Patran 2008 R1 Interface To Msc Nastran Preference Guide Volume 1: Structural Analysis
This document was uploaded by user and they confirmed that they have the permission to share it. If you are author or own the copyright of this book, please report to us by using this DMCA report form. Report DMCA
Overview
Download & View Patran 2008 R1 Interface To Msc Nastran Preference Guide Volume 1: Structural Analysis as PDF for free.
More details
- Words: 112,638
- Pages: 588
Patran 2008 r2 Interface To MSC Nastran Preference Guide Volume 1: Structural Analysis
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 2009 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*2008R2*Z*INT-NA*Z* DC-USR
Contents Patran Interface to MD Nastran Preference Guide
Patran Interface MD Nastran Pre ence Guide,
1
Overview Purpose 2 Using Patran with SOL 700
2
MD Nastran Product Information
2
3
Building A Model Introduction to Building a Model
6
Currently Supported MD Nastran Input Options MD Nastran Implicit Nonlinear (SOL 600) 14 MD Nastran Explicit Nonlinear (SOL 700) 15 Materials 15 Loads and Boundary Conditions 17 Elements and Properties 17 Solution Controls 17
8
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference 18 Element Creation 18 Element and p-Formulation Properties 19 Loads and Boundary Conditions 19 Analysis Definition 20 Results Import and Postprocessing 20 Potential Pitfalls 21 Adaptive Analysis of Existing Models 21 Coordinate Frames
22
Finite Elements 23 Nodes 23 Elements 24 Multi-point Constraints 27 MPC Types 28 Degrees of Freedom 31 Superelements 56
ii Patran Interface to MD Nastran Preference Guide
Select Boundary Nodes 58 Material Library 59 Materials Application Form 59 Material Input Properties Form 61 Material Constitutive Models 62 Linear Elastic 73 Nonlinear Elastic 74 Hyperelastic 75 Elastoplastic 78 Failure 81 Failure 1, Failure 2, Failure 3 82 Creep 84 Viscoelastic 85 Composite 85 Element Properties 87 Element Properties Form 87 Coupled Point Mass (CONM1) 91 Grounded Scalar Mass (CMASS1) 93 Lumped Point Mass (CONM2) 94 Grounded Scalar Spring (CELAS1/CELAS1D) 96 Grounded Scalar Damper (CDAMP1/CDAMP1D) 98 Bush 99 General Section Beam (CBAR) 102 P-Formulation General Beam (CBEAM) 107 Curved General Section Beam (CBEND) 110 Curved Pipe Section Beam (CBEND) 113 Lumped Area Beam (CBEAM/PBCOMP) 115 Tapered Beam (CBEAM) 119 General Section Beam (CBEAM) 124 General Section Rod (CROD) 131 General Section Rod (CONROD) 134 Pipe Section Rod (CTUBE) 136 Scalar Spring (CELAS1/CELAS1D) 137 Scalar Damper (CDAMP1/CDAMP1D) 139 Viscous Damper (CVISC) 141 Gap (CGAP) 142 Scalar Mass (CMASS1) 144 PLOTEL 146 (Scalar) Bush 146 Spot Weld Connector (CWELD) 150 Fastener Connector (CFAST) 152 Standard Homogeneous Plate (CQUAD4) 155 Revised Homogeneous Plate (CQUADR) 158
CONTENTS iii
P-Formulation Homogeneous Plate (CQUAD4) 161 Standard Laminate Plate (CQUAD4/PCOMP) 163 Revised Laminate Plate (CQUADR/PCOMP) 166 Standard Equivalent Section Plate (CQUAD4) 168 Revised Equivalent Section Plate (CQUADR) 171 P-Formulation Equivalent Section Plate (CQUAD4) 174 Field Point Mesh (CQUAD4/TRIA3)(Exterior Acoustics) 177 Standard Bending Panel (CQUAD4) 179 Revised Bending Panel (CQUADR) 181 P-Formulation Bending Panel (CQUAD4) 183 Standard Axisymmetric Solid (CTRIAX6) 186 PLPLANE Axisymmetric Solid (CTRIAX, CQUADX) 187 2D Axi-Symmetric Laminated Solid Composite 188 Standard Plane Strain Solid (CQUAD4) 190 Revised Plane Strain Solid (CQUADR) 191 P-Formulation Plane Strain Solid (CQUAD4) 193 Infinite (Exterior Acoustic Element)(CACINF3/CACINF4) 195 2D Plane Strain Laminated Solid Composite 196 Standard Membrane (CQUAD4) 197 Revised Membrane (CQUADR) 199 P-Formulation Membrane (CQUAD4) 201 Shear Panel (CSHEAR) 204 Solid (CHEXA) 206 P-Formulation Solid (CHEXA) 209 Hyperelastic Plane Strain Solid (CQUAD4) 211 Hyperelastic Axisym Solid (CTRIAX6) 212 Hyperelastic Solid (CHEXA) 214 3D Laminate Solid (CHEXA) 215 Beam Modeling 217 Cross Section Definition 217 Create Action 217 Supplied Functions 219 Cross Section Orientation 220 Cross Section End Offsets 222 Stiffened Cylinder Example 222 Loads and Boundary Conditions 224 Loads & Boundary Conditions Form 224 Object Tables 231 Preview Rigid Body Motion 239 Slideline (SOL 400 and SOL 600) 240 Deformable Body (SOL 400, SOL 600, and SOL 700 ) 241 Select Discontinuities Subform 241
iv Patran Interface to MD Nastran Preference Guide
Edge Contact Subform 242 Select Contact Area 242 Select Exclusion Region 242 Select Deactivation Region 242 Rigid Body (SOL 600 and SOL 700 only) 243 Load Cases
246
Defining Contact Regions Contact 249
247
Rotor Dynamics 250 Rotor Dynamics Form 251 Spin Profile Form 252 Spin History Form 252 Unbalance Form 253 Unbalance Properties Form 255
3
Running an Analysis Review of the Analysis Form 260 Analysis Form 261 Overview of Analysis Job Definition and Submittal Translation Parameters 265 External Superelement Specifications Numbering Options 268 Select File 270 Solution Types Direct Text Input
271 276
Solution Parameters 277 Linear Static 277 Nonlinear Static 279 Normal Modes 282 Buckling 287 Complex Eigenvalue 291 Frequency Response 296 Transient Response 299 Nonlinear Transient 302 Implicit Nonlinear 304 Solver Options Subform (SOL 600) 306 Contact Parameters Subform 307
268
263
CONTENTS v
Restart Parameters Subform 315 Advanced Job Control Subform (SOL 600) 317 Domain Decomposition 318 DDAM 321 DDAM in Patran 322 Explicit Nonlinear 326 Sol700 Parameters Subform 327 Hourglass Setting Subform 329 Merge Rigid Material Subform 331 Dynamic Relaxation for Restart Subform 333 Damping Per Property Subform 335 Rigid Body Switch and Merge Subform 337 Define Set of Parts to be Switched Subform 340 Define Inertial Properties of Rigid Body Subform 342 Eulerian Parameters Subform 343 SPH Control Parameters Subform 346 Results Output Format 348 ADAMS Preparation 350 Select Superelements Subcases 354 Deleting Subcases Editing Subcases
352 355 356
Subcase Parameters 357 Linear Static Subcase Parameters 358 Nonlinear Static Subcase Parameters 359 Arc-Length Method Parameters 361 Nonlinear Transient Subcase Parameters 362 Normal Modes Subcase Parameters 364 Complex Eigenvalue Subcase Parameters 366 Transient Response Subcase Parameters 367 Frequency Response Subcase Parameters 370 Implicit Nonlinear Subcase Parameters 375 Static Subcase Parameters for Implicit Nonlinear Solution Type 376 Implicit Nonlinear Normal Modes Subcase Parameters 377 Implicit Nonlinear Buckling Subcase Parameters 377 Implicit Nonlinear Transient Dynamic Subcase Parameters 378 Implicit Nonlinear Creep Subcase Parameters 380 Implicit Nonlinear Body Approach Subcase Parameters 381 Implicit Nonlinear Complex Eigenvalue Subcase Parameters 382 Load Increment Parameters 383 Iteration Parameters 391 Contact Table 396
vi Patran Interface to MD Nastran Preference Guide
Breaking Glue Parameters Subform 400 Edge Contact Subform 401 402 Active/Deactive Elements 402 Break Squeal Parameters 403 Solvers/Options 404 DDAM Subcase Parameters 407 Explicit Nonlinear Subcase Parameters 409 Contact Table 411 Additional Contact Data 412 Adaptive Mesh Post-Processing 413 Additional Information 413 Output Requests 415 Basic Output Requests 416 Advanced Output Requests 417 Edit Output Requests Form 426 Default Output Request Information Subcases Direct Text Input 432 SOL 600 Output Requests 433 DDAM Output Requests 439 Mode by Mode Output 440 Select Explicit MPCs...
444
Non-Structural Mass Properties Select NSM Properties... Subcase Select
428
445
450
452
Restart Parameters
455
Optimize 463 Optimization Parameters 467 Subcases 471 Subcase Parameters 474 Subcase Select Optimize 475 Customized Solutions (Topology Optimization) Design Domain 479 Objectives & Constraints 479 Optimization Control 479 Postprocessing 479 Interactive Analysis Assumptions 480
480
476
CONTENTS vii
Scenario 1 480 Scenario 2 480 The Process 481 Miscellaneous 481 Analysis Form 482 Select Modal Results .DBALL 484 Loading Form 484 Create a Field Form 488 Output Selection Form 489 Define Frequencies Form 490
4
Read Results Accessing Results 492 Results File Formats 493 Output2 Formats 493 XDB Formats 493 MASTER Formats 494 T16/T19 Formats 495 3dplot Formats 495 Translation Parameters 496 OUTPUT2 496 Defining Translation Parameters for DDAM (SOL 187) 497 XDB 498 MASTER 499 T16/T19 501 Supported OUTPUT2 Result and Model Quantities Results 502 Global Variables 508 Coordinate Systems 509 Projected Global System 509 XY Plots 509 Model Data 510 Supported T16/T19 Results Quantities
511
Supported MSC.Access Result Quantities Nodal Results 516 Elemental Results 523 Supported 3dplot Results Quantities
543
516
502
viii Patran Interface to MD Nastran Preference Guide
5
Read Input File Review of Read Input File Form Read Input File Form 547 Entity Selection Form 548 Define Offsets Form 550 Selection of Input File 551 Summary Data Form 551 Reject Card Form 553
546
Data Translated from the NASTRAN Input File Partial Decks 554 Coordinate Systems 554 Referential Integrity 554 Chaining 555 Grids and SPOINTs 555 SPOINTs 555 Referential Integrity 555 Elements and Element Properties 555 PSHELL Properties 559 BAROR and BEAMOR Definitions 559 Fields 559 Referential Integrity 559 Set Name Extensions 559 Materials 560 MPCs 561 Load Sets 562 Fields 563 TABLES 564
554
Conflict Resolution 565 Conflict Resolution for Entities Identified by IDs 565 Conflict Resolution for Entities Identified by Names 565
6
Delete Review of Delete Form
568
Deleting an MD Nastran Job
7
Files Files
572
569
CONTENTS ix
8
Errors/Warnings Errors/Warnings
A
576
Preference Configuration and Implementation Software Components in Patran MD Nastran
578
Patran MD Nastran Preference Components
579
Configuring the Patran MD Nastran Execute File
Index
583
582
x Patran Interface to MD Nastran Preference Guide
Chapter 1: Overview Patran Interface to MD Nastran Preference Guide
1
Overview
Purpose
2
MD Nastran Product Information
3
2
Patran Interface to MD Nastran Preference Guide Purpose
1.1
Purpose Patran is an analysis software system developed and maintained by MSC.Software Corporation. The core of the system is a finite element analysis pre and postprocessor. Several optional products are available including; advanced postprocessing programs, tightly coupled solvers, and interfaces to third party solvers. This document describes one of these interfaces. The Patran MD Nastran interface provides a communication link between Patran and MD Nastran. It also provides for the customization of certain features in Patran. The interface is a fully integrated part of the Patran system. Selecting MD Nastran as the analysis code preference in Patran, activates the customization process. These customizations ensure that sufficient and appropriate data is generated for the Patran MD Nastran interface. Specifically, the Patran forms in these main areas are modified: • Materials • Element Properties • Finite Elements/MPCs and Meshing • Loads and Boundary Conditions • Analysis Forms
More information on these topics is contained in Preference Configuration and Implementation (App. A).
Using Patran with SOL 700 The amount of information that needs to be conveyed in the MD Nastran Input file for a SOL 700 analysis is extensive for even a modest size model. The amount of information and the complexity of most models makes it virtually impossible to generate the MD Nastran Input file with a text editor alone. Patran provides a graphical user interface, an extensive line of model building tools that you can use to construct and view your SOL 700 model, and generate a MD Nastran Input file for SOL 700. When using Patran as a preprocessor for SOL 700, you are required to specify an analysis code. Selecting MD Nastran Explicit Nonlinear (SOL 700) as the analysis code under the Analysis Preference menu, customizes Patran in five main areas: • Material Library • Element Library • Loads and Boundary Conditions • MPCs • Analysis forms
The analysis preference also specifies that the model information be output in the MD Nastran Input File format.
Chapter 1: Overview 3 MD Nastran Product Information
1.2
MD Nastran Product Information MD Nastran is a general-purpose finite element computer program for engineering analyses. It is developed, supported, and maintained by MSC.Software Corporation, 2 MacArthur Place, Santa Ana, California 92707, (714) 540-8900. See the MD Nastran Reference Manual, Volume 1, for a general description of MD Nastran’s capabilities.
4
Patran Interface to MD Nastran Preference Guide MD Nastran Product Information
Chapter 2: Building A Model Patran Interface to MD Nastran Preference Guide
2
Building A Model
Introduction to Building a Model
6
Currently Supported MD Nastran Input Options
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
Coordinate Frames
Finite Elements
23
Material Library
59
Element Properties
Beam Modeling
Loads and Boundary Conditions
Load Cases
Defining Contact Regions
Rotor Dynamics
22
87
217
246
250
247
224
8 18
6
Patran Interface to MD Nastran Preference Guide Introduction to Building a Model
2.1
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 code and analysis type. Other parts of the model are created using standard forms. The Analysis option on the Preferences menu brings up a form where the user can select the analysis code (e.g., MD Nastran) and analysis type (e.g., Structural).
The analysis code may be changed at any time during model creation.This is especially useful if the model is to be used for different analyses in different analysis codes. As much data as possible will be converted if the analysis code is changed after the modeling process has begun. The analysis option defines what will be presented to the user 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
Chapter 2: Building A Model 7 Introduction to Building a Model
allowable selections in these same areas. For more details, see The Analysis Form (Ch. 2) in the MSC.Patran Reference Manual.
To use the Patran MD Nastran Application should be set to MD Nastran.
The currently supported Analysis Type fo Nastran are Structural, Thermal and Expl
Indicates the file suffixes used in creating MD Nastran input and output files.
8
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
2.2
Currently Supported MD Nastran Input Options The following tables summarize all the various MD Nastran commands supported by the Patran MD Nastran Application Preference. The tables indicate where to find more information in this manual on how the commands are supported.
Chapter 2: Building A Model 9 Currently Supported MD Nastran Input Options
Supported MD Nastran File Management Commands
Table2-1.
Description
ASSIGN
An ASSIGN command is used to assign a particular name (job name + user specified MD Nastran results suffix) to the MD Nastran OUTPUT2 file to be created during the analysis.
Supported MD Nastran Executive Control Commands
Table 2-2.
Pages
ECHO
230, 233, 235, 241, 245, 250, 253, 256
SOL
225
TIME
230, 233, 235, 241, 245, 250, 253, 256
Supported MD Nastran Case Control Commands
Table 2-3.
Pages
ACCELERATION
250, 253
ACFPMRESULTS
369
ACPOWER
369
ADACT
17, 314
ADAPT
16, 170
DATAREC
17
DISPLACEMENT
230, 241, 250, 253
ELSDCON
230
ESE
230
FORCE
230, 235, 241, 248, 250, 253
FREQUENCY
250
GPSTRESS
369
INTENSITY
369
MAXLINES
230, 233, 235, 241, 245, 250, 253, 256
MPCFORCES OLOAD
369 230, 241, 250, 253
SPCFORCES
230, 235, 241, 248, 250, 253
STRAIN
230, 235, 241, 248, 250, 253
Supported MD Nastran Bulk Data Entries
10
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
Command ADAPT
Pages 16, 170, 225, 233
BEGIN AFPM
147
BEGIN SUPER
219
BCONP
212
BFRIC
212
BFRIC
212
CACINF3
160
CACINF4
160
CBARAO
86
CBAR
86
CBEAM
97, 100
CBEND
93, 95
CDAMP1
82
CDAMP2
219, 438
CELAS1
81
CELAS2
219, 438
CGAP
116
CHEXA
168
CMASS1
119
CMASS2
219, 438
CONM1
76
CONM2
79
CONROD
111
CPENTA
168
CQUAD4
124, 140, 148, 156, 162
CQUAD8
124, 140, 148, 156, 162
CQUADR
131, 142, 150, 157, 163
Command
Pages
CROD
110
CSHEAR
166
CTETRA
168
CTRIAX6
153
Chapter 2: Building A Model 11 Currently Supported MD Nastran Input Options
CTUBE
112
CVISC
115
DCONST
416
DOPTPRM
411, 416
DPHASE
188, 190
DRESP1/2
416
DTI, SETREE
309
DYNRED
240
EIGB
243, 238
EIGC
248
EIGR
238
EIGRL
238
EXTSEOUT
222
FEFACE
15
FEEDGE
15
FORCE
190
FREQ1
250
GMBC
188
GRAV
196
MOMENT
190
MAT1
424
MAT2
424
MAT3
424
MAT8
424
MAT9
424
MPC
28
NLPARM
315
OUTPUT
17, 369
PACINF
160
PARAM, AUTOSPC
230, 233, 235, 241, 245, 250, 253, 256
PARAM, INREL
230
PARAM, ALTRED
230
12
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
PARAM, COUPMASS PARAM, K6ROT
230, 233, 235, 241, 245, 250, 253, 256 230, 233, 235, 241, 245, 250, 253, 256
PARAM, WTMASS
230, 233, 235, 241, 245, 250, 253, 256
PARAM, GRDPNT
230, 233, 235, 241, 245, 250, 253, 256
PARAM, LGDISP
233, 256
PARAM,G
245, 250, 253, 256
PARAM,W3
253, 256
PARAM,W4
253, 256
PARAM, POST
219
PBAR
86
PBCOMP
97
PBEAM
100
PBEAM71 PBEAMD PBELTD PBEND
93, 95
PCOMP
136, 139
PDAMP
82
PELAS
81
PELAS1 PGAP
116
PLOAD1
199
PLOAD2
191
PLOAD4
191
PLOADX1 PLOTEL
191, 149 120
PLPLANE PLSOLID PMASS
119
POINT
15, 170
Chapter 2: Building A Model 13 Currently Supported MD Nastran Input Options
Pages PROD
110
PSHEAR
166
PSHELL
124, 131, 140, 142, 148, 150, 156, 157, 162, 163
PSHELL1 PSHELLD PSOLID
168
PSPRMA PTUBE
112
PBEAM
100
PVAL
15, 170
PVISC
115
RBAR
29
RBE1
31
RBE2
32
RBE3
33
RFORCE
196
RROD
34
RSPLINE
35
RTRPLT SESET
36 42, 219
SETREE
309
SPC1
188
SPCD
188
TEMP
193
TEMPF
146
TEMPRB
193
TEMPP1
193
TIC TSTEP TSTEPNL
197, 198 253 256, 318
14
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
MD Nastran Implicit Nonlinear (SOL 600) The following Bulk Data entries are supported for SOL 600 analyses. 3D Contact Region BCBODY
Defines a flexible rigid contact body in 2D or 3D.
BCBOX*
Defines a 3D contact region.
BCHANGE
Changes definitions of contact bodies.
BCMATL*
Defines a 3D contact region by element material.
BCMOVE
Defines movement of bodies in contact.
BCPARA
Defines contact parameters.
BCPROP*
Defines a 3d contact region by element properties.
BCTABLE
Defines a contact table.
BSURF
Defines a contact body or surface by element IDs.
GMNURB
3D contact region made up of NURBS.
Initial Conditions IPSTRAIN*
Defines initial plastic strain values.
ISTRESS*
Defines initial stress values.
MARCIN
Insert a text string in MSC.Marc.
MARCOUT
Selects data recovery output.
Materials
MATEP
Elasto-plastic material properties.
MATF
Specifies material failure model.
MATG*
Gasket material properties.
MATHE
Hyperelastic material properties.
MATHP
Hyperelastic material properties.
MATHED
Damage model properties for hyperelastic materials.
MATORT
Elastic 3D orthotropic material properties.
MATTEP
Thermoelastic-Plastic material properties.
MATTG*
Temperature variation of interlaminar materials.
MATTHE
Thermo hyperelastic material.
MATTORT*
Thermoelastic orthotropic material
MATTVE*
Thermo-visco-elastic material properties
Chapter 2: Building A Model 15 Currently Supported MD Nastran Input Options
MATVE*
Viscoelastic material properties
MATVP
Viscoplastic or creep material properties
Note:
* Not supported in initial release of Patran (2004).
Note:
Solution Control
NLAUTO
Parameters for automatic load/time stepping.
NLDAMP
Defines damping constants.
NLSTRAT
Strategy Parameters for nonlinear structural analysis.
PARAMARC
Parallel domain decomposition.
RESTART
Restart data.
Note: Note: NTHICK
Element Properties
Defines nodal thickness values for beams, plates, and/or shells.
MD Nastran Explicit Nonlinear (SOL 700) The following Bulk Data entries are supported for SOL 700 analyses. Materials MATD001
Isotropic Elastic material for beam, shell and solid.
MATD003
Isotropic and kinematic hardening plasticity.
MATD005
Isotropic materials to model soil and foam.
MATD006
Isotropic viscoelastic material.
MATD007
Isotropic material to model nearly incompressible continuum rubber.
MATD012
Isotropic plasticity for 3D solids.
MATD014
Isotropic materials to model soil and foam with failure.
MATD015
Isotropic Johnson/Cook strain and temperature sensitive plasticity.
MATD019
Isotropic strain rate dependent material.
MATD020
Isotropic rigid material.
MATD022
Orthotropic material with optional brittle failure for composites.
MATD024
Isotropic elasto-plastic material with stress x strain curve and strain rate dependency.
MATD026
Anisotropic honeycomb and foam material.
MATD027
Isotropic material to model rubber using two variables.
MATD028
Isotropic elasto-plastic material for beam and shell.
16
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
MATD030
Isotropic superelastic material.
MATD031
Isotropic material to model rubber using the Frazer-Nash formulation.
MATD032
Orthotropic laminated glass material.
MATD057
Isotropic material to model highly compressible low density foams.
MATD058
*MAT_LAMINATED_COMPOSITE_FABRIC
MATD062
Isotropic material to model viscous foams.
MATD063
Isotropic material to model crushable foams.
MATD064
Isotropic elasto-plastic material with a power law hardening.
MATD067
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM
MATD068
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM
MATD069
*MAT_SID_DAMPER_DISCRETE_BEAM
MATD070
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM
MATD071
*MAT_CABLE_DISCRETE_BEAM
MATD073
*MAT_LOW_DENSITY_VISCOUS_FOAM
MATD074
*MAT_ELASTIC_SPRING_DISCRETE_BEAM
MATD076
*MAT_GENERAL_VISCOELASTIC
MATD083
*MAT_FU_CHANG_FOAM
MATD087
*MAT_CELLULAR_RUBBER
MATD093
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM
MATD094
*MAT_INELASTIC_SPRING_DISCRETE_BEAM
MATD095
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM
MATD097
*MAT_GENERAL_JOINT_DISCRETE_BEAM
MATD100
Isotropic spotweld material.
MATD103
Anisotropic viscoplastic material.
MATD119
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM
MATD121
*MAT_GURSON_RCDC
MATD126
*MAT_MODIFIED_HONEYCOMB
MATD20M
*MAT_RIGID
MATDB01
*MAT_SEATBELT
MATDS01
*MAT_SPRING_ELASTIC
MATDS02
*MAT_DAMPER_VISCOUS
MATDS03
*MAT_SPRING_ELASTOPLASTIC
MATDS04
*MAT_SPRING_NONLINEAR_ELASTIC
MATDS05
*MAT_DAMPER_NONLINEAR_VISCOUS
Chapter 2: Building A Model 17 Currently Supported MD Nastran Input Options
MATDS06
*MAT_SPRING_GENERAL_NONLINEAR
MATDS07
*MAT_SPRING_MAXWELL
MATDS08
*MAT_SPRING_INELASTIC
MATDS13
*MAT_SPRING_TRILINEAR_DEGRADING
MATDS14
*MAT_SPRING_SQUAT_SHEARWALL
MATDS15
*MAT_SPRING_MUSCLE
Loads and Boundary Conditions TIC3
Defines initial rotational field.
WALL
Defines planar rigid wall.
Elements and Properties CDAMP1D
Scalar damper connection for SOL 700
CELAS1D
Scalar spring connection for SOL 700.
Solution Controls Form
Parameters
Execution Control Parameters
DYSTATIC, DYBLDTIM, DYINISTEP, DYTSTEPERODE, DYMINSTEP, DYMAXSTEP, DYSTEPFCTL, DYTERMNENDMAS, DYTSTEPDT2MS
General Parameters
DYLDKND, DYCOWPRD, DYCOWPRP, DYBULKL, DYHRGIHQ, DYRGQH, DYENERGYHGEN, DYSHELLFORM, DYSHTHICK, DYSHNIP
Contact Parameters
DYCONSLSFAC, DYCONRWPNAL, DYCONPENOPT, DYCONTHKCHG, DYCONENMASS, DYCONECDT, DYCONIGNORE, DYCONSKIPTWG
Binary Output Database File Parameters
DYBEAMIP, DYMAXINT, DYNEIPS, DYNINTSL, DYNEIPH, DYSTRFLG, DYSIGFLG, DYEPSFLG, DYRLTFLG, DYENGFLG, DYCMPFLG, DYIEVERP, DYDCOMP, DYSHGE, DYSTSSZ, DYN3THDT
DAMPGBL
Dynamic relaxation control.
18
Patran Interface to MD Nastran Preference Guide
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
2.3
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference In Version 68 of MSC. Nastran, MSC introduced p-adaptive analysis using solid elements. The Patran MD Nastran Preference provides support for this new capability. There are some fundamental differences in approach to model building and results import for p-element analyses; this section will serve as a guide to these. MSC .Nastran Version 69 extends the Version 68 capabilities for p-adaptive analysis in two areas. Shell and beam elements have been added and p-shells and p-beams can be used for linear dynamic solution sequences. Patran Version 6.0 supports both of these capabilities. Element Creation MD Nastran supports adaptive, p-element analyses with the 3D-solid CTETRA, CPENTA, and CHEXA elements; 2D-solid TRIA, and QUAD elements; shells TRIA, and QUAD elements; beams BAR elements. Patran and MD Nastran allow TET4, TET10, TET16, TET40, WEDGE6, WEDGE15, WEDGE52, HEX8, HEX20, and HEX64 for p-adaptive analysis for 3D-solids; TRIA3, TRIA6, TRIA7, TRIA9, TRIA13, QUAD4, QUAD8, QUAD9, QUAD12, and QUAD16 for p-adaptive analysis for 2Dsolids and membranes; TRIA3, TRIA6, TRIA7, TRIA9, TRIA13, QUAD4, QUAD8, QUAD9, QUAD12, and QUAD16 for p-adaptive analysis for shells; BAR2, BAR3, and BAR4 for p-adaptive analysis for beams. The preferred approach, when beginning a new model, is to use the higher-order elements--HEX64, WEDGE52, TET40, and TET16, or TRIA13 and QUAD16, or BAR4. The support for lower-order elements is provided primarily to support existing models. The higher-order cubic elements allow more accurate definition of the geometry and more accurate postprocessing of results from the MD Nastran analysis.The translator generates the appropriate MD Nastran FEEDGE and POINT entities for all curved edges on the p-elements. Models with HEX64 and WEDGE52 elements are easily created with the Patran Iso Mesher; models with TET16 elements can be created with the Tet Mesher. Models with QUAD16 and TRIA13 elements can be created using the Iso Mesher or the Paver. For p-elements, Patran generates cubic edges to fit the underlying geometry. The cubic edge consists of two vertex grid points and two points in between. Adjacent cubic edges are not necessarily C1 continuous. If the original geometry is smooth, the cubic edges may introduce kinks which cause false stress concentrations. Then, the p-element produces unrealistic results especially for thin curved shells. In Version 7 of Patran, for cubic elements, the two midside nodes on each edge are adjusted so that the edges of adjacent elements are C1 continuous. The adjustment is done in the Pat3Nas translator. After the Pat3Nas translator is executed, the location of the two midside nodes in the Patran database has changed. The user is informed with a warning message. The user can turn the adjustment of midside nodes ON and OFF with the environment variable PEDGE_MOVE. By default, the midside nodes are adjusted to make the adjacent elements C1 continuous. For PEDGE_MOVE set to OFF, the points on a cubic edge are not adjusted. Patran generates the input for MD Nastran. For cubic edges, FEEDGE Bulk Data entries with POINTs are written. By default, the location of the two POINTs is moved to 1/3 and 2/3 of the edge in MD Nastran. The points generated by Patran must not be moved. Therefore, a parameter entry PARAM, PEDGEP, 1 is written by Patran. PEDGEP=1 indicates that incoming POINTs are not moved in MD
Chapter 2: Building A Model 19 Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
Nastran. The default is PEDGEP= 0, MD Nastran will move the two POINTs to 1/3 and 2/3 of the edge. The C1 continuous cubic edges improve the accuracy of p-element results. In the Version 69 Release Guide, a cylinder under internal pressure was tested to determine the quality of shell p-elements for curved geometry. The accuracy of the results was very good when exact geometry was used. With C1 continuous edges we recover the same quality of results within single precision accuracy. Element and p-Formulation Properties Both element and p-formulation properties are defined using the Element Properties application by choosing Action: Create, Dimension: 1D/2D/ or 3D, Type: Beam/Shell/Bending Panel/2D Solid/Membrane/ or Solid, and p-Formulation on the main form. The details of the property form for this case are described on (p. 209). Most of the properties are optional and have defaults; the material property name is required. Two properties that may need to be defined are Starting P-orders and Maximum P-orders. These properties specify the polynomial orders for the element interpolation functions in the three spatial directions. Although these are integer values, in Patran, each property is defined using the Patran vector definition. At first, this may seem peculiar, but it gives the user access to many useful tools in the Patran system for defining and manipulating these properties. Typically, a user would define these properties with a syntax like <3 4 2> to prescribe polynomial orders of 3, 4, and 2 in the X, Y, and Z directions. Patran will convert these values to floating point <3. 4. 2.>, but the Patran MD Nastran Preference will interpret them. This vector syntax is convenient primarily because it allows these properties to be defined using the Fields application. In a case where the material properties are constant over the model, but it is desirable to prescribe a distribution of p-orders, vector fields can be defined and specified in a single property definition. The Patran MD Nastran Preference will provide additional help for this modeling function. At the end of an adaptive analysis, when results are imported, vector, spatial fields will optionally be created containing the p-orders used for each element for each adaptive cycle. To repeat a single adaptive cycle, it is necessary only to modify the element properties by selecting the appropriate field. A common use of the Maximum P-orders property is in dealing with elements in the vicinity of stress singularities. These singularities may be caused by the modeling of the geometry (e.g., sharp corners), boundary conditions (e.g., point constraints), or applied forces (e.g., point forces). Sometimes it is easier to tell the adaptive analysis to “ignore” these singular regions than it is to change the model. This can be done by setting the Maximum P-orders property for elements in this region to low values (e.g., <1 1 1> or <2 2 2>. These elements are sometimes called “sacrificial” elements. Loads and Boundary Conditions It is well known in solid mechanics that point forces and constraints cause the stress field in the body to become infinite. In p-adaptive analyses, care must be taken in finite element creation and loads application to ensure that these artificial high-stress regions don’t dominate the analysis. Generally, the best results are obtained with distributed loads (pressures) or distributed displacements. There are two options under Loads/BCs for applying distributed displacements. The Element Uniform and Element Variable types under Displacements allow displacement constraints to be applied to the
20
Patran Interface to MD Nastran Preference Guide
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
faces of solid elements. If the elements are p-elements, the appropriate FEFACE and GMBC entries are produced. If applied to non-p-elements, the appropriate SPC1 or SPCD entries are produced. Several new loads and boundary conditions support the p-shell and p-beam elements. Distributed loads can be applied to beam elements or to the edge of shell elements. Pressure loads can be applied to the faces of p-shell elements. Temperature loads can be applied to either the nodes or the elements. Analysis Definition Adaptive linear static and normal modes analyses are supported in Version 68 of MSC .Nastran; both solution types are supported by the Patran MD Nastran Preference. Only a few parameters on the Analysis forms may need to be changed for p-element analyses. If running a version of MSC . Nastran prior to Version 68.2 (i.e., Version 68, or 68.1), the OUTPUT2 Request option on the Translation Parameters form must be set to Alter File in order to process the results in Patran. The Solution Parameters forms for the linear static and normal modes analyses contain a Max p-Adaptive Cycles option, which is defaulted to 3. The Subcase Parameters form under Subcase Create has options to limit the participation of this subcase in the adaptive error analysis. Finally, the Advanced Output Requests form under Subcase Create has an option to define whether results are to be produced for all adaptive cycles or only every nth adaptive cycle. Results Import and Postprocessing Two different approaches are provided for postprocessing results from MD Nastran p-element analyses. Both approaches rely on MD Nastran creating results for a “VU mesh” where each p-element is automatically subdivided into a number of smaller elements. In the standard approach with the default MD Nastran VU mesh (3 x 3 x 3 elements) for solids, (3 x 3 elements) for shells and (3 elements) for beams, the results will automatically be mapped onto the Patran nodes and elements during import. This mapping will occur for all 10, Patran solid element topologies mentioned above. The most accurate mapping and postprocessing takes place when results are mapped to the higher-order Patran elements. When the adaptive analysis process increases the p-orders in one or more elements beyond 3, the 3 x 3 x 3 VU mesh, mapping, and postprocessing may not be sufficiently accurate. The Patran MD Nastran Preference provides a second approach to handle this situation. In this case, a user can specify a higherorder VU mesh (e.g. 5 x 5 x 5) on the MD Nastran OUTRCV entry and then import both model data and results entities into a new, empty Patran database. In this case, the VU mesh and results are imported directly, rather than mapped and can be post-processed with greater accuracy. The OUTRCV entry is currently supported only with the Bulk Data Include File option on the Translation Parameters form. It should be noted that, with this import mode, displays of element results (e.g., fringe plots) may be discontinuous across parent, p-element boundaries. This occurs because the VU grids generated by MD Nastran are different in each p-element. Along element boundaries there are coincident nodes and a result associated with each one. The user should not try to perform an Equivalence operation to remove these coincident nodes. If this is done, subsequent postprocessing operations will likely be incorrect. For both postprocessing options, a result case is created for each adaptive cycle in the analysis. The result types in this result case will depend on specific options selected on the Output Request form. By default, the Adaptive Cycle Output Interval option is equal to zero. This means that output quantities specific to
Chapter 2: Building A Model 21 Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
p-elements will be written only for the last cycle. If postprocessing of results from intermediate cycles is desired, the Adaptive Cycle Output Interval option should be set equal to one. One of the key uses of output from intermediate adaptive cycles is in examining the convergence of selected quantities (e.g., stresses). This can be done using the X-Y plotting capability under the Results application. Potential Pitfalls There are several areas where a user can encounter problems producing correct p-element models for MD Nastran. One is the incorrect usage of the midside nodes in the Patran higher order-elements. These nodes are used in p-element analysis only for defining the element geometry; analysis degrees of freedom are not associated with these nodes. Therefore it is illegal, for example, to attach non p-elements to assign loads or boundary conditions to these nodes. One way this can occur inadvertently is if a nodal force is applied to the face of a Patran solid. This force is interpreted as a point force at every node (including the midside nodes) on the face of the solid. For the p-elements, this is not valid. This type of load should instead be applied as an element uniform or element variable pressure. Adaptive Analysis of Existing Models Modifying an existing solid model for adaptive, p-element analysis is relatively straightforward. The first step is to read the NASTRAN input file into Patran using the Analysis/Read Input File option. The model may contain any combination of linear or quadratic tetra, penta, or hexa elements. The second step is to use the Element Props/Modify function to change the Option for all solid properties from Standard Formulation to P-Formulation. The element properties form for p-formulation solids has many options specific to p-element analysis; but they all have appropriate defaults. This property modification step is the only change that must be made before submitting the model for analysis. Often, however, as discussed in Potential Pitfalls, 21, it is appropriate to modify the types of loads and boundary conditions applied to the model. For example, in non p-element models, displacement constraints are applied using MD Nastran SPC entries at grid points. In p-element analyses, elementoriented displacement constraints are more appropriate. Existing displacement LBCs can be modified using the Loads/BCs/Modify/Displacement option. For an SPC type of displacement constraint, the LBC type is nodal. For a p-element analysis, Element Uniform or Element Variable displacement constraints are more appropriate. The application region must be changed from a selection of nodes to a selection of element faces. As described above, nodal forces can be troublesome in p-element analyses. If possible, it is beneficial to redefine point forces as pressures acting on an element face. If this is not possible, an alternative is to limit the p-orders in the elements connected to the node with the point force; this can be done by defining a new element property for these elements and defining the Maximum P-orders vector appropriately. Element pressures, inertial loads, and nodal temperatures defined in the original model need not be changed for the p-element analysis.
22
Patran Interface to MD Nastran Preference Guide Coordinate Frames
2.4
Coordinate Frames Coordinate frames will generate a unique CORD2R, CORD2C, or CORD2S Bulk Data entry, depending on the specified coordinate frame type. The CID field is defined by the Coord ID assigned in Patran. The RID field may or may not be defined, depending on the coordinate frame construction method used in Patran. The A1, A2, A3, B1, B2, B3, C1, C2, and C3 fields are derived from the coordinate frame definition in Patran.
Only Coordinate Frames that are referenced by nodes, element properties, or loads and boundary conditions can be translated. For more information on creating coordinate frames see Creating Coordinate Frames (p. 393) in the Geometry Modeling - Reference Manual Part 2. To output all the coordinate frames defined in the model whether referenced or not, set the environment variable “WRITE_ALL_COORDS” to ON.
Chapter 2: Building A Model 23 Finite Elements
2.5
Finite Elements The Finite Elements Application in Patran allows the definition of basic finite element construction. Created under Finite Elements are the nodes, element topology, multi-point constraints, and Superelement.
For more information on how to create finite element meshes, see Mesh Seed and Mesh Forms (p. 25) in the Reference Manual - Part III.
Nodes Nodes in Patran will generate unique GRID Bulk Data entries in MD Nastran. Nodes can be created either directly using the Node object, or indirectly using the Mesh object. Each node has associated Reference (CP) and Analysis (CD) coordinate frames. The ID is taken directly from the assigned node
24
Patran Interface to MD Nastran Preference Guide Finite Elements
ID. The X1, X2, and X3 fields are defined in the specified CP coordinate frame. If no reference frame is assigned, the global system is used. The PS and SEID fields on the GRID entry are left blank.
The analysis frame (CD of the GRID) is the coordinate system in which the displacements, degrees of freedom, constraints, and solution vector are defined. The coordinate system in which the node location is defined (CP of the GRID) can be either the reference coordinate frame, the analysis coordinate frame, or a global reference (blank), depending on the value of the forward translation parameter “Node Coordinates.”
Elements The Finite Elements Application in Patran assigns element connectivity, such as Quad4, for standard finite elements. The type of MD Nastran element to be created is not determined until the element properties are assigned (for example, shell or 2D solid). See the Element Properties Form, 87 for details concerning the MD Nastran element types. Elements can be created either directly using the Element object, or indirectly using the Mesh object
Chapter 2: Building A Model 25 Finite Elements
.
26
Patran Interface to MD Nastran Preference Guide Finite Elements
This type of form is used to create a 1D, 2D, or 3D element mesh.
Beginning IDs for nodes and elements to be created. Elem Shape is used to specify the shape of the elements created by meshing. For example, the shape for a 2D element can be either triangular or quadralateral. Mesher is used to specify how the element mesh is to be created; for example, IsoMesh, Paver. The type of geometry (for example, simple (green) or complex (magenta) surface) may determine the choice of the mesher.
List of surface IDs of surfaces to be meshed. For example Surface 1, 2, 3, or Surface 1:3. The value of Global Edge Length specifies the approximate size of the elements created when meshing. The button Select Existing Prop... is used to select an existing element property (for example, 2D Shell) that will be assigned to the elements created by meshing. The button Create New Property is used to create an element property that will be assigned to the elements that will be created by meshing. During creating the element property no application region can be specified; it is specified automatically using all the elements created by meshing. This “ghosted” area will become dark when an element property is selected.
Chapter 2: Building A Model 27 Finite Elements
Multi-point Constraints Multi-point constraints (MPCs) can also be created from the Finite Elements Application. These are special element types that 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).
Used to specify the ID to associate to the MPC when it is created.
28
Patran Interface to MD Nastran Preference Guide Finite Elements
MPC Types To create an MPC, first select the type of MPC to be created from the option menu. The MPC types that appear in the option menu are dependent on the current settings of the Analysis Code and Analysis Type preferences. The following table describes the MPC types which are supported for MD Nastran. MPC Type
Analysis Type
Description
Explicit
Structural
Creates 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 can be specified, while only one dependent term can be specified. The constant term is not allowed in MD Nastran.
RSSCON Surf-Vol
Structural
Creates an RSSCON 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.
Rigid (Fixed)
Structural and Explicit Nonlinear
Creates a rigid 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 can be specified, while only one independent term can be specified. Each term consists of a single node. There is no constant term for this MPC type.
RBAR
Structural and Explicit Nonlinear
Creates an RBAR element, which defines a rigid bar between two nodes. Up to two dependent and two independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the two dependent terms must be the same as the nodes specified in the two independent terms. Any combination of the degrees of freedom of the two nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
RBE1
Structural
Creates an RBE1 element, which defines a rigid body connected to an arbitrary number of nodes. An arbitrary number of dependent terms can be specified. Each term consists of a node and a list of degrees of freedom. Any number of independent terms can be specified as long as the total number of degrees of freedom specified in all of the independent terms adds up to six. Since at least one degree of freedom must be specified for each term there is no way the user can create more that six independent terms. There is no constant term for this MPC type.
Chapter 2: Building A Model 29 Finite Elements
MPC Type
Analysis Type
Description
RBE2
Structuraland Explicit Nonlinear
Creates an RBE2 element, which defines a rigid body between an arbitrary number of nodes. Although the user can only specify one dependent term, an arbitrary number of nodes can be associated to this term. The user is also prompted to associate a list of degrees of freedom to this term. A single independent term can be specified, which consists of a single node. There is no constant term for this MPC type.
RBE3
Structuraland Explicit Nonlinear
Creates an RBE3 element, which defines the motion of a reference node as the weighted average of the motions of a set of nodes. An arbitrary number of dependent terms can be specified, each term consisting of a node and a list of degrees of freedom. The first dependent term is used to define the reference node. The other dependent terms define additional node/degrees of freedom, which are added to the m-set. An arbitrary number of independent terms can also be specified. Each independent term consists of a constant coefficient (weighting factor), a node, and a list of degrees of freedom. There is no constant term for this MPC type.
RROD
Structural
Creates an RROD element, which defines a pinned rod between two nodes that is rigid in extension. One dependent term is specified, which consists of a node and a single translational degree of freedom. One independent term is specified, which consists of a single node. There is no constant term for this MPC type.
RSPLINE
Structural
Creates an RSPLINE element, which interpolates the displacements of a set of independent nodes to define the displacements at a set of dependent nodes using elastic beam equations. An arbitrary number of dependent terms can be specified. Each dependent term consists of a node, a list of degrees of freedom, and a sequence number. An arbitrary number of independent nodes (minimum of two) can be specified. Each independent term consists of a node and a sequence number. The sequence number is used to order the dependent and independent terms with respect to each other. The only restriction is that the first and the last terms in the sequence must be independent terms. A constant term, called D/L Ratio, must also be specified.
30
Patran Interface to MD Nastran Preference Guide Finite Elements
MPC Type
Analysis Type
Description
RTRPLT
Structural
Creates an RTRPLT element, which defines a rigid triangular plate between three nodes. Up to three dependent and three independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the three dependent terms must be the same as the nodes specified in the three independent terms. Any combination of the degrees of freedom of the three nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
Cyclic Symmetry
Structural
Describes cyclic symmetry boundary conditions for a segment of the model. If a cyclic symmetry solution sequence is chosen, such as “SOL 114,” then CYJOIN, CYAX and CYSYM entries are created. If a solution sequence that is not explicitly cyclic symmetric is chosen, such as “SOL 101,” MPC and SPC entries are created. Be careful, for this option automatically alters the analysis coordinate references of the nodes involved. This could erroneously change the meaning of previously applied load and boundary conditions, as well as element properties.
Sliding Surface
Structural
Describes the boundary conditions of sliding surfaces, such as pipe sleeves. These boundary conditions are written to the NASTRAN input file as explicit MPCs. Be careful, for this option automatically redefines the analysis coordinate references of all affected nodes. This could erroneously alter the meaning of previously applied load and boundary conditions, as well as element properties.
RBAR1
Structural
This is an alternate (simplified) form for RBAR. Creates an RBAR1 element, which defines a rigid bar between two nodes, with six degrees of freedom at each end. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
Chapter 2: Building A Model 31 Finite Elements
MPC Type
Analysis Type
Description
RTRPLT1
Structural
Alternative format to define a rigid triangular plate element connecting three grid points. Creates an RTRPLT1 element, which defines a rigid triangular plate between three nodes. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of the node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
RJOINT
Structural
Creates an RJOINT element, which defines a rigid joint element connecting two coinciding grid points. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). There is no constant term for this MPC type.
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. The following degrees of freedom are supported by the Patran MD Nastran MPCs for the various analysis types: Degree of freedom
Analysis Type
UX
Structural
UY
Structural
UZ
Structural
RX
Structural
RY
Structural
RZ
Structural
Note:
Care must be taken to make sure that a degree of freedom that is 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 degrees of freedom at this node when defining an MPC.
Explicit MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Explicit is the selected type. This form is used to create an MD Nastran MPC Bulk Data entry. The difference in explicit MPC equations between Patran and MD Nastran will result in the A1 field of the MD Nastran entry being set to -1.0.
32
Patran Interface to MD Nastran Preference Guide Finite Elements
Holds the dependent term information. This term will define the fields for G1 and C1 on the MPC entry. Only one node and DOF combination may be defined for any given explicit MPC. The A1 field on the MPC entry is automatically set to -1.0.
Holds the independent term information. These terms define the Gi, Ci, and Ai fields on the MPC entry, where i is greater than one. As many coefficient, node, and DOF combinations as desired may be defined.
Chapter 2: Building A Model 33 Finite Elements
Rigid (Fixed)
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Rigid (Fixed) is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry. The CM field on the RBE2 entry will always be 123456.
Holds the dependent term information. This term defines the GMi fields on the RBE2 entry. As many nodes as desired may be selected as dependent terms.
Holds the independent term information. This term defines the GN field on the RBE2 entry. Only one node may be selected.
34
Patran Interface to MD Nastran Preference Guide Finite Elements
RBAR MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBAR is the selected type. This form is used to create an MD Nastran RBAR Bulk Data entry and defines a rigid bar with six degrees of freedom at each end. Both the Dependent Terms and the Independent Terms lists can have either 1 or 2 node references. The total number of referenced nodes,
Chapter 2: Building A Model 35 Finite Elements
however, must be 2. If either or both of these lists references 2 nodes, then there must be an overlap in the list of referenced nodes.
Holds the dependent term information. Either one or two nodes may be defined as having dependent terms. The Nodes define the GA and GB fields on the RBAR entry. The DOFs define the CMA and CMB fields.
Holds the independent term information. Either one or two nodes may be defined as having independent terms.The Nodes define the GA and GB fields on the RBAR entry.The DOFs define the CNA and CNB fields.
36
Patran Interface to MD Nastran Preference Guide Finite Elements
RBE1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE1 is the selected type. This form is used to create an MD Nastran RBE1 Bulk Data entry.
Chapter 2: Building A Model 37 Finite Elements
Holds the dependent term information. Defines the GMi and CMi fields on the RBE1 entry. An unlimited number of nodes and DOFs may be defined here.
Holds the independent term information. Defines the GNi and CNi fields on the RBE1 entry. The total number of Node/DOF pairs defined must equal 6, and be capable of representing any general rigid body motion.
38
Patran Interface to MD Nastran Preference Guide Finite Elements
RBE2 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE2 is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry.
Chapter 2: Building A Model 39 Finite Elements
Holds the dependent term information. This term defines the GMi and CM fields on the RBE2 entry. As many nodes as desired may be selected as dependent terms.
Holds the independent term information. This term defines the GN field on the RBE2 entry. Only one node may be selected.
RBE3 MPCs
40
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE3 is the selected type. This form is used to create a MD Nastran RBE3 Bulk Data entry.
Chapter 2: Building A Model 41 Finite Elements
Holds the dependent term information. Defines the GMi and CMi fields on the RBE3 entry. The first dependent term will be treated as the reference node, REFGRID and REFC. The rest of the dependent terms become the GMi and CMi components.
Holds the independent term information. Defines the Gi, j, Ci, and WTi fields on the RBE3 entry.
RROD MPCs
42
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RROD is the selected type. This form is used to create an MD Nastran RROD Bulk Data entry.
Chapter 2: Building A Model 43 Finite Elements
Holds the dependent term information. Defines the GB and CMB on the RROD entry. Only one translational DOF may be referenced for this entry.
Holds the independent term information. Defines the GA field on the RROD entry. The CMA field is left blank.
44
Patran Interface to MD Nastran Preference Guide Finite Elements
RSPLINE MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RSPLINE is the selected type. This form is used to create an MD Nastran RSPLINE Bulk Data entry. The D/L field for this entry is defined on the main MPC form. This MPC type is typically used to tie together two dissimilar meshes.
Chapter 2: Building A Model 45 Finite Elements
Holds the dependent term information.
Holds the independent term information. Terms with the highest and lowest sequence numbers must be independent.
Determines what sequence the independent and dependent terms will be written to the RSPLINE entry.
RTRPLT MPCs
46
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT is the selected type. This form is used to create an MD Nastran RTRPLT Bulk Data entry.
Chapter 2: Building A Model 47 Finite Elements
Holds the dependent term information. Defines the GA, GB, GC, CMA, CMB, and CMC fields of the RTRPLT entry.
Holds the independent term information. The total number of nodes referenced in both the dependent terms and the independent terms must equal three. There must be exactly six independent degrees of freedom, and they must be capable of describing rigid body motion. Defines the GA, GB, GC, CNA, CNB, and CNC fields of the RTRPLT entry.
Cyclic Symmetry MPCs
48
Patran Interface to MD Nastran Preference Guide Finite Elements
The Cyclic Symmetry MPC created by this form will be translated into CYJOIN, CYAX, and CYSYM entries if cyclic symmetric is the selected type, see Solution Parameters, 277, or into SPC and MPC entries if the requested type is not explicitly cyclic symmetric.
If the type selected is Cyclic Symmetry, the type of symmetry will always be rotational. NOTE: MPC option will automatically overwrite the analysis coordinate references on all the nodes belonging to the Dependent and Independent Regions. Be careful that this does not erroneously change the meaning of previously applied loads and boundary conditions, or element properties.
Any node lying on the Z axis will be automatically written to the CYAX entry.
Side 2 of the CYJOIN entries. Side 1 of the CYJOIN entries.
Sliding Surface MPCs
The Sliding Surface MPC created by this form will be translated into explicit MPCs in the NASTRAN input file.
Chapter 2: Building A Model 49 Finite Elements
If a Sliding Surface type is used, note that this MPC option will automatically overwrite the analysis coordinate references on all the nodes belonging to the Dependent and Independent Regions. Be careful that this does not erroneously change the meaning of previously applied loads and boundary conditions, or element properties.
RBAR1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements
50
Patran Interface to MD Nastran Preference Guide Finite Elements
form and RBAR1 is the selected type. This form is used to create an MD Nastran RBAR1 Bulk Data entry.
Chapter 2: Building A Model 51 Finite Elements
.
RTRPLT1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT1 is the selected type. This form is used to create an MD Nastran RTRPLT1 Bulk Data
52
Patran Interface to MD Nastran Preference Guide Finite Elements
entry.
Chapter 2: Building A Model 53 Finite Elements
.
RJOINT MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RJOINT is the selected type. This form is used to create an MD Nastran RJOINT Bulk Data
54
Patran Interface to MD Nastran Preference Guide Finite Elements
entry.
Chapter 2: Building A Model 55 Finite Elements
.
56
Patran Interface to MD Nastran Preference Guide Finite Elements
Superelements In superelement analysis, the model is partitioned into separate collections of elements. These smaller pieces of structure, called Superelement, are first solved as separate structures by reducing their stiffness matrix, mass matrix, damping matrix, loads and constraints to the boundary nodes and then combined to solve for the whole structure. The first step in creating a superelement is to create a Patran group (using Group/Create) that contains the elements in the superelement. This group is then selected in the Finite Elements application on the Create/ Superelement form.
Chapter 2: Building A Model 57 Finite Elements
List of existing superelements.
The group containing all the elements that define a superelement. Note that the group must contain elements not just nodes. If a group does not contain elements, it will not show up in the Element Definition Group listbox.
Brings up an optional subordinate form that allows a user to select boundary nodes of the superelement. By default, the common nodes between the elements in the group and the rest of the model are selected as the boundary nodes.
58
Patran Interface to MD Nastran Preference Guide Finite Elements
Select Boundary Nodes
Allows for manual selection of boundary nodes. Remove selected nodes from the Selected Boundary Nodes box.
Add selected nodes to the Selected Boundary Nodes box.
Chapter 2: Building A Model 59 Material Library
2.6
Material Library The Materials form appears when the Material toggle, located on the Patran application selections, is chosen. The selections made on the Materials menu will determine which material form appears, and ultimately, which Nastran material will be created. The following pages give an introduction to the Materials form and details of all the material property definitions supported by the Nastran Preference. Only material records that are referenced by an element property region or by a laminate lay-up are translated. References to externally defined materials result in special comments in the input Nastran file, e.g., materials that property values that are not defined in Patran. The forward translator performs material type conversions when needed. This applies to both constant material properties and temperature-dependent material properties. For example, a three-dimensional orthotropic material that is referenced by CHEXA elements is converted into a three-dimensional anisotropic material.
Materials Application Form This form appears when Materials is selected on the main menu. The Materials form is used to provide options to create the various Nastran materials.
60
Patran Interface to MD Nastran Preference Guide Material Library
This toggle defines the basic material directionality and can be set to Isotropic, 2D Orthotropic, 3D Orthotropic, 2D Anisotropic, 3D Anisotropic, or Composite. For Explicit Nonlinear additional materials can be defined.
Lists the existing materials with the specified directionality.
Defines the material name. A unique material ID will be assigned during translation.
Describes the material that is being created.
Generates a form that is used to define the material properties. See Material Input Properties Form, 61. Generates a form that is used to indicate the active portions of the material model. By default, all portions of a created material model are active.
Chapter 2: Building A Model 61 Material Library
Material Input Properties Form The Input Properties form is the form where all constitutive material models are defined for each material created. Multiple constitutive models can be created for each material created by pressing the Apply button on the main Materials form with the proper widgets set on this form. Multiple constitutive models of the same type are not allowed. The list of existing constitutive models are shown in the bottom list box. A list of valid constitutive models is given in the table below. Set the Constitutive Model here. Press the Apply button on the main Materials application form to create a constitutive model for the given material. Multiple constitutive models can be created for the same material.
Enter the property values in the databoxes. If a value can be temperature, model, strain rate, or strain dependent, a separate listbox will appear to select a field. These fields must be created in the Fields application as Material type fields.
This is a list of current constitutive models. Use the Change Material Status button to turn them on/off from translation into the Nastran input deck.
62
Patran Interface to MD Nastran Preference Guide Material Library
Material Constitutive Models The following table outlines the options when Create is the selected Action. Object
Option 1
Option 2
Option 3
Option 4
Option 5
Isotropic • Linear Elastic • Nonlinear Elastic • Hyperela • Nearly
stic
• Test Data
Incompressible
• Mooney
Rivlin
Order: 1 2 3
• Coefficients
• Mooney
Rivlin • Ogden • Foam • Arruda-Boyce • Gent
Order: 1 2 3 4 5
• Elastoplastic • Stress/Strain
Curve
• von Mises
• Isotropic
• Tresca
• Kinematic
• Mohr-
• Combined
Coulomb • Drucker-
Prager
Chapter 2: Building A Model 63 Material Library
Object
Option 1
Option 2
Option 3
Option 4
• Parabolic
• Isotropic
MohrColomb
• Kinematic
• Buyukoztu
Option 5
• Combined
• Piecewis
e Linear
• Cowper-
Symon ds
rk Concrete • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • None
• Power Law • Power Rate Law • Johnson-Cook • Kumar
• Hardening
Slope
• von
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager
64
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1
Option 2
Option 3
• Perfectly
• Parabolic
Plastic
MohrColomb
Option 4
Option 5
• None
• Piecewis
e Linear
• Cowper-
• Buyukoztu
Symon ds
rk Concrete • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • Rigid
Plastic
• None
• Power Law • Power Rate Law • Johnson-Cook • Kumar
PiecewiseLinear
• Failure
• n/a • Hill • Hoffman • Tsai-Wu • Maximum Strain
Piecewise Linear CowperSymonds
Chapter 2: Building A Model 65 Material Library
Object
Option 1 • Failure1/
2/3
Option 2 • Maximum
Stress • Maximum
Strain • Hoffman
Option 3
• No Progressive • Standard • Gradual Selective • Immediate Selective
• Hill • Tsai-Wu • Hashin • Puck • Hashin-
Tape • Hashin-
Fabric • User
Defined Failure • Creep
• Tabular Input • Creep Law 111 • Creep Law 112 • Creep Law 121 • Creep Law 122 • Creep Law 211 • Creep Law 212 • Creep Law 221 • Creep Law 222 • Creep Law 300 • MATVP
• Viscoelas
tic
• No Function • Williams-Landel-Ferry • Power Series Expansion
2D Orthotro pic
• Linear Elastic
Option 4
Option 5
66
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Failure
Option 2
Option 3
• Stress
• n/a
• Strain
• Hill
Option 4
Option 5
• Hoffman • Tsai-Wu • Maximum Strain • Failure1/
• See Isotropic Entry
2/3 • Elastopla
stic
• Stress/Strain
Curve
• von
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y
• Piecewis
e Linear
• Cowper-
Symon ds
Chapter 2: Building A Model 67 Material Library
Object
Option 1
Option 2 • Hardening
Slope
Option 3 • von
Option 4
Option 5
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager • Perfectly
Plastic
• von
Mises • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • Creep
• MATVP
• Viscoelas
• See Isotropic Entry
tic 3D Orthotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure1/
• See 2D Orthotropic Entry
2/3 • Creep
• See 2D Orthotropic Entry
• None
• Piecewis
e Linear
• Cowper-
Symon ds
68
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Viscoelas
Option 2
Option 3
Option 4
Option 5
• See Isotropic Entry
tic 2D Anisotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure
• See Isotropic Entry
• Failure1/
• See Isotropic Entry - progressive failure not supported
2/3 3D Anisotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure1/
• See 2D Orthotropic Entry - progressive failure not supported
2/3 • Creep
Fluid
• Linear Elastic
Composi te
• Laminate
• See Isotropic Entry
• Rule of Mixtures • HAL Cont. Fiber • HAL Disc. Fiber • HAL Cont. Ribbon • HAL Disc. Ribbon • HAL Particulate • Short Fiber 1D • Short Fiber 2D
Chapter 2: Building A Model 69 Material Library
Additional materials for Explicit Nonlinear (SOL 700) are listed in the following table. Object Isotropic
Option 1 • Linear Elastic
Option 2 • Linear Elastic
(MAT1) • Elastoplastic
• Plastic
Option 3 •
Option 4
Option 5
Solid
• Fluid • Bilinear
Kinematic(MAT 3) • Iso.Elastic
Plastic(MAT12) • Rate Dependent
(MAT19) • Piecewise Linear
(MAT24)
• Biliear
• Cowper Symonds
• Linearized
• General
• Table • Rate Sensitive
• Powerlaw
(MAT64) • Resultant (MAT28) • Shape Memory (MAT30) • With Failure (MAT13) • Power Law (MAT18) • Ramberg-Osgood (MAT80) • Hydro (MAT10)
• Linearized
• Viscoelastic
• Viscoelastic (MAT6)
• Rigid
• Material Type 20 • No Constraints • Global Directions • Local Directions • MATRIG (Rigid
• Geometry Body Properties) • Defined
• No Constraints • Global Directions • Local Directions
• Johnson Cook
• Material Type 15 • No
iteractions • Accurate
• Minimum Pressure • No Tension, Min. Stress • No Tension, Min.
Pressure
70
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Rubber
Option 2 • Frazer Nash
(MAT31)
Option 3
Option 4
• Coefficient
• Respect
• Least Square
• Ignore
Option 5
Fit • Blatz-Ko (MAT7) • General Viscoelastic (MAT76) • Cellular Rubber (MAT87) • Mooney Rivlin
(MAT27)
• Coeff. • Least Square
• Arruda-Boyce
(MAT127) • Hyperelastic
(MAT77) • Simplified
• Coefficients • Least Square Fit 1/2/3 • Tension-
Compresion Load • Compression
• True Strain • Simple • Engineering
Average
Strain Rate • 12 Point Average
Load • Tension-
Compressio n Identical • Foam
• Soil and Foam
(MAT5/14)
• Active
(MAT14)
• Allow Crushing • Reversible
• Inactive
(MAT 5) • Low Density
Urethane (MAT57) • Fu Chang Foam
(MAT83) • Low Density
Urethane (MAT57)
• Bulk
Viscosity Inactive
• No Tension • Maintain Tension
• Bulk
Viscosity Active • Bulk
Viscosity Inactive • Bulk
Viscosity Active
• No
Tension • Maintain
Tension
• With
Relaxati on curve • No
Relaxati on Curve
Chapter 2: Building A Model 71 Material Library
Object
Option 1
Option 2
Option 3
Option 4
Option 5
• Viscous Foam (MAT62) • Crushable (MAT63) • Elastoviscoplatic • With Damage
• Strain
(MAT81)
Damage • Orthotropic
• Bilinear • Linearized • Table
• RCDC • Discrete Beam
• Cowper
Symond s • General
• Nonlinear Elastic Discrete Beam (MAT67) • Nonlinear Plastic Discrete Beam (MAT68) • Side Impact Dummy (SID) Damper Discrete Beam (MAT69) • Hydraulic Gas Damper Discrete Beam (MAT70) • Cabel Discrete Beam (MAT71) • Elastic Spring Discrete Beam (MAT74) • Elastic 6 DOF Spring Discrete Beam (MAT93) • Inelastic Spring Discrete Beam (MAT94) • Inelastic 6 DOF Srping Discrete Beam (MAT95) • General Joint Discrete Beam (MAT97)
• Spring Damper • Nonlinear 6
• Follow Loading Curve DOF Discrete • Follow Unloading Curve Beam (MAT119) • Follow Unloading Stiffness • General • Follow Quadratic Unloading Nonlinear 1 DOF Discrete Beam (MAT121) • Elastic Spring (MATDS01) • Viscous Damper (MATDS02) • Elastic Spring (MATDS03) • Nonlinear Elastic Spring (MATDS04) • Nonlinear Viscous Damper (MATDS05) • General Nonlinear Spring (MATDS06) • Spring Maxwell (MATDS07) • Inelastic Spring (MATDS08) • Tri-linear Degrading (MATDS13) • Squat Shear Wall (MATDS14) • Muscle (MATDS15)
72
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1
Option 2
Option 3
• Seat Belt
• Seat Belt (MATB01)
• Spotweld
• MATDSW1
• DF
• MATDSW2
• DFRES
Option 4
Option 5
• DFRESNF • DFRESNFP • MATDSW3
• DFSTR
• MATDSW4
• DFRATE
• MATDSW5
• DFNS • DFSIF • DFSTRUC
2D Orthotro pic
• Glass
• Laminated Glass
(Laminated) • Composite
(MAT32) • Enh. Composite
Damage
• Glass • Polymer • Tsai-Wu Theory • Chang-Chang Theory
• Linear Elastic
• Linear Elastic (MAT2)
• Composites
• Composites and
and Fabrics
Fabrics (MAT58)
• Zero
• 0.0
• One
• 1.0
• Two
• -1.0
• Three
3D Orthotro pic
• Honeycomb
• Composite
•
Composite Honeycomb (MAT26)
• Bulk Viscosity Inactive • Bulk Viscosity Active
• Composite Damage (MAT22) • Composite
• Faceted Failure (MAT59) • Ellipsoidal
• Linear Elastic
• Linear Elastic (MAT2)
• Modified
•
Honeycomb
Modified Honeycomb (MAT126)
• Bulk
Viscosity Inactive • Bulk
Viscosity Active
• LCA .LT.
0 • LCA .GT.
0
• Zero • One • Two
Chapter 2: Building A Model 73 Material Library
Object 2D Anisotro pic 3D Anisotro pic
Option 1 • Viscoplastic
Option 2 • Viscoplastic
Option 3 • Shell
(MAT103)
Option 5
• From Curve • Manual Entry
• Linear Elastic
• Linear Elastic (MAT2)
• Viscoplastic
• Viscoplastic
• Brick
(MAT103) • Linear Elastic
Option 4
• From Curve • Manual Entry
• Linear Elastic (MAT2)
Linear Elastic The Input Properties form displays the following for linear elastic properties. The translator produces MAT1 entries for isotropic materials, MAT8 entries for 2D orthotropic materials, MAT3 entries using axisymmetric solid elements or MAT9 entries using 3D solid elements (CHEXA, CPENTA, CTETRA) for 3D orthotropic materials, MAT2 entries for 2D plane stress - 2D anisotropic materials, and MAT9 entries for 3D anisotropic materials. For temperature dependencies, the corresponding MATTi entries are written referencing TABLEMi entries. Temperature dependency is defined using material fields defined under the Fields application. SOL 600 jobs using 3D Orthotropic material the MATORT entry is written. Isotropic
Description
Elastic Modulus
Elastic modulus, E, (Young’s modulus). Can be temperature dependent.
Poisson Ratio
Poisson’s ratio (NU). Can be temperature dependent. Should be between -1.0 and 0.5.
Shear Modulus
Shear modulus (G). Can be temperature dependent.
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient
Thermal coefficient of expansion (A). Can be temperature dependent.
Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
2D/3D Orthotropic
Description
Elastic Modulus ii
Modulus of elasticity in 1-, 2-, and 3-directions. Can be temperature dependent.
Poisson Ratio ij
Poisson’s ratio for uniaxial loading in the three different directions. Can be temperature dependent.
Shear Modulus ij
In-plane and transverse shear moduli in ij planes. Can be temperature dependent.
74
Patran Interface to MD Nastran Preference Guide Material Library
2D/3D Orthotropic
Description
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient ii Thermal coefficients of expansion in the three directions. Can be temperature dependent. Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
2D/3D Anisotropic
Description
Stiffness ij
Elements of the 6x6 symmetric material property matrix in the material coordinate system. Can be temperature dependent.
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient ij Thermal coefficients of expansion. Can be temperature dependent. Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
Nonlinear Elastic The Input Properties form displays the following for nonlinear elastic properties. Use this form to define the nonlinear elastic stress-strain curve on the MATS1 entry. A stress-strain table defined using the Fields application can be selected on this form. Based on this information the translator will produce MATS1 of type NLELAST and TABLES1 entries. This is used primarily for SOL 106 and 129. This option is not supported by SOL 600. Use an elastoplastic constitutive model instead. Isotropic
Description
Stress/Strain Curve
Defines the nonlinear elastic stress-strain curve. You must select a field from the listbox. It can be strain and/or temperature dependent. Tabular definition of the stress-strain curve via the Fields application using a material field of strain should follow the specifications as outlined by Nastran. The first point of the material field should be the origin and the second point must be at the initial yield point. This material curve is elastic, meaning that in both loading and unloading the material behavior follows the stress-strain curve as defined. It is not recommended that both nonlinear elastic and elastoplastic constitutive models be active or defined for the same material. For work hardening, use the Elastoplastic constitutive model. See the Nastran Quick Reference Guide for more details.
Chapter 2: Building A Model 75 Material Library
Hyperelastic The Input Properties form displays the following for hyperelastic properties. Use this form to define the data describing hyperelastic behavior of a material. This data is placed on MATHP and TABLES1 entries or on the MATHE entry for SOL 600. If you select Test Data as the Data Type, the Input Options form reverts to the form used for non-SOL 600 solutions and data is placed on a MATHP entry (Mooney-Rivlin strain energy model). To use test data for MATHE/SOL 600 runs, use the Experimental Data Fitting features under the Tools menu to determine the coefficients and enter them manually. Test Data - Mooney Rivlin
Description
Tension/Compression TAB1
All data provided must reference a strain dependent field defining the test data. Please refer to the Nastran Quick Reference Guide for descriptions of each of these tabular inputs.
Equibiaxial Tension TAB2 Simple Shear Data TAB3 Pure Shear Data TAB4 Pure Volume Compression TABD
If Coefficients is selected as the Data Type, use the form to describe the strain energy potential. The Mooney Rivlin model can be written out as a MATHP or MATHE entry for SOL 600. Make sure you use the one that is consistent with the solution to be run. Ogden, Foam, Arruda-Boyce, and Gent models are used for SOL 600 MATHE entries only. Mooney Rivlin (MATHP)
Description
Distortional Deformation Coefficients, Aij
Material constants related to distortional deformation. The Order of the Polynomical determines the number of coefficients required as input.
Volumetric Deformation Coefficients, Di
Material constants related to volumetric deformation. The Order of the Polynomial determines the number of coefficients required as input.
Density RHO
Defines the mass density which is an optional property.
Volumetric Thermal Expansion Coefficient AV Coefficient of volumetric thermal expansion. Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Structural Damping Coefficient GE
Structural damping element coefficient.
76
Patran Interface to MD Nastran Preference Guide Material Library
Mooney Rivlin (MATHE)
Description
Strain Energy Function C10, C01, C11, C20, C30
Strain energy densities as a function of the strain invariants in the material. May vary with temperature via a defined material field. This option consolidates several of the hyperelastic material models, including Neo-Hookean (C10 only), Mooney-Rivlin (C10 & C01), and Full Third Order Invariant (all coefficients).
Density RHO
Defines the mass density
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field.
Bulk Modulus K
Defines the Bulk Modulus.
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Structural Damping Coefficient GE
Structural damping element coefficient.
Ogden
Description
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
Defines the material mass density.
Coefficient of Thermal Expansion
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Modulus k
k
in the Ogden equation. The number of
moduli required as input is dependent on the Order of the Polynomial. Exponent k
k
in the Ogden equation. The number of
exponents required as input is dependent on the Order of the Polynomial.
Foam
Description
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
Defines the material mass density.
Chapter 2: Building A Model 77 Material Library
Foam
Description
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Modulus n
un
in the Foam equation. The number of moduli
required as input is dependent on the Order of the Polynomial. Deviatoric Exponent n
n
in the Foam equation. The number of
exponents required as input is dependent on the Order of the Polynomial. Volumetric Exponent n
n
in the Foam equation. The number of
exponents required as input is dependent on the Order of the Polynomial.
78
Patran Interface to MD Nastran Preference Guide Material Library
Arruda- Boyce
Description
NKT
Chain density times Boltzmann constant times temperature. May vary with temperature via a defined material field.
Chain Length
Average chemical chain cross length. May vary with temperature via a defined material field.
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
This defines the material mass density.
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Gent
Description
Tensile Modulus
Defines standard tension modulus (E). May vary with temperature via a defined material field.
I 1*
Maximum 1st Invariant
Defines
*
I1 = I1 – 3
. May vary with
temperature via a defined material field. Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
This defines the material mass density.
Coefficient of Thermal Expansion
Defines the coefficient of thermal expansion.
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Elastoplastic The Input Properties form displays the following for elastoplastic properties. Use this form to define the data describing plastic behavior of a material. The stress-strain curve data is input via a material property field of strain and placed on MATS1 and TABLES1 entries. The data input should be the true equivalent stress vs. equivalent total strain. Other options are placed on the MATEP entry and are valid only for SOL
Chapter 2: Building A Model 79 Material Library
400 & 600. Note that the existence of both an elastoplastic and nonlinear elastic constitutive models in the same material is not recommended. Stress/Strain Curve
Description
Yield Function
Yield function (YF) criterion: von Mises, Tresca, Mohr-Coulomb, & DruckerPrager supported on MATS1 entry. All others are for SOL 600 and placed on the MATEP entry. SOL 400 only supports von Mises.
Hardening Rule
Hardening Rule (HR). These are Isotropic, Kinematic, and Combined isotropic and kinematic and are placed on the MATS1 entry or MATEP entry depending on solution sequence and yield function selected. Hardening rules Power Law, Rate Power Law, Johnson-Cook, Kumar are available when no Yield Function is specified. This is used for SOL 600 only on MATEP entry.
Strain Rate Method
Selects an option for strain-rate dependent yield stress used in SOL 600. Cowper-Symonds requires input of Denominator C and Inverse Exponent P.
Stress/Strain Curve
This data must reference a strain dependent field. It can also be temperature and strain rate dependent. LIMIT1 in MATS1 determined from supplied tabular field of stress-strain curve. Data is placed on TABLES1 entry.
Internal Friction Angle
Defined for Mohr-Coulomb and Drucker-Prager yield function placed on the MATS entry LIMIT2.
Yield Point
Initial yield stress.
Stress at Yield Beta
Parameter beta for parabolic Mohr-Coulomb or Buyukozturk concrete models. Placed on the MATEP entry.
10th Cycle Yield Stress
Equivalent 10th cycle tensile yield stress for Oak Ridge National Labs models (ORNL). Placed on the MATEP entry.
Denominator C
Constants for the Cowper-Symonds strain rate method.
Inverse Exponent P
80
Patran Interface to MD Nastran Preference Guide Material Library
Stress/Strain Curve
Description
Coefficient A / B / C / Bi
Coefficient and exponent data for Power Law, Rate Power Law, Johnson-Cook, and Kumar hardening rules.
Exponent M / N initial Strain Rate Room Temperature
Additional data input for the Johnson-Cook hardening rule.
Melt Temperature
Hardening Slope
Description
Yield Function
Yield function (YF) criterion: von Mises, Tresca, Mohr-Coulomb, & DruckerPrager supported on MATS1 entry.
Hardening Rule
Hardening Rule (HR). These are Isotropic, Kinematic, and Combined isotropic and kinematic and are placed on the MATS1 entry.
Strain Rate Method
No strain rate methods are available for the Hardening Slope data.
Hardening Slope
Work hardening slope (H) - slope of stress versus plastic strain. Defined in units of stress. For an elastic-perfectly plastic case, use the Perfectly Plastic data input option.
Internal Friction Angle
Defined for Mohr-Coulomb and Drucker-Prager yield function placed on the MATS entry LIMIT2.
Yield Point
Initial yield stress.
Perfectly Plastic
Description
Yield Function
See the Stress / Strain Curve table above. All options are identical except there must be a yield function selected.
Hardening Rule
None are available since no hardening is possible for a perfectly plastic material.
Strain Rate Method
Piecewise linear or Cowper-Symonds are available.
Chapter 2: Building A Model 81 Material Library
Perfectly Plastic
Description
Yield Point
Initial yield stress.
All other data input is described in the Stress/Strain Curve table above.
Rigid Plastic
Description
Yield Function
No yield functions are available as the material is defined as rigid and then plastic, so no yield is possible.
Hardening Rule
See the Stress / Strain Curve table above. Valid options are the Power Law, Power Rate Law, Johnson-Cook, Kumar, and Piecewise Linear.
Strain Rate Method
Piecewise linear or Cowper-Symonds are available only if the Piecewise Linear hardening rule is selected.
Stress/Strain Curve
Necessary only when not using one of the power law hardening rules (Piecewise-Linear). This data must reference a strain dependent field. It can also be temperature and strain rate dependent. LIMIT1 in MATS1 determined from supplied tabular field of stress-strain curve. Data is placed on TABLES1 entry.
All other data input is described in the Stress/Strain Curve table above. Rigid Plastic is only used in SOL 600 and only for isotropic materials. See the Nastran Quick Reference Guide for more information about the necessary data for MATS1 and MATEP entries. Failure The Input Properties form displays the following for failure material models. Note that this failure model is for non-SOL 400/600/700 solutions. See Failure 1/2/3 for SOL 400/600/700. No Composite Failure Theory
Description
Tension Stress Limit
Stress limits for tension, compression, and shear used to compute margins of safety in certain elements. They have no effect on the computational procedures.
Compression Stress Limit Shear Stress Limit
Failure criteria for the isotropic and two-dimensional orthotropic and anisotropic materials appear in the ST, SC, and SS fields on MAT1 and MAT2 entries and the Xt, Xc, Yt, Yc, and S fields on the MAT8 entry.
82
Patran Interface to MD Nastran Preference Guide Material Library
Composite Failure Theory:
Description
Hill, Hoffman, Tsai-Wu, Maximum Failure Limits
For 2D orthotropic on the MAT8 entry, the limits can be defined as stress or strain allowables. This is not applicable to isotropic and anisotropic materials.
Tension Stress Limit
Stress limits for tension, compression, and shear are the same as those defined for non-composite failure.
Compression Stress Limit Shear Stress Limit Bonding Shear Stress Limit
Allowable shear stress of the bonding material. SB field on the PCOMP entry.
Failure criteria for the isotropic and two-dimensional orthotropic and anisotropic materials appear in the ST, SC, and SS fields on MAT1 and MAT2 entries and the Xt, Xc, Yt, Yc, and S fields on the MAT8 entry unless composites are being used in which case the data is written to the PCOMP entry as necessary. Failure 1, Failure 2, Failure 3 The Input Properties form displays the following for failure material models used in SOL 400 and 600. Solution sequences other than SOL 400/600/700 should use the Failure constitutive model above instead. Up to three failure constitutive models can be defined for any one material. Failure 1 must exist in order for Failure 2 and 3 to be recognized and translated into the proper MATF and MATTF entries. Temperature dependent properties as defined by material fields are translated onto the MATTF entry. Note also that only Failure 1 allows for definition of progressive failure. Failure models 2 and 3 take on whatever progressive failure is defined in Failure 1. Different failure criterion may exist between all three in the same material definition. The table below outlines the allowable properties. All values are real, 0.0, or left blank with no defaults unless otherwise indicated. Which properties are available is dependent on the Failure Criterion selected. The following Failure Criteria are available: • Maximum Stress • Maximum Strain • Hill • Hoffman • Tsai-Wu • Hashin • Puck • Hashin-Tape
Chapter 2: Building A Model 83 Material Library
• Hashin-Fabric
Property
Description
Progressive Failure Options
Progressive failure options are None, standard Progressive Failure, Gradual or Immediate selective progressive failure for SOL 600. SOL 400 does not support progressive failure models and will ignore this setting if set to anything other than None. Only failure indices are computed when no progressive failure is specified. Anisotropic materials do not support progressive failure.
Tension Stress Limit X / Y /Z Tension Strain Limit X / Y / Z
Tension, compression, and shear stress or strain limits used in the Maximum Stress or Strain, Hill, Hoffman, and Tsai-Wu failure criteria.
Compression Stress Limit X / Y / Z Compression Strain Limit X / Y / Z Shear Stress Limit XY / YZ / ZX Shear Strain Limit XY / YZ / ZX Shear Stress Bond (SB)
Allowable shear stress of bonding material between layers for composites only. This is used in SOL 600 only and is ignored for SOL 400.
Failure Index
Failure index used for Hill, Hoffman, and Tsai-Wu criteria.
Interactive Strength XY / YZ / ZX
Interactive strength constants for specified plane used in the Tsai-Wu criterion.
Max Fiber / Matrix Tension Max Fiber / Matrix Compression
Definable stress limits for Hashin, Puck, HashinTape, and Hashin-Fiber criteria.
Max Tape Fiber Tension Max Tape Fiber Compression Max 1st Fiber Tension / Compression Max 2nd Cross Fiber Tension / Compression Max Thickness Tension Max Thickness Compression Layer Shear Strength Transverse Shear Strength YZ / ZX
Shear stress limits for Hashing, Puck, Hashin-Tape, and Hashin-Fiber criteria.
Slope P12C / P12T / P23C / P23T of Fracture Envelope
Slopes of the failure envelope used in Puck failure criterion.
84
Patran Interface to MD Nastran Preference Guide Material Library
Property
Description
Deactivate Tension X / Y/ Z Deactivate Compress X / Y / Z Deactivate Shear XY / YZ / ZX
If any value other than blank or 0.0 is entered for progressive failure options Gradual and Immediate, failed elements are deactivated (placed ICi fields in MATF entry). See the Nastran Quick Reference Guide for information.
Deactivate Elements Deactivate Fiber / Matrix Tension Deactivate Fiber /Matrix Compression Deactivate Matrix Tension Deactivate Matrix Compression Residual Stiffness Factor Matrix Compression Factor Shear Stiffness Factor E33 Fiber Failure Factor Shear Fiber Failure Factor
Reduction fractions or factors. Values can be between 0.0 and 1.0. Used only for Gradual or Immediate progressive failure modes (placed on Ai fields in MATF entry). See the Nastran Quick Reference Guide for more information.
Creep The Input Properties form displays the following for creep models. Tabular Input
Description
Data defined by the use of this form to define the primary stiffness, primary damping, and secondary damping for a creep model with tabular input appears on the CREEP entry for non-SOL 600 runs. Only isotropic materials use this data input method. Creep Law ijk
Description
Use this form to define the coefficients for one of many empirical creep models available appears on the CREEP entry for non-SOL 600 runs. Only isotropic materials use this creep definition. MATPV
Description
Use this form to define either the coefficients and exponents for creep model or provide tabular field data to define Temperature vs. Creep Strain, Creep Strain Rate vs. Stress, Strain Rate vs. Creep Strain, or Time vs. Creep Strain in SOL 600 runs. This data is written to the MATVP entry. If tabular data is provided, this data is written to TABLEM1 entries. It is not recommended to mix the exponents and coefficients and tabular data. Use one or the other.
Chapter 2: Building A Model 85 Material Library
Viscoelastic The Input Properties form displays the following for viscoelastic models. This material model is only used in SOL 600 runs and all data is placed on the MATVE, MATTVE entries. Linear elastic or hyperelastic constitutive models for isotropic or anisotropic materials must exist in addition to the viscoelastic model. Composite The Composite forms provide alternate ways of defining the linear elastic properties of materials. All the composite options, except for Laminated Composite, will always result in a homogeneous elastic material in MD Nastran. When the Laminated Composite option is used to create a material and this material is then referenced in a “Revised or Standard Laminate Plate” element property region, a PCOMP entry is created. However, if this material is referenced by a different type of element property region, for example, “Revised or Standard Homogeneous Plate,” then the equivalent homogeneous material properties are used instead of the laminate lay-up data. Only materials created through the Laminated Composite option should be referenced by a “Revised or Standard Laminate Plate” element property region. Refer to Composite Materials Construction (p. 116) in the Patran Reference Manual. Laminated
This subordinate form appears when the Input Properties button is selected on the Materials form, Composite is the selected Object, and Laminate is the selected Method. Use this form to define the laminate lay-up data for a composite material. If the resulting material is referenced in a “Revised or Standard Laminate Plate” element property region, then an MD Nastran PCOMP entry containing the lay-up data is written. If the resulting material is referenced by any other type of element property region, the equivalent homogeneous properties of the material are used
86
Patran Interface to MD Nastran Preference Guide Material Library
.
Chapter 2: Building A Model 87 Element Properties
2.7
Element Properties The Element Properties form appears when the Element Properties toggle, located on the Patran main form, is chosen.There are several option menus available when creating element properties. The selections made on the Element Properties menu will determine which element property form appears, and ultimately, which MD Nastran element will be created. The following pages give an introduction to the Element Properties form, and details of all the element property definitions supported by the Patran MD Nastran Preference.
Element Properties Form This form appears when Element Properties is selected on the main menu. There are four option menus on this form. Each will determine which MD Nastran element type will be created and which property forms will appear. The individual property forms are documented later in this section. For a full description of this form, see Element Properties Forms (p. 67) in the Patran Reference Manual.
88
Patran Interface to MD Nastran Preference Guide Element Properties
Use this option menu to define the element’s dimension. The options are: 0D (point elements) 1D (bar elements) 2D (tri and quad elements) 3D (tet, wedge, and hex elements)
This option menu depends on the selection made in the Dimension option menu. Use this menu to define the general type of element, such as: Mass versus Grounded Spring Shell versus 2D_Solid
This button is used to quickly edit an element property; for example change the shell thickness.
These option menus may or may not be present, and their contents depend heavily on the selections made in Dimension and Type. See Table 2-1 for more help.
This is used to specify element properties; for example shell thickness, or material orientation. This is used to specify the region (area) of geometry or elements that are to be included in the property definition.
Chapter 2: Building A Model 89 Element Properties
The following table outlines the option menus when Analysis Type is set to Structural. Table 2-1
Structural Options
Dimension 0D
Type • Mass
Option 1
Option 2
• Coupled • Grounded • Lumped
• Grounded Spring • Grounded Damper • Grounded Bush
1D
• Beam
• General Section
• Standard • P-Formulation
• Curved w/General
Section • Curved w/Pipe
Section • Lumped Section • Tapered Section
• Standard • P-element
• General Section
•
(CBEAM) • Rod
• General Section
• Standard • CONROD
• Pipe Section • Spring • Damper
• Scalar • Viscous
• Gap
• Adaptive • Non-Adaptive
• 1D Mass • PLOTEL • Bush • Spot Weld Connector • Fastener Connector
90
Patran Interface to MD Nastran Preference Guide Element Properties
Table 2-1 Dimension 2D
Structural Options Type • Shell
Option 1 • Homogeneous
Option 2 • Standard • Revised • P-element
• Laminate
• Standard • Revised
• Equivalent Section
• Standard • Revised • P-element
• Field Point Mesh (exterior acoustic element) • Bending Panel
• Standard • Revised
•
• P-element •
• 2D-Solid
• Plane Strain
• Standard • Revised • P-Formulation • Hyperelastic Formulation
• Axisymmetric
• Standard • Hyperelastic Formulation • PLPLANE
• Infinite (exterior acoustic element) • Membrane
• Revised
• •
3D
• Standard • P-Formulation
• Shear Panel • Solid
• Homogeneous
• Standard • P-Formulation • Hyperelastic Formulation
• Laminate • Gasket
Chapter 2: Building A Model 91 Element Properties
Coupled Point Mass (CONM1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Coupled
Point/1
Use this form to create a CONM1 element. This defines a 6 x 6 symmetric mass matrix at a geometric point of the structural model.
92
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the orientation of the 1-2-3 axes of the mass matrix. The value is a reference to an existing coordinate frame. The 12-3 axes will be aligned with the X-Y-Z axes of the specified coordinate system. If a non rectangular coordinate system is specified, the system will be evaluated into a local rectangular system, which is then used to orient the mass matrix. This property is the CID field on the CONM1 entry. This property is optional.
Defines the values of the mass matrix. These properties are the Mij fields on the CONM1 entry and can either be real values or references to existing field definitions. Each of these properties are optional; however, at least one must be defined.
Chapter 2: Building A Model 93 Element Properties
This is a list of Input Properties available for creating a CONM1 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description Defines the values of the mass matrix. These are the Mij fields on the CONM1 entry. These properties can either be real values or references to existing field definitions. Each of these properties are optional; however, at least one must be defined.
Mass Component 3,3 Mass Component 4,1 Mass Component 4,2 Mass Component 4,4 Mass Component 5,1 Mass Component 5,2 Mass Component 5,3 Mass Component 5,4 Mass Component 5,5 Mass Component 6,1 Mass Component 6,2 Mass Component 6,3 Mass Component 6,4 Mass Component 6,5 Mass Component 6,6
Grounded Scalar Mass (CMASS1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Grounded
Point/1
Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model. Only one node is used in this method, and the other node is defined to be grounded.
94
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the translation mass or rotational inertia value to be applied. This is the M field on the PMASS entry. This property can be either a real value or a reference to an existing field definition. This property is required.
Defines which degree of freedom this value will be attached to. This property can be set to UX, UY, UZ, RX, RY, or RZ and defines the setting for the C1 field on the CMASS1 entry. This property is required.
Lumped Point Mass (CONM2) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Lumped
Point/1
Use this form to create a CONM2 element. This defines a concentrated mass at a geometric point of the structural model.
Chapter 2: Building A Model 95 Element Properties
Defines an offset from the specified node to where the lumped mass actually is to exist in the structural mode. This vector is defined in the Mass Orientation coordinate system. Defines the X1, X2, and X3 fields on the CONM2 entry. This property is optional.
Defines the translational mass value to be used. This is the M field on the CONM2 entry. This property can either be a real value or a reference to an existing field definition. This property is required.
Defines the orientation of the 1-2-3 axes of the mass matrix. This is a reference to an existing coordinate frame. The 1-2-3 axes will be aligned with the X-Y-Z axes of the specified coordinate system. If a nonrectangular coordinate system is specified, the system will Inertia i,j defines the rotation inertia properties of be evaluated into a local rectangular system, this lumped mass. These properties are the Iij which is then used to orient the mass matrix. fields on the CONM2 record. These values can This is the CID field on the CONM2 entry. If the be either real values or references to existing Value Type is set to Vector then the field definitions. These values are optional. components of the vector define the center of gravity of the mass in the basic coordinate system and the field for CID is translated as -1. This property is optional.
This is a list of Input Properties available for creating a CONM2 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.
96
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description Inertia i,j defines the rotation inertia properties of this lumped mass. These are the Iij fields on the CONM2 entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 3,1 Inertia 3,2 Inertia 3,3
Grounded Scalar Spring (CELAS1/CELAS1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen. Action
Dimension
Type
Create
0D
Grounded Spring
Option(s)
Topologies Point/1
Chapter 2: Building A Model 97 Element Properties
Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring element of the structural model. Only one node is used in this method. The other node is defined to be grounded. Defines the coefficient to be used for this spring. This is the K field on the PELAS entry. This can either be a real value or a reference to an existing field definition. This property is required.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Defines the relationship between the spring deflection and the stresses within the spring. This property is the S field on the PELAS entry and can either be a real value, or a reference to an existing field definition. This property is optional.
Defines what damping is to be included. This is the GE field on the PELAS entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
Defines which degree of freedom this value is to be attached to. This can be set to UX, UY, UZ, RX, RY, or RZ. This property defines the setting of the C1 field on the CELAS1 entry. This property is required.
98
Patran Interface to MD Nastran Preference Guide Element Properties
Grounded Scalar Damper (CDAMP1/CDAMP1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen. Action
Dimension
Type
Create
0D
Grounded Damper
Option(s)
Topologies Point/1
Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model. Only one node is used in this method. The other node is defined to be grounded.
Defines the force per unit velocity value to be used. This property is the B field on the PDAMP entry and can either be a real value or a reference to an existing field definition. This property is optional.
Defines which degree of freedom this value is to be attached to. This property can be set to UX, UY, UZ, RY, or RZ and defines the setting for the C1 field on the CDAMP1 entry. This property is required.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Chapter 2: Building A Model 99 Element Properties
Bush This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Bush
Option(s)
Topologies Bar/2
100
Patran Interface to MD Nastran Preference Guide Element Properties
This toggle can also be set to Node Id or CID..
Chapter 2: Building A Model 101 Element Properties
This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bush Orientation System
CID specifies the Grounded Bush Orientation System. The element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the grid point specified locates the system. If CID = 0, the basic coordinate system is used.
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6
Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6
Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6
Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend
Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation
Stress recovery coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation
Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.
102
Patran Interface to MD Nastran Preference Guide Element Properties
General Section Beam (CBAR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
General Section
Bar/2
Chapter 2: Building A Model 103 Element Properties
Use this form to create a CBAR element and a PBAR or PBARL property. A CBARAO entry will be generated if any Station Distances are specified. This defines a simple beam element in the structural model.
Note:
CBAR entries will include all user input pin flags.
104
Patran Interface to MD Nastran Preference Guide Element Properties
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, (for the standard Beam Library) or PBRSECT/PBMSECT (for an Arbitrary section) will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the value to be used in the MID field on the PBAR entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBAR entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBAR entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBAR entry.
Chapter 2: Building A Model 105 Element Properties
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBAR entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBAR entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
These degrees of freedom are in the element local coordinate system. Values that can be specified are UX, UY, UZ, RX, RY, RZ, or any combination. These properties are used to remove connections between the node and selected degrees of freedom at the two ends of the beam. This option is commonly used to create a pin connection by specifying RX, RY, and RZ to be released. Defines the setting of the PA and PB fields on the CBAR record. These properties are optional.
Area
Defines the cross-sectional area of the element. This is the A field on the PBAR entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1
Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 2,2 Inertia 2,1
106
Patran Interface to MD Nastran Preference Guide Element Properties
Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBAR entry. These values can be either real value or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBAR entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C
Indicates the stress recovery. They define the Y and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C Y of Point D Z of Point D Y of Point E Z of Point E Y of Point F Z of Point F [Contact Beam Radius]
This allows the equivalent radius for beam-to-beam contact to be different for each beam cross section. The MD Nastran entry BCBMRAD is written to the .bdf file. The BCBMRAD entry format is different for SOL 400 and SOL 600.
[Station Distances]
Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO entry is not supported. These values are real values. These properties are optional.
Create Sections, I C L ..., Beam Library
Activates the Beam Library forms. These forms will allow the user to define beam properties by choosing a standard cross section type and inputing dimensions.
Chapter 2: Building A Model 107 Element Properties
P-Formulation General Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
General Section
Bar/2, Bar/3
P-Formulation
Bar/4
Use this form to create a CBEAM element and a PBEAM or PBEAML property. This form defines a simple beam element in the structural model for an adaptive, p-element analysis. Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
108
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam, and this orientation vector, which can be defined as either a vector or a reference to an existing node, is in the XY plane. This defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
Input Properties
Allows a beam section previously created using the beam library to be selected. When a beam section is chosen and the Associate Beam Section option is toggled, the cross sectional properties need not be input on this Input Properties form. Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the value to be used in the MID field on the PBAR entry. This property is required. Allows a user to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Activates the Beam Library forms. These forms will allow the user to define beam properties by choosing a standard cross section type and inputting dimensions.
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. On the CBEAM entry, these values are always in the displacement coordinate a system specified such as <0 1 0 Coord 5>. These properties are optional.
Chapter 2: Building A Model 109 Element Properties
This is a list of Input Properties available for creating a CBEAM element and a PBEAM or PBEAML property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Area
Defines the cross-sectional area of the element. This is the A field on the PBEAM entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1
Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 2,2 Inertia 2,1 Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBEAM entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBEAM entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C
Indicates the stress recovery. Define the Y and Z coordinates of the stress recovery points across the section of the beam as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C X of Point D Y of Point D X of Point E Y of Point E X of Point F Y of Point F Station Distances
Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO records is not supported. These values are real values. These properties are optional.
110
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description
Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting Porders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum Porders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The two sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Curved General Section Beam (CBEND) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Curved w/General Section
Bar/2
Use this form to create a CBEND element and a PBEND property. This form defines a curved beam element of the structural model. The CBEND element has several ways to define the radius of the bend and the orientation of that curvature.This element in Patran always uses the method of defining the center of curvature point (GEOM=1). An alternate property of the Curved Pipe element also exists.
Chapter 2: Building A Model 111 Element Properties
Defines the center of curvature of the pipe bend. It is done by either specifying a vector from the first node of the element or by referencing a node. The CBEND element in MD Nastran has several ways to define the radius of the pipe bend and the orientation of that curvature. This defines the settings of the X1, X2, X3, and G0 fields of the CBEND entry. This property is required.
Defines the cross-sec This property is the A This value can be eith to an existing field def optional.
112
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties available for creating a CBEND element and a PBEND property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Inertia 1,1 Inertia 2,2
Description Defines the various area moments of inertia of the cross section. These properties are the I1 and I2 fields on the PBEND entry. These values can either be real values or references to existing field definitions. These values are optional.
Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBEND entry. This value can be either a real value, or a reference to an existing field definition. This property is optional.
Shear Stiff, R
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can be either real value or a reference to an existing field definition. This property is optional.
Radial NA Offset
Defines the radial offset of the geometric centroid from the end nodes. Positive values move the centroid of the section towards the center of curvature of the pipe bend. This property is the DELTAN field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
R of Point C
These properties are for stress recovery. They define the R and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These properties are the C1, C2, D1, D2, E1, E2, F1 and F2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C R of Point D Z of Point D R of Point E Z of Point E R of Point F Z of Point F
Chapter 2: Building A Model 113 Element Properties
Curved Pipe Section Beam (CBEND) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Curved W/Pipe Section
Bar/2
Use this form to create a CBEND element and a PBEND property. This defines a curved pipe or elbow element of the structural model. The internal pressure is defined as part of the element definition because, for pipe elbows, the internal pressure affects the element stiffness.
114
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when Defines the data is entered. Either select from the list using the mouse, or type in the name. Defines the MID center of curvature of the field on the PBEND entry. This property is required. pipe bend. This can be done either by specifying a vector from the first node of the element or by referencing a node. The CBEND element in MD Nastran has several ways to define the radius of the pipe bend and the orientation of that curvature. Defines the settings of the X1, X2, X3, and G0 fields on the CBEND entry. This element in Patran always uses the method of defining the center of curvature point Indicates the wall thickness of the pipe. This is the t field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the offset from the nodes to the actual centroids of the pipe cross section. These are the RC and ZC fields on the PBEND entry. These values can either be real values or references to existing field definitions. These properties are optional.
Indicates the distance from the centroid of cross section to mid-wall location. This is t on the PBEND entry. This value can either value or a reference to an existing field de This property is required.
Chapter 2: Building A Model 115 Element Properties
This is a list of Input Properties available for creating a CBEND element and a PBEND property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Internal Pipe Pressure
Indicates the static pressure inside the pipe elbow. This is the P field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can either be a real value or a reference to an existing field definition. This property is optional.
