Options above create ELBOW31, ELBOW32, ELBOW31B, or C elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=ELBOW properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an elbow element.
Main Index
Chapter 2: Building A Model 131 Element Properties
More data input is available for creating Curved Pipe in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Torus Radius
Defines the radius of the elbow bend. This is one of the data values on the second card of the *BEAM SECTION option. This is either a real constant or a reference to an existing field definition. This property is required.
Integ Points around Pi
Defines the number of integration points to be used around the pipe cross section. This is the second value on the fourth card of the *BEAM SECTION option. This is an integer value. This property is required.
132 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Point Tangents Inters
Defines the orientation of the XY plane of the element coordinate system. This is the data on the second card of the *BEAM SECTION option. This is a Node ID. This property is required.
Integ Points thru Thick
Defines the number of integration points to be used through the pipe wall thickness. This is the first value on the fourth card of the *BEAM SECTION option. This is an integer value.
# Ovalization Modes
Defines the number of ovalization modes to be included in the shape functions of this element. This is the third value of the fourth card of the *BEAM SECTION option. This is an integer value.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
L-Section Beam in Space Analysis Type Dimension Structural
1D
Type Beam in Space
Option 1 L-Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Cubic Interpolation
Bar/2
Cubic Hybrid
Bar/2
Cubic Initially Straight
Bar/2
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. ∗BEAM SECTION, SECTION=L properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an L-section beam.
Main Index
Chapter 2: Building A Model 133 Element Properties
More data input is available for creating L-Section Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
134 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Shear Factor
The product of this factor, the beam cross sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Open Beam in Space Analysis Type Structural
Dimension 1D
Type Beam in Space
Option 1 Open Section
Option 2
Topologies
Standard Formulation
Bar/2, Bar/3
Hybrid
Bar/2, Bar/3
Options above create B31OS, B32OS, B31OSH, or B32OSH elements depending on the specified options and topology. ∗BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. ∗ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an open section beam.
Main Index
Chapter 2: Building A Model 135 Element Properties
More data input is available for creating Open Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
136 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Definition of XY Plane Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM GENERAL SECTION option. This is a real vector. This property is required. 1st. Sectorial Moment
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Warping Constant
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Centroid Coord 1
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Centroid Coord 2
Shear Center Coord 1 Defines the location of the shear centroid of the cross section with respect to the local cross section coordinate system. These values are either real Shear Center Coord 2 constants or references to existing field definitions. These are the values on the ∗SHEAR CENTER suboption of the ∗BEAM GENERAL SECTION option. Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Section Point Coord 1
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the ∗SECTION POINTS suboption of the ∗BEAM GENERAL SECTION option.
Section Point Coord 2
Truss Analysis Type Structural
Dimension 1D
Type Truss
Option 1 Standard Formulation
Option 2
Topologies Bar/2. Bar/3 Bar/2. Bar/3
Hybrid
Main Index
Chapter 2: Building A Model 137 Element Properties
Options above create T3D2, T3D2H, T3D3, or T3D3H elements depending on the specified options and topology. *SOLID SECTION properties are also created. The cross sectional area is included on the *SOLID SECTION option.
Linear Spring (Axial) Analysis Type Dimension Structural
1D
Type Spring
Option 1 Linear
Option 2 Standard Formulation
Topologies Bar/2
Options above create SPRINGA elements with *SPRING properties. This element defines a linear spring between two nodes whose line of action is the line joining the two nodes.
Main Index
138 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Spring (Fixed Direction) Analysis Type
Dimension
Structural
1D
Type Spring
Option 1 Linear
Option 2
Topologies
Fixed Direction Bar/2
Options above create SPRING2 elements with *SPRING properties.This element defines a linear spring between specified degrees-of-freedoms at two nodes. An *ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 139 Element Properties
Nonlinear Spring (Axial) Analysis Type Structural
Dimension 1D
Type Spring
Option 1 Nonlinear
Option 2 Standard Formulation
Topologies Bar/2
Options above create SPRINGA elements with *SPRING properties.This element defines a nonlinear spring between two nodes whose line of action is the line joining the two nodes.
Main Index
140 Patran Interface to ABAQUS Preference Guide Element Properties
Nonlinear Spring (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Spring
Option 1 Nonlinear
Option 2
Topologies
Fixed Direction Bar/2
Options above create SPRING2 elements with ∗SPRING properties. This element type defines a nonlinear spring between two nodes, acting in a fixed direction. An ∗ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 141 Element Properties
Linear Damper (Axial) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Linear
Option 2 Standard Formulation
Topologies Bar/2
Options above create DASHPOTA elements with ∗DASHPOT properties. This element type defines a linear damper between two nodes whose line of action is the line joining the two nodes.
Main Index
142 Patran Interface to ABAQUS Preference Guide Element Properties
Linear Damper (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Linear
Option 2 Fixed Direction
Topologies Bar/2
Options above create DASHPOT2 elements with ∗DASHPOT properties. This element type defines a linear damper between two nodes, acting in a fixed direction. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 143 Element Properties
Nonlinear Damper (Axial) Analysis Type
Dimension
Structural
1D
Type Damper
Option 1 Nonlinear
Option 2 Standard Formulation
Topologies Bar/2
Options above create DASHPOTA elements with ∗DASHPOT properties. This element type defines a nonlinear damper between two nodes whose line of action is the line joining the two nodes.
Main Index
144 Patran Interface to ABAQUS Preference Guide Element Properties
Nonlinear Damper (Fixed Direction) Analysis Type Structural
Dimension 1D
Type Damper
Option 1 Nonlinear
Option 2
Topologies
Fixed Direction Bar/2
Options above create DASHPOT2 elements with ∗a^pemlq properties. This element type defines a nonlinear damper between two specified nodes, acting in a fixed direction. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 145 Element Properties
Gap (Uniaxial), Gap (Cylindrical) Analysis Type Structural
Dimension 1D
Type Gap
Option 1
Cylindrical True Distance Uniaxial
Main Index
Option 2
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2
146 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create GAPUNI or GAPCYL elements with *GAP properties. The ∗FRICTION option is created, as required.
Main Index
Chapter 2: Building A Model 147 Element Properties
Gap (Spherical) Analysis Type Dimension Structural
1D
Type Gap
Option 1 Spherical
Option 2 True Distance Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2
Options above create GAPSPHER elements with *GAP properties. The *FRICTION option is created, as required.
Main Index
148 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Shell Analysis Type Structural
Dimension 1D
Type Axisymmetric Shell
Option 1 Homogeneous
Option 2
Topologies Bar/2 Bar/3
Options above create SAX1 or SAX2 elements, depending on the specified topology, with *SHELL SECTION properties.
Main Index
Chapter 2: Building A Model 149 Element Properties
Axisymmetric Shell (Laminate) Analysis Type Dimension Structural
1D
Type Axisymmetric Shell
Option 1 Laminate
Option 2
Topologies Bar/2
Options above create SAX1 or SAX2 elements, depending on the specified topology, with ∗SHELL SECTION, COMPOSITE properties.
Main Index
150 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 151 Element Properties
1D Interface Analysis Type Dimension Structural
1D
Type 1D Interface
Option 1 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2 Topologies Bar/2
Options above create INTER1 elements with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
Main Index
152 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating 1D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Chapter 2: Building A Model 153 Element Properties
Property Name
Description
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Planar ISL (In Plane)
Main Index
Analysis Type
Dimensio n
Structural
1D
Type ISL (in plane)
Option 1 Planar
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
154 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create ISL21 or ISL22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on a planar model and another part of the model.
More data input is available for creating Planar ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Chapter 2: Building A Model 155 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Pressure
Main Index
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
156 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric ISL (In Plane) Analysis Type
Dimension
Structural
1D
Type ISL (in plane)
Option 1
Option 2
Axisymmetric Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Topologies Bar/2, Bar/3
Options above create ISL21A or ISL22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on an axisymmetric model and another part of the model.
Main Index
Chapter 2: Building A Model 157 Element Properties
More data input is available for creating Axisymmetric ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
158 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Parallel ISL (In Space) Analysis Type Dimension Structural
Main Index
1D
Type ISL (in space)
Option 1 Parallel
Option 2
Topologies
Bar/2, Bar/3 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Dampin Lagrange Vis Damping No Separation
Chapter 2: Building A Model 159 Element Properties
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of an element and another part of the model.
More data input is available for creating Parallel ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Vector
Main Index
Defines the normal to the plane in which sliding contact occurs. This is the second card of the *INTERFACE option. This value is a global vector. This property is required.
160 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping Clearance at which the damping coefficient is zero. Damping Zero Clearance Damping coefficient at zero clearance. Frac Clearance Const Damping
Main Index
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 161 Element Properties
Radial ISL (In Space) Analysis Type Structural
Dimension 1D
Type
Option 1
ISL (in space) Radial
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element and another part of the model.
Main Index
162 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Radial ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Vector
Defines the normal to the plane in which sliding contact occurs. This is the second card of the ∗INTERFACE option. This value is a global vector. This property is required.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Chapter 2: Building A Model 163 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Slide Line
Analysis Type
Dimensio n
Structural
1D
Type Slide Line
Option 1
Option 2
Topologies Bar/2, Bar/3
Options above create Slide Lines for the ISL elements. These elements must be equivalenced and continuous.
Main Index
164 Patran Interface to ABAQUS Preference Guide Element Properties
IRS (Planar) Analysis Type Structural
Main Index
Dimension 1D
Type IRS (plane/axisym)
Option 1 Planar
Option 2
Topologies
Bar/2, Bar/3 Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Chapter 2: Building A Model 165 Element Properties
Options above create IRS21 or IRS22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on a planar model and a rigid surface.
More data input is available for creating IRS (planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
166 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 167 Element Properties
IRS (Axisymmetric) Analysis Type Structural
Dimensio n 1D
Type
Option 1
IRS Axisymmetric (plane/axisym)
Option 2
Topologies
Elastic Slip Soft Contact Bar/2, Bar/3 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create IRS21A or IRS22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on an axisymmetric model and a rigid surface.
Main Index
168 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (axisymmetric) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Chapter 2: Building A Model 169 Element Properties
Property Name
Description
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Beam/Pipe)
Main Index
Analysis Type
Dimension
Structural
1D
Type
Option 1
IRS (beam/pipe)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologies Bar/2, Bar/3
170 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create IRS31 or IRS32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between a beam or pipe element on a spatial model and a rigid surface.
More data input is available for creating IRS (beam/pipe) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Elastic Slip
Main Index
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Chapter 2: Building A Model 171 Element Properties
Property Name
Description
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Defines the ROUGH parameter on the *FRICTION option. This property is only used for the Lagrange option.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Rigid Surface (Segments) Analysis Type Dimension Structural
1D
Type Rigid Surf (Seg)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE=SEGMENTS option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The start Point (Node ID) defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Main Index
172 Patran Interface to ABAQUS Preference Guide Element Properties
Rigid Surface (Cylindrical) Analysis Type Dimension Structural
1D
Type Rigid Surf (Cyl)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE = CYLINDRICAL option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is first defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The rigid surface’s +x direction is defined from the start point (node ID) along the line of the rigid surface. The +y direction is away from the object the rigid surface will be in contact with. The +z direction (the surface generation vector) is defined by using right-hand rule, crossing the rigid surface’s +x axis with the +y axis.
Main Index
Chapter 2: Building A Model 173 Element Properties
Rigid Surface (Axisymmetric) Analysis Type
Dimension
Structural
1D
Type Rigid Surf (Axi)
Option 1
Option 2
Topologies Bar/2
Options above create a ∗RIGID SURFACE, TYPE=AXISYMMETRIC option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
Main Index
174 Patran Interface to ABAQUS Preference Guide Element Properties
The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Surface (Bezier 2D)
Main Index
Analysis Type
Dimension
Structural
1D
Type Rigid Surf (Bz2D)
Option 1
Option 2
Topologies Bar/2
Chapter 2: Building A Model 175 Element Properties
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in two-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s Manual). The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Line (LBC) Analysis Type Structural
Main Index
Dimension 1D
Type Rigid Line(LBC)
Option 1
Option 2
Topologies Bar/2
176 Patran Interface to ABAQUS Preference Guide Element Properties
This property set is created when the Rigid-Deform contact LBC is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R2D2 and RAX2 elements.
Rebar Analysis Type Structural
Dimension 1D
Type Rebar
Option 1 Axisymmetric General Axisymmetric
Option 2
Topologies Bar/2, Bar/3
The options above create SFMAX1, SFMAX2, SFMGAX1 and SFMGAX2 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
Main Index
Chapter 2: Building A Model 177 Element Properties
Main Index
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
178 Patran Interface to ABAQUS Preference Guide Element Properties
Rebar Orient. Angle
Defines the angular orientation of the rebar from the meridional plane in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Mech Joint (2D Model) - ALIGN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 ALIGN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 179 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
180 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - AXIAL Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 AXIAL
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 181 Element Properties
Main Index
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock, Min Disp
This property value defines the lower bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
182 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - BEAM Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 BEAM
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 183 Element Properties
Mech Joint (2D Model) - CARTESIAN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 CARTESIAN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Y Axis
Main Index
184 Patran Interface to ABAQUS Preference Guide Element Properties
Zero Force Ref Len
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (2D Model) - JOIN Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 JOIN
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 185 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - JOINTC Analysis Type Dimension Structural
1D
Type Mech Joint (2D Model)
Option 1 JOINTC
Option 2
Topologies Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
Main Index
186 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Y Axis
Main Index
Chapter 2: Building A Model 187 Element Properties
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis
Rot Damping, Z Axis
Main Index
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
188 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - LINK Analysis Type Structural
Dimension 1D
Type Mech Joint (2D Model)
Option 1 LINK
Option 2 Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 189 Element Properties
Mech Joint (2D Model) - ROTATION Analysis Type
Dimension
Type
Option 1
Structural
1D
Mech Joint (2D Model)
ROTATION
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
190 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, Z Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Chapter 2: Building A Model 191 Element Properties
jÉÅÜ=gçáåí=EOa=jçÇÉäF=J=pilq Analysis Type
Dimension
Structural
1D
Type Mech Joint (2D Model)
Option 1 SLOT
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
Main Index
192 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Chapter 2: Building A Model 193 Element Properties
Mech Joint (2D Model) - TRANSLATOR Analysis Type
Dimension
Structural
1D
Type
Option 1
Mech Joint TRANSLATOR (2D Model)
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
194 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (2D Model) - WELD Analysis Type Structural
Dimension 1D
Type
Option 1
Mech Joint WELD (2D Model)
Option 2
Topologies Bar/2
This option creates CONN2D2 elements. The connection type is set to WELD on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 195 Element Properties
Mech Joint (3D Model) - ALIGN Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 ALIGN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
196 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - AXIAL Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 AXIAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
Main Index
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Chapter 2: Building A Model 197 Element Properties
Main Index
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock Min Disp
This property value defines the upper bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
198 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - BEAM Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 BEAM
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 199 Element Properties
Mech Joint (3D Model) - CARDAN Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 CARDAN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CARDAN on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
200 Patran Interface to ABAQUS Preference Guide Element Properties
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n onspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Mom/Rot about Y Axis Mom/Rot about Z Axis
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
jÉÅÜ=gçáåí=EPa=jçÇÉäF=J=`^oqbpf^k Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 CARTESIAN
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 201 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, YAxis Force/Disp, Z Axis
Main Index
202 Patran Interface to ABAQUS Preference Guide Element Properties
Zero Force Ref Len
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis Damping, Z Axis
Mech Joint (3D Model) - CONSTANT VELOCITY Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 CONSTANT VELOCITY
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CONSTANT VELOCITY on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 203 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - CVJOINT Analysis Type Structural
Dimension 1D
Type
Option 1
Mech Joint CVJOINT (3D Model)
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CVJOINT on the *CONNECTOR SECTION option.
Main Index
204 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 205 Element Properties
Mech Joint (3D Model) - CYLINDRICAL Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 CYLINDRICAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to CYLINDRICAL on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
206 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - EULER Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 EULER
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to EULER on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 207 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
208 Patran Interface to ABAQUS Preference Guide Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - FLEXION-TORSION Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 FLEXION-TORSION
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to FLEXION-TORSION on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 209 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
210 Patran Interface to ABAQUS Preference Guide Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - HINGE Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 HINGE
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to HINGE on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 211 Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
212 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - JOIN Analysis Type
Dimension
Type
Option 1 Option 2 Topologies
Structural
1D
Mech Joint (3D Model)
JOIN
Bar/2
This option creates CONN3D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
Node A Analysis CID
Main Index
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 213 Element Properties
Mech Joint (3D Model) - JOINTC Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 JOINTC
Option 2
Topologies Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
214 Patran Interface to ABAQUS Preference Guide Element Properties
Force/Disp, X Axis Force/Disp, Y Axis Force/Disp, Z Axis
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
Main Index
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable. This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a nonspatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Chapter 2: Building A Model 215 Element Properties
Mech Joint (3D Model) - LINK Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 LINK
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
216 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - PLANAR Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 PLANAR
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to PLANAR on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 217 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - RADIAL-THRUST Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 RADIAL-THRUST
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to RADIAL-THRUST on the *CONNECTOR SECTION option.
Main Index
218 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, ZAxis
Zero Force Ref Len
Main Index
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Chapter 2: Building A Model 219 Element Properties
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, X Axis Damping, Z Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - REVOLUTE Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 REVOLUTE
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to REVOLUTE on the *CONNECTOR SECTION option.
Main Index
220 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Chapter 2: Building A Model 221 Element Properties
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Mech Joint (3D Model) - ROTATION Analysis Type
Dimension
Structural
1D
Type Mech Joint (3D Model)
Option 1 ROTATION
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
Main Index
222 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Chapter 2: Building A Model 223 Element Properties
Mom/Rot about X Axis Mom/Rot about Y Axis Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The nonspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - SLIDE-PLANE Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 SLIDE-PLANE
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to SLIDE-PLANE on the *CONNECTOR SECTION option.
Main Index
224 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, Y Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Force/Disp, Z Axis
Zero Force Ref Len
Main Index
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Chapter 2: Building A Model 225 Element Properties
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Damping, Y Axis Damping, Z Axis
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - SLOT Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 SLOT
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
Main Index
226 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Chapter 2: Building A Model 227 Element Properties
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Mech Joint (3D Model) - TRANSLATOR Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 TRANSLATOR
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
Main Index
228 Patran Interface to ABAQUS Preference Guide Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - UJOINT Analysis Type Dimension Structural
1D
Type Mech Joint (3D Model)
Option 1 UJOINT
Option 2 Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to UJOINT on the *CONNECTOR
Main Index
Chapter 2: Building A Model 229 Element Properties
SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
230 Patran Interface to ABAQUS Preference Guide Element Properties
Mech Joint (3D Model) - UNIVERSAL Analysis Type Structural
Dimension 1D
Type Mech Joint (3D Model)
Option 1 UNIVERSAL
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to UNIVERSAL on the *CONNECTOR SECTION option.
