Patran 2008 R1 Interface To Abaqus Preference Guide

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