Stress Intensification
Indicates the desired type of stress intensification to be used. This is a character string value. This property is the FSI field on the PBEND entry. Valid settings of this parameter are General, ASME, and Welding Council.
Lumped Area Beam (CBEAM/PBCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Lumped Section
Bar/2
Use this form to create a CBEAM element and a PBCOMP property. This defines a beam element of constant cross section, using a lumped area element formulation.The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.
116
Patran Interface to MD Nastran Preference Guide Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Chapter 2: Building A Model 117 Element Properties
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type
The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.
• Reference Coordinates
Analysis - Analysis Coordinate System. Coord 0 - Basic Coordinate System.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. On the CBEAM entry, these values are always in the displacement coordinate system of the node. In Patran, they are either global, or in a system specified such as <0 1 0 Coord 5>. These properties are optional.
• Value Type
Specifies that the offset is defined in terms of a vector.
• Reference Coordinates
Analysis - Analysis Coordinate System. Element - Element Coordinate System.
118
Patran Interface to MD Nastran Preference Guide Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Warp DOF @ Node 1 Warp DOF @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Defines a node ID where the warping degree-of-freedom constraints and results will be placed. These must reference existing nodes within the model. They are the SA and SB fields on the CBEAM entry. These properties are optional.
Area
Defines the cross-sectional area of the element. This is the A field on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBCOMP record. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Z Y of NSM Z of NSM
Symmetry Option
Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These properties are the M1 and M2 fields on the PBCOMP entry. These values can be either real values or references to existing field definitions. These properties are optional. Specifies which type of symmetry is being used to define the lumped areas of the beam cross section. This is a character string parameter. The valid settings are No Symmetry, YZ Symmetry, Y Symmetry, Z Symmetry, or Y=Z Symmetry. This defines the setting of the SECTION field on the PBCOMP entry. This property is optional.
Chapter 2: Building A Model 119 Element Properties
Ys of Lumped Areas Zs of Lumped Areas Area Factors
Defines the locations of the various lumped areas. These are defined in the cross-sectional coordinate system. These properties define the Yi and Zi fields on the PBCOMP entry. These values are lists of real values. These properties are optional. Defines the Fraction of the total area to be included in this lumped area. The sum of all area factors for a given section must equal 1.0. If the data provided does not meet this requirement, the values will all be scaled to the corrected value. These properties define the values for the Ci fields on the PBCOMP entry. These values are lists of real values. These properties are optional.
Tapered Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Tapered
Bar/2
120
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CBEAM element and a PBEAM or PBEAML property. This defines a beam element with varying cross sections.
Chapter 2: Building A Model 121 Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
122
Patran Interface to MD Nastran Preference Guide Element Properties
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Chapter 2: Building A Model 123 Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Warp DOF @ Node 1 Warp DOF @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Defines a node ID where the warping degree of freedom constraints and results will be placed. These must reference existing nodes within the model. These are the SA and SB fields on the CBEAM entry. These properties are optional.
Station Distances
Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. These values are real values. These properties are optional.
Cross-Sect. Areas
Defines the cross-sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, or reference to an existing field definition. This property is required.
Inertias 1,1
Defines the various area moments of inertia of the cross section. These defines the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are real values. These properties are optional.
Inertias 2,2 Inertias 1,2 Torsional Constants
Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
Ys of C Points
Defines the Y and Z locations in element coordinates, relative to the shear center for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These are lists of real values, one for each station location. These properties are optional.
Zs of C Points Ys of D points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points
124
Patran Interface to MD Nastran Preference Guide Element Properties
Nonstructural Masses
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
NSM Inertia @ Node 1
Specified the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
NSM Inertia @ Node 2
Y of NSM @ Node 1
Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2 Shear Stiff, Y
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Z Shear Relief Y
Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Shear Relief Z Warp Coeff. @ Node 1 Warp Coeff. @ Node 2 Y of NA @ Node 1
Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional. Defines the offset from the centroid of the cross section to the location of the neutral axis. These values are measured in the beam cross section coordinate system and are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2
General Section Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Create
1D
Beam
General Section (CBEAM)
Chapter 2: Building A Model 125 Element Properties
This set of options provides a method of creating beam models with warping due to torsion. The capabilities of this beam properties formulation option are similar to those of the “Tapered Section” formulation, except that warping due to torsion is handled more conveniently.
126
Patran Interface to MD Nastran Preference Guide Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
Chapter 2: Building A Model 127 Element Properties
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
128
Patran Interface to MD Nastran Preference Guide Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. Pin or sliding type connections can be created by releasing specified degrees of freedom. These degrees of freedom are in the element local coordinate system. The values specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry. These properties are optional.
Warping Option
This specifies how contraints should be applied to the warping SPOINTs of unmatched ends within the application region (see continuity rules above). The choices available include “A free B free”, “A fixed B fixed”, “A free B fixed”, “A fixed B free”, or “None”. The choice of “None” is used to disable warping altogether for the current element property set, in which case no SPOINTs will be generated or constrained. Only unmatched ends within the application region will be eligible for constraining, and whether or not a constraint is applied will depend on the option selected, and whether the unmatched end is “End A” or “End B” of its beam element. If no selection is made for this element property, “A free B free” is selected by default.
Warp Coeff. @ Node 1 Warp Coeff. @ Node 2
Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Station Distances
Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. This field consists of a set of real values separated by legal delimiters, such as white space and/or commas. If this list is entered, then the properties that follow may also be in the form of lists consisting of the same number of values. If they are in the form of a single real value, then that value will apply to all stations of the beam element. This property is optional. If it is not provided, then all other specified section properties apply to the entire beam, and lists of values will not be accepted.
Cross-Sect. Areas
Defines the cross sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, a list (if a list of stations has been provided), or a reference to an existing field definition, in which case a single real value will be evaluated for each element of the application region. This property is required.
Chapter 2: Building A Model 129 Element Properties
Inertias 1,1 Inertias 2,2 Inertias 1,2
Defines the various area moments of inertia of the cross section. These values define the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or a list of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Torsional Constants
Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
Ys of C Points Zs of C Points Ys of D Points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points
Defines the Y and Z locations in element coordinates, relative to the shear center, for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or lists of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Nonstructural Masses
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
NSM Inertia @ Node 1 NSM Inertia @ Node 2
Specifies the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Y of NSM @ Node 1 Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2
Defines the offset from the shear center of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Y Shear Stiff, Z
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
130
Patran Interface to MD Nastran Preference Guide Element Properties
Shear Relief Y Shear Relief Z
Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Y of NA @ Node 1 Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2
Defines the offset from the shear center of the cross section to the location of the neutral axis. These values are measured in the beam cross-section coordinate system. These are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Warping due to torsion is enabled by generating MD Nastran SPOINTs to contain the warping degrees of freedom. These SPOINTs are not actually present in the Patran database, and there is no way to recover any results for these SPOINTs. They are created during analysis deck translation, and provide the means to communicate to MD Nastran the continuity and constraint properties of the warping degrees of freedom in the model. These attributes of continuity and constraint are implied in the Patran database through the composition of the element properties application region and the set of options selected. These continuity and constraint attributes apply to both warping SPOINTs and end release flags. This connection of these attributes to the composition of the application region is new in Patran 2001r3, and represents a change in behavior from previous versions of Patran. The general rules of implied continuity are as follows. 1. Within the application region, two beam elements are taken to be continuous if a GRID ID at an end of one of the beam elements matches a GRID ID at one of the ends of the other beam element. If a third beam element in the same application region also contains the same GRID ID, it is assumed that none of the beam elements is continuous at this location. This condition is known as a “multiple junction”. Similarly, if none of the other beam elements in the application region contain a matching GRID ID, the corresponding end of the beam element is taken to be not continuous. This condition is known as an “unmatched end”. 2. If warping is enabled, then all instances of beam element continuity must have the matching GRID ID located at “End A” of one of the beam elements and at “End B” of the other. “End A” and “End B” positions are determined by the order of GRID IDs specified in the element connectivity array, and the positive direction of the x-axis of the element coordinate system points from “End A” to “End B”. If warping is not enabled, this restiction does not apply. If warping is enabled, any violation of this requirement will result in a failure to complete the translation of the finite element model. In this event, the user will have to reverse the direction of the improperly oriented beam elements and initiate the translation again. 3. When warping is enabled, all positions of beam element continuity within an application region will be represented by a single SPOINT at each of these positions, which will be generated at the time of analysis deck translation and will appear on the CBEAM entries for the appropriate end of both of the beam elements that are continuous at each location. If any end release codes have been prescribed for the application region, they will not be applied at locations of beam element continuity. This is new for Patran 2001r3. For earlier versions of Patran, end release codes would be applied to all elements of the application region, regardless of continuity.
Chapter 2: Building A Model 131 Element Properties
4. When warping is enabled, individual SPOINTs are generated for all beam ends that are not continuous. This applies to both “multiple junctions” and “unmatched ends”. 5. The specified end release codes are applied to all discontinuous beam element ends in the application region, whether “multiple junction” or “unmatched end”, with the applied end release codes dependent on what has been prescribed for “End A” and “End B” for the application region. If no end release codes have been prescribed for the application region, none are generated. 6. When warping is enabled, and for unmatched ends only (not multiple junctions), constraints applied to the SPOINTs are specified by the “warping option” specified in the element properties form. For example, if “A free B fixed” has been selected and the unmatched end is “End A” of its beam element, it will not be constrained. If it is “End B” of its element, it will be constrained. The warping SPOINT for a beam element end involved in a multiple junction will not be constrained under any circumstances. If the user wishes to constrain warping for a beam element involved in a multiple junction, he will have to do so by splitting the application region in such a way that the beam element end becomes an “unmatched end” within its new application region. 7. Warping is considered to be enabled when a value has been specified for the warping coefficient at either end of the beam element. When the user selects the “Beam Library” option, values for the warping coefficient get computed autamatically, and thus warping is implicitly enabled. If the user wishes to disable warping while using the Beam Library option, he must choose “None” as his “Warping Option” on the “Input Properties ...” form.
General Section Rod (CROD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
General Section
Bar/2
Standard
Use this form to create a CROD element and a PROD property. This defines a tensioncompression-torsion element of the structural model.
132
Patran Interface to MD Nastran Preference Guide Element Properties
Chapter 2: Building A Model 133 Element Properties
Defines the cross-sectional area of the element. This is the A field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the setting of the MID field on the PROD entry. This property is required.
Defines the coefficient to determine the torsional stress. This is the C field on the PROD entry. This property can be either a real value or a reference to an existing field definition. This property is optional.
Defines the torsional stiffness of the beam. This is the J field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam. This is the NSM field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
134
Patran Interface to MD Nastran Preference Guide Element Properties
General Section Rod (CONROD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
General Section
Bar/2
CONROD
Use this form to create a CONROD element. This defines a tension-compression-torsion element of the structural model.
Chapter 2: Building A Model 135 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the CONROD entry. This property is required. Defines the crosssectional area of the element. This property is the A field on the CONROD entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the CONROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the coefficient to determine the torsional stress. This property is the C field on the CONROD entry and can either be a real value or a reference to an existing field definition. This property is optional.
Defines the torsional stiffness of the beam. This property is the J field on the CONROD entry. This value can either be a real value or a reference to an existing field definition. This property is optional.
136
Patran Interface to MD Nastran Preference Guide Element Properties
Pipe Section Rod (CTUBE) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
Pipe Section
Bar/2
Use this form to create a CTUBE element and a PTUBE property. This defines a tensioncompression-torsion element with a thin-walled tube cross section.
Chapter 2: Building A Model 137 Element Properties
Defines the tube outer diameters at each end of the element. These are the OD and OD2 fields on the PTUBE entry. These values can either be real values or references to existing field definitions. The outer diameter at Node 1 property is required. The outer diameter at Node 2 Property is optional. Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. This property defines the setting of the MID field on the PTUBE entry. Either select from the list using the mouse, or type in the name. This property is required. Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PRTUBE entry. This value can be either a real value or reference to an existing field definition. This property is optional. Specifies the wall thickness of the pipe. This is the T field on the PTUBE entry. This value can either be a real value or a reference to an existing field definition. This property is required.
Scalar Spring (CELAS1/CELAS1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Spring
Option(s)
Topologies Bar/2
138
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring of the structural model.
Chapter 2: Building A Model 139 Element Properties
Defines the coefficient to be used for this spring. This property is the K field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is required.
Defines what damping is to be included. This property is the GE field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is optional. Defines which degree of freedom this value is to be attached to at each node. The degree of freedom can be set to UX, UY, UZ, RX, RY, or RZ. These properties define the settings of the C1 and C2 fields on the CELAS1 entry. These properties are required.
Defines the relationship between the spring deflection and the stresses within the spring. This property is the S field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is optional.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Scalar Damper (CDAMP1/CDAMP1D) This subordinate form appears when the Input Properties button is selected on the Element Properties
140
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Damper
Scalar
Bar/2
Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model.
Chapter 2: Building A Model 141 Element Properties
Defines the force per unit velocity value to be used. This is the B field on the PDAMP entry and can either be a real value or a reference to an existing field definition. This property is optional.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Defines which degree of freedom this value will be attached to at each node. This can be set to UX, UY, UZ, RX, RY, or RZ. These define the settings of the C1 and C2 field on the CDAMP1 entry. These properties are required.
Viscous Damper (CVISC) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Damper
Viscous
Bar/2
142
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CVISC element and a PVISC property. This defines a viscous damper element of the structural model.
This is the C1 field on the PVISC entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
This is the C2 field on the PVISC entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
Gap (CGAP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Gap
Adaptive
Bar/2
Nonadaptive
Use this form to create a CGAP element and a PGAP property. This defines a gap or frictional element of the structural model for non-linear analysis.
Chapter 2: Building A Model 143 Element Properties
Defines the local element coordinate system for this element that can be defined in one of three ways. If the two end nodes of the gap are not coincident, then the Gap Orientation can reference a vector or a node ID. This local x-axis would then run between the two end nodes and the orientation information would define the local xy plane. However, if the two end nodes are coincident, then the Gap Orientation refers to an existing coordinate system definition and will be used as the local element coordinate system. This Gap Orientation defines the settings of the X1, X2, X3, G0, and CID fields on the CGAP entry. This property is required. Defines the initial opening of the gap element. The nodal coordinates are only used to define the closure direction. This property is the U0 field on the PGAP entry and can be either a real value or a reference to an existing field definition. This property is optional.
Defines the artificial stiffness of the gap when the gap is open or closed. The closed stiffness should be chosen to closely match the stiffness of the surrounding elements. The open stiffness should be approximately 10 orders of magnitude less. These properties are the Ka and Kb fields on the PGAP entry and can either be real value or references to existing field definitions. The closed stiffness property is required. The opened stiffness property is optional. Defines an initial preload across an initially closed gap. For example, this can be used for initial thread loading. If the gap is initially open, setting this value to the initial opening stiffness will improve the solution convergence. This is the F0 field on the PGAP entry and can either be a real value or a reference to an existing field definition. This property is optional.
This is a list of Input Properties available for creating a CGAP element and a PGAP property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
144
Patran Interface to MD Nastran Preference Guide Element Properties
properties. Prop Name
Description
Sliding Stiffness
Defines the artificial shear stiffness of the element when the element is closed. This is the Kt field on the PGAP entry. This property can be either a real value or a reference to an existing field definition. This property is optional.
Static Friction
Defines the static friction coefficient. This property is the MU1 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Kinematic Friction
Defines the kinematic friction coefficient. This property is the MU2 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Penetration
Defines the maximum allowable penetration. This property is the TMAX field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Adjust Ratio
Defines the maximum allowable adjustment ratio. This property is the MAR field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Penet. Lower Bound
Defines the lower bound for the allowable penetration. This is the TRMIN field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Friction Coeff. y
Defines the coefficient of friction when sliding occurs along this element in the local y and z directions. These are the MU1 and MU2 fields on the PGAP entry and can be either real values or references to existing field definitions. These properties are optional.
Friction Coeff. Z
Scalar Mass (CMASS1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
1D Mass
Option(s)
Topologies Bar/2
Chapter 2: Building A Model 145 Element Properties
Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model.
Defines the translation mass or rotational inertia value to be applied. This property is the M field on the PMASS entry and can either be a real value or a reference to an existing field definition. This property is required.
Defines which degree of freedom this value will be attached to at each node. These can be set to UX, UY, UZ, RX, RY, or RZ and defines the settings of the C1 and C2 field on the CMASS1 entry. These properties are required.
146
Patran Interface to MD Nastran Preference Guide Element Properties
PLOTEL This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
PLOTEL
Option(s)
Topologies Bar/2
Use this form to create a PLOTEL element.
Dummy property data not required to define the PLOTEL property set.
(Scalar) Bush This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Bush
Option(s)
Topologies Bar/2
Chapter 2: Building A Model 147 Element Properties
This toggle can also be set to Node Id or CID.
148
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Bush Orientation
Description Element orientation strategy keys off of CID specification. If CID is blank, the element x-axis lies along the line which joins the elements grid points (GA, GB Element Properties/Application Region). The X-Y plane is determined by specifying the Bush Orientation. If a vector input is given, these components define an orientation vector v from the first grid point (GA) of the element in the displacement coordinate system at that point (GA). If the Bush Orientation references a grid point ID (Value), this orientation point forms an orientation vector which extends from the first element grid point to the orientation point.
If a CID 0 is specified for Bush Orientation System, the element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the first elemental grid point (GA) is used to locate the system. If CID = 0, the elemental coordinate system is the Basic Coordinate System.
If no orientation is specified in any form, the element x-axis is along the line which connects the element’s grid points. The material property inputs for this condition must be limited to simple axial and torsional stiffness and damping (k1,k4,B1,B4). Offset Location
Offset Location (0.0 s 1.0) specifies the spring-damper location along the line from GRIDGA to GRIDGB by setting the fraction of the distance from GRIDGA. s=0.50 centers the springdamper.
Offset Orientation System
Specifies the coordinate system used to locate the spring-damper offset when it is not on the line from GRIDGA to GRIDGB.
Offset Orientation Vector
Provides the location of the spring-damper in space relative to the offset coordinate system. If the offset orientation system is -1 or blank, the offset orientation vector is ignored.
Chapter 2: Building A Model 149 Element Properties
Prop Name
Description
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6
Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6
Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6
Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend
Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation
Stress Recovery Coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation
Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.
150
Patran Interface to MD Nastran Preference Guide Element Properties
Spot Weld Connector (CWELD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Spot Weld Connector
Option(s)
Topologies Connector
Chapter 2: Building A Model 151 Element Properties
.
Note that SPOTWELD properties are created automatically (or pre-existing properties selected) when creating Spotwelds through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying spotweld properties because the existence of the spotweld itself is the application region for the property set.
152
Patran Interface to MD Nastran Preference Guide Element Properties
Fastener Connector (CFAST) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Fastener Connector
Option(s)
Topologies Connector
Chapter 2: Building A Model 153 Element Properties
.
Note that FASTENER properties are created automatically (or pre-existing properties selected) when creating Fasteners through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying fastener properties because the existence of the fastener itself is the application region for the property set.
154
Patran Interface to MD Nastran Preference Guide Element Properties
The formula value can be any of the following: String None Douglas Huth Hi-Lok in CFRP Huth Hi-Lok in metal Huth solid rivet Note that Douglas or one of several Huth formulations can be used to calculate stiffness values of fastener connections automatically, minimizing the need for manual calculation. Stiffness coefficients for the CFAST element are calculated in different steps. Generally, either Douglas or three derivatives of Huth formulas are used. Regardless of the selected formula, the axial stiffness is always calculated the same way: 1 E f --- A˜ d 2 4 f k = -------------------l
The stiffness is inserted into the KT1 parameter of the PFAST entry. The length of the fastener will be determined by summation of the thickness of the two connected shell elements. The Douglas formula is*: 1 k = --c 5 1 1 c = ---------- + 0.8 ---------- + ---------- t E df Ef t 2 E 2 1 1
The formula according to Huth is*: k = 1 --c a t 1 + t 2 1 1 1 1 - ---------+ ---------- + ------------- + ------------- c = b -------------2d t E t 2 E 2 2E f t 1 2E f t 2 1 1 f
Hi-Lok in CFRP
a
b
0.6667
4.2
Chapter 2: Building A Model 155 Element Properties
a
b
Hi-Lok in metal
0.6667
3.0
Solid Rivet
0.4
2.2
In the case of composites, the Douglas and Huth formulas have to be used twice. First, the overall (engineering) Young’s modulus has to be calculated for both directions (E11 and E22), which then has to be applied to the formulas. In this case, the shear stillness of the fastener is direction dependent. For composites or anisotrophic material, the material tensors of the two connected shell elements have to be transformed into the coordinate system of the CFAST element before the Douglas or Huth formula is applied. The resulting stiffness is applied to the KT2 and KT3 parameters on the PFAST entry. * The following symbols are used in the formulas: Symbol
Meaning
Ef
Young’s modulus of fastener
df
Diameter of fastener
l
Length of fastener, evaluated from the FE model
E1
Young’s modulus of first property connected to the fastener
t1
Thickness of first property connected to the fastener
E2
Young’s modulus of second property connected to the fastener
t2
Thickness of second property connected to the fastener
Standard Homogeneous Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CQUAD4, CTRIA3, CQUAD8, or CTRIA6 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.
156
Patran Interface to MD Nastran Preference Guide Element Properties
Chapter 2: Building A Model 157 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select one from the list using the mouse or type in the name. This defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CQUADi or CTRIAi entry. This scalar value can either be a constant value in degrees, a vector, or a reference to an existing coordinate system. This property is optional. Defines the mass not derived from the material of the element. This is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the thickness, which will be uniform over each element. This value can either be a real value or a reference to an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CQUAD4/8 and CTRIA3/6 entries and/or the T field on the PSHELL entry. This property is required.
158
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties, available for creating a CQUADi and a CTRIAi element and a PSHELL property, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4/8 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the bottom and top most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Fiber Dist. 2 Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Revised Homogeneous Plate (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4
Revised Formulation
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.
Chapter 2: Building A Model 159 Element Properties
160
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. and this is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Chapter 2: Building A Model 161 Element Properties
P-Formulation Homogeneous Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4,Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P-Formulation
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.The p-formulation shell element is supported in MSC . Nastran Version 69 or later. Therefore, the MD Nastran Version in the Translation Parameter form must be set to 69.
162
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties are the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. These properties are optional. Defines the mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element and this is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines a uniform thickness, which will cover each element. This property defines the T1, T2, T3, and T4 fields on the CQUAD4 or CTRIA3 entry and/or the T field on the PSHELL entry and can be either a real value or a reference to existing field definition. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of the basic system.This defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
Chapter 2: Building A Model 163 Element Properties
properties. Prop Name
Description
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Fiber Dist. 2 Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P--order Coordinate System (default elemental). Starting Porders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag that controls whether or not this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis.By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
Standard Laminate Plate (CQUAD4/PCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Laminate
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
164
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PCOMP property.
Chapter 2: Building A Model 165 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type the name in. The specified material must be a laminate material in Patran. The data in this material definition defines the settings of the MIDi, Ti, and THETAi fields on the PCOMP entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6 CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines mass not included in the mass derived from the material of the element. This is the NSM field on the PCOMP entry. This property is defined in terms of mass per unit area of the element and can be either a real value or a reference to an existing field definition. This property is optional. Defines the offset of the element‘s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
166
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description
Laminate Options
Laminate option placed on the LAM field of the PCOMP/PCOMPG entry. No option implies all plies must be specified and all stiffness terms developed. MEM - all plies are specified but only membrane terms are computed. BEND - all plies specified but only bending terms computed. SMEAR - all plies specified, stacking sequence ignored and TS/T and 12I/T**3 terms set to zero. SMCORE - all plies specified with the last ply specifying core properties and the previous plies specifying face sheet properties. See the Nastran Quick Reference Guide for more details.
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Revised Laminate Plate (CQUADR/PCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Laminate
Tri/3, Quad/4
Revised Formulation
Chapter 2: Building A Model 167 Element Properties
Use this form to create a CQUADR or CTRIAR element and a PCOMP property.
Defines mass not included in the mass derived from the material of the element. This is the NSM field on the PCOMP entry. This property is defined in mass per unit area, of the element. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. The specified material must be a laminate material in Patran. The data in this material definition defines the settings of the MIDi, Ti, and THETAi fields on the PCOMP entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
See Standard Laminate Plate (CQUAD4/PCOMP), 163 for a description of the SOL 400 Laminate and Nonlinear Formulation options.
168
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Equivalent Section Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 169 Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can be either a constant value or a reference to an existing coordinate system. This property is optional.
This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4, or CQUAD8
170
Patran Interface to MD Nastran Preference Guide Element Properties
element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This property is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit area of the element. This property is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This property is the ZOFFS field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Distance 2
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Chapter 2: Building A Model 171 Element Properties
Revised Equivalent Section Plate (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4
Revised Formulation
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
172
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields, on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness, which will be used for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This value can be either a real value or a references to an existing field definition. This property is required.
Defines the basic orientation for any nonisotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA field on the CQUADR or CTRIAR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Chapter 2: Building A Model 173 Element Properties
This is a list of Input Properties available for creating a CTRIAR or CQUADR element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Distance 2
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
174
Patran Interface to MD Nastran Preference Guide Element Properties
P-Formulation Equivalent Section Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P-Formulation
Use this form to create a CQUAD4, or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC . Nastran Version 69 or later. Therefore, the MSC .Nastran Version in the Translation Parameter form must be set to 69.
Chapter 2: Building A Model 175 Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields, on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness, which will be used for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIAR3 or CQUAD4 entry and/or the T field on the PSHELL entry. This value can be either a real value or a references to an existing field definition. This property is required.
Defines the basic orientation for any nonisotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of basic system.This property is optional.
This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
176
Patran Interface to MD Nastran Preference Guide Element Properties
properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3entry and can be either real value or reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real value or references to existing field definitions. This property is optional.
Fiber Dist. 2 Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields in the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Chapter 2: Building A Model 177 Element Properties
Prop Name
Description
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default, equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default, equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
Field Point Mesh (CQUAD4/TRIA3)(Exterior Acoustics) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Field Point Mesh
Tri/3, Quad/4
Use this form to create a CTRIA3, CQUAD4 elements for creating acoustic field point mesh for an exterior acoustics analysis. No property cards are created. The material referenced should be the same as that defined for the 3D solid elements and exterior acoustic infinite elements used to define the surrounding fluid environment of the structure, although no actual materials is written. In order to recover results on these meshes, you must set the output request ACFPFRESULT.
178
Patran Interface to MD Nastran Preference Guide Element Properties
Each acoustic field point mesh defined is written to a seperate section of the bulk data using the BEGIN AFPM=id.
Input Properties
Chapter 2: Building A Model 179 Element Properties
Standard Bending Panel (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
Standard Formulation
Tri/3, Quad/4 Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
180
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines the uniform thickness for each element. This defines the T1, T2, T3, and T4 fields on the CQUAD4/8 and CTRIA3/6 entries and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is required. Defines the mass not derived from the material of the element. This property is defined in mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Chapter 2: Building A Model 181 Element Properties
This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4 or CQUAD8 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Fiber Dist. 1
Description Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and these values can be either real values or references to existing field definitions. These properties are optional.
Fiber Dist. 2
Revised Bending Panel (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
Revised Formulation
Tri/3, Quad/4
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
182
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines the uniform thickness, which will be used for each element. This defines the T1, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definitions. This property is required. Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. This property is optional.
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can either be real values or a reference to and existing field definition. This property is optional.
Chapter 2: Building A Model 183 Element Properties
P-Formulation Bending Panel (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
P- Formulation
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
Use this form to create a CTRIA3, or CQUAD4 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC .Nastran Version 69 or later. Therefore, the MSC. Nastran Version in the Translation Parameters form must be set to 69.
184
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis or (2) define a constant angle offset from the projected x-axis of basic system.This property defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Defines the uniform thickness, which will be used for each element. This defines the T1, T2, T3, and T4 fields on the CQUAD4 or CTRIA3 entry and/or the T field on the PSHELL entry and this value can be either a real value or a reference to an existing field definition. This property is required.
This is a list of Input Properties available for creating a CTRIA3 or CQUAD4 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form
Chapter 2: Building A Model 185 Element Properties
to view these properties. Prop Name
Description
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Dist. 2
Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
186
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Axisymmetric Solid (CTRIAX6) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Axisymmetric
Tri/3, Tri/6
Use this form to create a CTRIAX6 axisymmetric solid element. This defines an isoparametric and axisymmetric triangular cross section ring element with midside nodes.
Chapter 2: Building A Model 187 Element Properties
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the TH field on the CTRIAX6 entry. This scalar value can be either a constant value or a reference to an existing coordinate system. This property is optional.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the setting of the MID field on the CTRIAX6 entry. This property is required.
PLPLANE Axisymmetric Solid (CTRIAX, CQUADX) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option 1
Create
2D
2D Solid Axisymmetric
Option 2
Topologies
Hyperelastic
Tri/3, Tri/6, QUAD/4, QUAD/8
PLPLANE
Use this form to create axisymmetric solid elements. This defines an isoparametric and axisymmetric cross section ring element with or without midside nodes.
188
Patran Interface to MD Nastran Preference Guide Element Properties
For SOL600 solutions use the PLPLANE option and any material type. For non-SOL600 runs, use the Hypereleastic option with Mooney-Rivlin materials.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
2D Axi-Symmetric Laminated Solid Composite This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Laminate
CQUADX
Use this form to create CQUADX elements and a PLCOMP property.
Chapter 2: Building A Model 189 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PLCOMP entry to be used. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines element edge used as base ply orientation.
Not used for axisymmetric elements
190
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 191 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior. This property is required.
The orientation of the material directions can be specified by the Material Orientation parameter value CID, Real Scalar, or Vector.
The presence of nonstructural mass in the model does not change the stiffness of the model.
Revised Plane Strain Solid (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4
Revised Formulation Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
192
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior. This property is required.
Chapter 2: Building A Model 193 Element Properties
P-Formulation Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P- Formulation
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The pformulation shell element is supported in MSC. Nastran Version 69 or later. Therefore, the MSC .Nastran Version in the Translation Parameters form must be set to 69.
194
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. This property is required. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of basic system. This defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
Chapter 2: Building A Model 195 Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Infinite (Exterior Acoustic Element)(CACINF3/CACINF4) These elements are used in exterior acoustic analysis (frequency response) and placed on the outside of the solid mesh representing the fluid (coincident with the outside surface). The must share the same nodes as the solid mesh. They simulate the fluid proprties reaching to infinity beyond the boundary of the solid mesh representing the fluid. The surfaces that these elements connect to must be convex. However it is not necessary that the surface be smooth. They also take on the same fluid proprties as the solid fluid mesh. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Infinite
Tri/3, Quad/4
Use this form to create a CACINF3, CACINF4 elements and a PACINF property. The appropriate fields on the PACINF entry are filled in or left blank in order to achieve the requested behavior.
196
Patran Interface to MD Nastran Preference Guide Element Properties
Interger value that defines the radial interpolation order, which must be defined and greater than zero.
The pole of the acoustic infinite elements. This must be coorinate location defined in the global Patran coordinate system. A node ID can also be selected graphically.
Defines the material to be used. This material is generally the same material used to define the solid fluid mesh in an exterior acoustics analysis (MAT10). The same material should also be referenced when using acoustic field point meshes.
2D Plane Strain Laminated Solid Composite This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Laminate
QUAD/4, QUAD/8
Use this form to create quadratic elements and a PLCOMP property.
Chapter 2: Building A Model 197 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PLCOMP entry to be used. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines element edge used as base ply orientation.
Not used for axisymmetric elements
Standard Membrane (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties
198
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
Standard Formulation
Tri/3, Quad/4 Tri /6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 199 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1 field on the PSHELL entry. This property is required.
Defines the mass not derived from the material of the element. This property is defined in mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the uniform thickness that will be used for each element. This value can either be a real value or reference an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry and/or the T field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1)reference a coordinate system, which is then projected onto the element. (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Revised Membrane (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties
200
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
Revised Formulation
Tri/3, Quad/4
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 201 Element Properties
Defines the mass not derived from the material of the element. This property is defined in terms of mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional. Defines the uniform thickness that will be used for each element. This value can be either a real value or a reference to an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This property is required.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the settings of the MID1 field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
P-Formulation Membrane (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties
202
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
P- Formulation
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9. Tri/9, Quad/12, Tri/13, Quad/16
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The pformulation shell element is supported in MSC .Nastran Version 69 or later. Therefore, the MSC. Nastran Version in the Translation Parameters form must be set to 69.
Chapter 2: Building A Model 203 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis or (2) define a constant angle offset from the projected x-axis of basic system. This property defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
204
Patran Interface to MD Nastran Preference Guide Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Shear Panel (CSHEAR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
2D
Shear Panel
Option(s)
Topologies Quad/4
Use this form to create a CSHEAR element and a PSHEAR property. This defines a shear panel element of the structural model.
Chapter 2: Building A Model 205 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the settings of the MID field on the PSHEAR entry. This property is required.
Defines the uniform thickness, which will be used for each element. This defines the T field on the PSHEAR entry. This property is required. This value can be either a real value or a reference to an existing field definition.
Defines the effectiveness factor for extensional stiffness along the 2-3 and 1-4 sides. This is the F2 field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the effectiveness factor for extensional stiffness along the 1-2 and 3-4 sides. This is the F1 field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines mass not included in the mass derived from the material of the element. This is defined in mass per unit area of the element. This is the NSM field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
206
Patran Interface to MD Nastran Preference Guide Element Properties
Additional properties on the form which do not appear on the previous page are: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHEARN entry is written for this property set. Large Strain forces the PSHEARN entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option 1
Option 2
Topologies
Create
3D
Solid
Homogeneous
Standard
Tet/4, Wedge/6
Laminate (HEX/8 only)
Formulation
Hex/8, Tet/10
P-Formulation
Wedge/15, Hex/20
Hyperelastic Formulation
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property or a CHEXA and a PCOMP property.
Chapter 2: Building A Model 207 Element Properties
208
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID field on the PSOLID entryor references a PCOMP entry in the case of Laminated Composites. This property is required.
Defines both the orientation of referenced nonisotropic materials and solid element results. This can be set to Global, Elemental, or to a specific coordinate frame reference and defines the CORDM field on the PSOLID entry. The default is Global. Nonlinear stresses and strains are output in the Elemental system regardless of the setting. Defines where the output for these elements are to be reported. This property can be set to either Gauss or Grid and is the STRESS field on the PSOLID entry. This property is optional.
Defines the type of integration network to be used. This property is the IN field on the PSOLID entry and can be set to Bubble, Two, or Three. This property is optional.
Defines the integration scheme to be used. This property is the ISOP field on the PSOLID entry and can be set to Reduced or Full. This property is optional.
Chapter 2: Building A Model 209 Element Properties
Additional properties on the form which do not appear on the previous page are: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
P-Formulation Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis: Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
P-Formulation
Tet/4, Wedge/6 Hex/8, Tet/10 Wedge/15, Hex/20, Tet/16, Tet/40, Wedge/24,Wedge/52, Hex/32, Hex/64
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property.
210
Patran Interface to MD Nastran Preference Guide Element Properties
Defines orientation for the referenced material. This property can be set to Global, Elemental or to a user-defined coordinate system and defines the CORDM field on the PSOLID entry. The default is Global. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coord. System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PSOLID entry. This property is required.
Chapter 2: Building A Model 211 Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default the value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default the value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default the value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Integration Network
Defines the type of integration network to be used. This property is the IN field on the PSOLID entry and can be set to Bubble, Two, or Three. This property is optional.
Integration Scheme
Defines where the output for these elements are to be reported. This can be set to either Gauss or Grid. This property is the STRESS field on the PSOLID entry. This property is optional.
Hyperelastic Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Hyperelastic Formulation
212
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CQUAD, CQUAD4, CQUAD8, CTRIA3, or CTRIA6 element and a PLPLANE property.
Identification number of a coordinate system defining the plane of deformation. This defines the CID field on the PLPLANE entry.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLPLANE entry. This property is required.
Hyperelastic Axisym Solid (CTRIAX6) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Axisymmetric
CQUADX,
Hyperelastic Formulation
CTRIAX
Chapter 2: Building A Model 213 Element Properties
Use this form to create a CQUADX or CTRIAX element and a PLPLANE property.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLPLANE entry. This property is required.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
214
Patran Interface to MD Nastran Preference Guide Element Properties
Hyperelastic Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
Hyperelastic Formulation
HEX, PENT, TET
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PLSOLID property.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLSOLID entry. This property is required.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLSOLID entry.
Chapter 2: Building A Model 215 Element Properties
Additional properties on the form which do not appear on the form above: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
3D Laminate Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
Laminate
HEX, PENT, TET
Use this form to create CHEXA elements and a PCOMP (SOL 600) or PCOMPLS (SOL400) property.
216
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PCOMP entry to be used. This property is required.
Defines element face used as base ply orientation.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines available laminate options “MEM”, “BEND”, “SMEAR”, “SMCORE” (see MD Nastran QRG for definitions.
Chapter 2: Building A Model 217 Beam Modeling
2.8
Beam Modeling Modeling structures composed of beams can be more complicated than modeling shell, plate, or solid structures. First, it is necessary to define bending, extensional, and torsional stiffness that may be complex functions of the beam cross sectional dimensions. Then it is necessary to define the orientation of this cross section in space. Finally, if the centroid of the cross section is offset from the two finite element nodes defining the beam element, these offsets must be explicitly defined. Fortunately, Patran provides a number of tools to simplify these aspects of modeling.
Cross Section Definition The cross section properties are defined on the element property forms shown on pages General Section Beam (CBAR), 102 and Tapered Beam (CBEAM), 119. The properties can be entered directly into the data boxes labeled Area, Inertia i,j, Torsional Constant, etc. or by pushing the large I-beam icon on these forms to access the Beam Library form. The Beam Library forms are a much more convenient way of defining properties for standard cross sections and are shown below. Create Action The first step in using the beam library is to select the section icon for the particular cross section desired (e.g. I-section).Then the dimensions for each of the components of the beam section must be entered.
218
Patran Interface to MD Nastran Preference Guide Beam Modeling
Current beam section as selected from the section library icon palette. The required dimensions are shown. Enter the dimensions of the beam section here, referring to the beam section icon.
Writes the current beam properties to a report file. Calculates the beam properties based on the current dimensions and displays an image of the scaled section along with the properties.
These forward and backward arrows provide access to additional beam section icons. Beam section library icon palette. Select the icon representing the desired section.
Beam section name to be created. List of existing beam sections. This list can be filtered to contain only the section names of interest using the filter mechanism.
Chapter 2: Building A Model 219 Beam Modeling
Finally, a section name must be entered and the Apply button pushed. The other options available with the beam library are documented in the Patran Reference Manual, see Beam Library (p. 475) in the Patran Reference Manual. Once one or more beam sections have been defined, these can be selected in the section data box on the element properties form. Supplied Functions
I-Beam - Six dimensions -- lower flange thickness (t1), upper flange thickness (t2),lower flange width (w1), upper flange width (w2), overall height (H), and web thickness (t)-- allows for symmetric or unsymmetrical I-beam definition. Angle - Open section, four dimensions -- overall height (H), overall width (W), horizontal flange thickness (t1), vertical flange thickness (t2).
Tee - Four dimensions -- overall height (H), overall width (W), horizontal flange thickness (t1), vertical flange thickness (t2).
Solid-Rod - Solid section, one dimension -- radius (R).
Box-Symmetric - Closed section, four dimensions -- overall height (H), overall width (W), top and bottom flange thicknesses (t1), side flange thicknesses (t2).
Tube - Closed section, two dimensions -- outer radius (R1), inner radius (R2).
Channel - Open section, four dimensions -- overall height (H), overall width (W), top and bottom flange thicknesses (t1), shear web thickness (t).
220
Patran Interface to MD Nastran Preference Guide Beam Modeling
Bar - Solid section, two dimensions -- height (H) and width (W).
Box-Unsymmetrical - Closed section, six dimensions -- overall height (H), overall width (W), top flange thickness (t1), bottom flange thickness (t2), right side flange thickness (t3), left side flange thickness (t4). Hat - Four dimensions -- overall height (H), top of hat flange width (W), bottom of hat flange width for one side (W1), thickness (t).
H-Beam - Four dimensions -- overall height (H), width between inner edges of vertical flanges (W), horizontal shear web thickness (t), and thickness of one vertical flange (W1/2). Cross - Four dimensions -- overall height (H), vertical flange thickness (t), horizontal flange thickness (t2), length of free horizontal flange for one side (W/2).
Z-Beam - Four dimensions -- overall height (H2), height of vertical flange between as measured between horizontal flanges, length of free horizontal flange for one side (W), thickness (t1). Hexagonal - Solid section, three dimensions -- overall height (H), overall width (W), horizontal distance from side vertex to top or bottom surface vertex along the common edge (i.e., diagonal edge hypotenuse times the cosine of the exterior diagonal angle).
Cross Section Orientation The Bar Orientation data box on the Input Properties form is used to define how the y-axis of the beam cross section is oriented in space. By default the Value Type is Vector. This tells MSC Nastran that the cross section y-axis lies in the plane defined by the beam’s x-axis (the line connecting the two node points) and this vector. The Value Type pop up menu may be changed to Node ID. In this case the y-axis lies in the plane defined by the x-axis and the selected node.
Chapter 2: Building A Model 221 Beam Modeling
When the Value Type is Vector and the Bar Orientation data box is selected the following select box appears on the screen. These select tools provide different options for defining vectors. They are discussed in more detail in the Select Menu (p. 35) in the Patran Reference Manual.
These three tools define the orientation vector as the 1 (x), 2(y), or 3(z) axis of a selected coordinate system. This is a convenient way to specify the orientation when it is aligned with one of the three axes of a rectangular coordinate system. When the system is not rectangular (e.g. cylindrical) these tools may not provide the desired definition because the defined vector does not change direction at different points in space--these tools just provide an alternate way to define a global vector.
This tool may be used to define a general vector with respect to an alternate coordinate system. When this icon is picked, the select menu changes to the one on the right.
These tools provide different ways to define vectors. In addition, the user is requested to select a coordinate system in which this vector is defined. The simplest list processor syntax that appears in the databox for a vector in an alternate coordinate system is <x_component, y_component, z_component> coord cord_id (e.g. <1, 0, 0> coord 3). In many cases it is easy to simply type a definition in this form into the Bar Orientation databox.
After the orientation has been defined, there are two ways to verify its correctness in Patran. The first option is in the Element Properties application. By selecting the Show Action, the Definition of X Y Plane property, and Display Method Vector Plot, the vectors defining the orientation will be shown on the model. A second option can be used when the Beam Library has been used to define the beam cross section. There is an option on the Display form Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual called Beam Display. The menu allows different display options for displaying an outline of the defined cross section on the model in the correct location and orientation. Users should be aware of one difference between the Patran and MD Nastran definitions for cross section orientation. In Patran the orientation is completely independent of the analysis coordinate system at the beam nodes. In MD Nastran, the orientation vector is assumed to be defined in the same system as the analysis system at the first node of the beam. In Patran it is perfectly permissible to define the orientation in a different coordinate system from that analysis system. When the NASTRAN input file is generated, the necessary transformation of this vector to the analysis system at node 1 will be performed.
222
Patran Interface to MD Nastran Preference Guide Beam Modeling
Cross Section End Offsets Two data boxes are provided on the Element Properties, Input Properties form to optionally define an offset from either node 1 to the cross section centroid (Offset @ Node 1) or from node 2 to the cross section centroid (Offset @ Node 2). The same select menu tools are available for defining these vectors. One difference between the orientation definition and the offset definitions, however, is that for the offset the magnitude of the vector is important. Because of this, the select menu tools are usually not very convenient. Typically, offsets are defined by typing the definition (e.g <x, y, z> or <x, y, z> coord n>) into the appropriate data box. Two options are available for verifying the definitions of offsets; these options are very similar to those for orientations. The Element Properties, Show Action will allow the end offsets to be displayed as vectors on the model. This option is not especially useful because the vector plot shows only the direction of the offset, not the magnitude of the offset. It is usually much more useful to view the Beam Display menu on the Display form Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual to select the display option with offsets. The viewport will then show the beam displayed in both the offset and non-offset positions.
Stiffened Cylinder Example Figure 2-1 shows a simple example of a circular cylinder stiffened with Z-stiffeners. The cross section
was defined by selecting the Beam Library icon on the Element Properties/Input Properties form. The Z cross section was selected on the Beam Library form, the cross section dimensions input, a section name input, and the Apply button pushed. On the Input Properties form, the Use Beam Section toggle is set to ON. The defined section name is selected in the [Section Name] data box. The string <-1.0 0. 0.> coord 1 is typed into the Bar Orientation data box to align the cross section orientation with the radial direction of the global, cylindrical system. Similarly, the strings <-2.0 0.0 0.0> coord 1 and <-2.0 0.0 0.0> coord 1
Chapter 2: Building A Model 223 Beam Modeling
typed into the Offset @ Node 1 and Offset @ Node 2 data boxes define the end offsets to be radially inward.
T Z1
Y Z
Figure 2-1
X
Stiffened Cylinder
R
224
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
2.9
Loads and Boundary Conditions The Loads and Boundary Conditions form will appear when the Loads/BCs toggle, located on the Patran main form, is chosen. When creating a load and boundary condition there are several option menus. The selections made on the Loads and Boundary Conditions menu will determine which load and boundary conditions form appears, and ultimately, which MD Nastran loads and boundary conditions will be created. The following pages give an introduction to the Loads and Boundary Conditions form and details of all the loads and boundary conditions supported by the Patran MD Nastran Analysts Preference.
Loads & Boundary Conditions Form This form appears when Loads/BCs is selected on the main menu. The Loads and Boundary Conditions form is used to provide options to create the various MD Nastran loads and boundary conditions. For a definition of full functionality, see Loads and Boundary Conditions Form (p. 27) in the Patran Reference Manual. Options for defining slide line contact are also accessed from this main Loads and Boundary Conditions form. For more information see Defining Contact Regions, 247.
Chapter 2: Building A Model 225 Loads and Boundary Conditions
Defines the general load type to be applied. Object choices are Displacement, Force, Pressure, Temperature, Inertial Load, Initial Displacement, Initial Velocity, Velocity, Acceleration, Distributed Load, CID Distributed Load, Total Load, Contact, Initial Temperature, Planar Rigid Wall and Init.Rotation Field.
Defines what type of region is to be loaded. The available options depend on the selected Object. The general selections can be Nodal, Element Uniform, or Element Variable. Nodal is applied explicitly to nodes. Element Uniform defines a constant value to be applied over an entire element, element face, or element edge. Element Variable defines a value that varies across an entire element, element face, or element edge.
Current Load Case type is set on the Load Case menu. When the Load Cases toggle located on the main menu is chosen, the Load Cases menu will appear. Under Load Case Type, select either Static or Time Dependent, then enter the name of the case, and click on the Apply button.
Generates either a Static, 226 or Time Dependent, 229 Input Data form, depending on the current Load Case Type.
226
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
The following table outlines the options when Create is the selected Action. Object • Displacement
Type • Nodal • Element Uniform • Element Variable
• Force
• Nodal
• Pressure
• Element Uniform • Element Variable
• Temperature
• Nodal • Element Uniform • Element Variable
• Inertial Load
• Element Uniform
• Initial Displacement
• Nodal
• Initial Velocity
• Nodal
• Velocity
• Nodal
• Acceleration
• Nodal
• Distributed Load
• Element Uniform • Element Variable
• CID Distributed Load
• Element Uniform • Element Variable
• Total Load
• Element Uniform
• Contact
• Element Uniform
• Initial Plastic Strain
• Element Uniform
• Initial Stress
• Element Uniform
• Initial Temperature
• Nodal
• Planar Rigid Wall *
• Nodal
• Init. Rotation Field *
• Nodal
* For SOL 700 only. Static
This subordinate form appears when the Input Data button is selected on the Loads and Boundary Conditions form and the Current Load Case Type is Static. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 224. The information on the
Chapter 2: Building A Model 227 Loads and Boundary Conditions
Input Data form will vary depending on the selected Object. Defined below is the standard information found on this form.
228
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Defines a general scaling factor for all values defined on this form. The default value is 1.0. Primarily used when field definitions are used to define the load values.
Input Data in this section will vary. See Object Tables, 231 for detailed information. When specifying real values in the Input Data entries, spatial fields can be referenced. All defined spatial fields currently in the database are listed. If the input focus is placed in the Input Data entry and a spatial field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
This button will display a Discrete FEM Fields input form to allow field creation and modification within the loads/bcs application. Visible only when focus is set in a databox which can have a DFEM field reference.
Defines the coordinate frame used to interpret the degree-of-freedom data defined on this form. This only appears on the form for Nodal type loads. This can be a reference to any existing coordinate frame definition.
Chapter 2: Building A Model 229 Loads and Boundary Conditions
Time Dependent
This subordinate form appears when the Input Data button is selected on the Loads and Boundary Condition form and the Current Load Case Type is Time Dependent. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 224 and Load Cases, 246. The information on the Input Data form will vary, depending on the selected Object. Defined below is the standard information found on this form.
230
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data Load/BC Set Scale Factor
1 Spatial Dependence
* Time Dependence
Defines a general scaling factor for all values defined on this form.The default value is 1.0. Primarily used when field definitions are used to define the load values.
Trans Accel (A1,A2,A3) Input Data in this section will vary. See Object Tables, 231 for detailed information.
Rot Velocity (w1,w2,w3)
Rot Accel (a1,a2,a3)
Spatial Fields
Time Dependent Fields
FEM Dependent Data...
When specifying time dependent values in the Input Data entries, timedependent fields can be referenced. All defined timedependent fields currently in the database are listed. If the input focus is placed in the Input Data entry and a timedependent field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
Analysis Coordinate Frame Coord 0
OK
Reset
This button will display a Discrete FEM Fields input form to allow field creation and modification within the loads/bcs application. Visible only when focus is set in a databox which can have a DFEM field reference.
Defines the coordinate frame to be used to interpret the degree-of-freedom data defined on this form. This only appears on the form for Nodal type loads. This can be a reference to any existing coordinate frame definition.
When specifying real values in the Input Data entries, spatial fields can be referenced. All defined spatial fields currently in the database are listed. If the input focus is placed in the Input Data entry and a spatial field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
Chapter 2: Building A Model 231 Loads and Boundary Conditions
Object Tables These are areas on the static and transient input data forms where the load data values are defined. The data fields that appear depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. The following Object Tables outline and define the various input data that pertains to a specific selected object: Displacement / Velocty / Acceleration
Object
Type
Analysis Type
Option
Displacement Velocity Acceleration
Nodal
Structural
Standard
Creates MD Nastran SPC1 and SPCD Bulk Data for Displacement entries. All non blank entries will cause an SPC1 entry to be created. If the specified value is not 0.0, an SCPD entry will also be created to define the non zero enforced displacement or rotation. Phase angle specifications will create DPHASE entries for all corresponding non blank translational or rotational data in frequency response analysis. Displacement, Velocity and Acceleration LBCs used in frequency response / dynamic analysis also define the RLOAD1 entries with DISP, VELOC, and ACCEL keywords, respectively. For frequency response analysis, the LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this. Values given via this option are total enforced values. For relative enforced values used in SOL 400, see the description for the Relative Displacement option below. Input Data
Description
Translations (T1,T2,T3)
Defines the total enforced translational values. These are in model length units.
Rotations (R1,R2,R3)
Defines the total enforced rotational values. These are in radians.
Translational Phase Angles (Tth1,Tth2,Tth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the translational values. These are in degrees.
Rotational Phase Angles (Rth1,Rth2,Rth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the rotational values. These are in degrees.
Object
Type
Analysis Type
Dimension
Displacement
Element Uniform
Structural
3D
Element Variable Applies a zero or nonzero total displacement boundary condition to the face of solid elements. The primary use of this boundary condition is to apply constraints to p-elements; but it may also be used for standard solid elements. If applied to a p-element solid, the appropriate FEFACE and GMBC entries are created. If applied to a standard solid element, the appropriate SPC1 and SPCD entries are created. In
232
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
frequency response analysis, the phase angles are written as DPHASE entries. See comments above for nodal displacements. Input Data
Description
Translations (T1,T2,T3)
Defines the enforced translational displacement values. These values are in model-length units.
Translation Phases (Tth1,Tth2,Tth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the translational displacement values. These are in degrees.
Object
Type
Analysis Type
Option
Displacement
Nodal
Structural
Relative Displacement
Applies a zero or nonzero relative displacement boundary condition as opposed to a total magnitude. This is used in SOL 400 only with multiple steps and not applicable to other solution sequences. This LBC will be ignored if present in a referenced load case for solution sequences other than SOL 400. The appropriate SPC1 and SPCR entries are created. For example, if a DOF is specified on a SPCR with 0.0 for step 2, the relative displacement of this DOF for step 2 with respective to step 1 is 0.0. The total displacement of step 2 is 0.2 if the solution of step 1 for this DOF is 0.2. Input Data
Description
Relative Translations (T1,T2,T3) Defines the relative enforced translational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced translation is to be specified, the particular component should be left blank. Relative Rotations (R1,R2,R3)
Defined the relative enforced rotational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced rotation is to be specified, the particular component should be left blank.
Force
Object
Type
Analysis Type
Force
Nodal
Structural
Creates MD Nastran FORCE and MOMENT Bulk Data entries. Creates the DPHASE entries in frequency response analysis when specifying phase angles for out-of-phase loading. RLOAD1 entries are created for dynamic analysis and reference the appropriate FORCE entries. For frequency response analysis, the force LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this.
Chapter 2: Building A Model 233 Loads and Boundary Conditions
Input Data
Description
Force (F1,F2,F3)
Defines the applied forces in the translation degrees of freedom. This defines the N vector and the F magnitude on the FORCE entry.
Moment (M1,M2,M3)
Defines the applied moments in the rotational degrees of freedom. This defines the N vector and the M magnitude on the MOMENT entry.
Force Phase Angles (Fth1,Fth2,Fth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding force components. These are in degrees.
Moment Phase Angles (Mth1,Mth2,Mth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding moment components. These are in degrees.
Pressure
Object
Type
Analysis Type
Dimension
Pressure
Element Uniform
Structural
2D
Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries. Input Data
Description
Top Surf Pressure
Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. These values are all equal for a given element, producing a uniform pressure field across that face.
Bot Surf Pressure
Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values.These values are all equal for a given element, producing a uniform pressure field across that face.
Edge Pressure
For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (i.e. independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated at the middle of the application region.
Object
Type
Analysis Type
Dimension
Pressure
Element Uniform
Structural
3D
Creates MD Nastran PLOAD4 Bulk Data entries.
234
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Pressure
Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated once at the center of the applied region.
Object
Type
Analysis Type
Dimension
Pressure
Element Variable
Structural
2D
Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries. Input Data
Description
Top Surf Pressure
Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values.
Bot Surf Pressure
Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values.
Edge Pressure
For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (e.g., independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated independently at each node.
Object
Type
Analysis Type
Dimension
Pressure
Element Variable
Structural
3D
Creates MD Nastran PLOAD4 Bulk Data entries.
Chapter 2: Building A Model 235 Loads and Boundary Conditions
Input Data
Description
Pressure
Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for each of the P1 through P4 values.
Temperature
Object
Type
Analysis Type
Temperature
Nodal
Structural
Creates MD Nastran TEMP Bulk Data entries. Input Data
Description
Temperature
Defines the T fields on the TEMP entry.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform
Structural
1D
Creates MD Nastran TEMPRB Bulk Data entries. Input Data Temperature
Description Defines a uniform temperature field using a TEMPRB entry. The temperature value is used for both the TA and TB fields. The T1a, T1b, T2a, and T2b fields are all defined as 0.0.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform
Structural
2D
Creates MD Nastran TEMPP1 Bulk Data entries. Input Data
Description
Temperature
Defines a uniform temperature field using a TEMPP1 entry. The temperature value is used for the T field. The gradient through the thickness is defined to be 0.0.
Object
Type
Analysis Type
Dimension
Temperature
Element Variable
Structural
1D
Creates MD Nastran TEMPRB Bulk Data entries.
236
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Centroid Temp
Defines a variable temperature file using a TEMPRB entry. A field reference will be evaluated at either end of the element to define the TA and TB fields.
Axis-1 Gradient
Defines the temperature gradient in the 1 direction. A field reference will be evaluated at either end of the element to define the T1a and T1b fields.
Axis-2 Gradient
Defines the temperature gradient in the 2 direction. A field reference will be evaluated at either end of the element to define the T2a and T2b fields.
Object
Type
Analysis Type
Dimension
Temperature
Element Variable
Structural
2D
Creates MD Nastran TEMPP1 Bulk Data entries. Input Data
Description
Top Surf Temp
Defines the temperature on the top surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry.
Bot Surf Temp
Defines the temperature on the bottom surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform Element Variable
Structural
1D, 2D, 3D
This option applies only to the P-formulation elements. A TEMPF and DEQATN entry are created for the constant temperature case. A TEMPF and TABLE3D entry are created for the case when a spatial field is referenced. Input Data Temperature
Description Defines the temperature or temperature distribution in the element.
Inertial Load
Object
Type
Analysis Type
Inertial Load
Element Uniform
Structural
Creates MD Nastran GRAV and RFORCE Bulk Data entries.
Chapter 2: Building A Model 237 Loads and Boundary Conditions
Input Data
Description
Trans Accel (A1,A2,A3)
Defines the N vector and the G magnitude value on the GRAV entry.
Rot Velocity (w1,w2,w3)
Defines the R vector and the A magnitude value on the RFORCE entry.
Rot Accel (a1,a2,a3)
Defines the R vector and the RACC magnitude value on the RFORCE entry.
The acceleration and velocity vectors are defined with respect to the input analysis coordinate frame. The origin of the rotational vectors is the origin of the analysis coordinate frame. Note that rotational velocity and rotational acceleration cannot be defined together in the same set.In generating the GRAV and RFORCE entries, the interface produces one GRAV and/or RFORCE entry image for each Patran load set. Initial Displacement
Object
Type
Analysis Type
Initial Displacement
Nodal
Structural
Creates a set of MD Nastran TIC Bulk Data entries. Input Data
Description
Translations (T1,T2,T3)
Defines the U0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Rotations (R1,R2,R3)
Defines the U0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Initial Velocity
Object
Type
Analysis Type
Initial Velocity
Nodal
Structural
Creates a set of MD Nastran TIC Bulk Data entries.
238
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the V0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Rot Veloc (w1,w2,w3)
Defines the V0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Distributed Load
Object
Type
Analysis Type
Dimension
Distributed Load
Element Uniform Element Variable
Structural
1D
Defines distributed force or moment loading along beam elements using MD Nastran PLOAD1 entries. The coordinate system in which the load is applied is defined by the beam axis and the Bar Orientation element property. The Bar Orientation must be defined before this Distributed Load can be created. If the Bar Orientation is subsequently changed, the Distributed Load must be updated manually if necessary. For the element variable type, a field reference is evaluated at each end of the beam to define a linear load variation. Input Data
Description
Edge Distributed Load (f1,f2,f3)
Defines the FXE, FYE, and FZE fields on three PLOAD1 entries.
Edge Distributed Moment (m1,m2,m3)
Defines the MXE, MYE, and MZE fields on three PLOAD1 entries.
Object
Type
Analysis Type
Dimension
Distributed Load
Element Uniform Element Variable
Structural
2D
Defines a distributed force or moment load along the edges of 2D elements. The coordinate system for the load is defined by the surface or element edge and normal. The x direction is along the edge. Positive x is determined by the element corner node connectivity. See Patran Element Library (p. 341) in the Reference Manual - Part III. For example, if the element is a CQUAD4, with node connectivity of 1, 2, 3, 4. The positive x directions for each edge would be from nodes 1 to 2, 2 to 3, 3 to 4, and 4 to 1. The z direction is normal to the surface or element. Positive z is in the direction of the element normal. The y direction is normal to x and z. Positive y is determined by the cross product of the z and x axes and always points into the element. The MD Nastran entries generated, depend on the element type. For the element variable type, a field reference is evaluated at all element nodes lying on the edge.
Chapter 2: Building A Model 239 Loads and Boundary Conditions
Input Data
Description
Edge Distributed Load (f1,f2,f3)
For axisymmetric solid elements (CTRIAX6), the PA, PB, and THETA fields on the PLOADX1 entry are defined. For other 2D elements, the input vector is interpreted as load per unit length and converted into equivalent nodal loads (FORCE entries).
Edge Distributed Moment (m1,m2,m3)
For 2D shell elements, the input vector is interpreted as moment per unit length and converted into equivalent nodal moments (MOMENT entries).
Contact
Object
Type
Analysis Type
Contact
Element Uniform
Structural
This form is used to define certain data for the MD Nastran Input entries. Other data entries are defined under the Analysis Application when setting up a job for nonlinear static or nonlinear transient dynamic analysis. A contact table is also supported; by default, all contact bodies initially have the potential to interact with all other contact bodies and themselves. This default behavior can be modified under the Contact Table form, located on the Solution Parameters subform in the Analysis Application when creating a Load Step. Preview Rigid Body Motion After defining the Input Properties you can use the Preview Rigid Body Motion to check the movement of the rigid bodies in place. This is an effective tool for verifying the directions for LBCs.
240
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Slideline (SOL 400 and SOL 600) Input
Description
Penetration Type
If the Penetration Type is One Sided, nodes in the Slave Region are not allowed to penetrate the segments of the Master Region. If Symmetric, in addition, nodes in the Master Region are not allowed to penetrate segments of the Slave Region.
Static Friction Coefficient (MU1)
Coefficient of static friction between the two surfaces.
Stiffness in Stick (FSTIF)
FSTIF is a penalty parameter in the contact formulation. The default value is usually adequate.
Penalty Stiffness Scaling Factor (SFAC)
SFAC is a penalty parameter in the contact formulation. The default value is usually adequate.
Slideline Width (W1)
Slideline Width is constant along the slideline and is used to determine the area for contact stress calculation. This is the Wi field on the BFRIC entry.
Vector Pointing from A vector must be defined which lies in the contact plane and points from the Master to Slave Surface Master region to the Slave region. This vector is used to define the coordinate system on the BCONP entry and the BLSEG entries for each region.
Chapter 2: Building A Model 241 Loads and Boundary Conditions
Deformable Body (SOL 400, SOL 600, and SOL 700 ) .
Description Friction Coefficient (MU)
Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients, the average value is used.
Define (type of contact) Select 1) Analytic Contact, 2) Contact Area, 3) Exclusion Region, or 4) Glue Deactivation. The Contact Area and Exclusion Region are defined using MD Nastran entry BCHANGE in the .bdf file, with NODE for Contact Area, and EXCLUDE for Exclusion Region. The Glue Deactivation is defined using MD Nastran entry UNGLUE. Boundary Type
Select either 1) Analytic, or 2) Discrete. By default, a deformable contact body boundary is defined by the free faces of its elements; this is used by the Discrete option. However, instead of using the free faces of the elements (Discrete), it is possible to use spline surfaces (2D) to represent the outer faces (element faces) of the contact bodies; this is used by the Analytic option. The Analytic option can improve the accuracy of deformabledeformable contact analysis.
C0 Continuity
Using this, enforces C0-continuity at edges where the normal vector to the outer contour of the structure indicates a discontinuity. This is enabled for 3D analysis only.
Auto Detect Discontinuities
Select this to cause the automatic detection of any discontinuity.
Feature Angle
If the angle between the normals of two touching (adjacent) segments of contact bodies is greater than the Feature Angle, there is a discontinuity there, and the discontinuity (at edge) is preserved.
MFD Increment
The MFD file contains the spline surfaces that were created to represent some or all of the outer faces of the contact model. Using this causes the spline surfaces to be written to an MFD file every nth increment. This file is an Patran database, and can be opened with Patran, and the spline surfaces can be compared with the contact model.
Select Discontinuities...
See Select Deactivation Region, 242
Edge Contact...
See Edge Contact Subform, 242
Select Contact Area...
See Select Contact Area, 242
Select Exclusion Region...
See Select Exclusion Region, 242
Select Deactivation Region...
See Select Deactivation Region, 242
Select Discontinuities Subform
242
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
.
Description Select (entity type)
Choose to either select Geometry or FEM to define any discontinuities.
Detect Discontinuities
Click on this button to determine if there are any discontinuities for the entities that define the Application Region.
Define Discontinuities
Select entities to define the discontinuities.
Edge Contact Subform .
Description Include Outside (Solid Element)
When detecting contact of solid elements (for example, CHEXA elements) use this to include contact of the outside of the elements. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact).
Check Layers (Shell Element)
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges (Edges)
Use this to specify how body surfaces may contact. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact).
Select Contact Area .
Description Select (entity type)
Choose to either select Geometry or FEM to define the contact area.
Define Contact Area
Select entities to define the contact area.
Select Exclusion Region .
Description Select (entity type)
Choose to either select Geometry or FEM to define the exclusion region.
Define Exclusion Region
Select entities to define the exclusion region.
Select Deactivation Region
Chapter 2: Building A Model 243 Loads and Boundary Conditions
.
Description Select (entity type)
Choose to either select Geometry or FEM to define the glue deactivation region.
Define Deactivated Entities
Select entities to define the entities that are to be un-glued.
Rigid Body (SOL 600 and SOL 700 only) The input data form differs for 1D and 2D rigid bodies. One dimensional rigid surfaces are defined as beam elements, or as curves (which may optionally be meshed with beam elements prior to translation) and used in 2D problems. Two dimensional rigid surfaces must be defined as Quad/4 or Tri/3 elements, or as surfaces (which may optionally be meshed with Quad/4 or Tri/3 elements prior to translation) and are used in 3D problems. The elements will be translated as 4-node patches if meshed or as NURB surfaces if not meshed.
244
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input
Description
Flip Contact Side
Upon defining each rigid body, MSC.Patran displays normal vectors or tic marks. These should point inward to the rigid body. In other words, the side opposite the side with the vectors is the side of contact. Generally, the vector points away from the body in which it wants to contact. If it does not point inward, then use the modify option to turn this toggle ON. The direction of the inward normal will be reversed.
Symmetry Plane
This specifies that the surface or body is a symmetry plane. It is OFF by default.
Null Initial Motion
This toggle is enabled only for Velocity and Position type of Motion Control. If it is ON, the initial velocity, position, and angular velocity/rotation are set to zero in the CONTACT option regardless of their settings here (for increment zero).
Motion Control
Motion of rigid bodies can be controlled in a number of different ways: velocity, position (displacement), or forces/moments.
Velocity (vector)
For velocity controlled rigid bodies, define the X and Y velocity components for 2D problems or X, Y, and Z for 3D problems.
Angular Velocity (rad/time)
For velocity controlled rigid bodies, if the rigid body rotates, give its angular velocity in radians per time (seconds usually) about the center of rotation (global Z axis for 2D problems) or axis of rotation (for 3D problems).
Friction Coefficient (MU)
Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients the average value is used.
Rotation Reference Point
This is a point or node that defines the center of rotation of the rigid body. If left blank the rotation reference point will default to the origin.
Axis of Rotation
For 2D rigid surfaces in a 3D problem, aside from the rotation reference point, if you wish to define rotation you must also specify the axis in the form of a vector.
First Control Node
This is for Force or SPCD controlled rigid motion. It is the node to which the force or SPCD is applied. A separate LBC must be defined for the force, but the application node must also be specified here. If both force and moment are specified, they must use different control nodes even if they are coincident. If only 1 control node is specified the rigid body will not be allowed to rotate.
Second Control Node
This is for Moment controlled rigid motion. It is the node to which the moment is applied. A separate LBC must be defined for the moment, but the application node must also be specified here. It also acts as the rotation reference point. If both force and moment are specified, they must use different control nodes even if they are coincident.
Planar Rigid Wall (SOL 700 only)
Chapter 2: Building A Model 245 Loads and Boundary Conditions
Object
Type
Analysis Type
Planar Rigid Wall
Nodal
Explicit Nonlinear
Two different planar rigid wall options exist: 1. Kinematic rigid wall without friction 2. Penalty method based rigid wall with friction These are seen as options at the top of the Input Data form. The user must select which wall will be used. Both wall’s position and orientation are defined by selecting a coordinate system which has its origin on the plane and the local z axis as the outward normal from the contact surface. This defines a WALL Bulk Data entry. There are only parameters associated with the penalty based planar rigid wall. Input Data
Description
Static Friction Coefficient
Static coefficient of friction.
Kinetic Friction Coefficient
Kinetic coefficient of friction.
Exponential Decay Coefficient
Exponential decay coefficient EXP.
Initial Rotation Field (SOL 700 only)
Object
Type
Analysis Type
Init. Rotation Field
Nodal
Explicit Nonlinear
Defines a velocity field of grid points consisting of a rotation and a traslation specification. Creates a TIC3 Bulk Data entry. Input Data
Description
Trans Veloc(v1,v2,v3)
Defines the initial translational velocity values. These are in model length units per unit time.
Rot Veloc (w1,w2,w3)
Defines the initial rotational velocity values. These are in degrees per unit time.
Rotation Center
Defines a point at the center of rotation.
246
Patran Interface to MD Nastran Preference Guide Load Cases
2.10
Load Cases Load cases in Patran are used to group a series of load sets into one load environment for the model. Load cases are selected when defining an analysis job. The usage within MD Nastran is similar. The individual load sets are translated into MD Nastran load sets, and the load cases are used to create the SUBCASE commands in the Case Control Section. For information on how to define multiple static and/or transient load cases, see Load Cases Application (Ch. 5) in the Patran Reference Manual.
Chapter 2: Building A Model 247 Defining Contact Regions
2.11
Defining Contact Regions The MD Nastran preference supports 3D slideline contact functionality introduced in MSC.Nastran Version 68. This capability allows the user to model contact between 2D and 3D structural regions or rigid bodies. This functionality can be accessed by using in the Loads/BCs Application in Patran. After selecting the Contact Object on the main form, the first step is to define the regions that may come into contact. Pushing the Application Region button brings up the following form
248
Patran Interface to MD Nastran Preference Guide Defining Contact Regions
.
Application Region One or more curves, surface edges, or solid edges are defined for the Master and Slave application regions. The application region can only contain geometric entities. To model contact between FEM entities without associated geometry, curves must first be created from the nodes using the tools available in the Geometry application.
Geometry Filter u
Geometry
Master Surface: Slave Surface: Active Region:
Slide Line Slide Line Master
Toggles the select box between Master and Slave regions. The Master and Slave application regions can be defined in either order.
Select Curves Select the curve or edge.
Add
Remove Adds the entities in the Select Curves databox to either the Master Region or Slave Region depending on the setting of the Active Region option menu.
Master Region
Slave Region
OK
Clear
Chapter 2: Building A Model 249 Defining Contact Regions
Contact The second step is to define a set of properties of these contacting surfaces. This is done by pushing the Input Data button on the main Application form to bring up the following subordinate form. If the Penetration Type is One Sided, nodes in the Slave Region are not allowed to penetrate the segments of the Master Region. If Two Sided, in addition, nodes in the Master Region are not allowed to penetrate segments of the Slave Region. This is the PTYPE field on the BCONP entry.
Input Data Penetration Type:
One Sided
Friction Coefficient (MU1)
Stiffness in Stick (FSTIF)
Coefficient of static friction between the two surfaces. This is the MU1 field on the BFRIC entry.
Penalty Stiffness Scaling Factor (SFAC)
FSTIF on the BFRIC entry and SFAC on the BCONP entry are penalty parameters in the contact formulation. The default values are usually adequate.
1.0 Slideline Width (W1)
Slideline Width is constant along the slideline and is used to determine the area for contact stress calculation. This is the Wi field on the BFRIC entry.
A Vector Pointing from Master to Slave Surface
OK
Reset
A vector must be defined which lies in the contact plane and points from the Master region to the Slave region. This vector is used to define the coordinate system on the BCONP entry and the BLSEG entries for each region.
250
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
2.12
Rotor Dynamics The MD Nastran Preference supports steady state and transient rotor dynamics, introduced in MSC.Nastran 2004. This capability allows you to model structures with rotating parts, allowing for gyroscopic effects to be included. Rotor Dynamics are modelled using Rotor and Unbalance entities, created within the Rotor Dynamics... selection under the Tools menu:
Chapter 2: Building A Model 251 Rotor Dynamics
Rotor Dynamics Form The Rotor Dynamics form is accessed from the Rotor Dynamics... selection under the Tools menu. This form is used to create, modify, delete, or show Rotors, which define spin properties, including the axis of rotation, spin direction, damping factor, and speed.
Create Modify Delete Show
Steady State Transient Rotor Unbalance (Transient only)
A set of co-linear nodes that make up the rotor model (spin axis). These are the grids in the MD Nastran ROTORG Bulk Data entry. Two nodes defining the spin direction. These are the GRIDA and GRIDB fields in the MD Nastran RSPINR and RSPINT Bulk Data entries. These nodes must be included in the “Rotor Node List” above. Rotor structural damping factor (default 0.0). This is the GR field of the MD Nastran RSPINR and RSPINT Bulk Data entries.
Spin Profile (Steady State) Spin History (Transient)
252
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Spin Profile Form For Steady State analyses, the Spin Profile form is used to define the relative spin rates.
The unit for the speed entries. RPM for revolutions per minute, or Cycles/Time for frequency. This value defines the SPDUNIT field of the MD Nastran RSPINR Bulk Data entry, and are translated to either ‘RPM’ or ‘FREQ’. List of relative spin rates. Entries must be in ascending or descending order. At least one entry required (no default). These values make up the SPEEDi fields of the MD Nastran RSPINR Bulk Data entry.
Spin History Form For Transient analyses, the Spin History form is used to define the spin rates.
Chapter 2: Building A Model 253 Rotor Dynamics
The unit for the speed entries. RPM for revolutions per minute, or Cycles/Time for frequency. This value defines the SPDUNIT field of the MD Nastran RSPINT Bulk Data entry, and are translated to either ‘RPM’ or ‘FREQ’. A constant multiplier to be applied to the Time Dependent Field.
A time dependent field that defines the spin rate as a function of time. This field, with the Speed Amplitude applied to it, will be translated into an MD Nastran TABLED1 Bulk Data entry that is referenced by the RSPINT entry.
Unbalance Form The Rotor Dynamics Unbalance form is used to create, modify, delete, or show Unbalances, which define unbalance loads for transient analyses in terms of cylindrical system with the rotor axis as the Z axis.
254
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Create Modify Delete Show
The unbalance is applied to a node, which must be included in a transient rotor. When a transient rotor is selected, the “Node” listbox is populated with nodes from that rotor’s axis. The unbalance node may then be selected from that list, assuring that it belongs to an existing transient rotor. This node defines the GRID field of the MD Nastran UNBALNC Bulk Data entry.
Displays the Unbalance Properties form to define the remaining parameters for the MD Nastran UNBALNC Bulk Data entry.
Chapter 2: Building A Model 255 Rotor Dynamics
Unbalance Properties Form The Unbalance Properties Form is used to define the remaining parameters for the Unbalance.
256
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Define the MASS, ROFFSET, and ZOFFSET fields of the MD Nastran UNBALNC Bulk Data entry. For each of these values, either a constant real value may be specified, or a time dependent field my be selected from the list below. Time dependent fields are translated to TABLED1 entries, and referenced by integer ID values in the appropriate UNBALNC fields. Defaults are 1.0 for Radial Offset and 0.0 for Z Offset. There is no default for Mass.
Angular position, in degrees, of the mass in the unbalance coordinate system (default 0.0). This defines the THETA field of the MD Nastran UNBALNC Bulk Data entry. The start and termination times for applying the unbalance load. The default start time is 0.0, while the default termination time is 999999.0. These values define the Ton and Toff fields of the MD Nastran UNBALNC Bulk Data entry. Correction flag to specify whether 1) the mass will be used to modify the total mass in the transient response calculations, 2) the effect of the rotor spin rate change will be included in the transient response calculation, or 3) both. Possible values are None, Mass, Speed, or Both (default None). This value defines the CFLAG field of the MD Nastran UNBALNC Bulk Data entry.
Defines the coordinate system orientation relative to the ACID of the unbalance node (no default). This vector defines the X1, X2, and X3 fields of the MD Nastran UNBALNC Bulk Data entry.
Chapter 2: Building A Model 257 Rotor Dynamics
258
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Chapter 3: Running an Analysis Patran Interface to MD Nastran Preference Guide
3
Running an Analysis
Review of the Analysis Form
Translation Parameters
Solution Types
Direct Text Input
Solution Parameters
Select Superelements
Subcases
Subcase Parameters
Output Requests
Select Superelements
352
Select Explicit MPCs...
443
Non-Structural Mass Properties
Select NSM Properties...
Subcase Select
Restart Parameters
Optimize
Toptomize
Interactive Analysis
260
265
271 276 277 352
354 357
415
451 454
460 462 470
449
444
260
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
3.1
Review of the Analysis Form The Analysis form appears when the Analysis toggle, located on the Patran mainform, is chosen. To run an analysis, or to create a NASTRAN input file, select Analyze as the Action on the Analysis form. Other forms brought up by the Analysis form are used to define translation parameters, solution type, solution parameters, output requests, and the load cases. These forms are described on the following pages. For further information see The Analysis Form (p. 8) in the MSC.Patran Reference Manual.
Chapter 3: Running an Analysis 261 Review of the Analysis Form
Analysis Form This form appears when the Analysis toggle is chosen on the main menu. When preparing for an analysis run, select Analyze as the Action. Actions can be set to: Analyze or Optimize or Toptomize Access Results Read Input File Delete Monitor (if Patran Analysis Manager is installed). Abort (if Patran Analysis Manager is installed). Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual. List of already existing jobs. If one of these jobs is selected, the name will appear in the Job Name list box and all parameters for this job will be retrieved from the database. An existing job can be submitted again by simply selecting it and pushing Apply. It is often convenient to select an existing job, modify a few parameters and push Apply to submit the new job. Name of job. This name will be used as the base file name for all resulting MD Nastran files and message files. This text is used to generate the TITLE entry in the MD Nastran executive control section. Displays the Translation Parameters form to specify parameters not directly related to the solution. These are primarily used by the Application Preferences during the forward translation. Displays the Solution Types form to select the desired type of analysis to run. Opens the Direct Text Input form which allows you to directly enter data for the BULK DATA, Case Control, Executive Control and File Management sections of the NASTRAN input file. Opens the Select Superelements form which allows you to select the superelements active for the specified job. Displays the Subcases form to select a list of load cases to be included in this analysis run. The list of selected load cases is order dependent. Displays the Subcase Select form to select a sequence of subcases associated with an analysis job.
262
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
The following table outlines the selections for the Analyze action. Object Entire Model
Method Full Run Check Run Analysis Deck Model Only Load SimXpert
Selected Group
Full Run Check Run Analysis Deck Model Only Load SimXpert
Existing Deck
Full Run Load SimXpert
Restart
Full Run Check Run Analysis Deck
Interactive
Full Run
The Object indicates which part of the model is to be analyzed. There are four choices: Entire Model, Current Group, Existing Deck, and Restart. • Entire Model is the selected Object if the whole model is to be analyzed. • Selected Group is for specifying the group that contains the model that is to be analyzed. Select
the button Select Group..., under Existing Groups select the desired group, then select Cancel. The name of the selected group will appear in the Analysis form under Group: . For more information see The Group Menu (p. 262) in the Patran Reference Manual. • Existing Deck is selected if you wish to simply submit an existing input file to MD Nastran.
The jobname appearing in the Job Name listbox is appended with the suffix “.bdf” to form the input filename. This file must reside in the current directory. You may also use Existing Deck to directly edit the MD Nastran Bulk Data file.
Chapter 3: Running an Analysis 263 Review of the Analysis Form
• Restart is selected if you wish to restart an analysis. Currently, restarts are only supported for
the Linear Static (101), Nonlinear Static (106), and Normal Modes (103) solution types. The Restart Parameters, 454 form allows you to specify where to resume the analysis. • Interactive analysis utilizes the Patran Preference for MD Nastran capability for performing
visual interactive modal frequency response analysis. The process begins by creating a modal analysis solution using MD Nastran. The interactive modal frequency response analysis is then performed using Patran Analysis: Analyze / Interactive / Full Run. The chain that is followed is 1) using Select Nastran .MASTER... select a .DBALL file, 2) using Create Loading... specify the loading (for example, Acoustic, Force), 3) using Output Requests... specify the desired output, and 4) using View Results... view the results. The Method indicates how far the translation is to be taken.The methods are listed below: • Full Run is the selected type if an Analysis Deck translation is done, and the resulting input file
is submitted to MD Nastran for complete analysis. • Check Run is the selected type if an Analysis Deck translation is done, and the resulting input
file is submitted to MD Nastran for a check run only. • Analysis Deck is the selected type if the Model Deck translation is done, plus all load case,
analysis type and analysis parameter data are translated. A complete input file, ready for MD Nastran should be generated. • Model Only is the selected type if a Bulk Data file is created that contains only the model data
including node, element, coordinate frame, element property, material property, and loads and boundary condition data. The translation stops at that point. • Load SimXpert will lauch SimXpert and automatically transfer the finite element model. The
environment variable MSC_SX_HOME must be set to a valid local installation directory of SimXpert for this capability to be available.
Overview of Analysis Job Definition and Submittal To submit a single load case, linear static analysis job to MD Nastran it is necessary only to click the Apply button on the main Analysis form. Appropriate defaults and selections will be made automatically. Other solution types or multiple load cases will require access to one or more lower-level forms. Several different analysis examples are considered below. To perform a multiple load case, linear static analysis, it is necessary only to open the Subcase Select form. Subcases with the same names as the user-defined load case names and with appropriate defaults can be selected for inclusion in the job. If a change to one or more parameters for a subcase is desired (e.g., to change an output request), the Subcases... form must be accessed. Then it is simple to select a subcase and bring up the appropriate form (e.g., Output Requests) to make changes. For other analysis types (e.g., Normal Modes), the first step is to bring up the Solution Type form and make the appropriate selection. A lower-level Solution Parameters form can be accessed from the Solution Type form to change parameters that affect the overall analysis. Just as for the linear static case, subcases are automatically created for each defined load case. These can be selected on the Subcase Select form or modified on the Subcases form.
264
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
In the Patran MD Nastran Interface, a subcase can be thought of as a Patran load case with some additional parameters (e.g., Output Requests) associated with it. This association is further strengthened since the default subcases are created for each load case and have the same name as their associated load case. In the rest of this document, the terms load case and subcase will generally be used interchangeably. When a specific form is referenced, Load case and Subcase will be capitalized.
Chapter 3: Running an Analysis 265 Translation Parameters
3.2
Translation Parameters Translation parameters define output file formats, numerical tolerances, processing options, numbering offsets, and external include files.
266
Patran Interface to MD Nastran Preference Guide Translation Parameters
Tolerances
• Division - prevents divide by zero errors. • Numerical - determines if two real values are equal. • Writing determines if a value is approximately zero when generating a
Bulk Data entry field. Bulk Data Format
• Sorted Bulk Data - Sorts Bulk Data entries alphabetically. • Card Format - Determines whether the real number can be written to a
standard (8 character) NASTRAN field or to a double (16 character) NASTRAN field. • Write Stored Precision - When ON it writes all data as double precision if
the data double precision information. • Precision Control Options - Specifies where to round off a grid point
coordinate, material, property, or other entity value before its written out to the bdf file. For example if this value is specified as 2 the number 1.3398 will be written out as 1.34. Node Coordinates
Defines which coordinate frame is used when generating the grid coordinates.
Coordinate Frame Coordinates
Defines which coordinate frame is used when generating the grid coordinates. This can be set to reference frame, analysis frame, or global. This should not affect the analysis. It only changes the method used in the grid creation. This determines which coordinate frame is referenced in the CP field of the GRID entry.
MD Nastran Version
Specifies the version of MD Nastran. The version specified here is used for two purposes: to create the full name of the ALTER file to be used, and to determine which Solution Sequence to use. Use only whole numbers and letters; for example, 66a, 67 and 68; 67.5 is the same as 67. This version number can be overridden by setting the environment variable “NASTRAN_VERSION”.
Number of Tasks
Represents the number of processors to be used to run an analysis. It is assumed that the environment is configured for distributed parallel processing.
Write Properties on Element Entries
Specifies that properties will be written to the element entries for all elements where it is allowed in MD Nastran.
Write Continuation Markers
This option is OFF by default. This option can be turned ON to write continuation markers for Bulk Data entries.
Write Global Ply IDs Convert CBARs to CBEAMs
When ON, attempts to keep the Global Ply IDs consistent between MD Nastran and Patran. Converts all CBARs to CBEAMS
Chapter 3: Running an Analysis 267 Translation Parameters
Write PARTSuperelement
This is ON by default and if ON and superelements are selected (see Select Superelements, 352 then BEGIN BULK SUPER = id sections are written in to the input file for each selected superelement. If OFF and superelements are selected, then SESET entries are written instead to define the superelements.
Geometry Check
Use Iterative Solver Ext. Superelement Spec... Numbering Options... Bulk Data Include File...
Checks the element shapes to make sure they are valid. You can set different warning levels from None to Fatal depending on how crucial the element shapes are to your model. Activates the iterative solver for analysis. The analysis manger does not support this option and must be disabled when using this option. Subform used for defining superelement specifications. Subform used to indicate offsets for all IDS to be automatically assigned during translation. Prompts you for the filename of the include file.
268
Patran Interface to MD Nastran Preference Guide Translation Parameters
External Superelement Specifications With this form you can define the options for the External Superelements Bulk Data entry. Please see the MD Nastran Quick Reference Guide for more information about External Superelements.
The available methods are: NONE – No EXTSEOUT entry created. DMIGPCH – Requires an EXTID MATRIXDB DMIGDB DMIGOP2
ASM BULK and EXT BULK require the EXTID method.
Numbering Options This form is activated by the Numbering Options button on the Translation Parameters form. It allows the user to indicate offsets for all IDS to be automatically assigned during translation. For example, if the
Chapter 3: Running an Analysis 269 Translation Parameters
user types 100 into the Element Properties Offset box, the numbering of element properties in the resulting NASTRAN input file will begin at 101.
The Begin. Contin. Marker box allows the user to specify the continuation of the mnemonic format used on multiple line, Bulk Data entries.
IDs Encoded in Names allows the user to activate recognition of IDs encoded into the name of any named entity, such as a material.
Number Only will recognize and use an ID if, and only if, the name of the entity is an actual number like “105.” This option is ON by default. Beginning Number will recognize an ID if the number begins the name, such as “52_shell_property.” This option is OFF by default. Trailing Number will recognize an ID if it trails the name, such as “shell_property_52.” This option is OFF by default. Encoded Syntax will recognize an ID if it directly follows the first occurrence of the specified syntax. For example, with this option activated and the specified syntax set to “.”, the ID assigned to a material given the name “Steel_1027.32” would be 32.
Note that both the Patran Neutral file reader and the Patran MD Nastran input file reader preserve the IDs of named entities with a “.” syntax, so that a NASTRAN PSHELL record of ID 12 will be assigned the name “PSHELL.12.” This last option allows great continuity between input model data and output model data. This option is ON by default and the default Syntax Marker is “.”.
270
Patran Interface to MD Nastran Preference Guide Translation Parameters
Select File
Chapter 3: Running an Analysis 271 Solution Types
3.3
Solution Types The Solution Type form defines the type of analysis and Solution Parameters. Your choice for the Solution Type will in turn affect additional forms you complete for Solution Parameters, 277, Subcase Parameters, 357, and Output Requests, 415. See Table 3-1. To set the Solution Type: Click on the Analysis Application button.
272
Patran Interface to MD Nastran Preference Guide Solution Types
On the Analysis Application form, click Solution Type... and select the Solution Type from the list of available Solution Types. For Analysis Type Explicit Nonlinear:
Solution Type
Defines the solution type.
• Linear Static
Selects Solution Sequence (SOL) 101, 114, 1, or 47 depending on the selected Solution Parameters. You may select one or more subcases in SOLs 1 and 101.
Chapter 3: Running an Analysis 273 Solution Types
• Nonlinear Static
Selects Solution Sequence 66 or 106, depending on the version of MD Nastran. Version 66 and below yields SOL 66, and Version 67 and above yields SOL 106. You may select one or more subcases.
• Normal Modes
Selects Solution Sequence 103, 115, 3, or 48 depending on the Solution Parameters. You may select only one subcase.
• Buckling
Selects Solution Sequence 105, 77, or 5 depending on the selected Solution Parameters. Only one subcase may be selected that defines the static preload. The buckling subcase is automatically generated. The output requests for this Solution Type are applied to the static preload subcase. The default output requests for the buckling subcase are displacements and constraint forces.
• Complex Eigenvalue
Selects Solution Sequence 107, 110, 28, or 29 depending on the selected Solution Parameters. You may select only one subcase.
• Frequency Response
Selects Solution Sequence 108, 111, 118, 26, or 30 depending on the selected Solution Parameters. You may specify only one subcase for Solution Sequences 118, 26, or 30. For Solution Sequences 108 or 111, multiple subcases may be selected.
• Transient Response
Selects Solution Sequence 109, 112, 27, or 31 depending on the selected Solution Parameters. You may specify only one subcase for Solution Sequences 27 or 31. For Solutions Sequences 109 or 112, multiple subcases may be selected.
• Nonlinear Transient
Selects Solution Sequence 99 or 129, depending on the MD Nastran Version. Version 66 and below yields SOL 99; Version 67 and above yields SOL 129. You may select only one subcase.
• Implicit Nonlinear • DDAM Solution • Explicit Nonlinear
Selects Solution Sequence 400 or 600 (depending on “SOL400RUN* toggle). Selects Solution Sequence 187, Dynamic Design Analysis Method (DDAM). Selects Solution Sequence 700.
274
Patran Interface to MD Nastran Preference Guide Solution Types
Select ASET/QSET...
• Select existing Degree of Freedom Lists for use in making an ASET or
a QSET in the input file. • The ASET toggle creates a user selected unreferenced SPOINTS in the
ASET of input file. • The QSET toggle creates a user selected number of unreferenced
SPOINTS in the QSET of the input file. Solution Parameters...
Solution Type Linear Static
Brings up a solution-type-dependent subordinate form that allows you to specify parameters which apply to the complete solution.
Database Run
Cyclic Symmetry
Formulation
MD Nastran Version
Solution Parameter Settings
Off
Off
--
--
1
Off
On
--
--
47
On
Off
--
--
101
On
On
--
--
114
Chapter 3: Running an Analysis 275 Solution Types
Solution Type
Database Run
Cyclic Symmetry
Formulation
MD Nastran Version
Solution Parameter Settings
Nonlinear Static
--
--
--
66 or Below
66
--
--
--
67 or Above
106
Off
Off
--
--
3
Off
On
--
--
48
On
Off
--
--
103
On
On
--
--
115
Off
Off
--
--
5
On
On
--
--
77
On
Off
--
--
105
Off
--
Direct
--
28
Off
--
Modal
--
29
On
--
Direct
--
107
On
--
Modal
--
110
Off
--
Direct
--
26
Off
--
Modal
--
30
On
Off
Direct
--
108
On
--
Modal
--
111
On
On
Direct
--
118
Off
--
Direct
--
27
Off
--
Modal
--
31
On
--
Direct
--
109
On
--
Modal
--
112
--
--
--
66 or Below
99
--
--
--
67 or Above
129
Normal Modes
Buckling
Complex Eigenvalue
Frequency Response
Transient Response
Nonlinear Transient Implicit Nonlinear
400 600
DDAM Solution
2004
187
Explicit Nonlinear
2005
700
276
Patran Interface to MD Nastran Preference Guide Direct Text Input
3.4
Direct Text Input This form is used to directly enter entries in the File Management, Executive Control, Case Control, and BULK DATA sections of the NASTRAN input file. The input file reader also creates these entries for any unsupported entries in the input file. If the data is entered by the user the Write to Input Deck toggle default is ON. If the data comes from the input file reader the default for the Input Deck toggle is OFF. These entries may be reviewed and edited by the user. If they should be written to any input files subsequently created by the interface, the appropriate Write to Input Deck toggle should be set to ON. Text entered into the Case Control section is written to the input file before the first subcase. The Direct Text Input option on the Subcases form should be used to directly enter text within a subcase definition.
Switches to determine which data section the MD Nastran input would be sent.
Saves the current setting and data for the four sections and closes the form.
Clears the current form.
Resets the form back to the data values it had at the last OK.
Resets all four forms back to its previous value and closes the form.
Chapter 3: Running an Analysis 277 Solution Parameters
3.5
Solution Parameters Linear Static This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Linear Static is selected. Depending on the setting of the Database Run and Cyclic Symmetry parameters, this Solution Type will generate a SOL 101, 114, 1, or 47 input file.
278
Patran Interface to MD Nastran Preference Guide Solution Parameters
Database Run
Indicates whether a Structured Solution Sequence (SOL 101 or 114) is to be used or a Rigid Format (SOL 1 or 47). If selected, a Structured Solution Sequence is selected.
Cyclic Symmetry
Indicates that this model is a sector of a cyclically repeating part (SOL 114 or 47).
Automatic Constraints
Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Inertia Relief
Indicates that the inertia relief flags are to be set by including the PARAM, INREL,1 command. This flag can only be chosen if Database Run is selected and Cyclic Symmetry is disabled. If inertia relief is selected, a node-ID for weight generation must be selected. A PARAM, GRDPNT and a SUPORT command will be written to the input file using the same node-ID selected for weight generation. The SUPORT entry will specify all 6 degrees of freedom.
Alternate Reduction
Indicates that an alternate method of performing the static condensation is desired. The PARAM, ALTRED,YES command is included if selected and if Database Run is also selected
SOL 600 Run Contact Parameters Shell Normal Tolerance Angle
Indicates a SOL 600 run. Same as the contact parameters available for the Implicit Nonlinear solution type. Only used with linear contact capability. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Chapter 3: Running an Analysis 279 Solution Parameters
Default Initial Temperature
Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry. Rigid Element Type:
The Rigid element type optionmenu presents three different types of rigid elements, corresponding to the three possible values for the Nastran RIGID= case control. They are:
• LINEAR: Selects linear rigid elements, which are the rigid elements that
have been available in MD Nastran since its inception. • LAGR: Selects the new Lagrange rigid elements with the Lagrange multplier
method. • LGELIM: Selects the new Lagrange rigid elements with the Lagrange
elimination method. See the Nastran quick reference quide for more details. Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
The table outlines the Database Run and Cyclic Symmetry selections, and the SOL types that will be used. Database Run
Cyclic Symmetry
SOL
On
Off
101
On
On
114
Off
Off
1
Off
On
47
Nonlinear Static This subordinate form appears when the Solution Parameters button is selected on the Solution Type form, when Nonlinear Static is selected. If the MD Nastran version specified is Version 66 or lower, then Solution Sequence (SOL) 66 will be employed. However, if the MD Nastran version specified is version 67 or higher, then Solution Sequence 106 will be employed except as described below. For more
280
Patran Interface to MD Nastran Preference Guide Solution Parameters
information about specification of the MD Nastran version number, see the Translation Parameters, 265 form. Indicates that an AUTOSPC entry is requested. MD Nastran will automatically constrain model singularities. Indicates that displacements, which can cause a difference in the formulation of the stiffness matrix, may be encountered. Therefore, the stiffness matrix may need to be periodically recomputed based on the displaced shape. Indicates, as the part deflects, that the applied forces will remain aligned with the deformed part rather than maintaining their global orientation. This can only be selected if Large Displacements is also selected.
The default solution sequence for Nonlinear Static is 106, but can be changed to any one of the following if desired: 400, 600, 700. Only features of 106 are used in any case. For specific features particular to 600 or 700, please use the Implicit Nonlinear type or set the Analysis Type to Explicit Nonlinear, respectively.
Chapter 3: Running an Analysis 281 Solution Parameters
The following table outlines the selections for Large Displacements and Follower Forces, and the altered LGDISP parameter setting for each. Large Displacements
Follower Forces
LGDISP
Off
On
-1
On
On
1
On
Off
2
This is a list of the data input, available for defining the Nonlinear Static Solution Parameters, that were not shown on the previous page. Parameter Name
Description
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
282
Patran Interface to MD Nastran Preference Guide Solution Parameters
Normal Modes This subordinate form appears when Solution Parameters is selected on the Solution Type form when Normal Modes is selected. Use this form to generate a SOL 103, 115, 3, or 48 input file, depending on the Database Run and Cyclic Symmetry parameters below.
See Real Eigenvalue Extraction, 284. Not shown unless Cyclic Symmetry is on. If the version is Version Š 68 and the solution sequence is SOL 103, then these controls are selectable on the Normal Modes Subcase Parameters, 364 form.
The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each. Indicates whether a Structured Solution Sequence (SOLs 103 or 115) is to be used, or a Rigid Format (SOL 3 or 48). If Database Run is selected, a Structured Solution Sequence will be selected. Database Run
Cyclic Symmetry
SOL
On
Off
103
On
On
115
Off
Off
3
Off
On
48
Chapter 3: Running an Analysis 283 Solution Parameters
This is a list of data input, available for defining the Normal Modes Solution Parameters, that were not shown on the previous page. Parameter Name
Description
Cyclic Symmetry
Indicates that this model is a sector of a cyclically repeating part (SOL 115 or 48).
Automatic Constraints
Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
SOL 600 Run Residual Vector Computation Shell Normal Tolerance Angle
Select this to perform a SOL 600 analysis. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run (used to prevent runaway jobs). This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature Rigid Element Type Max p-Adaptive Cycles
Specify the initial temperature. There are three ways to define a rigid element. They are 1) Linear, 2) Lagrangian, or 3) Lgelim. Specify the maximum number of p-Adaptive cycles.
284
Patran Interface to MD Nastran Preference Guide Solution Parameters
Parameter Name
Description
• Dynamic Reduction
Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Real Eigenvalue Extraction
This subordinate form appears when the Eigenvalue Extraction button is selected on the Normal Modes, Frequency Response, or Transient Response Solution Parameters forms. It also appears when the Real Eigenvalue Extraction button is selected on the Complex Eigenvalue Solution Parameter form. Use this form to create either EIGR or EIGRL Bulk Data entries. Defines the method to use to extract the real eigenvalues. This parameter can be set to any one of the following: Lanczos, Automatic Givens, Automatic Householder, Modified Givens, Modified Householder, Givens, Householder, Enhanced Inverse Power, or Inverse Power. If this selection is set to Lanczos, an EIGRL Bulk Data entry should be created. Otherwise, this defines the setting of the METHOD field on the EIGR Bulk Data entry.