Main Index
Chapter 2: Building A Model 231 Element Properties
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n onspatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Mom/Rot about Z Axis
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Rot Damping, Z Axis
Mech Joint (3D Model) - WELD
Analysis Type
Dimensio n
Structural
1D
Type Mech Joint (3D Model)
Option 1 WELD
Option 2
Topologies Bar/2
This option creates CONN3D2 elements. The connection type is set to WELD on the *CONNECTOR
Main Index
232 Patran Interface to ABAQUS Preference Guide Element Properties
SECTION option.
Main Index
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Chapter 2: Building A Model 233 Element Properties
Axisym Link Gasket Analysis Type Structural
Dimension 1D
Type
Option 1
Option 2
Topologies
1D Gasket Axisymmetric Gasket Bar2 Link Behavior Model
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the membrane and transverse shear behaviors.
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
234 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Chapter 2: Building A Model 235 Element Properties
Axisym Link Gasket (Thick only) Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket Axisymmetric Link
Option 2 Thickness Behavior Only
Topologies Bar2
These options create GKAX2N elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
236 Patran Interface to ABAQUS Preference Guide Element Properties
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisym Link Gasket (Material)
Main Index
Chapter 2: Building A Model 237 Element Properties
Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket Axisymmetric Link
Option 2 Built-in Material
Topologies Bar2
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
238 Patran Interface to ABAQUS Preference Guide Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket Analysis Type Structural
Dimension 1D
Type
Option 1
1D Gasket 3D Link
Option 2 Gasket Behavior Model
Topologies Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
Chapter 2: Building A Model 239 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
240 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Chapter 2: Building A Model 241 Element Properties
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket (Thick only) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 3D Link
Option 2
Topologies
Thickness Behavior Only
Bar2
These options create GK3D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
242 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 243 Element Properties
Main Index
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
244 Patran Interface to ABAQUS Preference Guide Element Properties
3D Link Gasket (Material) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 3D Link
Option 2
Topologies
Built-in Material
Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 245 Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
246 Patran Interface to ABAQUS Preference Guide Element Properties
2D Link Gasket Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Gasket Behavior Model
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
Chapter 2: Building A Model 247 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
248 Patran Interface to ABAQUS Preference Guide Element Properties
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
2D Link Gasket (Thick only) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Thickness Behavior Only
Bar2
These options create GK2D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 249 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
250 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Chapter 2: Building A Model 251 Element Properties
2D Link Gasket (Material) Analysis Type
Dimension
Type
Option 1
Structural
1D
1D Gasket 2D Link
Option 2
Topologies
Built-in Material
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
252 Patran Interface to ABAQUS Preference Guide Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Thin Shell Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thin Shell
Option 2 Homogeneous
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This element defines a standard thin shell element.
Main Index
Chapter 2: Building A Model 253 Element Properties
More data input is available for creating Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Property Name
Description
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
254 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Normal Hourglass Stiffness Bending Hourglass Stiffness
Thin Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thin Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
Main Index
Chapter 2: Building A Model 255 Element Properties
Thick Shell Analysis Type
Dimension
Structural
2D
Type Shell
Option 1
Option 2
Topologies
Thick Shell
Homogeneous
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS and *HOURGLASS STIFFNESS options may also be created, as required. This defines a homogeneous thick shell element.
Main Index
256 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name Orientation System
Main Index
Description Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Chapter 2: Building A Model 257 Element Properties
Property Name
Description Defines the transverse shear stIffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K13 Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stIffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Thick Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Thick Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
Main Index
258 Patran Interface to ABAQUS Preference Guide Element Properties
General Thin Analysis Type Structural
Dimension 2D
Type Shell
Option 1
Option 2
Topologies
General Thin Shell
Homogenous
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thin shell element.
Main Index
Chapter 2: Building A Model 259 Element Properties
More data input is available for creating General Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
260 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Define the temperature effects on the *SHELL GENERAL SECTION Temperature Scaling Thermal Expansion Scaling option. These are lists of real values. Each list must have the same Temperature Values number of values. These values are optional.
Main Index
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Chapter 2: Building A Model 261 Element Properties
General Thin Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Thin Shell
Option 2 Laminate
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI3, STRI65, S4R5, S8R5 or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
Main Index
262 Patran Interface to ABAQUS Preference Guide Element Properties
General Thick Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Thick Shell
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thick shell element.
More data input is available for creating General Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
Chapter 2: Building A Model 263 Element Properties
Property Name Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling Thermal Expansion Scaling Temperature Values
Define the temperature effects on the *SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Shear Stiffness K13
Defines the transverse shear stiffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Main Index
Description
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
264 Patran Interface to ABAQUS Preference Guide Element Properties
General Thick Shell (Laminated) Analysis Type Structural
Dimension 2D
Type Shell
Option 1
Option 2
General Thick Laminate Shell
Topologies Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
Main Index
Chapter 2: Building A Model 265 Element Properties
Large Strain Analysis Type Structural
Dimension 2D
Type Shell
Option 1 Large Strain Shell
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, S4R, or S8R elements with ∗SHELL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a large strain element.
Main Index
266 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu .
Property Name
Description
Membrane Hourglass Stiff
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Normal Hourglass Stiff Bending Hourglass Stiff
General Large Strain Analysis Type Structural
Dimension 2D
Type Shell
Option 1 General Large Strain Shell
Option 2
Topologies Tri/3, Quad/4
Options above create S3R, S4R, or S8R elements with ∗SHELL GENERAL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a general large strain element.
Main Index
Chapter 2: Building A Model 267 Element Properties
More data input is available for creating General Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Main Index
268 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Property Name
Description
Section Stiffness D14 Section Stiffness D24 Section Stiffness D34 Section Stiffness D44 Section Stiffness D15 Section Stiffness D25 Section Stiffness D35 Section Stiffness D45 Section Stiffness D55 Section Stiffness D16 Section Stiffness D26 Section Stiffness D36 Section Stiffness D46 Section Stiffness D56 Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the ∗SHELL GENERAL SECTION option. These properties are required.
Force Vector F1...F6
Defines the 6 values of the {F} vector on the ∗SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling D Thermal Expansion Scaling Temperature Values
Define the temperature effects on the ∗SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the ∗ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the ∗SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit surface area for the shell element. This is the DENSITY parameter on the ∗SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *SHELL GENERAL SECTION option.
Chapter 2: Building A Model 269 Element Properties
Property Name
Description
Shear Stiffness K13
Defines the transverse shear stiffness. These are the values on the ∗TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Shear Stiffness K23 Membrane Hourglass Stiffness Normal Hourglass Stiffness Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Plane Strain Analysis Type Structural
Dimension 2D
Type 2D Solid
Option 1 Plane Strain
Option 2
Topologies
Standard Formulation
Tri/3, Quad/4, Tri/6, Quad/8
Hybrid Hybrid/Reduced Integration Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Tri/6 Tri/6
Modified Formulation Modified/Hybrid Options above create CPE3, CPE4, CPE4R, CPE6, CPE6M, CPE8, CPE8R, CPE3H, CPE4H, CPE4RH, CPE6H, CPE6MH, CPE8H, or CPE8RH (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular element are found where reduced integration is requested, standard integration elements will be used
Main Index
270 Patran Interface to ABAQUS Preference Guide Element Properties
.
Generalized Plane Strain Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Solid General Plane Strain
Option 2
Topologies
Standard Formulation
Tri/3, Quad/4
Hybrid
Tri/6, Quad/8
Hybrid/Reduced Integration Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Main Index
Chapter 2: Building A Model 271 Element Properties
These options create CGPE5, CGPE5H, CGPE6, CGPE6H, CGPE6I, CGPE6IH, CGPE6R, CGPE6RH, CGPE8, CGPE8H, CGPE10, CGPE10H, CGPE10R or CGPE10RH elements with *SOLID SECTION properties when writing an ABAQUS V5.X or V4.X input file. Otherwise, they create CPEG3, CPEG3H, CPEG4, CPEG4H, CPEG4I, CPEG4IH, CPEG4R, CPEG4RH, CPEG6, CPEG6H, CPEG8, CPEG8H, CPEG8R or CPEG8RH elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
272 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
[Reference Node] V6.X+
Defines the REF NODE parameter on the *SOLID SECTION option. The third degree of freedom of this node defines the change in length between the bounding planes. The fourth and fifth degrees of freedom of this node define the relative rotations of one bounding plane with respect to the other. This property is required when generating an ABAQUS version 6 or greater input file.
[Node A: DOF
This property is required when generating an ABAQUS version 4 or 5 input file.
[Node B: DOF
This property is required when generating an ABAQUS version 4 or 5 input file.
Plane Stress Analysis Type Dimension Structural
2D
Type 2D Solid
Option 1 Plane Stress
Option 2 Standard Formulation
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Reduced Integration Incompatible Modes Tri/6 Modified Formulation Options above create CPS3, CPS4, CPS4R, CPS6, CPS6M, CPS8, or CPS8R (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option will be included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
Chapter 2: Building A Model 273 Element Properties
Axisymmetric Solid Analysis Type Structural
Dimension 2D
Type
Option 1
2D Solid
Axisymmetric
Option 2
Topologies
Standard Formulation Tri/3, Quad/4, Tri/6, Quad/8 Reduced Integration Incompatible Modes Hybrid Tri/6 Modified Formulation Modified/Hybrid
Main Index
Tri/6
274 Patran Interface to ABAQUS Preference Guide Element Properties
Options above create CAX3, CAX4, CAX4R, CAX6, CAX6M, CAX8, CAX8R, CAX3H, CAX4H, CAX4RH, CAX6H, CAX6MH, CAX8H, or CAX8RH elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. *ORIENTATION and ∗HOURGLASS STIFFNESS option may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Axisymmetric Solid with Twist (General) Analysis Type Structural
Dimension 2D
Type 2D Solid
Option 1
Option 2
General Standard Formulation Axisymmetric Hybrid
Topologies Tri/3, Quad/4, Tri/6, Quad/8 Quad/4, Quad/8
Reduced Integration Hybrid/Reduced Integration Options above create CGAX3, CGAX4, CGAX4R, CGAX6, CGAX8, CGAX8R, CGAX3H, CGAX4H, CGAX4RH, CGAX6H, CGAX8H, or CGAX8RH elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. *ORIENTATION and ∗HOURGLASS STIFFNESS
Main Index
Chapter 2: Building A Model 275 Element Properties
options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Membrane Analysis Type
Dimension
Structural
2D
Type
Option 1
Membrane Standard Formulation
Option 2
Topologies Tri/3, Quad/4, Tri/6, Quad/8
Reduced Integration Options above create M3D3, M3D4, M3D4R, M3D6, M3D8, M3D8R, M3D9 or M3D9R elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. The thickness value on the ∗plifa=pb`qflk option is included. ∗lofbkq^qflk and ∗elrodi^pp= pqfcckbpp options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
276 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Chapter 2: Building A Model 277 Element Properties
Planar 2D Interface Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Interface Planar
Option 2
Topologies
Quad/4, Elastic Slip Soft Contact Quad/8 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create INTER2 or INTER3 elements (depending on the selected topology) with ∗fkqboc^`b, ∗cof`qflk, and ∗proc^`b=`lkq^`q properties. The SOFTENED parameter on the ∗proc^`b=`lkq^`q option may be included, depending on the selected option. This element defines an interface region between two portions of a planar model. These elements must be created from one contact surface to the other.
Main Index
278 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating Planar 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Main Index
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Press
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Chapter 2: Building A Model 279 Element Properties
Axisymmetric 2D Interface Analysis Type
Dimension
Structural
2D
Type
Option 1
2D Interface Axisymmetric
Option 2
Topologies
Elastic Slip Soft Contact Quad/4, Quad/8 Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Options above create INTER2A or INTER3A elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element
Main Index
280 Patran Interface to ABAQUS Preference Guide Element Properties
defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
More data input is available for creating Axisymmetric 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Main Index
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Chapter 2: Building A Model 281 Element Properties
Property Name
Description
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Shell/Solid) Analysis Type Structural
Dimensio n 2D
Type
Option 1
IRS (shell/solid)
Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologie s Quad/4
Options above create IRS3, IRS4, and IRS9 elements (depending on the selected topology) with ∗INTERFACE, ∗FRICTION and ∗SURFACE CONTACT properties. The SOFTENED parameter on the ∗SURFACE CONTACT option may be included, depending on the selected option. This defines a rigid surface element for use with solid or shell elements.
Main Index
282 Patran Interface to ABAQUS Preference Guide Element Properties
More data input is available for creating IRS (shell/solid) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Reference Node
Reference node common to the IRS elements and the rigid surface.
Friction in Dir_1
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Friction in Dir_2
Main Index
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Chapter 2: Building A Model 283 Element Properties
Property Name
Description
Maximum Friction Stress Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option. Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Rigid Surface (Bezier 3D) Analysis Type Dimension Structural
2D
Type Rigid Surf (Bz3D)
Option 1
Option 2
Topologies Quad 4
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in three-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s manual). All trias forming up the rigid surface must have the normals pointing towards the contacting surface. Trias must all be connected.
Main Index
284 Patran Interface to ABAQUS Preference Guide Element Properties
Rigid Surface (LBC) Analysis Type
Dimension
Structural
2D
Type Rigid Surface(LBC)
Option 1
Option 2
Topologies Quad4, Tria3
This property set is created when the Rigid-Deform contact lbc is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R3D3 and R3D4 elements.
Main Index
Chapter 2: Building A Model 285 Element Properties
2D Rebar Analysis Type Structural
Dimension 2D
Type Rebar
Option 1 Cylindrical
Option 2 Standard Formulation
General Reduced Integration
Topologies Quad/9 Tri/3, Tri/6, Quad/4, Quad/8 Quad/4, Quad/8
The options above create SFM3D3, SFM3D4, SFM3D4R, SFM3D6, SFM3D8, SFM3D8R and SFMCL9 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
Main Index
286 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Chapter 2: Building A Model 287 Element Properties
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
Rebar Orient. Angle
Defines the angular orientation of the rebar from the local 1-direction in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Orientation System
Defines a local coordinate system for orienting the rebars. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create an *ORIENTATION option. The orientation name is then used for the ORIENTATION parameter on the *REBAR LAYER option. This property is not required.
Orientation Axis
Defines the axis of rotation on the “Orientation System” to use for the additional rotation specified by the “Orientation Angle”. The axis should have a nonzero component in the direction of the normal to the surface. An integer value between 1 and 3 may be specified. The local 1-direction is the default value. This property is not required.
Orientation Angle
Defines the additional rotation in degrees about the “Orientation Axis” of the “Orientation System”. Either a real scalar or a reference to an existing field definition may be specified. The default value is zero. This property is not required.
Plane Strain Gasket Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Strain
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
288 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 289 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Strain Gasket (Material) Analysis Type Structural
Main Index
Dimension 2D
Type
Option 1
2D Gasket Plane Strain
Option 2 Built-in Material
Topologies Quad4
290 Patran Interface to ABAQUS Preference Guide Element Properties
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Chapter 2: Building A Model 291 Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Stress
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
292 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 293 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Thick only) Analysis Type Structural
Main Index
Dimension 2D
Type
Option 1
Option 2
2D Gasket Plane Stress
Thickness Behavior Only
Topologies Quad4
294 Patran Interface to ABAQUS Preference Guide Element Properties
These options create GKPS4N elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 295 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Material) Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Plane Stress
Option 2 Built-in Material
Topologies Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
296 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Chapter 2: Building A Model 297 Element Properties
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisymmetric Gasket Analysis Type
Dimension
Structural
2D
Type 2D Gasket
Option 1
Option 2
Axisymmetric Gasket Behavior Model
Topologies Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
298 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 299 Element Properties
Main Index
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
300 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Gasket (Thick only) Analysis Type Structural
Dimension 2D
Type
Option 1
2D Gasket Axisymmetric
Option 2 Thickness Behavior Only
Topologies Quad4
These options create GKAX4N elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 301 Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
302 Patran Interface to ABAQUS Preference Guide Element Properties
Axisymmetric Gasket (Material)
Analysis Type Structural
Dimensio n 2D
Type
Option 1
2D Gasket Axisymmetri c
Option 2 Built-in Material
Topologies Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 303 Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gaske t
Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Gasket Behavior Model
Topologies Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
304 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 305 Element Properties
F/L vs. Closure (Unloading) This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Main Index
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
306 Patran Interface to ABAQUS Preference Guide Element Properties
3D Line Gasket (Thick only) Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Thickness Behavior Only
Topologies Quad4
These options create GK3D4LN elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
Chapter 2: Building A Model 307 Element Properties
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading) This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Main Index
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
308 Patran Interface to ABAQUS Preference Guide Element Properties
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gasket (Material) Analysis Type Structural
Dimension 2D
Type 2D Gasket
Option 1 Line
Option 2 Built-in Material
Topologies Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
Main Index
Chapter 2: Building A Model 309 Element Properties
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Main Index
310 Patran Interface to ABAQUS Preference Guide Element Properties
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Analysis Type Structural
Dimension
Type
3D
Solid
Option 1 Standard Formulation Hybrid Hybrid/Reduced Integration
Option 2
Topologies
Laminate
Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20, Hex/27
Reduced Integration Incompatible Modes Hybrid/Incompatible Modes
Tet/10 Tet/10
Modified Formulation Modified/Hybrid Options above create C3D4, C3D6, C3D8, C3D8R, C3D10, C3D10M, C3D15, C3D20, C3D20R, C3D4H, C3D6H, C3D8H, C3D8RH, C3D10H, C3D10MH, C3D15H, C3D20H, C3D20RH, C3D27, C3D27R, C3D27H, or C3D27RH elements (depending on the selected options and topologies) with ∗SOLID SECTION properties. ∗ORIENTATION and ∗HOURGLASS STIFFNESS options may also be created, as required. If tetrahedral or wedge elements are found where reduced integration is requested, standard integration elements will be used.
Main Index
Chapter 2: Building A Model 311 Element Properties
Material Name
Defines the material to be used. When entering data, a list of all materials in the database is displayed. You can either pick one from the list with the mouse or type the name in. This identifies the material which will be referenced on the *SOLID SECTION option. This property is required.
Orientation Axis This property defines the the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option. Stack Direction
Main Index
This property defines the direction in which the material layers are stacked. This is the STACK DIRECTION parameter on the *SOLID SECTION option. An integer value of 1, 2 or 3 may be entered. Please see the section on defining composite solid elements in the ABAQUS Standard User’s Manual to determine the correct stack direction. This property is not required. The default value is 3.
312 Patran Interface to ABAQUS Preference Guide Element Properties
3D Interface Analysis Type Structural
Dimension 3D
Type
Option 1
3D Interface Elastic Slip Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Hard Contact Elastic Slip No Separation Lagrange No Separation Elastic Slip Vis Damping Elastic Slip Vis Damping No Separation Lagrange Vis Damping Lagrange Vis Damping No Separation
Option 2
Topologies Hex/8, Hex/20, Hex/27
Options above create INTER4, INTER8 or INTER9 elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of a spatial model. These elements must be created from one contact surface to the other.
Main Index
Chapter 2: Building A Model 313 Element Properties
More data input is available for creating 3D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Main Index
314 Patran Interface to ABAQUS Preference Guide Element Properties
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of F f to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the p 0 value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p 0 value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping Fraction of the clearance interval over which the damping coefficient is constant. Thermal Link Analysis Type Dimension Thermal
Main Index
1D
Type Link
Option 1
Option 2
Topologies Bar/2, Bar/3
Chapter 2: Building A Model 315 Element Properties
Options above create DC1D2 or DC1D3 elements, depending on the specified topology with *SOLID SECTION properties. The cross-sectional area value on the *SOLID SECTION option is included.
Thermal Axisymmetric Shell Analysis Type
Dimension
Thermal
1D
Type Axisymmetric Shell
Option 1 Homogeneous
Option 2
Topologies Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with *SHELL SECTION properties.
Main Index
316 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Axisymmetric Shell (Laminated) Analysis Type Thermal
Dimension 1D
Type Axisymmetric Shell
Option 1 Laminate
Option 2
Topologies Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with ∗pebii= pb`qflk, COMPOSITE properties.
Main Index
Chapter 2: Building A Model 317 Element Properties
Thermal 1D Interface Analysis Type Dimension Thermal
1D
Type 1D Interface
Option 1
Option 2
Topologies Bar/2
Options above create DINTER1 elements with ∗fkqboc^`b properties. These elements must be created from one contact surface to the other. ∗GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Main Index
318 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Shell Analysis Type Dimension Thermal
2D
Type Shell
Option 1 Homogeneous
Option 2
Topologies Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION properties. An *ORIENTATION option may also be created, as required.
Main Index
Chapter 2: Building A Model 319 Element Properties
Thermal Shell (Laminated) Analysis Type
Dimension
Type
Option 1
Thermal
2D
Shell
Laminate
Option 2
Topologies Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION, COMPOSITE properties. An *ORIENTATION option may also be created, as required.
Main Index
320 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Planar Solid Analysis Type Thermal
Dimension 2D
Type 2D Solid
Option 1
Option 2
Planar
Standard Formulation
Axisymmetric
Convection/Diffusion Convection/Diffusion w/Dispersion Control
Topologies Tri/3, Quad/4, Quad/8 Quad/4 Quad/4
Options above create DC2D3, DC2D4, DC2D6, DC2D8, DCC2D4, DCC2D4D, DCAX3, DCAX4, DCAX6, DCAX8,DCCAX4, or DCCAX4D elements (depending on the selected options and topologies) with ∗plifa=pb`qflk properties. The thickness value on the ∗plifa=pb`qflk option is included. An ∗lofbkq^qflk option may also be created, as required.
Main Index
Chapter 2: Building A Model 321 Element Properties
Thermal Preference (Planar) Analysis Type Dimension Thermal
2D
Type 2D Interface
Option 1 Planar
Option 2
Topologies Quad/4, Quad/8
Axisymmetric Options above create DINTER2, DINTER3, DINTER2A, or DINTER3A elements (depending on the selected option and topology) with *INTERFACE properties. These elements must be created from one
Main Index
322 Patran Interface to ABAQUS Preference Guide Element Properties
contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are created, as required.
Main Index
Chapter 2: Building A Model 323 Element Properties
Thermal Solid Analysis Type
Dimension
Thermal
3D
Type Solid
Option 1 Standard Formulation
Topologies Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20
Convection/Diffusion Hex/8 Convection/Diffusion w/ Dispersion Control Options above create DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20, DCC3D8, or DCC3D8D (depending on the selected options and topologies) elements with *SOLID SECTION properties. An *ORIENTATION option may also be created, as required.
Main Index
324 Patran Interface to ABAQUS Preference Guide Element Properties
Thermal Preference (Solid) Analysis Type Dimension Thermal
3D
Type 3D Interface
Option 1
Option 2
Topologies Hex/8, Hex/20
Options above create DINTER4 or DINTER8 elements (depending on the selected) with *INTERFACE properties. These elements must be created from one contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Main Index
Chapter 2: Building A Model 325 Element Properties
Solid Gasket Analysis Type Structural
Dimension 3D
Type
Option 1
Gasket
Gasket Behavior Model
Option 2
Topologies Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
326 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The nonspatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Chapter 2: Building A Model 327 Element Properties
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Thick only) Analysis Type Structural
Dimension 3D
Type Gasket
Option 1 Thickness Behavior Only
Option 2
Topologies Wedge6, Hex8
These options create GK3D8N or GK3D6N elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
Main Index
328 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
Chapter 2: Building A Model 329 Element Properties
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Material) Analysis Type Structural
Dimension 3D
Type Gasket
Option 1 Built-in Material
Option 2
Topologies Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
Main Index
330 Patran Interface to ABAQUS Preference Guide Element Properties
Main Index
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Chapter 2: Building A Model 331 Element Properties
Main Index
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
332 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Patran I nterface to ABAQU S Preference Gu ide
Loads and Boundary Conditions When choosing the Loads/BCs toggle, the Loads and Boundary Conditions form will appear. The selections made will determine which loads and boundary form is presented, and ultimately, which ABAQUS loads and boundaries will be created. The following pages give an introduction to the Loads and Boundary Conditions form, followed by the details of all the loads and boundary conditions supported by the Patran ABAQUS Application Preference.
Loads & Boundary Conditions Form The Loads & Boundary Conditions form shown below provides the following options for the purpose of creating ABAQUS loads and boundaries. The full functionality of the form is defined in Loads and Boundary Conditions Form (p. 27) in the Patran Reference Manual.
Main Index
Chapter 2: Building A Model 333 Loads and Boundary Conditions
The following table shows the allowable selections for all options when the Analysis Type is set to Structural.
Main Index
334 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Analysis Type Structural
Object
Type
• Displacement
Nodal
• Force
Nodal
• Pressure
Element Uniform
• Temperature
Nodal Element Uniform Element Variable
• Inertial Load
Element Uniform
• Initial Velocity
Nodal
• Velocity
Nodal
• Acceleration
Nodal
• Contact (Deform-Deform)
Element Uniform
• Contact (Rigid-Deform)
Element Uniform
• Pre-Tension
Element Uniform
The following table shows the allowable selections for all options when the Analysis Code is set to Thermal.
Analysis Type Thermal
Object
Type
• Temperature (Thermal)
Nodal
• Convection
Element Uniform
• Heat Flux
Element Uniform
• Heat Source
Nodal Element Uniform
• Initial Temperature
Nodal
Input Data Clicking on the Input Data button generates either a Static or Transient Input Data form, depending on the current Load Case Type. Static
This subordinate form appears whenever Load Case Type is set to Static and the Input Data button is clicked. The information contained on this form will vary according to the Object that has been selected. Information that remains standard to this form is defined below.
Main Index
Chapter 2: Building A Model 335 Loads and Boundary Conditions
Transient
This subordinate form appears whenever Load Case Type is set to Transient and the Input Data button is clicked. The information contained on this form will vary according to the Object that has been selected. Information that remains standard to this form is defined below.
Main Index
336 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Object Tables On the static and transient input data forms are areas where the load data values are defined. The data fields presented depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. These Object Tables list and define the various input data that pertains strictly to a specific selected object:
Main Index
Chapter 2: Building A Model 337 Loads and Boundary Conditions
Displacement
Object
Type
Type
Displacement
Nodal
Structural
Creates *BOUNDARY TYPE=DISPLACEMENT options.
Input Data
Description
Translations (T1,T2,T3)
Defines the enforced translational displacement values. These are in model length units.
Rotations (R1,R2,R3)
Defines the enforced rotational displacement values. These are in radians.
Force
Object
Type
Type
Force
Nodal
Structural
Creates *CLOAD options.
Input Data
Description
Force (F1,F2,F3)
Defines the applied forces in the translation degrees-of-freedom.
Moment (M1,M2,M3)
Defines the applied moments in the rotational degrees-of-freedom.
Pressure
Object
Type
Type
Pressure
Element Uniform Structural
Dimension 2D
Creates *DLOAD options.
Input Data Top Surf Pressure
Main Index
Description Defines the magnitude of the pressure in the direction of the negative normal to the shell.
338 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Input Data
Description
Bot Surf Pressure
Defines the magnitude of the pressure in the direction of the positive normal to the shell.
Edge Pressure
Defines the edge pressure value on axisymmetric, plane strain,and plane stress elements.
Object
Type
Type
Pressure
Element Uniform Structural
Dimension 3D
Creates *DLOAD options.
Input Data
Description
Pressure
Defines the face pressure value on solid elements.
Temperature
Object
Type
Type
Temperature
Nodal
Structural
Creates *TEMPERATURE options.
Input Data
Description
Temperature
Defines the nodal temperature value.
Object
Type
Type
Dimension
Temperature
Element Uniform
Structural
1D 2D 3D
Creates *TEMPERATURE options.
Input Data Temperature
Main Index
Description Defines the temperature on elements.
Chapter 2: Building A Model 339 Loads and Boundary Conditions
Object
Type
Type
Dimension
Temperature
Element Variable
Structural
1D 2D 3D
Creates *TEMPERATURE options.
Input Data
Description
Centroid Temp (1D)
Defines the temperature at the centroid of the beam.
Axis-1 Gradient (1D)
Defines the temperature gradient along the axis-1 of the beam section.
Axis-2 Gradient (1D)S
Defines the temperature gradient along the axis-2 of the beam section.
Top Surf Temp (2D)
Defines the temperature at the top of the shell element.
Bot Surf Temp (2D)
Defines the temperature at the bottom of the shell element.
Temperature (3D)
Defines the temperature in the solid element.
Inertial Load
Object
Type
Type
Inertial Load
Element Uniform
Structural
Creates *DLOAD options with the load type set to GRAV, CENT, or CORIO as appropriate.
Input Data
Description
Trans Accel (A1,A2,A3)
Defines the magnitude and direction of the gravity vector. This must be assigned to all elements which are to have gravity loads.
Rot Velocity (w1,w2,w3)
Defines the centrifugal and Coriolis forces to be applied to the elements.
Rot Accel (a1,a2,a3)
These load terms are not currently supported by Patran ABAQUS.
Initial Velocity
Main Index
Object
Type
Type
Initial Velocity
Nodal
Structural
340 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *INITIAL CONDITIONS TYPE=VELOCITY options.
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the initial velocity values for the translational degrees-offreedom.
Rot Veloc (w1,w2,w3)
Defines the initial velocity values for the rotational degrees-offreedom.
Velocity
Object
Type
Type
Velocity
Nodal
Structural
Creates *Boundary, Type=Velocity options.
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the velocity values for the translational degrees-of-freedom.
Rot Veloc (w1, w2, w3)
Defines the velocity values for the rotational degrees-of-freedom.
Acceleration
Object
Type
Type
Acceleration
Nodal
Structural
Creates *Boundary, Type=Acceleration options.
Input Data
Main Index
Description
Trans Accel (A1, A2, A3)
Defines the acceleration values for the translational degrees-of-freedom.
Rot Accel (a1, a2, a3)
Defines the acceleration values for the rotational degrees-of-freedom.
Chapter 2: Building A Model 341 Loads and Boundary Conditions
Contact (Deform-Deform)
Object
Type
Type
Contact
Element Uniform
Structural
Defines the contact between two deformable structural bodies and creates the following ABAQUS input cards: *Surface Definition: Master and Slave surface definitions. *Contact Pair: Pairing of the Master and Slave Surfaces. *Tie: Tying of the Master and Slave Surfaces (version 6 and greater). *Surface Interaction: Contact Interaction properties between Master and Slave. *Contact Controls: Set the Automatic Tolerances parameter *Contact Inerference: Set the Shrink parameter
Main Index
342 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Defines the Master and Slave surface interaction properties.
The contact type can be General (contacting surfaces move relative to each other) or Tied (contacting surfaces remain fixed with respect to each other usually used in mesh refinement). The sliding between the contacting surfaces can be Large or Small. For contact in 3D space the sliding is limited to Small sliding. Four types of contact surface behavior options are available, Hard, Softened, Modified Softened, and No Separation. The surfaces do not separate after contact in the case when No Separation option is used. Three types of friction formulations are available, Penalty, Lagrange, and No Slip. In the case of No Slip option there is no relative motion between the contacting surfaces after contact. The Penetration Type can be One Sided (Only the slave nodes are checked against the master surface) or Symmetric (Both the slave and master nodes are checked against each other by swapping the master and slave surfaces). The Contact Control can be turned On to activate the *Contact Control, Automatic Tolerances parameter. Use this parameter to have ABAQUS automatically compute an overclosure tolerance and a separation pressure tolerance to prevent chattering in contact. Shrink Fit can be turned On to activate the *Contact Interference, Shrink parameter. Use this parameter to invoke the automatic shrink fit capability. This capability can be used only in the first step of an analysis. When this parameter is invoked, no data are required other than the contact pairs to which the option is applied. The application region form is used to pick the master and slave surfaces.
Main Index
Chapter 2: Building A Model 343 Loads and Boundary Conditions
Application Region: Defines the Master and Slave contacting surfaces.
Contact (Rigid-Deform)
Object
Type
Type
Contact
Element Uniform
Structural
Defines the contact between the rigid surface and deformable structural body and creates the following ABAQUS input cards: *Surface Definition: Master and Slave surface definitions. *Contact Pair: Pairing of the Master and Slave Surfaces.
Main Index
344 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
*Surface Interaction: Contact Interaction properties between Master and Slave. *Contact Controls: Set the Automatic Tolerances parameter *Contact Inerference: Set the Shrink parameter Defines the Master and Slave surface interaction properties.
The sliding between the contacting surfaces can be Large or Small. Four types of contact surface behavior options are available, Hard, Softened, Modified Softened, and No Separation. The surfaces do not separate after contact in the case when No Separation option is used. Three types of friction formulations are available, Penalty, Lagrange, and No Slip. In the case of No Slip option there is no relative motion between the contacting surfaces after contact. The Contact Control can be turned On to activate the *Contact Control, Automatic Tolerances parameter. Use this parameter to have ABAQUS automatically compute an overclosure tolerance and a separation pressure tolerance to prevent chattering
Main Index
Chapter 2: Building A Model 345 Loads and Boundary Conditions
in contact. Shrink Fit can be turned On to activate the *Contact Interference, Shrink parameter. Use this parameter to invoke the automatic shrink fit capability. This capability can be used only in the first step of an analysis. When this parameter is invoked, no data are required other than the contact pairs to which the option is applied. A vector pointing from the rigid line to the slave surface must be defined. This vector is used to calculate the order of rigid bar elements. The vector should be defined such that the most of the vector markers point away from the rigid line. The application region form is used to pick the master and slave surfaces. Application Region: Defines the Master and Slave contacting surfaces.
Main Index
346 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Application Region: Defines the Master and Slave contacting surfaces. This form appears when Contact Type: is Rigid Geom. and Master: is Rigid Surface.
Main Index
Chapter 2: Building A Model 347 Loads and Boundary Conditions
Pre-tension
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Displacement
Structural
1D
Creates *BOUNDARY and *PRE-TENSION SECTION options.
Input Data
Description
Relative Displacement Defines the relative displacement to apply to the length of the elements.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Displacement
Structural
2D, 3D
Creates *BOUNDARY, *SURFACE and *PRE-TENSION SECTION options.
Input Data Relative Displacement
Description Defines the relative displacement to apply to the underlying elements in the direction of the section's normal.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Force
Structural
1D
Creates *CLOAD and *PRE-TENSION SECTION options.
Input Data
Description
Force
Main Index
Defines the pre-tension force to apply to the elements.
Object
Type
Option
Type
Dimension
Pre-tension
Element Uniform
Force
Structural
2D, 3D
348 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *CLOAD, *SURFACE and *PRE-TENSION SECTION options.
Input Data Force
Description Defines the pre-tension force to apply to the underlying elements in the direction of the section's normal.
Temperature (Thermal)
Object
Type
Type
Temp (Thermal)
Nodal
Thermal
Creates *BOUNDARY options.
Input Data
Description
Temperature
Defines the nodal temperature value.
Convection
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
2D
Creates *FILM options.
Input Data
Main Index
Description
Top Surf Convection
Defines the convection coefficient for the top surface of a shell element.
Bot Surf Convection
Defines the convection coefficient for the bottom surface of a shell element.
Edge Convection
Defines the convection coefficient for the edges of axisymmetric, plane strain, and plane stress type elements.
Ambient Temp
Defines the ambient temperature.
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
3D
Chapter 2: Building A Model 349 Loads and Boundary Conditions
Creates *FILM options.
Input Data
Description
Convection
Defines the convection coefficient for the face of a solid element.
Ambient Temp
Defines the ambient temperature.
Heat Flux
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
2D
Creates *DFLUX options.
Input Data
Description
Top Surf Heat Flux
Defines the heat flux for the top surface of a shell element.
Bot Surf Heat Flux
Defines the heat flux for the bottom surface of a shell element.
Edge Heat Flux
Defines the heat flux for the edges of axisymmetric, plane strain, and plane stress type elements.
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
3D
Creates *DFLUX options.
Input Data Heat Flux
Description Defines the heat flux for the face of a solid element.
Heat Source
Main Index
Object
Type
Type
Heat Source
Nodal
Thermal
350 Patran Interface to ABAQUS Preference Guide Loads and Boundary Conditions
Creates *CFLUX options.
Input Data Heat Source
Description Defines the reference magnitude for flux (units
Object
Type
Type
Heat Source
Element Uniform
Thermal
J T Ó 1 ).
Creates *DFLUX options.
Input Data Heat Source
Description Defines the reference magnitude for flux (units
J T Ó 1 ).
Initial Temperature
Object
Type
Type
Initial Temperature
Nodal
Thermal
Creates *INITIAL CONDITIONS TYPE=TEMPERATURE options
Input Data Temperature
Main Index
Description Defines the initial temperature for a specified node.
Chapter 2: Building A Model 351 Load Cases
Load Cases Load Cases in Patran ABAQUS are used to group a series of Load sets into one load environment for the model. A load case is selected when preparing an analysis, not load sets. The individual load sets are translated into the input options described in the Object Tables of the section on Loads and Boundary Conditions form.