Defines the lower and upper limits to the range of frequencies to be examined. These are the F1 and F2 fields on the EIGR Bulk Data entry or the V1 and V2 fields on the EIGRL Bulk Data entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Enhanced Inverse Power or Inverse Power. This is the NE field on the EIGR Bulk Data entry.
Chapter 3: Running an Analysis 285 Solution Parameters
This is a list of data input available for defining the Real Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed. This is the ND field on the EIGR or EIGRL Bulk Data entries.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value between 0 and 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of three settings: Mass, Maximum, or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. Defines the setting of the NORM field on the EIGR Bulk Data entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGR Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGR Bulk Data entry.
286
Patran Interface to MD Nastran Preference Guide Solution Parameters
Dynamic Reduction Parameters
This subordinate form appears when the Dynamic Reduction button is selected on the Normal Modes, Complex Eigenvalue, Frequency Response, or Transient Response Solution Parameters forms. Use this form to create the DYNRED Bulk Data entry. A flag that indicates whether or not any dynamic reduction is desired.
Indicates the maximum frequency to be considered when performing dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON. This is the FMAX field.
Indicates which method is to be used in selecting coordinates. This parameter can be set to either Automatic or Manual. This parameter can only be selected if Perform Dynamic Reduction is set to ON. This determines if the program will automatically select the number of generalized coordinates.
Indicates the number of scalar points that must be retained in this dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON and Method of Coordinate Selection is set to Manual. The Application Preference will automatically create this many SPOINTs, and place them in the a-set and the q-set. Defines the number of generalized coordinates to be included in the dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON, and Method of Coordinate Selection is set to Manual. This is the NQDES field.
Chapter 3: Running an Analysis 287 Solution Parameters
Buckling This subordinate form appears when Solution Parameters is selected on the Solution Type form when Buckling is selected. Use this form to generate a SOL 105, 77, or 5 input file, depending on the setting of the Database Run and Cyclic Symmetry parameters. Indicates that an AUTOSPC entry is requested, so that MD Nastran will automatically constrain model singularities.
Indicates whether a Structured Solution Sequence (SOL 105) is to be used or a Rigid Format or unstructured Solution Sequence (SOL 5 or 77). If Database Run is selected, a Structured Solution Sequence will be selected.
Indicates that this model is a sector of a cyclically repeating part.
See Real Eigenvalue Extraction, 284.
288
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each. Database Run
Cyclic Symmetry
SOL
On
Off
105
On
On
77
Off
Off
5
This is a list of data input available for defining the Buckling Solution Parameters that were not shown on the previous page. Parameter Name
Description
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
• Eigenvalue Extraction
Results Output Format
Brings up the Buckling Eigenvalue Extraction form for defining the eigenvalue extraction controls. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Chapter 3: Running an Analysis 289 Solution Parameters
Buckling Eigenvalue Extraction
This subordinate form appears when the Eigenvalue Extraction button is selected on the Buckling Solution Parameters form. Use this form to create either EIGB or EIGRL Bulk Data entries, depending on the selected extraction method. Defines the method to use to extract the buckling eigenvalues. This parameter can be set to any one of the following: Lanczos, Enhanced Inverse Power, or Inverse Power. If Lanczos is selected, an EIGRL entry will be created. If Inverse Power or Enhanced Inverse Power are selected, and EIGB entry will be created with the METHOD field set to either INV or SINV specified, respectively.
Defines the lower and upper limits to the range of eigenvalues to be examined. These are the L1 and L2 fields on the EIGB entry or the V1 and V2 fields on the EIGRL entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Inverse Power. This is the NEP field on the EIGB entry.
Indicates the limit to how many eigenvalues to be computed. This value can only be selected if Extraction Methods set to Lanczos. This is the NP field on the EIGRL entry.
290
Patran Interface to MD Nastran Preference Guide Solution Parameters
This is a list of data input, available for defining the Buckling Eigenvalue Extraction, that was not shown on the previous page. Parameter Name
Description
Number of Desired Positive Roots
Indicates the limit to how many positive eigenvalues to be computed. This value can only be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDP field on the EIGB entry.
Number of Desired Negative Roots
Indicates the limit to how many negative eigenvalues to be computed. This value cannot be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDN field on the EIGB entry.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value in the range of 0 through 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the NORM field on the EIGB entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGB entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This, too, can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGB entry.
Chapter 3: Running an Analysis 291 Solution Parameters
Complex Eigenvalue This subordinate form appears when Solution Parameters is selected on the Solution Type form when Complex Eigenvalue is selected. When you specify the Database Run and Formulation parameters (from the Solution Type form), Patran generates a SOL 107, 110, 28, or 29 input file.
See Complex Eigenvalue Extraction, 294.
See Real Eigenvalue Extraction, 284.
See Dynamic Reduction Parameters, 286.
292
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If you select Database Run, a Structured Solution Sequence (SOLs 107 or 110) will be selected. If you deselect Database Run a Rigid Format Solution Sequence (SOLs 28 or 29) will be selected. Database Run
Formulation
SOL
On
Direct
107
On
Modal
110
Off
Direct
28
Off
Modal
29
This is a list of data input available for defining the Complex Eigenvalue Solution Parameters that was not shown on the previous page. Parameter Name Automatic Constraints Residual Vector Computation Shell Normal Tolerance Angle
Description Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Chapter 3: Running an Analysis 293 Solution Parameters
Parameter Name
Description
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type Struct. Damping Coeff. • Complex Eigenvalue • Real Eigenvalue • Dynamic Reduction
Results Output Format
There is one rigid element type, Linear. Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value). Brings up the Complex Eigenvalue Extraction form for defining the complex eigenvalue extraction controls. Brings up the Real Eigenvalue Extraction form for defining the real eigenvalue extraction controls. Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
294
Patran Interface to MD Nastran Preference Guide Solution Parameters
Complex Eigenvalue Extraction
This subordinate form appears when the Complex Eigenvalue button is selected on the Complex Eigenvalue Solution Parameters form. Use this form to create an EIGC Bulk Data entry. Defines the method to use to extract the complex eigenvalues. This parameter can be set to any one of the following: Complex Lanczos, Upper Hessenberg, Inverse Power, or Determinate. This defines the setting of the METHOD field.
Defines the real component of the beginning of lines in the complex plane. These values cannot be selected if Extraction Method is set to Upper Hessenberg. This is a list of real values. They are the ALPHAAJ fields.
Defines the real component of the end of lines in the complex plane. These values cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the ALPHABJ fields.
Defines the imaginary component of the beginning of lines in the complex plane. These values cannot be selected if Extraction Method is set to Upper Hessenberg. This is a list of real values. They are the OMEGAAJ fields.
Chapter 3: Running an Analysis 295 Solution Parameters
This is a list of data input available for defining the Complex Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Omega of B Points
Defines the imaginary component of the end of lines in the complex plane. These values cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the OMEGABJ fields.
Width of Regions
Defines the width of the region in the complex plane. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the LJ fields.
Estimated Number of Roots
Indicates an estimate of the number of eigenvalues to be located within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NEJ fields.
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NDJ fields.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This is the NORM field on the EIGC entry.
Normalization Point
Defines the point to be used in the normalization. This is the G field on the EIGC Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Extraction Method is set to Inverse Power or Determinate. This is the C field on the EIGC Bulk Data entry.
296
Patran Interface to MD Nastran Preference Guide Solution Parameters
Frequency Response This subordinate form appears when Solution Parameters is selected on the Solution Type form when Frequency Response is selected. Patran generates a SOL 108, 111, 118, 26, or 30 input file when you specify the Database Run, Cyclic Symmetry, and Formulation parameters (from the Solution Type form).
See Real Eigenvalue Extraction, 284.
See Dynamic Reduction Parameters, 286.
The following table outlines the selections for Database Run, Formulation, and Cyclic Symmetry parameters, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 108, 111, 118) will be selected. If Database Run is deselected, a Rigid Format (SOLs 26 or 30) will be selected.
Chapter 3: Running an Analysis 297 Solution Parameters
Database Run
Formulation
Cyclic Symmetry
SOL
On
Direct
Off
108
On
Direct
On
118
On
Modal
--
111
Off
Direct
--
26
Off
Modal
--
30
This is a list of data input, available for defining the Frequency Response Solution Parameters that were not shown on the previous page. Parameter Name Cyclic Symmetry
Automatic Constraints Residual Vector Computation Shell Normal Tolerance Angle
Description Indicates that this model is a sector of a cyclically repeating part, and the appropriate flags will be set. This can only be set if Database Run is selected and Formulation is set to Direct (SOL 118). Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
298
Patran Interface to MD Nastran Preference Guide Solution Parameters
Parameter Name Node ID for Wt. Gener.
Description Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type Struct. Damping Coeff.
There is one rigid element type, Linear. Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value).
• Eigenvalue Extraction
Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal.
• Dynamic Reduction
Calls up another form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Chapter 3: Running an Analysis 299 Solution Parameters
Transient Response This subordinate form appears when Solution Parameters is selected on the Solution Type form when Transient Response is selected. Patran generates a SOL 109, 112, 27, or 31 input file, when you specify Database Run and Formulation parameters (from the Solution Type form).
These options are only available for a "Modal" solution.
300
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 109, 112) will be selected. If Database Run is deselected, a Rigid Format (SOLs 27 or 31) will be selected. Database Run
Formulation
SOL
On
Direct
109
On
Modal
112
Off
Direct
27
Off
Modal
31
This is a list of data input available for defining the Transient Solution Parameters that was not shown on the previous page. Parameter Name Automatic Constraints Residual Vector
Description Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Computation
The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
SOL 600 Run
Select this to perform a SOL 600 analysis.
SOL 700 Run
Select this to perform a SOL 700 analysis. To do this is necessary to use the Direct method.
Shell Normal
Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Tolerance Angle Mass Calculation
Defines how the mass matrix will be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Chapter 3: Running an Analysis 301 Solution Parameters
Parameter Name
Description
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type
There is one rigid element type, Linear.
Struct. Damping Coeff.
Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor
Defines W3 and W4 parameters. These parameters alter the damping characteristics of the model.
W4, Damping Factor1 • Eigenvalue
Extraction • Dynamic Reduction
Results Output Format
Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal. Calls up the Dynamic Reduction Parameters form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
302
Patran Interface to MD Nastran Preference Guide Solution Parameters
Nonlinear Transient This subordinate form appears when Solution Parameters is selected on the Solution Type form when Nonlinear Transient is selected. Use this form to generate either a SOL 99 or a SOL 129 input file, depending on the version of MD Nastran indicated on the translation parameter form except as indicated below. Version 66 and below yields SOL 99 and Version 67 and above yields SOL 129. Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The default solution sequence for Nonlinear Transient is 129, but can be changed to any one of the following if desired: 400, 600, 700. Only features of 129 are used in any case. For specific features particular to 600 or 700, please use the Implicit Nonlinear type or set the Analysis Type to Explicit Nonlinear, respectively.
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Indicates how the data file entry images are to be printed in theMD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Chapter 3: Running an Analysis 303 Solution Parameters
This is a list of data input available for defining the Nonlinear Transient Solution Parameters that was not shown on the previous page. Parameter Name
Description
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Struct. Damping Coeff.
Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor
Define W3 and W4 parameters. These parameters alter the damping characteristics of the model.
W4, Damping Factor Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
304
Patran Interface to MD Nastran Preference Guide Solution Parameters
Implicit Nonlinear This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Implicit Nonlinear is selected. Use this form to generate a SOL 400 or 600 input file.
The default solution sequence for Implicit Nonlinear is 600. By toggling the “SOL 400 Run” ON, Patran will write a SOL 400 input file. Not all features of SOL 600 are accessible using SOL 400, so use with caution and check your input file and results carefully.
Solver / Options...
See Solver Options Subform (SOL 600), 306.
Contact Parameters...
See Contact Parameters Subform, 307.
Direct Text Input...
This subform is used to directly enter entries in the File Management, Executive Control, Case Control, and Bulk Data sections of the MD Nastran input file. See Direct Text Input, 276.
Restart Parameters...
See Restart Parameters Subform, 315.
Advanced Job Control...
See Advanced Job Control Subform (SOL 600), 317.
Chapter 3: Running an Analysis 305 Solution Parameters
Domain Decomposition...
See Domain Decomposition, 318.
Assumed Strain
For SOL 600, if ON, (default is ON), places the MARCASUM parameter into the input file. This forces all elements that can deal with assumed strain to use this formulation. This improves the bending behavior of Marc elements 3, 7, and 11. For SOL 400, the NLMOPTS entry is written with the ASSUM option. Again, this is a global setting and forces all elements that can use this formulation to adopt it.
Constant Dilatation
If ON, (default is OFF), places the MARCDILT parameter into the input file. This will force all elements that can deal with constant dilatation (for nearly incompressible analysis) to use this formulation. This affects Marc element types 7, 10, 11, 19, and 20 only and recommended for elastic-plastic and creep analysis. (SOL 600 only)
Plane Stress
Replaces plane strain elements with plane stress elements. (SOL 600 only)
Reduced Integration
Specifies that a lower number of element integration points be used to integrate exactly. (SOL 600 only)
Creep
For SOL 400, writes the NLMOPTS entry with the CREEP option defaults for creep analysis.
Shell Shear Correction
For SOL 400 (only), forces all shell elements using nonlinear formulations to use the shear correction. This writes the NLMOPTS entry with the TSHEAR option.
SOL 400 Run
Use this to select a SOL 400 simulation, instead of a SOL 600 simulation.
Default Initial or Load Temperature
For SOL 400 allows for specification of a general initial temperature and a general loading temperature. TEMPD entries are written for both with Case Control TEMPERATURE(INITIAL) and TEMPERATURE(LOAD) entries calling out the corresponding TEMPD entries in the bulk data.
Results Output Format...
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
306
Patran Interface to MD Nastran Preference Guide Solution Parameters
Solver Options Subform (SOL 600) Specifies the solver to be used in numerically inverting the system matrix of linear equilibrium equations.
Inconsistent MPCs
There are three choices for dealing with problem MPCs, 1) Reorder (reorder the DOFs that are used to define the problem MPCs), 2) Continue (continue the analysis with no changes to the MPCs DOFs), or 3) Stop (stop the analysis).
Solver Type
Chooses Direct Profile, Iterative Sparse, Direct Sparse , Hardware Sparse, Multifrontal Sparse (default), or External Sparse as the solver.
Non-Symmetric
Specifies non-symmetric for Solver Type of Direct Profile or Multifrontal Sparse.
Non-Positive Definite
Specifies non-positive definite option valid for all solver types, use ON. On by default in SOL 600, use Nastran Default. Can un select this option by using OFF.
Memory
Defines the amount of work space in words. This can be left blank and the translator will automatically determine this based on model size.
Multifrontal Sparse Parameters
Chapter 3: Running an Analysis 307 Solution Parameters
• Out-of-Core Threshold
For Hardware and Multifrontal Sparse solvers only. Default is 100. Represents the number of real*4 words in millions of words. Only for SGI computers running the IRIX operating system.
Bandwidth Optimization
Turns on the optimize option for the Direct Profile or Multifrontal Sparse solvers and uses the Sloan algorithm. Other solvers have their own optimizer and use it by default.
Contact Parameters Subform Defines options for detecting and handling contact.
308
Patran Interface to MD Nastran Preference Guide Solution Parameters
Deformable-Deformable Method
In Double-Sided method, for each contact body pair, nodes of both bodies will be checked for contact. In Single-Sided method, for each contact body pair, only nodes of the lower-numbered body will be checked for contact. Results are dependent upon the order in which contact bodies are defined.
Optimize Constraint Equations
Use this to decrease the bandwidth of the model.
Contact Detection...
See Contact Detection Subform, 309.
Separation...
See Separation Subform, 311.
Friction Parameters...
See Friction Parameters Subform, 312.
Enable Initial Contact
Click on checkbox to activate the capability for control of initial contact. The initial contact is for creating an MD Nastran entry BCTABLE with ID = 0 to be used for increment 0. For SOL 600, this causes rigid contact bodies to be moved so they just touch adjacent flexible contact bodies. For SOL 101 and 400, a BCTABLE is used with ID = 0, which causes rigid contact bodies to be moved, as for SOL 600, and/or adjusting the coordinates of all active nodes on the surface of all deformable BCBODYs to remove any prestressed condition.
Initial Contact...
See Initial Contact Subform, 314.
Penetration Check
This controls contact penetration checking, sometimes referred to as the increment splitting option. Available options are: At End of Increment, Per Iteration (default), Suppressed (Fixed), Suppressed (Adaptive). At End of Increment means penetration is checked at the end of a load increment. Per Iteration means that penetration is checked at the end of every iteration within an increment. If penetration is detected, increments are split. Suppress is to suppress this feature for Fixed and Adaptive load stepping types.
Reduce Printout of Surface Definition
This controls reduction of printout of surface definition.
Chapter 3: Running an Analysis 309 Solution Parameters
Contact Detection Subform
On the Contact Control Parameters subform, select Contact Detection... This form controls general contact parameters for contact detection.
310
Patran Interface to MD Nastran Preference Guide Solution Parameters
Distance Tolerance
Distance below which a node is considered touching a body (error). Leave the box blank to have MSC.Marc calculate the tolerance as the smaller of 1/20 element edge length or 1/4 shell thickness.
Bias on Distance Tolerance
Contact tolerance BIAS factor. The value should be within the range of zero to one. Models with shell elements seem to be sensitive to this parameter. You may need to experiment with this value if you have shell element models that will not converge. The SOL 600 default is 0.9.
Suppress Bounding Box Check
Turn ON this button if you want to suppress bounding box checking. This might eliminate penetration, but slows down the solution.
Include Outside (Solid Element) When detecting contact of elements (beam/bar, shell, solid elements) use this to include contact of the outside of the elements. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid). Include Outside (Rigid Surface) When detecting contact of rigid surfaces use this to include contact of the edges of the surfaces. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid). Check Layers
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges
Use this to detect contact of edges. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid).
Activate Quadratic Contact
Use this to detect the contact of the edges of quadratic elements (midside nodes).
Activate 3D Beam-Beam Contact
Turn this button ON to activate 3D beam-beam contact. Activate 3D BeamBeam Contact enters a one(1) in the 13th field of the 2nd data block. This creates the MD Nastran Bulk Data entry BCPARA, and uses the entry BEAMP.
Chapter 3: Running an Analysis 311 Solution Parameters
Separation Subform
On the Contact Control Parameters subform, select Separation... This form controls general contact parameters for contact separation.
Maximum Separations
Maximum number of separations allowed in each increment. Maximum Separations is entered in the 6th field of the 2nd data block. Default is 9999.
Retain Value on NCYCLE
Turn ON this button if you do not want to reset NCYCLE to zero when separation occurs. This speeds up the solution, but might result in instabilities. You can not set this and Suppress Bounding Box simultaneously. Retain Value of NCYCLE enters a three(3) in field 8 of the 2nd data block.
Increment
Specifies whether chattering is allowed or not. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
Chattering
Specifies the separation criterion (forces or stresses) and the critical value at which the separation will take place. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
312
Patran Interface to MD Nastran Preference Guide Solution Parameters
Separation Criterion
Specifies in which increment (current or next) the separation is allowed to occur. Separation Criterion enters a one(1) in the 12th field of the 2nd data block if separation is based on stresses.
Force Value Stress Value
Force/Stress Value is placed in the 5th field of the 3rd data block.
Friction Parameters Subform
On the Contact Control Parameters subform, select Friction Parameters...
Chapter 3: Running an Analysis 313 Solution Parameters
Friction Type
Available options for friction Type are: None (default), Shear (for metal forming), Coulomb (for normal contact), Shear for Rolling, Coulomb for Rolling, StickSlip, Bilinear Shear, and Bilinear Coulomb. The MD Nastran entry BCPARA is written to the .bdf file, with FTYPE used. Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction. Stick-Slip is a Coulomb type friction.
Method
For Coulomb type of friction models (options 2, 4, and 5 above), there are 2 methods for computing friction: Nodal Stress, Nodal Force (default). Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction.
Relative Sliding Velocity
Critical value for sliding velocity below which surfaces will be simulated as sticking. Relative Sliding Velocity is placed in the 1st field of the 3rd data block for all friction models except Stick-Slip.
Transition Region
Slip-to-Stick transition region. Transition Region is placed in the 1st field of the 3rd data block for Stick-Slip model.
Multiplier to Friction Coefficient
Friction coefficient multiplier. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Friction Force Tolerance
Friction Force Tolerance. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Heat Generation Conversion Factor
A factor related to how much heat is generated by the friction process.
314
Patran Interface to MD Nastran Preference Guide Solution Parameters
Initial Contact Subform
On the Contact Control Parameters subform, select Initial Contact...
Chapter 3: Running an Analysis 315 Solution Parameters
Restart Parameters Subform Includes a Restart option in the MD Nastran input file. Restarts are only supported for SOL 600 in the current release.
Restart Type
You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File
If when restarting a job, you wish the results form the previous run to be copied into the new POST file, then turn this ON. This will place the RESTART or RESTART LAST options before the POST option in the input file. Otherwise they are placed after the POST option which flags MSC.Marc not to copy the results to the new POST file. If you turn this ON, you must have a restarname.t16 and/or restartname.t19 file in your local directory or the MSC.Marc analysis will fail.
Last Converged Increment
Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto
OFF by default. This places a REAUTO option in the input file. Any additional data needed for the REAUTO option are extracted from the first Load Step information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user.
316
Patran Interface to MD Nastran Preference Guide Solution Parameters
Restart from Increment
Defines the increment to be read from the file specified in the Select Restart File form. This is entered in the 3rd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing
Defines the number of increments between writing data to the restart file. This is entered in the 2nd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Write or Read and Write. When Last Converted Increment is ON, this is the 4th field of the 2nd data block of the RESTART LAST option.
Select Restart File...
This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write. This file is specified on the command line for invoking the MSC.Marc solver using the -r option.
Chapter 3: Running an Analysis 317 Solution Parameters
Advanced Job Control Subform (SOL 600) Sets alternate versions of the solver and alternate formats for the results file, for SOL 600 jobs.
Marc Version
Specifies the version of MSC.Marc to run the analysis.
Marc Results File Format
Specifies the file format for the output from the analysis.
Marc Results File Type
Defines the binary output and/or text format of output from the analysis. Binary is recommended since .t16 files are linarily compatible across platforms and take up less space.
318
Patran Interface to MD Nastran Preference Guide Solution Parameters
Marc scratch files w/ Nastran’s Use Environment Variables
Use to enable the use of environment variables.
Suppress Non-SOLMARC Errors
Suppress errors that are not SOL 600 errors.
Submit Marc Job
Submit SOL 600 jobs to Marc.
Use Marc License
Use this to search for, then use Marc licenses.
Copy Marc Files
Make copies of Marc files; for example copy .t16 file.
Filter Marc Text Delete Marc Files
Delete Marc files after the corresponding Patran files are created.
Gradually Release Constraints Analysis Control Defaults
Creates the Nastran Bulk Data entry PARAM, MARCDEF. Its three values are Nastran Development (recommended by Nastran development; Marc SHELL_SECT parameter is set to 11), Marc-Mentat (current Marc standard), Marc Development (recommended by both Marc and Nastran development).
Marc Submit Command
Locates the submit command to run the MSC.Marc analysis (optional). For Specify Full Command its list box will be un-ghosted.
Domain Decomposition Domain Decomposition is used to partition the model into seperate parts (domains) for parallel processing. The Method used to do this is named Domain Decomposition Method (DDM). This form designates that domain decomposition be done manually, semi-automatically, or automatically, for either SOL 400 or SOL 600 jobs.
Chapter 3: Running an Analysis 319 Solution Parameters
320
Patran Interface to MD Nastran Preference Guide Solution Parameters
Decomposition Method
Set this to Automatic if you wish MD Nastran to automatically create the domains during analysis run time. Set to Semi-Automatic if you wish to have MSC.Patran automatically break the model into domains which can be visualized before submittal. Set to Manual to have full control over the domains. This requires the creation of the groups before they can be selected here in this form and associated to a domain.
Number of Domains
This determines how many domains are to be created. When you change this number and press the Enter or Return key, the spread sheet updates with this number of rows. The default is 1. This corresponds to the number of CPUs desired to run the job. For the Automatic method, this is the only input that is required and the spreadsheet is not visible.
Model or Current Group
This is for choosing a part of the model to decompose for parallel processing: Model -- decompose all of the model, Current Group -decompose just the current group. This choice must be consistent with what part of the model is specified for analysis (Analysis: Analyze / Entire Model or Selected Group). This is only active if Decomposition Method is set to Automatic or Semi-Automatic.
Metis Method
There are three Methods that can be used to partition the Model or Current Group into Domains. They are, 1) Nodal Position, 2) Element Topology, or 3) Best (a procedure that accounts for the best of the nodal, element, or vector type algorithms). This method can only be used if Decomposition Method is set to Automatic.
Domain Island Removal
Using this option causes some parts of disjoint domains (domain islands) to be combined with adjacent domains. This can only be used if Decomposition Method is set to Automatic.
Coarse Graph
Using this option sometimes produces domain islands (disjoint domains). This option (the default) is recommended to reduce the time to decompose the initial global domain. Use this only if there is a definite need for a better decomposition. This can only be used if Decomposition Method is set to Automatic.
Single POST File
If more than one CPU processor is used to solve the problem, the seperate/multiple results files can be compiled into a single file for postprocessing using Single POST File.
Create
Click Create to create Domain Information spreadsheet rows. After doing this the number of rows will equal the value of Number of Domains in the form. If Decomposition Method is set to Manual, the previously created group names will be selectable in Select a Group window at the bottom.
Visualize
This is used to display groups. Select a group name for the heading Domain Information under Group. Click Visualize to display just that group. This can be done for some or all of the groups.
Chapter 3: Running an Analysis 321 Solution Parameters
Reset Graphics
Click Reset Graphics to reset the viewport graphics.
Validate
This is for validating (checking) that the domains are not disjoint. For two adjacent domains, the nodes at the interface of the domains must be in both domains.
Domain Information
The window with the definition of each Domain. For a given Domain there is a corresponding unique Group name.
DDAM DDAM is an acronym for Dynamic Design Analysis Method, or DDAM is a methodology for analyzing ship-mounted equipment that the US Navy uses in the event of a near-miss underwater. Most FEA products follow the DDAM methodology, as does any hand calculation. MSC has made several improvements to its products that make DDAM easier to use. To accommodate the special spectrum and summing conventions MSC made several modifications to MD Nastran. A DMAP alter in MD Nastran puts out data important for a DDAM analysis. A stand-alone Fortran program reads the MD Nastran data, calculates the spectral data, formats DDAM run information, and sends data back to MD Nastran for further postprocessing. MSC’s DDAM has the following capabilities. • Calculates all three shock directions simultaneously. • Automatically calculates the appropriate spectra from input of the coefficients. • Performs the NRL sum. • Contains modal selection following 3010 Rev 1 convention. • Provides manual mode selection if needed. • Provides mode-by-mode output if desired. • Uses all available MD Nastran elements. • Provides NRL summed output in MD Nastran OP2 format for use with most postprocessors. • Offers an alternate coefficient input method is available that avoids using the Fortran program,
but the classified coefficients must be entered directly in the data file. • Has unlimited model size. • Uses MSC’s Lanczos Eigenvalue solver for fast solutions.
DDAM has the following limitations. • All base input points must be rigidly connected to a single grid flagged on a SUPORT entry. • There is no easy method to handle closely spaced modes as defined by 3010. • MD Nastran printed output (.f06 file) is not labeled well, and must be used carefully in order to
avoid mistakes. This is especially true of the mode-by-mode output. • A DDAM data file will not read into Patran/MSC.FEA completely.
322
Patran Interface to MD Nastran Preference Guide Solution Parameters
• .XDB output not available for NRL summed quantities • MD Nastran requires additional input switch to be toggled in Patran in order to plot NRL
summed von Mises and combined beam stresses. • MD Nastran does not calculate beam and bar shear stresses. They are not included in the von
Mises and combined stresses reported by MD Nastran DDAM. DDAM in Patran DDAM in MD Nastran is a process that involves three main parts, and a number of smaller parts. The entire procedure is accessed from a simple interface in Patran that integrates the process. • Part 1, Modal Analysis - A modal analysis is run in MD Nastran. This supplies the frequencies,
mode shapes and modal participation for the model. • Part 2, Spectrum Generation – Using the output from Part 1, you can use a Fortran program to
calculate the shock spectrum. This is based on the DDS-072 or NRL 1396 documents, or you can manually enter your own spectrum. • Part 3, Spectrum Application and Data Recovery – The calculated spectrum from Part 2 is
applied to the mode shapes calculated in Part 1, and the results are calculated on a mode-bymode basis. The results from this are then summed using an NRL sum to produce results, one set for each shock direction. The Patran interface presents you with a selection of options to calculate the spectrum and sum the results. The options are stored, and when the MD Nastran modal analysis completes, the Fortran program automatically starts, using the stored options to drive it. MD Nastran automatically resumes after the completion of the Fortran program and finishes the analysis. During is process, a number of files will be created that are inputs and outputs from this process, all named jobname.xxx using the jobname chosen in Patran. The most important files are: jobname.ddd – the DDAM potions file that drives the Fortran program jobname.f11 – the modal information needed to calculate the spectrum jobname.f13 – the calculated spectra information for input back into MD Nastran jobname.ver – modal verification file jobname.opw – Nastran OP2 file with the mode shapes jobname.opx – Nastran op2 file with the NRL summed results for x-shock jobname.opy – Nastran op2 file with the NRL summed results for y-shock jobname.opz – Nastran op2 file with the NRL summed results for z-shock Once the run is complete, you can look over both the results and the modal verification file. If the results are not as expected or desired, there are a number of more advanced capabilities of this DDAM procedure for more control over the process. These include some that are on the Patran forms (changes in 80%
Chapter 3: Running an Analysis 323 Solution Parameters
criterion, minimum G value) and ones that can be accessed using the Patran Direct Text capability (modeby-mode output, specific mode selection). DDAM Model Preparation
In order to run DDAM, all of the fixed base points (excitation inputs) in the model must be rigidly connected to a single point. The MD Nastran RBE2 element is used for this, connecting the independent node (the SUPORT point) to all of the other fixed base/excitation points (dependent grids) in all 6 degrees of freedom. This point is flagged for the SUPORT entry in the DDAM setup. It is not necessary that this point is separated (spatially) from the other input points, you can select one of the base points to be the SUPORT point, as long as all the excitation points are then connected to it. It is not advisable to have any other translational constraints in the model, as they will remove modal mass from the model and the 80% criterion will not necessarily be correct, and the model will have base points that will not be excited. You may have rotational constraints to hold shafting and to remove plate and bar singularities, as the rotational components are not used in the DDAM excitation. No loads or other boundary conditions are needed for the analysis. As per 3010, you need to add operating loads to the shock loads at the conclusion of the analysis. Set up the model like any other modal analysis, with the exception of the SUPORT point. Mass and material density are required to obtain correct mode shapes. The modal analysis parameters are set up on the Subcase Options form, where you can select the number of desired modes, the lower frequency bound, and an upper frequency bound. The analysis uses a Lanczos extraction routine with mass normalization, and uses the default Lanczos debugging information level. You will not have control over these parameters in DDAM.
324
Patran Interface to MD Nastran Preference Guide Solution Parameters
DDAM Solution Parameters
This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when DDAM is selected. Use this form to generate a SOL 187 input file.
Automatic Constraints
Indicates that an AUTOSPC entry is requested. MD Nastran will automatically constrain model singularities.
Shell Normal Tol. Angle
Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Chapter 3: Running an Analysis 325 Solution Parameters
• Lumped • Coupled
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo • None • Sorted • Unsorted
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node id for Wt. Gener
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Initial Temperature
Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature
Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry.
SUPPORT Node
Selects the point you have chosen for your base input. Note that this is a required choice with no default, and that you can only pick one node. If multiple nodes are entered in the data box, only the first one is used.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
326
Patran Interface to MD Nastran Preference Guide Solution Parameters
Explicit Nonlinear This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Explicit Nonlinear is selected under Preferences: Analysis... . Use this form to generate a SOL 700 input file.
Parameter Name Large Displacements
Description Use this to cause the large displacement formulation to be used.
Follower Forces
Use this to cause the forces to move (translate and rotate) with the model.
Prestress Option
Use this to cause the pre-stresses to be calculated.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Chapter 3: Running an Analysis 327 Solution Parameters
Parameter Name
Description
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
SOL 700 Default Settings • Sol700 Parameters...
Either Dytran or Ls-Dyna default settings can be used. Displays the Sol700 Parameters and Extra Data form that is used for specifing parameter values for such things as execution control, dynamic relaxation (entry DAMPGBL), general parameters, contact, and Eulerian parameters. See Sol700 Parameters Subform, 327
• Resultts Output
Format...
Use this to specify the types of files that are to be written for the SOL 700 analysis. For example, XDB (jobname.xdb) and Print (jobname.f06).See Results Output Format, 348
Sol700 Parameters Subform This subordinate form appears when Sol700 Parameters button is selected on the Solution Parameters form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
328
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Execution Control Parameters...
DYSTATIC, DYBLDTIM, DYINISTEP, DYTSTEPERODE, DYMINSTEP, DYMAXSTEP, DYSTEPFCTL, DYTERMNENDMAS, DYTSTEPDT2MS
Dynamic Relaxation...
This is for specifying the entries for the DAMPGBL Bulk Data entry. This is for defining parameter values for static analysis using dynamic relaxation for SOL 700 only.
Chapter 3: Running an Analysis 329 Solution Parameters
Form
Parameters
General Parameters...
DYLDKND, DYCOWPRD, DYCOWPRP, DYBULKL, DYHRGIHQ, DYRGQH, DYENERGYHGEN, DYSHELLFORM, DYSHTHICK, DYSHNIP
Contact Parameters...
DYCONSLSFAC, DYCONRWPNAL, DYCONPENOPT, DYCONTHKCHG, DYCONENMASS, DYCONECDT, DYCONIGNORE, DYCONSKIPTWG
Binary Output Database File Parameters...
DYBEAMIP, DYMAXINT, DYNEIPS, DYNINTSL, DYNEIPH, DYSTRFLG, DYSIGFLG, DYEPSFLG, DYRLTFLG, DYENGFLG, DYCMPFLG, DYIEVERP, DYDCOMP, DYSHGE, DYSTSSZ, DYN3THDT
Time History Output This is for specifying the type of output file (Binary, ASCII, Both), and the Request... Output Time Interval. Hourglass Setting...
See Hourglass Setting Subform, 329
Merge Rigid Mat...
See Merge Rigid Material Subform, 331
Dynamic Relaxation for Restart...
See Dynamic Relaxation for Restart Subform, 333
Damping Per Property...
See Damping Per Property Subform, 335
Rigid Body Switch and Merge...
See Rigid Body Switch and Merge Subform, 337
Eulerian Parameters...
See Eulerian Parameters Subform, 343
SPH Control Parameters...
See SPH Control Parameters Subform, 346
Hourglass Setting Subform This subordinate form appears when Hourglass Setting button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
330
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
Chapter 3: Running an Analysis 331 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Existing Hourglass Setting
List of previously created hourglass settings.
Hourglass Name
Specify the name.
Property Type
Specify either a Shell (2D) or Solid (3D) element type.
Control Type
Choose one of several types of controlling the hourglass effects. The choices are: 1) Standard LSDyna Viscous (Property Type = Shell or Solid), 2) Flanagan-Belytschko Viscous (Property Type = Shell or Solid), 3) Flan-Bely. Visc. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 4) Flanagan-Belytschko Stiffness (Property Type = Shell or Solid), 5) Flan-Bely. Stiff. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 6) Flanagan-Bindeman Stiffness (Property Type = Solid), 7) Fully Integrated Shell (Property Type = Shell). These entries are defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Hourglass Coefficient
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Warping Hourglass Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Bending Hourglass Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Linear Bulk Visc. Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Quadr. Bulk Visc. Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Select Property Set
Select a previously created element property. For example, Properties > Create > 2D > Shell > Options: Explicit PSHELL1 > Input Properties... > Shell Formulations > HUGHES.
Add
Click Add after input all necessary data into the Hourglass Setting form to create an Existing Hourglass Setting.
Modify
Click Modify after input all changed data into the Hourglass Setting form to update an Existing Hourglass Setting. You must first select the particular Existing Hourglass Setting.
Merge Rigid Material Subform This subordinate form appears when Merge Rigid Mat button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:
332
Patran Interface to MD Nastran Preference Guide Solution Parameters
• SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 333 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Existing Merged Materials
List of previously merged MATRIG materials. MATRIG is an MD Nastran Bulk Data entry for defining rigid body properties.
Merged Material Name
Specify the name of merged material to be created.
Select Material to be Merged into
Specify the name of an MATRIG material to merge other MATRIG materials into.
Select Materials to be Merged
Specify the names of MATRIG materials that are to be merged into the merged material whos name is specified under Merged Material Name.
Add
Click Add after input all necessary data into the Rigid Materials form to create an Existing Merged Materials.
Modify
Click Modify after input all changed data into the Rigid Materials form to update an Existing Merged Materials. You must first select the particular Existing Merged Materials.
Dynamic Relaxation for Restart Subform This subordinate form appears when Dynamic Relaxation for Restart button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
334
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form Relaxation [Termination Time] Convergence Tolerance Number of Iterations Papadrakakis Auto Control
Parameters Use this to not use (None Active) or use (Activated Relaxation) relaxation in performing the simulation. The time to stop the simulation. This is optional ([ ]). Specify convergence tolerance. Specify the maximum number of iterations. Click the checkbox to specify that convergence control is to be automatic using the Papadrakakis method.
Chapter 3: Running an Analysis 335 Solution Parameters
Form Papadrakakis Convergence Tolerance
Parameters To use this it is necessary to not select Papadrakakis Auto Control.
Relaxation Factor Time step scale Factor
Specify the value of the Relaxation Factor. Specify the value of the Time step scale Factor.
Damping Per Property Subform This subordinate form appears when Damping Per Property button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
336
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Damping Type
Select either Property (use property) or Stiffness (use Rayleigh damping).
System Damping Constant Table
Select a time dependent field under Time Dependent Field. This field will be multiplied by the Scalar Factor for Load Curve entry. The (X,Y,Z) Trans. Damping Forces and (X,Y,Z) Rot. Damping Moments entries (all of these form a 6 component load vector) are multiplied by the scaled time dependent field.
Chapter 3: Running an Analysis 337 Solution Parameters
Form
Parameters
Time Dependent Field
Select a Field, with it being entered into the System Damping Constant Table list box. For example, select the field named damping_vs_time under Time Dependent Field. For System Damping Constant Table f:damping_vs_time appears.
Scale Factor for Load Curve
Specify the scale factor that will multiply the Time Dependent Field specified under System Damping Constant Table.
X Trans. Damping Forces
Scale factor for X translation damping forces, in the global coordinate system directions.
Y Trans. Damping Forces
Scale factor for Y translation damping forces, in the global coordinate system directions.
Z Trans. Damping Forces
Scale factor for Z translation damping forces, in the global coordinate system directions.
X Rot. Damping Moments
Scale factor for X rotation damping moments, in the global coordinate system directions.
Y Rot. Damping Moments
Scale factor for Y rotation damping moments, in the global coordinate system directions.
Z Rot. Damping Moments
Scale factor for Z rotation damping moments, in the global coordinate system directions.
Rayleigh Damping Coeff.
Specify the scalar coefficient () that the global stiffness matrix is multiplied by to obtain the Rayleigh damping matrix.
Rigid Body Switch and Merge Subform This subordinate form appears when Rigid Body Switch and Merge button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
338
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is At Start (D2R0000).
Existing Merged Properties
List of deformable body and rigid body properties that have already been merged.
Merged Body Name
Specify the name of the Existing Merged Properties entry to be created.
Deformable Property
Select an entry under Deformable Property
Chapter 3: Running an Analysis 339 Solution Parameters
Form
Parameters
Master Rigid Property
Select an entry under Master Rigid Property
Add
Click Add to create an entry under Existing Merged Properties.
Modify
Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Define Set of Parts to See Define Set of Parts to be Switched Subform, 340 be Switched Define Inertial Properties of Rigid Body
See Define Inertial Properties of Rigid Body Subform, 342
340
Patran Interface to MD Nastran Preference Guide Solution Parameters
Define Set of Parts to be Switched Subform This subordinate form appears when Define Set of Parts to be Switched button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient.
Chapter 3: Running an Analysis 341 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is At Stage (D2RAUTO).
Existing Merged Properties
List of deformable body and rigid body properties that have already been merged.
Merged Body Name
Specify the name of the Existing Merged Properties entry to be created.
Deformable Property
Select an entry under Deformable Property.
Master Rigid Property
Select an entry under Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
Add
Click Add to create an entry under Existing Merged Properties.
Modify
Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Starting Switch Time Specify the time to switch the deformable and rigid properties. Ending Switch Time
Specify the time to terminate the switching of the deformable and rigid properties.
Delay Period
Specify the time delay ( for switching.
Rigid Wall/Contact Surf Number
Specify the surface numbers for rigid walls/surfaces that are to contact.
Related Switch Set Max. Permited Time Specify the maximum time step. Step Size Number of Deformable Parts to Rigid
Specify the number of deformable parts that will be switched to rigid parts.
Number of Rigid Parts to Deformable
Specify the number of rigid parts that will be switched to deformable parts.
Activation Code Switch
Select one of the five flags, 1) EQ.0, 2) EQ.1, 3) EQ.2, 4) EQ.3, or 5) EQ.4.
Pair of Related Switches
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.-1.
Nodal Rigid Body Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Nodal Constraint Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Rigid Wall Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
342
Patran Interface to MD Nastran Preference Guide Solution Parameters
Define Inertial Properties of Rigid Body Subform This subordinate form appears when Define Inertial Properties of Rigid Body button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 343 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is New Rigid Props. (D2RINNER).
Master Rigid Property
Select a Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
X Coord of Center of X coordinate of center of mass. Mass Y Coord of Center of Y coordinate of center of mass. Mass Z Coord of Center of Z coordinate of center of mass. Mass Translational Mass
Scalar mass value for translation, not rotation.
XX Comp. of Inertia Tensor (IXX)
XX (1,1) component of inertia tensor matrix.
XY Comp. of Inertia Tensor (IXY)
XY (1,2) component of inertia tensor matrix.
XZComp. of Inertia Tensor (IXZ)
XZ (1,3) component of inertia tensor matrix.
YY Comp. of Inertia Tensor (IYY)
YY (2,2) component of inertia tensor matrix.
YZ Comp. of Inertia Tensor (IYZ)
YZ (2,3) component of inertia tensor matrix.
ZZ Comp. of Inertia Tensor (IZZ)
ZZ (3,3) component of inertia tensor matrix.
Eulerian Parameters Subform This subordinate form appears when Eulerian Parameters button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
344
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Euler Boundary Treatment
There are three choices, 1) Default, 2) Extrapolate (extrapolate structural mesh pressure to Euler elements at solid/fluid boundary), or 3) Element (solid/fluid boundary Euler element pressure equals the structural element pressure at the solid/fluid boundary).
Multi-Mat. Trans. Scheme
There are three choices, 1) Default (Impulse), 2) Average (face (surface) velocity is averaged simply), or 3) Impulse (face (surface) velocity is impulse weighted).
Material Failure Option
There are three choices, 1) Default (No Fail), 2) Fail (activates transport of fail fraction and thereby keeps track of material that has failed), or 3) No Fail (failed Euler material can support shear stress again as soon as new material enters the Euler element).
Chapter 3: Running an Analysis 345 Solution Parameters
Form
Parameters
Multi-Material Array Size
The multi-material Eulerian elements use an overflow array to store their material data. This array can hold “Multi-Material Array Size” times the number of Eulerian elements. If more the 10% of the Eulerian elements have more than one material, the value of “Multi-Material Array Size” must be increased.
Initial Condition Accuracy
A parameter value used to specify the accuracy of the initial conditions in Eulerian elements, when using the geometric shape definition. The parameter value is specified in the input file using PARAM, MICRO, value.
Mimimum Velocity
A parameter value used to specify the minimum velocity. If a calculated velocity is less than this, it is set to zero (0). It is mainly used to eliminate harmless small values. The parameter value is specified in the input file using PARAM, VELCUT, value.
Maximum Velocity
Specify the maximum velocity for Eulerian and Lagrangian meshes. Although it is not usually necessary to limit the velocity in Eulerian meshes, there are occasions in regions of near-vacuous flow where using this can be an advantage. The same thing applies to Lagrangian meshes, where there is contact. The parameter value is specified in the input file using PARAM, VELMAX, value, YES/NO. Default is 1.0e10, YES. See the next row for information on what YES/NO means.
Small Mass Removal Because very high velocities occur mostly in Eulerian elements with very small mass, the mass in these elements may need to be removed for the analysis to be stable. The above parameter (PARAM, VELMAX) is used to specify whether or not to eliminate small masses. YES = eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. NO = do not eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. Default = YES. Universal Gas Constant
Specify the value of the universal gas constant. The parameter value is specified in the input file using PARAM, UGASC, value.
Single Material Elements
Specify the minimum density of single material Eulerian elements. For arbitrary LagrangeEuler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Single Mats. with Strength
Specify the minimum density of single material Eulerian elements with strength. For arbitrary Lagrange-Euler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Multi-Material Elements
Specify the minimum density of multi-material Eulerian elements.
Roe Solver Scheme
Specify whether or not to use the Roe solver. The Roe solver accounts for momentum exchange between Lagrange (structure) and Eulerian material.
Spatial Accuracy
There are two schemes that can be used. They are, 1) 1st Order (left and right state variables are taken as the values the state variables have at the left- and the right-element center), or 2) 2nd Order (left- and right-state variable values at a face by including the left-left and the right-right element).
Time Integration Scheme
There are two schemes that can be used. They are, 1) 1st Order, or 2) 2nd Order (three-stage time integration scheme).
346
Patran Interface to MD Nastran Preference Guide Solution Parameters
SPH Control Parameters Subform This subordinate form appears when SPH Control Parameters (SPH refers to smooth “particle hydrodynamics”) button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 347 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Number of Cycles
Specify the number of cycles between particle sorting.
Death Time
Specify the time when SPH calculations are to be stopped.
Initial Number of Neighbors
Specify the initial number of neighbors per particle. This parameter is for specifying how much memory is to be allocated for arrays during initialization. If the value is positive, the memory will be dynamically allocated. If the value is negative, the memory allocation will be static (constant). During the calculation only the closest SPH elements will be considered as neighbors. Using this option can avoid memory allocation problems.
Particle Approx. Theory
There are six theories to choose from, 1) Renormalization (approximation), 2) Symmetric (formulation), 3) Sym. Renormalization (symmetric renormalization approximation), 4) Tensor (tensor formulation), 5) Fluid Particle (fluid particle approximation), 6) Fluid Particle Renorm (fluid particle with renormalization approximation).
Start Time
Specify the time to begin particle approximation.
Maximum Velocity
Maximum velocity for the SPH particles. Particles whos velocity > this value are deactivated.
Computation of Approx.
Select one of the following for two different SPH parts, 1) Particle Approximation (approximation is calculated), or 2) No Particle Approximation (approximation is not calculated; two different SPH materials cannot interact with each other, and penetration is allowed).
Intergration Type
Select 1) 0 ( d h t = 1--- h t div v ), or 2) 1 dt
d
( d h t = 1--- h t div v 1 3 ), for time integrating to obtain the dt
d
smoothing length. Smoothing Length Comput.
Select 1) Bucket (sort based on algorithm; very fast), or 2) Global (computation for all the model particles ). This is done during initialization.
Box Type
Select either 1) Fixed (the box remains fixed in space), or 2) Moving (the user specifies two corners of the box and a the time dependent Field to describe the motion of the two corners). As long as a given SPH particle is in a box, the SPH calculation for the particle is performed for the box. If the particle leaves the box it was inside, it is deactivated.
Select Box
Select the name of a box under Select Box. A box must have been previously created under Loads/BCs: Create / Box Definition / Nodal.
Tail Vector
Specify a vector, <X1 Y1 Z1>, that defines the minimum coordinates of the box (coordinates of the corner of the box at the minimum location).
348
Patran Interface to MD Nastran Preference Guide Solution Parameters
Form
Parameters
Head Vector
Specify a vector, <X2 Y2 Z2>, that defines the maximum coordinates of the box (coordinates of the corner of the box at the maximum location).
Motion Vs Time Data
Specify the time dependent Field that defines the motion of the two corners of the box.
Vel./Disp. Flag
Specify whether the time dependent Field is a Velocity or Displacement field.
Coord. System
Specify the coordinate system that the Tail and Head Vectors are defined in.
Results Output Format With the results output format form you can choose which output formats you want to use with each solution sequence. The appropriate defaults are set for each solution type. These defaults can be changed or set in the settings.pcl file.
Data Output
Defines the type of data output.
• OP2
Specifies output of data to a MD Nastran OUTPUT2 file (*.op2). This will place a PARAM, POST, -1 in the input file.
• XDB
Specifies output of data to a MSC.Access database (*.xdb). This will place a PARAM, POST, 0 in the input file.
• Print
Specifies output of data to a MD Nastran print file (*.f06).
• Punch
Specifies output of data to a MD Nastran punch file (*.pch).
• MASTER Only
When ON, only a .master file is written.
• MASTER/DBALL
When ON, both a .master file and a .dball file are written.
• XDB Buffer Size
For the XDB results file, defines the buffer size used for accessing results.
Chapter 3: Running an Analysis 349 Solution Parameters
OUTPUT2 Requests
Specifies type of OUTPUT2 commands. • P3 Built In - signals the use of MD Nastran internal OUTPUT2 commands geared
toward Patran. These commands are also appropriate for PATRAN 2. The “P3 Built In” option is appropriate only for Database Runs, see Solution Parameters, 277. If Database Run has been deselected, this option will be set internally to “Alter File”. • Alter File - specifies the use of an external alter file found on the Patran file path and following the “msc_v#_sol#.alt” naming convention. See Files, 572 for more
details. • CADA-X Alter - specifies the use of an LMS CADA-X specific alter file that is
identical to the “Alter File” but with an additional “.lms” extension, for example, “msc_v67_sol103.alt.lms”. • P2 Built In - specifies use of MD Nastran internal OUTPUT2 commands geared
toward PATRAN 2. OUTPUT2 Format
Specifies format of the MD Nastran OUTPUT2 (*.op2) files. Use “Text” format when the resulting OUTPUT2 file must be transported between heterogeneous computer platforms.
A new variable has been added to the settings.pcl file for results output format defaults per SOL sequence: NASTRAN_nnn_DATA_OUTPUT OP2+PUNCH Where nnn is the solution sequence 101, 400 etc... and OP2+XDB+PRINT+PUNCH+MASTER +DBALL are the options. This variable is only read from the settings.pcl file when opening a new database, creating a new job or changing the solution sequence of an existing job. Otherwise the results output settings are retrieved from the database for an existing job. Note that these variables must be added to the settings.pcl file by the user and if they do not exist, a standard default is used. Also note that OP2 and XDB are mutually exclusive and both cannot be specified at the same time. The same is true for MASTER Only and MASTER/DBALL. The settings.pcl file may have one of these variables for each SOL sequence defined in Patran (>100).
350
Patran Interface to MD Nastran Preference Guide Solution Parameters
ADAMS Preparation This form is used when you want to prepare a database for an Adams job.
Chapter 3: Running an Analysis 351 Solution Parameters
ADAMS Output
• MNF Only • Full Run + MNF
Units
• Mass - Your options are: Kilogram, Pound-Mass, Slug, Gram, Ounce-
Mass, Kilo-Pound-Mass, Megagram • Force - Newton, Pounds-Force, Ounce-Force, Dyne, Kilo-Newton, Kilo-
Pound-Force • Length - Millimeter, Centimeter, Meter, Kilometer, Inch, Foot, Mile • Time - Millisecond, Second, Minute, Hour
Craig-Bampton Modes Bounds
• Lower Bound • Upper Bound
Num. Shapes to Adams ADAMS Debug Print Strip Face Create .out(OP2 file) for MSC Fatigue Mass Options
• Partial • Constant File • Full • None
Output Requests Transfer Groups to ADAMS
352
Patran Interface to MD Nastran Preference Guide Select Superelements
3.6
Select Superelements The superelements created in the FEM menu are displayed in the form below. The superelements for a subcase are selected by highlighting the name in the listbox. Default button unselects all the superelements. If Write PART Superelements toggle is ON in the Translation Parameters, 265 form, then BEGIN BULK SUPER=id sections are written to the input file to define the superelements, otherwise if this is OFF, SESET entries are used. In addition to selecting the superelement, you can specify the superelement tree definition. This tell the analysis which superelement are upstream of others and thus, not directly connected to the residual structure or superelement zero (SE0). To define an upstream SE relative to its downstream SE, use the form shown below to fill out the spreadsheet. Put focus in the Downstream databox, select a superelement from the list, then select the upstream from the list and press Add. This adds a row to the spreadsheet. Repeat this for every upstream element you need to define. Clicking on a row in the spreadsheet and clicking Remove will remove the defintion. Downstream SEs can only appear in the speadsheet once. This writes the SETREE entry.
Chapter 3: Running an Analysis 353 Select Superelements
SE6
SE5 SE4
SE3
SE1
SE0
SE2 In this example, SE1, SE2, & SE3 are upstream of the residual. This is not necessary to define in the SE tree. However SE4 is upstream of SE3 and SE5 & SE6 are upstream of SE4. These should be defined in the tree.
354
Patran Interface to MD Nastran Preference Guide Subcases
3.7
Subcases This form appears when the Subcases... button is selected on the Analysis form. The subcase is the MD Nastran mechanism for associating loads and boundary conditions, output requests, and various other parameters to be used during part of a complete run. The Patran MD Nastran interface automatically associates default parameters and output requests with each Patran load case to create a subcase with the same name as the load case. You can access the Subcase Parameters... and Output Requests... forms to view or modify these defaults.
Options are Create, Delete, and Global Data.
Displays all the available subcases associated with the current Solution Sequence.
The subcase name that is being created or modified is displayed in this databox. It can be typed in or picked from the Available Subcases listbox.
Displays all the available loadcases in the current database. Only one loadcase can be selected per subcase. For Normal Modes and Complex Eigenvalue solution types, free-free runs can be generated by using an empty load case.
Chapter 3: Running an Analysis 355 Subcases
Deleting Subcases To delete subcases, select Subcases from the Analysis form, and set the Action to Delete.
Select the subcase(s) to delete.
Apply to delete the selected subcases.
356
Patran Interface to MD Nastran Preference Guide Subcases
Editing Subcases To edit global data for subcases, select Subcases from the Analysis form, and set the Action to Global Data. The following form appears.
Select Subcase(s) to edit associated data.
Use Output Requests... to edit the output requests associated with the selected subcases. The Edit Output Request form appears. See Edit Output Requests Form, 426.
Apply changes the output requests for all selected subcases. Cancel closes the form without changes.
Chapter 3: Running an Analysis 357 Subcase Parameters
3.8
Subcase Parameters The subcase parameters represent the settings in MD Nastran Case Control that take effect within a subcase and do not affect the analysis in other subcases. Currently, the following solution sequences have subcase parameters associated with them. Solution Sequences
Linear Static Subcase Parameters, 358
SOL 101
Nonlinear Static Subcase Parameters, 359
Other Conditions Model has p-elements and utilizes Version 68
Selects the subcase to participate in the error analysis calculations in an adaptive analysis. By default the subcase participates in the error analysis.
None
Selects nonlinear static iteration parameters.
None
Selects nonlinear transient iteration parameters.
Version 68
Selects real eigenvalue extraction parameters.
SOL 106, 66 Nonlinear Transient Subcase Parameters, 362
Description
SOL 129, 99 Normal Modes Subcase Parameters, 364
SOL 103 Implicit Nonlinear Subcase Parameters, 375 DDAM Subcase Parameters, 407 Explicit Nonlinear Subcase Parameters, 409
358
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Linear Static Subcase Parameters This form is available for solution sequence 101 for MSC.Nastran Version 68 and for models that contain p-elements. The form allows the inclusion of subcases in the error analysis. This toggle sets the ADACT Case Control command.
Used to turn rotor dynamics on for the linear static subcase. If enabled, the “Specify Rotor Speed” button will be enabled, and can be selected to display the Rotor Speed Form, below. See Contact Table, 396 for more information.
The reference rotor for the subcase. This drives the RGYRO case control and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speed to the reference rotor. These values define the SPDUNIT and SPEED fields of the MD Nastran RGYRO Bulk Data entry. The SPDHIGH and SPDLOW entries are left blank.
Chapter 3: Running an Analysis 359 Subcase Parameters
Nonlinear Static Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Nonlinear Static. This form allows the definition of the parameters that control the interation criteria for a Nonlinear Static analysis. All of the data is part of the NLPARM Bulk Data entry. If Arc-Length Method is selected, additional data for the NLPCI Bulk Data entry is generated. Defines the number of increments to be used to apply the full load. This is the NINC field.
Defines what method to use to control the stiffness. Matrix updates as the load is incrementally applied. This parameter can have one of three settings: Automatic, SemiAutomatic, or Controlled Iter. This defines the setting of the KMETHOD field. Defines the number of iterations to be used after each matrix update. This is the KSTEP field. Defines the limit for the number of iterations that can be done in any given increment. This is the MAXITER field.
Opens a subordinate form to activate the Arc-Length Method which is turned OFF by default. The Arc-Length Method is used to explore post-buckling paths.
Activates a buckling analysis at the end of the subcase.
Opens subordinate form to define eigenvalue extraction parameters. See Solvers/Options, 404 for more information.
Activates a normal mode analysis of the prestressed system at the end of the subcase.
360
Patran Interface to MD Nastran Preference Guide Subcase Parameters
This is a list of data input available for defining the Static Nonlinear Iterations that was not shown on the previous page. Parameter Name Displacement Error Displacement Tolerance
Load Error Load Tolerance
Work Error Work Tolerance
Default Load Temperatures
Description Indicates whether a displacement convergence criteria should be used. If Displacement Error is selected, the Displacement Tolerance field becomes active. This value defines the tolerance on displacements. The displacement tolerance must be met between iterations to define convergence. If Displacement Error is selected, a U is entered in the CONV field. The Displacement Tolerance is the EPSU field. Indicates whether a load convergence criteria should be used. If Load Error is selected, the Load Tolerance field becomes active. This value defines the tolerance on load equilibrium. The load equilibrium tolerance must be met between iterations to define convergence. If Load Error is selected, a P is entered in the CONV field. Load Tolerance is the EPSP field. Indicates whether a work convergence criteria should be used. If Work Error is selected, the Work Tolerance field becomes active. This value defines the tolerance on work error. The work tolerance must be met between iterations to define convergence. If Work Error is selected, a W is entered in the CONV field. Work Tolerance is the EPSW field. Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
Chapter 3: Running an Analysis 361 Subcase Parameters
Arc-Length Method Parameters This subordinate form appears when the Arc-Length Method button is selected on the Subcase Parameters form. This form allows the definition of parameters that control the Arc-Length Method. All of the data is part of the NLPCI Bulk Data entry. Defines the type of Arc-Length Method: CRIS = Crisfield method (default) RIKS = Riks method MRIKS = modified Riks method
Minimum allowable arc-length adjustment ratio between increments for the adaptive arc-length method 0.0MINALR1.0.
Maximum allowable arc-length adjustment ratio between increments for the adaptive arc-length method MAXALR1.0. Scale factor w for arc-length criteria: w=0, displacement control w>0, combined load and displacements control w»1, load control Desired number of iterations for convergence to be used for the adaptive arc-length adjustments. This is the DESITER field Maximum number of controlled increment steps allowed within the subcase. This is the MXINC field.
362
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Nonlinear Transient Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Nonlinear Transient. All of the data is part of the TSTEPNL Bulk Data entry.
Defines the Ending Time and Number of Time Steps for the subcase. Defines what method to use to control the stiffness. The Mass matrix updates as the load is incrementally applied. This parameter can have one of three settings: Adaptive, Automatic, or Time Step. This is the METHOD field.
Defines the number of time steps to be used in each matrix update. This can only be set if Matrix Update Method is set to Time Step. This is the NDT field. Defines the maximum number of time step bisections to be used in each matrix update. This can only be set if Matrix Update Method is set to Adaptive. This is the MAXBIS field. Defines the limit for the number of iterations that can be done in any given increment. This is the MAXITER field.
Chapter 3: Running an Analysis 363 Subcase Parameters
This is a list of data input available for defining the Transient Nonlinear Iterations that was not shown on the previous page. Parameter Name Displacement Error Displacement Tolerance
Load Error Load Tolerance
Work Error Work Tolerance
Default Load Temperatures
Description Indicates whether a displacement convergence criteria should be used. If Displacement Error is selected, the Displacement Tolerance field becomes active. This value defines the tolerance on displacements that must be met between interactions to define convergence. If Displacement Error is selected, a U is entered in the CONV field. The Displacement Tolerance is the EPSU field. Indicates whether a load convergence criteria should be used. If Load Error is selected, the Load Tolerance field becomes active. This value defines the tolerance on load equilibrium that must be met between iterations to define convergence. If Load Error is selected, a P is entered in the CONV field. Load Tolerance is the EPSP field. Indicates whether a work convergence criteria should be used. If Work Error is selected, the Work Tolerance field becomes active. This value defines the tolerance on work error that must be met between iterations to define convergence. If Work Error is selected, a W is entered in the CONV field. Work Tolerance is the EPSW field. Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
364
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Normal Modes Subcase Parameters The Normal Modes subcase parameters form is available only for Solution 106 for MSC.Nastran Version 70.7. Use this form to create either EIGR or EIGRL Bulk Data entries. Defines the method to use to extract the real eigenvalues. This parameter can be set to any one of the following: Lanczos, Automatic Givens, Automatic Householder, Modified Givens, Modified Householder, Givens, Householder, Enhanced Inverse Power, or Inverse Power. If this is set to Lanczos, this indicates that an EIGRL Bulk Data entry should be created. Otherwise, this defines the setting of the METHOD field on the EIGR Bulk Data entry.
Defines the lower and upper limits to the range of frequencies to be examined. These are the F1 and F2 fields on the EIGR Bulk Data entry or the V1 and V2 fields on the EIGRL Bulk Data entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Enhanced Inverse Power or Inverse Power. This is the NE field on the EIGR Bulk Data entry.
See Contact Table, 396 for more information.
Chapter 3: Running an Analysis 365 Subcase Parameters
This is a list of data input available for defining the Real Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed. This is the ND field on the EIGR or EIGRL Bulk Data entries.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value between 0 and 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of three settings: Mass, Maximum, or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. Defines the setting of the NORM field on the EIGR Bulk Data entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGR Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGR Bulk Data entry.
Number of Modes in Error Analysis
Indicates how many modes will participate in the error analysis when the model contains p-elements. This data sets the ADACT Case Control command.
Default Load Temperatures
Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
366
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Complex Eigenvalue Subcase Parameters This subordinate form appears when you select Subcase Parameters button on the Subcases form and the solution type is Complex Eigenvalue.
Used to turn rotor dynamics on for the complex eigenvalue subcase. If enabled, the “Specify Spin Properties” button will be enabled, and can be selected to display the Spinning Properties Form, below. Rotor dynamics is disabled by default.
See Contact Table, 396 for more information.
Synchronous (default) or Asynchronous Defines the SYNCFLG field of the MD Nastran RGYRO Bulk Data entry.
The reference rotor for the subcase. This drives the RGYRO Case Control and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speeds to the reference rotor. These values define the SPDUNIT, SPDHIGH, and SPDLOW fields of the MD Nastran RGYRO Bulk Data entry. The SPEED value is left lank. For Asynchronous analyses, a single Speed databox is presented, defining SPEED field, while SPDHIGH and SPDLOW are left blank.
Chapter 3: Running an Analysis 367 Subcase Parameters
Transient Response Subcase Parameters This subordinate form appears when you select Subcase Parameters button on the Subcases form and the solution type is Transient Response. Use this form to specify the time step interval and duration for a transient response analysis. All of the data is part of the TSTEP Bulk Data entry. Direct Transient and Modal Transient Solutions
This is the subcase parameters form for the Direct Transient and Modal Transient solution.
Use this button to define your TSTEP entry.
Modal Damping is only shown if you select Modal Damping formulation from the Solution Type form.
Use this button to define your TABDMP1 entry. You must enter at least one value of frequency and damping on the spreadsheet for damping to occur. See Contact Table, 396 for more information.
368
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Define Time Step
Use this form to define the time steps in a linear table. Values of Delta-T (Time Increment) must be positive. See MD Nastran Quick Reference Guide TSTEP for more information.
The "Skip Factor" column is optional. If the column is empty, MD Nastran assumes the Skip Factor is 1.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, select click on the row label and select "Add Row".
No. of Time Steps and Delta-T determine the solution points in time. The skip factor defines which of the solution points you wish to perform results processing on. A skip factor of 1 indicates every time step, 2 indicates every other solution step, etc. Total solution time accumulates in order of entry. For the example shown, MD Nastran will calculate output at 100 time steps ranging between 1. and 100. Define Damping
Use this form to define Damping in a linear table. Values of frequency must be positive. Discontinuities (same value of frequency, different value of damping) are allowed at all locations except the first and last entries in the table. See MD Nastran Quick Reference Guide TABDMP1 for more information. Modal Damping does not allow a discontinuity to exist as either the first or last entries in the modal damping data. This will cause an error in MD Nastran. It is strongly recommended that you do not create such scenario. If the first and second frequencies (two lowest frequencies) are the same value, a warning will be issued, even if the damping value for those frequencies are the same. If the last and second to last frequencies
Chapter 3: Running an Analysis 369 Subcase Parameters
(two highest frequencies) are the same value, a warning will be issued, even if the damping value for those frequencies are the same.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
370
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Frequency Response Subcase Parameters This subordinate form appears when you select the Subcase Parameters button on the Subcases form and the solution type is Frequency Response. Use this form to specify the frequencies for a frequency response analysis. All of the data is part of a FREQi Bulk Data entry. Frequency Solution
This is the Frequency Subcase Parameter Form.
Use this button to define FREQ,FREQ1,FREQ2, FREQ3, FREQ4 entries.
Modal Damping is only shown if you select Modal Damping formulation from the Solution Type form.
Use this button to define a TABDMP1 entry. At least one value of frequency and damping must be entered on the spreadsheet for damping to occur. Used to turn rotor dynamics on for the complex eigenvalue subcase. If enabled, the “Specify Spin Properties” button will be enabled, and can be selected to display the Spinning Properties Form, below. Rotor dynamics is disabled by default.
See Contact Table, 411 for more information. See Solvers/Options, 404 for more information.
Chapter 3: Running an Analysis 371 Subcase Parameters
Use this form to create FREQi entries.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
The driving column on this form is the Increment type. Direct Frequency
When the Increment type is...
Patran...
Discrete
Creates a FREQ entry where Start Freq is the frequency value. Multiple Discrete rows will be written to the same FREQ entry. End Freq. and No. Incr. columns are not used.
Linear
Creates a FREQ1 entry. The Start Freq. will be the first frequency and the End Freq. and No. Increments will have a linear progression in between.
Logarithmic
Creates a FREQ2. Same as Linear, except it will have a logarithmic progression.
Modal Frequency
When the Increment Type is... Discrete
Patran... Creates a FREQ entry where Start Freq is the frequency value. Multiple Discrete rows will be written to the same FREQ entry. End Freq, No. Incr. and Cluster/Spread columns are not used.
372
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Linear
Creates a FREQ1 entry. The Start Freq. will be the first frequency and the End Freq. and No. Increments will have a linear progression in between. The Cluster/Spread column is not used.
Logarithmic
Creates a FREQ2. Same as Linear, except it will have a logarithmic progression.
Lin. Cluster
Creates a FREQ3 with type set to LINEAR. This results in a linear distribution of solution frequencies between each successive pair of natural modes in the specified frequency interval. The Cluster value, which has a default of 1.0 is used to bias the linear distribution of solution frequencies. A smaller cluster value has a closer spacing towards the center, CLUSTER greater than 1.0 has a closer spacing at the ends of the frequency range.
Log. Cluster
Same as Lin. Cluster except that a logarithmic interpolation is used between the start and end frequencies.
Lin. Spread
Creates a FREQ4 entry. The default value of spread is 0.1. The spread is a fractional amount specified for each mode. With a spread of 0.3 and No. Incr. of 21, there will be 21 evenly spaced frequencies between 0.7*FN and 1.3*FN, where FN a natural frequency, for all natural frequencies between the specified “Start Freq” and “End Freq” values.
Fractional Spread
Creates a FREQ5 entry. Enter the Start Frequency and End Frequency. These are the lower and upper bound for the excitation (solution) frequency domain, respectively. It is desired to obtain a set of excitation frequencies around and at each natural frequency, obtained previously from the corresponding modal analysis for this simulation. This is done by providing a list of fractions; for example {fr_1, fr_2, ..., fr_n}. The list is “multiplied” by each natural frequency to provide a list of excitation frequencies for each natural frequency; for example fn_j * {fr_1, fr_2, ..., fr_n}, where fn_j is the jth natural frequency. The fractions cannot be inserted on a single row of the Define Frequencies form, but multiple rows must be created, with just one fraction per row.
Define Damping
Use this form to define the damping in a linear table. Values of frequency must be positive. Discontinuities (same value of frequency, different value of damping) are allowed at all locations except the first and last entries in the table. See MD Nastran Quick Reference Guide TABDMP1 for more information. Modal Damping does not allow a discontinuity to exist as either the first or last entry in the modal damping data. This will cause an error in MD Nastran. It is strongly recommended that you do not create such scenario. If the first and second frequencies (two lowest frequencies) are the same value, a warning will be issued, even if the damping values for those frequencies are the same. If the last and second to last frequencies
Chapter 3: Running an Analysis 373 Subcase Parameters
(two highest frequencies) are the same value, a warning will be issued, even if the damping values for those frequencies are the same.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
To create a Field for the damping data, click in the Create a Field checkbox.
To bring in damping data from an existing Field, click on the Load Data From Field button, then select the Field.
Spinning Properties, Frequency Response
Presented when Rotor Dynamics is ON and the Specify Spinning Properties button is selected.
374
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Synchronous (default) or Asynchronous Defines the SYNCFLG field of the MD Nastran RGYRO Bulk Data entry.
The reference rotor for the subcase. This drives the RGYRO Case Dontrol and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speeds to the reference rotor. These values define the SPDUNIT, SPDHIGH, and SPDLOW fields of the MD Nastran RGYRO Bulk Data entry. The SPEED value is left lank. For Asynchronous analyses, a single Speed databox is presented, defining SPEED field, while SPDHIGH and SPDLOW are left blank. For Synchronous analyses with Frequency Dependent Looping OFF, no speed databoxes are presented, and SPDHIGH, SPDLOW, SPEED are all left blank. Rather, a “param, gyroavg,-1” entry is generated. Frequency Dependent Looping is ON by default.
Chapter 3: Running an Analysis 375 Subcase Parameters
Implicit Nonlinear Subcase Parameters The type of nonlinear analysis can be changed in each SOL 600 or SOL 400 subcase. To specify this change, the Subcases form includes an Analysis Type pull-down menu with options for static, normal modes, buckling, transient dynamic, creep, and body approach analyses. For SOL 400 there is an additional Analysis Type, complex eigenvalue. In turn, specifying the subcase parameters is dependent on the Analysis Type selected for the subcase. The following sections define the subcase parameters for each analysis type.
376
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Static Subcase Parameters for Implicit Nonlinear Solution Type This subform defines the parameters for a SOL 400 or 600 static analysis subcase.
Linearity
Prescribes the nonlinear effects for the subcase.
Nonlinear Solution Parameters • Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Chapter 3: Running an Analysis 377 Subcase Parameters
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase.
Break Squeal Parameters
For defining parameter values for modeling break squeal for the subcase. (SOL 400 only).
Implicit Nonlinear Normal Modes Subcase Parameters This subform defines the parameters for a normal modes analysis subcase (SOL 400 and 600 only). See Normal Modes Subcase Parameters, 364 for more information. Implicit Nonlinear Buckling Subcase Parameters For buckling nonlinear analysis the subcase parameters control the eigenvalue extraction techniques and the range of frequencies to be targeted for extraction. This subform defines the parameters for a buckling analysis subcase (SOL 400 and 600 only). See Normal Modes Subcase Parameters, 364 for more information.
378
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Transient Dynamic Subcase Parameters This subform defines the parameters for a transient dynamic analysis subcase for SOL 600 and SOL 400.
Linearity
Prescribes the nonlinear effects for the subcase.
Nonlinear Solution Parameters • Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Chapter 3: Running an Analysis 379 Subcase Parameters
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase (SOL 600 only).
380
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Creep Subcase Parameters This subform defines the parameters for a SOL 600 and SOL 400 Creep analysis subcase.
Creep Solution Parameters • Procedure
Defines either Explicit creep formulation or Implicit creep formulation.
• Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Increment Type
Defines a fixed or adaptive increment method.
Chapter 3: Running an Analysis 381 Subcase Parameters
• Adaptive Increment Parameters...
For adaptive methods, sets boundaries for incrementation.
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase (SOL 600 only).
Break Squeal Parameters Implicit Nonlinear Body Approach Subcase Parameters This subform defines the parameters for a SOL 600 body approach analysis subcase
Body Approach Parameters • Total Time
Places a time step option in the Load Step.
• Synchronized
If ON, specifies that when the first rigid body comes into contact, the rest stop moving.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis. See Contact Table, 396
382
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Complex Eigenvalue Subcase Parameters This subform defines the parameters for a SOL 400 (only) complex eigenvalue analysis subcase
Formulation
Select either Direct or Modal.
Enable Rotor Dynamics
Click in checkbox to activate rotor dynamics.
Specify Spinning Properties...
Click to access the form for specifying the rotor speed. See Spinning Properties, Frequency Response, 373
Contact Table...
Activates, deactivates, and controls the behavior of contact bodies in the analysis. See Contact Table, 396
Chapter 3: Running an Analysis 383 Subcase Parameters
Load Increment Parameters Load and time step incrementation parameters for Statics and Transient Dynamics appear on this subordinate form. For other analysis types, this information appears directly on the Solution Parameters form.
The Load Increment Parameters form differs depending on your designation of a Fixed or Adaptive Increment Type and whether an arclength method is to be used if you select an Adaptive Incrementation scheme.
384
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Load Incrementation without Arclength
Static
Transient Dynamic
Increment Type
Adaptive
Arclength Method
None
Trial Time Step Size
Defines the initial time step size. Default is 1% of Total Time if left blank.
Time Step Scale Factor
Indicates load will be allowed to be scaled up by 20% each increment if possible. Default is 1.2.
Minimum Time Step
Indicates the smallest time step that can be used. Default is Trial Time Step / 1000 if left blank.
Maximum Time Step
Indicates the largest time step that can be used. Default is Total Time / 2 if left blank.
Maximum # of Steps
Defines the maximum number of time steps. It can be left blank which will default to the Initial Step Size divided by the Total Time.
Chapter 3: Running an Analysis 385 Subcase Parameters
Total Time
This is the total time of the analysis for a particular step. It defaults to one (1) if left blank for static load cases. For time dependent load cases, the total time is the length of time between distinct time points if left blank. Otherwise the actual value is used (not recommended because it can’t be variable).
# of Steps of Output
Indicates that this many increments evenly spaced in time will be place in the output file. Default is 0 if left blank. Which means all converged increments will be output (SOL 600 only).
Quasi-static Inertial Damping
ON by default.
Criteria
Multiple adaptive load stepping criteria is available. By default, none of this is necessary. These criteria are described below in Adaptive Load Incrementation Criteria, 387.
Time Integration Scheme
For Transient Dynamics, indicates the time integration scheme to use in dynamic analysis.
Minimum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Maximum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Matrix Update Method
This is the method for controlling stiffness updates. This is the KMETHOD field on the NLPARM entry for SOL 400 runs.
Load Increment Parameters for SOL 600 and SOL 400, Creep analysis. The MD Nastran entries used for this are NLADAPT, NLPARM, and TSTEPNL.
386
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Creep
Increment Type
There are three choices, 1) Fixed, 2) Adaptive, and 3) Adaptive Creep.
Suggested Time Increment
The approximate time step.
Total Time
The total time for the creep analysis.
Max # of Increment Allowed
This is for NSMAX.
Creep Tests
This is for RAC.
Relative Strain Tolerance
This is for TCSTRN.
Relative Stress Tolerance
This is for TCSTRS.
Low Stress Cut-off Tolerance
This is for TCOFF.
Chapter 3: Running an Analysis 387 Subcase Parameters
Adaptive Load Incrementation Criteria
This for the MD Nastran NLAUTO entry, Parameters for Automatic Load/Time Stepping. (SOL 600 only). Adaptive Criteria
Description
Treat Criteria as:
If Limits, sets 3rd field to zero (0) in 3rd data block (default). If Targets, sets field to one (1). This is for LIMITAR.
Use Automatic Criteria Continue if not Satisfied
Uses automatic physical criteria if top toggle is ON. Bottom toggle defines what happens if the criteria is not met. Both OFF by default. This is for IPHYS.
388
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Criteria
Description
Ratio Between Steps:
Defines the [Smallest] and [Largest] ratios acceptable between load increments. For Smallest, default = 0.1, For Largest, default=10.0. This is for RSMALL and RBIG.
[Number of Cutbacks]
Blank by default. default value is 10 if left blank or zero. This is for NCUT.
Increment Criteria
Selects the type of criteria to be used.The labels “XXX Range” and “XXX Increment Allowed” will change based on the Increment Criteria selected. This is for CRITERIA.
Loading Table Instances
Determines how loading tables (Use Tables must be ON in the Job Parameters form) are treated. By default loads are increased or decreased such that they always Reach Peaks-Valleys Only. If you wish you can Reach All Points in Tables or Ignore all Points in Tables.
Write Instances to Post File
Writes Loading Table Instances to the Post file if toggle is ON. Note that if toggle is ON, then only those instances are written to the POST file and not all the increments of the analysis. This is for IDMPFLG.
Nodal Temp. Check
There are three choices, 1) Omit Check, 2) Below Finish Temperature (to complete time period when all node temperatures are < FTEMP), and 3) Above Finish Temperature (to complete time period when all node temperatures are > FTEMP). This is for IFINISH.
Finish Temperature
The terminal temperature. This is for FTEMP.
Use Criterion
For a criteria to be used, this toggle must be turned ON.
“Criterion” Range
The first and last fields are zero and 1e20 respectively and cannot change. The second and third must be the same as well as the 4th/5th and 6th/7th which define the ranges. The “Criterion” title changes according to the Increment Criterion chosen.
“Criterion” Increment Allowed
The “Criterion” title changes according to the Increment Criteria chosen.
Select a Group (Optional)
You can optionally select a group of elements to which this criterion is to be applied. No group is selected by default.
Chapter 3: Running an Analysis 389 Subcase Parameters
Adaptive Load Incrementation with Arclength (SOL 600 only) Static
Adaptive Increment Parameter
Description
Arclength Method
Selects the arclength root procedure: Crisfield, Riks/Ramm, Modified Riks/Ramm, or Crisfield-Modified Riks/Ramm. The default is Modified Riks/Ram. If None is selected the form updates as shown (p. 383). For Transient Dynamics, this is the only option available for adaptive load incrementation.
Automatic Cutback
This feature is ON by default. If an increment does not converge, a restart from the last increment cuts the increment size in half.
Number of Cutbacks
This is associated with Automatic Cutback. This parameter determines how many times a cutback is allowed.
390
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Increment Parameter
Description
Initial Fraction of Load Applied to 1st Increment
This is the fraction of the total load that should be applied in the first iteration of the first increment.
Max. Fraction of Load Applied in Any Increment
This is the maximum fraction of the load that can be applied in any increment.
Max/Min Ratio Arc Length / Initial Arc Length
Used to define the minimal arclength. The default is 0.01.
Max. # of Increments
Defines the maximum number of increments. Program will end if this value is exceeded.
Total Time
This is the total time of the analysis for a particular step. It defaults to one (1) if left blank for static load cases. For time dependent load cases, the total time is the length of time between distinct time points if left blank. Otherwise the actual value is used (not recommended because it can’t be variable). Fixed Load Incrementation
Static
Transient Dynamic
Chapter 3: Running an Analysis 391 Subcase Parameters
Fixed Increment Parameter
Description
Automatic Cutback
Applies to Nonlinear Statics only. It is ON by default. If an increment does not converge, it allows for a restart from the last increment cuts the increment size in half.
Number of Cutbacks
This is associated with Automatic Cutback. This parameter determines how many times a cutback is allowed.
Number of Increments or Number of Steps
For Statics and Creep this is the number of increments specified in the NLAUTO option. Or for Transient Dynamics defines the number of steps to use throughout the analysis for Fixed time step type. Default is 10.
Total Time
For Statics, this enters the NLAUTO option which is the total time as defined in this widget. For Transient Dynamics this is the total time. For Creep, the total time is either placed in the 2nd data block of a CREEP INCREMENT option or the total time is divided by the Number of Increments, if this value is present, and the incremental time is written to the 2nd data block of the CREEP option.
Gamma / Beta
For Transient Dynamics only. Default is 0.5.
Time Integration Scheme
For Transient Dynamics, the Houbolt and Central Difference cannot be selected. Indicates the time integration scheme to use in dynamic analysis.Single Step Houbolt is the default.
Minimum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Maximum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Matrix Update Method
This is the method for controlling stiffness updates. This is the KMETHOD field on the NLPARM entry for SOL 400 runs.
Iteration Parameters This subordinate form appears when the Subcase Parameters... / Iteration Parameters... button is selected for Analysis Type: Static, Transient Dynamics, Creep, ... Subcases form. Unless otherwise specified all
392
Patran Interface to MD Nastran Preference Guide Subcase Parameters
parameter references apply to the NLSTRAT (SOL600) entry for the form on the left, and NLPARM (SOL 400) entry for the form on the right .
SOL 600 Iteration Parameter
Description
Proceed if not Converged
Forces the analysis to proceed even if the increment did not converge.
Initial Stress Stiffness
There are five choices, 1) Full, 2) None, 3) Tensile, 4) Deviatoric, and 5) Begin Increment.
Non-positive Definite
This forces the non-positive definite flag (IKNONPOS param) ON in the NLSTRAT option. A new NLSTRAT option is written for each step if a change in this flag has been detected from Subcase to Subcase.
Chapter 3: Running an Analysis 393 Subcase Parameters
SOL 600 Iteration Parameter
Description
Iteration Method
Indicates the iteration method (IKMETH param) to be used. This is can be set to Full Newton-Raphson, Modified Newton-Raphson, NewtonRaphson with Strain Correction, or Secant Method. Full Newton-Raphson is default.
Max # of Iterations per Increment
Defines the maximum number of iterations (MAXREC param) allowed for convergence in any increment. This number is negative if Proceed if not Converged is ON from the Solution Parameter form.
Minimum # of Iterations
This specifies the minimum number of iterations per Increment (MINREC param) option. It can be an integer number zero or greater. If this is set greater than zero, every increment will perform at least this many iterations.
per Increment Desired # of Iterations per Increment
Defines the number of desired iterations in an increment (ATRECYC param) which is placed on the NLSTRAT option. If the actual number of iterations is less than this value, this will be used to figure out how much to increase the load step for the next increment. In a similar manner if the actual number of iterations is greater than this number (but less than the Max # of Iterations per Increment, this will be used to decrease the load step in the next increment. Obviously if Adaptive incrementation is not specified, this data will not be used.
Matrix Update Method
There are six choices for updating the stiffness matrix, 1) Automatic (MD Nastran automatically selects the most efficient strategy based on convergence rates), 2) Controlled Iters.(MD Nastran updates the matrix at every KSTEP interations and at convergence if KSTEP <= MAXITER), 3) Adaptive, 4) Semi-Automatic (MD Nastran for each load increment (i) performs a single iteration based upon the new/next load, (ii) updates the stiffness matrix, and (iii) resumes the normal Automatic option), 5) Full Newton (MD Nastran updates the stiffness matrix every iteration), and 6) Pure Full Newton (the same as the Full Newton method, except EPSU = 0.01, EPSW = -0.01, and MAXLS = 0.0).
Tolerance Method
Defines the tolerance method to be used (CONVTYP param). This can be set to Residual, Incremental Displacement, or Incremental Strain Energy.
Residuals/Displacements
If you want the Tolerance Method to use both Residuals and Displacements to determine convergence set this to And. If you want either one or the other to determine convergence, set this to OR. If Tolerance Method is set to Residual or Displacement, then these two toggles are enabled. Both are OFF by default. If one is ON, the other is OFF. These toggles work in combination with Tolerance Method. If both are OFF, then Tolerance Method determines what is written.
And Or
Error Type
Indicates the type of error to use (IRELABS param). This can be set to Relative or Absolute or Both.
394
Patran Interface to MD Nastran Preference Guide Subcase Parameters
SOL 600 Iteration Parameter
Description
Automatic Switching
This controls automatic switching (the AUTOSW param on the NLSTRAT option) between Residuals and Displacement tolerances if one or the other fails to converge.
Residual Tolerances
Values and labels in this frame depend on the Tolerance Method and Error Type setting and are discussed below.
Relative Residual Force
The value of this widget (default is 0.1 on force) is written to the RCKI param.
Relative Displacement Relative Energy Relative Residual Moment Relative Rotation Minimum Reaction Force Minimum Displacement Minimum Reaction Moment Minimum Rotation Maximum Residual Force Maximum Displacement Maximum Residual Moment Maximum Rotation
SOL 400 Iteration Parameter
The value of these widgets (default is blank) is written to the appropriate MAXxx or MINxx param.
Description
Min # of Iterations per Increment
Specify the fewest number of iterations per load increment.
Max # of Iterations per Increment
Specify the largest number of iterations per load increment.
Number of Iterations per Update
Specify the allowable number of iterations per stiffness matrix update, (KSTEP).
Matrix Update Method
There are six choices for updating the stiffness matrix, 1) Automatic (MD Nastran automatically selects the most efficient strategy based on convergence rates), 2) Controlled Iters.(MD Nastran updates the matrix at every KSTEP interations and at convergence if KSTEP <= MAXITER), 3) Adaptive, 4) Semi-Automatic (MD Nastran for each load increment (i) performs a single iteration based upon the new/next load, (ii) updates the stiffness matrix, and (iii) resumes the normal Automatic option), 5) Full Newton (MD Nastran updates the stiffness matrix every iteration), and 6) Pure Full Newton (the same as the Full Newton method, except EPSU = 0.01, EPSW = -0.01, and MAXLS = 0.0).
Automatic Switching
If selected, automatically switch to an appropriate convergence checking flag if an unappropriated flag is selected.
Chapter 3: Running an Analysis 395 Subcase Parameters
SOL 400 Iteration Parameter
Description
Displacement Error Load Error Work Error Vector Componet Method Length Method
If any of these toggles are ON, then the appropriate CONV=U, P, W, V, or N is written to the NLPARM entry to activate the repective convergence criteria.
Displacement Tolerance Load Tolerance Work Tolerance
Specifies the tolerance value if the above corresponding toggles are activated. This is written in the EPSU, EPSP, and EPSW fields of the NLPARM entry. Leave blank for default values.
Maximum # of Divergence Conditions Specifies the MAXDIV, MAXQN, MAXLS, FSTRESS, LSTOL, MAXBLS, and RTOLB fields of the NLPARM entry. It is recommended Maximum # of Correction Vectors to use the default values. Please consult the MD Nastran Quick Reference Guide for more information. Maximum # of Line Searches Fraction of Effective Stress Line Search Tolerance Maximum # of Bisections Maximum Incremental Rotations
396
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Contact Table A contact table is used to control the behavior of and to activate or deactivate, or in some cases, remove contact bodies from the analysis. This is used for both linear and nonlinear contact.
Chapter 3: Running an Analysis 397 Subcase Parameters
. Input
Description
Global Contact Detection
• Changing this setting should be done with caution as it will over-write any contact
detection changes made to individual contact pairs in the cells. This option sets the contact detection method in all cells in the contact table. • Default (by body #) -This is the default where contact is checked in the order the
bodies are written to the input file which is the order in which they are created. In this scenario, the most finely meshed bodies should be listed first. There will be contact checks first for nodes of the first body with respect to the second body and then for nodes of the second body with respect to the first body. If Single Sided contact is activated on the Contact Parameters subform, then only the first check is done. • Automatic -Unlike the default, the contact detection is automatically determined
and is not dependent on the order they are listed but determined by the solver ordering the bodies starting with those having the smallest edge length. Then there will be only a check on contact for nodes of the first body with respect to the second body and not the other way around. • First ->Second - Blanks the lower triangular section of the table matrix such that
no input can be accepted. Only the contact bodies from the upper portion are written, which forces the contact check of the first body (the one higher in the contact table) with respect to the second body. • Second-> First - Blanks the upper triangular section of the table matrix such that
no input can be accepted. Only the contact bodies from the lower portion are written. Contact detection is done opposite of First->Second. • Double-Sided -Writes both upper and lower portions of the table matrix. This
overrules the Single Sided contact parameter set on the Contact Parameters subform. Touch All
Places a T to indicate touching status for all deformable-deformable or rigiddeformable bodies.
Glue All
Places a G to indicate glued status for all deformable-deformable or rigid-deformable bodies.
Deactivate All
Blanks the spreadsheet cells.
Import/Export
Import or Export a file with contact matrix definition data. The format must be CSV.
Select Existing
Select an existing Contact Table from a set of tables.
Contact Matrix
A matrix defining what and how contact bodies contact.
Body Type
Lists the body type for each body; either Deformable or Rigid.
Release
This cell can be toggled for each body to Y or N (Yes or No). If Y, this indicates that the particular contact body is to be removed from this Subcase. The forces associated with this body can be removed immediately in the first increment or gradually over the time of the entire Subcase with the Force Removal switch described below.
398
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Input
Description
The Contact Matrix entries
The rows correspond to Touching Body. The columns correspond to Touched Body. An entry of the matrix, for example (Row i,Column j), will have the entry of T, G, or “blank”. T = touching, G = glue, “blank” = no contact. To change a matrix cell entry, select the cell (click once) to select it, then click on the cell once to change to the next selection. For example, T -> G.
Touching Body Touched Body
These are informational or convenience list boxes to allow you to see which bodies an active cell references and to see what settings are active for Distance Tolerance and other related parameters below. You must click on the touched/touching bodies to see what values, if any, have been set for the pair combination.
Distance Tolerance
Set the Distance Tolerance for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Distance Tolerance.
Bias Factor
Bias the domain defined by the distance tolerance.
Analysis Properties
Select Structural.
Separation Threshold
Specify a threshold (force or stress) such that if the contact load (force or stress) is < this threshold value, the contacting body remains in contact with the contacted body.
Separation Force
Set the Separation Force for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Separation Force.
Friction Coefficient
Set the Friction Coefficient for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Friction Coefficient.
Interference Closure
Set the Interference Closure for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Interference Closure.
Friction Stress Limit
This is a bound on the maximum friction stress. This is the friction stress limit for the bilinear model, t limit . If the shear stress reaches the limit value, the applied friction force is reduced so that the maximum shear stress is given by min n limit . t
Slide Off Distance
Specify the distance a node must slide off a surface, at an edge, before the node travels on the surface, at the edge, that is at an angle to the surface that is being slid off of.
Chapter 3: Running an Analysis 399 Subcase Parameters
Input
Description
Heat Transfer Coefficient
Set the Heat Transfer Coefficient for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Heat Transfer Coefficient. This is only used in Coupled analysis (Heat transfer and Coupled analysis not supported in MSC.Nastran 2004.
Force Removal
Select 1) Immediate, or 2) Gradual. This is activated when a body is is set to Release. For example, 1-seal can be set to Release by clicking once on the corresponding Release cell, then clicking once again to change from N to Y. The MD Nastran entry BCMOVE is written to the .bdf file.
Contact Detection
Select 1) Automatic, 2) Double Sided, 3) 1st->2nd, or 4) 2nd->1st.
Retain Gaps/Overlaps
This is only applicable for the Glued option. Any initial gap or overlap between the node and the contacted body will not be removed (otherwise the node is projected onto the body which is the default). For deformable-deformable contact only.
Stress-free Initial Contact
This is only applicable for initial contact in increment zero, where coordinates of nodes in contact can be adapted such that they cause stress-free initial contact. This is important if, due to inaccuracies during mesh generation, there is a small gap/overlap between a node and the contacted element edge/face. For deformable-deformable contact only.
Delayed Slide Off
By default, at sharp corners, a node will slide off a contacted segment as soon as it passes the corner by a distance greater than the contact error tolerance. This extends this tangential tolerance. For deformable-deformable contact only.
Allow Separation Breaking Glue Parameters...
See Breaking Glue Parameters Subform, 400
Edge Contact...
See Edge Contact Subform, 401
400
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Breaking Glue Parameters Subform Un-gluing (breaking) a glued contact can be done by specifying the Breaking Glue Parameter values in the following form:
This form can only be used when there is glued contact (there is G in the Contact Table matrix cells). . Input
Description
Max Normal Stress
The maximum normal stress that will cause the glued contact to become un-glued.
Max Tangential Stress
The maximum tangential stress that will cause the glued contact to become un-glued.
First Exponent
The exponent of the tangential stress term (BGM) in the following equation: sigman -------------------- BGSN
Second Exponent
BGN
sigmat BGM + ------------------ 1.0 BGST
The exponent of the normal stress term (BGN) in the following equation: sigman -------------------- BGSN
BGN
sigmat BGM + ------------------ 1.0 BGST
Chapter 3: Running an Analysis 401 Subcase Parameters
Edge Contact Subform :
. Input
Description
Include Outside (Solid Element)
When detecting contact of solid elements (for example, CHEXA elements) use this to include contact of the outside of the elements.For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Include Outside of Rigid Surface
When detecting contact of rigid surfaces use this to include contact of the outside of the rigid surfaces. For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Check Layers
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
402
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Input
Description
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges
Use this to detect contact of edges. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Active/Deactive Elements Defines groups of elements to be active or deactive for the subcase.
Active/Deactive Group
Description
Group of Element to Deactivate
Lists all groups. Elements in the selected group will be deactivated.
Group of Elements to Activate
Lists all groups. Elements in the selected group will be activated.
Chapter 3: Running an Analysis 403 Subcase Parameters
Break Squeal Parameters Defines parameter values for modeling break squeal. (SOL 400 only).
Active/Deactive Group
Description
Enable Break Squeal
The form is activated when this checkbox is selected.
Load Factor
Defines the load factor for which the break squeal analysis is to be performed.
Average Stiffness
Approximate average stiffness per unit area between the break pads and disk. This parameter is used as a penalty contact stiffness for break squeal. It needs to be a large value, but not so large that numerical instabilities result. If this parameter is large eneough, increasing it by a few orders of magnitude will not appreciably affect the squeal modes.
Break Squeal Only
This is used to specify whether or not the nonlinear analysis will be continued after the break squeal event. If this is selected, the nonlinear iterations will cease immediatly after the event, otherwise the nonlinear iterations will be continued.
404
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Active/Deactive Group
Description
Axis of Rotation Vector
This is a vector of direction cosines, <X-dir cosine, Y-dir cosine, Z-dir cosine>, where this is for the axis of rotation, and the directions are in the basic coordinate system.
Point on Axis of Rotation
These are the coordinates of a point on the axis of rotation, [X,Y,Z]. The coordinates are in the basic coordinate system.
Solvers/Options In general, this form is used to select the Nastran solver and other possible options. An SMETHOD case control entry is written specifying the solver type to use and possibly an ITER bulk data entry for additional options. Only certain solutions allow the use of the SMETHOD case control as controlled by
Chapter 3: Running an Analysis 405 Subcase Parameters
the user interface. If a solution does not support a solver option, that option is not presented in the form or menus.
Solver Type
Description
Nastran Default
No SMETHOD or ITER entries are written. Nastran uses whatever solver is the default for the solution being used.
Iterative ElementBased (CASI)
An SMETHOD case control with the entry ELEMENT is used which invokes the iterative CASI (element-based) solver using all defaults. This is only available for SOL 101 and 400 and is generally used with large solid models. Certain restrictions apply and you should consult the Nastran Quick Reference Guide regarding the usage of this solver.
Iterative Matrix-Based
An SMETHOD case control with the entry MATRIX is used to invoke the matrix-based iterative solver using all defaults.
Iterative (Customized)
An SMETHOD case control referencing the ID of an ITER bulk data entry is written to the input deck. The ITER entry invokes the solver options. Those options are described in the table below.
406
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Iterative Option
Description
Preconditioner
Five preconditioners are available: Jacobi, Cholesky, Jacobi/Cholesky, and CASI. The CASI is the element-based iterative solver. See the table above. All other preconditioners are the matrix-based iterative solver. Various options are allowed for each as controlled by the user interface. See the entries below. To use a default preconditioner based on the solution type, set this to Analysis Default. Consult the Nastran Quick Reference Guide for more details as to which defaults are used for each solution type.
Maximum Number of Iterations
Leave this blank to accept the default. Otherwise specify the maximum number of iterations allowed.
Diagonal Scaling
The Jacobi and Cholesky preconditioners allow diagonal scaling.
Reduced
Turn this toggle on to invoke the reduced incomplete Cholesky preconditioner as opposed to just the incomplete Cholesky. This can be combined with or without diagonal scaling.
Block
Turn this toggle on to invoke the block incomplete Cholesky preconditioner. You must specify real or complex also.
Real / Complex
This is only used for the block incomplete Cholesky preconditioner.
p-version
For p-element analysis, you can turn this toggle on to invoke the Jacobi, Cholesky or combined Cholesky/Jacobi preconditioner. This cannot be combined with any other options.
Padding
Specify the padding value for reduced incomplete Cholesky with any of its options. Leave this blank to specify the defaults. Each option has its own default, therefore it is recommended that you leave this blank.
Extraction
Specify the extraction level for reduced or block incomplete Cholesky preconditioner. The default is zero.
Geometric Progression Turn this toggle on if you wish to use geometric progression convergence criterion. Epsilon
This is a user-given convergence parameter. Default is 1e-6. If present, the solver will use additional external convergence criterion. See the Nastran Quick Reference Guide for more details. Blank this field out if only the internal convergence criterion is required.
Print Messages for each Iteration
Off by default. Turn ON if you want more diagnostics for each iteration. Otherwise only minimal messaging is given.
Terminate Early (Resource Estimate Only)
Turn this toggle ON if you want the run to terminate with only a resource estimation.