Main Index
352 Patran Interface to ABAQUS Preference Guide Group
Group Groups in Patran ABAQUS are used to create groups of nodes (*NSET) and groups of elements (*ELSET). All the groups created in Patran will be translated as *NSETs and *ELSETs except for the “default_group” which always exists in the database, and group names which do not begin with an alphabetic character (a-z, A-Z).d
Main Index
Chapter 3 : Running Analysis Patran Interface to ABAQUS Preference Guide
3
Main Index
Running an Analysis
Review of the Analysis Form
Translation Parameters
Restart Parameters
Optional Controls
Direct Text Input
Step Creation
Step Selection
Read Input File
ABAQUS Input File Reader
354
357
358 359 360
361 432 433 435
354 Patran Interface to ABAQUS Preference Guide Review of the Analysis Form
Review of the Analysis Form The Analysis toggle located on the main form for Patran brings up The Analysis Form (p. 8) in the MSC.Patran Reference Manual. This form is used to request an analysis of the model with the ABAQUS finite element program. It can also be used to incorporate the contents of an ABAQUS results file into the database. See Read Results. The following page gives an introduction to the Analysis form used to prepare an ABAQUS analysis. This is followed by detailed descriptions of the subordinate forms that can be displayed from the Analysis form.
Main Index
Chapter 3 : Running Analysis 355 Review of the Analysis Form
Analysis Form Setting the Action option menu on the Analysis Form to Analyze indicates that an analysis run is being prepared.
The Object indicates which part of the model is to be analyzed. It can be set to either Entire Model or Current Group. If the whole model is to be analyzed, select Entire Model. If only a part of the model is
Main Index
356 Patran Interface to ABAQUS Preference Guide Review of the Analysis Form
to be analyzed, create a group of that part, set that as the current group, then select Current Group as the Object. The Method indicates how far the translation is to be taken. Currently only Analysis Deck is supported. The method generates an ABAQUS input deck.
Main Index
Chapter 3 : Running Analysis 357 Translation Parameters
Translation Parameters This subordinate form appears whenever the Translation Parameters button is selected. The parameters controlling the translation of the ABAQUS input deck are defined on this form.
Note:
Main Index
The spatially varying field property values are compared within the band of +half of field properties tolerance and -half of field properties tolerance to group the elements. The property values for this group of elements are added and divided by the number of elements in this group to get the average property value to be used.
358 Patran Interface to ABAQUS Preference Guide Restart Parameters
Restart Parameters This subordinate form appears whenever the Restart Parameters button is selected. This form creates a *RESTART option (see Section 7.10.1 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 359 Optional Controls
Optional Controls This subordinate form appears whenever the Restart Parameters button is selected.
Main Index
360 Patran Interface to ABAQUS Preference Guide Direct Text Input
Direct Text Input This subordinate form appears whenever the Direct Text Input button is selectedK This widget is to facilitate the input of the ABAQUS input data that cannot be created using the functionality available in Patran. All data input here will be appended to the ABAQUS model data before the step history block.
Note:
There is no checking available for invalid input.
Note:
The font for the text input may vary from one system to another. A default font is specified in app_defaults/Patran file: Patran*fixedFont: -misc-fixed-bold-r-normal--13-100-100-100-c-70-iso8859-1 For any problems with the text on a particular system, change the font specifications in the Patran file which should reside in your ~home directory. Use xfontsel, or xlxfonts commands to get the list of available fonts on a given system.
Main Index
Chapter 3 : Running Analysis 361 Step Creation
Step Creation This subordinate form appears whenever the Step Creation button is selected on the Analysis form. A step is defined by associating the load cases created and stored on the database, with the ABAQUS analysis procedure that best addresses that load case, and the relevant associated parameters that guide the solution path for the chosen analysis procedure. There is no importance to the order in which the Job Steps are created on this form--they will be ordered for the job in the Step Selection form.
Main Index
362 Patran Interface to ABAQUS Preference Guide Step Creation
Select Load Cases This subordinate form appears whenever the Select Load Cases button is selected on the Step Creation form.
Output Requests This subordinate form appears whenever the Output Requests button is selected on the Step Create form. It is used for specifying the specific variables to be included in the output from ABAQUS options such as: ∗EL PRINT, ∗ENERGY PRINT, ∗MODAL PRINT, ∗NODE PRINT, ∗PRINT, ∗EL FILE, ∗ENERGY FILE, ∗FILE FORMAT, ∗MODAL FILE, and ∗NODE FILE *ELEMENT MATRIX OUTPUT. An explanation of the output variables that can be requested is included in the Output Requests description for each solution type.
Main Index
Chapter 3 : Running Analysis 363 Step Creation
Direct Text Input This subordinate form appears whenever the Direct Text Input button is selectedK This widget is to facilitate the input of the ABAQUS input data that cannot be created using the functionality available in Patran menus. All data input here will be appended to the ABAQUS step history being created.
Note:
There is no checking available for invalid data. The font for the text input may vary from one system to another. A default font is specified in app_defaults/Patran file:
Main Index
364 Patran Interface to ABAQUS Preference Guide Step Creation
Patran*fixedFont: -misc-fixed-bold-r-normal--13-100-100-100-c-70-iso8859-1 For any problems with the text on a particular system, change the font specifications in the Patran file which should reside in your ~home directory. Use xfontsel, or xlxfonts commands to get the list of available fonts on a given system.
Solution Types Each step has an associated Solution type, and the information that is requested on the Solution Parameters and Output Requests forms varies based on this selection. ABAQUS calls these analysis procedures, and the full explanations of these procedures can be found in Chapter 2 “Procedures Library” of the ABAQUS/Standard User’s Manual.
Main Index
Parameter Type
Description
Linear Static
Static stress analysis is used when inertia effects can be neglected. During a linear static step, the model’s response is defined by the linear elastic stiffness at the base state, the state of deformation and stress at the beginning of the step. For ∗HYPERELASTIC and ∗HYPERFOAM materials, the tangent elastic moduli in the base state is used. Contact conditions cannot change during the step--they remain as they are defined in the base state.
Natural Frequency
This solution type uses eigenvalue techniques to extract the frequencies of the current system. The stiffness determined at the end of the previous step is used as the basis for the extraction, so that small vibrations of a preloaded structure can be modeled.
Chapter 3 : Running Analysis 365 Step Creation
Parameter Type
Description
Bifurcation Buckling
Eigenvalue buckling estimates are obtained. Classical eigenvalue buckling analysis (e.g., “Euler” buckling) is often used to estimate the critical (buckling) load of “stiff” structures. “Stiff” structures are those that carry their design loads primarily by axial or membrane action, rather than by bending action. Their response usually involves very little deformation prior to buckling.
Direct Linear Transient
This solution procedure integrates all of the equations of motion through time, and is significantly more expensive than modal methods for finding dynamic response for linear systems. For linear systems, the dynamic method, using the Hilber-Hughes-Taylor operator, is unconditionally stable, meaning there is no mathematical limit on the size of the time increment that can be used to integrate a linear system. Since the procedure uses a fixed time increment, the HAFTOL parameter on the *DYNAMIC card is not required.
Direct Steady State Dynamics Calculates steady state response for the given range of frequencies. The damping may be created by dashpots, by “Rayleigh” damping associated with materials, and by viscoelasticity included in the material definitions. Modal Linear Transient
This solution type gives the response of the model as a function of time, based on a given time dependent loading. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.The number of modes extracted must be sufficient to model the dynamic response of the system adequately. This is a matter of judgment on the part of the user. The modal amplitudes are integrated through time and the response synthesized from these modal responses.
Modal Steady State Dynamics This solution type provides the response of the system when it is excited by harmonic loading at a given frequency. This procedure is usually preceded by extraction of the natural modes using the NATURAL FREQUENCY solution type, although ABAQUS also allows the response to be calculated directly from the system matrices for use in those cases where the eigenvalues cannot be extracted, such as a nonsymmetric stiffness case, or models in which the behavior is itself a function of frequency, such as frequency dependent material damping.
Main Index
366 Patran Interface to ABAQUS Preference Guide Step Creation
Main Index
Parameter Type
Description
Response Spectrum
This solution type provides an estimate of the peak response of a structure to steady-state dynamic motion of its fixed points (“base motion”). The method is typically used when an approximate estimate of such peak response is required for design purposes. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.
Random Vibration
This solution type predicts the response of a system which is subjected to a nondeterministic continuous excitation that is expressed in a statistical sense using a power spectral density function. The procedure is based on using a subset of the eigenmodes of the system, which must first be extracted using the NATURAL FREQUENCY solution type.
Nonlinear Static
Nonlinear static analysis requires the solution of nonlinear equilibrium equations, for which ABAQUS uses Newton’s method. Many problems involve history dependent response, so that the solution is usually obtained as a series of increments, with iteration within each increment to obtain equilibrium. For most cases, the automatic incrementation provided by ABAQUS is preferred, although direct user control is also provided for those cases where the user has experience with a particular problem.
Chapter 3 : Running Analysis 367 Step Creation
Main Index
Parameter Type
Description
Nonlinear Transient Dynamic
This solution type is used when nonlinear dynamic response is being studied. Because all of the equations of motion of the system must be integrated through time, direct integration methods are generally significantly more expensive than modal methods. For most cases, the automatic incrementation provided by ABAQUS is preferred, although direct user control is also provided for those cases where the user has experience with a particular problem.
Creep
This analysis procedure performs a transient, static, stress⁄displacement analysis. It is especially provided for the analysis of materials which are described by the ∗CREEP material form.
Viscoelastic (Time Domain)
This is especially provided for the time domain analysis of materials which are described by the ∗VISCOELASTIC, TIME material option. The dissipative part of the material behavior is defined through a Prony series representation of the normalized shear and bulk relaxation moduli, either specified directly on the ∗VISCOELASTIC, TIME material option, determined from user input creep test data, or determined from user input relaxation test data.
Viscoelastic (Frequency Domain)
This is especially provided for the frequency domain analysis of materials which are described by the ∗VISCOELASTIC, FREQUENCY material option, which is activated by a ∗STEADY STATE DYNAMICS, DIRECT procedure.The dissipative part of the material behavior is defined by the real and imaginary parts of the Fourier transforms of the nondimensional shear viscoelasticity parameter g and, for compressible materials, of the bulk viscoelasticity parameter k.
Steady State Heat Transfer
This solution type is for pure heat transfer problems for which the ∗HEAT TRANSFER option is used and where the temperature field can be found without knowledge of stress and deformation of the bodies being studied.
Transient Heat Transfer
This solution type is for pure transient heat transfer problems for which the ∗HEAT TRANSFER option is used and where the temperature field can be found without knowledge of stress and deformation of the bodies being studied. For all transient heat transfer cases, the time increments may be specified directly, or will be selected automatically based on a user prescribed maximum nodal temperature change in a step. Automatic time incrementation is generally preferred.
368 Patran Interface to ABAQUS Preference Guide Step Creation
Linear Static
Read Temperature File= This option is used to specify temperatures via the results file which has been generated from a previous heat transfer analysis. Only one temperature results file is allowed in an analysis but the same file can be referenced by many steps.
Main Index
Chapter 3 : Running Analysis 369 Step Creation
Linear Static If the selected solution type is Linear Static then the following parameters may be defined on the Output Requests form.
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. S11, S22, S33, For example, the truss element outputs the axial stress (S11) only, S12, S13, S23 while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
SINV The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The strain E components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Elem Energy Densities
The strain energy per unit volume of each element. Plastic, creep, and viscous dissipative energy densities should not be affected by linear static analysis.
ENER
Elem Energy Magnitudes
The strain energy of each element. Plastic, creep, and viscous dissipative energy densities should not be affected by linear static analysis.
ELEN
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the axial SF force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
370 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N). Displacements
Displacements are output at nodes and are referred to as follows:
STH U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degreeof-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist RF changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Chapter 3 : Running Analysis 371 Step Creation
Parameter Name
Description
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Element Mass Matrix
Mass matrices output.
Output Variable Identifier ALLEN
Element Stiffness matrices output. Stiffness Matrix Natural Frequency This subordinate form appears whenever the Solution Parameters button is selected and the solution types is Natural Frequency. This generates ∗FREQUENCY procedures (see Section 9.3.5 of the ABAQUS/Standard User’s Manual). The optional NLGEOM parameter on the ∗STEP option may be included, as defined below. None of the other optional parameters on the ∗pqbm option (AMPLITUDE, INC, or MONOTONIC) are used.
Natural Frequency
If the selected Solution Type is Natural Frequency, then the following parameters may be defined on the Output Requests form. A complete discussion of the ABAQUS results file can be found in Chapter 6 of the ABAQUS/Standard User’s Manual. Note that the Natural Frequency solution type extracts the frequency and corresponding mode shapes (eigenvalues and eigenmodes), usually for use in a later analysis (e.g., Response Spectrum). The stresses and strains corresponding to the mode shapes can be
Main Index
372 Patran Interface to ABAQUS Preference Guide Step Creation
output, but are usually of limited direct value except as a possible means for guiding mode limitations for future analyses.
Parameter Name
Output Variable Identifier
Description
S11, S22, S33, S12, S13, S23
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, First principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system.
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
SE
Chapter 3 : Running Analysis 373 Step Creation
Parameter Name
Output Variable Identifier
Description
Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time. Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
RF
Bifurcation Buckling This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Bifurcation Buckling. This form defines the data required for a *BUCKLE command (see Section 9.3.2 of the ABAQUS/Standard User’s Manual). This step may be included either as the first step or when the structure has already been preloaded. If the structure has been preloaded, the buckle sensitivity around the preloaded state is calculated. The problem is a classical eigenvalue problem, with the
Main Index
374 Patran Interface to ABAQUS Preference Guide Step Creation
eigenvalues defined as the load multipliers of the load pattern for which buckling sensitivity is being investigated.
Bifurcation Buckling
If the selected Solution Type is Bifurcation Buckling then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
The stress components output depend on the elements analyzed. S11, S22, S33, S12, For example, the truss element outputs the axial stress (S11) S13, S23 only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Chapter 3 : Running Analysis 375 Step Creation
Parameter Name
Output Variable Identifier
Description E
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Section Forces
SF Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Sectiono 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
376 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Description Displacements are output at nodes and are referred to as follows:
Output Variable Identifier U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time. Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
RF
Direct Linear Transient This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Direct Linear Transient. This generates a *DYNAMIC procedure, with the optional DIRECT parameter included (see Section 9.3.4 of the ABAQUS/Standard User’s Manual). Note that modal methods are usually more economical for linear dynamic analysis. Many of the parameters described in the ABAQUS/Standard User’s Manual for the *DYNAMIC option are not used for this option.
Main Index
Chapter 3 : Running Analysis 377 Step Creation
Direct Linear Transient
If the selected Solution Type is Direct Linear Transient then the following parameters may be defined on this form.
Parameter Name
Description
Stress Components The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual. Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Main Index
Output Variable Identifier S11, S22, S33, S12, S13, S23
SINV
E
378 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Output Variable Identifier
Elem Energy Densities
The strain energy per unit volume of each element.
ENER
Elem Energy Magnitudes
The strain energy of each element.
ELEN
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, SE these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 379 Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
380 Patran Interface to ABAQUS Preference Guide Step Creation
Direct Steady State Dynamics This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Direct Steady State Dynamics. This generates a ∗STEADY STATE DYNAMIC procedure.
Direct Steady State Dynamics
If the selected solution type is Direct Steady State Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Ph Angle Stress Components
The phase angle shift of the stress components.
PHS
Chapter 3 : Running Analysis 381 Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Ph Angle Strain Components
The phase angle shift of the strain components.
PHE
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
382 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Phase Angle Rel. Displacements
The phase angle shift of the relative displacement components.
PU
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
The phase angle shift of the reaction force components.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 383 Step Creation
Modal Linear Transient This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Modal Linear Transient. This generates a *FREQUENCY procedure (see Section 9.3.5 of the ABAQUS/Standard User’s Manual) followed by a ∗MODAL DYNAMIC procedure (see Section 9.3.8 of the ABAQUS/Standard User’s Manual). A ∗MODAL DAMPING option will also be generated, as required. Only one load case may be selected.
Main Index
384 Patran Interface to ABAQUS Preference Guide Step Creation
Modal Linear Transient
This subordinate form appears whenever the Output Request button is selected on the Step Create form, and the Solution Type is Modal Linear Transient.
Parameter Name
Description
Stress Components
S11, S22, The stress components output depend on the elements S33, S12, analyzed. For example, the truss element outputs the axial S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal tress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
Chapter 3 : Running Analysis 385 Step Creation
Parameter Name Section Strains
Description
Output Variable Identifier
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N)
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Acceleration
Nodal accelerations, following the same convention as for displacements.
A
386 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Total Displacements
The summation of all individual modal components of displacement. The output follows the same convention as for the individual modal components.
TU
Total Velocities
The summation of all individual modal components of velocity. The output follows the same convention as for the individual modal components.
TV
Total Accelerations
The summation of all individual modal components of acceleration. The output follows the same convention as for the individual modal components.
TA
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads, (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration.
GA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix Mass matrices output. Element Stiffness Matrix
Main Index
Output Variable Identifier
Stiffness matrices output.
Chapter 3 : Running Analysis 387 Step Creation
Define Damping Direct When the type of Modal Damping selected is Direct, this subordinate form appears whenever Define Damping is selected. The data is used to define the *MODAL DAMPING option (see Section 9.6.6 of the ABAQUS/Standard User’s Manual) with the MODAL parameter set to DIRECT.
Main Index
388 Patran Interface to ABAQUS Preference Guide Step Creation
Define Damping Rayleigh When the type of Modal Damping selected is Rayleigh, this subordinate form appears whenever Define Damping is selected. This form defines the data required for the *MODAL DAMPING, RAYLEIGH option (see Section 9.6.6 of the ABAQUS/Standard User’s Manual).
Base Motion This subordinate form appears whenever Define Base Motion is selected from the Modal Linear Transient, Steady State Dynamics, or Viscoelasticity Frequency Domain Solution Parameter forms. It defines the values on the ∗BASE MOTION option (see Section 9.4.2 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 389 Step Creation
Steady State Dynamics This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Steady State Dynamics. This generates a *STEADY STATE DYNAMICS procedure (see Section 9.3.13 of the ABAQUS/Standard User’s Manual). A *FREQUENCY procedure may also be created prior to the *STEADY STATE DYNAMICS procedure, if required.
Main Index
390 Patran Interface to ABAQUS Preference Guide Step Creation
Steady State Dynamics
If the selected solution type is Steady State Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Ph Angle Stress Component
The phase angle shift of the stress components.
PHS
Chapter 3 : Running Analysis 391 Step Creation
Parameter Name
Output Variable Identifier
Description
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Ph Angle Strain Component
The phase angle shift of the strain components.
PHE
Element Energy Magnitudes
A scalar value for the energy content of the element.
ELEN
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
392 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for A displacements.
Total Displacements
The summation of all individual modal components of displacement. The output follows the same convention as for the individual modal components.
TU
Total Velocities
The summation of all individual modal components of velocity. The output follows the same convention as for the individual modal components.
TV
Total Accelerations
The summation of all individual modal components of acceleration. The output follows the same convention as for the individual modal components.
TA
Phase Angle Rel. Displacements
All components of the phase angle of the displacements at the node.
PU
Phase Angle Total Displacements
All components of the phase angle of the total displacements at the node.
PTU
Chapter 3 : Running Analysis 393 Step Creation
Parameter Name
Main Index
Output Variable Identifier
Description
Reaction Forces
The forces at the nodes which are constrained and so, therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
All components of the phase angle of the reaction forces at the node.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads, (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration. GA
Phase Angle Generalized Displacements
The phase angle of displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
Phase Angle Generalized Velocities
The phase angle of velocities associated with the modes of PGV vibration.
Phase Angle Generalized Accelerations
The phase angle of accelerations associated with the modes of vibration.
PGA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration). BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, ALLEN recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
PGU
394 Patran Interface to ABAQUS Preference Guide Step Creation
Define Frequencies The data on this form is used to define the input for the *STEADY STATE DYNAMICS option (see Section 9.3.13 of the ABAQUS/Standard User’s Manual).
Response Spectrum This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Response Spectrum. This generates a *FREQUENCY procedure, and a *RESPONSE SPECTRUM procedure (see Sections 9.3.5 and 9.3.10, respectively, of the ABAQUS/Standard User’s Manual). A ∗SPECTRUM option is also created (see Section 7.11.5 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 395 Step Creation
Define Response Spectra (Response Spectrum) This subordinate form appears whenever the Define Response Spectra button is selected on the Response Spectrum Solution Parameter form.
Main Index
396 Patran Interface to ABAQUS Preference Guide Step Creation
Define Spectrum (Response Spectrum) This form appears whenever the Define Spectrum button is selected on the Response Spectra form, which is itself subordinate to the Response Spectrum Solution Parameter Form. Similar forms are used for the second and third directions.The data on this form will define the *SPECTRUM option (see Section 7.11.5 of the ABAQUS/Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 397 Step Creation
Response Spectrum
If the selected solution type is Response Spectrum, then the following parameters may be defined on the Output Requests form.
Main Index
398 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
SF
Chapter 3 : Running Analysis 399 Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
400 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Main Index
Description
Output Variable Identifier
Reaction Forces
The forces at the nodes which are constrained and therefore, RF resist changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Chapter 3 : Running Analysis 401 Step Creation
Parameter Name
Description
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibration.
GV
Generalized Accelerations
The accelerations associated with the modes of vibration.
GA
Strain Energy per Mode
Elastic strain energy for the entire model per each mode.
SNE
Kinetic Energy per Mode
Kinetic energy for the entire model per each mode.
KE
External Work per Mode
External work for the entire model per each mode.
T
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
Main Index
Output Variable Identifier
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
ALLEN
402 Patran Interface to ABAQUS Preference Guide Step Creation
Random Vibration This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Random Vibration. This generates a *FREQUENCY procedure and a *RANDOM RESPONSE procedure (see Sections 9.3.5 and 9.3.9 of the ABAQUS⁄Standard User’s Manual).
Main Index
Chapter 3 : Running Analysis 403 Step Creation
Define Spectrum (Random Vibration) The Spectrum Data Table form is used to define the power spectral density function data for the ∗PSDDEFINITION option (see Section 7.11.3 of the ABAQUS/Standard User’s Manual).
Main Index
404 Patran Interface to ABAQUS Preference Guide Step Creation
Random Vibration
If the selected solution type is Random Vibration, then the following parameters may be defined on the Output Requests form.
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
R.M.S. Stress Components
The root mean square value of the stress components.
RA
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
R.M.S. Strain Components
The root mean square value of the strain components.
RE
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Main Index
Output Variable Identifier
Chapter 3 : Running Analysis 405 Step Creation
Parameter Name Section Strains
Output Variable Identifier
Description Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Displacements
Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
R.M.S. Relative Displacement
The root mean square value of the displacement components relative to the base motion.
RU
406 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
R.M.S. Relative Velocities
The root mean square value of the velocity components relative to the base motion.
RV
R.M.S. Relative Acceleration
The root mean square value of the acceleration components relative to the base motion.
RA
Total Displacements The total displacement (including base motion) of the nodes.
Main Index
Output Variable Identifier
TU
Total Velocities
The total velocity (including base motion) of the nodes.
TV
Total Acceleration
The total acceleration (including base motion) of the nodes.
TA
R.M.S. Total Displacements
The root mean square value of the displacement components including the base motion.
RTU
R.M.S. Total Velocities
The root mean square value of the velocity components including the base motion.
RTV
R.M.S. Total Accelerations
The root mean square value of the acceleration components including the base motion.
RTA
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
R.M.S. Reaction Forces
The root mean square value of the modal component of the reaction forces.
RRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Generalized Displacements
The displacements associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GU
Generalized Velocities
The velocities associated with the modes of vibrations, each of GV which have a shape (eigenmode) and associated frequency (eigenvalue).
Generalized Accelerations
The accelerations associated with the modes of vibrations, each of which have a shape (eigenmode) and associated frequency (eigenvalue).
GA
Base Motion
The base motion (displacement, velocity, or acceleration).
BM
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Chapter 3 : Running Analysis 407 Step Creation
Parameter Name
Description
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier
Nonlinear Static This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Nonlinear Static. This generates a *STATIC procedure with the associated *STEP option. The NLGEOM parameter on the *STEP command is included. The NLGEOM parameter is included on the *STEP option.
More data input is available for defining the Nonlinear Static Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu if the Riks method is not selected.
Main Index
408 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Max No of Increments
Defines the maximum number of increments that can be used within a single step. This is a positive integer value. This is the optional INC parameter on the ∗STEP option.
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Listed below are the remaining parameters contained in this menu if the Riks method is selected.
Main Index
Parameter Name
Description
Initial Load Fraction
Defines the initial load fraction to be applied to the model. This is a real constant. This is the initial time increment data value on the ∗STATIC command.
Minimum Load Fraction
Defines the minimum load fraction which will be added during any increment. These are real constants.
Maximum Load Fraction
Defines the maximum load fraction which will be added during any increment. These are real constants.
Stopping Condition
Indicates which stopping condition is to be used. This can be set to “Max. no. increments”, “Max. load multiplier”, or “Monitor a Node.” This indicates which stopping condition data values are to be defined on the ∗STATIC option.
Max. Load Multiplier
This defines the maximum load multiplier allowed before the iteration will be stopped. This is only used if “Max. load multiplier,” or “Monitor a Node” are selected.
Node Number
Indicates the node ID to be monitored. This is only used if “Monitor a Node” is selected.
Chapter 3 : Running Analysis 409 Step Creation
Parameter Name
Description
Limit Value
Defines the limiting displacement at the node being monitored. This is only used if “Monitor a Node” is selected.
DOF Number
Indicates which degree-of-freedom at this node is to be monitored. This is only used if “Monitor a Node” is selected.
Nonlinear Static
If the selected solution type is Nonlinear Static, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier S11, S22, S33, S12, S13, S23
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, SINV Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
E
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
410 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Output Variable Identifier
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, creep, and viscous dissipative energy densities are reported.
ENER
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, plastic, creep, and ELEN viscous dissipative energies are reported.
Internal Stress Forces
The forces that are found at each node by summing the element NFORC stress contributions at the nodes.
Section Forces
Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
SE Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 411 Step Creation
Parameter Name Displacement
Description Displacements are output at nodes and are referred to as follows:
Output Variable Identifier U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
412 Patran Interface to ABAQUS Preference Guide Step Creation
Nonlinear Transient Dynamic This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Nonlinear Transient Dynamic. This generates a ∗DYNAMIC procedure, with the associated ∗STEP option. The DIRECT and HAFTOL parameters are available on the ∗DYNAMIC option.
Main Index
Chapter 3 : Running Analysis 413 Step Creation
More data input is available for defining the Nonlinear Transient Dynamic Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Main Index
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Max Error in Mid Increment Residual
This is the HAFTOL parameter on the ∗DYNAMIC option. See Section 9.3.4 of the ABAQUS/Standard User’s Manual and Section 5.2.1 of the ABAQUS/Standard Example Problems.
414 Patran Interface to ABAQUS Preference Guide Step Creation
Nonlinear Transient Dynamic
If the selected solution type is Nonlinear Transient Dynamics, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Output Variable Identifier
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
E
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Chapter 3 : Running Analysis 415 Step Creation
Parameter Name Section Forces
Description Section forces are output for beam elements and include the axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
Output Variable Identifier SF
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SW
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, STH SAX2, SAXA1N, SAXA2N).
416 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads CF (e.g., the force at a node resulting from pressure distributions on adjacent elements).
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
ALLEN
Chapter 3 : Running Analysis 417 Step Creation
Creep This subordinate form appears whenever the Solution Parameters button is selected and the Solution Type is Creep. This generates a ∗VISCO procedure, with the associated ∗STEP option.
More data input is available for defining the Creep Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Main Index
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
418 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Admissable Error in Strain Increment
This is the CETOL parameter on the ∗VISCO option. See Section 9.3.15 of the ABAQUS/Standard User’s Manual.
Creep
The strain components output depend on the elements analyzed, analogous to the stress components. In addition, the total strain component can be separated into its contributory parts (e.g., elastic strain, plastic strains, etc.) and these are reported separately.
Main Index
Output Variable Identifier
Parameter Name
Description
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Chapter 3 : Running Analysis 419 Step Creation
Parameter Name
Output Variable Identifier
Description
Elastic Strains
The elastic strain component of the total strain. Note that the EE elastic strain component is the component from which the stress is computed.
Inelastic Strains
The total strain minus the elastic strain component.
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
IE
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
420 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, RF resist changes in the system. The direction convention is the same as that for nodal output.
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation are reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 421 Step Creation
Viscoelastic (Time Domain) This subordinate form appears whenever Solution Parameters is selected and the Solution Type is Viscoelastic (Time Domain). This generates a ∗VISCO procedure, with the associated ∗STEP command.
Main Index
422 Patran Interface to ABAQUS Preference Guide Step Creation
More data input is available for defining the Viscoelastic (Time Domain) Solution Parameters shown on the previous page. Listed below are the remaining parameters contained in this menu.
Parameter Name
Description
Initial DELTA-T
Defines the initial time increment to be used. This is a real constant. This will be modified as required if the automatic time stepping scheme is used. Otherwise, it will be used as a constant time increment.
Minimum DELTA-T
Defines the minimum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If ABAQUS finds it needs a smaller time increment than this value, the analysis is terminated.
Maximum DELTA-T
Defines the maximum time increment to be used. This is a real constant. It is only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
Time Duration of Step
Defines the total time period of the step. This is a real constant.
Viscoelastic (Time Domain)
If the selected Solution Type is Viscoelastic (Time Domain), then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
S11, S22, S33, The stress components output depend on the elements analyzed. For example, the truss element outputs the axial S12, S13, S23 stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
Stress Invariants
SINV The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
Chapter 3 : Running Analysis 423 Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that for linear elastic analyses, the total strain is equal to the elastic strain.
Plastic Strains
The plastic strain component of the total strain.
PE
Creep Strains
The creep strain component of the total strain.
CE
Elastic Strains
The elastic strain component of the total strain. Note that the elastic strain component is the component from which the stress is computed.
EE
Inelastic Strains
The total strain minus the elastic strain component.
IE
Elem Energy Densities
The energy per unit volume of each element. Strain, plastic, ENER creep, and viscous dissipative energy densities are reported.
Elem Energy Magnitudes
The energy of each element. Strain, kinetic, elastic, creep, and viscous dissipative energies are reported.
ELEM
Internal Stress Forces
The forces that are found at each node by summing the element stress contributions at the nodes.
NFORC
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual. For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual.
Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
424 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Reaction Forces
The forces at the nodes which are constrained and therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
Whole Model Energies
The summation of all the energy of the model. The kinetic, recoverable (elastic) strain, plastic dissipation, creep dissipation, and viscous dissipation is reported.
ALLEN
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Chapter 3 : Running Analysis 425 Step Creation
Viscoelastic (Frequency Domain) This subordinate form appears whenever the Solution Parameters button is selected and the solution type is Viscoelastic (Frequency Domain). This generates a *STEADY STATE DYNAMIC procedure.
Viscoelastic (Frequency Domain)
If the selected solution type is Viscoelastic (Frequency Domain), then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Stress Components
The stress components output depend on the elements analyzed. For example, the truss element outputs the axial stress (S11) only, while a three-dimensional solid element outputs all six components (S11, S22, S33, S12, S13, S23). Note that ABAQUS always reports the Cauchy, or true stress, which is equal to the force per current area. For more information about element output, see Chapter 3 of the ABAQUS/Standard User’s Manual.
S11, S22, S33, S12, S13, S23
Stress Invariants
The stress invariants output by ABAQUS are the Mises stress, Tresca stress, Hydrostatic pressure, first principal stress, second principal stress, third principal stress, and the third stress invariant. These quantities are scalar quantities which do not vary with a change of coordinate system. For elastic analyses, the von Mises and/or the Tresca stress invariants can be monitored to ensure that the analysis remains within the assumptions of linearity.
SINV
Ph Angle Stress Components
The phase angle shift of the stress components.
PHS
426 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Output Variable Identifier
Description
Strain Components
This is the total strain value for each component output. The E strain components output depend on the elements analyzed, analogous to the stress components. Note that, for linear elastic analyses, the total strain is equal to the elastic strain.
Ph Angle Strain Components
The phase angle shift of the strain components.
Section Forces
Section forces are output for beam elements and include the SF axial force, and, as applicable, the shears, bending moments and bimoment about the local axes. These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
PHE
For shell elements, the section forces include the direct membrane, shear, and moment forces per unit width, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Section Strains
Section strains are output for beam elements and, as applicable, these include the axial strain, transverse shear strains, curvature changes, and twist about the local axes.These are discussed in Section 3.5.1 and Section 7.5.2 of the ABAQUS/Standard User’s Manual.
SE
For shell elements, the section strains include the direct membrane, shear, curvature changes, and twist, as applicable. These are discussed in Section 3.6 of the ABAQUS/Standard User’s Manual. Shell Thickness
Main Index
Changes in thickness for shell elements (S3RF, S4RF,SAX1, SAX2, SAXA1N, SAXA2N).
STH
Chapter 3 : Running Analysis 427 Step Creation
Parameter Name Displacements
Output Variable Identifier
Description Displacements are output at nodes and are referred to as follows:
U
1. x-displacement 2. y-displacement 3. z-displacement 4. Rotation about the x-axis 5. Rotation about the y-axis 6. Rotation about the z-axis Except for axisymmetric elements, where the displacement and rotation degrees-of-freedom are: 1. r-displacement 2. z-displacement 3. Rotation in the r-z plane Here x, y, z, and r are global directions unless a coordinate transformation is used at the node. Note that the warping degree-of-freedom, the seventh displacement component of an open section beam element, is not supported by Patran at this time.
Main Index
Velocities
Nodal velocities, following the same convention as for displacements.
V
Accelerations
Nodal accelerations, following the same convention as for displacements.
A
Phase Angle Rel. Displacements
The phase angle shift of the relative displacement components.
PU
Reaction Forces
The forces at the nodes which are constrained and so, therefore, resist changes in the system. The direction convention is the same as that for nodal output.
RF
Phase Angle Reaction Forces
The phase angle shift of the reaction force components.
PRF
Point Forces
The forces at the nodes resulting from the imposed loads (e.g., the force at a node resulting from pressure distributions on adjacent elements).
CF
428 Patran Interface to ABAQUS Preference Guide Step Creation
Parameter Name
Description
Element Mass Matrix
Mass matrices output.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier
Steady State Heat Transfer This subordinate form appears whenever Solution Parameters is selected and the solution type is Steady State Heat Transfer. This generates a ∗HEAT TRANSFER, STEADY STATE procedure.
Steady State Heat Transfer
If the selected solution type is Steady State Heat Transfer, then the following parameters may be defined on the Output Requests form.
Parameter Name
Main Index
Description
Output Variable Identifier
Element Temperature
Temperature.
TEMP
Heat Flux
Current magnitude and components of the heat flux vector. The integration of points for these values are located at the Gauss points.
HFL
Nodal Temperatures
NT All temperature values at a node. These will be the temperatures defined as degrees-of-freedom if heat transfer elements are connected to the node, or predefined temperatures if the node is only connected to stress elements without temperature degrees-of-freedom.
Reaction Fluxes
All reaction flux values (conjugate to temperature).
RFL
Chapter 3 : Running Analysis 429 Step Creation
Parameter Name
Main Index
Description
Concentrated Fluxes
All concentrated flux values.
Element Stiffness Matrix
Stiffness matrices output.
Output Variable Identifier CFL
430 Patran Interface to ABAQUS Preference Guide Step Creation
Transient Heat Transfer This subordinate option is Transient Heat Transfer. This generates a ∗HEAT TRANSFER procedure.
Transient Heat Transfer
If the selected solution type is Transient Heat Transfer, then the following parameters may be defined on the Output Requests form.
Main Index
Chapter 3 : Running Analysis 431 Step Creation
Parameter Name
Main Index
Description
Output Variable Identifier
Element Temperature
Temperature.
TEMP
Heat Flux
Current magnitude and components of the heat flux vector. The integration of points for these values are located at the Gauss points.
HFL
Nodal Temperatures
NT All temperature values at a node. These will be the temperatures defined as degrees-of-freedom if heat transfer elements are connected to the node, or predefined temperatures if the node is only connected to stress elements without temperature degrees-of-freedom.
Reaction Fluxes
All reaction flux values (conjugate to temperature).
RFL
Concentrated Fluxes
All concentrated flux values.
CFL
Element Stiffness Matrix
Stiffness matrices output.
432 Patran Interface to ABAQUS Preference Guide Step Selection
Step Selection This subordinate form appears whenever the Step Selection button is selected on the main Analysis form. This form is used to select and order the Job Steps that will be analyzed for the ABAQUS Job.