Chapter 3: Running an Analysis 407 Subcase Parameters
DDAM Subcase Parameters This subform defines the parameters for a SOL 187 DDAM analysis subcase
408
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Spectrum Source
Select File for a user-defined spectrum, or Coef for a DDAM style coefficient equation. If you select File, a button appears to the right to let you select the file where the spectrum is defined. If you select Coef, two other buttons appear:
Coef Source
Select File for a user-written coefficient file, or Default to use the coefficients built into the Fortran program. Note that the built-in coefficients we deliver in the program are NOT the DDS-072 coefficients. If you use this option for a real DDAM analysis, the Fortran file must be edited and recompiled. If you select File, a button appears to the right to let you choose the file where the coefficient data is stored.
F(x) Type
Choices are NRL 1396 and DDS 072. This option toggles between the old NRL 1396 style equations, and the current DDS-072 style equations used for DDAM.
Coefficient Options • Ship Type
Select Surface or Submerged
• Mount Location
Choice of Deck, Hull, or Shell.
• Elastic/Plastic
Select Elastic or Plastic. Choosing Plastic uses the Elastic/Plastic coefficients; Elastic uses the elastic coefficients.
Weight Cutoff
Default uses the default value compiled into the PCL code, which is 80%. If you choose Enter Value the text box becomes available and you can enter a percentage manually. The number entered is the percentage, not the fraction, so 100% of the modal mass is entered as 100.
Minimum G Level
If you select N/A, no minimum G value is used. If you enter a value, all modal accelerations below the minimum are set to the minimum.
Fore/Aft Axis
It is necessary to have the model oriented orthogonal to a global cartesian axis system, although not necessarily in one particular orientation. This toggle identifies which global axis is to be interpreted as Fore/Aft.
Vertical Axis
This identifies the axis that is in the vertical direction.
Modal Analysis • Number of Desired Roots • Lower • Upper
These are the limits that control the eigenvalue analysis and are the values from the Nastran EIGRL entry. ND is the number of desired roots, V1 is the lower frequency limit, V2 is the upper frequency limit. For the effects of using one of more of these, see the EIGRL section of the MD Nastran Quick Reference Guide.
Chapter 3: Running an Analysis 409 Subcase Parameters
Explicit Nonlinear Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Explicit Nonlinear. All of the data is part of the TSTEPNL Bulk Data entry
Defines TSTEPNL. Similar to SOL 129, Nonlinear Transient
Defines BCTABLE. Similar to SOL 600 Implicit Nonlinear
Contact Table...
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
410
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Selects the highest and lowest natural frequenc values to be extracted
Selects which Degrees of Freedom are used to determine the peaks Selects the output interval of accelerations, velocities, or displacements of the eigenvalues
The “Type of Response” menu specifies whether Acceleration, Velocity, or Displacement response will be used to select the modes.
Selects which Degrees of Freedom to be in the eigenvectors (3 for translations only, 6 for translations and rotations
The “Method of Normalization” menu specifies the method used to normalize the eigenvectors
Chapter 3: Running an Analysis 411 Subcase Parameters
Contact Table A contact table is used to control the behavior of contact bodies and to activate or deactivate, or in some cases, remove contact bodies from the analysis. This form defines the BCTABLE entry.
Additional Data...
Additional Contact Data for Explicit Nonlinear.
412
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Additional Contact Data This subordinate form defines additional contact data for Explicit Nonlinear.
Chapter 3: Running an Analysis 413 Subcase Parameters
Adaptive Mesh Post-Processing Support has been added for adaptive mesh post-processing for airbag analysis. Below is an adapted mesh model as read in from the DBALL file and stored using offset ID’s in separate groups. The user can then select one or more time increments from the Quick Plot Results menu for postprocessing. The Quick Plot algorithm pulls up the mesh associated with the increment(s) selected for post-processing. Using this method a user can do a pseudo-animation to show the progression of the analysis. The model is loaded by a cylindrical rigid pin with a 200 lb load at the center.
Additional Information The following is also now supported for SOL 700 jobs: • Additional Properties • PBEAM71 • BPEAMD • PBELTD • PELAS1 • PLPLANE • PLSOLID • PSHELL1 • PSHELLD • PSPRMA
414
Patran Interface to MD Nastran Preference Guide Subcase Parameters
• GUI for time domain NVH • Many additional materials
Chapter 3: Running an Analysis 415 Output Requests
3.9
Output Requests This allows the definition of what data is desired from the analysis code in the form of results. For most solution sequences, the form consists of two formats: Basic and Advanced. The Basic form retains the simplicity of being able to specify the output requests over the entire model and uses the default settings of MD Nastran Case Control commands. There is a special set defined in Patran called ALL FEM. This set represents all nodes and elements associated with Object defined on the Analysis Form, 261. This default set is used for all output requests in the Basic Output Requests, 416 form. The Advanced version of this form allows the user to vary these default options. Since output requests have to be appropriate to the type of analysis, the form changes depending on the solution sequence. The Advanced Output Requests, 417 also adds the capability of being able to associate a given output request to a subset of the model using Patran groups. This capability can be used effectively in significantly reducing the results that are created for a model, optimizing the sizes and translation times of output files. The creation of Patran groups are documented in Group>Create (p. 263) in the Patran Reference Manual. The results types that will be brought into Patran due to any of these requests, are documented in Supported OUTPUT2 Result and Model Quantities, 502. In that chapter, tables are presented that correlate the MD Nastran results block, and the Patran primary and secondary results labels with the various output requests. Note:
Many of the output requests that can be defined on the Output Request forms currently apply only to the printed values in the MD Nastran output file; these result quantities cannot be imported and postprocessed in Patran. For guidance on specific quantities, review Supported OUTPUT2 Result and Model Quantities, 502.
MD Nastran Implicit Nonlinear (SOL 600) produces stress and strain results that differ from those results available with other solution sequences. A detailed discussion of the stress and strain measures for SOL 600 is given in Stress and Strain Measures for Nonlinear Analysis (Ch. 2) in the MSC.Nastran Implicit Nonlinear (SOL 600) User’s Guide.
416
Patran Interface to MD Nastran Preference Guide Output Requests
Basic Output Requests This form is used to select output requests with their default options. The set is always All FEM, which means results for all nodes or elements in the model. A default set of output requests is always preselected.
The available output requests depend on the active Solution Sequence as indicated by this value.
This option menu is used to switch between the advanced and basic versions of this form.
This listbox displays the appropriate result types that may be selected for the solution sequence indicated at the top of the form. The output requests are selected one at a time by clicking. This listbox displays the selected output requests for the subcase shown at the top of the form. The Delete button deletes the output request highlighted in the Output Requests listbox. The TITLE, SUBTITLE and LABEL are written to the MD Nastran output file.
Note:
The OK button accepts the output requests and closes the form. The Defaults button deletes all output requests and replaces them with defaults. The Cancel button closes the form without saving the output requests.
Chapter 3: Running an Analysis 417 Output Requests
Advanced Output Requests This form provides great flexibility in creating output requests. Output requests may be associated with different groups (SET options in MD Nastran) as well as different superelements1. The output requests available depend on the chosen Solution Types, 271, Solution Parameters, 277, and Translation Parameters, 265 . The Advanced Output Requests form is sensitive to the Result Type selected. The Form Type, Delete, OK, Defaults, and Cancel buttons operate exactly like on the Basic Output Requests, 416 form. A description of the output requests and their associated options are listed in Table 3-1 and Table 3-2.
1At the present time, superelement specifications are allowed only in the structured linear static solution
type (Solution Sequence 101).
418
Patran Interface to MD Nastran Preference Guide Output Requests
Use this listbox to select the result type to be created.
This listbox is used to select the group to which the output requests relate.
This databox appears for SOL 101 and 103 when the model contains p-elements. Other options will be presented, such as Percent of Step Output and Intermediate Output Options depending on conditions listed in Table 3-2.
Use this list box to select output requests that are to be modified or deleted.
These are the options that are appropriate to the highlighted result type. They also indicate the options that were selected for a highlighted output request. See Table 3-1.
Chapter 3: Running an Analysis 419 Output Requests
Table 3-1
Output Request Descriptions
Output Request
Case Control Command or Bulk Data Entry
Description
Acoustic Intensity
INTENSITY
Requests acoustic intensity for external acoustics analysis (frequency response).
Acoustic Power
ACPOWER
Requests acoustic power radiated from surface for external acoustics analysis (frequency response).
Acoustic Field Point Mesh
ACFPMRESULT
Requests acoustic field point mesh results for external acoustics analysis (frequency response). You are given a list of all acoustic field point meshes defined and groups with nodes. Each one selected is translated into its own BEGIN AFPM section in the bulk data.
Acoustic Velocities
VELOCITY
Requests nodal velocities. This is for acoustic velocities at the node points of Field Point Mesh.
Displacements
DISPLACEMENT
Requests nodal displacements.
Eigenvectors
VECTOR
Requests nodal eigenvectors.
Element Stresses
STRESS
Requests elemental stresses.
Constraint Forces
SPCFORCES
Requests forces of single- point constraints.
MultiPoint Constraint Forces
MPCFORCES
Requests forces of multipoint constraints (for versions 68 or higher).
Element Forces
FORCE
Requests elemental forces.
Applied Loads
OLOAD
Requests equivalent nodal applied loads.
Nonlinear Applied Loads
NLLOAD
Requests equivalent nonlinear applied loads. Sorting and format options are not allowed with this request.
Element Strain Energies
ESE
Requests elemental strain energies and energy densities. No options are allowed with this output request.
Element Strains
STRAIN
Requests elemental strains.
Grid Point Stresses
GPSTRESS
Requests stresses at grid points.
Velocities
VELOCITY
Requests nodal velocities.
420
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-1
Output Request Descriptions (continued) Case Control Command or Bulk Data Entry
Description
ACCELERATION
Requests nodal accelerations.
Grid Point Force Balance
GPFORCE
Requests grid point force balance at nodes. Sorting and format options are not allowed with this request.
Grid Point Stress Discontinuities
GPSDCON
Requests mesh stress discontinuities based on grid point stresses.
Element Stress Discontinuity
ELSDCON
Requests mesh stress discontinuities based on element stresses.
Nonlinear Stress
NLSTRESS
Requests the form and type of nonlinear element stress output.
Contact Results
BOUTPUT
Requests contact regions for output.
Output Request Accelerations
Table 3-2
Options Sorting
Output Request Form Options
Label By Node/
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
SORT1
Elements
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/ SORT2
Elements
No
Output is presented as tabular listing of frequency or time for each node or element.
Element
Time Format
Tensor
Descriptions
Rectangular
REAL
Elements
No
Requests real and imaginary format for complex output.
Polar
PHASE
Elements
No
Requests magnitude and phase format for complex output.
Von Mises
VONMISES
Elements
No
Requests von Mises stresses or strains.
Maximum Shear
MAXS
Elements
No
Requests Maximum shear or Octahedral stresses or strains.
Chapter 3: Running an Analysis 421 Output Requests
Table 3-2
Options Element Points
Composite Plate Options
Output Request Form Options (continued)
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Cubic
CUBIC
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach with cubic bending correction.
Corner
CORNER
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center.
Center
CENTER
Elements
No
Requests QUAD4 stresses or strains at the center only.
Strain Gage
SGAGE
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach.
Bilinear
BILIN
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using bilinear extrapolation.
Element Stresses
NOCOMPS= -1, LSTRN = 0 in Bulk Data
Elements: Surfaces
No
Composite element ply stresses and failure indices are suppressed. Element stresses for the equivalent homogeneous element are output.
Ply Stresses
NOCOMPS=1,LS Elements: TRN = 0 in Bulk Surfaces Data
No
Composite element ply stresses and failure indices are output. Model should contain PCOMP entry defining composites.
422
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued) Case Control or Bulk Data Options
Options
Label
Composite Plate Options
Ply Strains
NOCOMPS=1,LS Elements: TRN = 1 in Bulk Surfaces Data
No
Composite element ply strains and failure indices are output. Model should contain PCOMP entry defining composites.
Ply Element Stresses
NOCOMPS=0,LS Elements: TRN=0 in Bulk Surfaces Data
No
Composite element ply stresses and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Element and Ply Strains
NOCOMPS=0,LS Elements: TRN=1 in Bulk Surfaces Data
No
Composite element ply strains and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Plane Curv.
STRCUR
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains and curvatures are output at the reference plane for plate elements.
Fiber
FIBER
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains at locations Z1 and Z2 (specified under element properties) are output at the reference plane for plate elements.
By Node /Element
SORT1
Nodes
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/ Time
SORT2
Nodes
No
Output is presented as tabular listing of frequency or time for each node or element.
Rectangular
REAL
Nodes
No
Requests real and imaginary format for complex output.
Polar
PHASE
Nodes
No
Requests magnitude and phase format for complex output.
Plate Strain Options
Sorting
Format
Groups
Multiple Select Allowed
Descriptions
Chapter 3: Running an Analysis 423 Output Requests
Table 3-2
Output Request Form Options (continued)
Options
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Yes
Selects the output coordinate frame for grid point stress output. Coord 0 is the basic coordinate frame.
Elements: Volumes
Yes
Requests direct stress, principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
PRINCIPAL
Elements: Volumes
Yes
Requests principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
Direct
DIRECT
Elements: Volumes
Yes
Requests direct stress, mean pressure stress and von Mises equivalent stresses to be output.
Fiber
All
FIBER, ALL
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at all fibre locations, that is at Z1, Z2 and the reference plane. Z1 and Z2 distances are specified as element properties (default Z1=-thickness/2, Z2= +thickness/2).
Fiber
Mid
FIBER, MID
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at the reference plane.
Z1
FIBER, Z1
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z1 from the reference plane (default Z1=thickness/2).
Z2
FIBER, Z2
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z2 from the reference plane (default Z2=+thickness/2).
Output Coordinate
Coord
COORD CID
Volume Output
Both
Blank
Principal
Elements: Surfaces, Volumes
424
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued)
Options Normal
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
X1
NORMAL X1
Elements: Surfaces,
Yes
Specifies the x-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X2
NORMAL X2
Elements: Surfaces
Yes
Specifies the y-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X3
NORMAL X3
Elements: Surfaces
Yes
Specifies the z-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
Topological
TOPOLOGI-CAL Elements: Surfaces
Yes
Specifies the topological method for calculating average grid point stresses. This is the default.
Geometric
GEOMETRIC
Elements: Surfaces
Yes
Specifies the geometric interpolation method for calculating average grid point stresses. This method should be used when there are large differences in slope between adjacent elements.
X-axis of Basic Coord
X1
AXIS, X1
Elements: Surfaces
Yes
Specifies that the x-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X-axis of Basic Coord
X2
AXIS, X2
Elements: Surfaces
Yes
Specifies that the y-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X3
AXIS, X3
Elements: Surfaces
Yes
Specifies that the z-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
Method
Chapter 3: Running an Analysis 425 Output Requests
Table 3-2
Output Request Form Options (continued)
Options Branch
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Break
BREAK
Elements: Surfaces
Yes
Treats multiple element intersections as stress discontinuities in the geometric interpolation method.
No Break
NOBREAK
Elements: Surfaces
Yes
Does not treat multiple element intersections as stress discontinuities in the geometric interpolation method.
Tolerance
0.0
TOL=0.0
Elements: Surfaces
Yes
Defines the tolerance to be used for interelement slope differences. Slopes beyond this tolerance will signify discontinuous stresses.
Percent of Step Output
100
NOi Field of TSTEP and TSTEPNL entry
All
Once per subcase
An integer ‘n’ that specifies the percentage of intermediate outputs to be presented for transient and nonlinear transient analyses.
Adaptive Cycle Output Interval
0
BY = n on OUTPUT Bulk Data entry
p-elements Once per subcase
An integer ‘n’ that requests intermediate outputs for each nth adaptive cycle. For n=0, only the last adaptive cycle results are output. This is available for SOLs 101 and 103 for versions 68 and higher.
Intermediate Yes Output Options
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed load increment. Applicable for nonlinear static solution type only.
No
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for the last load of the subcase. Applicable for nonlinear static solution type only.
All
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed and userspecified load increment. Applicable for nonlinear static solution type only.
426
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued)
Options
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Suppress Print for Result Type
N/A
Specifies PLOT option instead of PRINT on the Case Control Output request entry.
All
Yes
Print to the .f06 file is suppressed for the result type when this is selected.
Output Device Options
Print
Specifies PRINT on a Case Control request entry, e.g. DISPL.
All
Yes
The printer will be the output medium for the .f06 file.
Punch
Specifies PUNCH All on a Case Control request entry, e.g. DISPL.
Yes
The punch file will be the output medium.
Both
Specifies both PRINT and PUNCH.
Yes
The printer and punch file will be the output medium.
All
Edit Output Requests Form Use this form to edit the outputs request associated with selected subcases. To access this form, select the Output Requests button on the Subcases form with the Action set to Global Data.
Chapter 3: Running an Analysis 427 Output Requests
Selecting the Default button when a single cell is selected resets the selected output request to its default setting.
The row labels for the spreadsheet are the selected subcases from the parent form. The Output Requests for each subcase are stored in cells of the spreadsheet.
Clears the selected cells. You can select individual cells, multiple cells in a column, entire columns, or entire rows. Inactive (greyed out) until a subcase label (column Closes the form and saves the selected changes. To apply the 1) is selected. When this button is selected, the top new output requests, you must select Apply on the parent half of the form will become inactive, and the default Subcases/Global Data form. output request function (named user_change_default_out_req) will be called. This will load user defined defaults or the system defined defaults if user ones do not exist.
Notes: • The Edit Output Requests form opens with focus in the first result type of the first subcase. • The top half of the Edit Output Requests form is similar to the Advanced Output Request form. • The spreadsheet column labels are the result types for the current solution type. • Putting focus in a cell causes the top half of the form to reflect the current setting, just like the
current advanced output request form. This means that the databox RESULT TYPE: gets updated with the result type of the currently selected cell. The OUTPUT REQUESTS: databox is also updated to show the actual content of the cell.
428
Patran Interface to MD Nastran Preference Guide Output Requests
• If a cell is initially empty, selecting it will cause the top half of the form to display the
appropriate default setting for the selected result type (i.e., column). • Selecting a column header will allow you to change all subcase output requests of a particular
type. The top half of the Edit Output Requests form will set to the default request of the particular result type. • When you select a set of contiguous column cells, the top half of the form will configure to the
upper most selected cell. • You cannot select multiple columns.
Default Output Request Information In order to make use of this new feature you will need to create a PCL file that contains the function user_change_default_out_req which will overwrite the existing default file in Patran. This new PCL file will need to be compiled and then the resulting library (.plb) will need to be loaded into Patran. This can be done using the p3midilog.pcl or the p3epilog.pcl file. The user_change_default_out_req function makes use of the mscn_user_add_out_req and the mscn_user_del_out_req functions to add and delete default Output Request types. These two functions are defined as follows:
mscn_user_add_out_req
(or_num, or_value)
Description: This function adds either a specified version or a default version of an Output Request type to the list of default Output Requests. Input: INTEGER or_num The OR number of the output request type to add (See Table 3-3). STRING or_value The value of the selected output request type. Blank implies the default value.
mscn_user_del_out_req
(or_num)
Description: This function deletes the specified Output Request type from the list of default Output Requests. Input: INTEGER or_num The OR number of the Output Request type to delete (See Table 3-3). Code Sample
FUNTION user_change_default_out_req(sol_seq) INTEGER sol_seq IF (sol_seq == 101 || sol_seq == 106) THEN
Chapter 3: Running an Analysis 429 Output Requests
/* This will add this version of the Output Request type to the list of default */ /* Output Requests for solution 101 and 106. */ mscn_user_add_out_req (4,”MPCFORCES(SORT2,REAL)=ALL FEM”) /* This will add the default version of these Output Request types from the list */ /* of default Output Requests for solution 101 and 106. */ mscn_user_add_out_req (10,“ ”) mscn_user_add_out_req (6,“ ”) /* This will delete these Output Request types from the list of default */ /* Output Requests for solution 101 and 106. */ mscn_user_del_out_req (1) mscn_user_del_out_req (2) mscn_user_del_out_req (3) END IF END FUNCTION The following is a table that shows the current predefined default Output Requests (those marked with an X) and the allowed options (those marked with an O) for the various solution sequences. Table 3-3
Result ID Number OR Number
Result ID Number (Solution Sequence )
1
2
3
4
5
6
101
x
x
x
o
o
o
103
o
o
x
o
o
105
x
o
x
o
o
o
106
x
x
x
o
o
107
o
o
x
o
o
108
x
o
x
o
o
o
109
x
o
x
o
o
o
110
o
o
x
o
o
111
x
o
x
o
o
o
112
x
o
x
o
o
o
114
x
x
x
o
o
o
115
o
o
x
o
o
129
x
o
x
153
o
o
o
159
o
o
o
400
o
7
8
9
10 11 12 13 14 15 16 17 18 19 20 21
o
o
o
o
o
o
o
o o
o o
o
o o
o
o
o
o
o
x
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
x
o
o
o
o
o
o
o
o o
x
x
x
o
o
o
o
o o
o
24
x
o o
o
23
x
o o
o
22
o
o
o
o
o
x
x
o
o
o
x
x
o
o
o o
o
o x
x
430
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-3
Result ID Number x
600
x
700
o
x
o
o
o
o
o
o
o
x
1 = Displacement, 2 = stress, 3 = spcforces, 4 = mpcforces, 5 = forces, 6 = oload, 7 = nlload, 8 = ese, 9 = strain, 10 = gpstress, 11 = velocity, 12 = acceleration, 13 = gpforce, 14 = gpsdcon, 15 = elsdcon, 16 = vector, 17 = thermal, 18 = flux, 19 = ht_oload, 20 = ht_spcforces, 21 =enthalpy, 22 = hdot
OR #
Default Value 1
DISPLACEMENT(SORT1,REAL)=All FEM
2
STRESS(SORT1,REAL,VONMISES,BILIN)=All FEM;PARAM,NOCOMPS,-1
3
SPCFORCES(SORT1,REAL)=All FEM
4
MPCFORCES(SORT1,REAL)=All FEM
5
FORCE(SORT1,REAL,BILIN)=All FEM
6
OLOAD(SORT1,REAL)=All FEM
7
NLLOAD=All FEM
8
ESE=All FEM
9
STRAIN(SORT1,REAL,VONMISES,STRCUR,BILIN)=All FEM
10
GPSTRESS=All FEM; VOLUME # SET,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL,BRANCH BREAK
11
VELOCITY(SORT1,REAL)=All FEM
12
ACCELERATION(SORT1,REAL)=All FEM
13
GPFORCE=All FEM
14
GPSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
15
ELSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
16
VECTOR(SORT1,REAL)=All FEM
17
THERMAL=(SORT1,PRINT)=All FEM
18
FLUX(SORT1,PRINT)=All FEM
19
OLOAD(SORT1,PRINT)=All FEM
20
SPCFORCES(SORT1,PRINT)=All FEM
21
ENTHALPY(SORT1,PRINT)=All FEM
22
HDOT(SORT1,PRINT)=All FEM
Chapter 3: Running an Analysis 431 Output Requests
23
NLSTRESS
24
BCCONTACT
Note:
In SOL 109, 112 & 159 will have SORT2 as the default in some versions of Patran.
Subcases Direct Text Input This form is used to directly enter entries into the Case Control section for the defined subcase. Directly entered entries may potentially conflict with those created by the interface. Writing these entries to the file can be controlled with this toggle.
Saves the current setting and data for the four sections and closes the form.
Clears the current form.
Resets the form back to the data values it had at the last OK.
Resets all four forms back to its previous value and closes the form.
432
Patran Interface to MD Nastran Preference Guide Output Requests
SOL 600 Output Requests This subform defines the output data for a SOL 600 analysis subcase
Echo Marc Input File
Produces an echo of the input file.
Results in Marc Print File
Writes results to a print file.
Results (POST) File Options • Increments between Writing Results
Defines the number of increments between writing results to the MD Nastran results file after the first increment of the analysis. The default is one (1) for every increment. Note: You can select a fixed number of increments of output on the subcase parameters-load increments parameters form.
• Select Nodal Results...
Brings up a subform for selecting nodal results
• Select Element Results...
Brings up a subform for selecting elemental results.
Output requests for all subcases.
Chapter 3: Running an Analysis 433 Output Requests
Select Nodal Results
This subform controls which nodal result quantities are returned from the analysis.
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers, that will be specified on the MARCOUT entry
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
434
Patran Interface to MD Nastran Preference Guide Output Requests
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis. Nodal Result
Postcode
Default(?)
DISPLACEMENT
1
YES
ROTATION
2
no
EXTERNAL FORCE
3
no
EXTERNAL MOMENT
4
no
REACTION FORCE
5
YES
REACTION MOMENT
6
no
PORE PRESSURE
23
no
VELOCITY
28
no
ROTATIONAL VELOCITY
29
no
ACCELERATION
30
no
ROTATIONAL ACCELERATION
31
no
MODAL MASS
32
no
ROTATION MODAL MASS
33
no
CONTACT NORMAL STRESS
34
no
CONTACT NORMAL FORCE
35
no
FRICTION STRESS
36
no
FRICTION FORCE
37
no
CONTACT STATUS
38
no
CONTACT TOUCHED BODY
39
no
HERRMANN VARIABLE
40
no
POST CODE, No. -11
-11 thru -16
no
POST CODE, No. -22
-21 thru -23
no
POST CODE, No. -31
-31
no
POST CODE, No. -41
-41
no
POST CODE, No. -51
-51
no
Note:
The POST CODE (<0) are for user-defined quantities via user subroutine UPSTNO.
Chapter 3: Running an Analysis 435 Output Requests
Element Output Requests
This subform controls which element result quantities are returned from the MSC.Marc analysis.
436
Patran Interface to MD Nastran Preference Guide Output Requests
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers.
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
Element X-section Results
Defines the number of layer points to use through the cross section of homogeneous shells, plates and beams. This number must be odd if not a composite.
Note:
If no changes are made to the default output requests, no MARCOUT entry will be written and MD Nastran will determine the appropriate output.
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis. Elemental Result
Postcode
Solutions
Default(?)
STRAIN, TOTAL COMPONENTS
301
nonlinear only
YES
STRAIN, TOTAL COMPONENTS (defined system)
461
nonlinear only
no
STRAIN, ELASTIC COMPONENTS
401
any
no
STRAIN, ELASTIC COMPONENTS (global system)
421
any
no
STRAIN, ELASTIC EQUIVALENT
127
any
no
STRAIN, PLASTIC COMPONENTS
321
nonlinear only
no
STRAIN, PLASTIC COMPONENTS (global system)
431
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT
27
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT (from rate)
7
nonlinear only
no
STRAIN, CRACKING COMPONENTS
381
nonlinear only
no
STRAIN, CREEP COMPONENTS
331
creep only
no
STRAIN, CREEP COMPONENTS (global system)
441
creep only
YES
STRAIN, CREEP EQUIVALENT
37
creep only
no
STRAIN, CREEP EQUIVALENT (from rate)
8
creep only
no
STRAIN, THERMAL
371
any
no
STRAIN, THICKNESS
49
any
no
STRAIN, VELOCITY
451
nonlinear only
no
Chapter 3: Running an Analysis 437 Output Requests
Elemental Result
Postcode
Solutions
Default(?)
STRESS, COMPONENTS
311
any
no
STRESS, COMPONENTS (defined system)
391
an
no
STRESS, COMPONENTS (global system)
411
any
YES
STRESS, EQUIVALENT YIELD
59
nonlinear only
no
STRESS, EQUIVALENT MISES
17
any
no
STRESS, MEAN NORMAL
18
any
no
STRESS, INTERLAMINAR SHEAR No. 1
108
any
no
STRESS, INTERLAMINAR SHEAR No. 2
109
any
no
STRESS, INTERLAMINAR COMPONENTS
501,511
any
no
STRESS, CAUCHY COMPONENTS
341
nonlinear only
no
STRESS, CAUCHY EQUIVALENT
47
nonlinear only
no
STRESS, HARMONIC COMPONENTS
351 (real) 361(imag)
harmonic only
no
STRESS, REBAR UNDEFORMED
471
any
no
STRESS, REBAR DEFORMED
481
any
no
FORCES, ELEMENT
264-269
any
no
BIMOMENT
270
any
no
STRAIN RATE, PLASTIC
28
nonlinear only
no
STRAIN RATE, EQUIVALENT VISCOPLASTIC
175
any
no
STATE VARIABLE, SECOND
29
any
no
STATE VARIABLE, THIRD
39
any
no
TEMPERATURE, ELEMENT TOTAL 9
any
no
TEMPERATURE, ELEMENT INCREMENTAL
any
no
STRAIN ENERGY DENSITY, TOTAL 48
nonlinear only
no
STRAIN ENERGY DENSITY, ELASTIC
58
any
no
STRAIN ENERGY DENSITY, PLASTIC
68
nonlinear only
no
THICKNESS, ELEMENT
20
any
no
10
438
Patran Interface to MD Nastran Preference Guide Output Requests
Elemental Result
Postcode
Solutions
Default(?)
VOLUME, ELEMENT
78
any
no
VOLUME, VOID FRACTION
177
any
no
GRAIN SIZE
79
any
no
FAILURE, INDEX No. 1-7
91-103
any
no
DENSITY, RELATIVE
179
any
no
POST CODE, No. 19
19
any
no
POST CODE, No. 38
38
any
no
POST CODE, No. -11
-11 thru -16
any
no
POST CODE, No. -21
-21 thru -23
any
no
POST CODE, No. -31
-31
any
no
POST CODE, No. -41
-41
any
no
POST CODE, No. -51
-51
any
no
DDAM Output Requests The output requests form has been altered for the DDAM solution. Because the program performs an NRL sum and has no explicit constraints, only a few result quantities are available: Nodal Results: Displacement Velocity Accelerations Element Results: Stress Force The results reported in the .f06 file are printed sequentially, first x-shock results, then y, then z, but all are labeled as TIME = 0.000000E+00. To differentiate these in the file, there is a small header printer prior to the results for each shock direction that looks something like this: ^^^ ^^^ *************************************** ^^^ ^^^ SUMMED MODAL RESPONSES IN X-DIRECTION ^^^ ^^^ *************************************** ^^^
Chapter 3: Running an Analysis 439 Output Requests
If you need to find the start of the X-shock results, search for X-DIRECTION to find this header and proceed from there. It is necessary to specify that Patran calculate the combined stresses on a mode-by-mode basis, and NRL sum the combined results. See Defining Translation Parameters for DDAM (SOL 187) (Ch. 4). Mode by Mode Output You can use the Direct Text Input section of Patran Analysis forms to obtain more data. Using the parameters XBYMODE, YBYMODE and ZBYMODE you can get mode by mode data for the selected direction. To get this data, enter the following lines into the Bulk Data direct text area: PARAM,XBYMODE,YES PARAM,YBYMODE,YES PARAM,ZBYMODE,YES You can select one or more of these parameters. Keep in mind that this generates a lot of data for an analysis with a lot of modes, and that you must have an output request for the corresponding data – e.g., if you want mode-by-mode displacements, you must have a DISPLACEMENT request as chosen above. Each of these parameters outputs the data to the .f06 file if you have the (PRINT) option on, or an .op2 file if the (PLOT) option is on. Both are on by default when you specify something like: DISPLACEMENT = ALL Alternately, DISPLACEMENT(PLOT) = ALL DISPLACEMENT(PRINT) = ALL plots or prints the results. If unassigned, the mode-by-mode results outputs to generic Fortran files (like fort.42), so it is necessary to add an ASSIGN statement to the file if you wish to have these files named appropriately. To do this, use the FMS section in the Direct Text Input form, and add lines like: ASSIGN OUTPUT2=’jobname_mbmx.op2’, UNIT=41, DELETE ASSIGN OUTPUT2=’jobname_mbmy.op2’, UNIT=42, DELETE ASSIGN OUTPUT2=’jobname_mbmz.op2’, UNIT=43, DELETE In the .f06 file, the mode-by-mode results are labeled with their own header prior to the section: ^^^ ^^^ ************************************************** ^^^ ^^^ INDIVIDUAL SCALED MODAL RESPONSES IN Y-DIRECTION ^^^ ^^^ ************************************************** ^^^
440
Patran Interface to MD Nastran Preference Guide Output Requests
Since the mode-by-mode velocities and accelerations are calculated by multiplying the displacements by the frequency (omega and omega2), MD Nastran labels them as Eigenvectors. If you ask for displacement, velocity, and acceleration for three modes, you will find nine Eigenvectors in the .f06 file with repeating frequencies – the first three (1-3) are displacements, the next three (4-6) velocities, and the last three (7-9) the accelerations. The .op2 files are similar, reporting the three as Eigenvectors with repeating frequencies. The magnitude of the values should be a clue as to what you are looking at for all but the lowest frequencies. The Fortran Driver File (jobname.ddd)
Some of the options you choose on the Subcase Parameters form are written to an external file that is read by the Fortran file when it calculates the spectrum. While you do not have the ability to edit this file when using MSC.FEA, the file is a hardcopy ASCII record of what options were used when running the DDAM analysis. The file is small and has just a few lines that comprise the answers to questions that the ddam.exe program asks if it is run interactively. File Format (varies depending on chosen options on the first record) Record 1 (user spectrum file) (user coef file) (DDS-072 format) user spectrum file= T (use a user defined spectrum) = F (use coefficients) user coef file = T (use an external coefficient file) = F (use the coefficients compiled into the Fortran) DDS-072 format = T (use DDS-072 style equations) = F (use NRL 1396 style equations) Record 1a (if either file option on record 1 was true) cp10 filename = name of either the spectrum file or coefficient file Record 2 (if using coefficients) nsurf nstruc nplast ship type mount location elastic/plastic
Record 3 pref pref
= 1 (surface ship equations) = 2 (submarine equations) = 1 (file mounted equipment) = 2 (hull mounted equipment) = 1 (use elastic factors) = 2 (use elastic/plastic factors)
= 0.0 (use default cutoff in program) = nnn.nn
Chapter 3: Running an Analysis 441 Output Requests
Record 4 Ming Ming
Record 5 (F/A axis) (Vert axis) F/A axis
Vert axis
= 0.0 (no minimum G) = n.n (use this minimum G value)
= X (F/A is along the X axis) = Y (F/A is along the Y axis) = Z (F/A is along the Z axis) = X (Vertical is along the X axis) = Y (Vertical is along the Y axis) = Z (Vertical is along the Z axis)
Record 6 .f11 filename .f11 filename
= name of the .f11 file
Record 7 .f13 filename .f13 filename
= name of the .f13 file
Record 8 .ver filename .ver filename
= name of the modal verification file
Depending on the chosen options, the file will look like one of the following: No special user options – coefficients from default source:
F F T nsurf nstruc nplast pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename
442
Patran Interface to MD Nastran Preference Guide Output Requests
User coefficient option:
F T T coef.dat filename nsurf nstruc nplast pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename User spectrum Option:
T F T spec.dat filename pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename Note:
Note that capitalization is required. The file is read free-format, so spacing is not important. A sample file for a conventional analysis might look like: F F T 1 1 1 100. 1. X Z d1.f11 d2.f11 d1.ver
Chapter 3: Running an Analysis 443 Select Explicit MPCs...
3.10
Select Explicit MPCs... The Explicit MPCs created in the Element menu can be selected for a given subcase. The highlight of selected Explicit MPCs is supported when this form is displayed. The All MPCs toggle indicates that all the Explicit MPCs already created or created later will be used for the subcase being created. The All MPCs toggle should be turned OFF in order to select MPCs. ‘MPXADD SID’ is the ID used for identifying the selected MPCs for the subcase.
444
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
3.11
Non-Structural Mass Properties MSC Nastran non-structural mass (NSM and NSML) are now supported in Patran. Note:
NSM and NSML are used to define masses that affect the behavior of specific element types but are not directly part of the structure of the model. NSM and NSML support:
Line Element Types
Surface Element Types
Property Types
CBAR, CBEAM, CBEND, CONROD, CROD, CTUBE
CCONEAX, CQUAD4, CQUAD8, CQUADR, CRAC2D, CSHEAR, CTRIA3, CTRIA6, CTRIAR
CONROD, PBAR, PBARL, PBCOMP, PBEAM, PBEAML, PBEND, PCOMP, PCONEAX. PRAC2D, PROD, PSHEAR, PSHELL, PTUBE
NSM and NSML forms are available through the Tools menu.
Selecting NSM Properties displays the NSM Properties form. NSM Properties forms are MSC Nastran preference specific. NSM mass can be applied as Lumped or Distributed.
Chapter 3: Running an Analysis 445 Non-Structural Mass Properties
For a distributed NSM, the mass is spread evenly over all of the elements in the application region. For a lumped NSM, the applied mass is applied directly to each element in the application region.
446
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
Non-structural mass can be applied to elements or property sets.
Chapter 3: Running an Analysis 447 Non-Structural Mass Properties
A Select form has been added to allow for the selection of NSM properties. Multiple sets of NSMs can be defined in the model. Only the selected sets will be used in the analysis.
The following examples display results of applying lumped and distributed NSMs.
448
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
A lumped mass value of 20 is applied to 10 elements
A distributed mass value of 20 is applied to 10 elements.
Chapter 3: Running an Analysis 449 Select NSM Properties...
3.12
Select NSM Properties... This Subcases dependant form allows you to select the defined Nonstructural Mass sets. The Defined NSM Sets box lists all defined Nonstructural Mass property sets. Since it is possible to have up to four property sets with the same set name, the Distributed vs Lumped and Element vs Property attributes of the sets are listed in columns to the left of the property set name. Individual groupings of Nonstructural Mass property sets can be selected in the form and then applied with the Apply button. By default, all of the listed Nonstructural Mass property sets are selected by the case control code even if they are not shown as selected in the Defined NSM Sets box. Groups of Nonstructual Mass properties can be excluded from an analysis by not including that specific subcase in the analysis job. Individual Nonstructural Mass properties can be excluded from an analysis by setting the applied mass for that property set to zero (0).
450
Patran Interface to MD Nastran Preference Guide Select NSM Properties...
This subform appears when the Select NSM Properties... button is selected from the Subcases form.
Chapter 3: Running an Analysis 451 Subcase Select
3.13
Subcase Select This form appears when the Subcase Select button is selected on the Analysis form. This form is used to select a sequence of subcases associated with an analysis job.
Displays all the available subcases for the current solution sequence. The current solution sequence is displayed at the top of the form. For example, SOL 101 subcases lc1, lc2, and lc3.
Displays all subcases that have been associated with the current job name. For example, subcases lc1 and lc3 have been selected; for SOL 101 the Bulk Data will contain two Case Control section SUBCASEs, SUBCASE 1 and SUBCASE 2. For SOL 600 a single run will be performed with it having two steps, lc1 and lc3. For optimization jobs, the solution type will be appended at the begining of the subcase name.
For SOL 400 runs the Subcase Select form looks the same, except for the Select Steps for New Subcase button being un-greyed (it is pickable).
452
Patran Interface to MD Nastran Preference Guide Subcase Select
Displays all the available subcases for SOL 400. For example, subcases lc1, lc2, lc3, lc4, and lc5.
Displays all subcases that have been associated with the current job name. If the button Select Steps for New Subcase is not used, the job run will be the same as for SOL 600 , a single run will be performed with five steps, 1c1, ..., lc5, in the order shown in the GUI going from top to bottom.
When the Select Steps for New Subcase button is used the following form appears.
Chapter 3: Running an Analysis 453 Subcase Select
Notice that the selected steps (lc1, lc2, lc3, lc4, and lc5) match the selected subcases of the parent form. This indicates that some or all of these steps can be used in defining the new subcases. By selecting the steps lc1 and lc3, under Steps Selected, the names are entered under New Subcase Starting with Steps. This indicates that two subcases will be defined, “subcase_lc1” and “subcase_lc3”.
Displays the steps names that are to be used at the begining of the (new) subcases to be created. The subcases that are defined are “subcase_lc1” with steps lc1 and lc2, and “subcase_lc3” with steps lc3, lc4 and lc5: • Subcase, “subcase_lc1” • Steps: lc1, lc2 • Subcase, “subcase_lc3” • Steps: lc3, lc4, lc5
454
Patran Interface to MD Nastran Preference Guide Restart Parameters
3.14
Restart Parameters This format of the Analysis form appears when the Action is set to Analyze and the Object is Restart. Currently, restarts are only supported for the Linear Static (101), Nonlinear Static (106), and Normal Modes (103) Solution Sequences. Linear and Nonlinear Static jobs can be restarted as Linear or Nonlinear Static. Normal Modes jobs can be restarted as Frequency Response, or Transient Response. The DBALL and the MASTER files for the initial job must be present in the current directory when the restart job is submitted.The Restart Parameters button on the main analysis form allows the user to enter information about where to resume the analysis. The Patran Analysis Manager User’s Manual contains
Chapter 3: Running an Analysis 455 Restart Parameters
more information on how to submit restart jobs with Analysis Manager. Restart for SOL 600 jobs are described on (p. 315) and (p. 458).
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of names for existing analysis jobs. Select the jobname of the analysis to restart from.
List of names for existing restart jobs. Select the name of an existing restart job or enter the name for a new restart job in the databox below.
Name to use for the restart job. An existing restart job may be modified and/or resubmitted by making a selection from the Available Restart Jobs listbox.
456
Patran Interface to MD Nastran Preference Guide Restart Parameters
Linear Static/Normal Modes
This subordinate form appears when the Restart Parameters button is selected on the Analysis form and the solution type of the initial job is Linear Static or Normal Modes.
Defines the version number from which to restart. This is the VERSION field on the RESTART file management statement.
Requests that the restart data for the specified version be saved. This results in a KEEP option on the RESTART File Management statement.
Chapter 3: Running an Analysis 457 Restart Parameters
Nonlinear Static
This subordinate form appears when the Restart Parameters button is selected on the Analysis form and the solution type is Nonlinear Static.
Defines the version number to restart the analysis from. This is the VERSION field on the RESTART File Management statement.
Defines the increment number to start the analysis from. This is the value of the PARAM,LOOPID Bulk Data entry.
Defines the subcase number to start from in the list of subcases for this job. The value entered should be one greater than the SUBID from the initial job’s print file (*.f06). This is the value of the PARAM,SUBID Bulk Data entry. Requests that the restart data for the specified version be saved. This results in a KEEP option on the RESTART File Management statement.
458
Patran Interface to MD Nastran Preference Guide Restart Parameters
SOL 600
This subordinate form appears when the Restart Parameters button is selected on the Solution Parameters form.
Set Restart Parameters Restart Parameters: None
Restart Type: Create Continuous Results File Last Converged Increment
Reauto
Restart from Increment =
Increments between Writing Data =
Select Restart File...
OK
Parameter
Cancel
Description
Restart Type
You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File
If, when restarting a job, you wish the results form the previous run to be copied into the new .t16 file, then turn this ON. Otherwise MSC.Marc will not copy the results to the new .t16 file. If you turn this ON, you must have a restarname.marc .t16 and/or restartname.marc.t19 file in your local directory or the MSC.Marc analysis will fail.
Last Converged Increment
Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto
OFF by default. This places a REAUTO option in the MSC.Marc input file. Any additional data needed for the REAUTO option are extracted from the first Subcase information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user.
Chapter 3: Running an Analysis 459 Restart Parameters
Parameter
Description
Restart from Increment
Defines the increment to be read from the file specified in the Select Restart File form. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing
Defines the number of increments between writing data to the restart file. It is only requested when Restart Type is set to Write or Read and Write.
Select Restart File...
This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write.
460
Patran Interface to MD Nastran Preference Guide Optimize
3.15
Optimize When preparing for an optimization analysis run, select Optimize as the Action on the Analysis application form. This allows setup and submission of SOL 200 jobs. The functionality is similar and in many cases identical to running a normal analysis as described in Review of the Analysis Form, 260 and other sections in this chapter. Each button and its subordinate form that appears when the Action is set to Optimize is explained briefly below. Use the Optimize action for sizing optimization and combined sizing and topology optimization. For pure topology, topography and topometry optimization, use the Toptomize action explained in Toptomize, 462.
Button/Subordinate Form:
Description:
Design Study Select...
From this form, select the design study of interest. Design studies can contain multiple design objectives, responses, constraints, and variables. Any particular job can only have one design objective. The specific objective and constraints to be used in an optimization job are selected in the Global Objective / Constraint Select form or they are associated to a solution specific subcase. Design Studies are setup under the Design Study tool under the Tools pull down menu. A Default design study is present if none are previously created, however a design study without any design variable defined will not run through Nastran properly.
Global Obj/Constr Select...
Once a design study has been selected, you may select from this form the specific global design objective and constraints to be active for this job. You can only have one objective in an optimization job. A global objective will override any other objective associated to a solution specific subcase that may be associated to this job, therefore it is not necessary to select a global objective or constraints when defined at the subcase level.
Translation Parameters...
These parameters are described in Translation Parameters, 265 and are not specific to optimization.
Optimization Parameters...
This form is used to define optimization parameter for the job. Parameters set in this form and its subordinate form define some of the values on the DOPTPRM entry. These are explained in the MSC Nastran Quick Reference Guide under this entry and the user if referred there for details. Results file formats can also be set in this form as described in Results Output Format, 348.
Direct Text Input...
Use of this form is described in Direct Text Input, 276.
Select Superelements...
Use of this form is described in Select Superelements, 352.
Subcases...
Use of this form is described in Subcases, 354. There are two differences that are significant to this form, however. For optimization, subcases are created based on solution sequence, e.g. Statics 101, Normal Modes 103, etc. You must set the solution sequence on this form before creating the subcase, otherwise the default 101 will be used. Secondly, an additional subordinate form allows you to select existing constraint sets and an objective for the particular subcase being created if necessary. Objectives and constraints are created using the Design Study tool under the Tools pull down menu. Note that not all subcase parameters are identical between a normal analysis and an optmization analysis. Also see the note on Contact below: page 461.
Chapter 3: Running an Analysis 461 Optimize
Button/Subordinate Form:
Description:
Subcase Select...
Use of this form is described in Subcase Select, 451. One difference is that for optimization you must set the solution type to see the subcases defined for a particular solution sequence. Otherwise by default only SOL 101 subcases are displayed. A selected subcase will display the associated solution sequence number in front of its label.
Analysis Manager...
This gives access to the Analysis Manager for submitting, monitoring, aborting and generally managing a Nastran job. This button will not appear if the Analysis Manager is not installed or licensed.
Note:
Using Contact Bodies in Optmization Jobs: Linear contact is supported in optimization jobs (SOL 200). If contact bodies are present in the model and included in the load cases associated to the the subcases created, then the contact bodies will be written to the deck. The most common scenario is using linear contact in optimization jobs to glue noncongruent meshes together. When this feature is used, you must “glue” the bodies together, which requires that you set up the proper contact tables to define body pairs that are properly glued. Usage of the contact table is described in Contact Table, 396.
462
Patran Interface to MD Nastran Preference Guide Toptomize
3.16
Toptomize When preparing for a pure topology, topometry, or topography optimization analysis run, select Toptomize as the Action on the Analysis application form. This allows setup and submission of SOL 200 jobs. The functionality is similar and in many cases identical to running a normal analysis as described in Review of the Analysis Form, 260 and other sections in this chapter. Each button and its subordinate form that appears when the Action is set to Toptomize is explained briefly below. Use the Optimize action for sizing optimization and combined sizing and topology optimization as explained in Optimize, 460. Button/Subordinate Form: Translation Parameters...
Description: These parameters are described in Translation Parameters, 265 and are not specific to optimization.
Optimization Parameters... This form is used to define optimization parameter for the job.
Parameters set in this form and its subordinate form define some of the values on the DOPTPRM entry. These are explained in the MSC Nastran Quick Reference Guide under this entry and the user if referred there for details. Note that no DOPTPRM entry is written if all values are default values. Results file formats can also be set in this form as described in Results Output Format, 348.
Objectives & Constraints... This form allows you to define the objective and constraints for the topology, topometry or topography optimization run. Please see Objectives & Constraints, 463 below.
Optimization Controls...
This form allows you to define various controls and settings necessary for topology, topometry, or topography optimization jobs. Please see Optimization Control, 464 below.
Design Domain...
This form allows you to select the property sets that define the active design domain. Manufacturing constraints are defined via this form also. Please see Design Domain, 466 below.
Direct Text Input...
Use of this form is described in Direct Text Input, 276.
Subcases...
Use of this form is described in Subcases, 354. There are two differences that are significant to this form, however. For optimization, subcases are created based on solution sequence, e.g. Statics 101, Normal Modes 103, etc. You must set the solution sequence before creating the subcase, otherwise the default 101 will be used. Secondly, an additional subordinate form allows you to select existing constraint sets and an objective for the particular subcase being created if necessary. Objectives and constraints are created using the Design Study tool under the Tools pull down menu. Note that not all subcase parameters are identical between a normal analysis and an optmization analysis. Also see the note on Contact above: page 461.
Subcase Select...
Use of this form is described in Subcase Select, 451. One difference is that for optimization you must set the solution type to see the subcases defined for a particular solution sequence. Otherwise by default only SOL 101 subcases are displayed. A selected subcase will display the associated solution sequence number in front of its label.
Analysis Manager...
This gives access to the Analysis Manager for submitting, monitoring, aborting and generally managing a Nastran job. This button will not appear if the Analysis Manager is not installed or licensed.
Chapter 3: Running an Analysis 463 Toptomize
Objectives & Constraints This form is used to define the optimization type and select the objective and constraints of the optimization run. All widgets on this form are explained in the table below. Widget Parameter:
Description:
Type
Select the optimization type for job to be set up, either Topology, Topometry, or Topography. Topology is the default.
Objective Function(s):
The objective of the optimization is set with the widgets in this frame. The default is to Minimize Compliance. Multiple static subcases are allowed.
Minimize Compliance Maximize Frequency Track Modes Mode Numbers
Optionally you can also maximize frequency (or eigenvalue). You specify the mode number in the provided databox. If the provided mode is not the first mode or you provide modes such as 1 5 and 6, you can turn on the Track Modes toggle. This is recommended as modes can change with each design cycle. The MODTRAK case and bulk data entries are written in this case using the number of modes called out for extraction as set up in the modal subcase. Multiple modal subcases are allowed. A DESOBJ case control entry is written to the deck which calls out the appropriate DRESP1 and/or DRESP2 entries with the COMP, FREQ, or EIGN options. Multiple DRESP1 entries are written when the Constraint Target is Mass Fraction with multiple property sets selected and subsequently referenced or combined using an average function on the DRESP2 entry. Only one objective is allowed, however you can specify to Minimize Compliance and Maximize Frequency in which case you need to also specify a single Frequency Constraint Target. This target along with the compliance minimization objective is combined onto a DRESP2 entry using a DEQATN entry to formulate the objective relationship. In this case a single modal subcase is required. Note that when multiple static subcases are selected, a DRSPAN entry is written to each subcase as necessary to ensure the objective function properly spans all subcases.
464
Patran Interface to MD Nastran Preference Guide Toptomize
Widget Parameter: Frequency Constraint Targets
Description: Specify the mode number(s) and corresponding frequencies to be constrained in the optimization run. At least one modal subcase is required. This is typically used when the Objective Function is set to Maximize Frequency. If the Objective Function is set to both Minimize Compliance and Maximize Frequency, then a singe mode frequency target is required and only one modal subcase is allowed. A DESSUB case control is written to the deck which calls out the appropriate DCONSTR and DRESP1 entries. This constraint because part of the objective if both Minimize Compliance and Maximize Frequency objective functions are specified and is incorporated via a DEQATN entry referenced on a DRESP2 entry called out by a DESOBJ case control.
Constraint Target
Specify the constraint target. For Topology, only Mass Fraction is allowed. For Topography, only Weigh or Volume is allowed. For Topometry, either of the three are allowed. You must specify the mass fraction, weight or volume target. By default, the mass fraction is 0.4 (40% of the original mass). However, volume and weight have no defaults. If the Objective Function is set to only Maximize Frequency, then a Constraint Target is not required (can be set to None) for Topometry and Topography only. A DESGLB case control is written, which calls out the appropriate DCONSTR and DRESP1 entries. For Weight and Volume, only a single DCONSTR/DRESP1 entry combination is written as the entire design domain can only have one weight or volume constraint. For Mass Fraction, multiple combinations are written with the same DCONSTR ID.
Optimization Control Use this form to set various controls used during the optimization run. They are briefly described here but the user is referred to the MSC Nastran Quick Reference Guide for further information. Leaving a field blank will trigger usage of the default in most cases. Some parameters must be provided or the analysis cannot proceed. Setting the Maximum Design Cycles is the most common usage of this form to limit the analysis to something reasonable. Each optimization type has different settings: Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Initial Design (XINIT)
Required. Initial value. It is recommended that this match the mass target constraint. This value defaults to the mass value target constraint set on the Objectives and Constraints form.
Lower Bounds (XLB)
Optional. Lower bound to prevent the singularity of the stiffness matrix. Leave blank to use Nastran default of 0.001. Real 0.0 < XLB <= 0.1
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Penalty Factor (POWER)
Optional. A penalty factor used in the relation between topology design variables and element Young’s modulus. Leave blank to use Nastran default of 3.0. Real 1.0 <= POWER <= 6.0
Chapter 3: Running an Analysis 465 Toptomize
Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Minimum Member Size (TDMIN)
Optional. Indicates the minimum member size. No default. No minimum is used if not specified. Recommendation is that it be set to three times a representative element dimension. Real > 0.0. This is written to the DOPTPRM entry and is for 2D and 3D elements only.
Checkboard-Free Method (TCHECK)
Optional. On by default. Turns on/off topology filtering (allows of minimizes checker boarding effects). This is written to the DOPTPRM.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
Topometry Parameters:
Description: (all values written to the TOMVAR entry unless otherwise indicated)
Initial Design (XINIT)
Required. Initial design value of property to optimize. Optimization job will not proceed without this value defined. Real > 0.0
Lower Bounds (XLB)
Optional. Lower bound of the property to optimize. Leave blank to use Nastran default of XLB=0.5*XINIT. Real > 0.0.
Upper Bounds (ULB)
Optional. Upper bound of the property to optimize. Leave blank to use Nastran default of XUB=1.5*XINIT. Real > 0.0.
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Property to Optimize (PNAME)
Required. The property to optimize. No Nastran default. This is dependent on the model dimensionality is some cases. Default is set to Thickness for 2d problems but is not appropriate for 1D models where cross sectional Area would be the most common choice.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
466
Patran Interface to MD Nastran Preference Guide Toptomize
Topography Parameters:
Description: (all values written to the BEADVAR entry unless otherwise indicated)
Lower Bounds (XLB)
Optional. Lower bound on the bead height. Leave blank to use Nastran default of 0.0. See the Upper Bounds (XUB) description.
Upper Bounds (XUB)
Optional. Upper bound on the bead height. Leave blank to use Nastran default of 1.0. To force grids to move only the positive bead vector direction (one side of the surface), use XLB = 0.0. To force grids to move only in the negative bead vector direction (the other side of the surface), use XUB = 0.0. To allow grids to move in both positive and negative bead vector directions, use XLB < 0.0 and XUB > 0.0.
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Minimum Bead Width (MW)
Required. Minimum bead width. There is no default. This controls the width of beads and the recommended value is 1.5 to 2.5 times the average element width. Real > 0.0
Maximum Bead Height (MH)
Required. Maximum bead height. There is no default. This controls the maximum height of beads when XUB = 1.0 (or left blank). Real > 0.0
Draw Angle (ANG)
Required. Draw angle in degrees. This controls the angel of the sides of the beads and the recommended values is between 60 and 75 degrees.
Buffer Zone (BF)
Optional. Buffer zone. This parameter creates a buffer zone between elements in the topography design region and elements outside the design region when turned on, which is the default.
Exclude from Design (SKIP)
Optional. Boundary skip. This indicates which element nodes are excluded from the design region. Constraints indicates all constrained nodes and Loads indicates all nodes referenced by forces, moments and enforced displacements. Both are on by default.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
Design Domain The property sets that define the intended design domain are set on this form as well as manufacturing constraints. The form works by clicking on a valid property set (row) in the top spread sheet. This action adds the selected row to the bottom spread sheet, which are the active domains during the optimization run. To remove domains, click on the rows of interest in the bottom spread sheet and press the Remove Selected Rows button.
Chapter 3: Running an Analysis 467 Toptomize
From this form you can also define manufacturing constraints to impose on the topology optimization. Each property set is written to a TOPVAR, TOMVAR, or BEADVAR entry in the input file depending on the optimization Type set in the Objectives & Constraints form. The values of various parameters on these entries can be different for each property set. It is recommended that you review the settings for each property set defined in the design domain before submitting the job. When a property set is added to the selected design domain properties spreadsheet, some of the values are set in the various columns from the settings on the Optimization Control form. To change these settings for an individual property set, simply click on the cell to be changed. A widget will appear above the spreadsheet allowing you to change the value. Use the Enter key to accept the new value into the spreadsheet. The same can be done when opening the Manufacturing Constraints form. The values set in the Manufacturing Constraint forms will correspond only to the property sets that are selected from the Design Domain spreadsheet. If you do not select any rows in the Design Domain spreadsheet, then any change made on the Manufacturing Constraints form will be applied to all property sets in this spreadsheet. For this reason, care should be taken to verify all changes are what is intended. The tables below indicate the parameters that can be set for each property set of the design domain. Any parameter set on this form overrides any global setting of that parameter that may be defined under the Objective & Constraints form or the Optimization Control form. For more information on each parameter, the user is directed to the MSC Nastran Quick Reference Guide. Topology Parameters:
Frac Mass Target (FRMASS)
Description: (all values written to the TOPVAR entry unless otherwise indicated) The fraction mass target for the specified property set. The initial value is picked up from the setting on the Objectives & Constraints form. If one of these cells is set, all rows must be set. You can remove the values from all rows and the value from the Objectives & Constraints form will be used. Otherwise these values override the value from the Objectives and Constraints form. Values in these cells are also written the corresponding DCONSTR/DRESP1 entries with FRMASS option as well as the TOPVAR entry.
468
Patran Interface to MD Nastran Preference Guide Toptomize
Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Lower Bounds (XLB)
Lower Bounds. The original value is picked up from the setting on the Optimization Control form. Typically these cells are blank by default. If one of these cells is set, all rows must be set. You can remove the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Manufacturing Constraints:
These are accessed from the Manufacturing Constraints form.
Ref. Coordinate System Minimum Member Size Symmetric Constraints Extrusion Constraints Casting Constraints
Topometry Parameters:
Any direction, plane, or axis specified for the constraints will be in the Reference Coordinate Frame specified. By default all constraints are off. You may turn any on that are applicable. Some combinations are not possible in Nastran and the interface should indicate if an incompatible combination is selected. Note that all of these values can differ for each selected design domain from the Design Domain form (bottom spreadsheet). By selecting a row from the spreadsheet, you can see the settings change on the Manufacturing Constraints form if there are differences. If multiple rows are selected, only the settings for the top row are displayed on the Manufacturing Constraints from. If a change is made to a value with multiple rows selected, the new value is associated to all the selected property sets. If no property sets are selected, it is the same as if all are selected. So care should be taken when changing values on this form to ensure only the property sets of interest are being affected.
Description: (all values written to the TOMVAR entry unless otherwise indicated)
Property to Optimize (PNAME)
The property to optimize. The original value is picked up from the setting on the Optimization Control form. If one of these cells is set, all rows must be set. You can clear the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Initial Design (XINIT)
Initial Value on the property value to optimize. Operates similar to Property to Optimize above.
Lower Bounds (XLB)
Lower Bounds on the property value to optimize. Operates similar to Initial Value above
Upper Bounds (ULB)
Upper Bound on the property value to optimize. Operates similar to Lower Bound above.
Manufacturing Constraints:
Not supported for Topometry.
Chapter 3: Running an Analysis 469 Toptomize
Topography Parameters:
Description: (all values written to the BEADVAR entry unless otherwise indicated)
Minimum Bead Width (MW)
Minimum bead width. The original value is picked up from the setting on the Optimization Control form. If one of these cells is set, all rows must be set. You can clear the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Maximum Bead Height (MH)
Maximum bead height. Operates similar to Minimum Bead Width.
Draw Angle (ANG)
Draw angle in degrees. Operates similar to the above parameters.
Lower Bounds (XLB)
Lower bound on the bead height. Operates similar to the above parameters.
Upper Bounds (XUB)
Upper bound on the bead height. Operates similar to the above parameters.
Buffer Zone (BF)
Buffer zone. Operates similar to the above parameters.
Exclude from Design (SKIP)
Boundary skip. Operates similar to the above parameters.
Manufacturing Constraints:
These are accessed from the Manufacturing Constraints form.
Ref. Coordinate Frame Extrusion Direction Nodes to Exclude/Include
Any vector specified for the draws direction of the beads will be in the Reference Coordinate Frame specified. By default the Extrusion Direction is Normal to the surface. If Vector is specified, a user defined vector can be specified in any acceptable manner with the select mechanism. Optionally the user may select a group of nodes to include or exclude from the design domain. Note that all of these values can differ for each selected design domain from the Design Domain form (bottom spreadsheet). By selecting a row from the spreadsheet, you can see the settings change on the Manufacturing Constraints form if there are differences. If multiple rows are selected, only the settings for the top row are displayed on the Manufacturing Constraints from. If a change is made to a value with multiple rows selected, the new value is associated to all the selected property sets. If no property sets are selected, it is the same as if all are selected. So care should be taken when changing values on this form to ensure only the property sets of interest are being affected.
Postprocessing Postprocessing topology optimization results requires that you read element density values (the new mesh from optimization) using the Nastran results .xdb file (e.g. jobname.xdb) or .des file (e.g. jobname.des) through the Tools | Design Study | Postprocessing menu and use that application to view the results rather than through the Patran Results application. See Tools>Design Studies>PostProcess (p. 546) in the Patran Reference Manual.
470
Patran Interface to MD Nastran Preference Guide Interactive Analysis
3.17
Interactive Analysis The Patran Preference for MD Nastran has a new capability that enables the user to perform visual interactive modal frequency response analysis. The process begins by creating a good modal analysis solution with MD Nastran. The interactive modal frequency response solution is then directed from a special set of Patran menus (wizard). The wizard assists the user in applying the desired loads, specifying damping, selecting result entities, and defining solution criteria for an automated fast restart in Nastran effected from the modal database selected. Patran running as the client spawns a fast restart job to Nastran functioning as a server. Solution results are automatically returned to the client for visualization. This procedure suggests that there might be several benefits to using this product. The wizard provides a guide for problem definition, minimizing confusion associated with general-purpose menu structures. The fast restart, as the name suggests, is fast, and is executed automatically, as are the client-server connections and the data transmission. The reduced solution space of the fast restart minimizes the amount of result data that is calculated, stored, transmitted, and displayed. The net result is the ability to quickly apply discrete loads to the structure and immediately visualize the response at select grids or elements of the model. The real time solution paradigm of the interactive scheme does not provide fringe or contour plots of the global structural response. Assumptions Interactive modal frequency response requires that a normal modes analysis of the structure has been completed using Nastran, and that a .DBALL/MASTER database exists containing the model data and the normal modes solution. Currently, the interactive paradigm presumes the Nastran executable, the modal database, and the Patran executable are all located in the same directory. To maintain optimal performance, licensing and security should be local also. Given these initial conditions, the following scenarios exist for performing interactive frequency response. Scenario 1 If the initial normal modes analysis was modeled in Patran, then that Patran database should be selected under File/Open when starting Patran. This provides the user with the model from which to exercise the interactive frequency response wizard, provided the correct flag was set to precondition the Nastran normal modes database for this purpose. This is done in Patran by going to Analysis/Solution Type/Interactive Modal Analysis, and activating the check box. Scenario 2 The normal modes model may have been built and run without using Patran. If the user intends to use the MSC integrated product to proceed with interactive frequency response, then special care must be taken when preparing the NASTRAN input file for the normal modes analysis. Specifically, the Nastran normal modes input file must contain the following statement just before the CEND delimiter: include `SSSALTERDIR:run0.V2001` Note that both “ticks” are right handed and that SSSALTERDIR must be capitalized. Nastran then creates an environment variable called SSSALTERDIR which points to where the sssalters are located when performing a standard installation.
Chapter 3: Running an Analysis 471 Interactive Analysis
If the user does not have a standard Nastran installation, then he will be required to specify the full directory path. For example, if the file run0.V2001 is located in the directory /scr2/mike/tmp, then he must include the following statement just prior to the CEND delimiter: include `/scr2/mike/tmp/run0.V2001` This include statement provides the DMAP alter required to precondition the large modal database. This conditioning enables efficient data manipulation during the interactive frequency response solution phase. Under this scenario, the model data will need to be imported by starting Patran and requesting “Read Input File” from the Analysis Menu. This procedure is described in greater detail in Chapter 5 of this user’s guide, and constitutes reading a NASTRAN Input File for the model data. Once the model data is placed in the Patran database, interactive frequency response can proceed. The Process Scenario 1 or 2 above can be followed to provide a Patran database with a data model suitable for performing interactive frequency response. The Analysis menu shown below controls the interactive analysis process. Submenus for Select NASTRAN .DBALL, Create Loading, Output Requests, Create a Field, and Define Frequencies are discussed. Solution Type--Is currently fixed to Frequency Response (Modal Frequency Response) as the only solution available in interactive analysis format. Subsequent versions of Nastran and Patran may expand this capability to other solution types. Loading Menu--The loading menu provides a spreadsheet to guide the user through load and boundary condition application. Miscellaneous The Interactive Modal Frequency response solution process is staged, in the sense that a normal mode solution is performed first to create what we refer to as the large database (so named for obvious reasons), and then a fast restart procedure is used to develop the frequency response. The normal modes solution is where the user specifies any weight to mass conversion quantities (see PARAM, WTMASS) as well as a specification of the mass matrix formulation desired (see PARAM, COUPMASS). The mass units and desired mass matrix formulation then, are automatically accounted for in the subsequent determination of the frequency response quantities calculated.
472
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Analysis Form
Every interactive solution will have a user assigned job name associated with it. This provides a record of applied loads, enforced motion boundary conditions, solution frequencies requested, structural damping definition, and output request entities. In a Nastran sense, each job represents a “loading condition” which reflects application of a number of loads and load types distributed on the structure. Maintaining a record of the interactive run provides a starting point for subsequent analyses whether they are done in the current session, or a subsequent session. Specifically, if a user wanted to change only a frequency dependent load function or damping function, the interactive job storage capacity makes this a simple procedure.
Each Interactive Analysis will have its solution specifications stored with a job name (Interactive Name). This allows recovery of all specifications required for performing that particular analysis : loading, damping, solution frequencies, and output entities. If an existing Interactive Job is selected, those input requirements automatically populate the interactive menus. If we want to rerun that analysis, all that is required is to hit APPLY on the Analysis Menu. When the calculations are finished in Nastran, the interactive system automatically positions the user in the Interactive Results section where XY plot requests can be made. Plot requests are not saved in the jobs data.
Load types include: Acoustic (Pressure), Force, Displacement, Velocity, or Acceleration.
Chapter 3: Running an Analysis 473 Interactive Analysis
Select Modal Results .DBALL The following form appears when you select Select Nastran .DBALL from the Analysis form. This form provides the pointer to the Nastran database which contains the preconditioned normal modes solution. Some additional data is retrieved from this database for use in Patran. Specifically, the Nastran modal constraint data is provided to Patran to guarantee that the allowable degrees of freedom available for enforced motion are exposed in the Loading Menu. (Application of enforced motion in modal frequency response requires that the effected degrees of freedom were constrained in the normal modes analysis.)
474
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Loading Form This form allows you to create loading sets. The following is the default form.
Load types include: Acoustic (Pressure), Force, Displacement, Velocity, or Acceleration.
The following shows the Loading Form filled out with a few different load conditions. If Load Type = Acoustic, Load Entity can only reference elements and the default direction for the load application is relative to the element normal regardless of the Coord Frame selection. The Basic coordinate system is the default reference (COORD 0), unless, the element was defined in a local coordinate system, in which case that Coord ID will appear in the Coord Frame column. If the user changes the Direction from NORMAL to a specific direction vector, then the applied pressure direction is relative to the Coord Frame referenced. If Load Type = Force, Load Entity can only reference nodes (grid points), and a direction vector is input to define application direction relative to the coordinate frame reference. If no coordinate reference frame is specified, the default becomes the Basic Coordinate system (Coord 0). If Load Type = Displacement, Velocity, or Acceleration, Load Entity can only be selected from nodes that will appear in the Load Entities list box. These nodes represent the set of all possible nodes to which enforced motion can be applied, and is limited to nodes that were constrained during the normal modes analysis. The Basic coordinate system is the default reference (COORD 0), unless, the node was defined in a local coordinate frame, in which case that Coord ID will appear in the Coord Frame column. When Load Type = Displacement, Velocity, or Acceleration, and a specific node has been selected in Load Entities, the Direction specification will indicate which directions are available X, Y, and / or Z in
Chapter 3: Running an Analysis 475 Interactive Analysis
the reference coordinate frame. When an enforced motion is defined for a selected degree of freedom, it is eliminated from the available enforced motion set. Only one enforced motion boundary condition per degree of freedom can be applied to a given node. (Enforced motion cannot be applied to rotational degrees of freedom for interactive analysis).
476
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Create a Field Form This form appears when you select the Create New Field/Table... button from the Loading Form.
Chapter 3: Running an Analysis 477 Interactive Analysis
Output Selection Form This form will allow the user to select nodes and elements for output, and allow him to select the frequencies which interest him in the analysis. The frequency selection form is the same form that is used in standard analysis for sol 111 subcase parameters.
Define Frequencies prompts a spreadsheet for defining the desired solution frequencies for which output will be available. Output Selection also provides for selecting Nodes / Grids and Elements for which output response is desired. Selection can be made to create output response for complex quantities in either Real / Imaginary or Magnitude / Phase formats. For Interactive Analysis, the output quantities are preset. Close the Output Selection menu.
Define Frequencies Form This form allows the user to define the frequencies of interest in the most complete way. This form allows the users access to FREQ, FREQ1, FREQ2, FREQ3, FREQ4, FREQ5.
478
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Chapter 4: Read Results Patran Interface to MD Nastran Preference Guide
4
Read Results
Accessing Results
492
Supported OUTPUT2 Result and Model Quantities
Supported T16/T19 Results Quantities
Supported MSC.Access Result Quantities
Supported 3dplot Results Quantities
511
543
516
502
492
Patran Interface to MD Nastran Preference Guide Accessing Results
4.1
Accessing Results This form appears when the Analysis toggle is selected on the main menu and the Action is set to Access Results. The Object you select defines the type of results file to be read or accessed from the analysis. The following file types are available: XDB, Output2, MASTER, T16/T19 and 3dplot (for SOL 700). The Method choices are: Result Entities, Model Data, or Both.
When the Object selected is Result Entities, the model data must already exist in the database. No results can be read into Patran if the associated node or element does not already exist. Model Data only reads the model data that exists in the results file. Both will first read the model data, then the result entities. If Model Data or Both are selected, it is up to the user to ensure that there will not be any ID conflicts with existing model entities.
Defines the job name to be used for this job. The same job name used for the Analysis menu should be used for the Read Results menu. This will allow Patran to load the results directly into the load cases that were used for the analysis.
Defines the results file to be read. The form that is called up lists all files recognized as being analysis code results files. By default this is all files with an op2 extension on them. This can be changed with the filter. If you are attaching a T16/T19 file that has the same jobname as your current database, you do not have to select the file. Patran automatically attaches the T16/T19 file that matches the database jobname. Defines any parameters used to control the results or model translation from the analysis code results file.
Chapter 4: Read Results 493 Accessing Results
Results File Formats Output2 Formats The Patran MD Nastran interface supports several different OUTPUT2 file formats. The interface, running on any platform can read a binary format OUTPUT2 file produced by MSC. Nastran running on any of these same platforms. For example, a binary OUTPUT2 file produced by MD Nastran running on an IBM RS/6000 can be read by Patran running on DEC Alpha. Patran may be able to read binary format OUTPUT2 files from other platforms if they contain 32 bit, IEEE format entities (either Big or Little Indian). For platforms that do not produce OUTPUT2 files in these formats, Patran MD Nastran can read OUTPUT2 files created with the FORM=FORMATTED option in MD Nastran. This option can be selected from the Analysis/Translation Parameters form in Patran and directs MD Nastran to produce an ASCII format OUTPUT2 file that can be moved between any platforms. The Patran MD Nastran interface detects this format when the OUTPUT2 file is opened, automatically converts it to the binary format, and then reads the model and/or results into the Patran database. An OUTPUT2 file is created by MD Nastran by placing a PARAM,POST,-1 in the bulk data portion of the input file. The formatted or unformatted OUTPUT2 file is specified in the FMS section using an ASSIGN OUTPUT2 = filename, UNIT=#, FORM=FORMATTED (or UNFORMATTED). See Translation Parameters, 265. XDB Formats The same basic issues exist for MSC.Access databases as for OUTPUT2 files. For example, the MSC.Access database (xdb file) may be exchanged between computer Systems that have binary compatibility. That is, an XDB file generated on a SUN Machine may be used on an IBM/AIX, HPUX or SGI computers. However, in order to exchange the XDB file on binary incompatible machines, one needs to use the TRANS and RECEIVE utilities delivered with every installation of MD Nastran. TRANS converts an XDB file generated by MD Nastran to an “equivalent” character, i.e. ASCII, file which can be transported to another computer across the network via ftp or rcp. RECEIVE converts the character file back into the XDB format for postprocessing. For more information on TRANS and RECEIVE utilities, please consult the “Configuration and Operations Guide” for V70 of MSC.Nastran. A MSC.Access XDB database is created by MD Nastran by placing a PARAM,POST,0 in the bulk data portion of the input file. See Translation Parameters, 265. In this release of the product, it is assumed that the Geometry, loads and results output all reside in the same physical XDB file. That is, "split" XDB databases are not supported.
494
Patran Interface to MD Nastran Preference Guide Accessing Results
MASTER Formats Using the MASTER format, you can attach to the MD Nastran database directly saving the extra step of creating alternate form of MD Nastran model and results data, i.e. OP2 and/or XDB. Because the model and results data in the MD Nastran database tends be sequential in nature, an index provides fast “direct” access to the data. The indexing is accomplished by two indexing modules in MD Nastran named: ifpindx and ofpindx. The DRA/DBALL capability uses the MD Nastran toolkit, i.e. MNT, capability. The MNT interfaces with the MD Nastran executable in a client-server. This means that in order to use the DRA/DBALL feature one needs to have access to MD Nastran installation. If you do not have access to a MD Nastran installation you will need to use the MD Nastran mini server that is delivered with Patran to import DRA/DBALL files. To point to a MD Nastran installation, the location of the MD Nastran executable is set in the following files: p3_trans.ini(NT), .site_setup(UNIX,LINUX). On Windows NT, the “ACommand20xx” must be set to the MD Nastran executable. On UNIX, on the other hand, “MSP_NASTRAN_CMD20xx” needs to be set to the MD Nastran executable. To point to a MD Nastran mini server, the location of the MD Nastran mini server executable must be set on Windows with the “AcommandNasServer” environment variable. On UNIX, you must set the environment variable “MSCP_NASTRAN_SERVER” . By default the MD Nastran mini server is located in $P3_Home/mscnastran_files/servermode/nastran.exe. Note that you are required to point to a V2004 or later version of MD Nastran. If you specify an MSC.Nastran executable earlier than V2004 you will be presented with a modal form preventing you from using this capability. However, you may bypass this restriction by setting the “DRA_NAST_NOVEDRCHK” environment variable. The DRA/MASTER functionality only supports static analysis (SOL101). This includes the support of Superelements, grid point forces and other result types available in the OP2 or XDB translators. This capability supports importing the model data into Patran database. Moreover, since this capability reuses the import/bdf functionality all of the model information available in the database shall be imported including Nodes, Elements, Coordinate systems, material properties, physical properties, loads and boundary conditions, load cases, parameters and etc... The “indexing” modules are tied to a system cell. That is, an MD Nastran database is indexed and saved by MD Nastran by setting system cell “316” to a value “7”. This system cell tells MD Nastran executable to create index files for IFP and OFP datablocks and move the indexed datablocks to the “MASTER” file. This means that one can even delete the “DBALL” file after the MD Nastran run completes. For example, if you would like to get an Indexed MASTER data file for the job some_job.bdf, the following must be executed: < ...>/nastran some_job.bdf sys316=7 scr=no sdir=/tmp This example generates a “some_job.MASTER and some_job.DBALL database files. You can delete the *.DBALL file because it does not contain any results or model data of importance. However, if you would like to perform a restart from the run then the DBALL file must be kept for future use but the “Master” file may be moved to other directories at will.
Chapter 4: Read Results 495 Accessing Results
The MD Nastran toolkit environment is derived from the MD Nastran installation via the use of the “rc” files which is documented in the MSC.Nastran (p. 1) in the MSC.Nastran 2004 Installation and Operations Guide. For example, you can set the amount of memory used by the MD Nastran to 20 megawords by setting the “memory=20MW” in one of the “rc” files, i.e. nastran.rcf file in the current working directory on the NT platform. This setting can be double checked using the MD Nastran “whence” command as follows: < ...>/nastran some_job.bdf whence=mem The same basic issues exist for attaching to an Indexed MD Nastran database as attaching an XDB database. That is, the MD Nastran database (MASTER file) may be exchanged among computer Systems that have binary compatibility. That is, a MASTER file generated on a SUN Machine can not be used on an IBM/AIX, HPUX or SGI computers. However, at this time it is not possible to exchange the MASTER file on binary incompatible machines. T16/T19 Formats The T16 file is the MSC.Marc binary results file and the T19 file is the MSC.Marc ASCII results (POST) file that are created by a SOL 600 analysis, the contents of which can be imported or attached for postprocessing. When domain decomposition is used, multiple files are produced where # is the domain number. This file format is recommended for post-processing SOL 600 runs since it has more information, such as contact info and additional nonlinear analysis information, then the xdbor OP2 formats. These results file types are used for accessing SOL 600 results. 3dplot Formats The 3dplot ptf file is the LS-Dyna binary results file that are created by a SOL 700 analysis, the contents of which can be attached for postprocessing. This option is available only for Explicit Nonlinear.
496
Patran Interface to MD Nastran Preference Guide Accessing Results
Translation Parameters OUTPUT2 This subordinate form appears when the Translation Parameters button is selected and Read Output2 is the selected Object. When reading results there are three Method options that may be selected: Result Entities, Model Data or Both. This form affects import of all these objects as noted below
Tolerances • Division • Numerical
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available.
Chapter 4: Read Results 497 Accessing Results
MSC.Nastran Version
Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation.
• P-element P-order Field
Creates a field that describes the polynomial orders in all p-elements in the model at the end of an adaptive cycle.
Element Results Positions
If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
Defining Translation Parameters for DDAM (SOL 187) Patran calculates combined stresses (like bar stresses, principal stresses and von Mises stresses by default, rather than reading these values from the OP2 files. If Patran does this, the combined stresses will be incorrectly calculated from summed results. It is necessary to calculate the combined stresses on a mode-by-mode basis, and NRL sum the combined results. To obtain correct results, it is necessary to explicitly tell Patran to read the combined values. Select the Translation Parameters button on the Analysis form when reading results in. On the form, you can select the box labeled Stress/Strain Invariants. This produces a number of additional results for each result case. These additional results are the correct von Mises and Principal stresses. The ones that Patran displays when you choose Stress Tensor are the incorrect values.
498
Patran Interface to MD Nastran Preference Guide Accessing Results
XDB This subordinate form appears when the Translation Parameters button is selected and Result Entities is the selected Object.
Tolerances • Division • Numerical
MSC.Nastran Version
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available. Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Chapter 4: Read Results 499 Accessing Results
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Element Results Positions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation. If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
MASTER This subordinate form appears when the Translation Parameters... button is selected and MASTER is the selected Object.
500
Patran Interface to MD Nastran Preference Guide Accessing Results
Tolerances • Division • Numerical
MSC.Nastran Version
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available. Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation.
• P-element P-order Field
Creates a field that describes the polynomial orders in all p-elements in the model at the end of an adaptive cycle.
Element Results Positions
If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
Chapter 4: Read Results 501 Accessing Results
T16/T19 This subordinate form appears when the Translation Parameters... button is selected and T16/T19 is the selected Object.
Model Import Options • Create Groups by PIDs
Creates groups for each element type encountered in the model.
• Geometry Import
Imports any NURB based rigid geometry found in the POST file into the database.
Select Mesh
Pertains to importing results and model data from adaptive meshing analyses. In order for this toggle to be active, a results file must have been selected first in which case it is scanned to show the available meshes and to which load increments they are associated. You can select which meshes/increments are imported in the provided list box. Adaptive meshing is not supported in MSC.Nastran 2004.
Available Increments
Defines the increments available for import from the results file.
502
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
4.2
Supported OUTPUT2 Result and Model Quantities The following table indicates all the possible results quantities that can be loaded into the Patran database during results translation from MD Nastran. The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor, and determines which postprocessing techniques are available to view the results quantity. Data Block indicates which MD Nastran OUTPUT2 data block the data comes from. The Description gives a brief discussion about the results quantity, such as if it is only for certain element types, and what Output Request selection will generate this data block. For design optimization, all of the listed results can be loaded as a function of design cycle. Results
Primary Label
Secondary Label
Type
DataBlocks
Description
Acoustic
Intensity
Scalar
OAIG1
Acoustic intensity on surface in contact with fluid.
Acoustic
Radiated Power
Scalar
OARPWR1
Acoustic power radiated from surface in contact with fluid.
Acoustic
Field Point Mesh
Vector
OUGFP1
Acoustic results for Field Point Mesh.
Acoustic
Velocity @ FPM Grids
Vector
OVGFP1
Acoustic velocities at the node points of Field Point Mesh.
Bar Forces
Rotational
Vector
OEF1
Bar moments
Translational
Vector
OEF1
Bar forces
Warping Torque
Scalar
OEF1
Warping torque
Axial Safety Margin
Scalar
OSTR1
Axial safety margin
Compression Safety Margin
Scalar
OSTR1
Safety margin in compression
Maximum Axial
Scalar
OSTR1
Maximum axial strain
Minimum Axial
Scalar
OSTR1
Minimum axial strain
Tension Safety Margin
Scalar
OSTR1
Safety margin in tension
Torsional Safety Margin
Scalar
OSTR1
Safety margin in torsion
Axial Safety Margin
Scalar
OES1
Axial safety margin
Compression Safety Margin
Scalar
OES1
Safety margin in compression
Maximum Axial
Scalar
OES1
Maximum axial stress
Minimum Axial
Scalar
OES1
Minimum axial stress
Tension Safety Margin
Scalar
OES1
Safety margin in tension
Torsional Safety Margin
Scalar
OES1
Safety margin in torsion
Bar Strains
Bar Stresses
Chapter 4: Read Results 503 Supported OUTPUT2 Result and Model Quantities
Primary Label Grid Point Stresses
Secondary Label
Type
DataBlocks
Description
Stress Tensor
Tensor
OGS1
Stress tensor
Zero Shear Angle
Scalar
OGS1
Zero shear angle
Major Principal
Scalar
OGS1
Major principal
Minor Principal
Scalar
OGS1
Minor principal
Maximum Shear
Scalar
OGS1
Maximum shear
von Mises
Scalar
OGS1
von mises
Displacement
Vector
OEF1 or OES1
Gap element displacement
Force
Vector
OEF1 or OES1
Gap element force
Slip
Vector
OEF1 or OES1
Gap element slip
Creep Strain
Scalar
OESNL1
Creep strain
Plastic Strain
Scalar
OESNL1
Plastic strain
Strain Tensor
Tensor
OESNL1
Strain tensor
Nonlinear Stresses
Equivalent Stress
Scalar
OESNL1
Equivalent stress
Stress Tensor
Tensor
OESNL1
Stress tensor
Principal Strain Direction
1st Principal x cosine
Scalar
OSTR1
1st Principal x cosine
1st Principal y cosine
Scalar
OSTR1
1st Principal y cosine
1st Principal z cosine
Scalar
OSTR1
1st Principal z cosine
2nd Principal x cosine
Scalar
OSTR1
2nd Principal x cosine
2nd Principal y cosine
Scalar
OSTR1
2nd Principal y cosine
2nd Principal z cosine
Scalar
OSTR1
2nd Principal z cosine
3rd Principal x cosine
Scalar
OSTR1
3rd Principal x cosine
3rd Principal y cosine
Scalar
OSTR1
3rd Principal y cosine
3rd Principal z cosine
Scalar
OSTR1
3rd Principal z cosine
Zero Shear Angle
Scalar
OSTR1
Zero shear angle
Gap Results
Nonlinear Strains
504
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Principal Stress Direction
Shear Panel Forces
Shear Panel Strains
Shear Panel Stresses
Shell Forces
Secondary Label
Type
DataBlocks
Description
1st Principal x cosine
Scalar
OES1
1st Principal x cosine
1st Principal y cosine
Scalar
OES1
1st Principal y cosine
1st Principal z cosine
Scalar
OES1
1st Principal z cosine
2nd Principal x cosine
Scalar
OES1
2nd Principal x cosine
2nd Principal y cosine
Scalar
OES1
2nd Principal y cosine
2nd Principal z cosine
Scalar
OES1
2nd Principal z cosine
3rd Principal x cosine
Scalar
OES1
3rd Principal x cosine
3rd Principal y cosine
Scalar
OES1
3rd Principal y cosine
3rd Principal z cosine
Scalar
OES1
3rd Principal z cosine
Zero Shear Angle
Scalar
OES1
Zero shear angle
Force12
Scalar
OEF1
Shear force from nodes 1 to 2
Force14
Scalar
OEF1
Shear force from nodes 1 to 4
Force21
Scalar
OEF1
Shear force from nodes 2 to 1
Force23
Scalar
OEF1
Shear force from nodes 2 to 3
Force32
Scalar
OEF1
Shear force from nodes 3 to 2
Force34
Scalar
OEF1
Shear force from nodes 3 to 4
Force41
Scalar
OEF1
Shear force from nodes 4 to 1
Force43
Scalar
OEF1
Shear force from nodes 4 to 3
Kick
Scalar
OEF1
Kick forces
Rotational
Vector
OEF1
Moments at nodes
Shear
Scalar
OEF1
Shear force in panel
Translational
Vector
OEF1
Forces at nodes
Average Shear
Scalar
OSTR1
Average shear strain in panel
Maximum Shear
Scalar
OSTR1
Maximum shear strain in panel
Safety Margin
Scalar
OSTR1
Shear safety margin of panel
Average Shear
Scalar
OES1
Average shear stress in panel
Maximum Shear
Scalar
OES1
Maximum shear stress in panel
Safety Margin
Scalar
OES1
Shear safety margin of panel
Force Resultant
Tensor
OEF1
Force resultants and moment resultants
Moment Resultant
Tensor
OEF1
Moment stress resultants
Chapter 4: Read Results 505 Supported OUTPUT2 Result and Model Quantities
Primary Label Strain Curvatures
Secondary Label
Type
DataBlocks
Description
Strain Tensor
Tensor
OSTR1
Strain curvatures of a plate
1st Principal
Scalar
OSTR1
Curvature of strain 1st principal
2nd Principal
Scalar
OSTR1
Curvature of strain 2nd principal
Maximum Shear
Scalar
OSTR1
Curvature of maximum shear strain
von Mises
Scalar
OSTR1
Curvature of von Mises strain
Zero Shear Angle
Scalar
OSTR1
Curvature of zero shear angle
Energy
Scalar
ONRGY1
Element’s total strain energy
Energy Density
Scalar
ONRGY1
Element’s strain energy density
Percent of Total
Scalar
ONRGY1
Element’s percentage of total strain density
1st Principal
Scalar
OSTR1
Strain 1st principal
2nd Principal
Scalar
OSTR1
Strain 2nd principal
3rd Principal
Scalar
OSTR1
Strain 3rd principal
Maximum Shear
Scalar
OSTR1
Maximum shear strain
Mean Pressure
Scalar
OSTR1
Mean strain pressure
Octahedral Shear
Scalar
OSTR1
Octahedral shear strain
von Mises
Scalar
OSTR1
von Mises equivalent strain
Strain Tensor
NONE
Tensor
OSTR1
Strain tensor
Stress Invariants
1st Principal
Scalar
OES1
Stress 1st Principal
2nd Principal
Scalar
OES1
Stress 2nd Principal
3rd Principal
Scalar
OES1
Strain 3rd Principal
Maximum Shear
Scalar
OES1
Maximum shear stress
Mean Pressure
Scalar
OES1
Mean stress principal
Octahedral Shear
Scalar
OES1
Octahedral shear stress
von Mises
Scalar
OES1
von Mises equivalent stress
Stress Tensor
NONE
Tensor
OES1
Stress tensor
Accelerations
Rotational
Vector
OUGV1
Nodal angular accelerations
Translational
Vector
OUGV1
Nodal translational accelerations
Rotational
Vector
OPG1
Nodal equivalent applied moments
Translational
Vector
OPG1
Nodal equivalent applied forces
Strain Energy
Strain Invariants
Applied Loads
506
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Constraint Forces
Displacements
Eigenvectors Nonlinear Applied Loads
Secondary Label
Type
DataBlocks
Description
Rotational
Vector
OQG1
Nodal moments of single-point constraints
Translational
Vector
OQG1
Nodal forces of single-point constraint
Rotational
Vector
OUGV1
Nodal rotational displacements
Translational
Vector
OUGV1
Nodal translational displacements
Rotational
Vector
OPHIG
Nodal rotational eigenvectors
Translational
Vector
OPHIG
Nodal translational eigenvectors
Rotational
Vector
OPNL1
Nodal nonlinear applied moments
Chapter 4: Read Results 507 Supported OUTPUT2 Result and Model Quantities
Primary Label
Secondary Label
Type
DataBlocks
Description
Translational
Vector
OPNL1
Nodal nonlinear applied forces
Rotational
Vector
OUGV1
Nodal angular velocity
Translational
Vector
OUGV1
Nodal translational velocity
Error
Estimate
Scalar
ERROR
Elemental error in adaptive analysis
Grid Point Forces
Elements
Vector
OGPFB1*
Internal nodal force contribution by element
Applied Loads
Vector
OGPFB1*
Nodal equivalent applied forces
Constraint Forces
Vector
OGPFB1*
Nodal equivalent constraint forces
Total
Vector
OGPFB1*
Total nodal equivalent forces due to internal loads, applied loads and constraint forces.
Elements
Vector
OGPFB1*
Internal nodal moment contribution by element
Applied Loads
Vector
OGPFB1*
Nodal equivalent applied moments
Constraint Forces
Vector
OGPFB1*
Nodal equivalent constraint moments
Total
Vector
OGPFB1*
Total nodal equivalent moments due to internal loads, applied loads and constraint forces.
None
Vector
GEOMIN
In a shape optimization run, this is the new shape displayed as a deformation of the original shape.
Velocities
Grid Point Moments
Shape Change
508
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Active Constraints
Secondary Label
Type
DataBlocks
Description
Element Stress
Scalar
R1TABRG
Element stress
Element Strain
Scalar
R1TABRG
Element strain
Element Force
Scalar
R1TABRG
Element force
Element Ply Failure
Scalar
R1TABRG
Element ply failure
Translational Displacement
Vector
R1TABRG
Nodal translational displacement
Rotational Displacement
Vector
R1TABRG
Nodal rotational displacement
Translational Velocity
Vector
R1TABRG
Nodal translational velocity
Rotational Velocity
Vector
R1TABRG
Nodal rotational velocity
Translational Acceleration
Vector
R1TABRG
Nodal translational acceleration
Rotational Acceleration
Vector
R1TABRG
Nodal rotational acceleration
Translational SPC
Vector
R1TABRG
Nodal translational SPC force
Rotational SPC
Vector
R1TABRG
Nodal rotational SPC force
Global Variables In addition to standard results quantities, a number of Global Variables can be created. This table outlines Global Variables that may be created. Global Variables are results quantities where one value is representative of the entire model. Labels
Type
DataBlocks
Description
Critical Load Factor
S
Oxxx
Value of buckling load for the given buckling mode.
Time
S
Oxxx
Time value of the time step.
Frequency
S
Oxxx
Frequency value of the frequency step or for the normal mode.
Damping Ratio
S
Oxxx
Damping ratio value of a complex eigenvalue analysis.
Eigenvalue
S
Oxxx
Eigenvalue for normal modes or complex eigenvalue analysis.
Percent of Load
S
Oxxx
Percent of load value for a nonlinear static analysis.
Adaptive Cycle
S
Oxxx
Cycle number in p-adaptive analysis.
Design Cycle
S
Oxxx
Cycle number in an optimization run (SOL 200).
Design Variable
S
DESTAB HISADD
Design Variable for optimization (Label from DESTAB, value from HISADD).
Maximum Constraint Value
S
HISADD
Maximum constraint value for optimization.
Objective Function
S
HISADD
Objective function for optimization.
Chapter 4: Read Results 509 Supported OUTPUT2 Result and Model Quantities
Coordinate Systems In some cases, the elemental stresses and strains are transformed from one coordinate frame to another when imported into the Patran database. The following describes the coordinate systems for these element results after they are imported into the Patran database. The coordinate system names referred to are described in the Patran or the MD Nastran documentation. CTRIA3
Table 4-1 Results are in the MD Nastran system which coincides with the Patran IJK system. At the user’s request during postprocessing, these results can be transformed by Patran to alternate coordinate systems. If the user selects a component of a stress or strain tensor to be displayed, by default, the Results application transforms the tensor to a projected global system (Projected Global System).
CQUAD4
Table 4-2 Results are in the MD Nastran “bisector” coordinate system but may be transformed by Patran to alternate coordinate systems (e.g., global) during postprocessing. If the user selects a component of a stress or strain tensor to be displayed, by default, the Results application transforms the tensor to a projected global system (Projected Global System). Import of results when this element is used in a hyperelastic analysis is not currently supported.
CHEXA, CPENTA, CTETRA
Table 4-3 The user can request that MD Nastran compute element results in either a local element or alternate coordinate system via the PSOLID entry. If the element results are in the local element system, these are converted to the Patran IJK system on import. If the results are in a system other than local element, they are imported in this system. These results may be transformed to alternate systems during postprocessing.
CQUAD8, CTRI6
Table 4-4 The elemental coordinate system, used by MD Nastran for results, is described in the MD Nastran documentation. These results are imported into the Patran database “asis”. These results can be postprocessed in Patran using the “As Is” options, but they cannot be transformed to alternate coordinate systems. Projected Global System The projected system is defined as follows. First, the normal to the shell surface is calculated. This varies for curved elements and is constant for flat elements. If the angle between the normal and the global xaxis is greater than .01 radians, the global x-axis is projected onto the shell surface as the local x-axis. If the angle is less than .01 radians, either the global y-axis or the z-axis (whichever makes the largest angle with the normal) is defined to be the local x-axis. The local y-axis is perpendicular to the plane defined by the normal and the local x-axis. XY Plots For results from MD Nastran design optimization solution 200 runs, three XY Plots are generated, but not posted, when the Read OUTPUT2 option is selected: 1. Objective Function vs. Design Cycle. 1. Maximum Constraint Value vs. Design Cycle. 1. Design Variable vs. Design Cycle.
510
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
These plots can be viewed under the XY Plot option in (p. 1) in the MSC.Patran User’s Guide. When they are initially posted, you will have to expand their windows to view them properly. Model Data The following table outlines all the data that will be created in the Patran database when reading model data from an MD Nastran OUTPUT2 file and the location in the OUTPUT2 file from where it is derived. This is the only data extracted from the OUTPUT2 file. This data should be sufficient for evaluating results values. Item Nodes
Block GEOM1
Description Node ID Nodal Coordinates Reference Coordinate Frame Analysis Coordinate Frame
Coordinate Frames
GEOM1
Coordinate Frame ID Transformation Matrix Origin Can be Rectangular, Cylindrical, or Spherical
Elements
GEOM2
Element ID Topology (e.g., Quad/4 or Hex20) Nodal Connectivity
Chapter 4: Read Results 511 Supported T16/T19 Results Quantities
4.3
Supported T16/T19 Results Quantities The following table indicates all the possible result quantities which can be loaded into the Patran database from the t16 file. The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor. These types will determine which postprocessing techniques will be available in order to view the results quantity. Postcodes indicates which MSC.Marc element postcodes (selected automatically or by MD Nastran Bulk Data entry MARCOUT) the data comes from. The Description gives a brief discussion about the results quantity. The Output Request forms use the actual primary and secondary labels which 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.
Primary Label
Secondary Label
Type
Postcodes
Description
Displacement
Translation
Vector
1 (nodal)
Translational displacements at nodes from a structural analysis.
Displacement
Rotation
Vector
2 (nodal)
Rotational displacements at nodes from a structural analysis.
Velocity
Translation
Vector
28 (nodal)
Translational velocities at nodes from a dynamic analysis.
Velocity
Rotation
Vector
29 (nodal)
Rotational velocities at nodes.
Acceleration
Translation
Vector
30 (nodal)
Translational accelerations at nodes from a dynamic analysis.
Acceleration
Rotation
Vector
31 (nodal)
Rotational accelerations at nodes from a dynamic analysis.
Force
Nodal External Applied
Vector
3 (nodal)
Forces applied to the model in a structural analysis.
Force
Nodal Reaction
Vector
5 (nodal)
Reaction forces at boundary conditions from a structural analysis.
Moment
Nodal External Applied
Vector
4 (nodal)
Moments applied to the model in a structural analysis.
Moment
Nodal Reaction
Vector
6 (nodal)
Reaction moments at boundary conditions from a structural analysis.
Modal Mass
Translation
Vector
32 (nodal)
Translational modal masses from modal extractions.
Modal Mass
Rotation
Vector
33 (nodal)
Rotational modal masses from modal extractions.
Temperature
Nodal
Scalar
14 (nodal)
Temperature at nodes from a thermal analysis.
Velocity
Fluid
Vector
7 (nodal)
Fluid Velocity
512
Patran Interface to MD Nastran Preference Guide Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Flux
Nodal
Scalar
15 (nodal)
Heat Flux applied to the model in a thermal analysis.