Main Index
Chapter 3 : Running Analysis 433 Read Input File
Read Input File It is possible to read an existing ABAQUS input file (jobname.inp) into Patran. This is not a fully supported feature and must be invoked by setting a special parameter. This is done by editing the settings.pcl file and adding the following line: pref_env_set_logical( "shareware_input_file", TRUE ) If this setting is set to TRUE, then an additional Action item will appear under the Analysis form called Read Input File. This file can exist in the installation, local or home directories.
Main Index
434 Patran Interface to ABAQUS Preference Guide Read Input File
Main Index
Chapter 3 : Running Analysis 435 ABAQUS Input File Reader
ABAQUS Input File Reader This section describes a software module that reads ABAQUS input files and writes the data to the MSC/PATRAN database in a form compatible with the MSC/PATRAN ABAQUS preference.
Input Deck Formats Both fixed format and free format entries are supported. Floating point formats with and without an “E” in the exponent are supported (e.g. 1.23E6 and 1.23+6 are both supported). Message File Informative, warning, and error messages are written to an external file with the name
ABAQUS ELSET and NSET Entries A PATRAN group is created for each ABAQUS ELSET or NSET entry. The name of the group is taken from the NAME parameter of the ELSET or NSET. Supported Element Types When the reader encounters a *ELEMENT entry, the combination of the element type and the ABAQUS property set entry are used to map the ABAQUS element type to the appropriate PATRAN element type. In some cases this is not possible because not all ABAQUS element types are currently supported in PATRAN. In these cases, the reader attempts to find the PATRAN element type that “best” matches the ABAQUS type. Thus, the ABAQUS elements retain their association to their property set. This allows the finite element mesh to be edited in PATRAN and an ABAQUS input deck output that can be easily edited to correct the property entry. Supported Keywords The table below describes the ABAQUS keywords that are supported in the current version of the product.
ABAQUS Keyword
Notes Model Section
Main Index
*AMPLITUDE
A PATRAN time- or frequency-dependent field is created.
*BEAM GENERAL SECTION
A PATRAN property set is created.
436 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
ABAQUS Keyword
Notes
*BEAM SECTION
A PATRAN property set is created.
*BOUNDARY
A PATRAN LBC set is created for each ABAQUS BOUNDARY and added to all load cases. Displacement, temperature, velocity, and acceleration boundary conditions are currently supported.
*CENTROID
Location is added to the PATRAN property set.
*CONDUCTIVITY
Value is added to the PATRAN material.
*CONTACT NODE SET
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*CONTACT PAIR
A PATRAN contact-type LBC set is created for each entry in *CONTACT PAIR.
*CORRELATION *DAMPING
Value is added to the PATRAN material or shell element property set.
*DASHPOT
A PATRAN property set is created.
*DENSITY
Value is added to the PATRAN material.
*ELASTIC
Values are added to the PATRAN material.
*ELCOPY
Element Generation Command
*ELEMENT
PATRAN elements are created. Both a PATRAN group and a property set are created with the ELSET name.
*ELGEN
PATRAN elements are created.
*ELSET
A PATRAN group is created.
*EQUATION
A PATRAN MPC is created. The use of node sets in *EQUATION entries is not currently supported.
*EXPANSION
Values are added to the PATRAN material.
*FRICTION
The *FRICTION keyword is supported within *GAP, *INTERFACE, and *SURFACE INTERACTION blocks. The friction properties are added to the appropriate property or LBC set.
*GAP
A PATRAN property set is created.
*HEADING
A PATRAN analysis job is created with this description.
*HOURGLASS STIFFNESS The values are added to the appropriate PATRAN property set.
Main Index
*INCLUDE
The referenced file is read. *INCLUDE entries may be nested to any reasonable depth.
*MASS
A PATRAN property set is created.
*MATERIAL
A PATRAN material is created.
*MEMBRANE SECTION
A PATRAN property set is created.
Chapter 3 : Running Analysis 437 ABAQUS Input File Reader
ABAQUS Keyword *MPC
Notes A PATRAN MPC is created. The use of node sets in *MPC entries is not currently supported.
*MODAL DAMPING *NCOPY
Generates additional nodes using NID and X/Y/Z offsets.
*NFILL
PATRAN nodes are created. The SINGULAR option is not currently supported.
*NGEN
PATRAN nodes are created. Nodes may be generated along a line or a circular arc (LINE=C) but not along a parabola (LINE=P).
*NODAL THICKNESS
A PATRAN nodal FEM field and property set are created.
*NODE
PATRAN nodes are created. If an NSET parameter is specified, a PATRAN group is created with this name, otherwise the nodes are added to the default group.
*NSET
A PATRAN group is created.
*ORIENTATION
Is used to define orientation for homogeneous or laminate material properties.
*PLASTIC
Only HARDENING=ISOTROPIC and HARDENING=KINEMATIC are currently supported. The RATE parameter is not currently supported; only the first set *PLASTIC entries for a material are imported.
*PSD
Main Index
*RIGID BODY
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*RIGID SURFACE
The *RIGID SURFACE keyword is currently supported in two ways by the PATRAN, ABAQUS preference. For the older style of ABAQUS contact, which required the use of IRSx type elements, *RIGID SURFACE entries were written out for “rigid surface type” element properties. For the newer style of ABAQUS contact ,which uses *CONTACT PAIR, geometric curves are selected directly in a PATRAN contact-type LBC. Only this second usage of *RIGID SURFACE is supported by the reader. When referenced in a *CONTACT PAIR entry, curves are created and references to them added to the contact-type LBC set.
*ROTARY INERTIA
A PATRAN property set is created.
*SECTION POINTS
Points are added to the PATRAN property set.
*SHEAR CENTER
Location is added to the PATRAN property set.
*SHELL GENERAL SECTION
A PATRAN property set is created.
*SHELL SECTION
A PATRAN property set is created.
438 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
ABAQUS Keyword *SOLID SECTION
Notes A PATRAN property set is created.
*SPECTRUM *SPECIFIC HEAT
Value is added to the PATRAN material.
*SPRING
A PATRAN property set is created.
*SURFACE DEFINITION
When referenced in a *CONTACT PAIR, this data is added to a contact-type LBC set.
*SURFACE INTERACTION The only keyword currently supported within this block is *FRICTION. The keyword parameters and friction data are added to the appropriate contact-type LBC set. *SYSTEM
PATRAN node locations are transformed to the coordinate system defined on this entry.
*TRANSFORM
A PATRAN coordinate frame is created and used to define the analysis system for the node.
*TRANSVERSE SHEAR STIFFNESS
The values are added to the appropriate PATRAN property set. History Section
Main Index
*BOUNDARY
A PATRAN LBC set is created for each ABAQUS BOUNDARY and added to the load case for this step. Displacement, temperature, velocity, and acceleration boundary conditions are currently supported.
*BUCKLE
The parameters associated with this entry are added to the PATRAN analysis step.
*CFLUX
A PATRAN LBC set is created for each ABAQUS CFLUX and added to the load case for this step.
*CLOAD
A PATRAN LBC set is created for each ABAQUS CLOAD and added to the load case for this step.
*DFLUX
A PATRAN LBC set is created for each ABAQUS DFLUX and added to the load case for this step.
*DLOAD
A PATRAN LBC set is created for each ABAQUS DLOAD and added to the load case for this step. The pressure DLOAD types as well as GRAV, CENT, CENTRIF, and CORIO are currently supported.
*DYNAMIC
The parameters associated with this entry are added to the PATRAN analysis step.
*FILM
A PATRAN LBC set is created for each ABAQUS FILM and added to the load case for this step.
*FREQUENCY
The parameters associated with this entry are added to the PATRAN analysis step.
Chapter 3 : Running Analysis 439 ABAQUS Input File Reader
ABAQUS Keyword
Notes
*HEAT TRANSFER
The parameters associated with this entry are added to the PATRAN analysis step.
*MODAL DYNAMIC
The parameters associated with this entry are added to the PATRAN analysis step.
*STATIC
The parameters associated with this entry are added to the PATRAN analysis step.
*STEADY STATE DYNAMICS
The parameters associated with this entry are added to the PATRAN analysis step.
*STEP
A PATRAN load case and an analysis job step are created for each ABAQUS step. The parameters on the *STEP entry are added to the analysis step
*TEMPERATURE
A PATRAN LBC set is created for each ABAQUS TEMPERATURE and added to the load case for this step.
*VISCO
The parameters associated with this entry are added to the PATRAN analysis step.
Both fixed format and free format entries are supported. The table below shows the PATRAN element property options that are created when a specific ABAQUS element type is imported. Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element
ABAQUS Element AC1D2 AC1D3 AC2D4 AC2D8 AC3D20 AC3D8 ACAX4 ACAX8 ASI1 ASI2 ASI2A ASI3
Dim 1D 1D 2D 2D 3D 3D 2D 2D 0D 1D 1D 2D
Name IRS (planar/axisym) ISL (in plane) Rigid Surface(LBC) 2D Interface Solid Solid Rigid Surface(LBC) 2D Interface IRS (single node) IRS (planar/axisym) IRS (planar/axisym) IRS (shell/solid)
ASI3A ASI4
2D 2D
Shell IRS (shell/solid)
Option1 Axisymmetric Axisymmetric
Option2 Elastic Slip Hard Contact Lagrange Soft Contact
Axisymmetric Homogeneous Homogeneous
Lagrange Vis Damping Standard Formulation Hybrid
Axisymmetric Planar Axisymmetric Axisymmetric Elastic Slip Hard Contact General Large Strain Lagrange Hard Contact
Lagrange Vis Damping Elas Slip Vis Damping Elastic Slip Hard Contact Elastic Slip Hard Contact
Homogeneous
440 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1 ABAQUS Element ASI8 B21 B21H B22 B22H B23 B23H B31 B31H B31OS B31OSH B32 B32H B32OS B32OSH B33 B33H B34 C1D2 C1D2H C1D2T C1D3 C1D3H C1D3T C3D10 C3D10E C3D10H C3D10M C3D10MH C3D15 C3D15E C3D15H C3D15V C3D15VH C3D20 C3D20E C3D20H C3D20HT C3D20P
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D
Name 2D Interface Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Beam in Space Truss Truss Truss Truss Truss Truss Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid
Option1 Axisymmetric General Section General Section General Section General Section General Section General Section General Section General Section Open Section Open Section General Section General Section Open Section Open Section General Section General Section General Section Standard Formulation Hybrid Hybrid Standard Formulation Hybrid Standard Formulation Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
Option2 Lagrange Vis Damping Standard Formulation Hybrid Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Hybrid Cubic Interpolation Cubic Hybrid Cubic Initially Straight
Standard Formulation Homogeneous Hybrid Modified Formulation Modified/Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Standard Formulation
Chapter 3 : Running Analysis 441 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element C3D20PH C3D20R C3D20RE C3D20RH
Dim 3D 3D 3D 3D
Solid Solid Solid Solid
Option1 Homogeneous Homogeneous Homogeneous Homogeneous
C3D20RHT C3D20RP C3D20RPH C3D20RT C3D20T C3D27 C3D27H C3D27R C3D27RH
3D 3D 3D 3D 3D 3D 3D 3D 3D
Solid Solid Solid Solid Solid Solid Solid Solid Solid
Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
C3D4 C3D4E C3D4H C3D6 C3D6E C3D6H C3D8 C3D8E C3D8H C3D8HT C3D8I C3D8IH
3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D 3D
Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid Solid
Homogeneous Standard Formulation Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
C3D8R C3D8RH
3D 3D
Solid Solid
Homogeneous Homogeneous
C3D8T CAX3 CAX3E CAX3H CAX4 CAX4E CAX4H CAX4HT
3D 2D 2D 2D 2D 2D 2D 2D
Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Homogeneous Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Name
Option2 Standard Formulation Reduced Integration Standard Formulation Hybrid/Reduced Integration Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Hybrid Hybrid Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation
442 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CAX4I CAX4IH
Dim 2D 2D
Name 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric
CAX4P CAX4PH CAX4R CAX4RH
2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAX4T CAX6 CAX6E CAX6H CAX6M CAX6MH CAX8 CAX8E CAX8H CAX8HT CAX8P CAX8PH CAX8R CAX8RE CAX8RH
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAX8RHT CAX8RP CAX8RPH CAX8RT CAX8T CAXA41 CAXA42 CAXA43 CAXA44 CAXA4H1 CAXA4H2 CAXA4H3 CAXA4H4 CAXA4R1 CAXA4R2
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Incompatible Modes Hybrid/Incompatible Modes Standard Formulation Standard Formulation Reduced Integration Hybrid/Reduced Integration Standard Formulation Standard Formulation Axisymmetric Hybrid Modified Formulation Modified/Hybrid Standard Formulation Hybrid Hybrid Hybrid Hybrid Hybrid Reduced Integration Hybrid Hybrid/Reduced Integration Hybrid Hybrid Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Hybrid Reduced Integration Reduced Integration
Chapter 3 : Running Analysis 443 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CAXA4R3 CAXA4R4 CAXA4RH1
Dim 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric Axisymmetric
CAXA4RH2
2D
2D Solid
Axisymmetric
CAXA4RH3
2D
2D Solid
Axisymmetric
CAXA4RH4
2D
2D Solid
Axisymmetric
CAXA81 CAXA82 CAXA83 CAXA84 CAXA8H1 CAXA8H2 CAXA8H3 CAXA8H4 CAXA8P1 CAXA8P2 CAXA8P3 CAXA8P4 CAXA8R1 CAXA8R2 CAXA8R3 CAXA8R4 CAXA8RH1
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CAXA8RH2
2D
2D Solid
Axisymmetric
CAXA8RH3
2D
2D Solid
Axisymmetric
CAXA8RH4
2D
2D Solid
Axisymmetric
CAXA8RP1 CAXA8RP2 CAXA8RP3 CAXA8RP4 CGAX3
2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Reduced Integration Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Hybrid Reduced Integration Reduced Integration Reduced Integration Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid/Reduced Integration Hybrid Hybrid Hybrid Hybrid Standard Formulation
444 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CGAX3H CGAX4 CGAX4H CGAX4I CGAX4IH
Dim 2D 2D 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Option1 Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CGAX4R CGAX4RH
2D 2D
2D Solid 2D Solid
Axisymmetric Axisymmetric
CGAX6 CGAX6H CGAX8 CGAX8H CGAX8R CGAX8RH
2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
CGPE10 CGPE10H CGPE10R CGPE10RH
2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid
General Plane Strain General Plane Strain General Plane Strain General Plane Strain
CGPE5 CGPE5H CGPE6 CGPE6H CGPE6I CGPE6IH
2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
General Plane Strain General Plane Strain General Plane Strain General Plane Strain General Plane Strain General Plane Strain
CGPE6R CGPE6RH
2D 2D
2D Solid 2D Solid
General Plane Strain General Plane Strain
CGPE8 CGPE8H
2D 2D
2D Solid 2D Solid
General Plane Strain General Plane Strain
Option2 Hybrid Standard Formulation Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Axisymmetric Hybrid Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid Standard Formulation Hybrid Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Standard Formulation Hybrid
Chapter 3 : Running Analysis 445 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CONN2D2
Dim 1D
Name Mech Joint (2D Model)
CONN3D2
1D
Mech Joint (3D Model)
CPE3 CPE3E CPE3H CPE4 CPE4E
2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Option1 ALIGN AXIAL BEAM CARTESIAN JOIN JOINTC LINK ROTATION SLOT TRANSLATOR WELD ALIGN AXIAL BEAM CARDAN CARTESIAN CONSTANT VELOCITY CVJOINT CYLINDRICAL EULER FLEXION-TORSION HINGE JOIN JOINTC LINK PLANAR RADIAL-THRUST REVOLUTE ROTATION SLIDE-PLANE SLOT TRANSLATOR UJOINT UNIVERSAL WELD Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain
Option2
Standard Formulation Plane Strain Hybrid Standard Formulation Reduced Integration
446 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CPE4H CPE4HT CPE4I CPE4IH
Dim 2D 2D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid
Option1 Plane Strain Plane Strain Plane Strain Plane Strain
CPE4R CPE4RH
2D 2D
2D Solid 2D Solid
Plane Strain Plane Strain
CPE4T CPE6 CPE6E CPE6H CPE8 CPE8E CPE8H CPE8HT CPE8P CPE8PH CPE8R CPE8RE CPE8RH
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain Plane Strain
CPE8RHT CPE8RP CPE8RPH
2D 2D 2D
2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Strain
CPE8RT CPE8T CPS3 CPS3E CPS4 CPS4E CPS4I CPS4R CPS4T CPS6 CPS6E CPS6M CPS8
2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D 2D
2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid
Plane Strain Plane Strain Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress
Option2 Hybrid Reduced Integration Incompatible Modes Hybrid/Incompatible Modes Reduced Integration Hybrid/Reduced Integration Reduced Integration Standard Formulation Standard Formulation Hybrid Standard Formulation Reduced Integration Hybrid Reduced Integration Standard Formulation Hybrid Reduced Integration Reduced Integration Hybrid/Reduced Integration Reduced Integration Reduced Integration Hybrid/Reduced Integration Reduced Integration Reduced Integration Standard Formulation Plane Stress Standard Formulation Reduced Integration Incompatible Modes Reduced Integration Reduced Integration Standard Formulation Standard Formulation Modified Formulation Standard Formulation
Chapter 3 : Running Analysis 447 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element CPS8E CPS8R CPS8RE CPS8RT CPS8T DASHPOT1 DASHPOT2 DASHPOTA DC1D2 DC1D2E DC1D3 DC1D3E DC2D3 DC2D4 DC2D6 DC2D8 DC3D10 DC3D15 DC3D20 DC3D4 DC3D6 DC3D8 DCAX3 DCAX4 DCAX6 DCAX8 DCC1D2 DCC1D2D DCC2D4 DCC2D4D
Dim 2D 2D 2D 2D 2D 0D 1D 1D 1D 1D 1D 1D 2D 2D 2D 2D 3D 3D 3D 3D 3D 3D 2D 2D 2D 2D 1D 1D 2D 2D
Name 2D Solid 2D Solid 2D Solid 2D Solid 2D Solid Grounded Damper Damper Damper Link Link Link Link 2D Solid 2D Solid 2D Solid 2D Solid Solid Solid Solid Solid Solid Solid 2D Solid 2D Solid 2D Solid 2D Solid IRS (planar/axisym) IRS (planar/axisym) 2D Solid 2D Solid
Option1 Plane Stress Plane Stress Plane Stress Plane Stress Plane Stress Linear Linear Linear
Option2 Standard Formulation Reduced Integration Standard Formulation Standard Formulation Standard Formulation
Planar Planar Planar Planar Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Planar Planar
Standard Formulation Standard Formulation Standard Formulation Standard Formulation
DCC3D8 DCC3D8D
3D 3D
Solid Solid
DCCAX2 DCCAX2D DCCAX4
1D 1D 2D
IRS (planar/axisym) IRS (planar/axisym) 2D Solid
Convection/Diffusion Convection/Diffusion with Dispersion Control Axisymmetric Axisymmetric Axisymmetric
Fixed Direction Standard Formulation
Standard Formulation Standard Formulation Standard Formulation Standard Formulation Elastic Slip Hard Contact Elastic Slip Hard Contact Convection/Diffusion Convection/Diffusion with Dispersion Control
Elastic Slip Hard Contact Elastic Slip Hard Contact Convection/Diffusion
448 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element DCCAX4D
Dim 2D
Name 2D Solid
DINTER1 DINTER2 DINTER2A DINTER3 DINTER3A DINTER4 DINTER8 DS4 DS8 DSAX1 DSAX2 ELBOW31
1D 2D 2D 2D 2D 3D 3D 2D 2D 1D 1D 1D
1D Interface 2D Interface 2D Interface 2D Interface 2D Interface 3D Interface 3D Interface Shell Shell Axisym Shell Axisym Shell Beam in Space
ELBOW31B
1D
Beam in Space
ELBOW31C
1D
Beam in Space
ELBOW32
1D
Beam in Space
F2D2 F3D3 F3D4 FAX2 FLINK GAPCYL GAPSPHER GAPUNI
1D 2D 2D 1D 1D 1D 1D 1D
IRS (planar/axisym) Shell Rigid Surface(LBC) IRS (planar/axisym) Link Gap Gap Gap
INTER1 INTER1P INTER1T INTER2
1D 1D 1D 2D
IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) IRS (shell/solid)
INTER2A INTER2AT INTER2T
2D 2D 2D
2D Interface 2D Interface IRS (shell/solid)
Option1 Axisymmetric
Planar Axisymmetric Planar Axisymmetric
Option2 Convection/Diffusion with Dispersion Control
Lagrange Vis Damping
Homogeneous Homogeneous Homogeneous Homogeneous Curved with Pipe Section Curved with Pipe Section Curved with Pipe Section Curved with Pipe Section Axisymmetric General Large Strain
Elastic Slip Hard Contact Homogeneous
Axisymmetric
Elastic Slip Hard Contact
Cylindrical Spherical Uniaxial
True Distance Elas Slip Vis Damping Lagrange Vis Damping No Sep Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact
Axisymmetric Axisymmetric Axisymmetric Lagrange Hard Contact Axisymmetric Axisymmetric Lagrange Hard Contact
Standard Formulation Ovalization Only Ovaliz Only with Approximated Fourier Standard Formulation
Lagrange Hard Contact Lagrange Hard Contact
Chapter 3 : Running Analysis 449 ABAQUS Input File Reader
Table 3-1
Main Index
PATRAN Property Options for Each ABAQUS Element (continued)
ABAQUS Element INTER3 INTER3A INTER3AP INTER3AT INTER3P INTER3T INTER4
Dim 2D 2D 2D 2D 2D 2D 3D
Name 2D Interface 2D Interface 2D Interface 2D Interface 2D Interface 2D Interface 3D Interface
INTER4T
3D
3D Interface
INTER8 INTER8T INTER9
3D 3D 3D
3D Interface 3D Interface 3D Interface
IRS12 IRS13 IRS21 IRS21A IRS22 IRS22A IRS3
0D 0D 1D 1D 1D 1D 2D
IRS (single node) IRS (single node) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane) IRS (shell/solid)
IRS31 IRS32 IRS4
1D 1D 2D
IRS (planar/axisym) ISL (in plane) IRS (shell/solid)
IRS9
2D
IRS (shell/solid)
ISL21 ISL21A ISL21AT ISL21T ISL22 ISL22A ISL22AT ISL31 ISL31A ISL32 ISL32A
1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D
IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane) ISL (in plane) IRS (planar/axisym) IRS (planar/axisym) ISL (in plane) ISL (in plane)
Option1 Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Lagrange Vis Damping Lagrange Vis Damping Elas Slip Vis Damping Elas Slip Vis Damping Lagrange Vis Damping Planar Planar Axisymmetric Axisymmetric Axisymmetric Axisymmetric Elastic Slip Hard Contact Axisymmetric Axisymmetric Lagrange Hard Contact Lagrange Hard Contact Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric Axisymmetric
Option2 Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping Lagrange Vis Damping
Elas Slip Vis Damping Elas Slip Vis Damping Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact
Elastic Slip Hard Contact Lagrange Soft Contact
Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact Lagrange Soft Contact Elastic Slip Hard Contact Elastic Slip Hard Contact Lagrange Soft Contact Lagrange Soft Contact
450 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Table 3-1 ABAQUS Element ISP1 ISP1T ISP3 ISP4 ISP4T JOINTC LS6 M3D3 M3D4 M3D4R M3D6 M3D8 M3D8R M3D9 M3D9R MASS MAX1 MAX2 MGAX1 MGAX2 PIPE21 PIPE21H PIPE22 PIPE22H PIPE31 PIPE31H PIPE32 PIPE32H R2D2 R3D3 R3D4 RAX2 RB2D2 RB3D2 ROTARYI S3 S3R S4 S4R
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 0D 0D 2D 2D 2D 1D 2D 2D 2D 2D 2D 2D 2D 2D 2D 0D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 2D 2D 1D 1D 1D 0D 2D 2D 2D 2D
Name IRS (single node) IRS (single node) Shell Shell Shell IRS (planar/axisym) Shell Membrane Membrane Membrane Membrane Membrane Membrane Membrane Membrane Mass IRS (planar/axisym) ISL (in plane) IRS (planar/axisym) ISL (in plane) Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in XY Plane Beam in Space Beam in Space IRS (planar/axisym) Rigid Surface(LBC) Rigid Surface(LBC) IRS (planar/axisym) Rigid Line(LBC) Rigid Line(LBC) Rotary Inertia Shell Shell Shell Shell
Option1 Planar Planar Thick General Large Strain General Large Strain Axisymmetric Thin Standard Formulation Standard Formulation Reduced Integration Standard Formulation Standard Formulation Reduced Integration Standard Formulation Reduced Integration
Option2 Elas Slip Vis Damping Elas Slip Vis Damping Homogeneous Homogeneous Homogeneous Elastic Slip Hard Contact Homogeneous
Axisymmetric Axisymmetric Axisymmetric Axisymmetric Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Pipe Section Axisymmetric
Elastic Slip Hard Contact Lagrange Soft Contact Elastic Slip Hard Contact Lagrange Soft Contact Standard Formulation Hybrid Standard Formulation Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Elastic Slip Hard Contact
Axisymmetric
Elastic Slip Hard Contact
Thick General Large Strain General Large Strain Thick
Homogeneous Homogeneous Homogeneous Homogeneous
Chapter 3 : Running Analysis 451 ABAQUS Input File Reader
Table 3-1 ABAQUS Element S4R5 S8R S8R5 S8RT S9R5 SAX1 SAX2 SAX2T SAXA11 SAXA12 SAXA13 SAXA14 SAXA21 SAXA22 SAXA23 SAXA24 SPRING1 SPRING2 SPRINGA STRI3 STRI35 STRI65 T2D2 T2D2E T2D2H T2D2T T2D3 T2D3E T2D3H T2D3T T3D2 T3D2E T3D2H T3D2T T3D3 T3D3E T3D3H T3D3T
Main Index
PATRAN Property Options for Each ABAQUS Element (continued) Dim 2D 2D 2D 2D 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 0D 1D 1D 2D 2D 2D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D 1D
Name Shell Shell Shell Shell Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Axisym Shell Grounded Spring Spring Spring Shell Shell Shell Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss Truss
Option1 Thin Thick Thin Thick Thin Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous Linear Linear Linear Thick Thin Thick Hybrid Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Standard Formulation Standard Formulation Standard Formulation Hybrid Hybrid Hybrid Standard Formulation Standard Formulation Hybrid Standard Formulation
Option2 Homogeneous Homogeneous Homogeneous Homogeneous Homogeneous
Fixed Direction Standard Formulation Homogeneous Homogeneous Homogeneous
452 Patran Interface to ABAQUS Preference Guide ABAQUS Input File Reader
Under some circumstances, the values of the option menus in Patran (Option 1 and Option 2) may be different than shown in the table. This is often the case when the ABAQUS element is one that is not directly supported by the Patran interface and the translator is making a “best guess” at which Patran element to choose. For many beam elements in the table, Option 1 is shown as “General Section”. Depending on the beam cross section type defined on the *BEAM SECTION or *BEAM GENERAL SECTION entry, Option 1 may be General Section, Box Section, Circular Section, Hexagonal Section, I Section, Pipe Section, Rectangular Section, or Trapezoid Section. For the 3D solid elements and shell elements in the table, Option 1 is shown as Homogeneous. Depending on the *SHELL SECTION or *SHELL GENERAL SECTION entry, Option 1 may be either Homogeneous or Laminate.
Main Index
Chapter 4: Read Results Patran Interface to ABAQUS preference Guide
4
Main Index
Read Results
Review of the Read Results Form
Translation Parameters
Select Results File
Data Translated from the Analysis Code Results File
Key Differences between Attach and Translate Methods
Delete Result Attachment Form
454
457
458
466
463 464
454 Patran Interface to ABAQUS preference Guide Review of the Read Results Form
Review of the Read Results Form By choosing the Analysis toggle located on the Patran main form, an Analysis form will appear.
Selecting Read Results as the Action on the Analysis form allows you to read results data into the Patran database from a text (“jobname”.fin) or binary (“jobname”.fil) ABAQUS results file, or to access ABAQUS results directly from an ABAQUS results output database (“jobname”.odb). Other forms that are accessible from here are used to define translation parameters and select the ABAQUS results file. These forms are described on the following pages.
Upgrading ABAQUS ODB Results Files Since the ABAQUS DRA in Patran is integrated with the ABAQUS 6.3-1 libraries, you must make sure your ODB results files have been upgraded to 6.3 before attempting to attach to them from within Patran. This can be done in one of two ways: Manually Upgrade ODB Files The procedure for upgrading ODB files is part of ABAQUS: abaqus upgrade job=job-name odb=old-odb-file-name Automatic Upgrade of ODB Files If you want to automatically upgrade your older ODB results files, you can set the following environment variable: Setenv ABAQUS_DRA_UPGRADE_ODB=YES By setting this variable, Patran will make a copy of the ODB results file and upgrade the copy to the current version of ABAQUS.
Main Index
Chapter 4: Read Results 455 Review of the Read Results Form
Read Results Form Read Results defines the type of data to be read from the analysis code results file into Patran. The Object box may only be set to Results Entities.
Main Index
456 Patran Interface to ABAQUS preference Guide Review of the Read Results Form
Flat File Results In some cases, the translation will not be able to write the data directly into the Patran database. In those cases, a text file will be created containing all the instructions as to how this data is to be loaded into the database. This file can be transferred between computers if necessary, then read into the proper database using the File Import functionality. The full functionality of this form is described in Working with Files (p. 45) in the Patran Reference Manual.
Main Index
Chapter 4: Read Results 457 Translation Parameters
Translation Parameters The Translation Parameters form is used to define filters for the data being accessed.
Attach Method There is only one filter control for the Attach method, which indicates whether or not to allow access to the results invariants, as calculated by Abaqus.
Translate and Control File Methods Translation parameters for the Translate and Control File methods include the results filtering options based on the step number and the increment number. If none of the options are specified, then all the results will be translated. If only step is specified, then all the increments in that step will be translated. If only increment is specified, then that increment for the first step will be translated. If both step and increment are specified, then only the increment for that step will be translated.
Main Index
458 Patran Interface to ABAQUS preference Guide Select Results File
Select Results File The Select file form allows you to select a file to be read. There are several features available. This form is brought up when you select the Select Results File button on the Read Results form. The default file filters will change depending on the Current analysis code in the Preferences menu.
Results Created in Patran For direct ODB access (Attach method), no results are created in Patran, and all result types represented within the field output data in the ODB file are available for postprocessing. The following table indicates all the possible results quantities which can be loaded into the Patran database during results translation (Translate method) from ABAQUS. The Primary and Secondary Labels are the items you select from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor. This determines which postprocessing techniques will be available to view this results quantity. Post Codes indicates which ABAQUS element post codes the data comes from. The Description gives a brief discussion about the results quantity. The Output Requests forms use the actual
Main Index
Chapter 4: Read Results 459 Select Results File
primary and secondary labels that will appear in the results. For example, if “Strain, Elastic” is selected on the Element Output Requests form, the “Strain, Elastic” is created for postprocessing. Table 4-1
Results Quantities Loaded into Patran During Translation
Primary Label Acceleration
Base Motion Change in Length Concentrated Flux (Nodal) Concentrated Deformation Displacements Elastic Strain Energy Density
Energy in Element
Total Energy
Force and Shear Force
Main Index
Secondary Label Generalized Rotational Generalized Translational Rotational Translational Rotational Translational Components Layer or Section Points Load Moment Displacements Rotations Generalized Displacements Generalized Rotations Components Artificial Strain Energy Creep Dissipation Plastic Dissipation Strain Energy Viscous Dissipation Artificial Strain Energy Creep Dissipation Kinetic Energy Plastic Dissipation Strain Energy Viscous Dissipation Total Artificial Strain Energy Total Creep Dissipation Total Energy Loss at Impact Total External Work Total Kinetic Total Plastic Dissipation Total Strain Total Viscous Dissipation Components
Type Vector Vector Vector Vector Vector Vector Tensor Scalar Vector Vector Vector Vector Vector Vector Tensor Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Scalar Tensor
Results Key 303 303 103 103 304 304 21 206 106 106 101 101 301 301 25 14 14 14 14 14 19 19 19 19 19 19 1999 1999 1999 1999 1999 1999 1999 1999 11
460 Patran Interface to ABAQUS preference Guide Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Force Frequency Heat Flux (Nodal) Heat Flux Inelastic Strain Internal Flux (Nodal) Internal Forces Mass Flux Modal
Mag-Phase Strain Mag-Phase Stress Phase Angle
Mag-Phase Reaction Mag-Phase Reaction Mag-Phase Displacements Mag-Phase Acceleration Mag-Phase Velocity Mag-Phase Displacements Mag-Phase Velocity Mag-Phase Total Displacement Mag-Phase Total Acceleration Mag-Phase Total Velocity Mag-Phase Total Displacement Mag-Phase Total Acceleration
Main Index
Secondary Label Components Steady State Dynamics Components Components Magnitude Components Layer or Section Points Components at Element Node Components Magnitude Composite Damping Effective Mass Eigen Values Generalized Mass Participation Factor Components Components Generalized Displacements Generalized Rotational Acceleration Generalized Rotational Velocities Generalized Rotations Generalized Translational Accelerations Generalized Translational Velocities Force Moment Displacements Rotational Rotational Rotations Translational Translational
Type Tensor Scalar Vector Vector Scalar Tensor Scalar Vector Vector Scalar Scalar Scalar Scalar Scalar Scalar Tensor Tensor Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector
Results Key 11 2000 10 28 28 24 214 15 39 39 1980 1980 1980 1980 1980 65 62 305 307 306 305 307 306 135 135 111 137 136 111 136 112
Rotational
Vector
140
Rotational Rotational
Vector Vector
139 112
Translational
Vector
140
Chapter 4: Read Results 461 Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Mag-Phase Total Velocity Mag-Phase Acceleration Plastic Strain
Pressure and Shear Stresses RMS Strain RMS Stress Reaction Relative Displacements and Shear Slips Rel. Normal & Tangential Displacements Residual Flux (Nodal) Root Mean Square
Strain
Main Index
Secondary Label Translational Translational Components Equivalent Magnitude Yield Flag Components
Type Vector Vector Tensor Scalar Scalar Scalar Tensor
Results Key 139 137 22 22 22 22 11
Components Components Force Moment Components
Tensor Tensor Vector Vector Tensor
66 63 104 104 21
Components
Tensor
21
Layer and Section Points Reaction Forces Reaction Moments Relative Displacements Relative Rotational Accelerations Relative Rotational Velocities Relative Rotations Relative Translational Velocities Total Displacements Total Rotational Accelerations Total Rotational Velocities Total Rotations Total Translational Accelerations Total Translational Velocities Relative Translational Accelerations Components
Scalar Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Vector Tensor
204 134 134 123 131 127 123 127 124 132 128 124 132 128 131 21
462 Patran Interface to ABAQUS preference Guide Select Results File
Table 4-1
Results Quantities Loaded into Patran During Translation (continued)
Primary Label Stress
Temperature (Nodal) Temperature Total Acceleration Total Displacement Total Velocity Total
Velocity
Creep Strain
Main Index
Secondary Label 1st Principal 2nd Principal 3rd Principal 3rd Stress Invariant Components Hydrostatic Pressure Maximum Stress in Section Mises Tresca Layer or Section Points Element Centroidal Temperature Rotational Translational Rotational Translational Rotational Translational Creep Time Dynamic Time Heat Transfer Time Soils Time Time Generalized Rotational Generalized Translational Rotational Translational Components Equivalent Magnitude Yield Flag
Type Scalar Scalar Scalar Scalar Tensor Scalar Scalar Scalar Scalar Scalar Scalar Vector Vector Vector Vector Vector Vector Scalar Scalar Scalar Scalar Scalar Vector Vector Vector Vector Tensor Scalar Scalar Scalar
Results Key 12 12 12 12 11 12 16 12 12 201 2 115 115 113 113 114 114 2000 2000 2000 2000 2000 302 302 102 102 23 23 23 23
Chapter 4: Read Results 463 Data Translated from the Analysis Code Results File
Data Translated from the Analysis Code Results File When reading model data from an ABAQUS results file, the following table defines all the data which will be created. No other model data is extracted from the results file. This data should be sufficient for evaluating any results values.
Item Nodes
Results Key 1901
Description Node ID Nodal Coordinates
Elements
1900
Element ID Nodal Connectivity
Groups
n/a, ODB access only
Group name Node and Element references Groups are generated for each part instance, as well as for each node and element set.
Main Index
464 Patran Interface to ABAQUS preference Guide Key Differences between Attach and Translate Methods
Key Differences between Attach and Translate Methods The most obvious difference between direct ODB access (Attach method) and results translation (Translate method) is that the results are not imported into the Patran database in the case of the former, while they are for the latter. Direct access avoids redundancy and saves disk space, while Translation uses more disk space, but takes less time to retrieve results for postprocessing. The following sections describe other differences that users should be aware of, before deciding which method to use.