Pressure
Fluid
Scalar
8 (nodal)
Fluid Pressure
Force
External Fluid
Vector
9 (nodal)
External Fluid Force
Force
Reaction Fluid
Vector
10 (nodal)
Reaction Fluid Force
Pressure
Sound
Scalar
11 (nodal)
Sound Pressure
Source
External Sound
Scalar
12 (nodal)
External Sound Source
Source
Reaction Sound
Scalar
13 (nodal)
Reaction Sound Source
Flux
Nodal Reaction
Scalar
16 (nodal)
Nodal Reaction Flux
Potential
Electric
Scalar
17 (nodal)
Electric Potential
Charge
External Electric
Scalar
18 (nodal)
External Electric Charge
Charge
Reaction Electric
Scalar
19 (nodal)
Reaction Electric Charge
Potential
Magnetic
Scalar
20 (nodal)
Magnetic Potential
Current
External Electric
Scalar
21 (nodal)
External Electric Current
Current
Reaction Electric
Scalar
22 (nodal)
Reaction Electric Current
Pressure
Pore
Scalar
23 (nodal)
Pore Pressure
Flux
External Mass
Scalar
24 (nodal)
External Mass Flux
Flux
Reaction Mass
Scalar
25 (nodal)
Reaction Mass Flux
Pressure
Bearing
Scalar
26 (nodal)
Bearing Pressure
Force
Bearing
Scalar
27 (nodal)
Bearing Force
Stress
Contact Normal
Vector
34 (nodal)
Contact Normal Stress
Force
Contact Normal
Vector
35 (nodal)
Contact Normal Force
Stress
Friction
Vector
36 (nodal)
Friction Stress
Force
Friction
Vector
37 (nodal)
Friction Force
Contact
Status
Scalar
38 (nodal)
Contact Status
Contact
Touched Body
Scalar
39 (nodal)
Touched Body Contact
Variable
Herrmann
Scalar
40 (nodal)
Herrmann Variable
Post Code
No. -11 through -16
Tensor
-11 thru -16, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -21 through -23
Vector
-21 thru -23, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -31
Scalar
-31, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Chapter 4: Read Results 513 Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Post Code
No. -41
Scalar
-41, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -51
Scalar
-51, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Strain
Cracking
Tensor
81-86 or 381
Cracking strain from a nonlinear structural analysis.
Strain
Creep
Tensor
31-36 or 331
Creep strain from a nonlinear structural analysis.
Strain
Creep Equivalent
Scalar
37
Equivalent creep strain from a nonlinear structural analysis.
Strain
Creep Equivalent (from rate)
Scalar
8
Equivalent creep strain determined from rate from a nonlinear structural analysis.
Strain
Elastic
Tensor
121-126 or 401
Elastic strain from a structural analysis.
Strain
Elastic Equivalent
Scalar
127
Equivalent elastic strain from a structural analysis.
Strain
Plastic
Tensor
21-26 or 321
Plastic strain from a nonlinear structural analysis.
Strain
Plastic Equivalent
Scalar
27
Equivalent plastic strain from a nonlinear structural analysis.
Strain
Plastic Equivalent (from rate)
Scalar
7
Equivalent plastic strain determined from rate from a nonlinear structural analysis.
Strain
Plastic Equivalent Rate
Scalar
28
Equivalent plastic strain rate from a nonlinear structural analysis.
Strain
Thermal
Tensor
71-76 or 371
Thermal strain from a structural analysis.
Strain
Thickness
Scalar
49
Thickness strain from a structural analysis.
Strain
Total
Tensor
1-6 or 301
Total strain from a structural analysis.
Temperature
Element
Scalar
9
Element temperature from a thermal or structural analysis.
Temperature
Element Gradient
Vector
181-183
Element temperature gradient from a thermal analysis.
Temperature
Element Incremental Scalar
10
Incremental element temperature from a thermal or structural analysis.
Tensor
11-16 or 311
Stress from a structural analysis.
Tensor
41-46 or 341
Cauchy stress from a nonlinear structural analysis.
Stress Stress
Cauchy
514
Patran Interface to MD Nastran Preference Guide Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Stress
Cauchy Equivalent Mises
Scalar
47
Equivalent Cauchy stress from a nonlinear structural analysis.
Stress
Equivalent Mises
Scalar
17
Equivalent (von mises) stress from a structural analysis.
Stress
Hydrostatic
Scalar
18
Hydrostatic stress from a structural analysis.
Stress
Interlaminar Shear No. 1
Scalar
108
Interlaminar shear in one direction from a structural analysis.
Stress
Interlaminar Shear No. 2
Scalar
109
Interlaminar shear in two direction from a structural analysis.
Energy Density
Elastic
Scalar
48
Elastic strain energy density from a structural analysis.
Energy Density
Plastic
Scalar
58
Plastic strain energy density from a nonlinear structural analysis.
Energy Density
Total
Scalar
68
Total strain energy density from a structural analysis.
Flux
Element
Vector
184-186
Element heat flux from a thermal analysis.
State Variable
Second
Scalar
29
Second state variable from a nonlinear thermal or structural analysis.
State Variable
Third
Scalar
39
Third state variable from a nonlinear thermal or structural analysis.
Failure
Index No. 1
Scalar
91
Failure index one from a structural analysis.
Failure
Index No. 2
Scalar
92
Failure index two from a structural analysis.
Failure
Index No. 3
Scalar
93
Failure index three from a structural analysis.
Failure
Index No. 4
Scalar
94
Failure index four from a structural analysis.
Failure
Index No. 5
Scalar
95
Failure index five from a structural analysis.
Failure
Index No. 6
Scalar
96
Failure index six from a structural analysis.
Failure
Index No. 7
Scalar
97
Failure index seven from a structural analysis.
Thickness
Scalar
20
Element thickness from a thermal or structural analysis.
Volume
Scalar
78
Element Volume from a thermal or structural analysis.
Chapter 4: Read Results 515 Supported T16/T19 Results Quantities
In addition to these standard results quantities, several Global Variable results can be created. Global Variables are results quantities where one value is representative of the entire model. The following table defines the Global Variables which may be created. Global Variable Label
Type
Description
Increment
Scalar
Increment of the analysis.
Time
Scalar
Time of the analysis.
Buckling Mode
Scalar
Buckling mode number.
Critical Load Factor
Scalar
Critical load factor for buckling analysis.
Dynamic Mode
Scalar
Dynamic mode number from modal extraction.
Frequency (radians/time)
Scalar
Frequency in radians per unit time for modal extraction.
516
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
4.4
Supported MSC.Access Result Quantities The following tables list the currently supported quantities from the MSC.Access database (xdb file).To get further information on the MSC.Access, i.e. XDB, objects supported in Patran, please use the ddlprt and ddlqry utilities delivered with every installation of MD Nastran. ddlprt is MSC.Access' on-line documentation. ddlqry is MSC.Access’ Data Definition Language (DDL) browser. See “Configuration and Operations Guide” for MSC.Nastran V70. Nodal Results
Primary Label Displacements
Eigenvectors
Velocities
Secondary Label
Type
Objects
Translational
VECTOR
DISPR
Rotational
VECTOR
DISPR
Translational
VECTOR
DISPRI
Rotational
VECTOR
DISPRI
Translational
VECTOR
DISPMP
Rotational
VECTOR
DISPMP
Translational
VECTOR
DISPR
Rotational
VECTOR
DISPR
Translational
VECTOR
DISPRI
Rotational
VECTOR
DISPRI
Translational
VECTOR
DISPMP
Rotational
VECTOR
DISPMP
Translational
VECTOR
VELOR
Rotational
VECTOR
VELOR
Translational
VECTOR
VELORI
Rotational
VECTOR
VELORI
Translational
VECTOR
VELOMP
Rotational
VECTOR
VELOMP
Chapter 4: Read Results 517 Supported MSC.Access Result Quantities
Primary Label Accelerations
Constraint Forces
Applied Loads
Grid Point Stresses
Secondary Label
Type
Objects
Translational
VECTOR
ACCER
Rotational
VECTOR
ACCER
Translational
VECTOR
ACCERI
Rotational
VECTOR
ACCERI
Translational
VECTOR
ACCEMP
Rotational
VECTOR
ACCEMP
Translational
VECTOR
SPCFR
Rotational
VECTOR
SPCFR
Translational
VECTOR
SPCFRI
Rotational
VECTOR
SPCFRI
Translational
VECTOR
SPCFMP
Rotational
VECTOR
SPCFMP
Translational
VECTOR
LOADR
Rotational
VECTOR
LOADR
Translational
VECTOR
LOADRI
Rotational
VECTOR
LOADRI
Translational
VECTOR
LOADMP
Rotational
VECTOR
LOADMP
Stress Tensor
TENSOR
SGSVR
Zero Shear Angle
SCALAR
SGSVR
Major Principal
SCALAR
SGSVR
Minor Principal
SCALAR
SGSVR
Maximum Shear
SCALAR
SGSVR
Von Mises
SCALAR
SGSVR
518
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Grid Point Stresses
Grid Point Strains
Secondary Label
Type
Objects
Stress Tensor
TENSOR
SGVVR
Mean Pressure
SCALAR
SGVVR
Octahedral Shear
SCALAR
SGVVR
Major Principal
SCALAR
SGVVR
Intermediate Principal
SCALAR
SGVVR
Minor Principal
SCALAR
SGSVR
Major Prin x cosine
SCALAR
SGSVR
Intermed Prin x cosine
SCALAR
SGSVR
Minor Prin x cosine
SCALAR
SGSVR
Major Prin y cosine
SCALAR
SGSVR
Intermed Prin y cosine
SCALAR
SGSVR
Minor Prin y cosine
SCALAR
SGSVR
Major Prin z cosine
SCALAR
SGSVR
Intermed Prin z cosine
SCALAR
SGSVR
Minor Prin z cosine
SCALAR
SGSVR
Strain Tensor
TENSOR
EGSVR
Zero Shear Angle
SCALAR
EGSVR
Major Principal
SCALAR
EGSVR
Minor Principal
SCALAR
EGSVR
Maximum Shear
SCALAR
EGSVR
Von Mises
SCALAR
EGSVR
Chapter 4: Read Results 519 Supported MSC.Access Result Quantities
Primary Label Grid Point Strains
GPS discontinunities
Secondary Label
Type
Objects
Strain Tensor
TENSOR
EGVVR
Mean Pressure
SCALAR
EGVVR
Octahedral Shear
SCALAR
EGVVR
Major Principal
SCALAR
EGVVR
Intermediate Principal
SCALAR
EGVVR
Minor Principal
SCALAR
EGSVR
Major Prin x cosine
SCALAR
EGSVR
Intermed Prin x cosine
SCALAR
EGSVR
Minor Prin x cosine
SCALAR
EGSVR
Major Prin y cosine
SCALAR
EGSVR
Intermed Prin y cosine
SCALAR
EGSVR
Minor Prin y cosine
SCALAR
EGSVR
Major Prin z cosine
SCALAR
EGSVR
Intermed Prin z cosine
SCALAR
EGSVR
Minor Prin z cosine
SCALAR
EGSVR
Stress Tensor
TENSOR
SGSDTR
Major Principal
SCALAR
SGSDTR
Minor Principal
SCALAR
SGSDTR
Maximum Shear
SCALAR
SGSDTR
Von Mises
SCALAR
SGSDTR
Error Estimate
SCALAR
SGSDTR
Stress Tensor
TENSOR
SGVDTR
Mean Pressure
SCALAR
SGVDTR
Octahedral Shear
SCALAR
SGVDTR
Major Principal
SCALAR
SGVDTR
Intermediate Principal
SCALAR
SGVDTR
Minor Principal
SCALAR
SGVDTR
Error Estimate Direct
SCALAR
SGVDTR
Error Estimate Principal
SCALAR
SGVDTR
520
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Elem Stress discontinunities Stress Tensor
MPC Constraint Forces
Type
Objects
TENSOR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Major Principal
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Minor Principal
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Maximum Shear
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Von Mises
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Error Estimate
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Stresss Tensor
TENSOR
DHEXVR, DPENVR, DTETVR
Mean Pressure
SCALAR
DHEXVR, DPENVR, DTETVR
Octahedral Shear
SCALAR
DHEXVR, DPENVR, DTETVR
Major Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Intermediate Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Minor Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Error Estimate Direct
SCALAR
DHEXVR, DPENVR, DTETVR
Error Estimate Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Translational
VECTOR
MPCFR, MPCFRI, MPCFMP
Rotational
VECTOR
MPCFR, MPCFRI, MPCFMP
Chapter 4: Read Results 521 Supported MSC.Access Result Quantities
Primary Label Grid Point Forces
Secondary Label
Type
Objects
Applied Loads
VECTOR
GPFV
Constraint Forces
VECTOR
GPFV
MPC Forces
VECTOR
GPFV
Elements
VECTOR
GPFV
Total
VECTOR
GPFV
Applied Loads
VECTOR
GPFV
Constraint Forces
VECTOR
GPFV
MPC Forces
VECTOR
GPFV
Elements
VECTOR
GPFV
Total
VECTOR
GPFV
Bushing Forces
Translational, Rotational
VECTOR
FBSHR, FBSHRI, FBSHMP
Bushing Stresses
Translational, Rotational
VECTOR
SBSHR, SBSHRI, SBSHMP
Bushing Strains
Translational, Rotational
VECTOR
EBSHR, EBSHRI, EBSHMP
Bushing 1-D Results
Axial Stress, Axial Strain, Axial Force, Axial Displacement
SCALAR
SBS1R, SBS1RI, SBS1MP
Nonlinear Bushing Force
Axial Stress, Axial Strain, Axial Force, Axial Displacement
SCALAR
NBS1R, NBS1RI, NBS1MP
Temperature
SCALAR
THERR
Enthalpies
SCALAR
ENTHR
Rates of Enthalpy Change
SCALAR
ENRCR
Constraint Heats
SCALAR
HTFFR
Applied Loads
SCALAR
HTFLR
Boundary Heat Flux
Applied Loads
SCALAR
QHBDY
Free Convection
SCALAR
QHBDY
Forced Convection
SCALAR
QHBDY
Radiation
SCALAR
QHBDY
Total
SCALAR
QHBDY
Grid Point Moments
522
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Heat Fluxes
VECTOR
QBARR, QBEMR,QCONR, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R
Temperature Gradients
VECTOR
QBARR, QBEMR, QCONR, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R
Chapter 4: Read Results 523 Supported MSC.Access Result Quantities
Elemental Results Primary Label Bar Forces
Secondary Label
Type
Objects
Translational
VECTOR
FBEMR
Rotational
VECTOR
FBEMR
Warping Torque
SCALAR
FBEMR
Translational
VECTOR
FBEMRI
Rotational
VECTOR
FBEMRI
Warping Torque
SCALAR
FBEMRI
Translational
VECTOR
FBEMMP
Rotational
VECTOR
FBEMMP
Warping Torque
SCALAR
FBEMMP
Translational
VECTOR
FTUBR
Rotational
VECTOR
FTUBR
Translational
VECTOR
FTUBRI
Rotational
VECTOR
FTUBRI
Translational
VECTOR
FTUBMP
Rotational
VECTOR
FTUBMP
Translational
VECTOR
FCONR
Rotational
VECTOR
FCONR
Translational
VECTOR
FCONRI
Rotational
VECTOR
FCONRI
Translational
VECTOR
FCONMP
Rotational
VECTOR
FCONMP
Translational
VECTORs
FELSR FELSRI FELSMP FDMPR FDMPRI FDMPMP
Rotational
VECTOR
FBARR
Translational
VECTOR
FBARR
Rotational
VECTOR
FBARRI
Translational
VECTOR
FBARRI
524
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Bar Forces (continued
Shear Panel Forces
Secondary Label
Type
Objects
Rotational
VECTOR
FBARMP
Translational
VECTOR
FBARMP
Translational
VECTOR
FBRXR
Rotational
VECTOR
FBRXR
Force41
SCALAR
FSHRR
Force21
SCALAR
FSHRR
Force12
SCALAR
FSHRR
Force32
SCALAR
FSHRR
Force23
SCALAR
FSHRR
Force43
SCALAR
FSHRR
Force34
SCALAR
FSHRR
Force14
SCALAR
FSHRR
Kick
SCALAR
FSHRR
Shear
SCALAR
FSHRR
Force41
SCALAR
FSHRRI
Force21
SCALAR
FSHRRI
Force12
SCALAR
FSHRRI
Force32
SCALAR
FSHRRI
Force23
SCALAR
FSHRRI
Force43
SCALAR
FSHRRI
Force34
SCALAR
FSHRRI
Force14
SCALAR
FSHRRI
Kick
SCALAR
FSHRRI
Shear
SCALAR
FSHRRI
Force41
SCALAR
FSHRMP
Force21
SCALAR
FSHRMP
Force12
SCALAR
FSHRMP
Force32
SCALAR
FSHRMP
Force23
SCALAR
FSHRMP
Force43
SCALAR
FSHRMP
Force34
SCALAR
FSHRMP
Force14
SCALAR
FSHRMP
Chapter 4: Read Results 525 Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Shear Panel Forces (continued)
Kick
SCALAR
FSHRMP
Shear
SCALAR
FSHRMP
Shell Forces
Force Resultant
TENSOR
FQD4R
Moment Resultant
TENSOR
FQD4R
Force Resultant
TENSOR
FQD4RI
Moment Resultant
TENSOR
FQD4RI
Force Resultant
TENSOR
FQD4MP
Moment Resultant
TENSOR
FQD4MP
Force Resultant
TENSOR
FQD8R
Moment Resultant
TENSOR
FQD8R
Force Resultant
TENSOR
FQD8RI
Moment Resultant
TENSOR
FQD8RI
Force Resultant
TENSOR
FQD8MP
Moment Resultant
TENSOR
FQD8MP
Force Resultant
TENSOR
FTRRR
Moment Resultant
TENSOR
FTRRR
Force Resultant
TENSOR
FTRRRI
Moment Resultant
TENSOR
FTRRRI
Force Resultant
TENSOR
FTRRMP
Moment Resultant
TENSOR
FTRRMP
Force Resultant
TENSOR
FTR3R
Moment Resultant
TENSOR
FTR3R
Force Resultant
TENSOR
FTR3RI
Moment Resultant
TENSOR
FTR3RI
Force Resultant
TENSOR
FTR3MP
Moment Resultant
TENSOR
FTR3MP
Force Resultant
TENSOR
FTR6R
Moment Resultant
TENSOR
FTR6R
Force Resultant
TENSOR
FTR6RI
Moment Resultant
TENSOR
FTR6RI
Force Resultant
TENSOR
FTR6MP
Moment Resultant
TENSOR
FTR6MP
526
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Shell Forces (continued)
Gap Results
Stress Tensor
Secondary Label
Type
Objects
Force Resultant
TENSOR
FQDRR
Moment Resultant
TENSOR
FQDRR
Force Resultant
TENSOR
FQDRRI
Moment Resultant
TENSOR
FQDRRI
Force Resultant
TENSOR
FQDRMP
Moment Resultant
TENSOR
FQDRMP
Force Resultant
TENSOR
FQD4XR
Moment Resultant
TENSOR
FQD4XR
Force Resultant
TENSOR
FQD4XRI
Moment Resultant
TENSOR
FQD4XRI
Force Resultant
TENSOR
FQD4XMP
Moment Resultant
TENSOR
FQD4XMP
Force
VECTOR
FGAPR
Displacement
VECTOR
FGAPR
Slip
VECTOR
FGAPR
Force
VECTOR
NGAPR
Displacement
VECTOR
NGAPR
Slip
VECTOR
NGAPR
NONE
TENSOR
SRODR
TENSOR
SRODRI
TENSOR
SRODMP
TENSOR
SBEMR
TENSOR
SBEMRI
TENSOR
SBEMMP
TENSOR
STUBR
TENSOR
STUBRI
TENSOR
STUBMP
TENSOR
SCONR
TENSOR
SCONRI
TENSOR
SCONMP
NONE NONE
NONE
Chapter 4: Read Results 527 Supported MSC.Access Result Quantities
Primary Label Stress Tensor (continued)
Secondary Label NONE
Type
Objects
TENSOR
SELSR
TENSOR
SELSRI
TENSOR
SELSMP
TENSOR
SQD4R
TENSOR
SQD4RI
TENSOR
SQD4MP
TENSOR
SBARR
TENSOR
SBARRI
TENSOR
SBARMP
TENSOR
STETR
TENSOR
STETRI
TENSOR
STETMP
NONE
TENSOR
STX6R
NONE
TENSOR
SQD8R
TENSOR
SQD8RI
TENSOR
SQD8MP
TENSOR
SHEXR
TENSOR
SHEXRI
TENSOR
SHEXMP
TENSOR
SPENR
TENSOR
SPENRI
TENSOR
SPENMP
TENSOR
STRRR
TENSOR
STRRRI
TENSOR
STRRMP
TENSOR
STR6R
TENSOR
STR6RI
TENSOR
STR6MP
TENSOR
STR3R
TENSOR
STR3RI
TENSOR
STR3MP
NONE
NONE
NONE
NONE
NONE
NONE
NONE
NONE
528
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Stress Tensor (continued)
Bar Stresses
Bar Strains
Secondary Label NONE
Type
Objects
TENSOR
SQDRR
TENSOR
SQDRRI
TENSOR
SQDRMP
NONE
TENSOR
TQD4R
NONE
TENSOR
TQD8R
NONE
TENSOR
TTR3R
NONE
TENSOR
TTR6R
NONE
TENSOR
SBRXR
NONE
TENSOR
SQD4XR
TENSOR
SQD4XRI
TENSOR
SQD4XMP
NONE
TENSOR
SBRXR
Maximum Axial
SCALAR
SBEMR
Minimum Axial
SCALAR
SBEMR
Maximum Axial
SCALAR
SBARR
Minimum Axial
SCALAR
SBARR
Tension Safety Margin
SCALAR
SBARR
Maximum Axial
SCALAR
SBRXR
Minimum Axial
SCALAR
SBRXR
Maximum Axial
SCALAR
SBRXR
Minimum Axial
SCALAR
SBRXR
Maximum Axial
SCALAR
EBEMR
Minimum Axial
SCALAR
EBEMR
Maximum Axial
SCALAR
EBARR
Minimum Axial
SCALAR
EBARR
Tension Safety Margin
SCALAR
EBARR
Compressive Safety Margin
SCALAR
EBARR
Maximum Axial
SCALAR
EBRXR
Minimum Axial
SCALAR
EBRXR
Maximum Axial
SCALAR
EBRXR
Minimum Axial
SCALAR
EBRXR
Chapter 4: Read Results 529 Supported MSC.Access Result Quantities
Primary Label Strain Tensor
Secondary Label NONE
NONE
NONE
NONE
NONE
NONE
NONE
NONE
Type
Objects
ENG_TENSOR
ERODR
ENG_TENSOR
ERODRI
ENG_TENSOR
ERODMP
ENG_TENSOR
EBEMR
ENG_TENSOR
EBEMRI
ENG_TENSOR
EBEMMP
ENG_TENSOR
ETUBR
ENG_TENSOR
ETUBRI
ENG_TENSOR
ETUBMP
ENG_TENSOR
ECONR
ENG_TENSOR
ECONRI
ENG_TENSOR
ECONMP
ENG_TENSOR
EELSR
ENG_TENSOR
EELSRI
ENG_TENSOR
EELSMP
ENG_TENSOR
EQD4R
ENG_TENSOR
EQD4RI
ENG_TENSOR
EQD4MP
ENG_TENSOR
EBARRI
ENG_TENSOR
EBARR
ENG_TENSOR
EBARMP
ENG_TENSOR
ETETR
ENG_TENSOR
ETETRI
ENG_TENSOR
ETETMP
ENG_TENSOR
EQD8R
ENG_TENSOR
EQD8RI
ENG_TENSOR
EQD8MP
530
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Tensor (continued)
Shear Panel Stresses
Shear Panel Strains
Secondary Label
Type
Objects
ENG_TENSOR
EQDRR
ENG_TENSOR
EQDRRI
ENG_TENSOR
EQDRMP
NONE
ENG_TENSOR
GQD4R
NONE
ENG_TENSOR
GQD8R
NONE
ENG_TENSOR
GTR3R
NONE
ENG_TENSOR
GTR6R
NONE
ENG_TENSOR
EBRXR
NONE
ENG_TENSOR
EQD4XR
ENG_TENSOR
EQD4XRI
ENG_TENSOR
EQD4XMP
NONE
ENG_TENSOR
EBRXR
Maximum Shear
SCALAR
SSHRR
Average Shear
SCALAR
SSHRR
Maximum Shear
SCALAR
SSHRRI
Average Shear
SCALAR
SSHRRI
Maximum Shear
SCALAR
SSHRMP
Average Shear
SCALAR
SSHRMP
Maximum Shear
SCALAR
SSHRR
Average Shear
SCALAR
SSHRR
Maximum Shear
SCALAR
SSHRRI
Average Shear
SCALAR
SSHRRI
Maximum Shear
SCALAR
SSHRMP
Average Shear
SCALAR
SSHRMP
Maximum Shear
SCALAR
ESHRR
Average Shear
SCALAR
ESHRR
Maximum Shear
SCALAR
ESHRRI
Average Shear
SCALAR
ESHRRI
Maximum Shear
SCALAR
ESHRMP
Average Shear
SCALAR
ESHRMP
NONE
Chapter 4: Read Results 531 Supported MSC.Access Result Quantities
Primary Label Principal Stress Direction
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
SQD4R
Major Prin x cosine
SCALAR
STETR
Minor Prin x cosine
SCALAR
STETR
Intermed Prin x cosine
SCALAR
STETR
Major Prin y cosine
SCALAR
STETR
Minor Prin y cosine
SCALAR
STETR
Intermed Prin y cosine
SCALAR
STETR
Major Prin z cosine
SCALAR
STETR
Minor Prin z cosine
SCALAR
STETR
Intermed Prin z cosine
SCALAR
STETR
Zero Shear Angle
SCALAR
SQD8R
Major Prin x cosine
SCALAR
SHEXR
Minor Prin x cosine
SCALAR
SHEXR
Intermed Prin x cosine
SCALAR
SHEXR
Major Prin y cosine
SCALAR
SHEXR
Minor Prin y cosine
SCALAR
SHEXR
Intermed Prin y cosine
SCALAR
SHEXR
Major Prin z cosine
SCALAR
SHEXR
Minor Prin z cosine
SCALAR
SHEXR
Intermed Prin z cosine
SCALAR
SHEXR
Major Prin x cosine
SCALAR
SPENR
Minor Prin x cosine
SCALAR
SPENR
Intermed Prin x cosine
SCALAR
SPENR
Major Prin y cosine
SCALAR
SPENR
Minor Prin y cosine
SCALAR
SPENR
Intermed Prin y cosine
SCALAR
SPENR
Major Prin z cosine
SCALAR
SPENR
Minor Prin z cosine
SCALAR
SPENR
Intermed Prin z cosine
SCALAR
SPENR
Zero Shear Angle
SCALAR
STRRR
Zero Shear Angle
SCALAR
STR6R
Zero Shear Angle
SCALAR
STR3R
532
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Principal Stress Direction (continued)
Stress Invariants
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
SQDRR
Zero Shear Angle
SCALAR
TQD4R
Zero Shear Angle
SCALAR
TQD8R
Zero Shear Angle
SCALAR
TTR3R
Zero Shear Angle
SCALAR
TTR6R
Zero Shear Angle
SCALAR
SQD4XR
Major Principal
SCALAR
SQD4R
Minor Principal
SCALAR
SQD4R
Maximum Shear
SCALAR
SQD4R
Major Principal
SCALAR
STETR
Mean Pressure
SCALAR
STETR
Minor Principal
SCALAR
STETR
Intermediate Principal
SCALAR
STETR
Octahedral Shear
SCALAR
STETR
Von Mises
SCALAR
STETR
Major Principal
SCALAR
STX6R
Maximum Shear
SCALAR
STX6R
Octahedral Shear
SCALAR
STX6R
Von Mises
SCALAR
STX6R
Major Principal
SCALAR
SQD8R
Minor Principal
SCALAR
SQD8R
Maximum Shear
SCALAR
SQD8R
Von Mises
SCALAR
SQD8R
Major Principal
SCALAR
SHEXR
Mean Pressure
SCALAR
SHEXR
Minor Principal
SCALAR
SHEXR
Intermediate Principal
SCALAR
SHEXR
Octahedral Shear
SCALAR
SHEXR
Von Mises
SCALAR
SHEXR
Major Principal
SCALAR
SPENR
Mean Pressure
SCALAR
SPENR
Minor Principal
SCALAR
SPENR
Chapter 4: Read Results 533 Supported MSC.Access Result Quantities
Primary Label Stress Invariants (continued)
Secondary Label
Type
Objects
Intermediate Principal
SCALAR
SPENR
Octahedral Shear
SCALAR
SPENR
Von Mises
SCALAR
SPENR
Major Principal
SCALAR
STRRR
Minor Principal
SCALAR
STRRR
Maximum Shear
SCALAR
STRRR
Von Mises
SCALAR
STRRR
Major Principal
SCALAR
STR6R
Minor Principal
SCALAR
STR6R
Maximum Shear
SCALAR
STR6R
Von Mises
SCALAR
STR6R
Major Principal
SCALAR
STR3R
Minor Principal
SCALAR
STR3R
Maximum Shear
SCALAR
STR3R
Von Mises
SCALAR
STR3R
Major Principal
SCALAR
SQDRR
Minor Principal
SCALAR
SQDRR
Maximum Shear
SCALAR
SQDRR
Von Mises
SCALAR
SQDRR
Major Principal
SCALAR
TQD4R
Minor Principal
SCALAR
TQD4R
Maximum Shear
SCALAR
TQD4R
Major Principal
SCALAR
TQD8R
Minor Principal
SCALAR
TQD8R
Maximum Shear
SCALAR
TQD8R
Major Principal
SCALAR
TTR3R
Minor Principal
SCALAR
TTR3R
Maximum Shear
SCALAR
TTR3R
Major Principal
SCALAR
TTR6R
Minor Principal
SCALAR
TTR6R
Maximum Shear
SCALAR
TTR6R
Major Principal
SCALAR
SQD4XR
534
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Stress Invariants (continued)
Principal Strain Direction
Secondary Label
Type
Objects
Minor Principal
SCALAR
SQD4XR
Maximum Shear
SCALAR
SQD4XR
Von Mises
SCALAR
SQD4XR
Zero Shear Angle
SCALAR
EQD4R
Major Prin x cosine
SCALAR
ETETR
Minor Prin x cosine
SCALAR
ETETR
Intermed Prin x cosine
SCALAR
ETETR
Major Prin y cosine
SCALAR
ETETR
Minor Prin y cosine
SCALAR
ETETR
Intermed Prin y cosine
SCALAR
ETETR
Major Prin z cosine
SCALAR
ETETR
Minor Prin z cosine
SCALAR
ETETR
Intermed Prin z cosine
SCALAR
ETETR
Zero Shear Angle
SCALAR
EQD8R
Major Prin x cosine
SCALAR
EHEXR
Minor Prin x cosine
SCALAR
EHEXR
Intermed Prin x cosine
SCALAR
EHEXR
Major Prin y cosine
SCALAR
EHEXR
Minor Prin y cosine
SCALAR
EHEXR
Intermed Prin y cosine
SCALAR
EHEXR
Major Prin z cosine
SCALAR
EHEXR
Minor Prin z cosine
SCALAR
EHEXR
Intermed Prin z cosine
SCALAR
EHEXR
Major Prin x cosine
SCALAR
EPENR
Minor Prin x cosine
SCALAR
EPENR
Intermed Prin x cosine
SCALAR
EPENR
Major Prin y cosine
SCALAR
EPENR
Minor Prin y cosine
SCALAR
EPENR
Intermed Prin y cosine
SCALAR
EPENR
Major Prin z cosine
SCALAR
EPENR
Minor Prin z cosine
SCALAR
EPENR
Intermed Prin z cosine
SCALAR
EPENR
Chapter 4: Read Results 535 Supported MSC.Access Result Quantities
Primary Label Principal Strain Direction (continued)
Strain Invariants
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
ETRRR
Zero Shear Angle
SCALAR
ETR6R
Zero Shear Angle
SCALAR
ETR3R
Zero Shear Angle
SCALAR
EQDRR
Zero Shear Angle
SCALAR
GQD4R
Zero Shear Angle
SCALAR
GQD8R
Zero Shear Angle
SCALAR
GTR3R
Zero Shear Angle
SCALAR
GTR6R
Zero Shear Angle
SCALAR
EQD4XR
Major Principal
SCALAR
EQD4R
Minor Principal
SCALAR
EQD4R
Maximum Shear
SCALAR
EQD4R
Major Principal
SCALAR
ETETR
Mean Pressure
SCALAR
ETETR
Minor Principal
SCALAR
ETETR
Intermediate Principal
SCALAR
ETETR
Octahedral Shear
SCALAR
ETETR
Von Mises
SCALAR
ETETR
Major Principal
SCALAR
EQD8R
Minor Principal
SCALAR
EQD8R
Maximum Shear
SCALAR
EQD8R
Von Mises
SCALAR
EQD8R
Major Principal
SCALAR
EHEXR
Mean Pressure
SCALAR
EHEXR
Minor Principal
SCALAR
EHEXR
Intermediate Principal
SCALAR
EHEXR
Octahedral Shear
SCALAR
EHEXR
Von Mises
SCALAR
EHEXR
Major Principal
SCALAR
EPENR
Mean Pressure
SCALAR
EPENR
Minor Principal
SCALAR
EPENR
Intermediate Principal
SCALAR
EPENR
536
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Invariants (continued)
Secondary Label
Type
Objects
Octahedral Shear
SCALAR
EPENR
Von Mises
SCALAR
EPENR
Major Principal
SCALAR
ETRRR
Minor Principal
SCALAR
ETRRR
Maximum Shear
SCALAR
ETRRR
Von Mises
SCALAR
ETRRR
Major Principal
SCALAR
ETR6R
Minor Principal
SCALAR
ETR6R
Maximum Shear
SCALAR
ETR6R
Von Mises
SCALAR
ETR6R
Major Principal
SCALAR
ETR3R
Minor Principal
SCALAR
ETR3R
Maximum Shear
SCALAR
ETR3R
Von Mises
SCALAR
ETR3R
Major Principal
SCALAR
EQDRR
Minor Principal
SCALAR
EQDRR
Maximum Shear
SCALAR
EQDRR
Von Mises
SCALAR
EQDRR
Major Principal
SCALAR
GQD4R
Minor Principal
SCALAR
GQD4R
Maximum Shear
SCALAR
GQD4R
Major Principal
SCALAR
GQD8R
Minor Principal
SCALAR
GQD8R
Maximum Shear
SCALAR
GQD8R
Major Principal
SCALAR
GTR3R
Minor Principal
SCALAR
GTR3R
Maximum Shear
SCALAR
GTR3R
Major Principal
SCALAR
GTR6R
Minor Principal
SCALAR
GTR6R
Maximum Shear
SCALAR
GTR6R
Major Principal
SCALAR
EQD4XR
Minor Principal
SCALAR
EQD4XR
Chapter 4: Read Results 537 Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Strain Invariants (continued)
Maximum Shear
SCALAR
EQD4XR
Von Mises
SCALAR
EQD4XR
Nonlinear Stresses
Stress Tensor
TENSOR
NTETR
Equivalent Stress
SCALAR
NTETR
Stress Tensor
TENSOR
NTUBR
Equivalent Stress
SCALAR
NTUBR
Stress Tensor
TENSOR
NTR3R
Equivalent Stress
SCALAR
NTR3R
Stress Tensor
TENSOR
NRODR
Equivalent Stress
SCALAR
NRODR
Stress Tensor
TENSOR
NQD4R
Equivalent Stress
SCALAR
NQD4R
Stress Tensor
TENSOR
NPENR
Equivalent Stress
SCALAR
NPENR
Stress Tensor
TENSOR
NCONR
Equivalent Stress
SCALAR
NCONR
Stress Tensor
TENSOR
NHEXR
Equivalent Stress
SCALAR
NHEXR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NTETR
Plastic Strain
SCALAR
NTETR
Creep Strain
SCALAR
NTETR
Strain Tensor
ENG_TENSOR
NTUBR
Plastic Strain
SCALAR
NTUBR
Creep Strain
SCALAR
NTUBR
Nonlinear Strains
538
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Nonlinear Strains (continued)
Secondary Label
Type
Objects
Strain Tensor
ENG_TENSOR
NTR3R
Plastic Strain
SCALAR
NTR3R
Creep Strain
SCALAR
NTR3R
Strain Tensor
ENG_TENSOR
NRODR
Plastic Strain
SCALAR
NRODR
Creep Strain
SCALAR
NRODR
Strain Tensor
ENG_TENSOR
NQD4R
Plastic Strain
SCALAR
NQD4R
Creep Strain
SCALAR
NQD4R
Strain Tensor
ENG_TENSOR
NPENR
Plastic Strain
SCALAR
NPENR
Creep Strain
SCALAR
NPENR
Strain Tensor
ENG_TENSOR
NCONR
Plastic Strain
SCALAR
NCONR
Creep Strain
SCALAR
NCONR
Strain Tensor
ENG_TENSOR
NHEXR
Plastic Strain
SCALAR
NHEXR
Creep Strain
SCALAR
NHEXR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Chapter 4: Read Results 539 Supported MSC.Access Result Quantities
Primary Label Strain Energy
Secondary Label
Type
Objects
Energy
SCALAR
URODR
Percent of Total
SCALAR
URODR
Energy Density
SCALAR
URODR
Energy
SCALAR
UBEMR
Percent of Total
SCALAR
UBEMR
Energy Density
SCALAR
UBEMR
Energy
SCALAR
UTUBR
Percent of Total
SCALAR
UTUBR
Energy Density
SCALAR
UTUBR
Energy
SCALAR
USHRR
Percent of Total
SCALAR
USHRR
Energy Density
SCALAR
USHRR
Energy
SCALAR
UCONR
Percent of Total
SCALAR
UCONR
Energy Density
SCALAR
UCONR
Energy
SCALAR
UELSR
Percent of Total
SCALAR
UELSR
Energy Density
SCALAR
UELSR
Energy
SCALAR
UDMPR
Percent of Total
SCALAR
UDMPR
Energy Density
SCALAR
UDMPR
Energy
SCALAR
UQD4R
Percent of Total
SCALAR
UQD4R
Energy Density
SCALAR
UQD4R
Energy
SCALAR
UBARR
Percent of Total
SCALAR
UBARR
Energy Density
SCALAR
UBARR
Energy
SCALAR
UGAPR
Percent of Total
SCALAR
UGAPR
Energy Density
SCALAR
UGAPR
Energy
SCALAR
UTETR
Percent of Total
SCALAR
UTETR
540
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Energy (continued)
Secondary Label
Type
Objects
Energy Density
SCALAR
UTETR
Energy
SCALAR
UTX6R
Percent of Total
SCALAR
UTX6R
Energy Density
SCALAR
UTX6R
Energy
SCALAR
UQD8R
Percent of Total
SCALAR
UQD8R
Energy Density
SCALAR
UQD8R
Energy
SCALAR
UHEXR
Percent of Total
SCALAR
UHEXR
Energy Density
SCALAR
UHEXR
Energy
SCALAR
UPENR
Percent of Total
SCALAR
UPENR
Energy Density
SCALAR
UPENR
Energy
SCALAR
UTRRR
Percent of Total
SCALAR
UTRRR
Energy Density
SCALAR
UTRRR
Energy
SCALAR
UTR3R
Percent of Total
SCALAR
UTR3R
Energy Density
SCALAR
UTR3R
Energy
SCALAR
UTR6R
Percent of Total
SCALAR
UTR6R
Energy Density
SCALAR
UTR6R
Energy
SCALAR
UQDRR
Percent of Total
SCALAR
UQDRR
Energy Density
SCALAR
UQDRR
Chapter 4: Read Results 541 Supported MSC.Access Result Quantities
Primary Label Cauchy Stresses
Secondary Label
Type TENSOR
Objects HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Logarithmic Strains
TENSOR
HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
542
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Pressure
Type TENSOR
Objects HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Volumetric Strains
TENSOR
HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Topology Optimization
Element Density
SCALAR
DVHIST
Chapter 4: Read Results 543 Supported 3dplot Results Quantities
4.5
Supported 3dplot Results Quantities The following table indicates all the possible result quantities which can be loaded into the Patran database from the LS-Dyna’s ptf file.
Global Variable Label
Type
Description
Displacement
Nodal
x, y, z displacements of nodes, in global coordinate frame.
Velocity
Nodal
x, y, z velocity of nodes, in global coordinate frame.
Acceleration
Nodal
x, y, z acceleration of nodes, in global coordinate frame.
Temperature
Nodal
Nodal temperature.
Forces
Nodal
Resultant beam forces and moments, in local beam coordinate.
Stress
Element
6 components of stress tensor, at element centre and gaussian points - top, middle, and bottom for shells.
Stress Resultants
Element
Stress Resultants at elements.
Strain
Element
6 components of strain tensor, at element centre and gaussian points - top, middle, and bottom for shells.
Eff. Plastic Strain
Element
Effective plastic strain, at element centre and gaussian points - top, middle, and bottom for shells.
Element Volume, Euler
Partition/ Element
Element of constant volume.
Mass, Euler
Partition/ Element
Mass of fluid in a partition (element of constant volume).
Density, Euler
Partition/ Element
Density of fluid in a partition (element of constant volume).
Specific Internal Energy, Euler
Partition/ Element
Specific internal energy of fluid in a partition (element of constant volume).
Total Energy, Euler
Partition/ Element
Total energy of fluid in a partition (element of constant volume).
Material Fraction, Euler
Partition/ Element
Material fraction of fluid * the volume uncovered fraction in a partition (element of constant volume).
Speed of Sound, Euler
Partition/ Element
Speed of sound of fluid in a partition (element of constant volume).
Momentum, Euler
Partition/ Element
Momentum of fluid in a partition (element of constant volume).
Volume Uncovered Fraction, Euler
Partition/ Element
Volume uncovered fraction of fluid in a partition (element of constant volume).
Mass Flow Rate, Euler
Partition/ Element
Mass flow rate of fluid in a partition (element of constant volume).
544
Patran Interface to MD Nastran Preference Guide Supported 3dplot Results Quantities
Global Variable Label
Type
Description
Total Mass Flow, Euler
Partition/ Element
Total mass flow over a given time of fluid in a partition (element of constant volume).
Heat Transfer Rate, Euler
Partition/ Element
Heat transfer rate for fluid in a partition (element of constant volume).
Total Heat Transfer, Euler
Partition/ Element
Total heat transfer over a given time of fluid in a partition (element of constant volume).
Velocity, Euler
Partition/ Element
Velocity of fluid in a partition (element of constant volume).
Chapter 5: Read Input File Patran Interface to MD Nastran Preference Guide
5
Read Input File
Review of Read Input File Form
Data Translated from the NASTRAN Input File
Conflict Resolution
565
546 554
546
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
5.1
Review of Read Input File Form The Analysis form will appear when the Analysis toggle, located on the Patran main menu, is chosen.
Read Input File as the selected Action on the Analysis form allows much of the model data from a MD Nastran input file to be translated into the Patran database. A subordinate File Selection form allows the user to specify the MD Nastran input file to translate. This form is described on the following pages.
Chapter 5: Read Input File 547 Review of Read Input File Form
Read Input File Form This form appears when the Analysis toggle is selected on the main menu. Read Input File, as the selected Action, specifies that model data is to be translated from the specified MD Nastran input file into the Patran database.
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of already existing jobs.
Name assigned to current translation job. This job name will be used as the base file name for the message file.
Activates a subordinate Entity Selection form which allows the user to specify the specific entry types to be read. Also defines ID offset values to be used during import.
Activates a subordinate File Select form which allows the user to specify the NASTRAN input file to be translated.
548
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
Entity Selection Form This subordinate form appears when the Entity Selection button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which MD Nastran entity types to import.
Highlighted entity types will be imported.
Activates the form to define ID offsets.
Select this button to create groups based on property sets and materials. Selecting this toggle will tell Patran to attempt to retrieve the names of properties and materials from the comments in the input file. This only applys to material and element properties names.
Chapter 5: Read Input File 549 Review of Read Input File Form
The following table shows the relation between the entity types listed above and the actual MD Nastran entry types effected. If an entity type is filtered out, it is treated as if those entries did not exist in the original input file. Entity Type
MD Nastran Cards
Nodes
GRID, GRDSET, SPOINT
Elements
BAROR, BEAMOR, CBAR, CBEAM, CBEND, CDAMP1, CDAMP2, CDAMP3, CDAMP4, CELAS1, CELAS2, CELAS3, CELAS4, CGAP, CHEXA, CMASS1, CMASS2, CMASS3, CMASS4, CONM1, CONM2, CONROD, CPENTA, CQUAD4, CQUAD8, CQUADR, CROD, CSHEAR, CTETRA, CTRIA3, CTRIA6, CTRIAR, CTRIAX6, CTUBE, CVISC, PLOTEL
Material Properties
MAT1, MAT2, MAT3, MAT8, MAT9
Element Properties
PBAR, PBCOMP, PBEAM, PBEND, PCOMP, PDAMP, PELAS, PGAP, PMASS, PROD, PSHEAR, PSHELL, PSOLID, PTUBE, PVISC
Coordinate Frames
CORD1C, CORD1R, CORD1S, CORD2C, CORD2R, CORD2S
Load Sets
FORCE, GRAV,MOMENT, PLOAD1, PLOAD2, PLOAD4, PLOADX1, RFORCE, TEMP, TEMPP1, TEMPRB, SPC, SPC1, SPCD
Subcases
LOAD, SPCADD, Case Control Section
MPC Data
MPC, RBAR, RBE1, RBE2, RBE3, RROD, RSPLINE, RTRPLT It should be noted that since the GRID entry is controlled with the Nodes filter, the grid.ps load set with the permanent single point constraint data will also be controlled by the Nodes filter.
550
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
Define Offsets Form This subordinate form appears when the Define Offsets button is selected on the Entity Selection form. It allows the user to specify the ID offsets used when reading a MD Nastran input file. If selected, the value in the Maximum column will be used as the offset for the selected rows.
Minimum and Maximum IDs currently found in the Patran database.
All offset data boxes can be selected at once by selecting this column header.
ID offset value to be used during import. The new ID value will be the ID found in the NASTRAN input file plus this offset value.
All references made in the input file will also be offset. If a node references a particular CID as its analysis frame, then the reference will be offset as well. If the coordinate frame is defined in the same input file, the proper references should be maintained. The preference will be properly maintained. If the coordinate frame existed in the file prior to the import, then it needs to be the offset CID. If a coordinate frame with that CID is not found in the database, an error message will be issued.
Chapter 5: Read Input File 551 Review of Read Input File Form
To determine which offset effects a particular MD Nastran entry type, refer to the table in the previous section. For Patran entities identified by integer IDs (nodes, elements, coordinate frames, and MPCs), the offset value is simply added to the MD Nastran ID to generate the Patran ID. For Patran entities identified by text names (materials, element properties, load sets, and load cases), the offset value is first added to the MSC Nastran ID. The new integer value is then used to generate the Patran name per the naming conventions described in later sections.
Selection of Input File This subordinate form appears when the Select Input File button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which MD Nastran input file to translate.
Summary Data Form This form appears after the import of the NASTRAN input file has completed. It displays the number of entities imported correctly, imported with warnings, or not imported due to errors. These figures reflect the number of Patran entities created. In some cases, there is not a one-to-one relation between the original MD Nastran entities and the generated Patran entities. For example, when material orientations on several CQUAD4s are defined using references to varying MCIDs while still referencing the same PID, Patran needs to create a unique property set for each different MCID reference.
552
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
When the OK button is selected, the newly imported data will be committed to the Patran database, and can not be undone. If there is any question as to whether or not this import was desired, review the graphics data prior to selecting OK on this form. If the import was not correct, select the undo button on the main menu bar before selecting OK on this form. NASTRAN Input File Import Summary Imported
Imported with Warning
Nodes Elements Coordinate Frames Materials Element Properties Load Sets Load Cases MPCs
Reject Cards...
OK
Not Imported
Chapter 5: Read Input File 553 Review of Read Input File Form
Reject Card Form During import of the NASTRAN input file, some entries types might not be understood by Patran. Those entries are brought into Patran in the direct text input data boxes. Selecting the Reject Cards button on the Summary Data form will bring up this Reject Card Form. You can review these entries here. Direct Text Import Bulk Data Section $ $CBEAM
215
MPCADD
100
213 101
214
0.
0.
1.
102
uu File Management Section
uu Case Control Section
uu Executive Control Section u Bulk Data Section OK
Only entry types not supported by Patran are sent to the reject entry blocks. (This includes comments.) Cards which are otherwise recognized, but can not be imported due to syntax or invalid data errors are not sent to the reject blocks. The rejected entries will have no characters in front of the command name. Commands preceded by the character $> are used by the MSC/AMS product to allow processing of comment lines. Note:
As long as you don not delete the reject casrd file, Patran will re-insert the rejected entries back into the input file if you use the same jobname.
554
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
5.2
Data Translated from the NASTRAN Input File The following sections describe which specific MD Nastran entry types can currently be read into Patran. The MD Nastran entries described in this document are the only entries read when importing a NASTRAN input file into Patran. All non-supported entries will be sent to the appropriate Direct Text Input data box for this job. When errors occur during the import of a supported entry type, the entry being processed may or may not be imported, depending on the severity of the problem encountered. An error message will be presented regardless of whether or not the offending entry is actually imported. Any references from supported entries to entries that were not imported (either due to not being a supported entry type or due to serious import errors) will still be attempted. If this reference is required in Patran for the entry currently being processed, it too will fail to import. For example, if there is a serious error on a GRID entry which causes it to not imported, then all elements attached to that GRID will also fail to import. Partial Decks This Patran function can read incomplete MD Nastran files (except where explicitly noted). However, if the BEGIN BULK command is missing, the program can get confused when trying to determine if a particular entry belongs to the case control or bulk data. If you experience any difficulties importing a file that does not have a BEGIN BULK command, add one to the top of the file. This should avoid any such confusion.
Coordinate Systems The following coordinate system definitions can be read into Patran. Command CORD1C CORD1R
Comments References to the GRIDs on these entries are lost. The locations of the referenced GRIDs are extracted, and those locations are used to create the Patran definition.
CORD1S CORD2C CORD2R CORD2S
References to RIDs are lost. The specified locations are converted to global cartesian for use in the Patran definitions. The original B and C points are not retained. Their values are recomputed when a new NASTRAN input file is created. The definition will be equivalent, but not identical.
Referential Integrity Coordinate systems and GRIDs which are referenced as part of a CORD definition must be in the same input file. If these are not found in the input file, the definition will be rejected.
Chapter 5: Read Input File 555 Data Translated from the NASTRAN Input File
References to coordinate frames other than for new coordinate frame definitions can be resolved with coordinate frames previously found in the Patran database. Chaining Due to limitations in the Patran definitions of coordinate systems, chained definitions (definitions based on other coordinate systems or grids) are modified during import. The resulting definitions are equivalent in global space, but are based on global cartesian coordinates rather than GRID references or coordinate locations in other systems. This change is carried through when a new NASTRAN input file is created. All coordinate systems will be created using CORD2 type definitions, and they will all reference global cartesian coordinates. These definitions will be different from, but equivalent to, the original definitions.
Grids and SPOINTs The MD Nastran GRID entry is read fully, except the SEID field. The CD and CP references are both maintained. The PS data is used to create a constraint set. The details of the created load set are defined in the load set import section. GRDSET data is merged into the GRID data during import. The data will be retained, but will appear directly on the GRID entry when a new NASTRAN input file is generated. SPOINTs SPOINTs are treated as GRIDs at the global origin. They are assumed to have their GRID CD and CP fields set to the basic system, and their PS field is set to permanently constrain degrees-of-freedom 2 through 6. Referential Integrity Coordinate frames referenced in the CP field must exist in the same input file. Coordinate frames referenced on the CD field can exist in either the same input file, or the Patran database prior to the import.
Elements and Element Properties The following MD Nastran elements and element properties can be read into Patran. Element CBAR
Property PBAR
Property Set Name pbar.
Comments Orientation and offset vectors are re-defined in global cartesian during import. (See BAROR comments below.)
PBARL
pbarl.
556
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element
Property
Property Set Name
Comments
CBARAO
New property sets are created for each occurrence of a CBAR entry referenced by a CBARAO entry
CBEAM
Orientation and offset vectors are re-defined in global cartesian during import. (See BEAMOR comments below.) PBEAM
pbeam.
PBEAML
pbeaml.
PBCOMP
pbcomp.
The MD Nastran documentation describes how the section data is used to create a complete set of lumped areas. The data imported into Patran is fully expanded, and therefore, is different from the data in the original input file. This definition is, however, fully equivalent to the original. The SO field is not currently supported. A YES is provided automatically when a new NASTRAN input file is created. Only the lumped areas definition is understood, If a uniform cross section is defined here, it will be converted to a lumped area definition, but no lumped areas will be defined.
CBEND
Patran only understands the GEOM = 1 orientation data. If other definitions are found, a vector will be computed to convert the definition to the GEOM = 1 format. If a GRID was referenced for GEOM other than 1, that reference will be lost. For the same reasons, the THETAB and RB data will also be lost since that data is not used for GEOM = 1 definitions. Orientation and offset vectors are re-defined in global cartesian during import. PBEND
CBUSH
PBUSH
pbend_g.
If standard cross section properties are found on the PBEND entry
pbend_p.
If the alternate format of the PBEND is used to define a pipe cross section.
pbush. pbush_g.
CDAMP1 CDAMP2
The grounded form of the PBUSH
PBUSHT
pbusht_1D.
PDAMP
pdamp.
For dampers connecting 2 GRIDs.
pdamp_g.
For grounded dampers attached to a single GRID.
cdamp2
For dampers connecting 2 GRIDs.
cdamp2_g
For grounded dampers attached to a single GRID.
Chapter 5: Read Input File 557 Data Translated from the NASTRAN Input File
Element CDAMP3
Property
Property Set Name
PDAMP
Treated identical to the CDAMP1 and CDAMP2 elements with the degree-of-freedom fields set to 1 (UX).
CDAMP4 CELAS1
PELAS
CELAS2 CELAS3
pelas.
For springs connecting 2 GRIDs.
pelas_g.
For grounded springs attached to a single GRID.
celas2
For springs connecting 2 GRIDs.
celas2_g
For grounded springs attached to a single GRID.
PELAS
Treated identical to the CELAS1 and CELAS2 elements with the degree-of-freedom fields set to 1 (UX).
CELAS4 CGAP
Orientation and offset vectors are re-defined in global cartesian during import. PGAP
CHBDYG
Comments
pgap.
For non-adaptive definitions on the PGAP entry.
pgap_a.
For adaptive definitions on the PGAP entry.
PHBDY
Note: The BDYOR command that may contain default values for CHBDY elements is not currently supported.
CHBDYP CHEXA
PSOLID
psolid.
CMASS1
PMASS
pmass.
For masses connecting 2 GRIDs.
pmass_g.
For masses attached to a single GRID.
cmass2
For masses connecting 2 GRIDs.
cmass2_g
For masses attached to a single GRID.
CMASS2 CMASS3
PMASS
Treated identical to the CMASS1 and CMASS2 elements with the degree-of-freedom fields set to 1 (UX).
CMASS4 CONM1
conm1
CONM2
conm2
CONROD
conrod
CPENTA
PSOLID
psolid.
CQUAD4
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
CQUAD8
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
558
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element CQUADR
Property
Property Set Name
Comments
PSHELL
pshellr.
(See PSHELL comments below.)
PCOMP
pcompr.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
CROD
PROD
prod.
CSHEAR
PSHEAR
pshear.
CTETRA
PSOLID
psolid.
CTRIA3
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
CTRIA6
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
CTRIAR
PSHELL
pshellr.
(See PSHELL comments below.)
PCOMP
pcompr.
A new material named pcomp. will be created and referenced. The SB and FT fields are currently not read.
CTRIAX6
ctriax6
CTUBE
PTUBE
ptube.
CVISC
PVISC
pvisc.
PLOTEL
Tapered tubes are converted to an equivalent constant section definition. Creates the connectivity only. These elements are not assigned to any property set region. PLOTEL entries will not be written when a new input file is created.
MBOLTU S
Defines a bolt in the form of an Overclosure MPC.
Higher order elements (CQUAD8, CTRIA6, CTRIAX6, CHEXA, CPENTA, CTETRA) will generate linear elements in Patran if none of the mid-edge nodes are specified.
Chapter 5: Read Input File 559 Data Translated from the NASTRAN Input File
PSHELL Properties PSHELL properties can be imported as any one of five Patran property types. The MID1, MID2, MID3, 12I/T3, and TS/T property fields are used to determine which one to choose. If MID2 is -1 and MID3 is 0, then a Plane Strain property set is used. If MID2 and MID3 are both 0, then a Membrane property set is chosen. If MID1 and MID3 are 0, then a Bending property set is used. If MID1, MID2, and MID3 are all the same, and the MD Nastran defaults are used for 12I/T3 and TS/T, then a Homogeneous property set is used. If all else fails, then an Equivalent Section property set is chosen. BAROR and BEAMOR Definitions The BAROR and BEAMOR data is merged onto the CBAR and CBEAM entries using the proper MD Nastran conventions. The data is treated as if it had originally been defined on the CBAR and CBEAM entries. When a new NASTRAN input file is created, the data will remain with the CBAR and CBEAM entries. No BAROR or BEAMOR entries are generated. Fields If a field is required to store varying data, the field will have the same name as the property set, with the name of the specific property word appended to it. For example, if property set “pshell.101” has a varying thickness, the field will be named “pshell.101.Thickness”. Referential Integrity Nodes and coordinate frames referenced on elements or element properties must exist, but they do not need to be in the input file. They could also have been defined in the Patran database prior to the import. If a material is referenced, but can not be found, a new material with no properties will be created. A message will be issued indicating the creation of this material. If an element property set is referenced, but can not be found, a new property set with no properties will be created. A message will be issued indicating the creation of this property set. Set Name Extensions In some cases, the data found on the element can not be defined in Patran in a single property set. In those cases, multiple property sets will be created to define the distinct definitions. The table below defines extensions to the Property Set Names shown in the previous table. If the values on the specified field changes, a new property set with the indicated extension will be created. If all elements which reference a single PID can be stored in a single property set, then no extension will be added to the Property Set Name. Element CBAR
Field
Extension
PA
.pa
PB
.pb
Comments
560
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element
Field
Extension
SA
.sa<SA>
SB
.sb<SB>
PA
.pa
PB
.pb
CDAMP1, CDAMP2,
C1
.ca
CELAS1, CELAS2,
C2
.cb
CDAMP3, CDAMP4,
C1
.ca1
CELAS3, CELAS4,
C2
.cb1
CGAP, CONM1, CONM2
CID
.c
CONROD, CTRIAX6
MID
.m<MID>
CQUAD4, CQUAD8,
MCID
.c<MCID>
CBEAM
Comments
CMASS1, CMASS2 These are automatically treated as component 1 (X translation).
CMASS3, CMASS4
CQUADR, CTRIA3, CTRIA6, CTRIAR
Materials The following MD Nastran material definitions can be read into Patran. Material Type
Material Name
Comments
CREEP MAT1
mat1.<mid>
The MCSID field is not currently supported. If the G field is blank in the input file, the MD Nastran default value will be filled in during import.
MATT1 MAT2
mat2.<mid>
MATT2 MAT3 MATT3 MAT4
mat3.<mid>
The MCSID field is not currently supported.
Chapter 5: Read Input File 561 Data Translated from the NASTRAN Input File
Material Type
Material Name
Comments
MATT4 MAT5 MATT5 MAT8
mat8.<mid>
MAT9
mat9.<mid>
MATT9
MPCs The following MD Nastran MPC and rigid element definitions can be read into Patran. Card Type MPC
MPC Type Explicit
Comments Unique MPC IDs will be assigned to these entities. Since Patran uses a slightly different basis MPC equation, the equation coefficients (Ai) will probably be scaled by a constant multiplier during import. The resulting equation will be equivalent, but not necessarily identical to the original definition in the NASTRAN input file.
RBAR
RBAR
RBE1
RBE1
RBE2
RBE2 Fixed
RBE3
RBE3
RROD
RROD
RSPLINE
RSPLINE
RSSCON
RSSCON
RTRPLT
RTRPLT MPCs in Patran are treated as elements and are not associated to load cases. As a result, all SUBCASE related data is lost. The MPCs are simply imported into the model and are no longer associated to a specific load case. MPCs can reference SPOINTs instead of GRIDs. If this is detected, the corresponding component field will be set to 1 (UX) to be consistent with the import of SPOINTs. The MPCADD command is not read since the MPCs are simply imported and no associated to a load case. The SID references on the MPC entry are also lost for the same reason. New MPC IDs are assigned to these elements during import.
562
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Load Sets The following MD Nastran Loads and Boundary Condition definitions can be read into Patran. Card Type
LBC Set Name
FORCE
force.<sid>
GRAV
grav.<sid>
MOMENT
moment.<sid>
PLOAD1
pload1.<sid>
PLOAD2
pload2.<sid>
PLOAD4
pload4.<sid>
PLOADX1
ploadx1.<sid>
CONV
conv.
Comments
Only PLOAD1s applied to the entire length of an element can be read. If a load is applied only to a portion of an element, the load will be ignored, and a message will be presented indicating the problem. Only pressure loads normal to the surface can be imported. If a surface traction is detected, it will be ignored, and a message will be presented indicating the problem.
PCONV CONVM
convm.
PCONVM QBDYi
qbdyi.
QVECT
qvect.
QVOL
qvol.
RADBC
radbc.
RADCAV
radcav.
Note: ELEAMB field is not supported by Patran. The ambient element is added to the application region.
rforce.<sid>
If the G point is not at the origin of the referenced CID, a new CID will be created and referenced.
RADM RADMT RFORCE
The METHOD field is not read. It is automatically set to 1 when writing a new file. SLOAD
sload.
TEMP
temp.<sid>
TEMPP1
tempp1.<sid>
Only the average temperature and effective linear gradient data fields are used. The specified temperatures at the Z1 and Z2 locations are ignored.
Chapter 5: Read Input File 563 Data Translated from the NASTRAN Input File
Card Type
LBC Set Name
TEMPRB
temprb.<sid>
grid#
grid.ps
SPC
spc.<sid>
Comments Only the average temperature and effective linear gradient data fields are used. The specified temperatures at the stress recovery locations are ignored.
SPCADD SPC1
spc1.<sid>
SPCD
spcd.<sid>
The required SPC or SPC1 entries for the same Degree-of-Freedom are removed from the load case when a SPCD is found. They will automatically be re-generated when a new input file is created.
VIEW VIEW3D Fields If a field is required to store varying data, the field will have the same name as the load set, with the name of the specific data word appended to it. For example, if load set “force.101” has a varying force magnitude, the field will be named “force.101.Force”. Load cases are created in Patran from the SUBCASE definitions in the NASTRAN input file. Load sets not referenced by a SUBCASE definition are created as load sets in Patran, but are not associated to a load case. Load sets defined above the first SUBCASE command, plus any permanent single point constraint sets from the GRID entries, are associated to all load cases created during this import. If there is no case control data, then load sets will be created, but they will not be assigned to any load cases. The SPCADD and LOAD entries are used in creating load cases in Patran, but the SID of these entries is lost. The SIDs on the individual SPCx, FORCE, MOMENT, GRAV, PLOADx, RFORCE, and TEMPx entries are used in creating the names of the load sets. The name for the created load cases is derived from the subtitle of the SUBCASE. This is done for consistency with the forward PAT3NAS translation. A job is created during the import. The name of the created job is the basename of the file being read. MD Nastran allows load sets to be referenced in multiple places with different scale factors. This is not possible in Patran. Therefore, in some cases, multiple copies of the same load set need to be created with the only difference being the scale factor. The name of these load sets are modified to include the subcase ID to create unique names.
564
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
TABLES The following table types are supported during import of a NASTRAN input file. Note that some forms of the table commands are converted to an equivalent version supported by Patran. Card Type
Field Name
Comments
TABLED1
Field.
TABLED2
Field.
Converted to an equivalent TABLED1 when read into Patran by NIFIMP.
TABLED3
Field.
Converted to an equivalent TABLED1 when read into Patran by NIFIMP.
TABLEM1
Field.
TABLEM2
Field.
Converted to an equivalent TABLEM1 when read into Patran by NIFIMP.
TABLEM3
Field.
Converted to an equivalent TABLEM1 when read into Patran by NIFIMP.
SOL 600 entries
Note:A
Additional entries specific to SOL 600 can be read into Patran. For more details see MD Nastran Implicit Nonlinear (SOL 600), 14.
Chapter 5: Read Input File 565 Conflict Resolution
5.3
Conflict Resolution If an entity can not be imported into Patran because another entity already exists with that ID or name, then the conflict resolution logic is used. There are 2 different approaches taken, depending on whether the entity is identified by an ID or by a name.
Conflict Resolution for Entities Identified by IDs If a new definition conflicts with a definition already in the Patran database, you will be asked if you want the ID of the new definition offset. If you select YES, a new ID will be chosen. If you select YES FOR ALL, a new ID will be chosen for this definition, as well as for any others found to be in conflict. In this case, then all references to the ID in the original Patran database will still reference the old ID, but references to the ID from within the input file will be altered to reference the new ID. If you do not want the CID to be offset, then you will be asked if you want the new definition to overwrite the existing definition. If this is done, then all references to this ID from both the original Patran database and the input file will be referencing the same ID. The definition for that ID will be either the old or the new definition, depending on how this second question is answered.
Conflict Resolution for Entities Identified by Names The user is not asked what to do in cases where the conflicting entities are identified by names. The name for the new entity will be modified by appending an extension to the name. The new name will be “.r”. The value of n is chosen to make the new name unique. No merging of data or application regions is done. The old definition is left unchanged.
566
Patran Interface to MD Nastran Preference Guide Conflict Resolution
Chapter 6: Delete Patran Interface to MD Nastran Preference Guide
6
Delete
Review of Delete Form
568
Deleting an MD Nastran Job
569
568
Patran Interface to MD Nastran Preference Guide Review of Delete Form
6.1
Review of Delete Form The Analysis form will appear when the Analysis toggle, located on the Patran main form, is chosen and the selected Action is Delete.
The Delete option under Action allows the user to delete jobs that have been created for the MD Nastran preference.
Chapter 6: Delete 569 Deleting an MD Nastran Job
6.2
Deleting an MD Nastran Job This format of the Analysis form appears when the Action is set to Delete. The user may delete job definitions that were created for the MD Nastran preference with this form.
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of already existing jobs. Select the jobs that are to be deleted.
Deletes the jobs selected in the Existing Jobs listbox.
570
Patran Interface to MD Nastran Preference Guide Deleting an MD Nastran Job
Chapter 7: Files Patran Interface to MD Nastran Preference Guide
7
Files
Files
572
572
Patran Interface to MD Nastran Preference Guide Files
7.1
Files The Patran MD Nastran interface uses or creates several files.The following table outlines each file and its uses. In the file name definition, jobname will be replaced with the jobname assigned by the user. File Name
Description
*.db
This is the Patran database. During an analyze pass, model data is read from this database and, during a Read Results pass, model and/or results data is written into it. This file typically resides in the current directory.
jobname.jbr
These are small files used to pass certain information between Patran and the independent translation programs during translation. There should never be a need to directly alter these files. These files typically reside in the current directory.
jobname.bdf
This is the NASTRAN input file created by the interface. This file typically resides in the current directory.
msc_v#_sol#.alt
These are a series of MD Nastran alters that are read during forward translation. These alters instruct MD Nastran to write information to the OUTPUT2 file that the results translation will be looking for. The forward translator searches the Patran file path for these files, but they typically reside in the/alters directory. If these files do not meet specific needs, edit them accordingly. However, the naming conversion of msc_v# _sol#<solution #>.alt must be preserved. Either place the edited file back into the /alters directory or in any directory on the Patran file path, which takes precedence over the /alters directory. If these files are not used, remove them from the Patran file path, rename them, or delete them altogether.
jobname.op2
This is the MD Nastran OUTPUT2 file, which is read by the Read Results pass. This file typically resides in the current directory and contains both model and results data. It is created by placing a PARAM,POST,-1 in the input file.
jobname.xdb
This is the MD Nastran XDB file or MSC.Access database, which is attached by the Read Results pass. This file typically resides in the current directory and contains results data. It is created by placing a PARAM, POST,0 in the input file.
jobname.marc.t16
SOL 600 file recommended for use in postprocessing SOL 600 analyses.
jobname.flat
This file may be generated during a Read Results pass. If the results translation cannot write data directly into the specified Patran database it will create this jobname flat file. This file typically resides in the current directory.
jobname.marc.xxx
File generated by a SOL 600 analysis. See the “MD Nastran Implicit Nonlinear (SOL 600) User’s Guide” for a complete list.
Chapter 7: Files 573 Files
File Name
Description
jobname.msg.xx
These message files contain any diagnostic output from the translation, either forward or reverse. This file typically resides in the current directory.
MscNastranExecute
This is a UNIX script file, which is called on to submit MD Nastran after translation is complete. This file might need customizing with site specific data, such as, host machine name and MD Nastran executable commands. This file contains many comments and should be easy to edit. Patran searches its file path to find this file, but it typically resides in the bin/exe directory. Either use the general copy in /bin/exe, or place a local copy in a directory on the file path, which takes precedence over the /bin/exe directory.
574
Patran Interface to MD Nastran Preference Guide Files
Chapter 8: Errors/Warnings Patran Interface to MD Nastran Preference Guide
8
Errors/Warnings
Errors/Warnings
576
576
Patran Interface to MD Nastran Preference Guide Errors/Warnings
8.1
Errors/Warnings There are many error or warning messages that may be generated by the Patran MD.Nastran Interface. The following table outlines some of these. Message
Description
Unable to open a new message file " ". Translation messages will be written to standard output.
If the translation tries to open a message file and cannot, it will write messages to Standard Output. On most systems, the translator automatically writes messages to standard output and never tries to create a separate message file.
Unable to open the specified OUTPUT2 file "
The OUTPUT2 file was not found. Check the OUTPUT2 file specification in the translation control file.
".
The specified OUTPUT2 file " " is not in standard binary format and cannot be translated.
The OUTPUT2 file is not in standard binary format. Check the OUTPUT2 file specification in the translation control file.
Group " " does not exist in the database. Model data will not be translated.
The name of a nonexistent group was specified in the translator control file. No model data will be translated from the OUTPUT2 file.
Needed file specification missing! The full name of the job file must be specified as the first commandline argument to this program.
The translation control file must be specified as the first online argument to the translator.
Unable to open the specified database " ". Writing the OUTPUT2 information to the PCL command file " ".
If the translator cannot communicate directly to the specified database. It will write the results and/or model data to a PCL session file.
Unable to open either the specified database " PCL command file, " ". Unable to open the NASTRAN input file " Unable to open the specified database, "
", or a The naspat3 translator is unable to open any output file. Check file specification and directory protection. ".
".
The translator was unable to open a file to where the input file information will be written. The forward Patran MD.Nastran translator was unable to open the specified Patran database.
Alter file of the name " " could not be found. No The OUTPUT2 DMAP alter file, for this type of analysis, OUPUT2 alter will be written to the NASTRAN input could not be found. Correct the search path to include the file. necessary directory if you want the alter files to be written to the input file. No property regions are defined in the database. No elements or element properties can be translated.
Elements referenced by an element property region in the Patran database will not get translated by the forward Patran MD.Nastran translator. If no element regions are defined, no elements will be translated.
Chapter A: Preference Configuration and Implementation Patran Interface to MD Nastran Preference Guide
A
Preference Configuration and Implementation
Software Components in Patran MD Nastran
578
Patran MD Nastran Preference Components
579
Configuring the Patran MD Nastran Execute File
582
578
Patran Interface to MD Nastran Preference Guide Software Components in Patran MD Nastran
1.1
Software Components in Patran MD Nastran The Patran MD Nastran product includes the following items: • A PCL function contained in p3patran.plb that will add MD Nastran specific definitions to
any Patran database (not already containing such definitions) at any time. • A PCL library called mscnastran.plb and contained in the
directory. This library is used by the analysis forms to produce forms for analysis code specific translation parameter, solution parameter, etc. • A script file called MscNastranExecute, contained in the/bin/exe
directory. This script controls the operation of the interface and the submission of MD Nastran analyses. This script can be run independent of Patran but typically run from within Patran, transparent to the user. • Several MD Nastran alter files are included. These files are used when creating the NASTRAN
input file. They ask MD Nastran to produce the results file required by the NASPAT3 results translator. These files can be found in the/alter directory. They must follow the naming convention msc_v_sol<solution_number>.alt. For example, msc_v67_sol3.alt. If these files do not meet the user’s needs, they should be modified. Alter files specific to LMS CADA-X are also included. These files are identical to the standard alter files except for an additional “.lms” extension, e.g., msc_v67_sol3.alt.lms. These files are usually needed only when the user requires support for older solution sequences. • This Patran MD Nastran Interface Manual is included as part of the product. An on-line version
is also provided to allow the direct access to this information from within Patran.
Chapter A: Preference Configuration and Implementation 579 Patran MD Nastran Preference Components
1.2
Patran MD Nastran Preference Components The diagrams shown below indicate how the functions, scripts, programs, and files that constitute the Patran MD Nastran interface affect the Patran environment. Site customization, in some cases, is indicated. Figure A-1 shows the process of running an analysis. The mscnastran.plb library defines the Translation Parameter, Solution Type, Solution Parameter, and Output Request forms called by the Analysis form. When the Apply button is pushed on the Analyze form, the interface process is initiated. The interface reads data from the database and creates the NASTRAN input file. Status messages from the interface are recorded in the Patran session file. A series of MD Nastran alter files is provided. They may be used during the creation of the input file depending upon the selected solution type and solution parameters. These alter files are mostly used in support of older solution sequences. If the interface successfully produces a NASTRAN input file, and the user requests it, the MscNastranExecute script will then start MD Nastran.
Patran
p3patran.plb
Analysis mscnastran.plb
Analyze
MscNastranExecute Patran Database Alter Library
jobname.bdf
Figure A-1
MD Nastran
Forward Translation
Figure A-2 shows the process of reading information from an MD Nastran OUTPUT2 file. When the Apply button is selected on the Read Output2 form, a <jobname>.jbr file is created and the results translation is started. The results interface process reads the data from the MD Nastran OUTPUT2 file
580
Patran Interface to MD Nastran Preference Guide Patran MD Nastran Preference Components
and stores the results in the Patran database. Status messages from the interface are recorded in the Patran session file.
p3patran.plb Patran Analysis
mscnastran.plb
Read Output2
jobname.jbr Patran database
MD Nastran
Figure A-2
jobname.OP2
OUTPUT2 File Translation
Figure A-3 shows the process of translating information from a NASTRAN input file into a Patran database. The behavior of the main Analysis/Read Input File form and the subordinate file select form is
Chapter A: Preference Configuration and Implementation 581 Patran MD Nastran Preference Components
dictated by the mscnastran.plb PCL library. The Apply button on the main form activates the input file reader program, which reads the specified NASTRAN input file.
Patran p3patran.plb Analysis
Read Input File
mscnastran.plb
MD Nastran Input
Patran database
File Reader
NASTRAN Input File
input_file_name.error.* Figure A-3
NASTRAN Input File Translation
582
Patran Interface to MD Nastran Preference Guide Configuring the Patran MD Nastran Execute File
1.3
Configuring the Patran MD Nastran Execute File During the installation of the Patran MD Nastran analysis preference, the mscsetup utility creates a default site_setup file in the installation directory. This file sets environment variables relating to Patran. To custom configure this site_setup file consult Environment Variables (p. 48) in the Patran Installation and Operations Guide.
MSC.Fatigue Quick Start Guide
Index Patran Interface to MD Nastran Preference Guide
Numerics
3rd Order Invariant, 76 I n d e x
Pa tra n Int erf ac e to M
A
ACFPMRESULT, 419 ACPOWER, 419 Adaptive Meshing, 413 adaptive meshing, 501 alternate reduction, 278, 474 ALTERS, 578 Alters, 265 ALTRED, 278, 474 analysis coordinate frames, 23 analysis form, 261 analysis job definition, 263 analysis job submittal, 263 analysis preferences, 6 analyze, 260 Arruda-Boyce model, 78
B
BCBODY, 14 BCBOX, 14 BCHANGE, 14 BCMATL, 14 BCMOVE, 14 BCPARA, 14 BCPROP, 14 BCTABLE, 14 BEGIN AFPM, 178, 419 BEGIN BULK SUPER, 267, 352 BSURF, 14 buckling, 287 bulk data, 9 bulk data file, 546
C
CACINF3, 195
CACINF4, 195 case control, 9 CBAR, 103 CBEAM, 107, 115, 120 CBEND, 110, 113 CDAMP1, 98, 140 CELAS1, 97, 138 CGAP, 142 CHEXA, 206 CMASS1, 93, 145 complex Eigenvalue, 291 CONM1, 91 CONM2, 94 contact penetration, 308 contact bodies deformable surfaces defining in MSC.Patran, 241, 242 rigid surface defining in MSC.Patran, 243 slideline defining in MSC.Patran, 240 coordinate frames, 22, 510 analysis, 23 reference, 23 coordinates, 266 COUPMASS, 283 CPENTA, 206 CQUAD4, 155, 158, 161, 164, 167, 168, 171, 174, 177, 179, 183, 190, 191, 198, 200 CQUAD8, 155, 164, 168, 179, 190, 198 CQUADR, 181 CREEP, 84 CROD, 131, 134 CSHEAR, 204 CTETRA, 206 CTRIA3, 155, 161, 164, 168, 174, 177, 179, 183, 190, 198 CTRIA6, 155, 164, 168, 179, 190, 198 CTRIAR, 158, 167, 171, 181, 191, 200
584 Patran Interface to MD Nastran Preference Guide
CTRIAX, 187 CTRIAX6, 186 CTUBE, 136 CVISC, 142 CYAX, 48 cyclic symmetry, 30, 48, 278, 287, 296, 474 CYJOIN, 48 CYSYM, 48
D
DCONSTR, 479 degrees-of-freedom, 31 DESGLB, 479 DISPLACEMENT, 419 displacements, 226, 231 distributed load, 226 DOPTPRM, 470, 479 DPHASE, 231, 232 DRESP1, 479 DRESP2, 479 dynamic reduction, 286 DYNRED, 286
E
EIGB, 289 EIGC, 294 Eigenvalue extraction, 282, 287 buckling, 289 complex, 294 real, 284 EIGR, 284 EIGRL, 289 element properties, 87
elements, 510 2d solid, 190, 191 acoustic field point mesh, 177 axisymmetric solid, 186, 187 coupled point mass, 91 curved general section, 110 curved pipe, 113 gap, 142 general beam, 124 general section beam, 102 general section rod, 131, 134 grounded scalar damper, 98 grounded scalar mass, 93 grounded scalar spring, 97 infinite exterior acoustic, 195 lumped area beam, 115 lumped point mass, 94 p-formulation, 18, 209 P-Formulation bending panel, 183 P-Formulation Equivalent Section plate, 174 P-Formulation general section beam, 107 P-Formulation homogeneous plate, 161 P-Formulation Membrane, 201 P-Formulation Plane Strain Solid, 193 pipe section, 136 plotel, 146 revised bending panel, 181 revised equivalent section plate, 171 revised homogeneous plate, 158 revised laminate plate, 166 revised membrane, 199 revised plane strain solid, 191 scalar damping, 139 scalar mass, 144 scalar spring, 137 shear panel, 204 solid, 206 standard bending panel, 179 standard equivalent section plate, 168 standard homogeneous plate, 155 standard laminate plate, 163 standard membrane, 197 standard plane strain solid, 190 tapered beam, 119 viscous damper, 141 ELSDCON, 420
INDEX 585
Environment Variables ACommand20xx, 494 ACommandNasServer, 494 DRA_NAST_NOVEDRCHK, 494 MSCP_NASTRAN_SERVER, 494 MSP_NASTRAN_CMD20xx, 494 errors, 576 ESE, 419 executive control, 9
F
failure criteria, 81, 82 FEEDGE, 18 FEFACE, 20 files, 572 finite elements, 23, 24 FMS, 9 Foam model, 76 follower forces, 280 FORCE, 232, 233, 419 force, 226, 232 frequency response, 296
G
Gent model, 78 GEOM1, 510 GEOM2, 510 GMBC, 20 GMNURB, 14 GPFORCE, 420 GRAV, 236 GRDPNT, 283
I
inertia relief, 278, 474 inertial load, 236 initial conditions, 226, 237 initial load, 226 initial velocity, 226 input file, 546 INREL, 278, 474 INTENSITY, 419 IPSTRAIN, 14
ISTRESS, 14 iteration parameters, 391 iterations static nonlinear, 359
J
Jamus-Green-Simpson model, 75, 76
K
keywords POST, 315 REAUTO, 315, 461
L
large displacements, 280 LGDISP, 281 linear static, 277 linear surf-vol, 28 linear transient, 299 load cases, 246 loads and boundary conditions, 224
M
MARCIN, 14 MARCOUT, 14 Mass properties, non-structural (MSC.Nastran), 445 MAT1, 73, 81, 82 MAT2, 81, 82 MAT3, 73 MAT8, 73, 81, 82 MATEP, 14, 15, 78 materials, 59 2D anisotropic, 68, 73, 74 2D orthotropic, 65, 72 3D anisotropic, 68, 73, 74 3D orthotropic, 67, 72 composite, 68, 85 Fluid, 68 isotropic, 62, 69, 73, 74 MATF, 14, 15, 82 MATG, 14 MATHE, 14, 15, 75 MATORT, 14, 15, 73
586 Patran Interface to MD Nastran Preference Guide
MATS1, 74, 75, 78 MATTEP, 14, 15 MATTF, 82 MATTG, 14 MATTHE, 14, 15 MATTi, 73 MATTORT, 14 MATTVE, 14, 85 MATVE, 15, 85 MATVP, 15, 84 model data, 496 MOMENT, 232 Mooney-Rivlin model, 75, 76 MPC, 28, 31, 48 MSC.Nastran enhancements Non-structural mass properties, 445 MSC.Nastran version, 266, 267, 497, 498, 500 multi-point constraints, 27
N
Neo-Hookean, 76 NLAUTO, 15 NLDAMP, 15 NLLOAD, 419 NLPARM, 359 NLSTRAT, 15 nodes, 23, 266, 510 nonlinear elastic, 74 nonlinear statics, 279 nonlinear transient, 302 Non-Structural mass properties (MSC.Nastran), 445 normal nodes, 282 NSM and NSML forms (MSC.Nastran), 445 NTHICK, 15 numbering options, 268
O
OEF1, 502, 503 OESNL1, 503 Ogden model, 76 OLOAD, 419 ONRGY1, 505 OPG1, 505 OPHIG, 506
OPNL1, 506 optimize, 463 optimization parameters, 467 subcase create, 471 subcase parameters, 474 subcase select optimize, 475 topology optimization, 476 OSTR1, 502, 503 OUGV1, 505 output requests, 415 OUTPUT2, 265 OUTRCV, 20
P
PACINF, 195 PARAM, SNORM, 278, 283, 292, 297, 300, 324 PARAMARC, 15 PBAR, 103 PBCOMP, 115 PBEAM, 107, 120 PBEND, 110, 113 PCOMP, 82, 85, 164, 167 PDAMP, 98, 140 PELAS, 97, 138 penetration, 308 PGAP, 142 PLOAD4, 233 PLOADX1, 233 PMASS, 93, 145 POINT, 18 Postprocessing, 413 preferences, 6 pressure, 226, 233 PROD, 131 properties, 87 PSHEAR, 204 PSHELL, 155, 158, 168, 171, 179, 181, 190, 191, 198, 200 PSOLID, 206 PTUBE, 136 PVISC, 142
R
RBAR, 28, 34 rbar1, 50
INDEX 587
RBE1, 28, 36 RBE2, 29, 33, 38 RBE3, 29, 40 read input file, 546 reference coordinate frames, 23 RESTART, 15 restart file, 316, 462 results, 492 element, 436 nodal, 434 supported entities, 502, 516 types, 511 results output format, 348 RFORCE, 236 rjoint, 53 RLOAD1, 231 RROD, 29, 42 RSPLINE, 29, 44 RSSCON, 28 RTRPLT, 30, 46 rtrplt1, 51
S
SESET, 352 SETREE, 352 sliding surface, 30, 48 solution parameters, 277 SOL 109, 299 SOL 112, 299 SOL 27, 299 SOL 31, 299
solution sequences SOL 1, 272, 278 SOL 101, 272, 278 SOL 103, 273 SOL 105, 273, 287 SOL 106, 273, 279 SOL 107, 291 SOL 108, 273, 296 SOL 109, 273 SOL 110, 273, 291 SOL 111, 273, 296 SOL 112, 273 SOL 114, 272, 278 SOL 115, 273 SOL 118, 273, 296, 297 SOL 129, 273, 302 SOL 147, 273 SOL 26, 273, 296 SOL 27, 273 SOL 28, 273, 291 SOL 29, 273, 291 SOL 3, 273 SOL 30, 273, 296 SOL 37, 273 SOL 47, 272, 278 SOL 48, 273 SOL 5, 273, 287 SOL 600, 273, 304, 324, 326 SOL 66, 273, 279 SOL 77, 273, 287 SOL 99, 273, 302 solution types, 271 SPC1, 231 SPCD, 231 SPCFORCES, 419 SPCR, 232 static data, 226 STRAIN, 419, 420 STRESS, 419, 420 structural damping, 293, 301, 303 superelements, 267, 352 supported entities, 8
T
t16 file, 511, 543
588 Patran Interface to MD Nastran Preference Guide
TABLEDi, 231, 232 TABLEMi, 73 TABLES1, 75 TEMP, 235 temperature, 226, 235 TEMPP1, 235 TEMPRB, 235 TIC, 237 time dependent, 229 tolerances, 265, 496, 498, 500 TOPVAR, 479 translation parameters, 265, 496, 498 TSTEPNL, 362, 409
V
VECTOR, 419 VU mesh, 20
W
warnings, 576 WTMASS, 283
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 2009 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*2008R2*Z*INT-NA*Z* DC-USR
Contents Patran Interface to MD Nastran Preference Guide
Patran Interface MD Nastran Pre ence Guide,
1
Overview Purpose 2 Using Patran with SOL 700
2
MD Nastran Product Information
2
3
Building A Model Introduction to Building a Model
6
Currently Supported MD Nastran Input Options MD Nastran Implicit Nonlinear (SOL 600) 14 MD Nastran Explicit Nonlinear (SOL 700) 15 Materials 15 Loads and Boundary Conditions 17 Elements and Properties 17 Solution Controls 17
8
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference 18 Element Creation 18 Element and p-Formulation Properties 19 Loads and Boundary Conditions 19 Analysis Definition 20 Results Import and Postprocessing 20 Potential Pitfalls 21 Adaptive Analysis of Existing Models 21 Coordinate Frames
22
Finite Elements 23 Nodes 23 Elements 24 Multi-point Constraints 27 MPC Types 28 Degrees of Freedom 31 Superelements 56
ii Patran Interface to MD Nastran Preference Guide
Select Boundary Nodes 58 Material Library 59 Materials Application Form 59 Material Input Properties Form 61 Material Constitutive Models 62 Linear Elastic 73 Nonlinear Elastic 74 Hyperelastic 75 Elastoplastic 78 Failure 81 Failure 1, Failure 2, Failure 3 82 Creep 84 Viscoelastic 85 Composite 85 Element Properties 87 Element Properties Form 87 Coupled Point Mass (CONM1) 91 Grounded Scalar Mass (CMASS1) 93 Lumped Point Mass (CONM2) 94 Grounded Scalar Spring (CELAS1/CELAS1D) 96 Grounded Scalar Damper (CDAMP1/CDAMP1D) 98 Bush 99 General Section Beam (CBAR) 102 P-Formulation General Beam (CBEAM) 107 Curved General Section Beam (CBEND) 110 Curved Pipe Section Beam (CBEND) 113 Lumped Area Beam (CBEAM/PBCOMP) 115 Tapered Beam (CBEAM) 119 General Section Beam (CBEAM) 124 General Section Rod (CROD) 131 General Section Rod (CONROD) 134 Pipe Section Rod (CTUBE) 136 Scalar Spring (CELAS1/CELAS1D) 137 Scalar Damper (CDAMP1/CDAMP1D) 139 Viscous Damper (CVISC) 141 Gap (CGAP) 142 Scalar Mass (CMASS1) 144 PLOTEL 146 (Scalar) Bush 146 Spot Weld Connector (CWELD) 150 Fastener Connector (CFAST) 152 Standard Homogeneous Plate (CQUAD4) 155 Revised Homogeneous Plate (CQUADR) 158
CONTENTS iii
P-Formulation Homogeneous Plate (CQUAD4) 161 Standard Laminate Plate (CQUAD4/PCOMP) 163 Revised Laminate Plate (CQUADR/PCOMP) 166 Standard Equivalent Section Plate (CQUAD4) 168 Revised Equivalent Section Plate (CQUADR) 171 P-Formulation Equivalent Section Plate (CQUAD4) 174 Field Point Mesh (CQUAD4/TRIA3)(Exterior Acoustics) 177 Standard Bending Panel (CQUAD4) 179 Revised Bending Panel (CQUADR) 181 P-Formulation Bending Panel (CQUAD4) 183 Standard Axisymmetric Solid (CTRIAX6) 186 PLPLANE Axisymmetric Solid (CTRIAX, CQUADX) 187 2D Axi-Symmetric Laminated Solid Composite 188 Standard Plane Strain Solid (CQUAD4) 190 Revised Plane Strain Solid (CQUADR) 191 P-Formulation Plane Strain Solid (CQUAD4) 193 Infinite (Exterior Acoustic Element)(CACINF3/CACINF4) 195 2D Plane Strain Laminated Solid Composite 196 Standard Membrane (CQUAD4) 197 Revised Membrane (CQUADR) 199 P-Formulation Membrane (CQUAD4) 201 Shear Panel (CSHEAR) 204 Solid (CHEXA) 206 P-Formulation Solid (CHEXA) 209 Hyperelastic Plane Strain Solid (CQUAD4) 211 Hyperelastic Axisym Solid (CTRIAX6) 212 Hyperelastic Solid (CHEXA) 214 3D Laminate Solid (CHEXA) 215 Beam Modeling 217 Cross Section Definition 217 Create Action 217 Supplied Functions 219 Cross Section Orientation 220 Cross Section End Offsets 222 Stiffened Cylinder Example 222 Loads and Boundary Conditions 224 Loads & Boundary Conditions Form 224 Object Tables 231 Preview Rigid Body Motion 239 Slideline (SOL 400 and SOL 600) 240 Deformable Body (SOL 400, SOL 600, and SOL 700 ) 241 Select Discontinuities Subform 241
iv Patran Interface to MD Nastran Preference Guide
Edge Contact Subform 242 Select Contact Area 242 Select Exclusion Region 242 Select Deactivation Region 242 Rigid Body (SOL 600 and SOL 700 only) 243 Load Cases
246
Defining Contact Regions Contact 249
247
Rotor Dynamics 250 Rotor Dynamics Form 251 Spin Profile Form 252 Spin History Form 252 Unbalance Form 253 Unbalance Properties Form 255
3
Running an Analysis Review of the Analysis Form 260 Analysis Form 261 Overview of Analysis Job Definition and Submittal Translation Parameters 265 External Superelement Specifications Numbering Options 268 Select File 270 Solution Types Direct Text Input
271 276
Solution Parameters 277 Linear Static 277 Nonlinear Static 279 Normal Modes 282 Buckling 287 Complex Eigenvalue 291 Frequency Response 296 Transient Response 299 Nonlinear Transient 302 Implicit Nonlinear 304 Solver Options Subform (SOL 600) 306 Contact Parameters Subform 307
268
263
CONTENTS v
Restart Parameters Subform 315 Advanced Job Control Subform (SOL 600) 317 Domain Decomposition 318 DDAM 321 DDAM in Patran 322 Explicit Nonlinear 326 Sol700 Parameters Subform 327 Hourglass Setting Subform 329 Merge Rigid Material Subform 331 Dynamic Relaxation for Restart Subform 333 Damping Per Property Subform 335 Rigid Body Switch and Merge Subform 337 Define Set of Parts to be Switched Subform 340 Define Inertial Properties of Rigid Body Subform 342 Eulerian Parameters Subform 343 SPH Control Parameters Subform 346 Results Output Format 348 ADAMS Preparation 350 Select Superelements Subcases 354 Deleting Subcases Editing Subcases
352 355 356
Subcase Parameters 357 Linear Static Subcase Parameters 358 Nonlinear Static Subcase Parameters 359 Arc-Length Method Parameters 361 Nonlinear Transient Subcase Parameters 362 Normal Modes Subcase Parameters 364 Complex Eigenvalue Subcase Parameters 366 Transient Response Subcase Parameters 367 Frequency Response Subcase Parameters 370 Implicit Nonlinear Subcase Parameters 375 Static Subcase Parameters for Implicit Nonlinear Solution Type 376 Implicit Nonlinear Normal Modes Subcase Parameters 377 Implicit Nonlinear Buckling Subcase Parameters 377 Implicit Nonlinear Transient Dynamic Subcase Parameters 378 Implicit Nonlinear Creep Subcase Parameters 380 Implicit Nonlinear Body Approach Subcase Parameters 381 Implicit Nonlinear Complex Eigenvalue Subcase Parameters 382 Load Increment Parameters 383 Iteration Parameters 391 Contact Table 396
vi Patran Interface to MD Nastran Preference Guide
Breaking Glue Parameters Subform 400 Edge Contact Subform 401 402 Active/Deactive Elements 402 Break Squeal Parameters 403 Solvers/Options 404 DDAM Subcase Parameters 407 Explicit Nonlinear Subcase Parameters 409 Contact Table 411 Additional Contact Data 412 Adaptive Mesh Post-Processing 413 Additional Information 413 Output Requests 415 Basic Output Requests 416 Advanced Output Requests 417 Edit Output Requests Form 426 Default Output Request Information Subcases Direct Text Input 432 SOL 600 Output Requests 433 DDAM Output Requests 439 Mode by Mode Output 440 Select Explicit MPCs...
444
Non-Structural Mass Properties Select NSM Properties... Subcase Select
428
445
450
452
Restart Parameters
455
Optimize 463 Optimization Parameters 467 Subcases 471 Subcase Parameters 474 Subcase Select Optimize 475 Customized Solutions (Topology Optimization) Design Domain 479 Objectives & Constraints 479 Optimization Control 479 Postprocessing 479 Interactive Analysis Assumptions 480
480
476
CONTENTS vii
Scenario 1 480 Scenario 2 480 The Process 481 Miscellaneous 481 Analysis Form 482 Select Modal Results .DBALL 484 Loading Form 484 Create a Field Form 488 Output Selection Form 489 Define Frequencies Form 490
4
Read Results Accessing Results 492 Results File Formats 493 Output2 Formats 493 XDB Formats 493 MASTER Formats 494 T16/T19 Formats 495 3dplot Formats 495 Translation Parameters 496 OUTPUT2 496 Defining Translation Parameters for DDAM (SOL 187) 497 XDB 498 MASTER 499 T16/T19 501 Supported OUTPUT2 Result and Model Quantities Results 502 Global Variables 508 Coordinate Systems 509 Projected Global System 509 XY Plots 509 Model Data 510 Supported T16/T19 Results Quantities
511
Supported MSC.Access Result Quantities Nodal Results 516 Elemental Results 523 Supported 3dplot Results Quantities
543
516
502
viii Patran Interface to MD Nastran Preference Guide
5
Read Input File Review of Read Input File Form Read Input File Form 547 Entity Selection Form 548 Define Offsets Form 550 Selection of Input File 551 Summary Data Form 551 Reject Card Form 553
546
Data Translated from the NASTRAN Input File Partial Decks 554 Coordinate Systems 554 Referential Integrity 554 Chaining 555 Grids and SPOINTs 555 SPOINTs 555 Referential Integrity 555 Elements and Element Properties 555 PSHELL Properties 559 BAROR and BEAMOR Definitions 559 Fields 559 Referential Integrity 559 Set Name Extensions 559 Materials 560 MPCs 561 Load Sets 562 Fields 563 TABLES 564
554
Conflict Resolution 565 Conflict Resolution for Entities Identified by IDs 565 Conflict Resolution for Entities Identified by Names 565
6
Delete Review of Delete Form
568
Deleting an MD Nastran Job
7
Files Files
572
569
CONTENTS ix
8
Errors/Warnings Errors/Warnings
A
576
Preference Configuration and Implementation Software Components in Patran MD Nastran
578
Patran MD Nastran Preference Components
579
Configuring the Patran MD Nastran Execute File
Index
583
582
x Patran Interface to MD Nastran Preference Guide
Chapter 1: Overview Patran Interface to MD Nastran Preference Guide
1
Overview
Purpose
2
MD Nastran Product Information
3
2
Patran Interface to MD Nastran Preference Guide Purpose
1.1
Purpose Patran is an analysis software system developed and maintained by MSC.Software Corporation. The core of the system is a finite element analysis pre and postprocessor. Several optional products are available including; advanced postprocessing programs, tightly coupled solvers, and interfaces to third party solvers. This document describes one of these interfaces. The Patran MD Nastran interface provides a communication link between Patran and MD Nastran. It also provides for the customization of certain features in Patran. The interface is a fully integrated part of the Patran system. Selecting MD Nastran as the analysis code preference in Patran, activates the customization process. These customizations ensure that sufficient and appropriate data is generated for the Patran MD Nastran interface. Specifically, the Patran forms in these main areas are modified: • Materials • Element Properties • Finite Elements/MPCs and Meshing • Loads and Boundary Conditions • Analysis Forms
More information on these topics is contained in Preference Configuration and Implementation (App. A).
Using Patran with SOL 700 The amount of information that needs to be conveyed in the MD Nastran Input file for a SOL 700 analysis is extensive for even a modest size model. The amount of information and the complexity of most models makes it virtually impossible to generate the MD Nastran Input file with a text editor alone. Patran provides a graphical user interface, an extensive line of model building tools that you can use to construct and view your SOL 700 model, and generate a MD Nastran Input file for SOL 700. When using Patran as a preprocessor for SOL 700, you are required to specify an analysis code. Selecting MD Nastran Explicit Nonlinear (SOL 700) as the analysis code under the Analysis Preference menu, customizes Patran in five main areas: • Material Library • Element Library • Loads and Boundary Conditions • MPCs • Analysis forms
The analysis preference also specifies that the model information be output in the MD Nastran Input File format.