Result Type Naming Conventions The names used for the result types within an ODB attachment come directly from the field output description fields of the ODB database. Using the “direct access” philosophy of bringing the data in asis, there is no attempt to map those names to the same names used by the Translate method (listed in Table 4-1). Therefore, direct ODB access will use Abaqus terminology exclusively in generating the result type names. The primary name is equal to the field output description field, while the secondary name is the field output key. For example, the stress tensor result type is “Stress components, S”, where “Stress components” is the field output description, and “S” is the field output key.
Vector vs. Scalar Moment and Rotational Results For results such as reaction moments or rotational displacements, the ODB database saves space by only storing results for the non-zero component, whenever possible. So, if non-zero values for moments only occur in the Z component, then the ODB database stores it as a scalar result (e.g. key RM3). However, the Translate method will import the results as vector results, with the X and Y values always being zero. This difference may cause confusion when comparing translated results against direct ODB access via the quick or fringe plot operations, where reaction moments and rotational displacements are concerned. The default “invariant” for fringe plots of vector data is “Magnitude”, which is always a positive value. If the magnitude of the translated vector data is compared against the ODB scalar data, then they will not always match (all negative data from the ODB access will be flipped positive in the translated plot). To compare “apples with apples”, one must display the appropriate component (Z from our example) from the translated case, and compare that against the scalar (key RM3) from the direct ODB access case.
Main Index
Chapter 4: Read Results 465 Key Differences between Attach and Translate Methods
Reaction Forces During translation, only non-zero reaction force data is imported. Direct ODB access, on the other hand, returns zero vectors for any nodes that do not have any reaction forces. This makes no difference for the display of reaction force vectors; however, if one displays a fringe plot distribution of the reaction forces, the fringe plots vary between translation and direct ODB access dramatically. The translation plot is all black, with only the min/max values displayed on a hidden line plot; while the ODB fringe plot shows a color distribution from the zero values (white over most of the model) to the non-zero values. For the latter, the contours only vary over elements with nodes having non-zero reaction forces.
Main Index
466 Patran Interface to ABAQUS preference Guide Delete Result Attachment Form
Delete Result Attachment Form The following form may be used to remove a results attachment, created via the Attach method, from the database.
Main Index
Chapter 5 : Files Patran Interface to ABAQUS Preference Guide
5
Files
Main Index
Files
468
468 Patran Interface to ABAQUS Preference Guide Files
Files There are several files associated which are either used or created by the Patran ABAQUS Application Preference. The following table describes each file and how it is used. In the definition of the file names, any occurrence of “jobname” would be replaced with the jobname the user assigns.
File Name
Main Index
Description
jobname.db
This is the Patran database from which the model data is read during an analyze pass, and into which model and⁄or results data is written during a Read Results pass.
jobname.jbm jobname.jbr
These are small files used to pass certain information between Patran and the Application Preference during translation. You should never have need to do anything directly with these files.
jobname.inp
This is the ABAQUS input file created by the interface.
jobname.fil
This is the ABAQUS results file which is read by the Read Results pass.
jobname.flat
This file may be generated during a Read Results pass. If the results translation cannot, for any reason, write data directly into the jobname.db Patran database, it will create this jobname.flat file.
jobname.msg
These message files contain any diagnostic output from the translation, either forward or reverse.
AbaqusExecute
This is a UNIX script file which is called on to submit both the forward PAT3ABA translation program, as well as to submit ABAQUS after translation is complete. This file should be customized for your particular site installation.
ResultsSubmit
This is another UNIX script which is called on to submit the reverse, ABAPAT3 translation program. This file should also be customized for your particular site.
load_abaqus.ses
This file is only used when creating a new Patran template database. This file loads in all the element, material, MPCs and loads and boundary condition tables for the Patran ABAQUS product.
Chapter 6 : Errors/Warnings Patran Intreface to ABAQUS Preference Guide
6
Errors/Warnings
Main Index
Errors/Warnings
470
470 Patran Intreface to ABAQUS Preference Guide Errors/Warnings
Errors/Warnings There are several error or warning messages which may be generated by the Patran ABAQUS Application Preference.
Message
Main Index
Description
Fatal
This error stops the translation and exits the Preference.
Warning
Some expected action did not execute. Translation continues. Check the .msg file.
Information
General Messages about the translation.
jp`Kc~íáÖìÉ=nìáÅâ=pí~êí=dìáÇÉ
Index Patran Interface to ABAQUS Preference Guide få Ç É ñ= Index
Numerics 1D interface, 96, 104, 151 2D interface, 101, 104 2D orthotropic, 81 2D orthotropic lamina, 54 2D solid, 100, 104 3D anisotropic, 56, 84 3D anisotropic thermal, 88 3D interface, 103, 105, 312 3D orthotropic, 55, 82 3D orthotropic thermal, 87
A abapat3, 4 ABAQUS, 3 abaqus.plb, 4, 5 AbaqusExecute, 468 AbaqusSubmit, 5, 7 acceleration, 334, 340 Acommand, 7 amplitude, 14 analysis, 354 arbitrary beam, 127 area moment I12, 126 average shear stiffness, 254 axisymmetric 2D interface, 279 axisymmetric ISL, 156 axisymmetric shell, 95, 104, 148 laminate, 149 axisymmetric solid, 273
B base motion, 15, 388
Main Index
beam, 28, 32 circular, 122 cross-sectional shape, 122 elements, 16, 17, 18 general section, 11, 117, 125 hexagonal, 122 in space, 93 in XY plane, 92 section, 11 bifurcation buckling, 365, 373, 374 bilinear, 28, 36 boundary, 14, 15 box beam, 119 buckle, 15
C C biquad, 29, 39 cap hardening, 13, 78 plasticity, 13 centrifugal force, 339 centroid, 11 centroid coordinate, 126 CETOL, 418 CFLUX, 15 change material status, 52 circular beam, 122 solid, 122 clearance zero damping, 114, 117, 153 clearance zero-pressure, 114, 117, 153 CLOAD, 15 combined creep test data, 71 combined test data, 13 composite, 56, 88, 319 conductivity, 13 constitutive models, 52 control, 104 convection, 104, 334, 348 convection/diffusion, 320, 323
472 Patran Interface to ABAQUS Preference Guide
coordinate frames, 22 Coriolis force, 339 correlation, 15 creep, 13, 54, 55, 56, 79, 80, 367, 417, 418 creep test data, 71 cubic hybrid, 92, 93 cubic initially straight, 93 cubic interpolation, 92, 93 curved pipe, 130
D damper, 94 damping, 13 direct, 387 Rayleigh, 388 zero clearance, 114, 117, 153 dashpot, 12 elements, 19 DASHPOT1, 110 DASHPOT2, 142, 144 DASHPOTA, 141, 143 deformation plasticity, 13, 54, 73 degree-of-freedom, 30 density, 13, 67, 88 DFLUX, 15 diffusion, 104 direct linear transient, 365, 376, 377 direct steady state dynamics, 365, 380 direct text input, 360, 363 dispersion, 104 displacement, 334, 337 DLOAD, 15 Drucker-Prager, 13, 77 dynamic, 15
E eigenvalue, 364 eigenvalue buckling, 365 EL file, 16, 362 print, 16, 362 elastic, 13, 53, 54, 55, 56, 58, 81, 82, 83 elastic slip, 113, 116, 152, 154, 157, 160, 162,
Main Index
165, 168, 170, 278, 280, 282, 314 hard contact, 92 no separation, 92 soft contact, 92 vis damping, 92 vis damping no separation, 92 elbow, 29, 42 elements, 19 MPC, 42 ELBOW31, 42, 130 ELBOW31B, 130 ELBOW32, 42, 130 element, 11, 25 definition, 11 matrix output, 16, 362 properties, 90 elements beam, 16, 17, 18 dashpot, 19 elbow, 19 gap, 20 heat transfer, 20, 21 mass, 19 membrane, 18 rigid surface contact, 20 rotary inertia, 19 shell, 19 slide line contact, 20 small sliding contact, 20 spring, 19 ELSET, 11, 352 end step, 15 energy file, 16, 362 print, 16, 362 engineering constants, 82 equation, 14, 28, 31 expansion, 13, 67 explicit, 28
F fatal, 470
INDEX
file EL, 16, 362 energy, 16, 362 format, 16, 362 modal, 16, 362 node, 16, 362 output definition, 16 film, 15 finite elements, 23 flat file results, 456 force, 334, 337 Frac Clearance Const Damping, 114, 117, 153 fraction of critical damping, 59 frequency, 15, 394 friction, 12, 112 Friction in Dir_1, 113, 116 Friction in Dir_2, 116
G gap, 12, 95 conductance, 12, 317, 324 cylindrical, 145 elements, 20 radiation, 12, 317, 324 spherical, 147 uniaxial, 145 GAPCYL, 146 GAPSPHER, 147 GAPUNI, 146 general beam, 117, 124 general large strain, 266 general thick, 262 general thick shell laminated, 264 general thin, 258 general thin shell laminated, 261 gravity loads, 339 grounded damper, 92 grounded spring, 92 group, 352
H HAFTOL, 412, 413 hard contact, 114, 117, 153, 155, 158, 160, 163,
Main Index
166, 169, 171, 278, 281, 283, 314 harmonic loading, 365 heat flux, 334, 349 heat source, 334, 349 heat transfer, 15 elements, 20, 21 hexagonal beam, 122 Hilber-Hughes-Taylor operator, 365 host, 7 hourglass stiffness, 12, 255 bending, 254, 257, 260, 263, 266, 269 membrane, 254, 257, 260, 263, 266, 269 normal, 254, 257, 260, 263, 266, 269 hybrid, 92, 93, 100, 269, 310 integration, 100 modes, 100 hyperbolic, 80 hyperelastic, 13, 53, 60, 61, 62, 63, 64, 65, 66, 68 hyperfoam, 13, 67
I import input file, 433 incompatible modes, 100, 269, 270, 272, 273, 274, 310 inertia rotary, 12 inertial load, 334, 339 information, 470 initial conditions, 14 initial temperature, 334, 350 initial velocity, 334, 339 input data, 334 interface, 12, 112 IRS, 97, 102, 112, 115 axisymmetric, 167 beam/pipe, 169 planar, 164 shell/solid, 281 single node, 92 IRS12, 112 IRS13, 115 I-section, 123 ISL, 96, 97
473
474 Patran Interface to ABAQUS Preference Guide
isotropic, 53, 58, 75 thermal, 86
J jobname.db, 468
K kinematic, 76 constraints, 14
L Lagrange hard contact, 92 no separation, 92 soft contact, 92 vis damping, 92 vis damping no separation, 92 Lamina, 81 laminate, 56, 89 large strain, 265 latent heat, 13 linear, 28, 34 linear damper, 109, 141, 142 grounded, 109 linear spring, 108, 137, 138 grounded, 108 linear static, 364, 368, 369 linear surf-surf, 28 linear surf-surf MPC, 34 linear surf-vol, 28 linear surf-vol MPC, 34, 35 linear vol-vol, 28 linear vol-vol MPC, 36 link, 28, 33, 104 load cases, 351, 362 loading definition, 15 loads and boundary conditions, 332 L-section beam, 132
M mass, 12, 92, 106 elements, 19 mass proportional damping, 59
material, 13 change status, 52 definition, 13 orientation, 14 temperature dependent, 53 materials, 51 form, 52 maximum friction stress, 114, 117, 152 maximum negative pressure, 114, 117, 153 maximum overclosure, 114, 117, 153 membrane, 101, 275 elements, 18 Mises/Hill, 74, 75, 76 modal damping, 15 dynamic, 15 file, 16, 362 print, 16, 362 steady state dynamics, 365 modal linear transient, 365, 383, 384 modified Drucker-Prager/Cap, 78 Moony Rivlin, 62 MPC, 14 elbow, 42 explicit, 31 linear surf-surf, 34 linear surf-vol, 34, 35 linear vol-vol, 36 pin, 43 quad surf-surf, 37 quad surf-vol, 37, 38 quad vol-vol, 39 revolute, 44 rigid fixed, 32 rigid pinned, 33 slider, 40 SS bilinear, 48 SS linear, 47 SSF bilinear, 49 tie, 43 universal, 47 V Local, 46 multi-point constraints, 27
N natural frequency, 364, 371
Main Index
INDEX
Neo Hookean, 62 Newton’s method, 366 no compression, 13 no sliding contact, 114, 117, 153 no tension, 13 node, 11, 23 definition, 11 file, 16, 362 print, 16, 362 nondeterministic continuous excitation, 366 nonlinear damper, 110, 143, 144 grounded, 110 nonlinear spring, 109, 139, 140 grounded, 109 nonlinear static, 366, 407, 409 nonlinear transient dynamic, 367, 412, 414 NSET, 11, 23, 352
O object tables, 336 Ogden, 60, 61, 63, 64, 66, 68 open beam, 134 optional controls, 359 orientation, 14, 22, 89 system, 253 output requests, 362
P parallel ISL, 158 pat3aba, 4 peak response, 366 perfect plasticity, 74 pin, 43 pin MPC, 43 pipe beam, 123 planar 2D interface, 277 ISL, 153 test data, 13 plane strain, 269, 270 plane stress, 272 plastic, 13, 54, 55, 56, 74, 75, 76, 77, 78 point mass, 106 Poisson parameter, 118, 121, 126, 128, 133, 136
Main Index
Poisson’s ratio, 67 polynomial, 60, 62, 63, 65 potential, 13 power spectral density, 403 preferences, 10 analysis, 10 preprint, 16 prescribed boundary conditions, 15 pressure, 334, 337 pressure zero clearance, 114, 117, 153 pre-tension, 347 print, 16, 362 definition, 16 EL, 16, 362 energy, 16, 362 modal, 16, 362 node, 16, 362 procedure definition, 15 Prony, 70, 367 property definition, 11 PSD-Definition, 14
Q quad surf-surf, 29 quad surf-surf MPC, 37 quad surf-vol, 29 quad surf-vol MPC, 37, 38 quad vol-vol, 29 quad vol-vol MPC, 39 quadratic, 29, 37
R radial ISL, 161 random response, 15 random vibration, 366, 402, 403, 404 rate dependent, 13 read input file, 433 read results, 454, 455 read temperature file, 368 rebar 2D, 285 rectangular beam, 124 reduced integration, 100, 269, 270, 272, 273, 274, 275, 310 reference temperature, 59 relaxation test data, 72
475
476 Patran Interface to ABAQUS Preference Guide
response spectrum, 15, 366, 394, 395, 396, 397 restart, 14 restart parameters, 358 results file select, 458 ResultsSubmit, 5, 468 revolute, 29, 44 revolute MPC, 44 rigid fixed, 28 pinned, 28 rigid fixed MPC, 32 rigid line, 98 LBC, 175 rigid pinned MPC, 33 rigid surf, 98, 102 rigid surface, 11, 112, 115, 165, 167, 170, 171, 172, 174, 175, 281, 283 axisymmetric, 173 Bezier 2D, 174 Bezier 3D, 283 cylindrical, 172 LBC, 284 segments, 171 rigid surface contact elements, 20 ROTARI, 107 rotary inertia, 12, 92, 107 elements, 19 rough (no slip) friction, 114, 117, 153, 155, 158, 160, 163, 166, 169, 278, 281, 283, 314 rough parameter, 171
S Scratchdir, 7 section point coordinate, 126 shear centroid coordinate, 126 shear factor, 118, 121, 126, 129, 134, 136 shear test data, 13 shell, 100, 104 elements, 19 general section, 12, 262 section, 12, 255 simple shear test data, 14 slide line, 11, 97, 163
Main Index
slide line contact elements, 20 slider, 29, 40 slider MPC, 40 sliding friction, 113, 154, 157, 159, 162, 165, 168, 170, 282 slip tolerance, 113, 116, 152 small sliding contact elements, 20 soft contact, 114, 117, 153, 155, 158, 160, 163, 166, 169, 171, 278, 280, 283, 314 solid, 103, 105, 310 solid section, 12 solution types, 364 specific heat, 14, 88 spectrum, 14 spring, 12, 94 elements, 19 SPRING1, 108, 109 SPRING2, 138, 140 SPRINGA, 137, 139 SS bilinear, 29, 30, 38, 48 SS bilinear MPC, 48 SS linear, 28, 30, 35, 47 SS linear MPC, 47 SSF bilinear, 30, 49 SSF bilinear MPC, 49 standard formulation, 92, 93, 100, 104 static, 15, 334 steady state dynamics, 15, 389, 390 steady state heat transfer, 367, 428 steady state response, 365 step, 15 creation, 361 initialization, 15 selection, 432 termination, 15 stiffness hourglass, 12 transverse shear, 13 stiffness in stick, 113, 117, 152 stiffness proportional damping, 59 strain, 79 surface contact, 12, 279
INDEX
T tabular formula, 69 tangent elastic moduli, 364 TAUMAX, 152, 155, 158, 160, 163, 166, 169, 171, 278, 280, 283, 314 temperature, 15, 334, 338 thermal, 334, 348 temperature dependent material, 53 test data combined, 13 creep, 71 creep combined, 71 Ogden, 66 planar, 13 relaxation, 72 shear, 13 simple shear, 14 uniaxial, 14 volumetric, 14 thermal 1D interface, 317 thermal axisymmetric shell, 315 laminated, 316 thermal expansion coefficient, 59, 67 thermal interface planar, 321 solid, 324 thermal link, 314 thermal planar solid, 320 thermal shell, 318 laminated, 319 thermal solid, 323 thermal strain, 59 thick shell, 255 laminated, 257 thin shell, 252 laminated, 254 tie, 29, 43 tie MPC, 43 time, 79 time dependent loading, 365 torsional constant, 126, 135 transform, 11, 22 transient, 335 transient heat transfer, 367, 430 translation parameters, 357, 457
Main Index
transverse shear stiffness, 13, 122, 125, 127 trapezoid beam, 124 true distance, 95 truss, 94, 136
U uniaxial test data, 14 universal, 30, 47 universal MPC, 47
V V Local, 29, 46 V Local MPC, 46 velocity, 334, 340 VISCO, 15, 417 viscoelastic, 14, 54, 55, 56, 69, 70, 71, 72 frequency domain, 367, 425 time domain, 367, 421, 422 volumetric pressure, 67 volumetric test data, 14, 67
W warning, 470 warping constant, 136 wavefront minimization, 14
X XY plane definition, 126, 128
Y yield, 14
477
478 Patran Interface to ABAQUS Preference Guide
Main Index
Related Documents
More Documents from "Kevin"
Resumen De La Exposicion De Regimen.docx
November 2019 7
What Is Hiv Lbl F.docx
May 2020 4
Centrobiblia
May 2020 1