Chapter 1: Overview 3 MD Nastran Product Information
1.2
MD Nastran Product Information MD Nastran is a general-purpose finite element computer program for engineering analyses. It is developed, supported, and maintained by MSC.Software Corporation, 2 MacArthur Place, Santa Ana, California 92707, (714) 540-8900. See the MD Nastran Reference Manual, Volume 1, for a general description of MD Nastran’s capabilities.
4
Patran Interface to MD Nastran Preference Guide MD Nastran Product Information
Chapter 2: Building A Model Patran Interface to MD Nastran Preference Guide
2
Building A Model
Introduction to Building a Model
6
Currently Supported MD Nastran Input Options
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
Coordinate Frames
Finite Elements
23
Material Library
59
Element Properties
Beam Modeling
Loads and Boundary Conditions
Load Cases
Defining Contact Regions
Rotor Dynamics
22
87
217
246
250
247
224
8 18
6
Patran Interface to MD Nastran Preference Guide Introduction to Building a Model
2.1
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 code and analysis type. Other parts of the model are created using standard forms. The Analysis option on the Preferences menu brings up a form where the user can select the analysis code (e.g., MD Nastran) and analysis type (e.g., Structural).
The analysis code may be changed at any time during model creation.This is especially useful if the model is to be used for different analyses in different analysis codes. As much data as possible will be converted if the analysis code is changed after the modeling process has begun. The analysis option defines what will be presented to the user 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
Chapter 2: Building A Model 7 Introduction to Building a Model
allowable selections in these same areas. For more details, see The Analysis Form (Ch. 2) in the MSC.Patran Reference Manual.
To use the Patran MD Nastran Application should be set to MD Nastran.
The currently supported Analysis Type fo Nastran are Structural, Thermal and Expl
Indicates the file suffixes used in creating MD Nastran input and output files.
8
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
2.2
Currently Supported MD Nastran Input Options The following tables summarize all the various MD Nastran commands supported by the Patran MD Nastran Application Preference. The tables indicate where to find more information in this manual on how the commands are supported.
Chapter 2: Building A Model 9 Currently Supported MD Nastran Input Options
Supported MD Nastran File Management Commands
Table2-1.
Description
ASSIGN
An ASSIGN command is used to assign a particular name (job name + user specified MD Nastran results suffix) to the MD Nastran OUTPUT2 file to be created during the analysis.
Supported MD Nastran Executive Control Commands
Table 2-2.
Pages
ECHO
230, 233, 235, 241, 245, 250, 253, 256
SOL
225
TIME
230, 233, 235, 241, 245, 250, 253, 256
Supported MD Nastran Case Control Commands
Table 2-3.
Pages
ACCELERATION
250, 253
ACFPMRESULTS
369
ACPOWER
369
ADACT
17, 314
ADAPT
16, 170
DATAREC
17
DISPLACEMENT
230, 241, 250, 253
ELSDCON
230
ESE
230
FORCE
230, 235, 241, 248, 250, 253
FREQUENCY
250
GPSTRESS
369
INTENSITY
369
MAXLINES
230, 233, 235, 241, 245, 250, 253, 256
MPCFORCES OLOAD
369 230, 241, 250, 253
SPCFORCES
230, 235, 241, 248, 250, 253
STRAIN
230, 235, 241, 248, 250, 253
Supported MD Nastran Bulk Data Entries
10
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
Command ADAPT
Pages 16, 170, 225, 233
BEGIN AFPM
147
BEGIN SUPER
219
BCONP
212
BFRIC
212
BFRIC
212
CACINF3
160
CACINF4
160
CBARAO
86
CBAR
86
CBEAM
97, 100
CBEND
93, 95
CDAMP1
82
CDAMP2
219, 438
CELAS1
81
CELAS2
219, 438
CGAP
116
CHEXA
168
CMASS1
119
CMASS2
219, 438
CONM1
76
CONM2
79
CONROD
111
CPENTA
168
CQUAD4
124, 140, 148, 156, 162
CQUAD8
124, 140, 148, 156, 162
CQUADR
131, 142, 150, 157, 163
Command
Pages
CROD
110
CSHEAR
166
CTETRA
168
CTRIAX6
153
Chapter 2: Building A Model 11 Currently Supported MD Nastran Input Options
CTUBE
112
CVISC
115
DCONST
416
DOPTPRM
411, 416
DPHASE
188, 190
DRESP1/2
416
DTI, SETREE
309
DYNRED
240
EIGB
243, 238
EIGC
248
EIGR
238
EIGRL
238
EXTSEOUT
222
FEFACE
15
FEEDGE
15
FORCE
190
FREQ1
250
GMBC
188
GRAV
196
MOMENT
190
MAT1
424
MAT2
424
MAT3
424
MAT8
424
MAT9
424
MPC
28
NLPARM
315
OUTPUT
17, 369
PACINF
160
PARAM, AUTOSPC
230, 233, 235, 241, 245, 250, 253, 256
PARAM, INREL
230
PARAM, ALTRED
230
12
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
PARAM, COUPMASS PARAM, K6ROT
230, 233, 235, 241, 245, 250, 253, 256 230, 233, 235, 241, 245, 250, 253, 256
PARAM, WTMASS
230, 233, 235, 241, 245, 250, 253, 256
PARAM, GRDPNT
230, 233, 235, 241, 245, 250, 253, 256
PARAM, LGDISP
233, 256
PARAM,G
245, 250, 253, 256
PARAM,W3
253, 256
PARAM,W4
253, 256
PARAM, POST
219
PBAR
86
PBCOMP
97
PBEAM
100
PBEAM71 PBEAMD PBELTD PBEND
93, 95
PCOMP
136, 139
PDAMP
82
PELAS
81
PELAS1 PGAP
116
PLOAD1
199
PLOAD2
191
PLOAD4
191
PLOADX1 PLOTEL
191, 149 120
PLPLANE PLSOLID PMASS
119
POINT
15, 170
Chapter 2: Building A Model 13 Currently Supported MD Nastran Input Options
Pages PROD
110
PSHEAR
166
PSHELL
124, 131, 140, 142, 148, 150, 156, 157, 162, 163
PSHELL1 PSHELLD PSOLID
168
PSPRMA PTUBE
112
PBEAM
100
PVAL
15, 170
PVISC
115
RBAR
29
RBE1
31
RBE2
32
RBE3
33
RFORCE
196
RROD
34
RSPLINE
35
RTRPLT SESET
36 42, 219
SETREE
309
SPC1
188
SPCD
188
TEMP
193
TEMPF
146
TEMPRB
193
TEMPP1
193
TIC TSTEP TSTEPNL
197, 198 253 256, 318
14
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
MD Nastran Implicit Nonlinear (SOL 600) The following Bulk Data entries are supported for SOL 600 analyses. 3D Contact Region BCBODY
Defines a flexible rigid contact body in 2D or 3D.
BCBOX*
Defines a 3D contact region.
BCHANGE
Changes definitions of contact bodies.
BCMATL*
Defines a 3D contact region by element material.
BCMOVE
Defines movement of bodies in contact.
BCPARA
Defines contact parameters.
BCPROP*
Defines a 3d contact region by element properties.
BCTABLE
Defines a contact table.
BSURF
Defines a contact body or surface by element IDs.
GMNURB
3D contact region made up of NURBS.
Initial Conditions IPSTRAIN*
Defines initial plastic strain values.
ISTRESS*
Defines initial stress values.
MARCIN
Insert a text string in MSC.Marc.
MARCOUT
Selects data recovery output.
Materials
MATEP
Elasto-plastic material properties.
MATF
Specifies material failure model.
MATG*
Gasket material properties.
MATHE
Hyperelastic material properties.
MATHP
Hyperelastic material properties.
MATHED
Damage model properties for hyperelastic materials.
MATORT
Elastic 3D orthotropic material properties.
MATTEP
Thermoelastic-Plastic material properties.
MATTG*
Temperature variation of interlaminar materials.
MATTHE
Thermo hyperelastic material.
MATTORT*
Thermoelastic orthotropic material
MATTVE*
Thermo-visco-elastic material properties
Chapter 2: Building A Model 15 Currently Supported MD Nastran Input Options
MATVE*
Viscoelastic material properties
MATVP
Viscoplastic or creep material properties
Note:
* Not supported in initial release of Patran (2004).
Note:
Solution Control
NLAUTO
Parameters for automatic load/time stepping.
NLDAMP
Defines damping constants.
NLSTRAT
Strategy Parameters for nonlinear structural analysis.
PARAMARC
Parallel domain decomposition.
RESTART
Restart data.
Note: Note: NTHICK
Element Properties
Defines nodal thickness values for beams, plates, and/or shells.
MD Nastran Explicit Nonlinear (SOL 700) The following Bulk Data entries are supported for SOL 700 analyses. Materials MATD001
Isotropic Elastic material for beam, shell and solid.
MATD003
Isotropic and kinematic hardening plasticity.
MATD005
Isotropic materials to model soil and foam.
MATD006
Isotropic viscoelastic material.
MATD007
Isotropic material to model nearly incompressible continuum rubber.
MATD012
Isotropic plasticity for 3D solids.
MATD014
Isotropic materials to model soil and foam with failure.
MATD015
Isotropic Johnson/Cook strain and temperature sensitive plasticity.
MATD019
Isotropic strain rate dependent material.
MATD020
Isotropic rigid material.
MATD022
Orthotropic material with optional brittle failure for composites.
MATD024
Isotropic elasto-plastic material with stress x strain curve and strain rate dependency.
MATD026
Anisotropic honeycomb and foam material.
MATD027
Isotropic material to model rubber using two variables.
MATD028
Isotropic elasto-plastic material for beam and shell.
16
Patran Interface to MD Nastran Preference Guide Currently Supported MD Nastran Input Options
MATD030
Isotropic superelastic material.
MATD031
Isotropic material to model rubber using the Frazer-Nash formulation.
MATD032
Orthotropic laminated glass material.
MATD057
Isotropic material to model highly compressible low density foams.
MATD058
*MAT_LAMINATED_COMPOSITE_FABRIC
MATD062
Isotropic material to model viscous foams.
MATD063
Isotropic material to model crushable foams.
MATD064
Isotropic elasto-plastic material with a power law hardening.
MATD067
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM
MATD068
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM
MATD069
*MAT_SID_DAMPER_DISCRETE_BEAM
MATD070
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM
MATD071
*MAT_CABLE_DISCRETE_BEAM
MATD073
*MAT_LOW_DENSITY_VISCOUS_FOAM
MATD074
*MAT_ELASTIC_SPRING_DISCRETE_BEAM
MATD076
*MAT_GENERAL_VISCOELASTIC
MATD083
*MAT_FU_CHANG_FOAM
MATD087
*MAT_CELLULAR_RUBBER
MATD093
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM
MATD094
*MAT_INELASTIC_SPRING_DISCRETE_BEAM
MATD095
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM
MATD097
*MAT_GENERAL_JOINT_DISCRETE_BEAM
MATD100
Isotropic spotweld material.
MATD103
Anisotropic viscoplastic material.
MATD119
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM
MATD121
*MAT_GURSON_RCDC
MATD126
*MAT_MODIFIED_HONEYCOMB
MATD20M
*MAT_RIGID
MATDB01
*MAT_SEATBELT
MATDS01
*MAT_SPRING_ELASTIC
MATDS02
*MAT_DAMPER_VISCOUS
MATDS03
*MAT_SPRING_ELASTOPLASTIC
MATDS04
*MAT_SPRING_NONLINEAR_ELASTIC
MATDS05
*MAT_DAMPER_NONLINEAR_VISCOUS
Chapter 2: Building A Model 17 Currently Supported MD Nastran Input Options
MATDS06
*MAT_SPRING_GENERAL_NONLINEAR
MATDS07
*MAT_SPRING_MAXWELL
MATDS08
*MAT_SPRING_INELASTIC
MATDS13
*MAT_SPRING_TRILINEAR_DEGRADING
MATDS14
*MAT_SPRING_SQUAT_SHEARWALL
MATDS15
*MAT_SPRING_MUSCLE
Loads and Boundary Conditions TIC3
Defines initial rotational field.
WALL
Defines planar rigid wall.
Elements and Properties CDAMP1D
Scalar damper connection for SOL 700
CELAS1D
Scalar spring connection for SOL 700.
Solution Controls Form
Parameters
Execution Control Parameters
DYSTATIC, DYBLDTIM, DYINISTEP, DYTSTEPERODE, DYMINSTEP, DYMAXSTEP, DYSTEPFCTL, DYTERMNENDMAS, DYTSTEPDT2MS
General Parameters
DYLDKND, DYCOWPRD, DYCOWPRP, DYBULKL, DYHRGIHQ, DYRGQH, DYENERGYHGEN, DYSHELLFORM, DYSHTHICK, DYSHNIP
Contact Parameters
DYCONSLSFAC, DYCONRWPNAL, DYCONPENOPT, DYCONTHKCHG, DYCONENMASS, DYCONECDT, DYCONIGNORE, DYCONSKIPTWG
Binary Output Database File Parameters
DYBEAMIP, DYMAXINT, DYNEIPS, DYNINTSL, DYNEIPH, DYSTRFLG, DYSIGFLG, DYEPSFLG, DYRLTFLG, DYENGFLG, DYCMPFLG, DYIEVERP, DYDCOMP, DYSHGE, DYSTSSZ, DYN3THDT
DAMPGBL
Dynamic relaxation control.
18
Patran Interface to MD Nastran Preference Guide
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
2.3
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference In Version 68 of MSC. Nastran, MSC introduced p-adaptive analysis using solid elements. The Patran MD Nastran Preference provides support for this new capability. There are some fundamental differences in approach to model building and results import for p-element analyses; this section will serve as a guide to these. MSC .Nastran Version 69 extends the Version 68 capabilities for p-adaptive analysis in two areas. Shell and beam elements have been added and p-shells and p-beams can be used for linear dynamic solution sequences. Patran Version 6.0 supports both of these capabilities. Element Creation MD Nastran supports adaptive, p-element analyses with the 3D-solid CTETRA, CPENTA, and CHEXA elements; 2D-solid TRIA, and QUAD elements; shells TRIA, and QUAD elements; beams BAR elements. Patran and MD Nastran allow TET4, TET10, TET16, TET40, WEDGE6, WEDGE15, WEDGE52, HEX8, HEX20, and HEX64 for p-adaptive analysis for 3D-solids; TRIA3, TRIA6, TRIA7, TRIA9, TRIA13, QUAD4, QUAD8, QUAD9, QUAD12, and QUAD16 for p-adaptive analysis for 2Dsolids and membranes; TRIA3, TRIA6, TRIA7, TRIA9, TRIA13, QUAD4, QUAD8, QUAD9, QUAD12, and QUAD16 for p-adaptive analysis for shells; BAR2, BAR3, and BAR4 for p-adaptive analysis for beams. The preferred approach, when beginning a new model, is to use the higher-order elements--HEX64, WEDGE52, TET40, and TET16, or TRIA13 and QUAD16, or BAR4. The support for lower-order elements is provided primarily to support existing models. The higher-order cubic elements allow more accurate definition of the geometry and more accurate postprocessing of results from the MD Nastran analysis.The translator generates the appropriate MD Nastran FEEDGE and POINT entities for all curved edges on the p-elements. Models with HEX64 and WEDGE52 elements are easily created with the Patran Iso Mesher; models with TET16 elements can be created with the Tet Mesher. Models with QUAD16 and TRIA13 elements can be created using the Iso Mesher or the Paver. For p-elements, Patran generates cubic edges to fit the underlying geometry. The cubic edge consists of two vertex grid points and two points in between. Adjacent cubic edges are not necessarily C1 continuous. If the original geometry is smooth, the cubic edges may introduce kinks which cause false stress concentrations. Then, the p-element produces unrealistic results especially for thin curved shells. In Version 7 of Patran, for cubic elements, the two midside nodes on each edge are adjusted so that the edges of adjacent elements are C1 continuous. The adjustment is done in the Pat3Nas translator. After the Pat3Nas translator is executed, the location of the two midside nodes in the Patran database has changed. The user is informed with a warning message. The user can turn the adjustment of midside nodes ON and OFF with the environment variable PEDGE_MOVE. By default, the midside nodes are adjusted to make the adjacent elements C1 continuous. For PEDGE_MOVE set to OFF, the points on a cubic edge are not adjusted. Patran generates the input for MD Nastran. For cubic edges, FEEDGE Bulk Data entries with POINTs are written. By default, the location of the two POINTs is moved to 1/3 and 2/3 of the edge in MD Nastran. The points generated by Patran must not be moved. Therefore, a parameter entry PARAM, PEDGEP, 1 is written by Patran. PEDGEP=1 indicates that incoming POINTs are not moved in MD
Chapter 2: Building A Model 19 Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
Nastran. The default is PEDGEP= 0, MD Nastran will move the two POINTs to 1/3 and 2/3 of the edge. The C1 continuous cubic edges improve the accuracy of p-element results. In the Version 69 Release Guide, a cylinder under internal pressure was tested to determine the quality of shell p-elements for curved geometry. The accuracy of the results was very good when exact geometry was used. With C1 continuous edges we recover the same quality of results within single precision accuracy. Element and p-Formulation Properties Both element and p-formulation properties are defined using the Element Properties application by choosing Action: Create, Dimension: 1D/2D/ or 3D, Type: Beam/Shell/Bending Panel/2D Solid/Membrane/ or Solid, and p-Formulation on the main form. The details of the property form for this case are described on (p. 209). Most of the properties are optional and have defaults; the material property name is required. Two properties that may need to be defined are Starting P-orders and Maximum P-orders. These properties specify the polynomial orders for the element interpolation functions in the three spatial directions. Although these are integer values, in Patran, each property is defined using the Patran vector definition. At first, this may seem peculiar, but it gives the user access to many useful tools in the Patran system for defining and manipulating these properties. Typically, a user would define these properties with a syntax like <3 4 2> to prescribe polynomial orders of 3, 4, and 2 in the X, Y, and Z directions. Patran will convert these values to floating point <3. 4. 2.>, but the Patran MD Nastran Preference will interpret them. This vector syntax is convenient primarily because it allows these properties to be defined using the Fields application. In a case where the material properties are constant over the model, but it is desirable to prescribe a distribution of p-orders, vector fields can be defined and specified in a single property definition. The Patran MD Nastran Preference will provide additional help for this modeling function. At the end of an adaptive analysis, when results are imported, vector, spatial fields will optionally be created containing the p-orders used for each element for each adaptive cycle. To repeat a single adaptive cycle, it is necessary only to modify the element properties by selecting the appropriate field. A common use of the Maximum P-orders property is in dealing with elements in the vicinity of stress singularities. These singularities may be caused by the modeling of the geometry (e.g., sharp corners), boundary conditions (e.g., point constraints), or applied forces (e.g., point forces). Sometimes it is easier to tell the adaptive analysis to “ignore” these singular regions than it is to change the model. This can be done by setting the Maximum P-orders property for elements in this region to low values (e.g., <1 1 1> or <2 2 2>. These elements are sometimes called “sacrificial” elements. Loads and Boundary Conditions It is well known in solid mechanics that point forces and constraints cause the stress field in the body to become infinite. In p-adaptive analyses, care must be taken in finite element creation and loads application to ensure that these artificial high-stress regions don’t dominate the analysis. Generally, the best results are obtained with distributed loads (pressures) or distributed displacements. There are two options under Loads/BCs for applying distributed displacements. The Element Uniform and Element Variable types under Displacements allow displacement constraints to be applied to the
20
Patran Interface to MD Nastran Preference Guide
Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
faces of solid elements. If the elements are p-elements, the appropriate FEFACE and GMBC entries are produced. If applied to non-p-elements, the appropriate SPC1 or SPCD entries are produced. Several new loads and boundary conditions support the p-shell and p-beam elements. Distributed loads can be applied to beam elements or to the edge of shell elements. Pressure loads can be applied to the faces of p-shell elements. Temperature loads can be applied to either the nodes or the elements. Analysis Definition Adaptive linear static and normal modes analyses are supported in Version 68 of MSC .Nastran; both solution types are supported by the Patran MD Nastran Preference. Only a few parameters on the Analysis forms may need to be changed for p-element analyses. If running a version of MSC . Nastran prior to Version 68.2 (i.e., Version 68, or 68.1), the OUTPUT2 Request option on the Translation Parameters form must be set to Alter File in order to process the results in Patran. The Solution Parameters forms for the linear static and normal modes analyses contain a Max p-Adaptive Cycles option, which is defaulted to 3. The Subcase Parameters form under Subcase Create has options to limit the participation of this subcase in the adaptive error analysis. Finally, the Advanced Output Requests form under Subcase Create has an option to define whether results are to be produced for all adaptive cycles or only every nth adaptive cycle. Results Import and Postprocessing Two different approaches are provided for postprocessing results from MD Nastran p-element analyses. Both approaches rely on MD Nastran creating results for a “VU mesh” where each p-element is automatically subdivided into a number of smaller elements. In the standard approach with the default MD Nastran VU mesh (3 x 3 x 3 elements) for solids, (3 x 3 elements) for shells and (3 elements) for beams, the results will automatically be mapped onto the Patran nodes and elements during import. This mapping will occur for all 10, Patran solid element topologies mentioned above. The most accurate mapping and postprocessing takes place when results are mapped to the higher-order Patran elements. When the adaptive analysis process increases the p-orders in one or more elements beyond 3, the 3 x 3 x 3 VU mesh, mapping, and postprocessing may not be sufficiently accurate. The Patran MD Nastran Preference provides a second approach to handle this situation. In this case, a user can specify a higherorder VU mesh (e.g. 5 x 5 x 5) on the MD Nastran OUTRCV entry and then import both model data and results entities into a new, empty Patran database. In this case, the VU mesh and results are imported directly, rather than mapped and can be post-processed with greater accuracy. The OUTRCV entry is currently supported only with the Bulk Data Include File option on the Translation Parameters form. It should be noted that, with this import mode, displays of element results (e.g., fringe plots) may be discontinuous across parent, p-element boundaries. This occurs because the VU grids generated by MD Nastran are different in each p-element. Along element boundaries there are coincident nodes and a result associated with each one. The user should not try to perform an Equivalence operation to remove these coincident nodes. If this is done, subsequent postprocessing operations will likely be incorrect. For both postprocessing options, a result case is created for each adaptive cycle in the analysis. The result types in this result case will depend on specific options selected on the Output Request form. By default, the Adaptive Cycle Output Interval option is equal to zero. This means that output quantities specific to
Chapter 2: Building A Model 21 Adaptive (p-Element) Analysis with the Patran MD Nastran Preference
p-elements will be written only for the last cycle. If postprocessing of results from intermediate cycles is desired, the Adaptive Cycle Output Interval option should be set equal to one. One of the key uses of output from intermediate adaptive cycles is in examining the convergence of selected quantities (e.g., stresses). This can be done using the X-Y plotting capability under the Results application. Potential Pitfalls There are several areas where a user can encounter problems producing correct p-element models for MD Nastran. One is the incorrect usage of the midside nodes in the Patran higher order-elements. These nodes are used in p-element analysis only for defining the element geometry; analysis degrees of freedom are not associated with these nodes. Therefore it is illegal, for example, to attach non p-elements to assign loads or boundary conditions to these nodes. One way this can occur inadvertently is if a nodal force is applied to the face of a Patran solid. This force is interpreted as a point force at every node (including the midside nodes) on the face of the solid. For the p-elements, this is not valid. This type of load should instead be applied as an element uniform or element variable pressure. Adaptive Analysis of Existing Models Modifying an existing solid model for adaptive, p-element analysis is relatively straightforward. The first step is to read the NASTRAN input file into Patran using the Analysis/Read Input File option. The model may contain any combination of linear or quadratic tetra, penta, or hexa elements. The second step is to use the Element Props/Modify function to change the Option for all solid properties from Standard Formulation to P-Formulation. The element properties form for p-formulation solids has many options specific to p-element analysis; but they all have appropriate defaults. This property modification step is the only change that must be made before submitting the model for analysis. Often, however, as discussed in Potential Pitfalls, 21, it is appropriate to modify the types of loads and boundary conditions applied to the model. For example, in non p-element models, displacement constraints are applied using MD Nastran SPC entries at grid points. In p-element analyses, elementoriented displacement constraints are more appropriate. Existing displacement LBCs can be modified using the Loads/BCs/Modify/Displacement option. For an SPC type of displacement constraint, the LBC type is nodal. For a p-element analysis, Element Uniform or Element Variable displacement constraints are more appropriate. The application region must be changed from a selection of nodes to a selection of element faces. As described above, nodal forces can be troublesome in p-element analyses. If possible, it is beneficial to redefine point forces as pressures acting on an element face. If this is not possible, an alternative is to limit the p-orders in the elements connected to the node with the point force; this can be done by defining a new element property for these elements and defining the Maximum P-orders vector appropriately. Element pressures, inertial loads, and nodal temperatures defined in the original model need not be changed for the p-element analysis.
22
Patran Interface to MD Nastran Preference Guide Coordinate Frames
2.4
Coordinate Frames Coordinate frames will generate a unique CORD2R, CORD2C, or CORD2S Bulk Data entry, depending on the specified coordinate frame type. The CID field is defined by the Coord ID assigned in Patran. The RID field may or may not be defined, depending on the coordinate frame construction method used in Patran. The A1, A2, A3, B1, B2, B3, C1, C2, and C3 fields are derived from the coordinate frame definition in Patran.
Only Coordinate Frames that are referenced by nodes, element properties, or loads and boundary conditions can be translated. For more information on creating coordinate frames see Creating Coordinate Frames (p. 393) in the Geometry Modeling - Reference Manual Part 2. To output all the coordinate frames defined in the model whether referenced or not, set the environment variable “WRITE_ALL_COORDS” to ON.
Chapter 2: Building A Model 23 Finite Elements
2.5
Finite Elements The Finite Elements Application in Patran allows the definition of basic finite element construction. Created under Finite Elements are the nodes, element topology, multi-point constraints, and Superelement.
For more information on how to create finite element meshes, see Mesh Seed and Mesh Forms (p. 25) in the Reference Manual - Part III.
Nodes Nodes in Patran will generate unique GRID Bulk Data entries in MD Nastran. Nodes can be created either directly using the Node object, or indirectly using the Mesh object. Each node has associated Reference (CP) and Analysis (CD) coordinate frames. The ID is taken directly from the assigned node
24
Patran Interface to MD Nastran Preference Guide Finite Elements
ID. The X1, X2, and X3 fields are defined in the specified CP coordinate frame. If no reference frame is assigned, the global system is used. The PS and SEID fields on the GRID entry are left blank.
The analysis frame (CD of the GRID) is the coordinate system in which the displacements, degrees of freedom, constraints, and solution vector are defined. The coordinate system in which the node location is defined (CP of the GRID) can be either the reference coordinate frame, the analysis coordinate frame, or a global reference (blank), depending on the value of the forward translation parameter “Node Coordinates.”
Elements The Finite Elements Application in Patran assigns element connectivity, such as Quad4, for standard finite elements. The type of MD Nastran element to be created is not determined until the element properties are assigned (for example, shell or 2D solid). See the Element Properties Form, 87 for details concerning the MD Nastran element types. Elements can be created either directly using the Element object, or indirectly using the Mesh object
Chapter 2: Building A Model 25 Finite Elements
.
26
Patran Interface to MD Nastran Preference Guide Finite Elements
This type of form is used to create a 1D, 2D, or 3D element mesh.
Beginning IDs for nodes and elements to be created. Elem Shape is used to specify the shape of the elements created by meshing. For example, the shape for a 2D element can be either triangular or quadralateral. Mesher is used to specify how the element mesh is to be created; for example, IsoMesh, Paver. The type of geometry (for example, simple (green) or complex (magenta) surface) may determine the choice of the mesher.
List of surface IDs of surfaces to be meshed. For example Surface 1, 2, 3, or Surface 1:3. The value of Global Edge Length specifies the approximate size of the elements created when meshing. The button Select Existing Prop... is used to select an existing element property (for example, 2D Shell) that will be assigned to the elements created by meshing. The button Create New Property is used to create an element property that will be assigned to the elements that will be created by meshing. During creating the element property no application region can be specified; it is specified automatically using all the elements created by meshing. This “ghosted” area will become dark when an element property is selected.
Chapter 2: Building A Model 27 Finite Elements
Multi-point Constraints Multi-point constraints (MPCs) can also be created from the Finite Elements Application. These are special element types that 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).
Used to specify the ID to associate to the MPC when it is created.
28
Patran Interface to MD Nastran Preference Guide Finite Elements
MPC Types To create an MPC, first select the type of MPC to be created from the option menu. The MPC types that appear in the option menu are dependent on the current settings of the Analysis Code and Analysis Type preferences. The following table describes the MPC types which are supported for MD Nastran. MPC Type
Analysis Type
Description
Explicit
Structural
Creates 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 can be specified, while only one dependent term can be specified. The constant term is not allowed in MD Nastran.
RSSCON Surf-Vol
Structural
Creates an RSSCON 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.
Rigid (Fixed)
Structural and Explicit Nonlinear
Creates a rigid 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 can be specified, while only one independent term can be specified. Each term consists of a single node. There is no constant term for this MPC type.
RBAR
Structural and Explicit Nonlinear
Creates an RBAR element, which defines a rigid bar between two nodes. Up to two dependent and two independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the two dependent terms must be the same as the nodes specified in the two independent terms. Any combination of the degrees of freedom of the two nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
RBE1
Structural
Creates an RBE1 element, which defines a rigid body connected to an arbitrary number of nodes. An arbitrary number of dependent terms can be specified. Each term consists of a node and a list of degrees of freedom. Any number of independent terms can be specified as long as the total number of degrees of freedom specified in all of the independent terms adds up to six. Since at least one degree of freedom must be specified for each term there is no way the user can create more that six independent terms. There is no constant term for this MPC type.
Chapter 2: Building A Model 29 Finite Elements
MPC Type
Analysis Type
Description
RBE2
Structuraland Explicit Nonlinear
Creates an RBE2 element, which defines a rigid body between an arbitrary number of nodes. Although the user can only specify one dependent term, an arbitrary number of nodes can be associated to this term. The user is also prompted to associate a list of degrees of freedom to this term. A single independent term can be specified, which consists of a single node. There is no constant term for this MPC type.
RBE3
Structuraland Explicit Nonlinear
Creates an RBE3 element, which defines the motion of a reference node as the weighted average of the motions of a set of nodes. An arbitrary number of dependent terms can be specified, each term consisting of a node and a list of degrees of freedom. The first dependent term is used to define the reference node. The other dependent terms define additional node/degrees of freedom, which are added to the m-set. An arbitrary number of independent terms can also be specified. Each independent term consists of a constant coefficient (weighting factor), a node, and a list of degrees of freedom. There is no constant term for this MPC type.
RROD
Structural
Creates an RROD element, which defines a pinned rod between two nodes that is rigid in extension. One dependent term is specified, which consists of a node and a single translational degree of freedom. One independent term is specified, which consists of a single node. There is no constant term for this MPC type.
RSPLINE
Structural
Creates an RSPLINE element, which interpolates the displacements of a set of independent nodes to define the displacements at a set of dependent nodes using elastic beam equations. An arbitrary number of dependent terms can be specified. Each dependent term consists of a node, a list of degrees of freedom, and a sequence number. An arbitrary number of independent nodes (minimum of two) can be specified. Each independent term consists of a node and a sequence number. The sequence number is used to order the dependent and independent terms with respect to each other. The only restriction is that the first and the last terms in the sequence must be independent terms. A constant term, called D/L Ratio, must also be specified.
30
Patran Interface to MD Nastran Preference Guide Finite Elements
MPC Type
Analysis Type
Description
RTRPLT
Structural
Creates an RTRPLT element, which defines a rigid triangular plate between three nodes. Up to three dependent and three independent terms can be specified. Each term consists of a node and a list of degrees of freedom. The nodes specified in the three dependent terms must be the same as the nodes specified in the three independent terms. Any combination of the degrees of freedom of the three nodes can be specified as independent as long as the total number of independent degrees of freedom adds up to six. There is no constant term for this MPC type.
Cyclic Symmetry
Structural
Describes cyclic symmetry boundary conditions for a segment of the model. If a cyclic symmetry solution sequence is chosen, such as “SOL 114,” then CYJOIN, CYAX and CYSYM entries are created. If a solution sequence that is not explicitly cyclic symmetric is chosen, such as “SOL 101,” MPC and SPC entries are created. Be careful, for this option automatically alters the analysis coordinate references of the nodes involved. This could erroneously change the meaning of previously applied load and boundary conditions, as well as element properties.
Sliding Surface
Structural
Describes the boundary conditions of sliding surfaces, such as pipe sleeves. These boundary conditions are written to the NASTRAN input file as explicit MPCs. Be careful, for this option automatically redefines the analysis coordinate references of all affected nodes. This could erroneously alter the meaning of previously applied load and boundary conditions, as well as element properties.
RBAR1
Structural
This is an alternate (simplified) form for RBAR. Creates an RBAR1 element, which defines a rigid bar between two nodes, with six degrees of freedom at each end. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
Chapter 2: Building A Model 31 Finite Elements
MPC Type
Analysis Type
Description
RTRPLT1
Structural
Alternative format to define a rigid triangular plate element connecting three grid points. Creates an RTRPLT1 element, which defines a rigid triangular plate between three nodes. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of the node (with all six degrees of freedom implied). The constant term is the thermal expansion coefficient, ALPHA.
RJOINT
Structural
Creates an RJOINT element, which defines a rigid joint element connecting two coinciding grid points. Each dependent term consists of a node and a list of degrees of freedom, while the independent term consists only of a node (with all six degrees of freedom implied). There is no constant term for this MPC type.
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. The following degrees of freedom are supported by the Patran MD Nastran MPCs for the various analysis types: Degree of freedom
Analysis Type
UX
Structural
UY
Structural
UZ
Structural
RX
Structural
RY
Structural
RZ
Structural
Note:
Care must be taken to make sure that a degree of freedom that is 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 degrees of freedom at this node when defining an MPC.
Explicit MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Explicit is the selected type. This form is used to create an MD Nastran MPC Bulk Data entry. The difference in explicit MPC equations between Patran and MD Nastran will result in the A1 field of the MD Nastran entry being set to -1.0.
32
Patran Interface to MD Nastran Preference Guide Finite Elements
Holds the dependent term information. This term will define the fields for G1 and C1 on the MPC entry. Only one node and DOF combination may be defined for any given explicit MPC. The A1 field on the MPC entry is automatically set to -1.0.
Holds the independent term information. These terms define the Gi, Ci, and Ai fields on the MPC entry, where i is greater than one. As many coefficient, node, and DOF combinations as desired may be defined.
Chapter 2: Building A Model 33 Finite Elements
Rigid (Fixed)
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and Rigid (Fixed) is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry. The CM field on the RBE2 entry will always be 123456.
Holds the dependent term information. This term defines the GMi fields on the RBE2 entry. As many nodes as desired may be selected as dependent terms.
Holds the independent term information. This term defines the GN field on the RBE2 entry. Only one node may be selected.
34
Patran Interface to MD Nastran Preference Guide Finite Elements
RBAR MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBAR is the selected type. This form is used to create an MD Nastran RBAR Bulk Data entry and defines a rigid bar with six degrees of freedom at each end. Both the Dependent Terms and the Independent Terms lists can have either 1 or 2 node references. The total number of referenced nodes,
Chapter 2: Building A Model 35 Finite Elements
however, must be 2. If either or both of these lists references 2 nodes, then there must be an overlap in the list of referenced nodes.
Holds the dependent term information. Either one or two nodes may be defined as having dependent terms. The Nodes define the GA and GB fields on the RBAR entry. The DOFs define the CMA and CMB fields.
Holds the independent term information. Either one or two nodes may be defined as having independent terms.The Nodes define the GA and GB fields on the RBAR entry.The DOFs define the CNA and CNB fields.
36
Patran Interface to MD Nastran Preference Guide Finite Elements
RBE1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE1 is the selected type. This form is used to create an MD Nastran RBE1 Bulk Data entry.
Chapter 2: Building A Model 37 Finite Elements
Holds the dependent term information. Defines the GMi and CMi fields on the RBE1 entry. An unlimited number of nodes and DOFs may be defined here.
Holds the independent term information. Defines the GNi and CNi fields on the RBE1 entry. The total number of Node/DOF pairs defined must equal 6, and be capable of representing any general rigid body motion.
38
Patran Interface to MD Nastran Preference Guide Finite Elements
RBE2 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE2 is the selected type. This form is used to create an MD Nastran RBE2 Bulk Data entry.
Chapter 2: Building A Model 39 Finite Elements
Holds the dependent term information. This term defines the GMi and CM fields on the RBE2 entry. As many nodes as desired may be selected as dependent terms.
Holds the independent term information. This term defines the GN field on the RBE2 entry. Only one node may be selected.
RBE3 MPCs
40
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RBE3 is the selected type. This form is used to create a MD Nastran RBE3 Bulk Data entry.
Chapter 2: Building A Model 41 Finite Elements
Holds the dependent term information. Defines the GMi and CMi fields on the RBE3 entry. The first dependent term will be treated as the reference node, REFGRID and REFC. The rest of the dependent terms become the GMi and CMi components.
Holds the independent term information. Defines the Gi, j, Ci, and WTi fields on the RBE3 entry.
RROD MPCs
42
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RROD is the selected type. This form is used to create an MD Nastran RROD Bulk Data entry.
Chapter 2: Building A Model 43 Finite Elements
Holds the dependent term information. Defines the GB and CMB on the RROD entry. Only one translational DOF may be referenced for this entry.
Holds the independent term information. Defines the GA field on the RROD entry. The CMA field is left blank.
44
Patran Interface to MD Nastran Preference Guide Finite Elements
RSPLINE MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RSPLINE is the selected type. This form is used to create an MD Nastran RSPLINE Bulk Data entry. The D/L field for this entry is defined on the main MPC form. This MPC type is typically used to tie together two dissimilar meshes.
Chapter 2: Building A Model 45 Finite Elements
Holds the dependent term information.
Holds the independent term information. Terms with the highest and lowest sequence numbers must be independent.
Determines what sequence the independent and dependent terms will be written to the RSPLINE entry.
RTRPLT MPCs
46
Patran Interface to MD Nastran Preference Guide Finite Elements
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT is the selected type. This form is used to create an MD Nastran RTRPLT Bulk Data entry.
Chapter 2: Building A Model 47 Finite Elements
Holds the dependent term information. Defines the GA, GB, GC, CMA, CMB, and CMC fields of the RTRPLT entry.
Holds the independent term information. The total number of nodes referenced in both the dependent terms and the independent terms must equal three. There must be exactly six independent degrees of freedom, and they must be capable of describing rigid body motion. Defines the GA, GB, GC, CNA, CNB, and CNC fields of the RTRPLT entry.
Cyclic Symmetry MPCs
48
Patran Interface to MD Nastran Preference Guide Finite Elements
The Cyclic Symmetry MPC created by this form will be translated into CYJOIN, CYAX, and CYSYM entries if cyclic symmetric is the selected type, see Solution Parameters, 277, or into SPC and MPC entries if the requested type is not explicitly cyclic symmetric.
If the type selected is Cyclic Symmetry, the type of symmetry will always be rotational. NOTE: MPC option will automatically overwrite the analysis coordinate references on all the nodes belonging to the Dependent and Independent Regions. Be careful that this does not erroneously change the meaning of previously applied loads and boundary conditions, or element properties.
Any node lying on the Z axis will be automatically written to the CYAX entry.
Side 2 of the CYJOIN entries. Side 1 of the CYJOIN entries.
Sliding Surface MPCs
The Sliding Surface MPC created by this form will be translated into explicit MPCs in the NASTRAN input file.
Chapter 2: Building A Model 49 Finite Elements
If a Sliding Surface type is used, note that this MPC option will automatically overwrite the analysis coordinate references on all the nodes belonging to the Dependent and Independent Regions. Be careful that this does not erroneously change the meaning of previously applied loads and boundary conditions, or element properties.
RBAR1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements
50
Patran Interface to MD Nastran Preference Guide Finite Elements
form and RBAR1 is the selected type. This form is used to create an MD Nastran RBAR1 Bulk Data entry.
Chapter 2: Building A Model 51 Finite Elements
.
RTRPLT1 MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RTRPLT1 is the selected type. This form is used to create an MD Nastran RTRPLT1 Bulk Data
52
Patran Interface to MD Nastran Preference Guide Finite Elements
entry.
Chapter 2: Building A Model 53 Finite Elements
.
RJOINT MPCs
This subordinate MPC form appears when the Define Terms button is selected on the Finite Elements form and RJOINT is the selected type. This form is used to create an MD Nastran RJOINT Bulk Data
54
Patran Interface to MD Nastran Preference Guide Finite Elements
entry.
Chapter 2: Building A Model 55 Finite Elements
.
56
Patran Interface to MD Nastran Preference Guide Finite Elements
Superelements In superelement analysis, the model is partitioned into separate collections of elements. These smaller pieces of structure, called Superelement, are first solved as separate structures by reducing their stiffness matrix, mass matrix, damping matrix, loads and constraints to the boundary nodes and then combined to solve for the whole structure. The first step in creating a superelement is to create a Patran group (using Group/Create) that contains the elements in the superelement. This group is then selected in the Finite Elements application on the Create/ Superelement form.
Chapter 2: Building A Model 57 Finite Elements
List of existing superelements.
The group containing all the elements that define a superelement. Note that the group must contain elements not just nodes. If a group does not contain elements, it will not show up in the Element Definition Group listbox.
Brings up an optional subordinate form that allows a user to select boundary nodes of the superelement. By default, the common nodes between the elements in the group and the rest of the model are selected as the boundary nodes.
58
Patran Interface to MD Nastran Preference Guide Finite Elements
Select Boundary Nodes
Allows for manual selection of boundary nodes. Remove selected nodes from the Selected Boundary Nodes box.
Add selected nodes to the Selected Boundary Nodes box.
Chapter 2: Building A Model 59 Material Library
2.6
Material Library The Materials form appears when the Material toggle, located on the Patran application selections, is chosen. The selections made on the Materials menu will determine which material form appears, and ultimately, which Nastran material will be created. The following pages give an introduction to the Materials form and details of all the material property definitions supported by the Nastran Preference. Only material records that are referenced by an element property region or by a laminate lay-up are translated. References to externally defined materials result in special comments in the input Nastran file, e.g., materials that property values that are not defined in Patran. The forward translator performs material type conversions when needed. This applies to both constant material properties and temperature-dependent material properties. For example, a three-dimensional orthotropic material that is referenced by CHEXA elements is converted into a three-dimensional anisotropic material.
Materials Application Form This form appears when Materials is selected on the main menu. The Materials form is used to provide options to create the various Nastran materials.
60
Patran Interface to MD Nastran Preference Guide Material Library
This toggle defines the basic material directionality and can be set to Isotropic, 2D Orthotropic, 3D Orthotropic, 2D Anisotropic, 3D Anisotropic, or Composite. For Explicit Nonlinear additional materials can be defined.
Lists the existing materials with the specified directionality.
Defines the material name. A unique material ID will be assigned during translation.
Describes the material that is being created.
Generates a form that is used to define the material properties. See Material Input Properties Form, 61. Generates a form that is used to indicate the active portions of the material model. By default, all portions of a created material model are active.
Chapter 2: Building A Model 61 Material Library
Material Input Properties Form The Input Properties form is the form where all constitutive material models are defined for each material created. Multiple constitutive models can be created for each material created by pressing the Apply button on the main Materials form with the proper widgets set on this form. Multiple constitutive models of the same type are not allowed. The list of existing constitutive models are shown in the bottom list box. A list of valid constitutive models is given in the table below. Set the Constitutive Model here. Press the Apply button on the main Materials application form to create a constitutive model for the given material. Multiple constitutive models can be created for the same material.
Enter the property values in the databoxes. If a value can be temperature, model, strain rate, or strain dependent, a separate listbox will appear to select a field. These fields must be created in the Fields application as Material type fields.
This is a list of current constitutive models. Use the Change Material Status button to turn them on/off from translation into the Nastran input deck.
62
Patran Interface to MD Nastran Preference Guide Material Library
Material Constitutive Models The following table outlines the options when Create is the selected Action. Object
Option 1
Option 2
Option 3
Option 4
Option 5
Isotropic • Linear Elastic • Nonlinear Elastic • Hyperela • Nearly
stic
• Test Data
Incompressible
• Mooney
Rivlin
Order: 1 2 3
• Coefficients
• Mooney
Rivlin • Ogden • Foam • Arruda-Boyce • Gent
Order: 1 2 3 4 5
• Elastoplastic • Stress/Strain
Curve
• von Mises
• Isotropic
• Tresca
• Kinematic
• Mohr-
• Combined
Coulomb • Drucker-
Prager
Chapter 2: Building A Model 63 Material Library
Object
Option 1
Option 2
Option 3
Option 4
• Parabolic
• Isotropic
MohrColomb
• Kinematic
• Buyukoztu
Option 5
• Combined
• Piecewis
e Linear
• Cowper-
Symon ds
rk Concrete • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • None
• Power Law • Power Rate Law • Johnson-Cook • Kumar
• Hardening
Slope
• von
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager
64
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1
Option 2
Option 3
• Perfectly
• Parabolic
Plastic
MohrColomb
Option 4
Option 5
• None
• Piecewis
e Linear
• Cowper-
• Buyukoztu
Symon ds
rk Concrete • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • Rigid
Plastic
• None
• Power Law • Power Rate Law • Johnson-Cook • Kumar
PiecewiseLinear
• Failure
• n/a • Hill • Hoffman • Tsai-Wu • Maximum Strain
Piecewise Linear CowperSymonds
Chapter 2: Building A Model 65 Material Library
Object
Option 1 • Failure1/
2/3
Option 2 • Maximum
Stress • Maximum
Strain • Hoffman
Option 3
• No Progressive • Standard • Gradual Selective • Immediate Selective
• Hill • Tsai-Wu • Hashin • Puck • Hashin-
Tape • Hashin-
Fabric • User
Defined Failure • Creep
• Tabular Input • Creep Law 111 • Creep Law 112 • Creep Law 121 • Creep Law 122 • Creep Law 211 • Creep Law 212 • Creep Law 221 • Creep Law 222 • Creep Law 300 • MATVP
• Viscoelas
tic
• No Function • Williams-Landel-Ferry • Power Series Expansion
2D Orthotro pic
• Linear Elastic
Option 4
Option 5
66
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Failure
Option 2
Option 3
• Stress
• n/a
• Strain
• Hill
Option 4
Option 5
• Hoffman • Tsai-Wu • Maximum Strain • Failure1/
• See Isotropic Entry
2/3 • Elastopla
stic
• Stress/Strain
Curve
• von
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y
• Piecewis
e Linear
• Cowper-
Symon ds
Chapter 2: Building A Model 67 Material Library
Object
Option 1
Option 2 • Hardening
Slope
Option 3 • von
Option 4
Option 5
• Isotropic
Mises
• Kinematic
• Tresca
• Combined
• Mohr-
Coulom b • Drucker-
Prager • Perfectly
Plastic
• von
Mises • Oak
Ridge National Labs • 2-1/4 Cr-
Mo ORNL • Reversed
Plasticit y ORNL • Fully
Alpha Reset ORNL • Generalize
d Plasticit y • Creep
• MATVP
• Viscoelas
• See Isotropic Entry
tic 3D Orthotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure1/
• See 2D Orthotropic Entry
2/3 • Creep
• See 2D Orthotropic Entry
• None
• Piecewis
e Linear
• Cowper-
Symon ds
68
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Viscoelas
Option 2
Option 3
Option 4
Option 5
• See Isotropic Entry
tic 2D Anisotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure
• See Isotropic Entry
• Failure1/
• See Isotropic Entry - progressive failure not supported
2/3 3D Anisotro pic
• Linear Elastic
• Elastopla
• See 2D Orthotropic Entry
stic • Failure1/
• See 2D Orthotropic Entry - progressive failure not supported
2/3 • Creep
Fluid
• Linear Elastic
Composi te
• Laminate
• See Isotropic Entry
• Rule of Mixtures • HAL Cont. Fiber • HAL Disc. Fiber • HAL Cont. Ribbon • HAL Disc. Ribbon • HAL Particulate • Short Fiber 1D • Short Fiber 2D
Chapter 2: Building A Model 69 Material Library
Additional materials for Explicit Nonlinear (SOL 700) are listed in the following table. Object Isotropic
Option 1 • Linear Elastic
Option 2 • Linear Elastic
(MAT1) • Elastoplastic
• Plastic
Option 3 •
Option 4
Option 5
Solid
• Fluid • Bilinear
Kinematic(MAT 3) • Iso.Elastic
Plastic(MAT12) • Rate Dependent
(MAT19) • Piecewise Linear
(MAT24)
• Biliear
• Cowper Symonds
• Linearized
• General
• Table • Rate Sensitive
• Powerlaw
(MAT64) • Resultant (MAT28) • Shape Memory (MAT30) • With Failure (MAT13) • Power Law (MAT18) • Ramberg-Osgood (MAT80) • Hydro (MAT10)
• Linearized
• Viscoelastic
• Viscoelastic (MAT6)
• Rigid
• Material Type 20 • No Constraints • Global Directions • Local Directions • MATRIG (Rigid
• Geometry Body Properties) • Defined
• No Constraints • Global Directions • Local Directions
• Johnson Cook
• Material Type 15 • No
iteractions • Accurate
• Minimum Pressure • No Tension, Min. Stress • No Tension, Min.
Pressure
70
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1 • Rubber
Option 2 • Frazer Nash
(MAT31)
Option 3
Option 4
• Coefficient
• Respect
• Least Square
• Ignore
Option 5
Fit • Blatz-Ko (MAT7) • General Viscoelastic (MAT76) • Cellular Rubber (MAT87) • Mooney Rivlin
(MAT27)
• Coeff. • Least Square
• Arruda-Boyce
(MAT127) • Hyperelastic
(MAT77) • Simplified
• Coefficients • Least Square Fit 1/2/3 • Tension-
Compresion Load • Compression
• True Strain • Simple • Engineering
Average
Strain Rate • 12 Point Average
Load • Tension-
Compressio n Identical • Foam
• Soil and Foam
(MAT5/14)
• Active
(MAT14)
• Allow Crushing • Reversible
• Inactive
(MAT 5) • Low Density
Urethane (MAT57) • Fu Chang Foam
(MAT83) • Low Density
Urethane (MAT57)
• Bulk
Viscosity Inactive
• No Tension • Maintain Tension
• Bulk
Viscosity Active • Bulk
Viscosity Inactive • Bulk
Viscosity Active
• No
Tension • Maintain
Tension
• With
Relaxati on curve • No
Relaxati on Curve
Chapter 2: Building A Model 71 Material Library
Object
Option 1
Option 2
Option 3
Option 4
Option 5
• Viscous Foam (MAT62) • Crushable (MAT63) • Elastoviscoplatic • With Damage
• Strain
(MAT81)
Damage • Orthotropic
• Bilinear • Linearized • Table
• RCDC • Discrete Beam
• Cowper
Symond s • General
• Nonlinear Elastic Discrete Beam (MAT67) • Nonlinear Plastic Discrete Beam (MAT68) • Side Impact Dummy (SID) Damper Discrete Beam (MAT69) • Hydraulic Gas Damper Discrete Beam (MAT70) • Cabel Discrete Beam (MAT71) • Elastic Spring Discrete Beam (MAT74) • Elastic 6 DOF Spring Discrete Beam (MAT93) • Inelastic Spring Discrete Beam (MAT94) • Inelastic 6 DOF Srping Discrete Beam (MAT95) • General Joint Discrete Beam (MAT97)
• Spring Damper • Nonlinear 6
• Follow Loading Curve DOF Discrete • Follow Unloading Curve Beam (MAT119) • Follow Unloading Stiffness • General • Follow Quadratic Unloading Nonlinear 1 DOF Discrete Beam (MAT121) • Elastic Spring (MATDS01) • Viscous Damper (MATDS02) • Elastic Spring (MATDS03) • Nonlinear Elastic Spring (MATDS04) • Nonlinear Viscous Damper (MATDS05) • General Nonlinear Spring (MATDS06) • Spring Maxwell (MATDS07) • Inelastic Spring (MATDS08) • Tri-linear Degrading (MATDS13) • Squat Shear Wall (MATDS14) • Muscle (MATDS15)
72
Patran Interface to MD Nastran Preference Guide Material Library
Object
Option 1
Option 2
Option 3
• Seat Belt
• Seat Belt (MATB01)
• Spotweld
• MATDSW1
• DF
• MATDSW2
• DFRES
Option 4
Option 5
• DFRESNF • DFRESNFP • MATDSW3
• DFSTR
• MATDSW4
• DFRATE
• MATDSW5
• DFNS • DFSIF • DFSTRUC
2D Orthotro pic
• Glass
• Laminated Glass
(Laminated) • Composite
(MAT32) • Enh. Composite
Damage
• Glass • Polymer • Tsai-Wu Theory • Chang-Chang Theory
• Linear Elastic
• Linear Elastic (MAT2)
• Composites
• Composites and
and Fabrics
Fabrics (MAT58)
• Zero
• 0.0
• One
• 1.0
• Two
• -1.0
• Three
3D Orthotro pic
• Honeycomb
• Composite
•
Composite Honeycomb (MAT26)
• Bulk Viscosity Inactive • Bulk Viscosity Active
• Composite Damage (MAT22) • Composite
• Faceted Failure (MAT59) • Ellipsoidal
• Linear Elastic
• Linear Elastic (MAT2)
• Modified
•
Honeycomb
Modified Honeycomb (MAT126)
• Bulk
Viscosity Inactive • Bulk
Viscosity Active
• LCA .LT.
0 • LCA .GT.
0
• Zero • One • Two
Chapter 2: Building A Model 73 Material Library
Object 2D Anisotro pic 3D Anisotro pic
Option 1 • Viscoplastic
Option 2 • Viscoplastic
Option 3 • Shell
(MAT103)
Option 5
• From Curve • Manual Entry
• Linear Elastic
• Linear Elastic (MAT2)
• Viscoplastic
• Viscoplastic
• Brick
(MAT103) • Linear Elastic
Option 4
• From Curve • Manual Entry
• Linear Elastic (MAT2)
Linear Elastic The Input Properties form displays the following for linear elastic properties. The translator produces MAT1 entries for isotropic materials, MAT8 entries for 2D orthotropic materials, MAT3 entries using axisymmetric solid elements or MAT9 entries using 3D solid elements (CHEXA, CPENTA, CTETRA) for 3D orthotropic materials, MAT2 entries for 2D plane stress - 2D anisotropic materials, and MAT9 entries for 3D anisotropic materials. For temperature dependencies, the corresponding MATTi entries are written referencing TABLEMi entries. Temperature dependency is defined using material fields defined under the Fields application. SOL 600 jobs using 3D Orthotropic material the MATORT entry is written. Isotropic
Description
Elastic Modulus
Elastic modulus, E, (Young’s modulus). Can be temperature dependent.
Poisson Ratio
Poisson’s ratio (NU). Can be temperature dependent. Should be between -1.0 and 0.5.
Shear Modulus
Shear modulus (G). Can be temperature dependent.
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient
Thermal coefficient of expansion (A). Can be temperature dependent.
Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
2D/3D Orthotropic
Description
Elastic Modulus ii
Modulus of elasticity in 1-, 2-, and 3-directions. Can be temperature dependent.
Poisson Ratio ij
Poisson’s ratio for uniaxial loading in the three different directions. Can be temperature dependent.
Shear Modulus ij
In-plane and transverse shear moduli in ij planes. Can be temperature dependent.
74
Patran Interface to MD Nastran Preference Guide Material Library
2D/3D Orthotropic
Description
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient ii Thermal coefficients of expansion in the three directions. Can be temperature dependent. Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
2D/3D Anisotropic
Description
Stiffness ij
Elements of the 6x6 symmetric material property matrix in the material coordinate system. Can be temperature dependent.
Density
Density (RHO). Can be temperature dependent.
Thermal Expansion Coefficient ij Thermal coefficients of expansion. Can be temperature dependent. Structural Damping Coefficient
Structural damping coefficient (GE). Can be temperature dependent.
Reference Temperature
Reference temperature (TREF).
Nonlinear Elastic The Input Properties form displays the following for nonlinear elastic properties. Use this form to define the nonlinear elastic stress-strain curve on the MATS1 entry. A stress-strain table defined using the Fields application can be selected on this form. Based on this information the translator will produce MATS1 of type NLELAST and TABLES1 entries. This is used primarily for SOL 106 and 129. This option is not supported by SOL 600. Use an elastoplastic constitutive model instead. Isotropic
Description
Stress/Strain Curve
Defines the nonlinear elastic stress-strain curve. You must select a field from the listbox. It can be strain and/or temperature dependent. Tabular definition of the stress-strain curve via the Fields application using a material field of strain should follow the specifications as outlined by Nastran. The first point of the material field should be the origin and the second point must be at the initial yield point. This material curve is elastic, meaning that in both loading and unloading the material behavior follows the stress-strain curve as defined. It is not recommended that both nonlinear elastic and elastoplastic constitutive models be active or defined for the same material. For work hardening, use the Elastoplastic constitutive model. See the Nastran Quick Reference Guide for more details.
Chapter 2: Building A Model 75 Material Library
Hyperelastic The Input Properties form displays the following for hyperelastic properties. Use this form to define the data describing hyperelastic behavior of a material. This data is placed on MATHP and TABLES1 entries or on the MATHE entry for SOL 600. If you select Test Data as the Data Type, the Input Options form reverts to the form used for non-SOL 600 solutions and data is placed on a MATHP entry (Mooney-Rivlin strain energy model). To use test data for MATHE/SOL 600 runs, use the Experimental Data Fitting features under the Tools menu to determine the coefficients and enter them manually. Test Data - Mooney Rivlin
Description
Tension/Compression TAB1
All data provided must reference a strain dependent field defining the test data. Please refer to the Nastran Quick Reference Guide for descriptions of each of these tabular inputs.
Equibiaxial Tension TAB2 Simple Shear Data TAB3 Pure Shear Data TAB4 Pure Volume Compression TABD
If Coefficients is selected as the Data Type, use the form to describe the strain energy potential. The Mooney Rivlin model can be written out as a MATHP or MATHE entry for SOL 600. Make sure you use the one that is consistent with the solution to be run. Ogden, Foam, Arruda-Boyce, and Gent models are used for SOL 600 MATHE entries only. Mooney Rivlin (MATHP)
Description
Distortional Deformation Coefficients, Aij
Material constants related to distortional deformation. The Order of the Polynomical determines the number of coefficients required as input.
Volumetric Deformation Coefficients, Di
Material constants related to volumetric deformation. The Order of the Polynomial determines the number of coefficients required as input.
Density RHO
Defines the mass density which is an optional property.
Volumetric Thermal Expansion Coefficient AV Coefficient of volumetric thermal expansion. Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Structural Damping Coefficient GE
Structural damping element coefficient.
76
Patran Interface to MD Nastran Preference Guide Material Library
Mooney Rivlin (MATHE)
Description
Strain Energy Function C10, C01, C11, C20, C30
Strain energy densities as a function of the strain invariants in the material. May vary with temperature via a defined material field. This option consolidates several of the hyperelastic material models, including Neo-Hookean (C10 only), Mooney-Rivlin (C10 & C01), and Full Third Order Invariant (all coefficients).
Density RHO
Defines the mass density
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field.
Bulk Modulus K
Defines the Bulk Modulus.
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Structural Damping Coefficient GE
Structural damping element coefficient.
Ogden
Description
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
Defines the material mass density.
Coefficient of Thermal Expansion
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Modulus k
k
in the Ogden equation. The number of
moduli required as input is dependent on the Order of the Polynomial. Exponent k
k
in the Ogden equation. The number of
exponents required as input is dependent on the Order of the Polynomial.
Foam
Description
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
Defines the material mass density.
Chapter 2: Building A Model 77 Material Library
Foam
Description
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Modulus n
un
in the Foam equation. The number of moduli
required as input is dependent on the Order of the Polynomial. Deviatoric Exponent n
n
in the Foam equation. The number of
exponents required as input is dependent on the Order of the Polynomial. Volumetric Exponent n
n
in the Foam equation. The number of
exponents required as input is dependent on the Order of the Polynomial.
78
Patran Interface to MD Nastran Preference Guide Material Library
Arruda- Boyce
Description
NKT
Chain density times Boltzmann constant times temperature. May vary with temperature via a defined material field.
Chain Length
Average chemical chain cross length. May vary with temperature via a defined material field.
Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
This defines the material mass density.
Thermal Expansion Coefficient
Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Gent
Description
Tensile Modulus
Defines standard tension modulus (E). May vary with temperature via a defined material field.
I 1*
Maximum 1st Invariant
Defines
*
I1 = I1 – 3
. May vary with
temperature via a defined material field. Bulk Modulus K
Defines the Bulk Modulus.
Density RHO
This defines the material mass density.
Coefficient of Thermal Expansion
Defines the coefficient of thermal expansion.
Reference Temperature TREF
Defines the reference temperature for the thermal expansion coefficient.
Elastoplastic The Input Properties form displays the following for elastoplastic properties. Use this form to define the data describing plastic behavior of a material. The stress-strain curve data is input via a material property field of strain and placed on MATS1 and TABLES1 entries. The data input should be the true equivalent stress vs. equivalent total strain. Other options are placed on the MATEP entry and are valid only for SOL
Chapter 2: Building A Model 79 Material Library
400 & 600. Note that the existence of both an elastoplastic and nonlinear elastic constitutive models in the same material is not recommended. Stress/Strain Curve
Description
Yield Function
Yield function (YF) criterion: von Mises, Tresca, Mohr-Coulomb, & DruckerPrager supported on MATS1 entry. All others are for SOL 600 and placed on the MATEP entry. SOL 400 only supports von Mises.
Hardening Rule
Hardening Rule (HR). These are Isotropic, Kinematic, and Combined isotropic and kinematic and are placed on the MATS1 entry or MATEP entry depending on solution sequence and yield function selected. Hardening rules Power Law, Rate Power Law, Johnson-Cook, Kumar are available when no Yield Function is specified. This is used for SOL 600 only on MATEP entry.
Strain Rate Method
Selects an option for strain-rate dependent yield stress used in SOL 600. Cowper-Symonds requires input of Denominator C and Inverse Exponent P.
Stress/Strain Curve
This data must reference a strain dependent field. It can also be temperature and strain rate dependent. LIMIT1 in MATS1 determined from supplied tabular field of stress-strain curve. Data is placed on TABLES1 entry.
Internal Friction Angle
Defined for Mohr-Coulomb and Drucker-Prager yield function placed on the MATS entry LIMIT2.
Yield Point
Initial yield stress.
Stress at Yield Beta
Parameter beta for parabolic Mohr-Coulomb or Buyukozturk concrete models. Placed on the MATEP entry.
10th Cycle Yield Stress
Equivalent 10th cycle tensile yield stress for Oak Ridge National Labs models (ORNL). Placed on the MATEP entry.
Denominator C
Constants for the Cowper-Symonds strain rate method.
Inverse Exponent P
80
Patran Interface to MD Nastran Preference Guide Material Library
Stress/Strain Curve
Description
Coefficient A / B / C / Bi
Coefficient and exponent data for Power Law, Rate Power Law, Johnson-Cook, and Kumar hardening rules.
Exponent M / N initial Strain Rate Room Temperature
Additional data input for the Johnson-Cook hardening rule.
Melt Temperature
Hardening Slope
Description
Yield Function
Yield function (YF) criterion: von Mises, Tresca, Mohr-Coulomb, & DruckerPrager supported on MATS1 entry.
Hardening Rule
Hardening Rule (HR). These are Isotropic, Kinematic, and Combined isotropic and kinematic and are placed on the MATS1 entry.
Strain Rate Method
No strain rate methods are available for the Hardening Slope data.
Hardening Slope
Work hardening slope (H) - slope of stress versus plastic strain. Defined in units of stress. For an elastic-perfectly plastic case, use the Perfectly Plastic data input option.
Internal Friction Angle
Defined for Mohr-Coulomb and Drucker-Prager yield function placed on the MATS entry LIMIT2.
Yield Point
Initial yield stress.
Perfectly Plastic
Description
Yield Function
See the Stress / Strain Curve table above. All options are identical except there must be a yield function selected.
Hardening Rule
None are available since no hardening is possible for a perfectly plastic material.
Strain Rate Method
Piecewise linear or Cowper-Symonds are available.
Chapter 2: Building A Model 81 Material Library
Perfectly Plastic
Description
Yield Point
Initial yield stress.
All other data input is described in the Stress/Strain Curve table above.
Rigid Plastic
Description
Yield Function
No yield functions are available as the material is defined as rigid and then plastic, so no yield is possible.
Hardening Rule
See the Stress / Strain Curve table above. Valid options are the Power Law, Power Rate Law, Johnson-Cook, Kumar, and Piecewise Linear.
Strain Rate Method
Piecewise linear or Cowper-Symonds are available only if the Piecewise Linear hardening rule is selected.
Stress/Strain Curve
Necessary only when not using one of the power law hardening rules (Piecewise-Linear). This data must reference a strain dependent field. It can also be temperature and strain rate dependent. LIMIT1 in MATS1 determined from supplied tabular field of stress-strain curve. Data is placed on TABLES1 entry.
All other data input is described in the Stress/Strain Curve table above. Rigid Plastic is only used in SOL 600 and only for isotropic materials. See the Nastran Quick Reference Guide for more information about the necessary data for MATS1 and MATEP entries. Failure The Input Properties form displays the following for failure material models. Note that this failure model is for non-SOL 400/600/700 solutions. See Failure 1/2/3 for SOL 400/600/700. No Composite Failure Theory
Description
Tension Stress Limit
Stress limits for tension, compression, and shear used to compute margins of safety in certain elements. They have no effect on the computational procedures.
Compression Stress Limit Shear Stress Limit
Failure criteria for the isotropic and two-dimensional orthotropic and anisotropic materials appear in the ST, SC, and SS fields on MAT1 and MAT2 entries and the Xt, Xc, Yt, Yc, and S fields on the MAT8 entry.
82
Patran Interface to MD Nastran Preference Guide Material Library
Composite Failure Theory:
Description
Hill, Hoffman, Tsai-Wu, Maximum Failure Limits
For 2D orthotropic on the MAT8 entry, the limits can be defined as stress or strain allowables. This is not applicable to isotropic and anisotropic materials.
Tension Stress Limit
Stress limits for tension, compression, and shear are the same as those defined for non-composite failure.
Compression Stress Limit Shear Stress Limit Bonding Shear Stress Limit
Allowable shear stress of the bonding material. SB field on the PCOMP entry.
Failure criteria for the isotropic and two-dimensional orthotropic and anisotropic materials appear in the ST, SC, and SS fields on MAT1 and MAT2 entries and the Xt, Xc, Yt, Yc, and S fields on the MAT8 entry unless composites are being used in which case the data is written to the PCOMP entry as necessary. Failure 1, Failure 2, Failure 3 The Input Properties form displays the following for failure material models used in SOL 400 and 600. Solution sequences other than SOL 400/600/700 should use the Failure constitutive model above instead. Up to three failure constitutive models can be defined for any one material. Failure 1 must exist in order for Failure 2 and 3 to be recognized and translated into the proper MATF and MATTF entries. Temperature dependent properties as defined by material fields are translated onto the MATTF entry. Note also that only Failure 1 allows for definition of progressive failure. Failure models 2 and 3 take on whatever progressive failure is defined in Failure 1. Different failure criterion may exist between all three in the same material definition. The table below outlines the allowable properties. All values are real, 0.0, or left blank with no defaults unless otherwise indicated. Which properties are available is dependent on the Failure Criterion selected. The following Failure Criteria are available: • Maximum Stress • Maximum Strain • Hill • Hoffman • Tsai-Wu • Hashin • Puck • Hashin-Tape
Chapter 2: Building A Model 83 Material Library
• Hashin-Fabric
Property
Description
Progressive Failure Options
Progressive failure options are None, standard Progressive Failure, Gradual or Immediate selective progressive failure for SOL 600. SOL 400 does not support progressive failure models and will ignore this setting if set to anything other than None. Only failure indices are computed when no progressive failure is specified. Anisotropic materials do not support progressive failure.
Tension Stress Limit X / Y /Z Tension Strain Limit X / Y / Z
Tension, compression, and shear stress or strain limits used in the Maximum Stress or Strain, Hill, Hoffman, and Tsai-Wu failure criteria.
Compression Stress Limit X / Y / Z Compression Strain Limit X / Y / Z Shear Stress Limit XY / YZ / ZX Shear Strain Limit XY / YZ / ZX Shear Stress Bond (SB)
Allowable shear stress of bonding material between layers for composites only. This is used in SOL 600 only and is ignored for SOL 400.
Failure Index
Failure index used for Hill, Hoffman, and Tsai-Wu criteria.
Interactive Strength XY / YZ / ZX
Interactive strength constants for specified plane used in the Tsai-Wu criterion.
Max Fiber / Matrix Tension Max Fiber / Matrix Compression
Definable stress limits for Hashin, Puck, HashinTape, and Hashin-Fiber criteria.
Max Tape Fiber Tension Max Tape Fiber Compression Max 1st Fiber Tension / Compression Max 2nd Cross Fiber Tension / Compression Max Thickness Tension Max Thickness Compression Layer Shear Strength Transverse Shear Strength YZ / ZX
Shear stress limits for Hashing, Puck, Hashin-Tape, and Hashin-Fiber criteria.
Slope P12C / P12T / P23C / P23T of Fracture Envelope
Slopes of the failure envelope used in Puck failure criterion.
84
Patran Interface to MD Nastran Preference Guide Material Library
Property
Description
Deactivate Tension X / Y/ Z Deactivate Compress X / Y / Z Deactivate Shear XY / YZ / ZX
If any value other than blank or 0.0 is entered for progressive failure options Gradual and Immediate, failed elements are deactivated (placed ICi fields in MATF entry). See the Nastran Quick Reference Guide for information.
Deactivate Elements Deactivate Fiber / Matrix Tension Deactivate Fiber /Matrix Compression Deactivate Matrix Tension Deactivate Matrix Compression Residual Stiffness Factor Matrix Compression Factor Shear Stiffness Factor E33 Fiber Failure Factor Shear Fiber Failure Factor
Reduction fractions or factors. Values can be between 0.0 and 1.0. Used only for Gradual or Immediate progressive failure modes (placed on Ai fields in MATF entry). See the Nastran Quick Reference Guide for more information.
Creep The Input Properties form displays the following for creep models. Tabular Input
Description
Data defined by the use of this form to define the primary stiffness, primary damping, and secondary damping for a creep model with tabular input appears on the CREEP entry for non-SOL 600 runs. Only isotropic materials use this data input method. Creep Law ijk
Description
Use this form to define the coefficients for one of many empirical creep models available appears on the CREEP entry for non-SOL 600 runs. Only isotropic materials use this creep definition. MATPV
Description
Use this form to define either the coefficients and exponents for creep model or provide tabular field data to define Temperature vs. Creep Strain, Creep Strain Rate vs. Stress, Strain Rate vs. Creep Strain, or Time vs. Creep Strain in SOL 600 runs. This data is written to the MATVP entry. If tabular data is provided, this data is written to TABLEM1 entries. It is not recommended to mix the exponents and coefficients and tabular data. Use one or the other.
Chapter 2: Building A Model 85 Material Library
Viscoelastic The Input Properties form displays the following for viscoelastic models. This material model is only used in SOL 600 runs and all data is placed on the MATVE, MATTVE entries. Linear elastic or hyperelastic constitutive models for isotropic or anisotropic materials must exist in addition to the viscoelastic model. Composite The Composite forms provide alternate ways of defining the linear elastic properties of materials. All the composite options, except for Laminated Composite, will always result in a homogeneous elastic material in MD Nastran. When the Laminated Composite option is used to create a material and this material is then referenced in a “Revised or Standard Laminate Plate” element property region, a PCOMP entry is created. However, if this material is referenced by a different type of element property region, for example, “Revised or Standard Homogeneous Plate,” then the equivalent homogeneous material properties are used instead of the laminate lay-up data. Only materials created through the Laminated Composite option should be referenced by a “Revised or Standard Laminate Plate” element property region. Refer to Composite Materials Construction (p. 116) in the Patran Reference Manual. Laminated
This subordinate form appears when the Input Properties button is selected on the Materials form, Composite is the selected Object, and Laminate is the selected Method. Use this form to define the laminate lay-up data for a composite material. If the resulting material is referenced in a “Revised or Standard Laminate Plate” element property region, then an MD Nastran PCOMP entry containing the lay-up data is written. If the resulting material is referenced by any other type of element property region, the equivalent homogeneous properties of the material are used
86
Patran Interface to MD Nastran Preference Guide Material Library
.
Chapter 2: Building A Model 87 Element Properties
2.7
Element Properties The Element Properties form appears when the Element Properties toggle, located on the Patran main form, is chosen.There are several option menus available when creating element properties. The selections made on the Element Properties menu will determine which element property form appears, and ultimately, which MD Nastran element will be created. The following pages give an introduction to the Element Properties form, and details of all the element property definitions supported by the Patran MD Nastran Preference.
Element Properties Form This form appears when Element Properties is selected on the main menu. There are four option menus on this form. Each will determine which MD Nastran element type will be created and which property forms will appear. The individual property forms are documented later in this section. For a full description of this form, see Element Properties Forms (p. 67) in the Patran Reference Manual.
88
Patran Interface to MD Nastran Preference Guide Element Properties
Use this option menu to define the element’s dimension. The options are: 0D (point elements) 1D (bar elements) 2D (tri and quad elements) 3D (tet, wedge, and hex elements)
This option menu depends on the selection made in the Dimension option menu. Use this menu to define the general type of element, such as: Mass versus Grounded Spring Shell versus 2D_Solid
This button is used to quickly edit an element property; for example change the shell thickness.
These option menus may or may not be present, and their contents depend heavily on the selections made in Dimension and Type. See Table 2-1 for more help.
This is used to specify element properties; for example shell thickness, or material orientation. This is used to specify the region (area) of geometry or elements that are to be included in the property definition.
Chapter 2: Building A Model 89 Element Properties
The following table outlines the option menus when Analysis Type is set to Structural. Table 2-1
Structural Options
Dimension 0D
Type • Mass
Option 1
Option 2
• Coupled • Grounded • Lumped
• Grounded Spring • Grounded Damper • Grounded Bush
1D
• Beam
• General Section
• Standard • P-Formulation
• Curved w/General
Section • Curved w/Pipe
Section • Lumped Section • Tapered Section
• Standard • P-element
• General Section
•
(CBEAM) • Rod
• General Section
• Standard • CONROD
• Pipe Section • Spring • Damper
• Scalar • Viscous
• Gap
• Adaptive • Non-Adaptive
• 1D Mass • PLOTEL • Bush • Spot Weld Connector • Fastener Connector
90
Patran Interface to MD Nastran Preference Guide Element Properties
Table 2-1 Dimension 2D
Structural Options Type • Shell
Option 1 • Homogeneous
Option 2 • Standard • Revised • P-element
• Laminate
• Standard • Revised
• Equivalent Section
• Standard • Revised • P-element
• Field Point Mesh (exterior acoustic element) • Bending Panel
• Standard • Revised
•
• P-element •
• 2D-Solid
• Plane Strain
• Standard • Revised • P-Formulation • Hyperelastic Formulation
• Axisymmetric
• Standard • Hyperelastic Formulation • PLPLANE
• Infinite (exterior acoustic element) • Membrane
• Revised
• •
3D
• Standard • P-Formulation
• Shear Panel • Solid
• Homogeneous
• Standard • P-Formulation • Hyperelastic Formulation
• Laminate • Gasket
Chapter 2: Building A Model 91 Element Properties
Coupled Point Mass (CONM1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Coupled
Point/1
Use this form to create a CONM1 element. This defines a 6 x 6 symmetric mass matrix at a geometric point of the structural model.
92
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the orientation of the 1-2-3 axes of the mass matrix. The value is a reference to an existing coordinate frame. The 12-3 axes will be aligned with the X-Y-Z axes of the specified coordinate system. If a non rectangular coordinate system is specified, the system will be evaluated into a local rectangular system, which is then used to orient the mass matrix. This property is the CID field on the CONM1 entry. This property is optional.
Defines the values of the mass matrix. These properties are the Mij fields on the CONM1 entry and can either be real values or references to existing field definitions. Each of these properties are optional; however, at least one must be defined.
Chapter 2: Building A Model 93 Element Properties
This is a list of Input Properties available for creating a CONM1 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description Defines the values of the mass matrix. These are the Mij fields on the CONM1 entry. These properties can either be real values or references to existing field definitions. Each of these properties are optional; however, at least one must be defined.
Mass Component 3,3 Mass Component 4,1 Mass Component 4,2 Mass Component 4,4 Mass Component 5,1 Mass Component 5,2 Mass Component 5,3 Mass Component 5,4 Mass Component 5,5 Mass Component 6,1 Mass Component 6,2 Mass Component 6,3 Mass Component 6,4 Mass Component 6,5 Mass Component 6,6
Grounded Scalar Mass (CMASS1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Grounded
Point/1
Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model. Only one node is used in this method, and the other node is defined to be grounded.
94
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the translation mass or rotational inertia value to be applied. This is the M field on the PMASS entry. This property can be either a real value or a reference to an existing field definition. This property is required.
Defines which degree of freedom this value will be attached to. This property can be set to UX, UY, UZ, RX, RY, or RZ and defines the setting for the C1 field on the CMASS1 entry. This property is required.
Lumped Point Mass (CONM2) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
0D
Mass
Lumped
Point/1
Use this form to create a CONM2 element. This defines a concentrated mass at a geometric point of the structural model.
Chapter 2: Building A Model 95 Element Properties
Defines an offset from the specified node to where the lumped mass actually is to exist in the structural mode. This vector is defined in the Mass Orientation coordinate system. Defines the X1, X2, and X3 fields on the CONM2 entry. This property is optional.
Defines the translational mass value to be used. This is the M field on the CONM2 entry. This property can either be a real value or a reference to an existing field definition. This property is required.
Defines the orientation of the 1-2-3 axes of the mass matrix. This is a reference to an existing coordinate frame. The 1-2-3 axes will be aligned with the X-Y-Z axes of the specified coordinate system. If a nonrectangular coordinate system is specified, the system will Inertia i,j defines the rotation inertia properties of be evaluated into a local rectangular system, this lumped mass. These properties are the Iij which is then used to orient the mass matrix. fields on the CONM2 record. These values can This is the CID field on the CONM2 entry. If the be either real values or references to existing Value Type is set to Vector then the field definitions. These values are optional. components of the vector define the center of gravity of the mass in the basic coordinate system and the field for CID is translated as -1. This property is optional.
This is a list of Input Properties available for creating a CONM2 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.
96
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description Inertia i,j defines the rotation inertia properties of this lumped mass. These are the Iij fields on the CONM2 entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 3,1 Inertia 3,2 Inertia 3,3
Grounded Scalar Spring (CELAS1/CELAS1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen. Action
Dimension
Type
Create
0D
Grounded Spring
Option(s)
Topologies Point/1
Chapter 2: Building A Model 97 Element Properties
Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring element of the structural model. Only one node is used in this method. The other node is defined to be grounded. Defines the coefficient to be used for this spring. This is the K field on the PELAS entry. This can either be a real value or a reference to an existing field definition. This property is required.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Defines the relationship between the spring deflection and the stresses within the spring. This property is the S field on the PELAS entry and can either be a real value, or a reference to an existing field definition. This property is optional.
Defines what damping is to be included. This is the GE field on the PELAS entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
Defines which degree of freedom this value is to be attached to. This can be set to UX, UY, UZ, RX, RY, or RZ. This property defines the setting of the C1 field on the CELAS1 entry. This property is required.
98
Patran Interface to MD Nastran Preference Guide Element Properties
Grounded Scalar Damper (CDAMP1/CDAMP1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen. Action
Dimension
Type
Create
0D
Grounded Damper
Option(s)
Topologies Point/1
Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model. Only one node is used in this method. The other node is defined to be grounded.
Defines the force per unit velocity value to be used. This property is the B field on the PDAMP entry and can either be a real value or a reference to an existing field definition. This property is optional.
Defines which degree of freedom this value is to be attached to. This property can be set to UX, UY, UZ, RY, or RZ and defines the setting for the C1 field on the CDAMP1 entry. This property is required.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Chapter 2: Building A Model 99 Element Properties
Bush This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Bush
Option(s)
Topologies Bar/2
100
Patran Interface to MD Nastran Preference Guide Element Properties
This toggle can also be set to Node Id or CID..
Chapter 2: Building A Model 101 Element Properties
This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bush Orientation System
CID specifies the Grounded Bush Orientation System. The element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the grid point specified locates the system. If CID = 0, the basic coordinate system is used.
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6
Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6
Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6
Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend
Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation
Stress recovery coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation
Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.
102
Patran Interface to MD Nastran Preference Guide Element Properties
General Section Beam (CBAR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
General Section
Bar/2
Chapter 2: Building A Model 103 Element Properties
Use this form to create a CBAR element and a PBAR or PBARL property. A CBARAO entry will be generated if any Station Distances are specified. This defines a simple beam element in the structural model.
Note:
CBAR entries will include all user input pin flags.
104
Patran Interface to MD Nastran Preference Guide Element Properties
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, (for the standard Beam Library) or PBRSECT/PBMSECT (for an Arbitrary section) will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the value to be used in the MID field on the PBAR entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBAR entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBAR entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBAR entry.
Chapter 2: Building A Model 105 Element Properties
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBAR entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBAR entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
These degrees of freedom are in the element local coordinate system. Values that can be specified are UX, UY, UZ, RX, RY, RZ, or any combination. These properties are used to remove connections between the node and selected degrees of freedom at the two ends of the beam. This option is commonly used to create a pin connection by specifying RX, RY, and RZ to be released. Defines the setting of the PA and PB fields on the CBAR record. These properties are optional.
Area
Defines the cross-sectional area of the element. This is the A field on the PBAR entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1
Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 2,2 Inertia 2,1
106
Patran Interface to MD Nastran Preference Guide Element Properties
Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBAR entry. These values can be either real value or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBAR entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C
Indicates the stress recovery. They define the Y and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C Y of Point D Z of Point D Y of Point E Z of Point E Y of Point F Z of Point F [Contact Beam Radius]
This allows the equivalent radius for beam-to-beam contact to be different for each beam cross section. The MD Nastran entry BCBMRAD is written to the .bdf file. The BCBMRAD entry format is different for SOL 400 and SOL 600.
[Station Distances]
Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO entry is not supported. These values are real values. These properties are optional.
Create Sections, I C L ..., Beam Library
Activates the Beam Library forms. These forms will allow the user to define beam properties by choosing a standard cross section type and inputing dimensions.
Chapter 2: Building A Model 107 Element Properties
P-Formulation General Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
General Section
Bar/2, Bar/3
P-Formulation
Bar/4
Use this form to create a CBEAM element and a PBEAM or PBEAML property. This form defines a simple beam element in the structural model for an adaptive, p-element analysis. Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
108
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam, and this orientation vector, which can be defined as either a vector or a reference to an existing node, is in the XY plane. This defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
Input Properties
Allows a beam section previously created using the beam library to be selected. When a beam section is chosen and the Associate Beam Section option is toggled, the cross sectional properties need not be input on this Input Properties form. Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the value to be used in the MID field on the PBAR entry. This property is required. Allows a user to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Activates the Beam Library forms. These forms will allow the user to define beam properties by choosing a standard cross section type and inputting dimensions.
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. On the CBEAM entry, these values are always in the displacement coordinate a system specified such as <0 1 0 Coord 5>. These properties are optional.
Chapter 2: Building A Model 109 Element Properties
This is a list of Input Properties available for creating a CBEAM element and a PBEAM or PBEAML property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Area
Defines the cross-sectional area of the element. This is the A field on the PBEAM entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1
Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These values are optional.
Inertia 2,2 Inertia 2,1 Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBEAM entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBEAM entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C
Indicates the stress recovery. Define the Y and Z coordinates of the stress recovery points across the section of the beam as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C X of Point D Y of Point D X of Point E Y of Point E X of Point F Y of Point F Station Distances
Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO records is not supported. These values are real values. These properties are optional.
110
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description
Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting Porders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum Porders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The two sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Curved General Section Beam (CBEND) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Curved w/General Section
Bar/2
Use this form to create a CBEND element and a PBEND property. This form defines a curved beam element of the structural model. The CBEND element has several ways to define the radius of the bend and the orientation of that curvature.This element in Patran always uses the method of defining the center of curvature point (GEOM=1). An alternate property of the Curved Pipe element also exists.
Chapter 2: Building A Model 111 Element Properties
Defines the center of curvature of the pipe bend. It is done by either specifying a vector from the first node of the element or by referencing a node. The CBEND element in MD Nastran has several ways to define the radius of the pipe bend and the orientation of that curvature. This defines the settings of the X1, X2, X3, and G0 fields of the CBEND entry. This property is required.
Defines the cross-sec This property is the A This value can be eith to an existing field def optional.
112
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties available for creating a CBEND element and a PBEND property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Inertia 1,1 Inertia 2,2
Description Defines the various area moments of inertia of the cross section. These properties are the I1 and I2 fields on the PBEND entry. These values can either be real values or references to existing field definitions. These values are optional.
Torsional Constant
Defines the torsional stiffness of the beam. This is the J field on the PBEND entry. This value can be either a real value, or a reference to an existing field definition. This property is optional.
Shear Stiff, R
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. This property is optional.
Shear Stiff, Z Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can be either real value or a reference to an existing field definition. This property is optional.
Radial NA Offset
Defines the radial offset of the geometric centroid from the end nodes. Positive values move the centroid of the section towards the center of curvature of the pipe bend. This property is the DELTAN field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
R of Point C
These properties are for stress recovery. They define the R and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These properties are the C1, C2, D1, D2, E1, E2, F1 and F2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of Point C R of Point D Z of Point D R of Point E Z of Point E R of Point F Z of Point F
Chapter 2: Building A Model 113 Element Properties
Curved Pipe Section Beam (CBEND) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Curved W/Pipe Section
Bar/2
Use this form to create a CBEND element and a PBEND property. This defines a curved pipe or elbow element of the structural model. The internal pressure is defined as part of the element definition because, for pipe elbows, the internal pressure affects the element stiffness.
114
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when Defines the data is entered. Either select from the list using the mouse, or type in the name. Defines the MID center of curvature of the field on the PBEND entry. This property is required. pipe bend. This can be done either by specifying a vector from the first node of the element or by referencing a node. The CBEND element in MD Nastran has several ways to define the radius of the pipe bend and the orientation of that curvature. Defines the settings of the X1, X2, X3, and G0 fields on the CBEND entry. This element in Patran always uses the method of defining the center of curvature point Indicates the wall thickness of the pipe. This is the t field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the offset from the nodes to the actual centroids of the pipe cross section. These are the RC and ZC fields on the PBEND entry. These values can either be real values or references to existing field definitions. These properties are optional.
Indicates the distance from the centroid of cross section to mid-wall location. This is t on the PBEND entry. This value can either value or a reference to an existing field de This property is required.
Chapter 2: Building A Model 115 Element Properties
This is a list of Input Properties available for creating a CBEND element and a PBEND property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Internal Pipe Pressure
Indicates the static pressure inside the pipe elbow. This is the P field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can either be a real value or a reference to an existing field definition. This property is optional.
Stress Intensification
Indicates the desired type of stress intensification to be used. This is a character string value. This property is the FSI field on the PBEND entry. Valid settings of this parameter are General, ASME, and Welding Council.
Lumped Area Beam (CBEAM/PBCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Lumped Section
Bar/2
Use this form to create a CBEAM element and a PBCOMP property. This defines a beam element of constant cross section, using a lumped area element formulation.The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.
116
Patran Interface to MD Nastran Preference Guide Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Chapter 2: Building A Model 117 Element Properties
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type
The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.
• Reference Coordinates
Analysis - Analysis Coordinate System. Coord 0 - Basic Coordinate System.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. On the CBEAM entry, these values are always in the displacement coordinate system of the node. In Patran, they are either global, or in a system specified such as <0 1 0 Coord 5>. These properties are optional.
• Value Type
Specifies that the offset is defined in terms of a vector.
• Reference Coordinates
Analysis - Analysis Coordinate System. Element - Element Coordinate System.
118
Patran Interface to MD Nastran Preference Guide Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Warp DOF @ Node 1 Warp DOF @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Defines a node ID where the warping degree-of-freedom constraints and results will be placed. These must reference existing nodes within the model. They are the SA and SB fields on the CBEAM entry. These properties are optional.
Area
Defines the cross-sectional area of the element. This is the A field on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBCOMP record. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y
Defines the shear stiffness values. These are the K1 and K2 fields on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Z Y of NSM Z of NSM
Symmetry Option
Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These properties are the M1 and M2 fields on the PBCOMP entry. These values can be either real values or references to existing field definitions. These properties are optional. Specifies which type of symmetry is being used to define the lumped areas of the beam cross section. This is a character string parameter. The valid settings are No Symmetry, YZ Symmetry, Y Symmetry, Z Symmetry, or Y=Z Symmetry. This defines the setting of the SECTION field on the PBCOMP entry. This property is optional.
Chapter 2: Building A Model 119 Element Properties
Ys of Lumped Areas Zs of Lumped Areas Area Factors
Defines the locations of the various lumped areas. These are defined in the cross-sectional coordinate system. These properties define the Yi and Zi fields on the PBCOMP entry. These values are lists of real values. These properties are optional. Defines the Fraction of the total area to be included in this lumped area. The sum of all area factors for a given section must equal 1.0. If the data provided does not meet this requirement, the values will all be scaled to the corrected value. These properties define the values for the Ci fields on the PBCOMP entry. These values are lists of real values. These properties are optional.
Tapered Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Beam
Tapered
Bar/2
120
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CBEAM element and a PBEAM or PBEAML property. This defines a beam element with varying cross sections.
Chapter 2: Building A Model 121 Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
122
Patran Interface to MD Nastran Preference Guide Element Properties
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Chapter 2: Building A Model 123 Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Warp DOF @ Node 1 Warp DOF @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Defines a node ID where the warping degree of freedom constraints and results will be placed. These must reference existing nodes within the model. These are the SA and SB fields on the CBEAM entry. These properties are optional.
Station Distances
Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. These values are real values. These properties are optional.
Cross-Sect. Areas
Defines the cross-sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, or reference to an existing field definition. This property is required.
Inertias 1,1
Defines the various area moments of inertia of the cross section. These defines the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are real values. These properties are optional.
Inertias 2,2 Inertias 1,2 Torsional Constants
Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
Ys of C Points
Defines the Y and Z locations in element coordinates, relative to the shear center for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These are lists of real values, one for each station location. These properties are optional.
Zs of C Points Ys of D points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points
124
Patran Interface to MD Nastran Preference Guide Element Properties
Nonstructural Masses
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
NSM Inertia @ Node 1
Specified the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
NSM Inertia @ Node 2
Y of NSM @ Node 1
Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2 Shear Stiff, Y
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Z Shear Relief Y
Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Shear Relief Z Warp Coeff. @ Node 1 Warp Coeff. @ Node 2 Y of NA @ Node 1
Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional. Defines the offset from the centroid of the cross section to the location of the neutral axis. These values are measured in the beam cross section coordinate system and are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2
General Section Beam (CBEAM) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Create
1D
Beam
General Section (CBEAM)
Chapter 2: Building A Model 125 Element Properties
This set of options provides a method of creating beam models with warping due to torsion. The capabilities of this beam properties formulation option are similar to those of the “Tapered Section” formulation, except that warping due to torsion is handled more conveniently.
126
Patran Interface to MD Nastran Preference Guide Element Properties
Note:
Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.
Section Name
Specifies a beam section previously created using the beam library
• Value Type
Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation
Defines the local element coordinate system to be used for any crosssectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
Chapter 2: Building A Model 127 Element Properties
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2
Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type
Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates
Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
128
Patran Interface to MD Nastran Preference Guide Element Properties
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2
Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. Pin or sliding type connections can be created by releasing specified degrees of freedom. These degrees of freedom are in the element local coordinate system. The values specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry. These properties are optional.
Warping Option
This specifies how contraints should be applied to the warping SPOINTs of unmatched ends within the application region (see continuity rules above). The choices available include “A free B free”, “A fixed B fixed”, “A free B fixed”, “A fixed B free”, or “None”. The choice of “None” is used to disable warping altogether for the current element property set, in which case no SPOINTs will be generated or constrained. Only unmatched ends within the application region will be eligible for constraining, and whether or not a constraint is applied will depend on the option selected, and whether the unmatched end is “End A” or “End B” of its beam element. If no selection is made for this element property, “A free B free” is selected by default.
Warp Coeff. @ Node 1 Warp Coeff. @ Node 2
Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Station Distances
Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. This field consists of a set of real values separated by legal delimiters, such as white space and/or commas. If this list is entered, then the properties that follow may also be in the form of lists consisting of the same number of values. If they are in the form of a single real value, then that value will apply to all stations of the beam element. This property is optional. If it is not provided, then all other specified section properties apply to the entire beam, and lists of values will not be accepted.
Cross-Sect. Areas
Defines the cross sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, a list (if a list of stations has been provided), or a reference to an existing field definition, in which case a single real value will be evaluated for each element of the application region. This property is required.
Chapter 2: Building A Model 129 Element Properties
Inertias 1,1 Inertias 2,2 Inertias 1,2
Defines the various area moments of inertia of the cross section. These values define the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or a list of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Torsional Constants
Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
Ys of C Points Zs of C Points Ys of D Points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points
Defines the Y and Z locations in element coordinates, relative to the shear center, for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or lists of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Nonstructural Masses
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
NSM Inertia @ Node 1 NSM Inertia @ Node 2
Specifies the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Y of NSM @ Node 1 Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2
Defines the offset from the shear center of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Y Shear Stiff, Z
Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
130
Patran Interface to MD Nastran Preference Guide Element Properties
Shear Relief Y Shear Relief Z
Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Y of NA @ Node 1 Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2
Defines the offset from the shear center of the cross section to the location of the neutral axis. These values are measured in the beam cross-section coordinate system. These are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Warping due to torsion is enabled by generating MD Nastran SPOINTs to contain the warping degrees of freedom. These SPOINTs are not actually present in the Patran database, and there is no way to recover any results for these SPOINTs. They are created during analysis deck translation, and provide the means to communicate to MD Nastran the continuity and constraint properties of the warping degrees of freedom in the model. These attributes of continuity and constraint are implied in the Patran database through the composition of the element properties application region and the set of options selected. These continuity and constraint attributes apply to both warping SPOINTs and end release flags. This connection of these attributes to the composition of the application region is new in Patran 2001r3, and represents a change in behavior from previous versions of Patran. The general rules of implied continuity are as follows. 1. Within the application region, two beam elements are taken to be continuous if a GRID ID at an end of one of the beam elements matches a GRID ID at one of the ends of the other beam element. If a third beam element in the same application region also contains the same GRID ID, it is assumed that none of the beam elements is continuous at this location. This condition is known as a “multiple junction”. Similarly, if none of the other beam elements in the application region contain a matching GRID ID, the corresponding end of the beam element is taken to be not continuous. This condition is known as an “unmatched end”. 2. If warping is enabled, then all instances of beam element continuity must have the matching GRID ID located at “End A” of one of the beam elements and at “End B” of the other. “End A” and “End B” positions are determined by the order of GRID IDs specified in the element connectivity array, and the positive direction of the x-axis of the element coordinate system points from “End A” to “End B”. If warping is not enabled, this restiction does not apply. If warping is enabled, any violation of this requirement will result in a failure to complete the translation of the finite element model. In this event, the user will have to reverse the direction of the improperly oriented beam elements and initiate the translation again. 3. When warping is enabled, all positions of beam element continuity within an application region will be represented by a single SPOINT at each of these positions, which will be generated at the time of analysis deck translation and will appear on the CBEAM entries for the appropriate end of both of the beam elements that are continuous at each location. If any end release codes have been prescribed for the application region, they will not be applied at locations of beam element continuity. This is new for Patran 2001r3. For earlier versions of Patran, end release codes would be applied to all elements of the application region, regardless of continuity.
Chapter 2: Building A Model 131 Element Properties
4. When warping is enabled, individual SPOINTs are generated for all beam ends that are not continuous. This applies to both “multiple junctions” and “unmatched ends”. 5. The specified end release codes are applied to all discontinuous beam element ends in the application region, whether “multiple junction” or “unmatched end”, with the applied end release codes dependent on what has been prescribed for “End A” and “End B” for the application region. If no end release codes have been prescribed for the application region, none are generated. 6. When warping is enabled, and for unmatched ends only (not multiple junctions), constraints applied to the SPOINTs are specified by the “warping option” specified in the element properties form. For example, if “A free B fixed” has been selected and the unmatched end is “End A” of its beam element, it will not be constrained. If it is “End B” of its element, it will be constrained. The warping SPOINT for a beam element end involved in a multiple junction will not be constrained under any circumstances. If the user wishes to constrain warping for a beam element involved in a multiple junction, he will have to do so by splitting the application region in such a way that the beam element end becomes an “unmatched end” within its new application region. 7. Warping is considered to be enabled when a value has been specified for the warping coefficient at either end of the beam element. When the user selects the “Beam Library” option, values for the warping coefficient get computed autamatically, and thus warping is implicitly enabled. If the user wishes to disable warping while using the Beam Library option, he must choose “None” as his “Warping Option” on the “Input Properties ...” form.
General Section Rod (CROD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
General Section
Bar/2
Standard
Use this form to create a CROD element and a PROD property. This defines a tensioncompression-torsion element of the structural model.
132
Patran Interface to MD Nastran Preference Guide Element Properties
Chapter 2: Building A Model 133 Element Properties
Defines the cross-sectional area of the element. This is the A field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the setting of the MID field on the PROD entry. This property is required.
Defines the coefficient to determine the torsional stress. This is the C field on the PROD entry. This property can be either a real value or a reference to an existing field definition. This property is optional.
Defines the torsional stiffness of the beam. This is the J field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam. This is the NSM field on the PROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
134
Patran Interface to MD Nastran Preference Guide Element Properties
General Section Rod (CONROD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
General Section
Bar/2
CONROD
Use this form to create a CONROD element. This defines a tension-compression-torsion element of the structural model.
Chapter 2: Building A Model 135 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the CONROD entry. This property is required. Defines the crosssectional area of the element. This property is the A field on the CONROD entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the CONROD entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the coefficient to determine the torsional stress. This property is the C field on the CONROD entry and can either be a real value or a reference to an existing field definition. This property is optional.
Defines the torsional stiffness of the beam. This property is the J field on the CONROD entry. This value can either be a real value or a reference to an existing field definition. This property is optional.
136
Patran Interface to MD Nastran Preference Guide Element Properties
Pipe Section Rod (CTUBE) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Rod
Pipe Section
Bar/2
Use this form to create a CTUBE element and a PTUBE property. This defines a tensioncompression-torsion element with a thin-walled tube cross section.
Chapter 2: Building A Model 137 Element Properties
Defines the tube outer diameters at each end of the element. These are the OD and OD2 fields on the PTUBE entry. These values can either be real values or references to existing field definitions. The outer diameter at Node 1 property is required. The outer diameter at Node 2 Property is optional. Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. This property defines the setting of the MID field on the PTUBE entry. Either select from the list using the mouse, or type in the name. This property is required. Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PRTUBE entry. This value can be either a real value or reference to an existing field definition. This property is optional. Specifies the wall thickness of the pipe. This is the T field on the PTUBE entry. This value can either be a real value or a reference to an existing field definition. This property is required.
Scalar Spring (CELAS1/CELAS1D) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Spring
Option(s)
Topologies Bar/2
138
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring of the structural model.
Chapter 2: Building A Model 139 Element Properties
Defines the coefficient to be used for this spring. This property is the K field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is required.
Defines what damping is to be included. This property is the GE field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is optional. Defines which degree of freedom this value is to be attached to at each node. The degree of freedom can be set to UX, UY, UZ, RX, RY, or RZ. These properties define the settings of the C1 and C2 fields on the CELAS1 entry. These properties are required.
Defines the relationship between the spring deflection and the stresses within the spring. This property is the S field on the PELAS entry and can be either a real value or a reference to an existing field definition. This property is optional.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Scalar Damper (CDAMP1/CDAMP1D) This subordinate form appears when the Input Properties button is selected on the Element Properties
140
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Damper
Scalar
Bar/2
Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model.
Chapter 2: Building A Model 141 Element Properties
Defines the force per unit velocity value to be used. This is the B field on the PDAMP entry and can either be a real value or a reference to an existing field definition. This property is optional.
Number of a User Defined Coordinate system, used only for Explicit Nonlinear (SOL 700). This property is optional.
Defines which degree of freedom this value will be attached to at each node. This can be set to UX, UY, UZ, RX, RY, or RZ. These define the settings of the C1 and C2 field on the CDAMP1 entry. These properties are required.
Viscous Damper (CVISC) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Damper
Viscous
Bar/2
142
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CVISC element and a PVISC property. This defines a viscous damper element of the structural model.
This is the C1 field on the PVISC entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
This is the C2 field on the PVISC entry. This property can either be a real value or a reference to an existing field definition. This property is optional.
Gap (CGAP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
1D
Gap
Adaptive
Bar/2
Nonadaptive
Use this form to create a CGAP element and a PGAP property. This defines a gap or frictional element of the structural model for non-linear analysis.
Chapter 2: Building A Model 143 Element Properties
Defines the local element coordinate system for this element that can be defined in one of three ways. If the two end nodes of the gap are not coincident, then the Gap Orientation can reference a vector or a node ID. This local x-axis would then run between the two end nodes and the orientation information would define the local xy plane. However, if the two end nodes are coincident, then the Gap Orientation refers to an existing coordinate system definition and will be used as the local element coordinate system. This Gap Orientation defines the settings of the X1, X2, X3, G0, and CID fields on the CGAP entry. This property is required. Defines the initial opening of the gap element. The nodal coordinates are only used to define the closure direction. This property is the U0 field on the PGAP entry and can be either a real value or a reference to an existing field definition. This property is optional.
Defines the artificial stiffness of the gap when the gap is open or closed. The closed stiffness should be chosen to closely match the stiffness of the surrounding elements. The open stiffness should be approximately 10 orders of magnitude less. These properties are the Ka and Kb fields on the PGAP entry and can either be real value or references to existing field definitions. The closed stiffness property is required. The opened stiffness property is optional. Defines an initial preload across an initially closed gap. For example, this can be used for initial thread loading. If the gap is initially open, setting this value to the initial opening stiffness will improve the solution convergence. This is the F0 field on the PGAP entry and can either be a real value or a reference to an existing field definition. This property is optional.
This is a list of Input Properties available for creating a CGAP element and a PGAP property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
144
Patran Interface to MD Nastran Preference Guide Element Properties
properties. Prop Name
Description
Sliding Stiffness
Defines the artificial shear stiffness of the element when the element is closed. This is the Kt field on the PGAP entry. This property can be either a real value or a reference to an existing field definition. This property is optional.
Static Friction
Defines the static friction coefficient. This property is the MU1 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Kinematic Friction
Defines the kinematic friction coefficient. This property is the MU2 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Penetration
Defines the maximum allowable penetration. This property is the TMAX field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Adjust Ratio
Defines the maximum allowable adjustment ratio. This property is the MAR field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Penet. Lower Bound
Defines the lower bound for the allowable penetration. This is the TRMIN field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Friction Coeff. y
Defines the coefficient of friction when sliding occurs along this element in the local y and z directions. These are the MU1 and MU2 fields on the PGAP entry and can be either real values or references to existing field definitions. These properties are optional.
Friction Coeff. Z
Scalar Mass (CMASS1) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
1D Mass
Option(s)
Topologies Bar/2
Chapter 2: Building A Model 145 Element Properties
Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model.
Defines the translation mass or rotational inertia value to be applied. This property is the M field on the PMASS entry and can either be a real value or a reference to an existing field definition. This property is required.
Defines which degree of freedom this value will be attached to at each node. These can be set to UX, UY, UZ, RX, RY, or RZ and defines the settings of the C1 and C2 field on the CMASS1 entry. These properties are required.
146
Patran Interface to MD Nastran Preference Guide Element Properties
PLOTEL This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
PLOTEL
Option(s)
Topologies Bar/2
Use this form to create a PLOTEL element.
Dummy property data not required to define the PLOTEL property set.
(Scalar) Bush This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Bush
Option(s)
Topologies Bar/2
Chapter 2: Building A Model 147 Element Properties
This toggle can also be set to Node Id or CID.
148
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Bush Orientation
Description Element orientation strategy keys off of CID specification. If CID is blank, the element x-axis lies along the line which joins the elements grid points (GA, GB Element Properties/Application Region). The X-Y plane is determined by specifying the Bush Orientation. If a vector input is given, these components define an orientation vector v from the first grid point (GA) of the element in the displacement coordinate system at that point (GA). If the Bush Orientation references a grid point ID (Value), this orientation point forms an orientation vector which extends from the first element grid point to the orientation point.
If a CID 0 is specified for Bush Orientation System, the element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the first elemental grid point (GA) is used to locate the system. If CID = 0, the elemental coordinate system is the Basic Coordinate System.
If no orientation is specified in any form, the element x-axis is along the line which connects the element’s grid points. The material property inputs for this condition must be limited to simple axial and torsional stiffness and damping (k1,k4,B1,B4). Offset Location
Offset Location (0.0 s 1.0) specifies the spring-damper location along the line from GRIDGA to GRIDGB by setting the fraction of the distance from GRIDGA. s=0.50 centers the springdamper.
Offset Orientation System
Specifies the coordinate system used to locate the spring-damper offset when it is not on the line from GRIDGA to GRIDGB.
Offset Orientation Vector
Provides the location of the spring-damper in space relative to the offset coordinate system. If the offset orientation system is -1 or blank, the offset orientation vector is ignored.
Chapter 2: Building A Model 149 Element Properties
Prop Name
Description
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6
Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6
Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6
Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend
Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation
Stress Recovery Coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation
Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.
150
Patran Interface to MD Nastran Preference Guide Element Properties
Spot Weld Connector (CWELD) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Spot Weld Connector
Option(s)
Topologies Connector
Chapter 2: Building A Model 151 Element Properties
.
Note that SPOTWELD properties are created automatically (or pre-existing properties selected) when creating Spotwelds through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying spotweld properties because the existence of the spotweld itself is the application region for the property set.
152
Patran Interface to MD Nastran Preference Guide Element Properties
Fastener Connector (CFAST) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
1D
Fastener Connector
Option(s)
Topologies Connector
Chapter 2: Building A Model 153 Element Properties
.
Note that FASTENER properties are created automatically (or pre-existing properties selected) when creating Fasteners through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying fastener properties because the existence of the fastener itself is the application region for the property set.
154
Patran Interface to MD Nastran Preference Guide Element Properties
The formula value can be any of the following: String None Douglas Huth Hi-Lok in CFRP Huth Hi-Lok in metal Huth solid rivet Note that Douglas or one of several Huth formulations can be used to calculate stiffness values of fastener connections automatically, minimizing the need for manual calculation. Stiffness coefficients for the CFAST element are calculated in different steps. Generally, either Douglas or three derivatives of Huth formulas are used. Regardless of the selected formula, the axial stiffness is always calculated the same way: 1 E f --- A˜ d 2 4 f k = -------------------l
The stiffness is inserted into the KT1 parameter of the PFAST entry. The length of the fastener will be determined by summation of the thickness of the two connected shell elements. The Douglas formula is*: 1 k = --c 5 1 1 c = ---------- + 0.8 ---------- + ---------- t E df Ef t 2 E 2 1 1
The formula according to Huth is*: k = 1 --c a t 1 + t 2 1 1 1 1 - ---------+ ---------- + ------------- + ------------- c = b -------------2d t E t 2 E 2 2E f t 1 2E f t 2 1 1 f
Hi-Lok in CFRP
a
b
0.6667
4.2
Chapter 2: Building A Model 155 Element Properties
a
b
Hi-Lok in metal
0.6667
3.0
Solid Rivet
0.4
2.2
In the case of composites, the Douglas and Huth formulas have to be used twice. First, the overall (engineering) Young’s modulus has to be calculated for both directions (E11 and E22), which then has to be applied to the formulas. In this case, the shear stillness of the fastener is direction dependent. For composites or anisotrophic material, the material tensors of the two connected shell elements have to be transformed into the coordinate system of the CFAST element before the Douglas or Huth formula is applied. The resulting stiffness is applied to the KT2 and KT3 parameters on the PFAST entry. * The following symbols are used in the formulas: Symbol
Meaning
Ef
Young’s modulus of fastener
df
Diameter of fastener
l
Length of fastener, evaluated from the FE model
E1
Young’s modulus of first property connected to the fastener
t1
Thickness of first property connected to the fastener
E2
Young’s modulus of second property connected to the fastener
t2
Thickness of second property connected to the fastener
Standard Homogeneous Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CQUAD4, CTRIA3, CQUAD8, or CTRIA6 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.
156
Patran Interface to MD Nastran Preference Guide Element Properties
Chapter 2: Building A Model 157 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select one from the list using the mouse or type in the name. This defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CQUADi or CTRIAi entry. This scalar value can either be a constant value in degrees, a vector, or a reference to an existing coordinate system. This property is optional. Defines the mass not derived from the material of the element. This is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the thickness, which will be uniform over each element. This value can either be a real value or a reference to an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CQUAD4/8 and CTRIA3/6 entries and/or the T field on the PSHELL entry. This property is required.
158
Patran Interface to MD Nastran Preference Guide Element Properties
This is a list of Input Properties, available for creating a CQUADi and a CTRIAi element and a PSHELL property, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4/8 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the bottom and top most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Fiber Dist. 2 Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Revised Homogeneous Plate (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4
Revised Formulation
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.
Chapter 2: Building A Model 159 Element Properties
160
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. and this is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Chapter 2: Building A Model 161 Element Properties
P-Formulation Homogeneous Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Homogeneous
Tri/3, Quad/4,Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P-Formulation
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.The p-formulation shell element is supported in MSC . Nastran Version 69 or later. Therefore, the MD Nastran Version in the Translation Parameter form must be set to 69.
162
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties are the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. These properties are optional. Defines the mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element and this is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines a uniform thickness, which will cover each element. This property defines the T1, T2, T3, and T4 fields on the CQUAD4 or CTRIA3 entry and/or the T field on the PSHELL entry and can be either a real value or a reference to existing field definition. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of the basic system.This defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
Chapter 2: Building A Model 163 Element Properties
properties. Prop Name
Description
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Fiber Dist. 2 Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P--order Coordinate System (default elemental). Starting Porders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag that controls whether or not this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis.By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
Standard Laminate Plate (CQUAD4/PCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Laminate
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
164
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PCOMP property.
Chapter 2: Building A Model 165 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type the name in. The specified material must be a laminate material in Patran. The data in this material definition defines the settings of the MIDi, Ti, and THETAi fields on the PCOMP entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6 CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines mass not included in the mass derived from the material of the element. This is the NSM field on the PCOMP entry. This property is defined in terms of mass per unit area of the element and can be either a real value or a reference to an existing field definition. This property is optional. Defines the offset of the element‘s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
166
Patran Interface to MD Nastran Preference Guide Element Properties
Prop Name
Description
Laminate Options
Laminate option placed on the LAM field of the PCOMP/PCOMPG entry. No option implies all plies must be specified and all stiffness terms developed. MEM - all plies are specified but only membrane terms are computed. BEND - all plies specified but only bending terms computed. SMEAR - all plies specified, stacking sequence ignored and TS/T and 12I/T**3 terms set to zero. SMCORE - all plies specified with the last ply specifying core properties and the previous plies specifying face sheet properties. See the Nastran Quick Reference Guide for more details.
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Revised Laminate Plate (CQUADR/PCOMP) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Laminate
Tri/3, Quad/4
Revised Formulation
Chapter 2: Building A Model 167 Element Properties
Use this form to create a CQUADR or CTRIAR element and a PCOMP property.
Defines mass not included in the mass derived from the material of the element. This is the NSM field on the PCOMP entry. This property is defined in mass per unit area, of the element. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. The specified material must be a laminate material in Patran. The data in this material definition defines the settings of the MIDi, Ti, and THETAi fields on the PCOMP entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
See Standard Laminate Plate (CQUAD4/PCOMP), 163 for a description of the SOL 400 Laminate and Nonlinear Formulation options.
168
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Equivalent Section Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 169 Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can be either a constant value or a reference to an existing coordinate system. This property is optional.
This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4, or CQUAD8
170
Patran Interface to MD Nastran Preference Guide Element Properties
element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This property is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit area of the element. This property is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This property is the ZOFFS field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Distance 2
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Chapter 2: Building A Model 171 Element Properties
Revised Equivalent Section Plate (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4
Revised Formulation
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
172
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields, on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness, which will be used for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This value can be either a real value or a references to an existing field definition. This property is required.
Defines the basic orientation for any nonisotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA field on the CQUADR or CTRIAR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Chapter 2: Building A Model 173 Element Properties
This is a list of Input Properties available for creating a CTRIAR or CQUADR element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Distance 2
Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
174
Patran Interface to MD Nastran Preference Guide Element Properties
P-Formulation Equivalent Section Plate (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Equivalent Section
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P-Formulation
Use this form to create a CQUAD4, or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC . Nastran Version 69 or later. Therefore, the MSC .Nastran Version in the Translation Parameter form must be set to 69.
Chapter 2: Building A Model 175 Element Properties
Defines the materials to be used to describe the membrane, bending, shear, and coupling behavior of the element. A list of all materials currently in the database is displayed when data is entered. These properties define the settings of the MID1, MID2, MID3, and MID4 fields, on the PSHELL entry. Either select from the list using the mouse or type in the name. These properties are optional.
Defines the uniform thickness, which will be used for each element. This property defines the setting of the Ti, T2, T3, and T4 fields on the CTRIAR3 or CQUAD4 entry and/or the T field on the PSHELL entry. This value can be either a real value or a references to an existing field definition. This property is required.
Defines the basic orientation for any nonisotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of basic system.This property is optional.
This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these
176
Patran Interface to MD Nastran Preference Guide Element Properties
properties. Prop Name
Description
Bending Stiffness
Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio
Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset
Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3entry and can be either real value or reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real value or references to existing field definitions. This property is optional.
Fiber Dist. 2 Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields in the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Chapter 2: Building A Model 177 Element Properties
Prop Name
Description
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default, equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default, equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
Field Point Mesh (CQUAD4/TRIA3)(Exterior Acoustics) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Shell
Field Point Mesh
Tri/3, Quad/4
Use this form to create a CTRIA3, CQUAD4 elements for creating acoustic field point mesh for an exterior acoustics analysis. No property cards are created. The material referenced should be the same as that defined for the 3D solid elements and exterior acoustic infinite elements used to define the surrounding fluid environment of the structure, although no actual materials is written. In order to recover results on these meshes, you must set the output request ACFPFRESULT.
178
Patran Interface to MD Nastran Preference Guide Element Properties
Each acoustic field point mesh defined is written to a seperate section of the bulk data using the BEGIN AFPM=id.
Input Properties
Chapter 2: Building A Model 179 Element Properties
Standard Bending Panel (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
Standard Formulation
Tri/3, Quad/4 Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
180
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines the uniform thickness for each element. This defines the T1, T2, T3, and T4 fields on the CQUAD4/8 and CTRIA3/6 entries and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is required. Defines the mass not derived from the material of the element. This property is defined in mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Chapter 2: Building A Model 181 Element Properties
This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4 or CQUAD8 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties. Prop Name Fiber Dist. 1
Description Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and these values can be either real values or references to existing field definitions. These properties are optional.
Fiber Dist. 2
Revised Bending Panel (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
Revised Formulation
Tri/3, Quad/4
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
182
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Defines the uniform thickness, which will be used for each element. This defines the T1, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definitions. This property is required. Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. This property is optional.
Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can either be real values or a reference to and existing field definition. This property is optional.
Chapter 2: Building A Model 183 Element Properties
P-Formulation Bending Panel (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Bending Panel
P- Formulation
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
Use this form to create a CTRIA3, or CQUAD4 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC .Nastran Version 69 or later. Therefore, the MSC. Nastran Version in the Translation Parameters form must be set to 69.
184
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1, MID2, MID3, and MID4 fields on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis or (2) define a constant angle offset from the projected x-axis of basic system.This property defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Defines the uniform thickness, which will be used for each element. This defines the T1, T2, T3, and T4 fields on the CQUAD4 or CTRIA3 entry and/or the T field on the PSHELL entry and this value can be either a real value or a reference to an existing field definition. This property is required.
This is a list of Input Properties available for creating a CTRIA3 or CQUAD4 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form
Chapter 2: Building A Model 185 Element Properties
to view these properties. Prop Name
Description
Nonstructural Mass
Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1
Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Fiber Dist. 2
Starting P-orders and Maximum P-orders
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.
186
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Axisymmetric Solid (CTRIAX6) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Axisymmetric
Tri/3, Tri/6
Use this form to create a CTRIAX6 axisymmetric solid element. This defines an isoparametric and axisymmetric triangular cross section ring element with midside nodes.
Chapter 2: Building A Model 187 Element Properties
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the TH field on the CTRIAX6 entry. This scalar value can be either a constant value or a reference to an existing coordinate system. This property is optional.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the setting of the MID field on the CTRIAX6 entry. This property is required.
PLPLANE Axisymmetric Solid (CTRIAX, CQUADX) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option 1
Create
2D
2D Solid Axisymmetric
Option 2
Topologies
Hyperelastic
Tri/3, Tri/6, QUAD/4, QUAD/8
PLPLANE
Use this form to create axisymmetric solid elements. This defines an isoparametric and axisymmetric cross section ring element with or without midside nodes.
188
Patran Interface to MD Nastran Preference Guide Element Properties
For SOL600 solutions use the PLPLANE option and any material type. For non-SOL600 runs, use the Hypereleastic option with Mooney-Rivlin materials.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
2D Axi-Symmetric Laminated Solid Composite This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Laminate
CQUADX
Use this form to create CQUADX elements and a PLCOMP property.
Chapter 2: Building A Model 189 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PLCOMP entry to be used. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines element edge used as base ply orientation.
Not used for axisymmetric elements
190
Patran Interface to MD Nastran Preference Guide Element Properties
Standard Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4
Standard Formulation
Tri/6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 191 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior. This property is required.
The orientation of the material directions can be specified by the Material Orientation parameter value CID, Real Scalar, or Vector.
The presence of nonstructural mass in the model does not change the stiffness of the model.
Revised Plane Strain Solid (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4
Revised Formulation Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
192
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior. This property is required.
Chapter 2: Building A Model 193 Element Properties
P-Formulation Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16
P- Formulation
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The pformulation shell element is supported in MSC. Nastran Version 69 or later. Therefore, the MSC .Nastran Version in the Translation Parameters form must be set to 69.
194
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. This property is required. The MID2 field on the PSHELL entry will be set to -1 to define plane strain behavior.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis (2) define a constant angle offset from the projected x-axis of basic system. This defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
Chapter 2: Building A Model 195 Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Infinite (Exterior Acoustic Element)(CACINF3/CACINF4) These elements are used in exterior acoustic analysis (frequency response) and placed on the outside of the solid mesh representing the fluid (coincident with the outside surface). The must share the same nodes as the solid mesh. They simulate the fluid proprties reaching to infinity beyond the boundary of the solid mesh representing the fluid. The surfaces that these elements connect to must be convex. However it is not necessary that the surface be smooth. They also take on the same fluid proprties as the solid fluid mesh. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Infinite
Tri/3, Quad/4
Use this form to create a CACINF3, CACINF4 elements and a PACINF property. The appropriate fields on the PACINF entry are filled in or left blank in order to achieve the requested behavior.
196
Patran Interface to MD Nastran Preference Guide Element Properties
Interger value that defines the radial interpolation order, which must be defined and greater than zero.
The pole of the acoustic infinite elements. This must be coorinate location defined in the global Patran coordinate system. A node ID can also be selected graphically.
Defines the material to be used. This material is generally the same material used to define the solid fluid mesh in an exterior acoustics analysis (MAT10). The same material should also be referenced when using acoustic field point meshes.
2D Plane Strain Laminated Solid Composite This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Laminate
QUAD/4, QUAD/8
Use this form to create quadratic elements and a PLCOMP property.
Chapter 2: Building A Model 197 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PLCOMP entry to be used. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines element edge used as base ply orientation.
Not used for axisymmetric elements
Standard Membrane (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties
198
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
Standard Formulation
Tri/3, Quad/4 Tri /6, Quad/8
Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 199 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID1 field on the PSHELL entry. This property is required.
Defines the mass not derived from the material of the element. This property is defined in mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the uniform thickness that will be used for each element. This value can either be a real value or reference an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry and/or the T field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1)reference a coordinate system, which is then projected onto the element. (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This property defines the setting of the THETA or MCID field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
Revised Membrane (CQUADR) This subordinate form appears when the Input Properties button is selected on the Element Properties
200
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
Revised Formulation
Tri/3, Quad/4
Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.
Chapter 2: Building A Model 201 Element Properties
Defines the mass not derived from the material of the element. This property is defined in terms of mass per unit area of the element and is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional. Defines the uniform thickness that will be used for each element. This value can be either a real value or a reference to an existing field definition. This property defines the T1, T2, T3, and T4 fields on the CTRIAR or CQUADR entry and/or the T field on the PSHELL entry. This property is required.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the settings of the MID1 field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This defines the setting of the THETA or MCID field on the CTRIAR or CQUADR entry. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional.
P-Formulation Membrane (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties
202
Patran Interface to MD Nastran Preference Guide Element Properties
form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis. Action
Dimension
Type
Option(s)
Topologies
Create
2D
Membrane
P- Formulation
Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9. Tri/9, Quad/12, Tri/13, Quad/16
Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The pformulation shell element is supported in MSC .Nastran Version 69 or later. Therefore, the MSC. Nastran Version in the Translation Parameters form must be set to 69.
Chapter 2: Building A Model 203 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID1 field on the PSHELL entry. This property is required.
Defines the basic orientation for any non-isotropic material within the element. There are two ways to assign this definition: (1) reference a coordinate system, then the projected x-axis of the coordinate system is the material x-axis or (2) define a constant angle offset from the projected x-axis of basic system. This property defines the setting of the THETA or MCID field on the CQUAD4 or CTRIA3 entry. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
204
Patran Interface to MD Nastran Preference Guide Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Shear Panel (CSHEAR) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Create
2D
Shear Panel
Option(s)
Topologies Quad/4
Use this form to create a CSHEAR element and a PSHEAR property. This defines a shear panel element of the structural model.
Chapter 2: Building A Model 205 Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This defines the settings of the MID field on the PSHEAR entry. This property is required.
Defines the uniform thickness, which will be used for each element. This defines the T field on the PSHEAR entry. This property is required. This value can be either a real value or a reference to an existing field definition.
Defines the effectiveness factor for extensional stiffness along the 2-3 and 1-4 sides. This is the F2 field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines the effectiveness factor for extensional stiffness along the 1-2 and 3-4 sides. This is the F1 field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Defines mass not included in the mass derived from the material of the element. This is defined in mass per unit area of the element. This is the NSM field on the PSHEAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
206
Patran Interface to MD Nastran Preference Guide Element Properties
Additional properties on the form which do not appear on the previous page are: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHEARN entry is written for this property set. Large Strain forces the PSHEARN entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option 1
Option 2
Topologies
Create
3D
Solid
Homogeneous
Standard
Tet/4, Wedge/6
Laminate (HEX/8 only)
Formulation
Hex/8, Tet/10
P-Formulation
Wedge/15, Hex/20
Hyperelastic Formulation
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property or a CHEXA and a PCOMP property.
Chapter 2: Building A Model 207 Element Properties
208
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the settings of the MID field on the PSOLID entryor references a PCOMP entry in the case of Laminated Composites. This property is required.
Defines both the orientation of referenced nonisotropic materials and solid element results. This can be set to Global, Elemental, or to a specific coordinate frame reference and defines the CORDM field on the PSOLID entry. The default is Global. Nonlinear stresses and strains are output in the Elemental system regardless of the setting. Defines where the output for these elements are to be reported. This property can be set to either Gauss or Grid and is the STRESS field on the PSOLID entry. This property is optional.
Defines the type of integration network to be used. This property is the IN field on the PSOLID entry and can be set to Bubble, Two, or Three. This property is optional.
Defines the integration scheme to be used. This property is the ISOP field on the PSOLID entry and can be set to Reduced or Full. This property is optional.
Chapter 2: Building A Model 209 Element Properties
Additional properties on the form which do not appear on the previous page are: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
P-Formulation Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis: Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
P-Formulation
Tet/4, Wedge/6 Hex/8, Tet/10 Wedge/15, Hex/20, Tet/16, Tet/40, Wedge/24,Wedge/52, Hex/32, Hex/64
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property.
210
Patran Interface to MD Nastran Preference Guide Element Properties
Defines orientation for the referenced material. This property can be set to Global, Elemental or to a user-defined coordinate system and defines the CORDM field on the PSOLID entry. The default is Global. This property is optional.
Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coord. System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PSOLID entry. This property is required.
Chapter 2: Building A Model 211 Element Properties
Additional properties on the form which do not appear on the previous page are: Prop Name
Description
P-order Coord. System
The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate
Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity
Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance
The tolerance used to determine if the adaptive analysis is complete. By default the value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value
Elements with von Mises stress below this value will not participate in the error analysis. By default the value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value
Elements with von Mises strain below this value will not participate in the error analysis. By default the value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Integration Network
Defines the type of integration network to be used. This property is the IN field on the PSOLID entry and can be set to Bubble, Two, or Three. This property is optional.
Integration Scheme
Defines where the output for these elements are to be reported. This can be set to either Gauss or Grid. This property is the STRESS field on the PSOLID entry. This property is optional.
Hyperelastic Plane Strain Solid (CQUAD4) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Plane Strain
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Hyperelastic Formulation
212
Patran Interface to MD Nastran Preference Guide Element Properties
Use this form to create a CQUAD, CQUAD4, CQUAD8, CTRIA3, or CTRIA6 element and a PLPLANE property.
Identification number of a coordinate system defining the plane of deformation. This defines the CID field on the PLPLANE entry.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLPLANE entry. This property is required.
Hyperelastic Axisym Solid (CTRIAX6) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
2D
2D Solid
Axisymmetric
CQUADX,
Hyperelastic Formulation
CTRIAX
Chapter 2: Building A Model 213 Element Properties
Use this form to create a CQUADX or CTRIAX element and a PLPLANE property.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLPLANE entry. This property is required.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLPLANE entry.
214
Patran Interface to MD Nastran Preference Guide Element Properties
Hyperelastic Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for a nonlinear analysis: Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
Hyperelastic Formulation
HEX, PENT, TET
Use this form to create a CHEXA, CTETRA, or CPENTA element and a PLSOLID property.
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the setting of the MID field on the PLSOLID entry. This property is required.
Location of stress and strain output. the options are “GAUS” (default) or “GRID.” this defines the STR field on the PLSOLID entry.
Chapter 2: Building A Model 215 Element Properties
Additional properties on the form which do not appear on the form above: Nonlinear Formulation
This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 376.
3D Laminate Solid (CHEXA) This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Action
Dimension
Type
Option(s)
Topologies
Create
3D
Solid
Laminate
HEX, PENT, TET
Use this form to create CHEXA elements and a PCOMP (SOL 600) or PCOMPLS (SOL400) property.
216
Patran Interface to MD Nastran Preference Guide Element Properties
Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse or type in the name. This property defines the PCOMP entry to be used. This property is required.
Defines element face used as base ply orientation.
Defines the basic orientation for any non-isotropic material within the element. There are three ways to assign this definition: (1) reference a coordinate system, which is then projected onto the element, (2) define a vector that will be projected onto the element, or (3) define a constant angle offset from the default element coordinate system. This scalar value can either be a constant value or a reference to an existing coordinate system. This property is optional. Note: Only method 3 is supported in this release.
Defines available laminate options “MEM”, “BEND”, “SMEAR”, “SMCORE” (see MD Nastran QRG for definitions.
Chapter 2: Building A Model 217 Beam Modeling
2.8
Beam Modeling Modeling structures composed of beams can be more complicated than modeling shell, plate, or solid structures. First, it is necessary to define bending, extensional, and torsional stiffness that may be complex functions of the beam cross sectional dimensions. Then it is necessary to define the orientation of this cross section in space. Finally, if the centroid of the cross section is offset from the two finite element nodes defining the beam element, these offsets must be explicitly defined. Fortunately, Patran provides a number of tools to simplify these aspects of modeling.
Cross Section Definition The cross section properties are defined on the element property forms shown on pages General Section Beam (CBAR), 102 and Tapered Beam (CBEAM), 119. The properties can be entered directly into the data boxes labeled Area, Inertia i,j, Torsional Constant, etc. or by pushing the large I-beam icon on these forms to access the Beam Library form. The Beam Library forms are a much more convenient way of defining properties for standard cross sections and are shown below. Create Action The first step in using the beam library is to select the section icon for the particular cross section desired (e.g. I-section).Then the dimensions for each of the components of the beam section must be entered.
218
Patran Interface to MD Nastran Preference Guide Beam Modeling
Current beam section as selected from the section library icon palette. The required dimensions are shown. Enter the dimensions of the beam section here, referring to the beam section icon.
Writes the current beam properties to a report file. Calculates the beam properties based on the current dimensions and displays an image of the scaled section along with the properties.
These forward and backward arrows provide access to additional beam section icons. Beam section library icon palette. Select the icon representing the desired section.
Beam section name to be created. List of existing beam sections. This list can be filtered to contain only the section names of interest using the filter mechanism.
Chapter 2: Building A Model 219 Beam Modeling
Finally, a section name must be entered and the Apply button pushed. The other options available with the beam library are documented in the Patran Reference Manual, see Beam Library (p. 475) in the Patran Reference Manual. Once one or more beam sections have been defined, these can be selected in the section data box on the element properties form. Supplied Functions
I-Beam - Six dimensions -- lower flange thickness (t1), upper flange thickness (t2),lower flange width (w1), upper flange width (w2), overall height (H), and web thickness (t)-- allows for symmetric or unsymmetrical I-beam definition. Angle - Open section, four dimensions -- overall height (H), overall width (W), horizontal flange thickness (t1), vertical flange thickness (t2).
Tee - Four dimensions -- overall height (H), overall width (W), horizontal flange thickness (t1), vertical flange thickness (t2).
Solid-Rod - Solid section, one dimension -- radius (R).
Box-Symmetric - Closed section, four dimensions -- overall height (H), overall width (W), top and bottom flange thicknesses (t1), side flange thicknesses (t2).
Tube - Closed section, two dimensions -- outer radius (R1), inner radius (R2).
Channel - Open section, four dimensions -- overall height (H), overall width (W), top and bottom flange thicknesses (t1), shear web thickness (t).
220
Patran Interface to MD Nastran Preference Guide Beam Modeling
Bar - Solid section, two dimensions -- height (H) and width (W).
Box-Unsymmetrical - Closed section, six dimensions -- overall height (H), overall width (W), top flange thickness (t1), bottom flange thickness (t2), right side flange thickness (t3), left side flange thickness (t4). Hat - Four dimensions -- overall height (H), top of hat flange width (W), bottom of hat flange width for one side (W1), thickness (t).
H-Beam - Four dimensions -- overall height (H), width between inner edges of vertical flanges (W), horizontal shear web thickness (t), and thickness of one vertical flange (W1/2). Cross - Four dimensions -- overall height (H), vertical flange thickness (t), horizontal flange thickness (t2), length of free horizontal flange for one side (W/2).
Z-Beam - Four dimensions -- overall height (H2), height of vertical flange between as measured between horizontal flanges, length of free horizontal flange for one side (W), thickness (t1). Hexagonal - Solid section, three dimensions -- overall height (H), overall width (W), horizontal distance from side vertex to top or bottom surface vertex along the common edge (i.e., diagonal edge hypotenuse times the cosine of the exterior diagonal angle).
Cross Section Orientation The Bar Orientation data box on the Input Properties form is used to define how the y-axis of the beam cross section is oriented in space. By default the Value Type is Vector. This tells MSC Nastran that the cross section y-axis lies in the plane defined by the beam’s x-axis (the line connecting the two node points) and this vector. The Value Type pop up menu may be changed to Node ID. In this case the y-axis lies in the plane defined by the x-axis and the selected node.
Chapter 2: Building A Model 221 Beam Modeling
When the Value Type is Vector and the Bar Orientation data box is selected the following select box appears on the screen. These select tools provide different options for defining vectors. They are discussed in more detail in the Select Menu (p. 35) in the Patran Reference Manual.
These three tools define the orientation vector as the 1 (x), 2(y), or 3(z) axis of a selected coordinate system. This is a convenient way to specify the orientation when it is aligned with one of the three axes of a rectangular coordinate system. When the system is not rectangular (e.g. cylindrical) these tools may not provide the desired definition because the defined vector does not change direction at different points in space--these tools just provide an alternate way to define a global vector.
This tool may be used to define a general vector with respect to an alternate coordinate system. When this icon is picked, the select menu changes to the one on the right.
These tools provide different ways to define vectors. In addition, the user is requested to select a coordinate system in which this vector is defined. The simplest list processor syntax that appears in the databox for a vector in an alternate coordinate system is <x_component, y_component, z_component> coord cord_id (e.g. <1, 0, 0> coord 3). In many cases it is easy to simply type a definition in this form into the Bar Orientation databox.
After the orientation has been defined, there are two ways to verify its correctness in Patran. The first option is in the Element Properties application. By selecting the Show Action, the Definition of X Y Plane property, and Display Method Vector Plot, the vectors defining the orientation will be shown on the model. A second option can be used when the Beam Library has been used to define the beam cross section. There is an option on the Display form Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual called Beam Display. The menu allows different display options for displaying an outline of the defined cross section on the model in the correct location and orientation. Users should be aware of one difference between the Patran and MD Nastran definitions for cross section orientation. In Patran the orientation is completely independent of the analysis coordinate system at the beam nodes. In MD Nastran, the orientation vector is assumed to be defined in the same system as the analysis system at the first node of the beam. In Patran it is perfectly permissible to define the orientation in a different coordinate system from that analysis system. When the NASTRAN input file is generated, the necessary transformation of this vector to the analysis system at node 1 will be performed.
222
Patran Interface to MD Nastran Preference Guide Beam Modeling
Cross Section End Offsets Two data boxes are provided on the Element Properties, Input Properties form to optionally define an offset from either node 1 to the cross section centroid (Offset @ Node 1) or from node 2 to the cross section centroid (Offset @ Node 2). The same select menu tools are available for defining these vectors. One difference between the orientation definition and the offset definitions, however, is that for the offset the magnitude of the vector is important. Because of this, the select menu tools are usually not very convenient. Typically, offsets are defined by typing the definition (e.g <x, y, z> or <x, y, z> coord n>) into the appropriate data box. Two options are available for verifying the definitions of offsets; these options are very similar to those for orientations. The Element Properties, Show Action will allow the end offsets to be displayed as vectors on the model. This option is not especially useful because the vector plot shows only the direction of the offset, not the magnitude of the offset. It is usually much more useful to view the Beam Display menu on the Display form Display>LBC/Element Property Attributes (p. 385) in the Patran Reference Manual to select the display option with offsets. The viewport will then show the beam displayed in both the offset and non-offset positions.
Stiffened Cylinder Example Figure 2-1 shows a simple example of a circular cylinder stiffened with Z-stiffeners. The cross section
was defined by selecting the Beam Library icon on the Element Properties/Input Properties form. The Z cross section was selected on the Beam Library form, the cross section dimensions input, a section name input, and the Apply button pushed. On the Input Properties form, the Use Beam Section toggle is set to ON. The defined section name is selected in the [Section Name] data box. The string <-1.0 0. 0.> coord 1 is typed into the Bar Orientation data box to align the cross section orientation with the radial direction of the global, cylindrical system. Similarly, the strings <-2.0 0.0 0.0> coord 1 and <-2.0 0.0 0.0> coord 1
Chapter 2: Building A Model 223 Beam Modeling
typed into the Offset @ Node 1 and Offset @ Node 2 data boxes define the end offsets to be radially inward.
T Z1
Y Z
Figure 2-1
X
Stiffened Cylinder
R
224
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
2.9
Loads and Boundary Conditions The Loads and Boundary Conditions form will appear when the Loads/BCs toggle, located on the Patran main form, is chosen. When creating a load and boundary condition there are several option menus. The selections made on the Loads and Boundary Conditions menu will determine which load and boundary conditions form appears, and ultimately, which MD Nastran loads and boundary conditions will be created. The following pages give an introduction to the Loads and Boundary Conditions form and details of all the loads and boundary conditions supported by the Patran MD Nastran Analysts Preference.
Loads & Boundary Conditions Form This form appears when Loads/BCs is selected on the main menu. The Loads and Boundary Conditions form is used to provide options to create the various MD Nastran loads and boundary conditions. For a definition of full functionality, see Loads and Boundary Conditions Form (p. 27) in the Patran Reference Manual. Options for defining slide line contact are also accessed from this main Loads and Boundary Conditions form. For more information see Defining Contact Regions, 247.
Chapter 2: Building A Model 225 Loads and Boundary Conditions
Defines the general load type to be applied. Object choices are Displacement, Force, Pressure, Temperature, Inertial Load, Initial Displacement, Initial Velocity, Velocity, Acceleration, Distributed Load, CID Distributed Load, Total Load, Contact, Initial Temperature, Planar Rigid Wall and Init.Rotation Field.
Defines what type of region is to be loaded. The available options depend on the selected Object. The general selections can be Nodal, Element Uniform, or Element Variable. Nodal is applied explicitly to nodes. Element Uniform defines a constant value to be applied over an entire element, element face, or element edge. Element Variable defines a value that varies across an entire element, element face, or element edge.
Current Load Case type is set on the Load Case menu. When the Load Cases toggle located on the main menu is chosen, the Load Cases menu will appear. Under Load Case Type, select either Static or Time Dependent, then enter the name of the case, and click on the Apply button.
Generates either a Static, 226 or Time Dependent, 229 Input Data form, depending on the current Load Case Type.
226
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
The following table outlines the options when Create is the selected Action. Object • Displacement
Type • Nodal • Element Uniform • Element Variable
• Force
• Nodal
• Pressure
• Element Uniform • Element Variable
• Temperature
• Nodal • Element Uniform • Element Variable
• Inertial Load
• Element Uniform
• Initial Displacement
• Nodal
• Initial Velocity
• Nodal
• Velocity
• Nodal
• Acceleration
• Nodal
• Distributed Load
• Element Uniform • Element Variable
• CID Distributed Load
• Element Uniform • Element Variable
• Total Load
• Element Uniform
• Contact
• Element Uniform
• Initial Plastic Strain
• Element Uniform
• Initial Stress
• Element Uniform
• Initial Temperature
• Nodal
• Planar Rigid Wall *
• Nodal
• Init. Rotation Field *
• Nodal
* For SOL 700 only. Static
This subordinate form appears when the Input Data button is selected on the Loads and Boundary Conditions form and the Current Load Case Type is Static. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 224. The information on the
Chapter 2: Building A Model 227 Loads and Boundary Conditions
Input Data form will vary depending on the selected Object. Defined below is the standard information found on this form.
228
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Defines a general scaling factor for all values defined on this form. The default value is 1.0. Primarily used when field definitions are used to define the load values.
Input Data in this section will vary. See Object Tables, 231 for detailed information. When specifying real values in the Input Data entries, spatial fields can be referenced. All defined spatial fields currently in the database are listed. If the input focus is placed in the Input Data entry and a spatial field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
This button will display a Discrete FEM Fields input form to allow field creation and modification within the loads/bcs application. Visible only when focus is set in a databox which can have a DFEM field reference.
Defines the coordinate frame used to interpret the degree-of-freedom data defined on this form. This only appears on the form for Nodal type loads. This can be a reference to any existing coordinate frame definition.
Chapter 2: Building A Model 229 Loads and Boundary Conditions
Time Dependent
This subordinate form appears when the Input Data button is selected on the Loads and Boundary Condition form and the Current Load Case Type is Time Dependent. The Current Load Case Type is set on the Load Case form. For more information see Loads & Boundary Conditions Form, 224 and Load Cases, 246. The information on the Input Data form will vary, depending on the selected Object. Defined below is the standard information found on this form.
230
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data Load/BC Set Scale Factor
1 Spatial Dependence
* Time Dependence
Defines a general scaling factor for all values defined on this form.The default value is 1.0. Primarily used when field definitions are used to define the load values.
Trans Accel (A1,A2,A3) Input Data in this section will vary. See Object Tables, 231 for detailed information.
Rot Velocity (w1,w2,w3)
Rot Accel (a1,a2,a3)
Spatial Fields
Time Dependent Fields
FEM Dependent Data...
When specifying time dependent values in the Input Data entries, timedependent fields can be referenced. All defined timedependent fields currently in the database are listed. If the input focus is placed in the Input Data entry and a timedependent field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
Analysis Coordinate Frame Coord 0
OK
Reset
This button will display a Discrete FEM Fields input form to allow field creation and modification within the loads/bcs application. Visible only when focus is set in a databox which can have a DFEM field reference.
Defines the coordinate frame to be used to interpret the degree-of-freedom data defined on this form. This only appears on the form for Nodal type loads. This can be a reference to any existing coordinate frame definition.
When specifying real values in the Input Data entries, spatial fields can be referenced. All defined spatial fields currently in the database are listed. If the input focus is placed in the Input Data entry and a spatial field is selected by clicking in this list, a reference to that field will be entered in the Input Data entry.
Chapter 2: Building A Model 231 Loads and Boundary Conditions
Object Tables These are areas on the static and transient input data forms where the load data values are defined. The data fields that appear depend on the selected load Object and Type. In some cases, the data fields also depend on the selected Target Element Type. The following Object Tables outline and define the various input data that pertains to a specific selected object: Displacement / Velocty / Acceleration
Object
Type
Analysis Type
Option
Displacement Velocity Acceleration
Nodal
Structural
Standard
Creates MD Nastran SPC1 and SPCD Bulk Data for Displacement entries. All non blank entries will cause an SPC1 entry to be created. If the specified value is not 0.0, an SCPD entry will also be created to define the non zero enforced displacement or rotation. Phase angle specifications will create DPHASE entries for all corresponding non blank translational or rotational data in frequency response analysis. Displacement, Velocity and Acceleration LBCs used in frequency response / dynamic analysis also define the RLOAD1 entries with DISP, VELOC, and ACCEL keywords, respectively. For frequency response analysis, the LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this. Values given via this option are total enforced values. For relative enforced values used in SOL 400, see the description for the Relative Displacement option below. Input Data
Description
Translations (T1,T2,T3)
Defines the total enforced translational values. These are in model length units.
Rotations (R1,R2,R3)
Defines the total enforced rotational values. These are in radians.
Translational Phase Angles (Tth1,Tth2,Tth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the translational values. These are in degrees.
Rotational Phase Angles (Rth1,Rth2,Rth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the rotational values. These are in degrees.
Object
Type
Analysis Type
Dimension
Displacement
Element Uniform
Structural
3D
Element Variable Applies a zero or nonzero total displacement boundary condition to the face of solid elements. The primary use of this boundary condition is to apply constraints to p-elements; but it may also be used for standard solid elements. If applied to a p-element solid, the appropriate FEFACE and GMBC entries are created. If applied to a standard solid element, the appropriate SPC1 and SPCD entries are created. In
232
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
frequency response analysis, the phase angles are written as DPHASE entries. See comments above for nodal displacements. Input Data
Description
Translations (T1,T2,T3)
Defines the enforced translational displacement values. These values are in model-length units.
Translation Phases (Tth1,Tth2,Tth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the translational displacement values. These are in degrees.
Object
Type
Analysis Type
Option
Displacement
Nodal
Structural
Relative Displacement
Applies a zero or nonzero relative displacement boundary condition as opposed to a total magnitude. This is used in SOL 400 only with multiple steps and not applicable to other solution sequences. This LBC will be ignored if present in a referenced load case for solution sequences other than SOL 400. The appropriate SPC1 and SPCR entries are created. For example, if a DOF is specified on a SPCR with 0.0 for step 2, the relative displacement of this DOF for step 2 with respective to step 1 is 0.0. The total displacement of step 2 is 0.2 if the solution of step 1 for this DOF is 0.2. Input Data
Description
Relative Translations (T1,T2,T3) Defines the relative enforced translational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced translation is to be specified, the particular component should be left blank. Relative Rotations (R1,R2,R3)
Defined the relative enforced rotational displacement values in vector form, each value separated by a comma between the brackets <>. If no enforced rotation is to be specified, the particular component should be left blank.
Force
Object
Type
Analysis Type
Force
Nodal
Structural
Creates MD Nastran FORCE and MOMENT Bulk Data entries. Creates the DPHASE entries in frequency response analysis when specifying phase angles for out-of-phase loading. RLOAD1 entries are created for dynamic analysis and reference the appropriate FORCE entries. For frequency response analysis, the force LBCs must reference a frequency range of interest defined as a non-spatial frequency field such that a TABLEDi entry is created. The load case needs to be defined as Time/Frequency dependent to do this.
Chapter 2: Building A Model 233 Loads and Boundary Conditions
Input Data
Description
Force (F1,F2,F3)
Defines the applied forces in the translation degrees of freedom. This defines the N vector and the F magnitude on the FORCE entry.
Moment (M1,M2,M3)
Defines the applied moments in the rotational degrees of freedom. This defines the N vector and the M magnitude on the MOMENT entry.
Force Phase Angles (Fth1,Fth2,Fth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding force components. These are in degrees.
Moment Phase Angles (Mth1,Mth2,Mth3)
Defines the phase angle for out-of-phase loading in frequency response analysis for the corresponding moment components. These are in degrees.
Pressure
Object
Type
Analysis Type
Dimension
Pressure
Element Uniform
Structural
2D
Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries. Input Data
Description
Top Surf Pressure
Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. These values are all equal for a given element, producing a uniform pressure field across that face.
Bot Surf Pressure
Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values.These values are all equal for a given element, producing a uniform pressure field across that face.
Edge Pressure
For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (i.e. independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated at the middle of the application region.
Object
Type
Analysis Type
Dimension
Pressure
Element Uniform
Structural
3D
Creates MD Nastran PLOAD4 Bulk Data entries.
234
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Pressure
Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated once at the center of the applied region.
Object
Type
Analysis Type
Dimension
Pressure
Element Variable
Structural
2D
Creates MD Nastran, PLOAD4, PLOADX1, or FORCE Bulk Data entries. Input Data
Description
Top Surf Pressure
Defines the top surface pressure load on shell elements using a PLOAD4 entry. The negative of this value defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values.
Bot Surf Pressure
Defines the bottom surface pressure load on shell elements using a PLOAD4 entry. This value defines the P1 through P4 values. If a scalar field is referenced, it will be evaluated separately for the P1 through P4 values.
Edge Pressure
For Axisymmetric Solid elements (CTRIAX6), defines the P1 through P3 values on the PLOADX1 entry where THETA on that entry is defined as zero. For other 2D elements, this will be interpreted as a load per unit length (e.g., independent of thickness) and converted into equivalent nodal loads (FORCE entries). If a scalar field is referenced, it will be evaluated independently at each node.
Object
Type
Analysis Type
Dimension
Pressure
Element Variable
Structural
3D
Creates MD Nastran PLOAD4 Bulk Data entries.
Chapter 2: Building A Model 235 Loads and Boundary Conditions
Input Data
Description
Pressure
Defines the face pressure value on solid elements using a PLOAD4 entry. This defines the P1, P2, P3, and P4 values. If a scalar field is referenced, it will be evaluated separately for each of the P1 through P4 values.
Temperature
Object
Type
Analysis Type
Temperature
Nodal
Structural
Creates MD Nastran TEMP Bulk Data entries. Input Data
Description
Temperature
Defines the T fields on the TEMP entry.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform
Structural
1D
Creates MD Nastran TEMPRB Bulk Data entries. Input Data Temperature
Description Defines a uniform temperature field using a TEMPRB entry. The temperature value is used for both the TA and TB fields. The T1a, T1b, T2a, and T2b fields are all defined as 0.0.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform
Structural
2D
Creates MD Nastran TEMPP1 Bulk Data entries. Input Data
Description
Temperature
Defines a uniform temperature field using a TEMPP1 entry. The temperature value is used for the T field. The gradient through the thickness is defined to be 0.0.
Object
Type
Analysis Type
Dimension
Temperature
Element Variable
Structural
1D
Creates MD Nastran TEMPRB Bulk Data entries.
236
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Centroid Temp
Defines a variable temperature file using a TEMPRB entry. A field reference will be evaluated at either end of the element to define the TA and TB fields.
Axis-1 Gradient
Defines the temperature gradient in the 1 direction. A field reference will be evaluated at either end of the element to define the T1a and T1b fields.
Axis-2 Gradient
Defines the temperature gradient in the 2 direction. A field reference will be evaluated at either end of the element to define the T2a and T2b fields.
Object
Type
Analysis Type
Dimension
Temperature
Element Variable
Structural
2D
Creates MD Nastran TEMPP1 Bulk Data entries. Input Data
Description
Top Surf Temp
Defines the temperature on the top surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry.
Bot Surf Temp
Defines the temperature on the bottom surface of a shell element. The top and bottom values are used to compute the average and gradient values on the TEMPP1 entry.
Object
Type
Analysis Type
Dimension
Temperature
Element Uniform Element Variable
Structural
1D, 2D, 3D
This option applies only to the P-formulation elements. A TEMPF and DEQATN entry are created for the constant temperature case. A TEMPF and TABLE3D entry are created for the case when a spatial field is referenced. Input Data Temperature
Description Defines the temperature or temperature distribution in the element.
Inertial Load
Object
Type
Analysis Type
Inertial Load
Element Uniform
Structural
Creates MD Nastran GRAV and RFORCE Bulk Data entries.
Chapter 2: Building A Model 237 Loads and Boundary Conditions
Input Data
Description
Trans Accel (A1,A2,A3)
Defines the N vector and the G magnitude value on the GRAV entry.
Rot Velocity (w1,w2,w3)
Defines the R vector and the A magnitude value on the RFORCE entry.
Rot Accel (a1,a2,a3)
Defines the R vector and the RACC magnitude value on the RFORCE entry.
The acceleration and velocity vectors are defined with respect to the input analysis coordinate frame. The origin of the rotational vectors is the origin of the analysis coordinate frame. Note that rotational velocity and rotational acceleration cannot be defined together in the same set.In generating the GRAV and RFORCE entries, the interface produces one GRAV and/or RFORCE entry image for each Patran load set. Initial Displacement
Object
Type
Analysis Type
Initial Displacement
Nodal
Structural
Creates a set of MD Nastran TIC Bulk Data entries. Input Data
Description
Translations (T1,T2,T3)
Defines the U0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Rotations (R1,R2,R3)
Defines the U0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Initial Velocity
Object
Type
Analysis Type
Initial Velocity
Nodal
Structural
Creates a set of MD Nastran TIC Bulk Data entries.
238
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input Data
Description
Trans Veloc (v1,v2,v3)
Defines the V0 fields for translational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Rot Veloc (w1,w2,w3)
Defines the V0 fields for rotational degrees of freedom on the TIC entry. A unique TIC entry will be created for each non blank entry.
Distributed Load
Object
Type
Analysis Type
Dimension
Distributed Load
Element Uniform Element Variable
Structural
1D
Defines distributed force or moment loading along beam elements using MD Nastran PLOAD1 entries. The coordinate system in which the load is applied is defined by the beam axis and the Bar Orientation element property. The Bar Orientation must be defined before this Distributed Load can be created. If the Bar Orientation is subsequently changed, the Distributed Load must be updated manually if necessary. For the element variable type, a field reference is evaluated at each end of the beam to define a linear load variation. Input Data
Description
Edge Distributed Load (f1,f2,f3)
Defines the FXE, FYE, and FZE fields on three PLOAD1 entries.
Edge Distributed Moment (m1,m2,m3)
Defines the MXE, MYE, and MZE fields on three PLOAD1 entries.
Object
Type
Analysis Type
Dimension
Distributed Load
Element Uniform Element Variable
Structural
2D
Defines a distributed force or moment load along the edges of 2D elements. The coordinate system for the load is defined by the surface or element edge and normal. The x direction is along the edge. Positive x is determined by the element corner node connectivity. See Patran Element Library (p. 341) in the Reference Manual - Part III. For example, if the element is a CQUAD4, with node connectivity of 1, 2, 3, 4. The positive x directions for each edge would be from nodes 1 to 2, 2 to 3, 3 to 4, and 4 to 1. The z direction is normal to the surface or element. Positive z is in the direction of the element normal. The y direction is normal to x and z. Positive y is determined by the cross product of the z and x axes and always points into the element. The MD Nastran entries generated, depend on the element type. For the element variable type, a field reference is evaluated at all element nodes lying on the edge.
Chapter 2: Building A Model 239 Loads and Boundary Conditions
Input Data
Description
Edge Distributed Load (f1,f2,f3)
For axisymmetric solid elements (CTRIAX6), the PA, PB, and THETA fields on the PLOADX1 entry are defined. For other 2D elements, the input vector is interpreted as load per unit length and converted into equivalent nodal loads (FORCE entries).
Edge Distributed Moment (m1,m2,m3)
For 2D shell elements, the input vector is interpreted as moment per unit length and converted into equivalent nodal moments (MOMENT entries).
Contact
Object
Type
Analysis Type
Contact
Element Uniform
Structural
This form is used to define certain data for the MD Nastran Input entries. Other data entries are defined under the Analysis Application when setting up a job for nonlinear static or nonlinear transient dynamic analysis. A contact table is also supported; by default, all contact bodies initially have the potential to interact with all other contact bodies and themselves. This default behavior can be modified under the Contact Table form, located on the Solution Parameters subform in the Analysis Application when creating a Load Step. Preview Rigid Body Motion After defining the Input Properties you can use the Preview Rigid Body Motion to check the movement of the rigid bodies in place. This is an effective tool for verifying the directions for LBCs.
240
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Slideline (SOL 400 and SOL 600) Input
Description
Penetration Type
If the Penetration Type is One Sided, nodes in the Slave Region are not allowed to penetrate the segments of the Master Region. If Symmetric, in addition, nodes in the Master Region are not allowed to penetrate segments of the Slave Region.
Static Friction Coefficient (MU1)
Coefficient of static friction between the two surfaces.
Stiffness in Stick (FSTIF)
FSTIF is a penalty parameter in the contact formulation. The default value is usually adequate.
Penalty Stiffness Scaling Factor (SFAC)
SFAC is a penalty parameter in the contact formulation. The default value is usually adequate.
Slideline Width (W1)
Slideline Width is constant along the slideline and is used to determine the area for contact stress calculation. This is the Wi field on the BFRIC entry.
Vector Pointing from A vector must be defined which lies in the contact plane and points from the Master to Slave Surface Master region to the Slave region. This vector is used to define the coordinate system on the BCONP entry and the BLSEG entries for each region.
Chapter 2: Building A Model 241 Loads and Boundary Conditions
Deformable Body (SOL 400, SOL 600, and SOL 700 ) .
Description Friction Coefficient (MU)
Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients, the average value is used.
Define (type of contact) Select 1) Analytic Contact, 2) Contact Area, 3) Exclusion Region, or 4) Glue Deactivation. The Contact Area and Exclusion Region are defined using MD Nastran entry BCHANGE in the .bdf file, with NODE for Contact Area, and EXCLUDE for Exclusion Region. The Glue Deactivation is defined using MD Nastran entry UNGLUE. Boundary Type
Select either 1) Analytic, or 2) Discrete. By default, a deformable contact body boundary is defined by the free faces of its elements; this is used by the Discrete option. However, instead of using the free faces of the elements (Discrete), it is possible to use spline surfaces (2D) to represent the outer faces (element faces) of the contact bodies; this is used by the Analytic option. The Analytic option can improve the accuracy of deformabledeformable contact analysis.
C0 Continuity
Using this, enforces C0-continuity at edges where the normal vector to the outer contour of the structure indicates a discontinuity. This is enabled for 3D analysis only.
Auto Detect Discontinuities
Select this to cause the automatic detection of any discontinuity.
Feature Angle
If the angle between the normals of two touching (adjacent) segments of contact bodies is greater than the Feature Angle, there is a discontinuity there, and the discontinuity (at edge) is preserved.
MFD Increment
The MFD file contains the spline surfaces that were created to represent some or all of the outer faces of the contact model. Using this causes the spline surfaces to be written to an MFD file every nth increment. This file is an Patran database, and can be opened with Patran, and the spline surfaces can be compared with the contact model.
Select Discontinuities...
See Select Deactivation Region, 242
Edge Contact...
See Edge Contact Subform, 242
Select Contact Area...
See Select Contact Area, 242
Select Exclusion Region...
See Select Exclusion Region, 242
Select Deactivation Region...
See Select Deactivation Region, 242
Select Discontinuities Subform
242
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
.
Description Select (entity type)
Choose to either select Geometry or FEM to define any discontinuities.
Detect Discontinuities
Click on this button to determine if there are any discontinuities for the entities that define the Application Region.
Define Discontinuities
Select entities to define the discontinuities.
Edge Contact Subform .
Description Include Outside (Solid Element)
When detecting contact of solid elements (for example, CHEXA elements) use this to include contact of the outside of the elements. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact).
Check Layers (Shell Element)
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges (Edges)
Use this to specify how body surfaces may contact. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCBODY entry (defines a flexible or rigid contact body in 2D or 3D) of the MD Nastran QRG. The entry that is used for the BCBODY entry is COPTB (flag that indicates how body surfaces may contact).
Select Contact Area .
Description Select (entity type)
Choose to either select Geometry or FEM to define the contact area.
Define Contact Area
Select entities to define the contact area.
Select Exclusion Region .
Description Select (entity type)
Choose to either select Geometry or FEM to define the exclusion region.
Define Exclusion Region
Select entities to define the exclusion region.
Select Deactivation Region
Chapter 2: Building A Model 243 Loads and Boundary Conditions
.
Description Select (entity type)
Choose to either select Geometry or FEM to define the glue deactivation region.
Define Deactivated Entities
Select entities to define the entities that are to be un-glued.
Rigid Body (SOL 600 and SOL 700 only) The input data form differs for 1D and 2D rigid bodies. One dimensional rigid surfaces are defined as beam elements, or as curves (which may optionally be meshed with beam elements prior to translation) and used in 2D problems. Two dimensional rigid surfaces must be defined as Quad/4 or Tri/3 elements, or as surfaces (which may optionally be meshed with Quad/4 or Tri/3 elements prior to translation) and are used in 3D problems. The elements will be translated as 4-node patches if meshed or as NURB surfaces if not meshed.
244
Patran Interface to MD Nastran Preference Guide Loads and Boundary Conditions
Input
Description
Flip Contact Side
Upon defining each rigid body, MSC.Patran displays normal vectors or tic marks. These should point inward to the rigid body. In other words, the side opposite the side with the vectors is the side of contact. Generally, the vector points away from the body in which it wants to contact. If it does not point inward, then use the modify option to turn this toggle ON. The direction of the inward normal will be reversed.
Symmetry Plane
This specifies that the surface or body is a symmetry plane. It is OFF by default.
Null Initial Motion
This toggle is enabled only for Velocity and Position type of Motion Control. If it is ON, the initial velocity, position, and angular velocity/rotation are set to zero in the CONTACT option regardless of their settings here (for increment zero).
Motion Control
Motion of rigid bodies can be controlled in a number of different ways: velocity, position (displacement), or forces/moments.
Velocity (vector)
For velocity controlled rigid bodies, define the X and Y velocity components for 2D problems or X, Y, and Z for 3D problems.
Angular Velocity (rad/time)
For velocity controlled rigid bodies, if the rigid body rotates, give its angular velocity in radians per time (seconds usually) about the center of rotation (global Z axis for 2D problems) or axis of rotation (for 3D problems).
Friction Coefficient (MU)
Coefficient of static friction for this contact body. For contact between two bodies with different friction coefficients the average value is used.
Rotation Reference Point
This is a point or node that defines the center of rotation of the rigid body. If left blank the rotation reference point will default to the origin.
Axis of Rotation
For 2D rigid surfaces in a 3D problem, aside from the rotation reference point, if you wish to define rotation you must also specify the axis in the form of a vector.
First Control Node
This is for Force or SPCD controlled rigid motion. It is the node to which the force or SPCD is applied. A separate LBC must be defined for the force, but the application node must also be specified here. If both force and moment are specified, they must use different control nodes even if they are coincident. If only 1 control node is specified the rigid body will not be allowed to rotate.
Second Control Node
This is for Moment controlled rigid motion. It is the node to which the moment is applied. A separate LBC must be defined for the moment, but the application node must also be specified here. It also acts as the rotation reference point. If both force and moment are specified, they must use different control nodes even if they are coincident.
Planar Rigid Wall (SOL 700 only)
Chapter 2: Building A Model 245 Loads and Boundary Conditions
Object
Type
Analysis Type
Planar Rigid Wall
Nodal
Explicit Nonlinear
Two different planar rigid wall options exist: 1. Kinematic rigid wall without friction 2. Penalty method based rigid wall with friction These are seen as options at the top of the Input Data form. The user must select which wall will be used. Both wall’s position and orientation are defined by selecting a coordinate system which has its origin on the plane and the local z axis as the outward normal from the contact surface. This defines a WALL Bulk Data entry. There are only parameters associated with the penalty based planar rigid wall. Input Data
Description
Static Friction Coefficient
Static coefficient of friction.
Kinetic Friction Coefficient
Kinetic coefficient of friction.
Exponential Decay Coefficient
Exponential decay coefficient EXP.
Initial Rotation Field (SOL 700 only)
Object
Type
Analysis Type
Init. Rotation Field
Nodal
Explicit Nonlinear
Defines a velocity field of grid points consisting of a rotation and a traslation specification. Creates a TIC3 Bulk Data entry. Input Data
Description
Trans Veloc(v1,v2,v3)
Defines the initial translational velocity values. These are in model length units per unit time.
Rot Veloc (w1,w2,w3)
Defines the initial rotational velocity values. These are in degrees per unit time.
Rotation Center
Defines a point at the center of rotation.
246
Patran Interface to MD Nastran Preference Guide Load Cases
2.10
Load Cases Load cases in Patran are used to group a series of load sets into one load environment for the model. Load cases are selected when defining an analysis job. The usage within MD Nastran is similar. The individual load sets are translated into MD Nastran load sets, and the load cases are used to create the SUBCASE commands in the Case Control Section. For information on how to define multiple static and/or transient load cases, see Load Cases Application (Ch. 5) in the Patran Reference Manual.
Chapter 2: Building A Model 247 Defining Contact Regions
2.11
Defining Contact Regions The MD Nastran preference supports 3D slideline contact functionality introduced in MSC.Nastran Version 68. This capability allows the user to model contact between 2D and 3D structural regions or rigid bodies. This functionality can be accessed by using in the Loads/BCs Application in Patran. After selecting the Contact Object on the main form, the first step is to define the regions that may come into contact. Pushing the Application Region button brings up the following form
248
Patran Interface to MD Nastran Preference Guide Defining Contact Regions
.
Application Region One or more curves, surface edges, or solid edges are defined for the Master and Slave application regions. The application region can only contain geometric entities. To model contact between FEM entities without associated geometry, curves must first be created from the nodes using the tools available in the Geometry application.
Geometry Filter u
Geometry
Master Surface: Slave Surface: Active Region:
Slide Line Slide Line Master
Toggles the select box between Master and Slave regions. The Master and Slave application regions can be defined in either order.
Select Curves Select the curve or edge.
Add
Remove Adds the entities in the Select Curves databox to either the Master Region or Slave Region depending on the setting of the Active Region option menu.
Master Region
Slave Region
OK
Clear
Chapter 2: Building A Model 249 Defining Contact Regions
Contact The second step is to define a set of properties of these contacting surfaces. This is done by pushing the Input Data button on the main Application form to bring up the following subordinate form. If the Penetration Type is One Sided, nodes in the Slave Region are not allowed to penetrate the segments of the Master Region. If Two Sided, in addition, nodes in the Master Region are not allowed to penetrate segments of the Slave Region. This is the PTYPE field on the BCONP entry.
Input Data Penetration Type:
One Sided
Friction Coefficient (MU1)
Stiffness in Stick (FSTIF)
Coefficient of static friction between the two surfaces. This is the MU1 field on the BFRIC entry.
Penalty Stiffness Scaling Factor (SFAC)
FSTIF on the BFRIC entry and SFAC on the BCONP entry are penalty parameters in the contact formulation. The default values are usually adequate.
1.0 Slideline Width (W1)
Slideline Width is constant along the slideline and is used to determine the area for contact stress calculation. This is the Wi field on the BFRIC entry.
A Vector Pointing from Master to Slave Surface
OK
Reset
A vector must be defined which lies in the contact plane and points from the Master region to the Slave region. This vector is used to define the coordinate system on the BCONP entry and the BLSEG entries for each region.
250
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
2.12
Rotor Dynamics The MD Nastran Preference supports steady state and transient rotor dynamics, introduced in MSC.Nastran 2004. This capability allows you to model structures with rotating parts, allowing for gyroscopic effects to be included. Rotor Dynamics are modelled using Rotor and Unbalance entities, created within the Rotor Dynamics... selection under the Tools menu:
Chapter 2: Building A Model 251 Rotor Dynamics
Rotor Dynamics Form The Rotor Dynamics form is accessed from the Rotor Dynamics... selection under the Tools menu. This form is used to create, modify, delete, or show Rotors, which define spin properties, including the axis of rotation, spin direction, damping factor, and speed.
Create Modify Delete Show
Steady State Transient Rotor Unbalance (Transient only)
A set of co-linear nodes that make up the rotor model (spin axis). These are the grids in the MD Nastran ROTORG Bulk Data entry. Two nodes defining the spin direction. These are the GRIDA and GRIDB fields in the MD Nastran RSPINR and RSPINT Bulk Data entries. These nodes must be included in the “Rotor Node List” above. Rotor structural damping factor (default 0.0). This is the GR field of the MD Nastran RSPINR and RSPINT Bulk Data entries.
Spin Profile (Steady State) Spin History (Transient)
252
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Spin Profile Form For Steady State analyses, the Spin Profile form is used to define the relative spin rates.
The unit for the speed entries. RPM for revolutions per minute, or Cycles/Time for frequency. This value defines the SPDUNIT field of the MD Nastran RSPINR Bulk Data entry, and are translated to either ‘RPM’ or ‘FREQ’. List of relative spin rates. Entries must be in ascending or descending order. At least one entry required (no default). These values make up the SPEEDi fields of the MD Nastran RSPINR Bulk Data entry.
Spin History Form For Transient analyses, the Spin History form is used to define the spin rates.
Chapter 2: Building A Model 253 Rotor Dynamics
The unit for the speed entries. RPM for revolutions per minute, or Cycles/Time for frequency. This value defines the SPDUNIT field of the MD Nastran RSPINT Bulk Data entry, and are translated to either ‘RPM’ or ‘FREQ’. A constant multiplier to be applied to the Time Dependent Field.
A time dependent field that defines the spin rate as a function of time. This field, with the Speed Amplitude applied to it, will be translated into an MD Nastran TABLED1 Bulk Data entry that is referenced by the RSPINT entry.
Unbalance Form The Rotor Dynamics Unbalance form is used to create, modify, delete, or show Unbalances, which define unbalance loads for transient analyses in terms of cylindrical system with the rotor axis as the Z axis.
254
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Create Modify Delete Show
The unbalance is applied to a node, which must be included in a transient rotor. When a transient rotor is selected, the “Node” listbox is populated with nodes from that rotor’s axis. The unbalance node may then be selected from that list, assuring that it belongs to an existing transient rotor. This node defines the GRID field of the MD Nastran UNBALNC Bulk Data entry.
Displays the Unbalance Properties form to define the remaining parameters for the MD Nastran UNBALNC Bulk Data entry.
Chapter 2: Building A Model 255 Rotor Dynamics
Unbalance Properties Form The Unbalance Properties Form is used to define the remaining parameters for the Unbalance.
256
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Define the MASS, ROFFSET, and ZOFFSET fields of the MD Nastran UNBALNC Bulk Data entry. For each of these values, either a constant real value may be specified, or a time dependent field my be selected from the list below. Time dependent fields are translated to TABLED1 entries, and referenced by integer ID values in the appropriate UNBALNC fields. Defaults are 1.0 for Radial Offset and 0.0 for Z Offset. There is no default for Mass.
Angular position, in degrees, of the mass in the unbalance coordinate system (default 0.0). This defines the THETA field of the MD Nastran UNBALNC Bulk Data entry. The start and termination times for applying the unbalance load. The default start time is 0.0, while the default termination time is 999999.0. These values define the Ton and Toff fields of the MD Nastran UNBALNC Bulk Data entry. Correction flag to specify whether 1) the mass will be used to modify the total mass in the transient response calculations, 2) the effect of the rotor spin rate change will be included in the transient response calculation, or 3) both. Possible values are None, Mass, Speed, or Both (default None). This value defines the CFLAG field of the MD Nastran UNBALNC Bulk Data entry.
Defines the coordinate system orientation relative to the ACID of the unbalance node (no default). This vector defines the X1, X2, and X3 fields of the MD Nastran UNBALNC Bulk Data entry.
Chapter 2: Building A Model 257 Rotor Dynamics
258
Patran Interface to MD Nastran Preference Guide Rotor Dynamics
Chapter 3: Running an Analysis Patran Interface to MD Nastran Preference Guide
3
Running an Analysis
Review of the Analysis Form
Translation Parameters
Solution Types
Direct Text Input
Solution Parameters
Select Superelements
Subcases
Subcase Parameters
Output Requests
Select Superelements
352
Select Explicit MPCs...
443
Non-Structural Mass Properties
Select NSM Properties...
Subcase Select
Restart Parameters
Optimize
Toptomize
Interactive Analysis
260
265
271 276 277 352
354 357
415
451 454
460 462 470
449
444
260
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
3.1
Review of the Analysis Form The Analysis form appears when the Analysis toggle, located on the Patran mainform, is chosen. To run an analysis, or to create a NASTRAN input file, select Analyze as the Action on the Analysis form. Other forms brought up by the Analysis form are used to define translation parameters, solution type, solution parameters, output requests, and the load cases. These forms are described on the following pages. For further information see The Analysis Form (p. 8) in the MSC.Patran Reference Manual.
Chapter 3: Running an Analysis 261 Review of the Analysis Form
Analysis Form This form appears when the Analysis toggle is chosen on the main menu. When preparing for an analysis run, select Analyze as the Action. Actions can be set to: Analyze or Optimize or Toptomize Access Results Read Input File Delete Monitor (if Patran Analysis Manager is installed). Abort (if Patran Analysis Manager is installed). Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual. List of already existing jobs. If one of these jobs is selected, the name will appear in the Job Name list box and all parameters for this job will be retrieved from the database. An existing job can be submitted again by simply selecting it and pushing Apply. It is often convenient to select an existing job, modify a few parameters and push Apply to submit the new job. Name of job. This name will be used as the base file name for all resulting MD Nastran files and message files. This text is used to generate the TITLE entry in the MD Nastran executive control section. Displays the Translation Parameters form to specify parameters not directly related to the solution. These are primarily used by the Application Preferences during the forward translation. Displays the Solution Types form to select the desired type of analysis to run. Opens the Direct Text Input form which allows you to directly enter data for the BULK DATA, Case Control, Executive Control and File Management sections of the NASTRAN input file. Opens the Select Superelements form which allows you to select the superelements active for the specified job. Displays the Subcases form to select a list of load cases to be included in this analysis run. The list of selected load cases is order dependent. Displays the Subcase Select form to select a sequence of subcases associated with an analysis job.
262
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
The following table outlines the selections for the Analyze action. Object Entire Model
Method Full Run Check Run Analysis Deck Model Only Load SimXpert
Selected Group
Full Run Check Run Analysis Deck Model Only Load SimXpert
Existing Deck
Full Run Load SimXpert
Restart
Full Run Check Run Analysis Deck
Interactive
Full Run
The Object indicates which part of the model is to be analyzed. There are four choices: Entire Model, Current Group, Existing Deck, and Restart. • Entire Model is the selected Object if the whole model is to be analyzed. • Selected Group is for specifying the group that contains the model that is to be analyzed. Select
the button Select Group..., under Existing Groups select the desired group, then select Cancel. The name of the selected group will appear in the Analysis form under Group: . For more information see The Group Menu (p. 262) in the Patran Reference Manual. • Existing Deck is selected if you wish to simply submit an existing input file to MD Nastran.
The jobname appearing in the Job Name listbox is appended with the suffix “.bdf” to form the input filename. This file must reside in the current directory. You may also use Existing Deck to directly edit the MD Nastran Bulk Data file.
Chapter 3: Running an Analysis 263 Review of the Analysis Form
• Restart is selected if you wish to restart an analysis. Currently, restarts are only supported for
the Linear Static (101), Nonlinear Static (106), and Normal Modes (103) solution types. The Restart Parameters, 454 form allows you to specify where to resume the analysis. • Interactive analysis utilizes the Patran Preference for MD Nastran capability for performing
visual interactive modal frequency response analysis. The process begins by creating a modal analysis solution using MD Nastran. The interactive modal frequency response analysis is then performed using Patran Analysis: Analyze / Interactive / Full Run. The chain that is followed is 1) using Select Nastran .MASTER... select a .DBALL file, 2) using Create Loading... specify the loading (for example, Acoustic, Force), 3) using Output Requests... specify the desired output, and 4) using View Results... view the results. The Method indicates how far the translation is to be taken.The methods are listed below: • Full Run is the selected type if an Analysis Deck translation is done, and the resulting input file
is submitted to MD Nastran for complete analysis. • Check Run is the selected type if an Analysis Deck translation is done, and the resulting input
file is submitted to MD Nastran for a check run only. • Analysis Deck is the selected type if the Model Deck translation is done, plus all load case,
analysis type and analysis parameter data are translated. A complete input file, ready for MD Nastran should be generated. • Model Only is the selected type if a Bulk Data file is created that contains only the model data
including node, element, coordinate frame, element property, material property, and loads and boundary condition data. The translation stops at that point. • Load SimXpert will lauch SimXpert and automatically transfer the finite element model. The
environment variable MSC_SX_HOME must be set to a valid local installation directory of SimXpert for this capability to be available.
Overview of Analysis Job Definition and Submittal To submit a single load case, linear static analysis job to MD Nastran it is necessary only to click the Apply button on the main Analysis form. Appropriate defaults and selections will be made automatically. Other solution types or multiple load cases will require access to one or more lower-level forms. Several different analysis examples are considered below. To perform a multiple load case, linear static analysis, it is necessary only to open the Subcase Select form. Subcases with the same names as the user-defined load case names and with appropriate defaults can be selected for inclusion in the job. If a change to one or more parameters for a subcase is desired (e.g., to change an output request), the Subcases... form must be accessed. Then it is simple to select a subcase and bring up the appropriate form (e.g., Output Requests) to make changes. For other analysis types (e.g., Normal Modes), the first step is to bring up the Solution Type form and make the appropriate selection. A lower-level Solution Parameters form can be accessed from the Solution Type form to change parameters that affect the overall analysis. Just as for the linear static case, subcases are automatically created for each defined load case. These can be selected on the Subcase Select form or modified on the Subcases form.
264
Patran Interface to MD Nastran Preference Guide Review of the Analysis Form
In the Patran MD Nastran Interface, a subcase can be thought of as a Patran load case with some additional parameters (e.g., Output Requests) associated with it. This association is further strengthened since the default subcases are created for each load case and have the same name as their associated load case. In the rest of this document, the terms load case and subcase will generally be used interchangeably. When a specific form is referenced, Load case and Subcase will be capitalized.
Chapter 3: Running an Analysis 265 Translation Parameters
3.2
Translation Parameters Translation parameters define output file formats, numerical tolerances, processing options, numbering offsets, and external include files.
266
Patran Interface to MD Nastran Preference Guide Translation Parameters
Tolerances
• Division - prevents divide by zero errors. • Numerical - determines if two real values are equal. • Writing determines if a value is approximately zero when generating a
Bulk Data entry field. Bulk Data Format
• Sorted Bulk Data - Sorts Bulk Data entries alphabetically. • Card Format - Determines whether the real number can be written to a
standard (8 character) NASTRAN field or to a double (16 character) NASTRAN field. • Write Stored Precision - When ON it writes all data as double precision if
the data double precision information. • Precision Control Options - Specifies where to round off a grid point
coordinate, material, property, or other entity value before its written out to the bdf file. For example if this value is specified as 2 the number 1.3398 will be written out as 1.34. Node Coordinates
Defines which coordinate frame is used when generating the grid coordinates.
Coordinate Frame Coordinates
Defines which coordinate frame is used when generating the grid coordinates. This can be set to reference frame, analysis frame, or global. This should not affect the analysis. It only changes the method used in the grid creation. This determines which coordinate frame is referenced in the CP field of the GRID entry.
MD Nastran Version
Specifies the version of MD Nastran. The version specified here is used for two purposes: to create the full name of the ALTER file to be used, and to determine which Solution Sequence to use. Use only whole numbers and letters; for example, 66a, 67 and 68; 67.5 is the same as 67. This version number can be overridden by setting the environment variable “NASTRAN_VERSION”.
Number of Tasks
Represents the number of processors to be used to run an analysis. It is assumed that the environment is configured for distributed parallel processing.
Write Properties on Element Entries
Specifies that properties will be written to the element entries for all elements where it is allowed in MD Nastran.
Write Continuation Markers
This option is OFF by default. This option can be turned ON to write continuation markers for Bulk Data entries.
Write Global Ply IDs Convert CBARs to CBEAMs
When ON, attempts to keep the Global Ply IDs consistent between MD Nastran and Patran. Converts all CBARs to CBEAMS
Chapter 3: Running an Analysis 267 Translation Parameters
Write PARTSuperelement
This is ON by default and if ON and superelements are selected (see Select Superelements, 352 then BEGIN BULK SUPER = id sections are written in to the input file for each selected superelement. If OFF and superelements are selected, then SESET entries are written instead to define the superelements.
Geometry Check
Use Iterative Solver Ext. Superelement Spec... Numbering Options... Bulk Data Include File...
Checks the element shapes to make sure they are valid. You can set different warning levels from None to Fatal depending on how crucial the element shapes are to your model. Activates the iterative solver for analysis. The analysis manger does not support this option and must be disabled when using this option. Subform used for defining superelement specifications. Subform used to indicate offsets for all IDS to be automatically assigned during translation. Prompts you for the filename of the include file.
268
Patran Interface to MD Nastran Preference Guide Translation Parameters
External Superelement Specifications With this form you can define the options for the External Superelements Bulk Data entry. Please see the MD Nastran Quick Reference Guide for more information about External Superelements.
The available methods are: NONE – No EXTSEOUT entry created. DMIGPCH – Requires an EXTID MATRIXDB DMIGDB DMIGOP2
ASM BULK and EXT BULK require the EXTID method.
Numbering Options This form is activated by the Numbering Options button on the Translation Parameters form. It allows the user to indicate offsets for all IDS to be automatically assigned during translation. For example, if the
Chapter 3: Running an Analysis 269 Translation Parameters
user types 100 into the Element Properties Offset box, the numbering of element properties in the resulting NASTRAN input file will begin at 101.
The Begin. Contin. Marker box allows the user to specify the continuation of the mnemonic format used on multiple line, Bulk Data entries.
IDs Encoded in Names allows the user to activate recognition of IDs encoded into the name of any named entity, such as a material.
Number Only will recognize and use an ID if, and only if, the name of the entity is an actual number like “105.” This option is ON by default. Beginning Number will recognize an ID if the number begins the name, such as “52_shell_property.” This option is OFF by default. Trailing Number will recognize an ID if it trails the name, such as “shell_property_52.” This option is OFF by default. Encoded Syntax will recognize an ID if it directly follows the first occurrence of the specified syntax. For example, with this option activated and the specified syntax set to “.”, the ID assigned to a material given the name “Steel_1027.32” would be 32.
Note that both the Patran Neutral file reader and the Patran MD Nastran input file reader preserve the IDs of named entities with a “.” syntax, so that a NASTRAN PSHELL record of ID 12 will be assigned the name “PSHELL.12.” This last option allows great continuity between input model data and output model data. This option is ON by default and the default Syntax Marker is “.”.
270
Patran Interface to MD Nastran Preference Guide Translation Parameters
Select File
Chapter 3: Running an Analysis 271 Solution Types
3.3
Solution Types The Solution Type form defines the type of analysis and Solution Parameters. Your choice for the Solution Type will in turn affect additional forms you complete for Solution Parameters, 277, Subcase Parameters, 357, and Output Requests, 415. See Table 3-1. To set the Solution Type: Click on the Analysis Application button.
272
Patran Interface to MD Nastran Preference Guide Solution Types
On the Analysis Application form, click Solution Type... and select the Solution Type from the list of available Solution Types. For Analysis Type Explicit Nonlinear:
Solution Type
Defines the solution type.
• Linear Static
Selects Solution Sequence (SOL) 101, 114, 1, or 47 depending on the selected Solution Parameters. You may select one or more subcases in SOLs 1 and 101.
Chapter 3: Running an Analysis 273 Solution Types
• Nonlinear Static
Selects Solution Sequence 66 or 106, depending on the version of MD Nastran. Version 66 and below yields SOL 66, and Version 67 and above yields SOL 106. You may select one or more subcases.
• Normal Modes
Selects Solution Sequence 103, 115, 3, or 48 depending on the Solution Parameters. You may select only one subcase.
• Buckling
Selects Solution Sequence 105, 77, or 5 depending on the selected Solution Parameters. Only one subcase may be selected that defines the static preload. The buckling subcase is automatically generated. The output requests for this Solution Type are applied to the static preload subcase. The default output requests for the buckling subcase are displacements and constraint forces.
• Complex Eigenvalue
Selects Solution Sequence 107, 110, 28, or 29 depending on the selected Solution Parameters. You may select only one subcase.
• Frequency Response
Selects Solution Sequence 108, 111, 118, 26, or 30 depending on the selected Solution Parameters. You may specify only one subcase for Solution Sequences 118, 26, or 30. For Solution Sequences 108 or 111, multiple subcases may be selected.
• Transient Response
Selects Solution Sequence 109, 112, 27, or 31 depending on the selected Solution Parameters. You may specify only one subcase for Solution Sequences 27 or 31. For Solutions Sequences 109 or 112, multiple subcases may be selected.
• Nonlinear Transient
Selects Solution Sequence 99 or 129, depending on the MD Nastran Version. Version 66 and below yields SOL 99; Version 67 and above yields SOL 129. You may select only one subcase.
• Implicit Nonlinear • DDAM Solution • Explicit Nonlinear
Selects Solution Sequence 400 or 600 (depending on “SOL400RUN* toggle). Selects Solution Sequence 187, Dynamic Design Analysis Method (DDAM). Selects Solution Sequence 700.
274
Patran Interface to MD Nastran Preference Guide Solution Types
Select ASET/QSET...
• Select existing Degree of Freedom Lists for use in making an ASET or
a QSET in the input file. • The ASET toggle creates a user selected unreferenced SPOINTS in the
ASET of input file. • The QSET toggle creates a user selected number of unreferenced
SPOINTS in the QSET of the input file. Solution Parameters...
Solution Type Linear Static
Brings up a solution-type-dependent subordinate form that allows you to specify parameters which apply to the complete solution.
Database Run
Cyclic Symmetry
Formulation
MD Nastran Version
Solution Parameter Settings
Off
Off
--
--
1
Off
On
--
--
47
On
Off
--
--
101
On
On
--
--
114
Chapter 3: Running an Analysis 275 Solution Types
Solution Type
Database Run
Cyclic Symmetry
Formulation
MD Nastran Version
Solution Parameter Settings
Nonlinear Static
--
--
--
66 or Below
66
--
--
--
67 or Above
106
Off
Off
--
--
3
Off
On
--
--
48
On
Off
--
--
103
On
On
--
--
115
Off
Off
--
--
5
On
On
--
--
77
On
Off
--
--
105
Off
--
Direct
--
28
Off
--
Modal
--
29
On
--
Direct
--
107
On
--
Modal
--
110
Off
--
Direct
--
26
Off
--
Modal
--
30
On
Off
Direct
--
108
On
--
Modal
--
111
On
On
Direct
--
118
Off
--
Direct
--
27
Off
--
Modal
--
31
On
--
Direct
--
109
On
--
Modal
--
112
--
--
--
66 or Below
99
--
--
--
67 or Above
129
Normal Modes
Buckling
Complex Eigenvalue
Frequency Response
Transient Response
Nonlinear Transient Implicit Nonlinear
400 600
DDAM Solution
2004
187
Explicit Nonlinear
2005
700
276
Patran Interface to MD Nastran Preference Guide Direct Text Input
3.4
Direct Text Input This form is used to directly enter entries in the File Management, Executive Control, Case Control, and BULK DATA sections of the NASTRAN input file. The input file reader also creates these entries for any unsupported entries in the input file. If the data is entered by the user the Write to Input Deck toggle default is ON. If the data comes from the input file reader the default for the Input Deck toggle is OFF. These entries may be reviewed and edited by the user. If they should be written to any input files subsequently created by the interface, the appropriate Write to Input Deck toggle should be set to ON. Text entered into the Case Control section is written to the input file before the first subcase. The Direct Text Input option on the Subcases form should be used to directly enter text within a subcase definition.
Switches to determine which data section the MD Nastran input would be sent.
Saves the current setting and data for the four sections and closes the form.
Clears the current form.
Resets the form back to the data values it had at the last OK.
Resets all four forms back to its previous value and closes the form.
Chapter 3: Running an Analysis 277 Solution Parameters
3.5
Solution Parameters Linear Static This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Linear Static is selected. Depending on the setting of the Database Run and Cyclic Symmetry parameters, this Solution Type will generate a SOL 101, 114, 1, or 47 input file.
278
Patran Interface to MD Nastran Preference Guide Solution Parameters
Database Run
Indicates whether a Structured Solution Sequence (SOL 101 or 114) is to be used or a Rigid Format (SOL 1 or 47). If selected, a Structured Solution Sequence is selected.
Cyclic Symmetry
Indicates that this model is a sector of a cyclically repeating part (SOL 114 or 47).
Automatic Constraints
Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Inertia Relief
Indicates that the inertia relief flags are to be set by including the PARAM, INREL,1 command. This flag can only be chosen if Database Run is selected and Cyclic Symmetry is disabled. If inertia relief is selected, a node-ID for weight generation must be selected. A PARAM, GRDPNT and a SUPORT command will be written to the input file using the same node-ID selected for weight generation. The SUPORT entry will specify all 6 degrees of freedom.
Alternate Reduction
Indicates that an alternate method of performing the static condensation is desired. The PARAM, ALTRED,YES command is included if selected and if Database Run is also selected
SOL 600 Run Contact Parameters Shell Normal Tolerance Angle
Indicates a SOL 600 run. Same as the contact parameters available for the Implicit Nonlinear solution type. Only used with linear contact capability. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Chapter 3: Running an Analysis 279 Solution Parameters
Default Initial Temperature
Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry. Rigid Element Type:
The Rigid element type optionmenu presents three different types of rigid elements, corresponding to the three possible values for the Nastran RIGID= case control. They are:
• LINEAR: Selects linear rigid elements, which are the rigid elements that
have been available in MD Nastran since its inception. • LAGR: Selects the new Lagrange rigid elements with the Lagrange multplier
method. • LGELIM: Selects the new Lagrange rigid elements with the Lagrange
elimination method. See the Nastran quick reference quide for more details. Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
The table outlines the Database Run and Cyclic Symmetry selections, and the SOL types that will be used. Database Run
Cyclic Symmetry
SOL
On
Off
101
On
On
114
Off
Off
1
Off
On
47
Nonlinear Static This subordinate form appears when the Solution Parameters button is selected on the Solution Type form, when Nonlinear Static is selected. If the MD Nastran version specified is Version 66 or lower, then Solution Sequence (SOL) 66 will be employed. However, if the MD Nastran version specified is version 67 or higher, then Solution Sequence 106 will be employed except as described below. For more
280
Patran Interface to MD Nastran Preference Guide Solution Parameters
information about specification of the MD Nastran version number, see the Translation Parameters, 265 form. Indicates that an AUTOSPC entry is requested. MD Nastran will automatically constrain model singularities. Indicates that displacements, which can cause a difference in the formulation of the stiffness matrix, may be encountered. Therefore, the stiffness matrix may need to be periodically recomputed based on the displaced shape. Indicates, as the part deflects, that the applied forces will remain aligned with the deformed part rather than maintaining their global orientation. This can only be selected if Large Displacements is also selected.
The default solution sequence for Nonlinear Static is 106, but can be changed to any one of the following if desired: 400, 600, 700. Only features of 106 are used in any case. For specific features particular to 600 or 700, please use the Implicit Nonlinear type or set the Analysis Type to Explicit Nonlinear, respectively.
Chapter 3: Running an Analysis 281 Solution Parameters
The following table outlines the selections for Large Displacements and Follower Forces, and the altered LGDISP parameter setting for each. Large Displacements
Follower Forces
LGDISP
Off
On
-1
On
On
1
On
Off
2
This is a list of the data input, available for defining the Nonlinear Static Solution Parameters, that were not shown on the previous page. Parameter Name
Description
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
282
Patran Interface to MD Nastran Preference Guide Solution Parameters
Normal Modes This subordinate form appears when Solution Parameters is selected on the Solution Type form when Normal Modes is selected. Use this form to generate a SOL 103, 115, 3, or 48 input file, depending on the Database Run and Cyclic Symmetry parameters below.
See Real Eigenvalue Extraction, 284. Not shown unless Cyclic Symmetry is on. If the version is Version Š 68 and the solution sequence is SOL 103, then these controls are selectable on the Normal Modes Subcase Parameters, 364 form.
The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each. Indicates whether a Structured Solution Sequence (SOLs 103 or 115) is to be used, or a Rigid Format (SOL 3 or 48). If Database Run is selected, a Structured Solution Sequence will be selected. Database Run
Cyclic Symmetry
SOL
On
Off
103
On
On
115
Off
Off
3
Off
On
48
Chapter 3: Running an Analysis 283 Solution Parameters
This is a list of data input, available for defining the Normal Modes Solution Parameters, that were not shown on the previous page. Parameter Name
Description
Cyclic Symmetry
Indicates that this model is a sector of a cyclically repeating part (SOL 115 or 48).
Automatic Constraints
Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
SOL 600 Run Residual Vector Computation Shell Normal Tolerance Angle
Select this to perform a SOL 600 analysis. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run (used to prevent runaway jobs). This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature Rigid Element Type Max p-Adaptive Cycles
Specify the initial temperature. There are three ways to define a rigid element. They are 1) Linear, 2) Lagrangian, or 3) Lgelim. Specify the maximum number of p-Adaptive cycles.
284
Patran Interface to MD Nastran Preference Guide Solution Parameters
Parameter Name
Description
• Dynamic Reduction
Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Real Eigenvalue Extraction
This subordinate form appears when the Eigenvalue Extraction button is selected on the Normal Modes, Frequency Response, or Transient Response Solution Parameters forms. It also appears when the Real Eigenvalue Extraction button is selected on the Complex Eigenvalue Solution Parameter form. Use this form to create either EIGR or EIGRL Bulk Data entries. Defines the method to use to extract the real eigenvalues. This parameter can be set to any one of the following: Lanczos, Automatic Givens, Automatic Householder, Modified Givens, Modified Householder, Givens, Householder, Enhanced Inverse Power, or Inverse Power. If this selection is set to Lanczos, an EIGRL Bulk Data entry should be created. Otherwise, this defines the setting of the METHOD field on the EIGR Bulk Data entry.
Defines the lower and upper limits to the range of frequencies to be examined. These are the F1 and F2 fields on the EIGR Bulk Data entry or the V1 and V2 fields on the EIGRL Bulk Data entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Enhanced Inverse Power or Inverse Power. This is the NE field on the EIGR Bulk Data entry.
Chapter 3: Running an Analysis 285 Solution Parameters
This is a list of data input available for defining the Real Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed. This is the ND field on the EIGR or EIGRL Bulk Data entries.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value between 0 and 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of three settings: Mass, Maximum, or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. Defines the setting of the NORM field on the EIGR Bulk Data entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGR Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGR Bulk Data entry.
286
Patran Interface to MD Nastran Preference Guide Solution Parameters
Dynamic Reduction Parameters
This subordinate form appears when the Dynamic Reduction button is selected on the Normal Modes, Complex Eigenvalue, Frequency Response, or Transient Response Solution Parameters forms. Use this form to create the DYNRED Bulk Data entry. A flag that indicates whether or not any dynamic reduction is desired.
Indicates the maximum frequency to be considered when performing dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON. This is the FMAX field.
Indicates which method is to be used in selecting coordinates. This parameter can be set to either Automatic or Manual. This parameter can only be selected if Perform Dynamic Reduction is set to ON. This determines if the program will automatically select the number of generalized coordinates.
Indicates the number of scalar points that must be retained in this dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON and Method of Coordinate Selection is set to Manual. The Application Preference will automatically create this many SPOINTs, and place them in the a-set and the q-set. Defines the number of generalized coordinates to be included in the dynamic reduction. This parameter can only be selected if Perform Dynamic Reduction is set to ON, and Method of Coordinate Selection is set to Manual. This is the NQDES field.
Chapter 3: Running an Analysis 287 Solution Parameters
Buckling This subordinate form appears when Solution Parameters is selected on the Solution Type form when Buckling is selected. Use this form to generate a SOL 105, 77, or 5 input file, depending on the setting of the Database Run and Cyclic Symmetry parameters. Indicates that an AUTOSPC entry is requested, so that MD Nastran will automatically constrain model singularities.
Indicates whether a Structured Solution Sequence (SOL 105) is to be used or a Rigid Format or unstructured Solution Sequence (SOL 5 or 77). If Database Run is selected, a Structured Solution Sequence will be selected.
Indicates that this model is a sector of a cyclically repeating part.
See Real Eigenvalue Extraction, 284.
288
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Cyclic Symmetry, and the altered SOL type for each. Database Run
Cyclic Symmetry
SOL
On
Off
105
On
On
77
Off
Off
5
This is a list of data input available for defining the Buckling Solution Parameters that were not shown on the previous page. Parameter Name
Description
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
• Eigenvalue Extraction
Results Output Format
Brings up the Buckling Eigenvalue Extraction form for defining the eigenvalue extraction controls. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Chapter 3: Running an Analysis 289 Solution Parameters
Buckling Eigenvalue Extraction
This subordinate form appears when the Eigenvalue Extraction button is selected on the Buckling Solution Parameters form. Use this form to create either EIGB or EIGRL Bulk Data entries, depending on the selected extraction method. Defines the method to use to extract the buckling eigenvalues. This parameter can be set to any one of the following: Lanczos, Enhanced Inverse Power, or Inverse Power. If Lanczos is selected, an EIGRL entry will be created. If Inverse Power or Enhanced Inverse Power are selected, and EIGB entry will be created with the METHOD field set to either INV or SINV specified, respectively.
Defines the lower and upper limits to the range of eigenvalues to be examined. These are the L1 and L2 fields on the EIGB entry or the V1 and V2 fields on the EIGRL entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Inverse Power. This is the NEP field on the EIGB entry.
Indicates the limit to how many eigenvalues to be computed. This value can only be selected if Extraction Methods set to Lanczos. This is the NP field on the EIGRL entry.
290
Patran Interface to MD Nastran Preference Guide Solution Parameters
This is a list of data input, available for defining the Buckling Eigenvalue Extraction, that was not shown on the previous page. Parameter Name
Description
Number of Desired Positive Roots
Indicates the limit to how many positive eigenvalues to be computed. This value can only be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDP field on the EIGB entry.
Number of Desired Negative Roots
Indicates the limit to how many negative eigenvalues to be computed. This value cannot be selected if Extraction Method is set to Inverse Power or Enhanced Inverse Power. This is the NDN field on the EIGB entry.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value in the range of 0 through 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the NORM field on the EIGB entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGB entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This, too, can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGB entry.
Chapter 3: Running an Analysis 291 Solution Parameters
Complex Eigenvalue This subordinate form appears when Solution Parameters is selected on the Solution Type form when Complex Eigenvalue is selected. When you specify the Database Run and Formulation parameters (from the Solution Type form), Patran generates a SOL 107, 110, 28, or 29 input file.
See Complex Eigenvalue Extraction, 294.
See Real Eigenvalue Extraction, 284.
See Dynamic Reduction Parameters, 286.
292
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If you select Database Run, a Structured Solution Sequence (SOLs 107 or 110) will be selected. If you deselect Database Run a Rigid Format Solution Sequence (SOLs 28 or 29) will be selected. Database Run
Formulation
SOL
On
Direct
107
On
Modal
110
Off
Direct
28
Off
Modal
29
This is a list of data input available for defining the Complex Eigenvalue Solution Parameters that was not shown on the previous page. Parameter Name Automatic Constraints Residual Vector Computation Shell Normal Tolerance Angle
Description Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Chapter 3: Running an Analysis 293 Solution Parameters
Parameter Name
Description
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type Struct. Damping Coeff. • Complex Eigenvalue • Real Eigenvalue • Dynamic Reduction
Results Output Format
There is one rigid element type, Linear. Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value). Brings up the Complex Eigenvalue Extraction form for defining the complex eigenvalue extraction controls. Brings up the Real Eigenvalue Extraction form for defining the real eigenvalue extraction controls. Brings up the Dynamic Reduction Parameters form for defining the dynamic reduction controls. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
294
Patran Interface to MD Nastran Preference Guide Solution Parameters
Complex Eigenvalue Extraction
This subordinate form appears when the Complex Eigenvalue button is selected on the Complex Eigenvalue Solution Parameters form. Use this form to create an EIGC Bulk Data entry. Defines the method to use to extract the complex eigenvalues. This parameter can be set to any one of the following: Complex Lanczos, Upper Hessenberg, Inverse Power, or Determinate. This defines the setting of the METHOD field.
Defines the real component of the beginning of lines in the complex plane. These values cannot be selected if Extraction Method is set to Upper Hessenberg. This is a list of real values. They are the ALPHAAJ fields.
Defines the real component of the end of lines in the complex plane. These values cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the ALPHABJ fields.
Defines the imaginary component of the beginning of lines in the complex plane. These values cannot be selected if Extraction Method is set to Upper Hessenberg. This is a list of real values. They are the OMEGAAJ fields.
Chapter 3: Running an Analysis 295 Solution Parameters
This is a list of data input available for defining the Complex Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Omega of B Points
Defines the imaginary component of the end of lines in the complex plane. These values cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the OMEGABJ fields.
Width of Regions
Defines the width of the region in the complex plane. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of real values. They are the LJ fields.
Estimated Number of Roots
Indicates an estimate of the number of eigenvalues to be located within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NEJ fields.
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed within the specified region. This value cannot be selected if Extraction Method is set to Complex Lanczos or Upper Hessenberg. This is a list of integer values. They are the NDJ fields.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of two settings: Maximum or Point. This is the NORM field on the EIGC entry.
Normalization Point
Defines the point to be used in the normalization. This is the G field on the EIGC Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Extraction Method is set to Inverse Power or Determinate. This is the C field on the EIGC Bulk Data entry.
296
Patran Interface to MD Nastran Preference Guide Solution Parameters
Frequency Response This subordinate form appears when Solution Parameters is selected on the Solution Type form when Frequency Response is selected. Patran generates a SOL 108, 111, 118, 26, or 30 input file when you specify the Database Run, Cyclic Symmetry, and Formulation parameters (from the Solution Type form).
See Real Eigenvalue Extraction, 284.
See Dynamic Reduction Parameters, 286.
The following table outlines the selections for Database Run, Formulation, and Cyclic Symmetry parameters, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 108, 111, 118) will be selected. If Database Run is deselected, a Rigid Format (SOLs 26 or 30) will be selected.
Chapter 3: Running an Analysis 297 Solution Parameters
Database Run
Formulation
Cyclic Symmetry
SOL
On
Direct
Off
108
On
Direct
On
118
On
Modal
--
111
Off
Direct
--
26
Off
Modal
--
30
This is a list of data input, available for defining the Frequency Response Solution Parameters that were not shown on the previous page. Parameter Name Cyclic Symmetry
Automatic Constraints Residual Vector Computation Shell Normal Tolerance Angle
Description Indicates that this model is a sector of a cyclically repeating part, and the appropriate flags will be set. This can only be set if Database Run is selected and Formulation is set to Direct (SOL 118). Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors. Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
298
Patran Interface to MD Nastran Preference Guide Solution Parameters
Parameter Name Node ID for Wt. Gener.
Description Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type Struct. Damping Coeff.
There is one rigid element type, Linear. Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value).
• Eigenvalue Extraction
Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal.
• Dynamic Reduction
Calls up another form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
Chapter 3: Running an Analysis 299 Solution Parameters
Transient Response This subordinate form appears when Solution Parameters is selected on the Solution Type form when Transient Response is selected. Patran generates a SOL 109, 112, 27, or 31 input file, when you specify Database Run and Formulation parameters (from the Solution Type form).
These options are only available for a "Modal" solution.
300
Patran Interface to MD Nastran Preference Guide Solution Parameters
The following table outlines the selections for Database Run and Formulation, and the altered SOL type for each. If Database Run is selected, a Structured Solution Sequence (SOLs 109, 112) will be selected. If Database Run is deselected, a Rigid Format (SOLs 27 or 31) will be selected. Database Run
Formulation
SOL
On
Direct
109
On
Modal
112
Off
Direct
27
Off
Modal
31
This is a list of data input available for defining the Transient Solution Parameters that was not shown on the previous page. Parameter Name Automatic Constraints Residual Vector
Description Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities.
Computation
The Residual Vector Computation toggle writes RESVEC=YES or RESVEC=NO to the Case Control. This calculates residual vectors due to applied loads. The default is to calculate residual vectors.
SOL 600 Run
Select this to perform a SOL 600 analysis.
SOL 700 Run
Select this to perform a SOL 700 analysis. To do this is necessary to use the Direct method.
Shell Normal
Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Tolerance Angle Mass Calculation
Defines how the mass matrix will be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Chapter 3: Running an Analysis 301 Solution Parameters
Parameter Name
Description
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Inital Temperature
Specify the initial temperature.
Default Load Temperature
Specify load temperature.
Rigid Element Type
There is one rigid element type, Linear.
Struct. Damping Coeff.
Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor
Defines W3 and W4 parameters. These parameters alter the damping characteristics of the model.
W4, Damping Factor1 • Eigenvalue
Extraction • Dynamic Reduction
Results Output Format
Calls up the Real Eigenvalue Extraction form that is used to define the eigenvalue extraction controls. These parameters can only be specified if Formulation is set to Modal. Calls up the Dynamic Reduction Parameters form that is used to define the dynamic reduction controls. These parameters can only be specified if Formulation is set to Modal. On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
302
Patran Interface to MD Nastran Preference Guide Solution Parameters
Nonlinear Transient This subordinate form appears when Solution Parameters is selected on the Solution Type form when Nonlinear Transient is selected. Use this form to generate either a SOL 99 or a SOL 129 input file, depending on the version of MD Nastran indicated on the translation parameter form except as indicated below. Version 66 and below yields SOL 99 and Version 67 and above yields SOL 129. Indicates that an AUTOSPC entry is requested, so that MD Nastran will constrain model singularities. The default solution sequence for Nonlinear Transient is 129, but can be changed to any one of the following if desired: 400, 600, 700. Only features of 129 are used in any case. For specific features particular to 600 or 700, please use the Implicit Nonlinear type or set the Analysis Type to Explicit Nonlinear, respectively.
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Indicates how the data file entry images are to be printed in theMD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Chapter 3: Running an Analysis 303 Solution Parameters
This is a list of data input available for defining the Nonlinear Transient Solution Parameters that was not shown on the previous page. Parameter Name
Description
Plate Rz Stiffness Factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Struct. Damping Coeff.
Defines a global damping coefficient to applied. This defines the G parameter (e.g., PARAM, G, value.)
W3, Damping Factor
Define W3 and W4 parameters. These parameters alter the damping characteristics of the model.
W4, Damping Factor Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
304
Patran Interface to MD Nastran Preference Guide Solution Parameters
Implicit Nonlinear This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Implicit Nonlinear is selected. Use this form to generate a SOL 400 or 600 input file.
The default solution sequence for Implicit Nonlinear is 600. By toggling the “SOL 400 Run” ON, Patran will write a SOL 400 input file. Not all features of SOL 600 are accessible using SOL 400, so use with caution and check your input file and results carefully.
Solver / Options...
See Solver Options Subform (SOL 600), 306.
Contact Parameters...
See Contact Parameters Subform, 307.
Direct Text Input...
This subform is used to directly enter entries in the File Management, Executive Control, Case Control, and Bulk Data sections of the MD Nastran input file. See Direct Text Input, 276.
Restart Parameters...
See Restart Parameters Subform, 315.
Advanced Job Control...
See Advanced Job Control Subform (SOL 600), 317.
Chapter 3: Running an Analysis 305 Solution Parameters
Domain Decomposition...
See Domain Decomposition, 318.
Assumed Strain
For SOL 600, if ON, (default is ON), places the MARCASUM parameter into the input file. This forces all elements that can deal with assumed strain to use this formulation. This improves the bending behavior of Marc elements 3, 7, and 11. For SOL 400, the NLMOPTS entry is written with the ASSUM option. Again, this is a global setting and forces all elements that can use this formulation to adopt it.
Constant Dilatation
If ON, (default is OFF), places the MARCDILT parameter into the input file. This will force all elements that can deal with constant dilatation (for nearly incompressible analysis) to use this formulation. This affects Marc element types 7, 10, 11, 19, and 20 only and recommended for elastic-plastic and creep analysis. (SOL 600 only)
Plane Stress
Replaces plane strain elements with plane stress elements. (SOL 600 only)
Reduced Integration
Specifies that a lower number of element integration points be used to integrate exactly. (SOL 600 only)
Creep
For SOL 400, writes the NLMOPTS entry with the CREEP option defaults for creep analysis.
Shell Shear Correction
For SOL 400 (only), forces all shell elements using nonlinear formulations to use the shear correction. This writes the NLMOPTS entry with the TSHEAR option.
SOL 400 Run
Use this to select a SOL 400 simulation, instead of a SOL 600 simulation.
Default Initial or Load Temperature
For SOL 400 allows for specification of a general initial temperature and a general loading temperature. TEMPD entries are written for both with Case Control TEMPERATURE(INITIAL) and TEMPERATURE(LOAD) entries calling out the corresponding TEMPD entries in the bulk data.
Results Output Format...
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
306
Patran Interface to MD Nastran Preference Guide Solution Parameters
Solver Options Subform (SOL 600) Specifies the solver to be used in numerically inverting the system matrix of linear equilibrium equations.
Inconsistent MPCs
There are three choices for dealing with problem MPCs, 1) Reorder (reorder the DOFs that are used to define the problem MPCs), 2) Continue (continue the analysis with no changes to the MPCs DOFs), or 3) Stop (stop the analysis).
Solver Type
Chooses Direct Profile, Iterative Sparse, Direct Sparse , Hardware Sparse, Multifrontal Sparse (default), or External Sparse as the solver.
Non-Symmetric
Specifies non-symmetric for Solver Type of Direct Profile or Multifrontal Sparse.
Non-Positive Definite
Specifies non-positive definite option valid for all solver types, use ON. On by default in SOL 600, use Nastran Default. Can un select this option by using OFF.
Memory
Defines the amount of work space in words. This can be left blank and the translator will automatically determine this based on model size.
Multifrontal Sparse Parameters
Chapter 3: Running an Analysis 307 Solution Parameters
• Out-of-Core Threshold
For Hardware and Multifrontal Sparse solvers only. Default is 100. Represents the number of real*4 words in millions of words. Only for SGI computers running the IRIX operating system.
Bandwidth Optimization
Turns on the optimize option for the Direct Profile or Multifrontal Sparse solvers and uses the Sloan algorithm. Other solvers have their own optimizer and use it by default.
Contact Parameters Subform Defines options for detecting and handling contact.
308
Patran Interface to MD Nastran Preference Guide Solution Parameters
Deformable-Deformable Method
In Double-Sided method, for each contact body pair, nodes of both bodies will be checked for contact. In Single-Sided method, for each contact body pair, only nodes of the lower-numbered body will be checked for contact. Results are dependent upon the order in which contact bodies are defined.
Optimize Constraint Equations
Use this to decrease the bandwidth of the model.
Contact Detection...
See Contact Detection Subform, 309.
Separation...
See Separation Subform, 311.
Friction Parameters...
See Friction Parameters Subform, 312.
Enable Initial Contact
Click on checkbox to activate the capability for control of initial contact. The initial contact is for creating an MD Nastran entry BCTABLE with ID = 0 to be used for increment 0. For SOL 600, this causes rigid contact bodies to be moved so they just touch adjacent flexible contact bodies. For SOL 101 and 400, a BCTABLE is used with ID = 0, which causes rigid contact bodies to be moved, as for SOL 600, and/or adjusting the coordinates of all active nodes on the surface of all deformable BCBODYs to remove any prestressed condition.
Initial Contact...
See Initial Contact Subform, 314.
Penetration Check
This controls contact penetration checking, sometimes referred to as the increment splitting option. Available options are: At End of Increment, Per Iteration (default), Suppressed (Fixed), Suppressed (Adaptive). At End of Increment means penetration is checked at the end of a load increment. Per Iteration means that penetration is checked at the end of every iteration within an increment. If penetration is detected, increments are split. Suppress is to suppress this feature for Fixed and Adaptive load stepping types.
Reduce Printout of Surface Definition
This controls reduction of printout of surface definition.
Chapter 3: Running an Analysis 309 Solution Parameters
Contact Detection Subform
On the Contact Control Parameters subform, select Contact Detection... This form controls general contact parameters for contact detection.
310
Patran Interface to MD Nastran Preference Guide Solution Parameters
Distance Tolerance
Distance below which a node is considered touching a body (error). Leave the box blank to have MSC.Marc calculate the tolerance as the smaller of 1/20 element edge length or 1/4 shell thickness.
Bias on Distance Tolerance
Contact tolerance BIAS factor. The value should be within the range of zero to one. Models with shell elements seem to be sensitive to this parameter. You may need to experiment with this value if you have shell element models that will not converge. The SOL 600 default is 0.9.
Suppress Bounding Box Check
Turn ON this button if you want to suppress bounding box checking. This might eliminate penetration, but slows down the solution.
Include Outside (Solid Element) When detecting contact of elements (beam/bar, shell, solid elements) use this to include contact of the outside of the elements. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid). Include Outside (Rigid Surface) When detecting contact of rigid surfaces use this to include contact of the edges of the surfaces. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid). Check Layers
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges
Use this to detect contact of edges. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCPARA entry (contact parameters) of the MD Nastran QRG. The entries that are used for the BCPARA entry are ITOPBM (beam/bar), ITOPSH (plate/shell), and ITOPSD (solid).
Activate Quadratic Contact
Use this to detect the contact of the edges of quadratic elements (midside nodes).
Activate 3D Beam-Beam Contact
Turn this button ON to activate 3D beam-beam contact. Activate 3D BeamBeam Contact enters a one(1) in the 13th field of the 2nd data block. This creates the MD Nastran Bulk Data entry BCPARA, and uses the entry BEAMP.
Chapter 3: Running an Analysis 311 Solution Parameters
Separation Subform
On the Contact Control Parameters subform, select Separation... This form controls general contact parameters for contact separation.
Maximum Separations
Maximum number of separations allowed in each increment. Maximum Separations is entered in the 6th field of the 2nd data block. Default is 9999.
Retain Value on NCYCLE
Turn ON this button if you do not want to reset NCYCLE to zero when separation occurs. This speeds up the solution, but might result in instabilities. You can not set this and Suppress Bounding Box simultaneously. Retain Value of NCYCLE enters a three(3) in field 8 of the 2nd data block.
Increment
Specifies whether chattering is allowed or not. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
Chattering
Specifies the separation criterion (forces or stresses) and the critical value at which the separation will take place. Increment and Chattering enters the appropriate flag in the 9th field of the 2nd data block.
312
Patran Interface to MD Nastran Preference Guide Solution Parameters
Separation Criterion
Specifies in which increment (current or next) the separation is allowed to occur. Separation Criterion enters a one(1) in the 12th field of the 2nd data block if separation is based on stresses.
Force Value Stress Value
Force/Stress Value is placed in the 5th field of the 3rd data block.
Friction Parameters Subform
On the Contact Control Parameters subform, select Friction Parameters...
Chapter 3: Running an Analysis 313 Solution Parameters
Friction Type
Available options for friction Type are: None (default), Shear (for metal forming), Coulomb (for normal contact), Shear for Rolling, Coulomb for Rolling, StickSlip, Bilinear Shear, and Bilinear Coulomb. The MD Nastran entry BCPARA is written to the .bdf file, with FTYPE used. Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction. Stick-Slip is a Coulomb type friction.
Method
For Coulomb type of friction models (options 2, 4, and 5 above), there are 2 methods for computing friction: Nodal Stress, Nodal Force (default). Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type, and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses, respectively for Coulomb fiction.
Relative Sliding Velocity
Critical value for sliding velocity below which surfaces will be simulated as sticking. Relative Sliding Velocity is placed in the 1st field of the 3rd data block for all friction models except Stick-Slip.
Transition Region
Slip-to-Stick transition region. Transition Region is placed in the 1st field of the 3rd data block for Stick-Slip model.
Multiplier to Friction Coefficient
Friction coefficient multiplier. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Friction Force Tolerance
Friction Force Tolerance. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Heat Generation Conversion Factor
A factor related to how much heat is generated by the friction process.
314
Patran Interface to MD Nastran Preference Guide Solution Parameters
Initial Contact Subform
On the Contact Control Parameters subform, select Initial Contact...
Chapter 3: Running an Analysis 315 Solution Parameters
Restart Parameters Subform Includes a Restart option in the MD Nastran input file. Restarts are only supported for SOL 600 in the current release.
Restart Type
You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File
If when restarting a job, you wish the results form the previous run to be copied into the new POST file, then turn this ON. This will place the RESTART or RESTART LAST options before the POST option in the input file. Otherwise they are placed after the POST option which flags MSC.Marc not to copy the results to the new POST file. If you turn this ON, you must have a restarname.t16 and/or restartname.t19 file in your local directory or the MSC.Marc analysis will fail.
Last Converged Increment
Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto
OFF by default. This places a REAUTO option in the input file. Any additional data needed for the REAUTO option are extracted from the first Load Step information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user.
316
Patran Interface to MD Nastran Preference Guide Solution Parameters
Restart from Increment
Defines the increment to be read from the file specified in the Select Restart File form. This is entered in the 3rd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing
Defines the number of increments between writing data to the restart file. This is entered in the 2nd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Write or Read and Write. When Last Converted Increment is ON, this is the 4th field of the 2nd data block of the RESTART LAST option.
Select Restart File...
This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write. This file is specified on the command line for invoking the MSC.Marc solver using the -r option.
Chapter 3: Running an Analysis 317 Solution Parameters
Advanced Job Control Subform (SOL 600) Sets alternate versions of the solver and alternate formats for the results file, for SOL 600 jobs.
Marc Version
Specifies the version of MSC.Marc to run the analysis.
Marc Results File Format
Specifies the file format for the output from the analysis.
Marc Results File Type
Defines the binary output and/or text format of output from the analysis. Binary is recommended since .t16 files are linarily compatible across platforms and take up less space.
318
Patran Interface to MD Nastran Preference Guide Solution Parameters
Marc scratch files w/ Nastran’s Use Environment Variables
Use to enable the use of environment variables.
Suppress Non-SOLMARC Errors
Suppress errors that are not SOL 600 errors.
Submit Marc Job
Submit SOL 600 jobs to Marc.
Use Marc License
Use this to search for, then use Marc licenses.
Copy Marc Files
Make copies of Marc files; for example copy .t16 file.
Filter Marc Text Delete Marc Files
Delete Marc files after the corresponding Patran files are created.
Gradually Release Constraints Analysis Control Defaults
Creates the Nastran Bulk Data entry PARAM, MARCDEF. Its three values are Nastran Development (recommended by Nastran development; Marc SHELL_SECT parameter is set to 11), Marc-Mentat (current Marc standard), Marc Development (recommended by both Marc and Nastran development).
Marc Submit Command
Locates the submit command to run the MSC.Marc analysis (optional). For Specify Full Command its list box will be un-ghosted.
Domain Decomposition Domain Decomposition is used to partition the model into seperate parts (domains) for parallel processing. The Method used to do this is named Domain Decomposition Method (DDM). This form designates that domain decomposition be done manually, semi-automatically, or automatically, for either SOL 400 or SOL 600 jobs.
Chapter 3: Running an Analysis 319 Solution Parameters
320
Patran Interface to MD Nastran Preference Guide Solution Parameters
Decomposition Method
Set this to Automatic if you wish MD Nastran to automatically create the domains during analysis run time. Set to Semi-Automatic if you wish to have MSC.Patran automatically break the model into domains which can be visualized before submittal. Set to Manual to have full control over the domains. This requires the creation of the groups before they can be selected here in this form and associated to a domain.
Number of Domains
This determines how many domains are to be created. When you change this number and press the Enter or Return key, the spread sheet updates with this number of rows. The default is 1. This corresponds to the number of CPUs desired to run the job. For the Automatic method, this is the only input that is required and the spreadsheet is not visible.
Model or Current Group
This is for choosing a part of the model to decompose for parallel processing: Model -- decompose all of the model, Current Group -decompose just the current group. This choice must be consistent with what part of the model is specified for analysis (Analysis: Analyze / Entire Model or Selected Group). This is only active if Decomposition Method is set to Automatic or Semi-Automatic.
Metis Method
There are three Methods that can be used to partition the Model or Current Group into Domains. They are, 1) Nodal Position, 2) Element Topology, or 3) Best (a procedure that accounts for the best of the nodal, element, or vector type algorithms). This method can only be used if Decomposition Method is set to Automatic.
Domain Island Removal
Using this option causes some parts of disjoint domains (domain islands) to be combined with adjacent domains. This can only be used if Decomposition Method is set to Automatic.
Coarse Graph
Using this option sometimes produces domain islands (disjoint domains). This option (the default) is recommended to reduce the time to decompose the initial global domain. Use this only if there is a definite need for a better decomposition. This can only be used if Decomposition Method is set to Automatic.
Single POST File
If more than one CPU processor is used to solve the problem, the seperate/multiple results files can be compiled into a single file for postprocessing using Single POST File.
Create
Click Create to create Domain Information spreadsheet rows. After doing this the number of rows will equal the value of Number of Domains in the form. If Decomposition Method is set to Manual, the previously created group names will be selectable in Select a Group window at the bottom.
Visualize
This is used to display groups. Select a group name for the heading Domain Information under Group. Click Visualize to display just that group. This can be done for some or all of the groups.
Chapter 3: Running an Analysis 321 Solution Parameters
Reset Graphics
Click Reset Graphics to reset the viewport graphics.
Validate
This is for validating (checking) that the domains are not disjoint. For two adjacent domains, the nodes at the interface of the domains must be in both domains.
Domain Information
The window with the definition of each Domain. For a given Domain there is a corresponding unique Group name.
DDAM DDAM is an acronym for Dynamic Design Analysis Method, or DDAM is a methodology for analyzing ship-mounted equipment that the US Navy uses in the event of a near-miss underwater. Most FEA products follow the DDAM methodology, as does any hand calculation. MSC has made several improvements to its products that make DDAM easier to use. To accommodate the special spectrum and summing conventions MSC made several modifications to MD Nastran. A DMAP alter in MD Nastran puts out data important for a DDAM analysis. A stand-alone Fortran program reads the MD Nastran data, calculates the spectral data, formats DDAM run information, and sends data back to MD Nastran for further postprocessing. MSC’s DDAM has the following capabilities. • Calculates all three shock directions simultaneously. • Automatically calculates the appropriate spectra from input of the coefficients. • Performs the NRL sum. • Contains modal selection following 3010 Rev 1 convention. • Provides manual mode selection if needed. • Provides mode-by-mode output if desired. • Uses all available MD Nastran elements. • Provides NRL summed output in MD Nastran OP2 format for use with most postprocessors. • Offers an alternate coefficient input method is available that avoids using the Fortran program,
but the classified coefficients must be entered directly in the data file. • Has unlimited model size. • Uses MSC’s Lanczos Eigenvalue solver for fast solutions.
DDAM has the following limitations. • All base input points must be rigidly connected to a single grid flagged on a SUPORT entry. • There is no easy method to handle closely spaced modes as defined by 3010. • MD Nastran printed output (.f06 file) is not labeled well, and must be used carefully in order to
avoid mistakes. This is especially true of the mode-by-mode output. • A DDAM data file will not read into Patran/MSC.FEA completely.
322
Patran Interface to MD Nastran Preference Guide Solution Parameters
• .XDB output not available for NRL summed quantities • MD Nastran requires additional input switch to be toggled in Patran in order to plot NRL
summed von Mises and combined beam stresses. • MD Nastran does not calculate beam and bar shear stresses. They are not included in the von
Mises and combined stresses reported by MD Nastran DDAM. DDAM in Patran DDAM in MD Nastran is a process that involves three main parts, and a number of smaller parts. The entire procedure is accessed from a simple interface in Patran that integrates the process. • Part 1, Modal Analysis - A modal analysis is run in MD Nastran. This supplies the frequencies,
mode shapes and modal participation for the model. • Part 2, Spectrum Generation – Using the output from Part 1, you can use a Fortran program to
calculate the shock spectrum. This is based on the DDS-072 or NRL 1396 documents, or you can manually enter your own spectrum. • Part 3, Spectrum Application and Data Recovery – The calculated spectrum from Part 2 is
applied to the mode shapes calculated in Part 1, and the results are calculated on a mode-bymode basis. The results from this are then summed using an NRL sum to produce results, one set for each shock direction. The Patran interface presents you with a selection of options to calculate the spectrum and sum the results. The options are stored, and when the MD Nastran modal analysis completes, the Fortran program automatically starts, using the stored options to drive it. MD Nastran automatically resumes after the completion of the Fortran program and finishes the analysis. During is process, a number of files will be created that are inputs and outputs from this process, all named jobname.xxx using the jobname chosen in Patran. The most important files are: jobname.ddd – the DDAM potions file that drives the Fortran program jobname.f11 – the modal information needed to calculate the spectrum jobname.f13 – the calculated spectra information for input back into MD Nastran jobname.ver – modal verification file jobname.opw – Nastran OP2 file with the mode shapes jobname.opx – Nastran op2 file with the NRL summed results for x-shock jobname.opy – Nastran op2 file with the NRL summed results for y-shock jobname.opz – Nastran op2 file with the NRL summed results for z-shock Once the run is complete, you can look over both the results and the modal verification file. If the results are not as expected or desired, there are a number of more advanced capabilities of this DDAM procedure for more control over the process. These include some that are on the Patran forms (changes in 80%
Chapter 3: Running an Analysis 323 Solution Parameters
criterion, minimum G value) and ones that can be accessed using the Patran Direct Text capability (modeby-mode output, specific mode selection). DDAM Model Preparation
In order to run DDAM, all of the fixed base points (excitation inputs) in the model must be rigidly connected to a single point. The MD Nastran RBE2 element is used for this, connecting the independent node (the SUPORT point) to all of the other fixed base/excitation points (dependent grids) in all 6 degrees of freedom. This point is flagged for the SUPORT entry in the DDAM setup. It is not necessary that this point is separated (spatially) from the other input points, you can select one of the base points to be the SUPORT point, as long as all the excitation points are then connected to it. It is not advisable to have any other translational constraints in the model, as they will remove modal mass from the model and the 80% criterion will not necessarily be correct, and the model will have base points that will not be excited. You may have rotational constraints to hold shafting and to remove plate and bar singularities, as the rotational components are not used in the DDAM excitation. No loads or other boundary conditions are needed for the analysis. As per 3010, you need to add operating loads to the shock loads at the conclusion of the analysis. Set up the model like any other modal analysis, with the exception of the SUPORT point. Mass and material density are required to obtain correct mode shapes. The modal analysis parameters are set up on the Subcase Options form, where you can select the number of desired modes, the lower frequency bound, and an upper frequency bound. The analysis uses a Lanczos extraction routine with mass normalization, and uses the default Lanczos debugging information level. You will not have control over these parameters in DDAM.
324
Patran Interface to MD Nastran Preference Guide Solution Parameters
DDAM Solution Parameters
This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when DDAM is selected. Use this form to generate a SOL 187 input file.
Automatic Constraints
Indicates that an AUTOSPC entry is requested. MD Nastran will automatically constrain model singularities.
Shell Normal Tol. Angle
Indicates that MD Nastran will define grid point normals for a Faceted Shell Surface based on the Tolerance Angle. This data appears on a PARAM, SNORM entry.
Mass Calculation
Chapter 3: Running an Analysis 325 Solution Parameters
• Lumped • Coupled
Defines how the mass matrix is to be treated within MD Nastran. This controls the setting of the COUPMASS parameter. This parameter can be set to either Coupled or Lumped. If set to Coupled, COUPMASS will be set to +1, otherwise, it will be set to -1.
Data Deck Echo • None • Sorted • Unsorted
Indicates how the data file entry images are to be printed in the MD Nastran print file. This controls the setting used for the ECHO Case Control command. This parameter can have one of three settings: Sorted, Unsorted, or None.
Plate Rz Stiffness factor
Defines the in plane stiffness factor to be applied to shell elements. This defines the K6ROT parameter. This is an alternate method to suppress the grid point singularities and is intended primarily for geometric nonlinear analysis.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node id for Wt. Gener
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
Default Initial Temperature
Defines the Default Initial Temperature: TEMPD value for subcase entry TEMP(INITIAL)
Default Load Temperature
Defines the Default Load Temperature: Sets the TEMPD value for the subcase entry TEMP(LOAD) subcase entry.
SUPPORT Node
Selects the point you have chosen for your base input. Note that this is a required choice with no default, and that you can only pick one node. If multiple nodes are entered in the data box, only the first one is used.
Results Output Format
On the Results Output Format form you choose which output formats you want to use with your solution type. For more details, please see Results Output Format, 348.
326
Patran Interface to MD Nastran Preference Guide Solution Parameters
Explicit Nonlinear This subordinate form appears when the Solution Parameters button is selected on the Solution Type form when Explicit Nonlinear is selected under Preferences: Analysis... . Use this form to generate a SOL 700 input file.
Parameter Name Large Displacements
Description Use this to cause the large displacement formulation to be used.
Follower Forces
Use this to cause the forces to move (translate and rotate) with the model.
Prestress Option
Use this to cause the pre-stresses to be calculated.
Maximum Printed Lines
Limits the size of the MD Nastran print file that will be generated. This defines the setting of the MAXLINES Case Control command.
Maximum Run Time
Limits the amount of CPU time expressed in CPU minutes that can be used by this run. This is used to prevent runaway jobs. This defines the setting of the TIME Executive Control statement.
Chapter 3: Running an Analysis 327 Solution Parameters
Parameter Name
Description
Wt-Mass Conversion
Defines the conversion factor between weight and mass measures. This defines the setting of the WTMASS parameter.
Node ID for Wt. Gener.
Indicates the node ID that is to be used for the Grid Point Weight Generator. This is the GRDPNT parameter.
SOL 700 Default Settings • Sol700 Parameters...
Either Dytran or Ls-Dyna default settings can be used. Displays the Sol700 Parameters and Extra Data form that is used for specifing parameter values for such things as execution control, dynamic relaxation (entry DAMPGBL), general parameters, contact, and Eulerian parameters. See Sol700 Parameters Subform, 327
• Resultts Output
Format...
Use this to specify the types of files that are to be written for the SOL 700 analysis. For example, XDB (jobname.xdb) and Print (jobname.f06).See Results Output Format, 348
Sol700 Parameters Subform This subordinate form appears when Sol700 Parameters button is selected on the Solution Parameters form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
328
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Execution Control Parameters...
DYSTATIC, DYBLDTIM, DYINISTEP, DYTSTEPERODE, DYMINSTEP, DYMAXSTEP, DYSTEPFCTL, DYTERMNENDMAS, DYTSTEPDT2MS
Dynamic Relaxation...
This is for specifying the entries for the DAMPGBL Bulk Data entry. This is for defining parameter values for static analysis using dynamic relaxation for SOL 700 only.
Chapter 3: Running an Analysis 329 Solution Parameters
Form
Parameters
General Parameters...
DYLDKND, DYCOWPRD, DYCOWPRP, DYBULKL, DYHRGIHQ, DYRGQH, DYENERGYHGEN, DYSHELLFORM, DYSHTHICK, DYSHNIP
Contact Parameters...
DYCONSLSFAC, DYCONRWPNAL, DYCONPENOPT, DYCONTHKCHG, DYCONENMASS, DYCONECDT, DYCONIGNORE, DYCONSKIPTWG
Binary Output Database File Parameters...
DYBEAMIP, DYMAXINT, DYNEIPS, DYNINTSL, DYNEIPH, DYSTRFLG, DYSIGFLG, DYEPSFLG, DYRLTFLG, DYENGFLG, DYCMPFLG, DYIEVERP, DYDCOMP, DYSHGE, DYSTSSZ, DYN3THDT
Time History Output This is for specifying the type of output file (Binary, ASCII, Both), and the Request... Output Time Interval. Hourglass Setting...
See Hourglass Setting Subform, 329
Merge Rigid Mat...
See Merge Rigid Material Subform, 331
Dynamic Relaxation for Restart...
See Dynamic Relaxation for Restart Subform, 333
Damping Per Property...
See Damping Per Property Subform, 335
Rigid Body Switch and Merge...
See Rigid Body Switch and Merge Subform, 337
Eulerian Parameters...
See Eulerian Parameters Subform, 343
SPH Control Parameters...
See SPH Control Parameters Subform, 346
Hourglass Setting Subform This subordinate form appears when Hourglass Setting button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
330
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
Chapter 3: Running an Analysis 331 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Existing Hourglass Setting
List of previously created hourglass settings.
Hourglass Name
Specify the name.
Property Type
Specify either a Shell (2D) or Solid (3D) element type.
Control Type
Choose one of several types of controlling the hourglass effects. The choices are: 1) Standard LSDyna Viscous (Property Type = Shell or Solid), 2) Flanagan-Belytschko Viscous (Property Type = Shell or Solid), 3) Flan-Bely. Visc. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 4) Flanagan-Belytschko Stiffness (Property Type = Shell or Solid), 5) Flan-Bely. Stiff. + Vol. Integ. (exact volume integration for solid elements) (Property Type = Solid), 6) Flanagan-Bindeman Stiffness (Property Type = Solid), 7) Fully Integrated Shell (Property Type = Shell). These entries are defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Hourglass Coefficient
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Warping Hourglass Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Bending Hourglass Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Linear Bulk Visc. Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Quadr. Bulk Visc. Coeff.
This entry is defined on the HGSUPPR Bulk Data entry in the MD Nastran Quick Reference Guide.
Select Property Set
Select a previously created element property. For example, Properties > Create > 2D > Shell > Options: Explicit PSHELL1 > Input Properties... > Shell Formulations > HUGHES.
Add
Click Add after input all necessary data into the Hourglass Setting form to create an Existing Hourglass Setting.
Modify
Click Modify after input all changed data into the Hourglass Setting form to update an Existing Hourglass Setting. You must first select the particular Existing Hourglass Setting.
Merge Rigid Material Subform This subordinate form appears when Merge Rigid Mat button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as:
332
Patran Interface to MD Nastran Preference Guide Solution Parameters
• SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 333 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Existing Merged Materials
List of previously merged MATRIG materials. MATRIG is an MD Nastran Bulk Data entry for defining rigid body properties.
Merged Material Name
Specify the name of merged material to be created.
Select Material to be Merged into
Specify the name of an MATRIG material to merge other MATRIG materials into.
Select Materials to be Merged
Specify the names of MATRIG materials that are to be merged into the merged material whos name is specified under Merged Material Name.
Add
Click Add after input all necessary data into the Rigid Materials form to create an Existing Merged Materials.
Modify
Click Modify after input all changed data into the Rigid Materials form to update an Existing Merged Materials. You must first select the particular Existing Merged Materials.
Dynamic Relaxation for Restart Subform This subordinate form appears when Dynamic Relaxation for Restart button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
334
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form Relaxation [Termination Time] Convergence Tolerance Number of Iterations Papadrakakis Auto Control
Parameters Use this to not use (None Active) or use (Activated Relaxation) relaxation in performing the simulation. The time to stop the simulation. This is optional ([ ]). Specify convergence tolerance. Specify the maximum number of iterations. Click the checkbox to specify that convergence control is to be automatic using the Papadrakakis method.
Chapter 3: Running an Analysis 335 Solution Parameters
Form Papadrakakis Convergence Tolerance
Parameters To use this it is necessary to not select Papadrakakis Auto Control.
Relaxation Factor Time step scale Factor
Specify the value of the Relaxation Factor. Specify the value of the Time step scale Factor.
Damping Per Property Subform This subordinate form appears when Damping Per Property button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
336
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Damping Type
Select either Property (use property) or Stiffness (use Rayleigh damping).
System Damping Constant Table
Select a time dependent field under Time Dependent Field. This field will be multiplied by the Scalar Factor for Load Curve entry. The (X,Y,Z) Trans. Damping Forces and (X,Y,Z) Rot. Damping Moments entries (all of these form a 6 component load vector) are multiplied by the scaled time dependent field.
Chapter 3: Running an Analysis 337 Solution Parameters
Form
Parameters
Time Dependent Field
Select a Field, with it being entered into the System Damping Constant Table list box. For example, select the field named damping_vs_time under Time Dependent Field. For System Damping Constant Table f:damping_vs_time appears.
Scale Factor for Load Curve
Specify the scale factor that will multiply the Time Dependent Field specified under System Damping Constant Table.
X Trans. Damping Forces
Scale factor for X translation damping forces, in the global coordinate system directions.
Y Trans. Damping Forces
Scale factor for Y translation damping forces, in the global coordinate system directions.
Z Trans. Damping Forces
Scale factor for Z translation damping forces, in the global coordinate system directions.
X Rot. Damping Moments
Scale factor for X rotation damping moments, in the global coordinate system directions.
Y Rot. Damping Moments
Scale factor for Y rotation damping moments, in the global coordinate system directions.
Z Rot. Damping Moments
Scale factor for Z rotation damping moments, in the global coordinate system directions.
Rayleigh Damping Coeff.
Specify the scalar coefficient () that the global stiffness matrix is multiplied by to obtain the Rayleigh damping matrix.
Rigid Body Switch and Merge Subform This subordinate form appears when Rigid Body Switch and Merge button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
338
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is At Start (D2R0000).
Existing Merged Properties
List of deformable body and rigid body properties that have already been merged.
Merged Body Name
Specify the name of the Existing Merged Properties entry to be created.
Deformable Property
Select an entry under Deformable Property
Chapter 3: Running an Analysis 339 Solution Parameters
Form
Parameters
Master Rigid Property
Select an entry under Master Rigid Property
Add
Click Add to create an entry under Existing Merged Properties.
Modify
Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Define Set of Parts to See Define Set of Parts to be Switched Subform, 340 be Switched Define Inertial Properties of Rigid Body
See Define Inertial Properties of Rigid Body Subform, 342
340
Patran Interface to MD Nastran Preference Guide Solution Parameters
Define Set of Parts to be Switched Subform This subordinate form appears when Define Set of Parts to be Switched button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient.
Chapter 3: Running an Analysis 341 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is At Stage (D2RAUTO).
Existing Merged Properties
List of deformable body and rigid body properties that have already been merged.
Merged Body Name
Specify the name of the Existing Merged Properties entry to be created.
Deformable Property
Select an entry under Deformable Property.
Master Rigid Property
Select an entry under Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
Add
Click Add to create an entry under Existing Merged Properties.
Modify
Click Modify to save the changed selections under Deformable Property and Master Rigid Property to update an Existing Merged Properties. You must first select the particular Existing Merged Properties.
Starting Switch Time Specify the time to switch the deformable and rigid properties. Ending Switch Time
Specify the time to terminate the switching of the deformable and rigid properties.
Delay Period
Specify the time delay ( for switching.
Rigid Wall/Contact Surf Number
Specify the surface numbers for rigid walls/surfaces that are to contact.
Related Switch Set Max. Permited Time Specify the maximum time step. Step Size Number of Deformable Parts to Rigid
Specify the number of deformable parts that will be switched to rigid parts.
Number of Rigid Parts to Deformable
Specify the number of rigid parts that will be switched to deformable parts.
Activation Code Switch
Select one of the five flags, 1) EQ.0, 2) EQ.1, 3) EQ.2, 4) EQ.3, or 5) EQ.4.
Pair of Related Switches
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.-1.
Nodal Rigid Body Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Nodal Constraint Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
Rigid Wall Activation Flag
Select one of the three flags, 1) EQ.0, 2) EQ.1, 3) EQ.2.
342
Patran Interface to MD Nastran Preference Guide Solution Parameters
Define Inertial Properties of Rigid Body Subform This subordinate form appears when Define Inertial Properties of Rigid Body button is selected on the Rigid or Deformable Parts Switching form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 343 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Option
Only option is New Rigid Props. (D2RINNER).
Master Rigid Property
Select a Master Rigid Property. For example, a 2D Shell Element Property created using an Isotropic (SOL 700) Rigid MATRIG material.
X Coord of Center of X coordinate of center of mass. Mass Y Coord of Center of Y coordinate of center of mass. Mass Z Coord of Center of Z coordinate of center of mass. Mass Translational Mass
Scalar mass value for translation, not rotation.
XX Comp. of Inertia Tensor (IXX)
XX (1,1) component of inertia tensor matrix.
XY Comp. of Inertia Tensor (IXY)
XY (1,2) component of inertia tensor matrix.
XZComp. of Inertia Tensor (IXZ)
XZ (1,3) component of inertia tensor matrix.
YY Comp. of Inertia Tensor (IYY)
YY (2,2) component of inertia tensor matrix.
YZ Comp. of Inertia Tensor (IYZ)
YZ (2,3) component of inertia tensor matrix.
ZZ Comp. of Inertia Tensor (IZZ)
ZZ (3,3) component of inertia tensor matrix.
Eulerian Parameters Subform This subordinate form appears when Eulerian Parameters button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
344
Patran Interface to MD Nastran Preference Guide Solution Parameters
.
The supported parameters are shown in the following table: Form
Parameters
Euler Boundary Treatment
There are three choices, 1) Default, 2) Extrapolate (extrapolate structural mesh pressure to Euler elements at solid/fluid boundary), or 3) Element (solid/fluid boundary Euler element pressure equals the structural element pressure at the solid/fluid boundary).
Multi-Mat. Trans. Scheme
There are three choices, 1) Default (Impulse), 2) Average (face (surface) velocity is averaged simply), or 3) Impulse (face (surface) velocity is impulse weighted).
Material Failure Option
There are three choices, 1) Default (No Fail), 2) Fail (activates transport of fail fraction and thereby keeps track of material that has failed), or 3) No Fail (failed Euler material can support shear stress again as soon as new material enters the Euler element).
Chapter 3: Running an Analysis 345 Solution Parameters
Form
Parameters
Multi-Material Array Size
The multi-material Eulerian elements use an overflow array to store their material data. This array can hold “Multi-Material Array Size” times the number of Eulerian elements. If more the 10% of the Eulerian elements have more than one material, the value of “Multi-Material Array Size” must be increased.
Initial Condition Accuracy
A parameter value used to specify the accuracy of the initial conditions in Eulerian elements, when using the geometric shape definition. The parameter value is specified in the input file using PARAM, MICRO, value.
Mimimum Velocity
A parameter value used to specify the minimum velocity. If a calculated velocity is less than this, it is set to zero (0). It is mainly used to eliminate harmless small values. The parameter value is specified in the input file using PARAM, VELCUT, value.
Maximum Velocity
Specify the maximum velocity for Eulerian and Lagrangian meshes. Although it is not usually necessary to limit the velocity in Eulerian meshes, there are occasions in regions of near-vacuous flow where using this can be an advantage. The same thing applies to Lagrangian meshes, where there is contact. The parameter value is specified in the input file using PARAM, VELMAX, value, YES/NO. Default is 1.0e10, YES. See the next row for information on what YES/NO means.
Small Mass Removal Because very high velocities occur mostly in Eulerian elements with very small mass, the mass in these elements may need to be removed for the analysis to be stable. The above parameter (PARAM, VELMAX) is used to specify whether or not to eliminate small masses. YES = eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. NO = do not eliminate the mass for Eulerian elements for which the velocity is > the value of VELMAX. Default = YES. Universal Gas Constant
Specify the value of the universal gas constant. The parameter value is specified in the input file using PARAM, UGASC, value.
Single Material Elements
Specify the minimum density of single material Eulerian elements. For arbitrary LagrangeEuler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Single Mats. with Strength
Specify the minimum density of single material Eulerian elements with strength. For arbitrary Lagrange-Euler (ALE) coupling, Eulerian single material elements with strength cannot be used.
Multi-Material Elements
Specify the minimum density of multi-material Eulerian elements.
Roe Solver Scheme
Specify whether or not to use the Roe solver. The Roe solver accounts for momentum exchange between Lagrange (structure) and Eulerian material.
Spatial Accuracy
There are two schemes that can be used. They are, 1) 1st Order (left and right state variables are taken as the values the state variables have at the left- and the right-element center), or 2) 2nd Order (left- and right-state variable values at a face by including the left-left and the right-right element).
Time Integration Scheme
There are two schemes that can be used. They are, 1) 1st Order, or 2) 2nd Order (three-stage time integration scheme).
346
Patran Interface to MD Nastran Preference Guide Solution Parameters
SPH Control Parameters Subform This subordinate form appears when SPH Control Parameters (SPH refers to smooth “particle hydrodynamics”) button is selected on the Sol700 Parameters and Extra Data form of either Explicit Nonlinear or other structural Solution Type where Sol700 is available such as: • SOL700,101 - Linear Static • SOL700,106 - NonLinear Static • SOL700,109 - Direct Transient Response • SOL700,129 - NonLinear Transient
.
Chapter 3: Running an Analysis 347 Solution Parameters
The supported parameters are shown in the following table: Form
Parameters
Number of Cycles
Specify the number of cycles between particle sorting.
Death Time
Specify the time when SPH calculations are to be stopped.
Initial Number of Neighbors
Specify the initial number of neighbors per particle. This parameter is for specifying how much memory is to be allocated for arrays during initialization. If the value is positive, the memory will be dynamically allocated. If the value is negative, the memory allocation will be static (constant). During the calculation only the closest SPH elements will be considered as neighbors. Using this option can avoid memory allocation problems.
Particle Approx. Theory
There are six theories to choose from, 1) Renormalization (approximation), 2) Symmetric (formulation), 3) Sym. Renormalization (symmetric renormalization approximation), 4) Tensor (tensor formulation), 5) Fluid Particle (fluid particle approximation), 6) Fluid Particle Renorm (fluid particle with renormalization approximation).
Start Time
Specify the time to begin particle approximation.
Maximum Velocity
Maximum velocity for the SPH particles. Particles whos velocity > this value are deactivated.
Computation of Approx.
Select one of the following for two different SPH parts, 1) Particle Approximation (approximation is calculated), or 2) No Particle Approximation (approximation is not calculated; two different SPH materials cannot interact with each other, and penetration is allowed).
Intergration Type
Select 1) 0 ( d h t = 1--- h t div v ), or 2) 1 dt
d
( d h t = 1--- h t div v 1 3 ), for time integrating to obtain the dt
d
smoothing length. Smoothing Length Comput.
Select 1) Bucket (sort based on algorithm; very fast), or 2) Global (computation for all the model particles ). This is done during initialization.
Box Type
Select either 1) Fixed (the box remains fixed in space), or 2) Moving (the user specifies two corners of the box and a the time dependent Field to describe the motion of the two corners). As long as a given SPH particle is in a box, the SPH calculation for the particle is performed for the box. If the particle leaves the box it was inside, it is deactivated.
Select Box
Select the name of a box under Select Box. A box must have been previously created under Loads/BCs: Create / Box Definition / Nodal.
Tail Vector
Specify a vector, <X1 Y1 Z1>, that defines the minimum coordinates of the box (coordinates of the corner of the box at the minimum location).
348
Patran Interface to MD Nastran Preference Guide Solution Parameters
Form
Parameters
Head Vector
Specify a vector, <X2 Y2 Z2>, that defines the maximum coordinates of the box (coordinates of the corner of the box at the maximum location).
Motion Vs Time Data
Specify the time dependent Field that defines the motion of the two corners of the box.
Vel./Disp. Flag
Specify whether the time dependent Field is a Velocity or Displacement field.
Coord. System
Specify the coordinate system that the Tail and Head Vectors are defined in.
Results Output Format With the results output format form you can choose which output formats you want to use with each solution sequence. The appropriate defaults are set for each solution type. These defaults can be changed or set in the settings.pcl file.
Data Output
Defines the type of data output.
• OP2
Specifies output of data to a MD Nastran OUTPUT2 file (*.op2). This will place a PARAM, POST, -1 in the input file.
• XDB
Specifies output of data to a MSC.Access database (*.xdb). This will place a PARAM, POST, 0 in the input file.
Specifies output of data to a MD Nastran print file (*.f06).
• Punch
Specifies output of data to a MD Nastran punch file (*.pch).
• MASTER Only
When ON, only a .master file is written.
• MASTER/DBALL
When ON, both a .master file and a .dball file are written.
• XDB Buffer Size
For the XDB results file, defines the buffer size used for accessing results.
Chapter 3: Running an Analysis 349 Solution Parameters
OUTPUT2 Requests
Specifies type of OUTPUT2 commands. • P3 Built In - signals the use of MD Nastran internal OUTPUT2 commands geared
toward Patran. These commands are also appropriate for PATRAN 2. The “P3 Built In” option is appropriate only for Database Runs, see Solution Parameters, 277. If Database Run has been deselected, this option will be set internally to “Alter File”. • Alter File - specifies the use of an external alter file found on the Patran file path and following the “msc_v#_sol#.alt” naming convention. See Files, 572 for more
details. • CADA-X Alter - specifies the use of an LMS CADA-X specific alter file that is
identical to the “Alter File” but with an additional “.lms” extension, for example, “msc_v67_sol103.alt.lms”. • P2 Built In - specifies use of MD Nastran internal OUTPUT2 commands geared
toward PATRAN 2. OUTPUT2 Format
Specifies format of the MD Nastran OUTPUT2 (*.op2) files. Use “Text” format when the resulting OUTPUT2 file must be transported between heterogeneous computer platforms.
A new variable has been added to the settings.pcl file for results output format defaults per SOL sequence: NASTRAN_nnn_DATA_OUTPUT OP2+PUNCH Where nnn is the solution sequence 101, 400 etc... and OP2+XDB+PRINT+PUNCH+MASTER +DBALL are the options. This variable is only read from the settings.pcl file when opening a new database, creating a new job or changing the solution sequence of an existing job. Otherwise the results output settings are retrieved from the database for an existing job. Note that these variables must be added to the settings.pcl file by the user and if they do not exist, a standard default is used. Also note that OP2 and XDB are mutually exclusive and both cannot be specified at the same time. The same is true for MASTER Only and MASTER/DBALL. The settings.pcl file may have one of these variables for each SOL sequence defined in Patran (>100).
350
Patran Interface to MD Nastran Preference Guide Solution Parameters
ADAMS Preparation This form is used when you want to prepare a database for an Adams job.
Chapter 3: Running an Analysis 351 Solution Parameters
ADAMS Output
• MNF Only • Full Run + MNF
Units
• Mass - Your options are: Kilogram, Pound-Mass, Slug, Gram, Ounce-
Mass, Kilo-Pound-Mass, Megagram • Force - Newton, Pounds-Force, Ounce-Force, Dyne, Kilo-Newton, Kilo-
Pound-Force • Length - Millimeter, Centimeter, Meter, Kilometer, Inch, Foot, Mile • Time - Millisecond, Second, Minute, Hour
Craig-Bampton Modes Bounds
• Lower Bound • Upper Bound
Num. Shapes to Adams ADAMS Debug Print Strip Face Create .out(OP2 file) for MSC Fatigue Mass Options
• Partial • Constant File • Full • None
Output Requests Transfer Groups to ADAMS
352
Patran Interface to MD Nastran Preference Guide Select Superelements
3.6
Select Superelements The superelements created in the FEM menu are displayed in the form below. The superelements for a subcase are selected by highlighting the name in the listbox. Default button unselects all the superelements. If Write PART Superelements toggle is ON in the Translation Parameters, 265 form, then BEGIN BULK SUPER=id sections are written to the input file to define the superelements, otherwise if this is OFF, SESET entries are used. In addition to selecting the superelement, you can specify the superelement tree definition. This tell the analysis which superelement are upstream of others and thus, not directly connected to the residual structure or superelement zero (SE0). To define an upstream SE relative to its downstream SE, use the form shown below to fill out the spreadsheet. Put focus in the Downstream databox, select a superelement from the list, then select the upstream from the list and press Add. This adds a row to the spreadsheet. Repeat this for every upstream element you need to define. Clicking on a row in the spreadsheet and clicking Remove will remove the defintion. Downstream SEs can only appear in the speadsheet once. This writes the SETREE entry.
Chapter 3: Running an Analysis 353 Select Superelements
SE6
SE5 SE4
SE3
SE1
SE0
SE2 In this example, SE1, SE2, & SE3 are upstream of the residual. This is not necessary to define in the SE tree. However SE4 is upstream of SE3 and SE5 & SE6 are upstream of SE4. These should be defined in the tree.
354
Patran Interface to MD Nastran Preference Guide Subcases
3.7
Subcases This form appears when the Subcases... button is selected on the Analysis form. The subcase is the MD Nastran mechanism for associating loads and boundary conditions, output requests, and various other parameters to be used during part of a complete run. The Patran MD Nastran interface automatically associates default parameters and output requests with each Patran load case to create a subcase with the same name as the load case. You can access the Subcase Parameters... and Output Requests... forms to view or modify these defaults.
Options are Create, Delete, and Global Data.
Displays all the available subcases associated with the current Solution Sequence.
The subcase name that is being created or modified is displayed in this databox. It can be typed in or picked from the Available Subcases listbox.
Displays all the available loadcases in the current database. Only one loadcase can be selected per subcase. For Normal Modes and Complex Eigenvalue solution types, free-free runs can be generated by using an empty load case.
Chapter 3: Running an Analysis 355 Subcases
Deleting Subcases To delete subcases, select Subcases from the Analysis form, and set the Action to Delete.
Select the subcase(s) to delete.
Apply to delete the selected subcases.
356
Patran Interface to MD Nastran Preference Guide Subcases
Editing Subcases To edit global data for subcases, select Subcases from the Analysis form, and set the Action to Global Data. The following form appears.
Select Subcase(s) to edit associated data.
Use Output Requests... to edit the output requests associated with the selected subcases. The Edit Output Request form appears. See Edit Output Requests Form, 426.
Apply changes the output requests for all selected subcases. Cancel closes the form without changes.
Chapter 3: Running an Analysis 357 Subcase Parameters
3.8
Subcase Parameters The subcase parameters represent the settings in MD Nastran Case Control that take effect within a subcase and do not affect the analysis in other subcases. Currently, the following solution sequences have subcase parameters associated with them. Solution Sequences
Linear Static Subcase Parameters, 358
SOL 101
Nonlinear Static Subcase Parameters, 359
Other Conditions Model has p-elements and utilizes Version 68
Selects the subcase to participate in the error analysis calculations in an adaptive analysis. By default the subcase participates in the error analysis.
None
Selects nonlinear static iteration parameters.
None
Selects nonlinear transient iteration parameters.
Version 68
Selects real eigenvalue extraction parameters.
SOL 106, 66 Nonlinear Transient Subcase Parameters, 362
Description
SOL 129, 99 Normal Modes Subcase Parameters, 364
SOL 103 Implicit Nonlinear Subcase Parameters, 375 DDAM Subcase Parameters, 407 Explicit Nonlinear Subcase Parameters, 409
358
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Linear Static Subcase Parameters This form is available for solution sequence 101 for MSC.Nastran Version 68 and for models that contain p-elements. The form allows the inclusion of subcases in the error analysis. This toggle sets the ADACT Case Control command.
Used to turn rotor dynamics on for the linear static subcase. If enabled, the “Specify Rotor Speed” button will be enabled, and can be selected to display the Rotor Speed Form, below. See Contact Table, 396 for more information.
The reference rotor for the subcase. This drives the RGYRO case control and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speed to the reference rotor. These values define the SPDUNIT and SPEED fields of the MD Nastran RGYRO Bulk Data entry. The SPDHIGH and SPDLOW entries are left blank.
Chapter 3: Running an Analysis 359 Subcase Parameters
Nonlinear Static Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Nonlinear Static. This form allows the definition of the parameters that control the interation criteria for a Nonlinear Static analysis. All of the data is part of the NLPARM Bulk Data entry. If Arc-Length Method is selected, additional data for the NLPCI Bulk Data entry is generated. Defines the number of increments to be used to apply the full load. This is the NINC field.
Defines what method to use to control the stiffness. Matrix updates as the load is incrementally applied. This parameter can have one of three settings: Automatic, SemiAutomatic, or Controlled Iter. This defines the setting of the KMETHOD field. Defines the number of iterations to be used after each matrix update. This is the KSTEP field. Defines the limit for the number of iterations that can be done in any given increment. This is the MAXITER field.
Opens a subordinate form to activate the Arc-Length Method which is turned OFF by default. The Arc-Length Method is used to explore post-buckling paths.
Activates a buckling analysis at the end of the subcase.
Opens subordinate form to define eigenvalue extraction parameters. See Solvers/Options, 404 for more information.
Activates a normal mode analysis of the prestressed system at the end of the subcase.
360
Patran Interface to MD Nastran Preference Guide Subcase Parameters
This is a list of data input available for defining the Static Nonlinear Iterations that was not shown on the previous page. Parameter Name Displacement Error Displacement Tolerance
Load Error Load Tolerance
Work Error Work Tolerance
Default Load Temperatures
Description Indicates whether a displacement convergence criteria should be used. If Displacement Error is selected, the Displacement Tolerance field becomes active. This value defines the tolerance on displacements. The displacement tolerance must be met between iterations to define convergence. If Displacement Error is selected, a U is entered in the CONV field. The Displacement Tolerance is the EPSU field. Indicates whether a load convergence criteria should be used. If Load Error is selected, the Load Tolerance field becomes active. This value defines the tolerance on load equilibrium. The load equilibrium tolerance must be met between iterations to define convergence. If Load Error is selected, a P is entered in the CONV field. Load Tolerance is the EPSP field. Indicates whether a work convergence criteria should be used. If Work Error is selected, the Work Tolerance field becomes active. This value defines the tolerance on work error. The work tolerance must be met between iterations to define convergence. If Work Error is selected, a W is entered in the CONV field. Work Tolerance is the EPSW field. Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
Chapter 3: Running an Analysis 361 Subcase Parameters
Arc-Length Method Parameters This subordinate form appears when the Arc-Length Method button is selected on the Subcase Parameters form. This form allows the definition of parameters that control the Arc-Length Method. All of the data is part of the NLPCI Bulk Data entry. Defines the type of Arc-Length Method: CRIS = Crisfield method (default) RIKS = Riks method MRIKS = modified Riks method
Minimum allowable arc-length adjustment ratio between increments for the adaptive arc-length method 0.0MINALR1.0.
Maximum allowable arc-length adjustment ratio between increments for the adaptive arc-length method MAXALR1.0. Scale factor w for arc-length criteria: w=0, displacement control w>0, combined load and displacements control w»1, load control Desired number of iterations for convergence to be used for the adaptive arc-length adjustments. This is the DESITER field Maximum number of controlled increment steps allowed within the subcase. This is the MXINC field.
362
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Nonlinear Transient Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Nonlinear Transient. All of the data is part of the TSTEPNL Bulk Data entry.
Defines the Ending Time and Number of Time Steps for the subcase. Defines what method to use to control the stiffness. The Mass matrix updates as the load is incrementally applied. This parameter can have one of three settings: Adaptive, Automatic, or Time Step. This is the METHOD field.
Defines the number of time steps to be used in each matrix update. This can only be set if Matrix Update Method is set to Time Step. This is the NDT field. Defines the maximum number of time step bisections to be used in each matrix update. This can only be set if Matrix Update Method is set to Adaptive. This is the MAXBIS field. Defines the limit for the number of iterations that can be done in any given increment. This is the MAXITER field.
Chapter 3: Running an Analysis 363 Subcase Parameters
This is a list of data input available for defining the Transient Nonlinear Iterations that was not shown on the previous page. Parameter Name Displacement Error Displacement Tolerance
Load Error Load Tolerance
Work Error Work Tolerance
Default Load Temperatures
Description Indicates whether a displacement convergence criteria should be used. If Displacement Error is selected, the Displacement Tolerance field becomes active. This value defines the tolerance on displacements that must be met between interactions to define convergence. If Displacement Error is selected, a U is entered in the CONV field. The Displacement Tolerance is the EPSU field. Indicates whether a load convergence criteria should be used. If Load Error is selected, the Load Tolerance field becomes active. This value defines the tolerance on load equilibrium that must be met between iterations to define convergence. If Load Error is selected, a P is entered in the CONV field. Load Tolerance is the EPSP field. Indicates whether a work convergence criteria should be used. If Work Error is selected, the Work Tolerance field becomes active. This value defines the tolerance on work error that must be met between iterations to define convergence. If Work Error is selected, a W is entered in the CONV field. Work Tolerance is the EPSW field. Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
364
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Normal Modes Subcase Parameters The Normal Modes subcase parameters form is available only for Solution 106 for MSC.Nastran Version 70.7. Use this form to create either EIGR or EIGRL Bulk Data entries. Defines the method to use to extract the real eigenvalues. This parameter can be set to any one of the following: Lanczos, Automatic Givens, Automatic Householder, Modified Givens, Modified Householder, Givens, Householder, Enhanced Inverse Power, or Inverse Power. If this is set to Lanczos, this indicates that an EIGRL Bulk Data entry should be created. Otherwise, this defines the setting of the METHOD field on the EIGR Bulk Data entry.
Defines the lower and upper limits to the range of frequencies to be examined. These are the F1 and F2 fields on the EIGR Bulk Data entry or the V1 and V2 fields on the EIGRL Bulk Data entry.
Indicates an estimate of the number of eigenvalues to be located. This parameter can only be specified if Extraction Method is set to Enhanced Inverse Power or Inverse Power. This is the NE field on the EIGR Bulk Data entry.
See Contact Table, 396 for more information.
Chapter 3: Running an Analysis 365 Subcase Parameters
This is a list of data input available for defining the Real Eigenvalue Extraction that was not shown on the previous page. Parameter Name
Description
Number of Desired Roots
Indicates the limit to how many eigenvalues to be computed. This is the ND field on the EIGR or EIGRL Bulk Data entries.
Diagnostic Output Level
Defines the level of desired output. This can take any integer value between 0 and 3. This parameter can only be specified if Extraction Method is set to Lanczos. This is the MSGLVL field on the EIGRL Bulk Data entry.
Normalization Method
Indicates what type of eigenvalue normalization is to be done. This parameter can take one of three settings: Mass, Maximum, or Point. This parameter cannot be specified if Extraction Method is set to Lanczos. Defines the setting of the NORM field on the EIGR Bulk Data entry.
Normalization Point
Defines the point to be used in the normalization. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the G field on the EIGR Bulk Data entry.
Normalization Component
Defines the degree-of-freedom component at the Normalization Point to be used. This can only be selected if Normalization Method is set to Point. This parameter cannot be specified if Extraction Method is set to Lanczos. This is the C field on the EIGR Bulk Data entry.
Number of Modes in Error Analysis
Indicates how many modes will participate in the error analysis when the model contains p-elements. This data sets the ADACT Case Control command.
Default Load Temperatures
Creates TEMPD entry for specified Subcase and is called out using TEMP case control. This defines temperatures on all grids(modes) that do not have specific temperature LBCs defined
366
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Complex Eigenvalue Subcase Parameters This subordinate form appears when you select Subcase Parameters button on the Subcases form and the solution type is Complex Eigenvalue.
Used to turn rotor dynamics on for the complex eigenvalue subcase. If enabled, the “Specify Spin Properties” button will be enabled, and can be selected to display the Spinning Properties Form, below. Rotor dynamics is disabled by default.
See Contact Table, 396 for more information.
Synchronous (default) or Asynchronous Defines the SYNCFLG field of the MD Nastran RGYRO Bulk Data entry.
The reference rotor for the subcase. This drives the RGYRO Case Control and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speeds to the reference rotor. These values define the SPDUNIT, SPDHIGH, and SPDLOW fields of the MD Nastran RGYRO Bulk Data entry. The SPEED value is left lank. For Asynchronous analyses, a single Speed databox is presented, defining SPEED field, while SPDHIGH and SPDLOW are left blank.
Chapter 3: Running an Analysis 367 Subcase Parameters
Transient Response Subcase Parameters This subordinate form appears when you select Subcase Parameters button on the Subcases form and the solution type is Transient Response. Use this form to specify the time step interval and duration for a transient response analysis. All of the data is part of the TSTEP Bulk Data entry. Direct Transient and Modal Transient Solutions
This is the subcase parameters form for the Direct Transient and Modal Transient solution.
Use this button to define your TSTEP entry.
Modal Damping is only shown if you select Modal Damping formulation from the Solution Type form.
Use this button to define your TABDMP1 entry. You must enter at least one value of frequency and damping on the spreadsheet for damping to occur. See Contact Table, 396 for more information.
368
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Define Time Step
Use this form to define the time steps in a linear table. Values of Delta-T (Time Increment) must be positive. See MD Nastran Quick Reference Guide TSTEP for more information.
The "Skip Factor" column is optional. If the column is empty, MD Nastran assumes the Skip Factor is 1.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, select click on the row label and select "Add Row".
No. of Time Steps and Delta-T determine the solution points in time. The skip factor defines which of the solution points you wish to perform results processing on. A skip factor of 1 indicates every time step, 2 indicates every other solution step, etc. Total solution time accumulates in order of entry. For the example shown, MD Nastran will calculate output at 100 time steps ranging between 1. and 100. Define Damping
Use this form to define Damping in a linear table. Values of frequency must be positive. Discontinuities (same value of frequency, different value of damping) are allowed at all locations except the first and last entries in the table. See MD Nastran Quick Reference Guide TABDMP1 for more information. Modal Damping does not allow a discontinuity to exist as either the first or last entries in the modal damping data. This will cause an error in MD Nastran. It is strongly recommended that you do not create such scenario. If the first and second frequencies (two lowest frequencies) are the same value, a warning will be issued, even if the damping value for those frequencies are the same. If the last and second to last frequencies
Chapter 3: Running an Analysis 369 Subcase Parameters
(two highest frequencies) are the same value, a warning will be issued, even if the damping value for those frequencies are the same.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
370
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Frequency Response Subcase Parameters This subordinate form appears when you select the Subcase Parameters button on the Subcases form and the solution type is Frequency Response. Use this form to specify the frequencies for a frequency response analysis. All of the data is part of a FREQi Bulk Data entry. Frequency Solution
This is the Frequency Subcase Parameter Form.
Use this button to define FREQ,FREQ1,FREQ2, FREQ3, FREQ4 entries.
Modal Damping is only shown if you select Modal Damping formulation from the Solution Type form.
Use this button to define a TABDMP1 entry. At least one value of frequency and damping must be entered on the spreadsheet for damping to occur. Used to turn rotor dynamics on for the complex eigenvalue subcase. If enabled, the “Specify Spin Properties” button will be enabled, and can be selected to display the Spinning Properties Form, below. Rotor dynamics is disabled by default.
See Contact Table, 411 for more information. See Solvers/Options, 404 for more information.
Chapter 3: Running an Analysis 371 Subcase Parameters
Use this form to create FREQi entries.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
The driving column on this form is the Increment type. Direct Frequency
When the Increment type is...
Patran...
Discrete
Creates a FREQ entry where Start Freq is the frequency value. Multiple Discrete rows will be written to the same FREQ entry. End Freq. and No. Incr. columns are not used.
Linear
Creates a FREQ1 entry. The Start Freq. will be the first frequency and the End Freq. and No. Increments will have a linear progression in between.
Logarithmic
Creates a FREQ2. Same as Linear, except it will have a logarithmic progression.
Modal Frequency
When the Increment Type is... Discrete
Patran... Creates a FREQ entry where Start Freq is the frequency value. Multiple Discrete rows will be written to the same FREQ entry. End Freq, No. Incr. and Cluster/Spread columns are not used.
372
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Linear
Creates a FREQ1 entry. The Start Freq. will be the first frequency and the End Freq. and No. Increments will have a linear progression in between. The Cluster/Spread column is not used.
Logarithmic
Creates a FREQ2. Same as Linear, except it will have a logarithmic progression.
Lin. Cluster
Creates a FREQ3 with type set to LINEAR. This results in a linear distribution of solution frequencies between each successive pair of natural modes in the specified frequency interval. The Cluster value, which has a default of 1.0 is used to bias the linear distribution of solution frequencies. A smaller cluster value has a closer spacing towards the center, CLUSTER greater than 1.0 has a closer spacing at the ends of the frequency range.
Log. Cluster
Same as Lin. Cluster except that a logarithmic interpolation is used between the start and end frequencies.
Lin. Spread
Creates a FREQ4 entry. The default value of spread is 0.1. The spread is a fractional amount specified for each mode. With a spread of 0.3 and No. Incr. of 21, there will be 21 evenly spaced frequencies between 0.7*FN and 1.3*FN, where FN a natural frequency, for all natural frequencies between the specified “Start Freq” and “End Freq” values.
Fractional Spread
Creates a FREQ5 entry. Enter the Start Frequency and End Frequency. These are the lower and upper bound for the excitation (solution) frequency domain, respectively. It is desired to obtain a set of excitation frequencies around and at each natural frequency, obtained previously from the corresponding modal analysis for this simulation. This is done by providing a list of fractions; for example {fr_1, fr_2, ..., fr_n}. The list is “multiplied” by each natural frequency to provide a list of excitation frequencies for each natural frequency; for example fn_j * {fr_1, fr_2, ..., fr_n}, where fn_j is the jth natural frequency. The fractions cannot be inserted on a single row of the Define Frequencies form, but multiple rows must be created, with just one fraction per row.
Define Damping
Use this form to define the damping in a linear table. Values of frequency must be positive. Discontinuities (same value of frequency, different value of damping) are allowed at all locations except the first and last entries in the table. See MD Nastran Quick Reference Guide TABDMP1 for more information. Modal Damping does not allow a discontinuity to exist as either the first or last entry in the modal damping data. This will cause an error in MD Nastran. It is strongly recommended that you do not create such scenario. If the first and second frequencies (two lowest frequencies) are the same value, a warning will be issued, even if the damping values for those frequencies are the same. If the last and second to last frequencies
Chapter 3: Running an Analysis 373 Subcase Parameters
(two highest frequencies) are the same value, a warning will be issued, even if the damping values for those frequencies are the same.
"Add Row" adds a row after the selected row. To insert a row at the beginning of the table, click on the row label and select "Add Row".
To create a Field for the damping data, click in the Create a Field checkbox.
To bring in damping data from an existing Field, click on the Load Data From Field button, then select the Field.
Spinning Properties, Frequency Response
Presented when Rotor Dynamics is ON and the Specify Spinning Properties button is selected.
374
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Synchronous (default) or Asynchronous Defines the SYNCFLG field of the MD Nastran RGYRO Bulk Data entry.
The reference rotor for the subcase. This drives the RGYRO Case Dontrol and Bulk Data (REFROTR field) in the MD Nastran Bulk Data file.
Relative speeds to the reference rotor. These values define the SPDUNIT, SPDHIGH, and SPDLOW fields of the MD Nastran RGYRO Bulk Data entry. The SPEED value is left lank. For Asynchronous analyses, a single Speed databox is presented, defining SPEED field, while SPDHIGH and SPDLOW are left blank. For Synchronous analyses with Frequency Dependent Looping OFF, no speed databoxes are presented, and SPDHIGH, SPDLOW, SPEED are all left blank. Rather, a “param, gyroavg,-1” entry is generated. Frequency Dependent Looping is ON by default.
Chapter 3: Running an Analysis 375 Subcase Parameters
Implicit Nonlinear Subcase Parameters The type of nonlinear analysis can be changed in each SOL 600 or SOL 400 subcase. To specify this change, the Subcases form includes an Analysis Type pull-down menu with options for static, normal modes, buckling, transient dynamic, creep, and body approach analyses. For SOL 400 there is an additional Analysis Type, complex eigenvalue. In turn, specifying the subcase parameters is dependent on the Analysis Type selected for the subcase. The following sections define the subcase parameters for each analysis type.
376
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Static Subcase Parameters for Implicit Nonlinear Solution Type This subform defines the parameters for a SOL 400 or 600 static analysis subcase.
Linearity
Prescribes the nonlinear effects for the subcase.
Nonlinear Solution Parameters • Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Chapter 3: Running an Analysis 377 Subcase Parameters
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase.
Break Squeal Parameters
For defining parameter values for modeling break squeal for the subcase. (SOL 400 only).
Implicit Nonlinear Normal Modes Subcase Parameters This subform defines the parameters for a normal modes analysis subcase (SOL 400 and 600 only). See Normal Modes Subcase Parameters, 364 for more information. Implicit Nonlinear Buckling Subcase Parameters For buckling nonlinear analysis the subcase parameters control the eigenvalue extraction techniques and the range of frequencies to be targeted for extraction. This subform defines the parameters for a buckling analysis subcase (SOL 400 and 600 only). See Normal Modes Subcase Parameters, 364 for more information.
378
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Transient Dynamic Subcase Parameters This subform defines the parameters for a transient dynamic analysis subcase for SOL 600 and SOL 400.
Linearity
Prescribes the nonlinear effects for the subcase.
Nonlinear Solution Parameters • Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Chapter 3: Running an Analysis 379 Subcase Parameters
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase (SOL 600 only).
380
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Creep Subcase Parameters This subform defines the parameters for a SOL 600 and SOL 400 Creep analysis subcase.
Creep Solution Parameters • Procedure
Defines either Explicit creep formulation or Implicit creep formulation.
• Nonlinear Geometric Effects
Defines the type of geometric or material nonlinearity to be included in the subcase.
• Follower Forces
Specifies whether forces will follow displacements.
Increment Type
Defines a fixed or adaptive increment method.
Chapter 3: Running an Analysis 381 Subcase Parameters
• Adaptive Increment Parameters...
For adaptive methods, sets boundaries for incrementation.
Load Increment Parameters
Defines whether the load increments will be fixed or adapted in each iteration and the method by which adaptive load increments will be determined.
Iteration Parameters
Sets forth the iterative procedures that are employed to solve the equilibrium problem at each load increment.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
Active/Deactive Elements
Defines groups of elements to be active or deactive for the subcase (SOL 600 only).
Break Squeal Parameters Implicit Nonlinear Body Approach Subcase Parameters This subform defines the parameters for a SOL 600 body approach analysis subcase
Body Approach Parameters • Total Time
Places a time step option in the Load Step.
• Synchronized
If ON, specifies that when the first rigid body comes into contact, the rest stop moving.
Contact Table
Activates, deactivates, and controls the behavior of contact bodies in the analysis. See Contact Table, 396
382
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Implicit Nonlinear Complex Eigenvalue Subcase Parameters This subform defines the parameters for a SOL 400 (only) complex eigenvalue analysis subcase
Formulation
Select either Direct or Modal.
Enable Rotor Dynamics
Click in checkbox to activate rotor dynamics.
Specify Spinning Properties...
Click to access the form for specifying the rotor speed. See Spinning Properties, Frequency Response, 373
Contact Table...
Activates, deactivates, and controls the behavior of contact bodies in the analysis. See Contact Table, 396
Chapter 3: Running an Analysis 383 Subcase Parameters
Load Increment Parameters Load and time step incrementation parameters for Statics and Transient Dynamics appear on this subordinate form. For other analysis types, this information appears directly on the Solution Parameters form.
The Load Increment Parameters form differs depending on your designation of a Fixed or Adaptive Increment Type and whether an arclength method is to be used if you select an Adaptive Incrementation scheme.
384
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Load Incrementation without Arclength
Static
Transient Dynamic
Increment Type
Adaptive
Arclength Method
None
Trial Time Step Size
Defines the initial time step size. Default is 1% of Total Time if left blank.
Time Step Scale Factor
Indicates load will be allowed to be scaled up by 20% each increment if possible. Default is 1.2.
Minimum Time Step
Indicates the smallest time step that can be used. Default is Trial Time Step / 1000 if left blank.
Maximum Time Step
Indicates the largest time step that can be used. Default is Total Time / 2 if left blank.
Maximum # of Steps
Defines the maximum number of time steps. It can be left blank which will default to the Initial Step Size divided by the Total Time.
Chapter 3: Running an Analysis 385 Subcase Parameters
Total Time
This is the total time of the analysis for a particular step. It defaults to one (1) if left blank for static load cases. For time dependent load cases, the total time is the length of time between distinct time points if left blank. Otherwise the actual value is used (not recommended because it can’t be variable).
# of Steps of Output
Indicates that this many increments evenly spaced in time will be place in the output file. Default is 0 if left blank. Which means all converged increments will be output (SOL 600 only).
Quasi-static Inertial Damping
ON by default.
Criteria
Multiple adaptive load stepping criteria is available. By default, none of this is necessary. These criteria are described below in Adaptive Load Incrementation Criteria, 387.
Time Integration Scheme
For Transient Dynamics, indicates the time integration scheme to use in dynamic analysis.
Minimum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Maximum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Matrix Update Method
This is the method for controlling stiffness updates. This is the KMETHOD field on the NLPARM entry for SOL 400 runs.
Load Increment Parameters for SOL 600 and SOL 400, Creep analysis. The MD Nastran entries used for this are NLADAPT, NLPARM, and TSTEPNL.
386
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Creep
Increment Type
There are three choices, 1) Fixed, 2) Adaptive, and 3) Adaptive Creep.
Suggested Time Increment
The approximate time step.
Total Time
The total time for the creep analysis.
Max # of Increment Allowed
This is for NSMAX.
Creep Tests
This is for RAC.
Relative Strain Tolerance
This is for TCSTRN.
Relative Stress Tolerance
This is for TCSTRS.
Low Stress Cut-off Tolerance
This is for TCOFF.
Chapter 3: Running an Analysis 387 Subcase Parameters
Adaptive Load Incrementation Criteria
This for the MD Nastran NLAUTO entry, Parameters for Automatic Load/Time Stepping. (SOL 600 only). Adaptive Criteria
Description
Treat Criteria as:
If Limits, sets 3rd field to zero (0) in 3rd data block (default). If Targets, sets field to one (1). This is for LIMITAR.
Use Automatic Criteria Continue if not Satisfied
Uses automatic physical criteria if top toggle is ON. Bottom toggle defines what happens if the criteria is not met. Both OFF by default. This is for IPHYS.
388
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Criteria
Description
Ratio Between Steps:
Defines the [Smallest] and [Largest] ratios acceptable between load increments. For Smallest, default = 0.1, For Largest, default=10.0. This is for RSMALL and RBIG.
[Number of Cutbacks]
Blank by default. default value is 10 if left blank or zero. This is for NCUT.
Increment Criteria
Selects the type of criteria to be used.The labels “XXX Range” and “XXX Increment Allowed” will change based on the Increment Criteria selected. This is for CRITERIA.
Loading Table Instances
Determines how loading tables (Use Tables must be ON in the Job Parameters form) are treated. By default loads are increased or decreased such that they always Reach Peaks-Valleys Only. If you wish you can Reach All Points in Tables or Ignore all Points in Tables.
Write Instances to Post File
Writes Loading Table Instances to the Post file if toggle is ON. Note that if toggle is ON, then only those instances are written to the POST file and not all the increments of the analysis. This is for IDMPFLG.
Nodal Temp. Check
There are three choices, 1) Omit Check, 2) Below Finish Temperature (to complete time period when all node temperatures are < FTEMP), and 3) Above Finish Temperature (to complete time period when all node temperatures are > FTEMP). This is for IFINISH.
Finish Temperature
The terminal temperature. This is for FTEMP.
Use Criterion
For a criteria to be used, this toggle must be turned ON.
“Criterion” Range
The first and last fields are zero and 1e20 respectively and cannot change. The second and third must be the same as well as the 4th/5th and 6th/7th which define the ranges. The “Criterion” title changes according to the Increment Criterion chosen.
“Criterion” Increment Allowed
The “Criterion” title changes according to the Increment Criteria chosen.
Select a Group (Optional)
You can optionally select a group of elements to which this criterion is to be applied. No group is selected by default.
Chapter 3: Running an Analysis 389 Subcase Parameters
Adaptive Load Incrementation with Arclength (SOL 600 only) Static
Adaptive Increment Parameter
Description
Arclength Method
Selects the arclength root procedure: Crisfield, Riks/Ramm, Modified Riks/Ramm, or Crisfield-Modified Riks/Ramm. The default is Modified Riks/Ram. If None is selected the form updates as shown (p. 383). For Transient Dynamics, this is the only option available for adaptive load incrementation.
Automatic Cutback
This feature is ON by default. If an increment does not converge, a restart from the last increment cuts the increment size in half.
Number of Cutbacks
This is associated with Automatic Cutback. This parameter determines how many times a cutback is allowed.
390
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Adaptive Increment Parameter
Description
Initial Fraction of Load Applied to 1st Increment
This is the fraction of the total load that should be applied in the first iteration of the first increment.
Max. Fraction of Load Applied in Any Increment
This is the maximum fraction of the load that can be applied in any increment.
Max/Min Ratio Arc Length / Initial Arc Length
Used to define the minimal arclength. The default is 0.01.
Max. # of Increments
Defines the maximum number of increments. Program will end if this value is exceeded.
Total Time
This is the total time of the analysis for a particular step. It defaults to one (1) if left blank for static load cases. For time dependent load cases, the total time is the length of time between distinct time points if left blank. Otherwise the actual value is used (not recommended because it can’t be variable). Fixed Load Incrementation
Static
Transient Dynamic
Chapter 3: Running an Analysis 391 Subcase Parameters
Fixed Increment Parameter
Description
Automatic Cutback
Applies to Nonlinear Statics only. It is ON by default. If an increment does not converge, it allows for a restart from the last increment cuts the increment size in half.
Number of Cutbacks
This is associated with Automatic Cutback. This parameter determines how many times a cutback is allowed.
Number of Increments or Number of Steps
For Statics and Creep this is the number of increments specified in the NLAUTO option. Or for Transient Dynamics defines the number of steps to use throughout the analysis for Fixed time step type. Default is 10.
Total Time
For Statics, this enters the NLAUTO option which is the total time as defined in this widget. For Transient Dynamics this is the total time. For Creep, the total time is either placed in the 2nd data block of a CREEP INCREMENT option or the total time is divided by the Number of Increments, if this value is present, and the incremental time is written to the 2nd data block of the CREEP option.
Gamma / Beta
For Transient Dynamics only. Default is 0.5.
Time Integration Scheme
For Transient Dynamics, the Houbolt and Central Difference cannot be selected. Indicates the time integration scheme to use in dynamic analysis.Single Step Houbolt is the default.
Minimum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Maximum Iteration per Increment
Enter these values for a SOL 400 run. For SOL 600 these values are defined on the Iteration Parameters, 391 form.
Matrix Update Method
This is the method for controlling stiffness updates. This is the KMETHOD field on the NLPARM entry for SOL 400 runs.
Iteration Parameters This subordinate form appears when the Subcase Parameters... / Iteration Parameters... button is selected for Analysis Type: Static, Transient Dynamics, Creep, ... Subcases form. Unless otherwise specified all
392
Patran Interface to MD Nastran Preference Guide Subcase Parameters
parameter references apply to the NLSTRAT (SOL600) entry for the form on the left, and NLPARM (SOL 400) entry for the form on the right .
SOL 600 Iteration Parameter
Description
Proceed if not Converged
Forces the analysis to proceed even if the increment did not converge.
Initial Stress Stiffness
There are five choices, 1) Full, 2) None, 3) Tensile, 4) Deviatoric, and 5) Begin Increment.
Non-positive Definite
This forces the non-positive definite flag (IKNONPOS param) ON in the NLSTRAT option. A new NLSTRAT option is written for each step if a change in this flag has been detected from Subcase to Subcase.
Chapter 3: Running an Analysis 393 Subcase Parameters
SOL 600 Iteration Parameter
Description
Iteration Method
Indicates the iteration method (IKMETH param) to be used. This is can be set to Full Newton-Raphson, Modified Newton-Raphson, NewtonRaphson with Strain Correction, or Secant Method. Full Newton-Raphson is default.
Max # of Iterations per Increment
Defines the maximum number of iterations (MAXREC param) allowed for convergence in any increment. This number is negative if Proceed if not Converged is ON from the Solution Parameter form.
Minimum # of Iterations
This specifies the minimum number of iterations per Increment (MINREC param) option. It can be an integer number zero or greater. If this is set greater than zero, every increment will perform at least this many iterations.
per Increment Desired # of Iterations per Increment
Defines the number of desired iterations in an increment (ATRECYC param) which is placed on the NLSTRAT option. If the actual number of iterations is less than this value, this will be used to figure out how much to increase the load step for the next increment. In a similar manner if the actual number of iterations is greater than this number (but less than the Max # of Iterations per Increment, this will be used to decrease the load step in the next increment. Obviously if Adaptive incrementation is not specified, this data will not be used.
Matrix Update Method
There are six choices for updating the stiffness matrix, 1) Automatic (MD Nastran automatically selects the most efficient strategy based on convergence rates), 2) Controlled Iters.(MD Nastran updates the matrix at every KSTEP interations and at convergence if KSTEP <= MAXITER), 3) Adaptive, 4) Semi-Automatic (MD Nastran for each load increment (i) performs a single iteration based upon the new/next load, (ii) updates the stiffness matrix, and (iii) resumes the normal Automatic option), 5) Full Newton (MD Nastran updates the stiffness matrix every iteration), and 6) Pure Full Newton (the same as the Full Newton method, except EPSU = 0.01, EPSW = -0.01, and MAXLS = 0.0).
Tolerance Method
Defines the tolerance method to be used (CONVTYP param). This can be set to Residual, Incremental Displacement, or Incremental Strain Energy.
Residuals/Displacements
If you want the Tolerance Method to use both Residuals and Displacements to determine convergence set this to And. If you want either one or the other to determine convergence, set this to OR. If Tolerance Method is set to Residual or Displacement, then these two toggles are enabled. Both are OFF by default. If one is ON, the other is OFF. These toggles work in combination with Tolerance Method. If both are OFF, then Tolerance Method determines what is written.
And Or
Error Type
Indicates the type of error to use (IRELABS param). This can be set to Relative or Absolute or Both.
394
Patran Interface to MD Nastran Preference Guide Subcase Parameters
SOL 600 Iteration Parameter
Description
Automatic Switching
This controls automatic switching (the AUTOSW param on the NLSTRAT option) between Residuals and Displacement tolerances if one or the other fails to converge.
Residual Tolerances
Values and labels in this frame depend on the Tolerance Method and Error Type setting and are discussed below.
Relative Residual Force
The value of this widget (default is 0.1 on force) is written to the RCKI param.
Relative Displacement Relative Energy Relative Residual Moment Relative Rotation Minimum Reaction Force Minimum Displacement Minimum Reaction Moment Minimum Rotation Maximum Residual Force Maximum Displacement Maximum Residual Moment Maximum Rotation
SOL 400 Iteration Parameter
The value of these widgets (default is blank) is written to the appropriate MAXxx or MINxx param.
Description
Min # of Iterations per Increment
Specify the fewest number of iterations per load increment.
Max # of Iterations per Increment
Specify the largest number of iterations per load increment.
Number of Iterations per Update
Specify the allowable number of iterations per stiffness matrix update, (KSTEP).
Matrix Update Method
There are six choices for updating the stiffness matrix, 1) Automatic (MD Nastran automatically selects the most efficient strategy based on convergence rates), 2) Controlled Iters.(MD Nastran updates the matrix at every KSTEP interations and at convergence if KSTEP <= MAXITER), 3) Adaptive, 4) Semi-Automatic (MD Nastran for each load increment (i) performs a single iteration based upon the new/next load, (ii) updates the stiffness matrix, and (iii) resumes the normal Automatic option), 5) Full Newton (MD Nastran updates the stiffness matrix every iteration), and 6) Pure Full Newton (the same as the Full Newton method, except EPSU = 0.01, EPSW = -0.01, and MAXLS = 0.0).
Automatic Switching
If selected, automatically switch to an appropriate convergence checking flag if an unappropriated flag is selected.
Chapter 3: Running an Analysis 395 Subcase Parameters
SOL 400 Iteration Parameter
Description
Displacement Error Load Error Work Error Vector Componet Method Length Method
If any of these toggles are ON, then the appropriate CONV=U, P, W, V, or N is written to the NLPARM entry to activate the repective convergence criteria.
Displacement Tolerance Load Tolerance Work Tolerance
Specifies the tolerance value if the above corresponding toggles are activated. This is written in the EPSU, EPSP, and EPSW fields of the NLPARM entry. Leave blank for default values.
Maximum # of Divergence Conditions Specifies the MAXDIV, MAXQN, MAXLS, FSTRESS, LSTOL, MAXBLS, and RTOLB fields of the NLPARM entry. It is recommended Maximum # of Correction Vectors to use the default values. Please consult the MD Nastran Quick Reference Guide for more information. Maximum # of Line Searches Fraction of Effective Stress Line Search Tolerance Maximum # of Bisections Maximum Incremental Rotations
396
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Contact Table A contact table is used to control the behavior of and to activate or deactivate, or in some cases, remove contact bodies from the analysis. This is used for both linear and nonlinear contact.
Chapter 3: Running an Analysis 397 Subcase Parameters
. Input
Description
Global Contact Detection
• Changing this setting should be done with caution as it will over-write any contact
detection changes made to individual contact pairs in the cells. This option sets the contact detection method in all cells in the contact table. • Default (by body #) -This is the default where contact is checked in the order the
bodies are written to the input file which is the order in which they are created. In this scenario, the most finely meshed bodies should be listed first. There will be contact checks first for nodes of the first body with respect to the second body and then for nodes of the second body with respect to the first body. If Single Sided contact is activated on the Contact Parameters subform, then only the first check is done. • Automatic -Unlike the default, the contact detection is automatically determined
and is not dependent on the order they are listed but determined by the solver ordering the bodies starting with those having the smallest edge length. Then there will be only a check on contact for nodes of the first body with respect to the second body and not the other way around. • First ->Second - Blanks the lower triangular section of the table matrix such that
no input can be accepted. Only the contact bodies from the upper portion are written, which forces the contact check of the first body (the one higher in the contact table) with respect to the second body. • Second-> First - Blanks the upper triangular section of the table matrix such that
no input can be accepted. Only the contact bodies from the lower portion are written. Contact detection is done opposite of First->Second. • Double-Sided -Writes both upper and lower portions of the table matrix. This
overrules the Single Sided contact parameter set on the Contact Parameters subform. Touch All
Places a T to indicate touching status for all deformable-deformable or rigiddeformable bodies.
Glue All
Places a G to indicate glued status for all deformable-deformable or rigid-deformable bodies.
Deactivate All
Blanks the spreadsheet cells.
Import/Export
Import or Export a file with contact matrix definition data. The format must be CSV.
Select Existing
Select an existing Contact Table from a set of tables.
Contact Matrix
A matrix defining what and how contact bodies contact.
Body Type
Lists the body type for each body; either Deformable or Rigid.
Release
This cell can be toggled for each body to Y or N (Yes or No). If Y, this indicates that the particular contact body is to be removed from this Subcase. The forces associated with this body can be removed immediately in the first increment or gradually over the time of the entire Subcase with the Force Removal switch described below.
398
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Input
Description
The Contact Matrix entries
The rows correspond to Touching Body. The columns correspond to Touched Body. An entry of the matrix, for example (Row i,Column j), will have the entry of T, G, or “blank”. T = touching, G = glue, “blank” = no contact. To change a matrix cell entry, select the cell (click once) to select it, then click on the cell once to change to the next selection. For example, T -> G.
Touching Body Touched Body
These are informational or convenience list boxes to allow you to see which bodies an active cell references and to see what settings are active for Distance Tolerance and other related parameters below. You must click on the touched/touching bodies to see what values, if any, have been set for the pair combination.
Distance Tolerance
Set the Distance Tolerance for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Distance Tolerance.
Bias Factor
Bias the domain defined by the distance tolerance.
Analysis Properties
Select Structural.
Separation Threshold
Specify a threshold (force or stress) such that if the contact load (force or stress) is < this threshold value, the contacting body remains in contact with the contacted body.
Separation Force
Set the Separation Force for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Separation Force.
Friction Coefficient
Set the Friction Coefficient for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Friction Coefficient.
Interference Closure
Set the Interference Closure for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Interference Closure.
Friction Stress Limit
This is a bound on the maximum friction stress. This is the friction stress limit for the bilinear model, t limit . If the shear stress reaches the limit value, the applied friction force is reduced so that the maximum shear stress is given by min n limit . t
Slide Off Distance
Specify the distance a node must slide off a surface, at an edge, before the node travels on the surface, at the edge, that is at an angle to the surface that is being slid off of.
Chapter 3: Running an Analysis 399 Subcase Parameters
Input
Description
Heat Transfer Coefficient
Set the Heat Transfer Coefficient for this pair of contact bodies. You must press the Enter or Return key to accept the data in this data box. A nonspatial field can be referenced that will write this data in TABLE format, if this parameter varies with time, temperature, or some other independent variable. This overrides any other settings for Heat Transfer Coefficient. This is only used in Coupled analysis (Heat transfer and Coupled analysis not supported in MSC.Nastran 2004.
Force Removal
Select 1) Immediate, or 2) Gradual. This is activated when a body is is set to Release. For example, 1-seal can be set to Release by clicking once on the corresponding Release cell, then clicking once again to change from N to Y. The MD Nastran entry BCMOVE is written to the .bdf file.
Contact Detection
Select 1) Automatic, 2) Double Sided, 3) 1st->2nd, or 4) 2nd->1st.
Retain Gaps/Overlaps
This is only applicable for the Glued option. Any initial gap or overlap between the node and the contacted body will not be removed (otherwise the node is projected onto the body which is the default). For deformable-deformable contact only.
Stress-free Initial Contact
This is only applicable for initial contact in increment zero, where coordinates of nodes in contact can be adapted such that they cause stress-free initial contact. This is important if, due to inaccuracies during mesh generation, there is a small gap/overlap between a node and the contacted element edge/face. For deformable-deformable contact only.
Delayed Slide Off
By default, at sharp corners, a node will slide off a contacted segment as soon as it passes the corner by a distance greater than the contact error tolerance. This extends this tangential tolerance. For deformable-deformable contact only.
Allow Separation Breaking Glue Parameters...
See Breaking Glue Parameters Subform, 400
Edge Contact...
See Edge Contact Subform, 401
400
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Breaking Glue Parameters Subform Un-gluing (breaking) a glued contact can be done by specifying the Breaking Glue Parameter values in the following form:
This form can only be used when there is glued contact (there is G in the Contact Table matrix cells). . Input
Description
Max Normal Stress
The maximum normal stress that will cause the glued contact to become un-glued.
Max Tangential Stress
The maximum tangential stress that will cause the glued contact to become un-glued.
First Exponent
The exponent of the tangential stress term (BGM) in the following equation: sigman -------------------- BGSN
Second Exponent
BGN
sigmat BGM + ------------------ 1.0 BGST
The exponent of the normal stress term (BGN) in the following equation: sigman -------------------- BGSN
BGN
sigmat BGM + ------------------ 1.0 BGST
Chapter 3: Running an Analysis 401 Subcase Parameters
Edge Contact Subform :
. Input
Description
Include Outside (Solid Element)
When detecting contact of solid elements (for example, CHEXA elements) use this to include contact of the outside of the elements.For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Include Outside of Rigid Surface
When detecting contact of rigid surfaces use this to include contact of the outside of the rigid surfaces. For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Check Layers
For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
402
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Input
Description
Ignore Thickness
Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Include Edges
Use this to detect contact of edges. There are three options, Beam/Bar, Free and Hard Shell, or Both. For details refer to the BCTABLE entry (defines contact table) of the MD Nastran QRG. The entries that are used for the BCTABLE entry are COPTM and COPTS. These flags indicate how master and slave surfaces may contact.
Active/Deactive Elements Defines groups of elements to be active or deactive for the subcase.
Active/Deactive Group
Description
Group of Element to Deactivate
Lists all groups. Elements in the selected group will be deactivated.
Group of Elements to Activate
Lists all groups. Elements in the selected group will be activated.
Chapter 3: Running an Analysis 403 Subcase Parameters
Break Squeal Parameters Defines parameter values for modeling break squeal. (SOL 400 only).
Active/Deactive Group
Description
Enable Break Squeal
The form is activated when this checkbox is selected.
Load Factor
Defines the load factor for which the break squeal analysis is to be performed.
Average Stiffness
Approximate average stiffness per unit area between the break pads and disk. This parameter is used as a penalty contact stiffness for break squeal. It needs to be a large value, but not so large that numerical instabilities result. If this parameter is large eneough, increasing it by a few orders of magnitude will not appreciably affect the squeal modes.
Break Squeal Only
This is used to specify whether or not the nonlinear analysis will be continued after the break squeal event. If this is selected, the nonlinear iterations will cease immediatly after the event, otherwise the nonlinear iterations will be continued.
404
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Active/Deactive Group
Description
Axis of Rotation Vector
This is a vector of direction cosines, <X-dir cosine, Y-dir cosine, Z-dir cosine>, where this is for the axis of rotation, and the directions are in the basic coordinate system.
Point on Axis of Rotation
These are the coordinates of a point on the axis of rotation, [X,Y,Z]. The coordinates are in the basic coordinate system.
Solvers/Options In general, this form is used to select the Nastran solver and other possible options. An SMETHOD case control entry is written specifying the solver type to use and possibly an ITER bulk data entry for additional options. Only certain solutions allow the use of the SMETHOD case control as controlled by
Chapter 3: Running an Analysis 405 Subcase Parameters
the user interface. If a solution does not support a solver option, that option is not presented in the form or menus.
Solver Type
Description
Nastran Default
No SMETHOD or ITER entries are written. Nastran uses whatever solver is the default for the solution being used.
Iterative ElementBased (CASI)
An SMETHOD case control with the entry ELEMENT is used which invokes the iterative CASI (element-based) solver using all defaults. This is only available for SOL 101 and 400 and is generally used with large solid models. Certain restrictions apply and you should consult the Nastran Quick Reference Guide regarding the usage of this solver.
Iterative Matrix-Based
An SMETHOD case control with the entry MATRIX is used to invoke the matrix-based iterative solver using all defaults.
Iterative (Customized)
An SMETHOD case control referencing the ID of an ITER bulk data entry is written to the input deck. The ITER entry invokes the solver options. Those options are described in the table below.
406
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Iterative Option
Description
Preconditioner
Five preconditioners are available: Jacobi, Cholesky, Jacobi/Cholesky, and CASI. The CASI is the element-based iterative solver. See the table above. All other preconditioners are the matrix-based iterative solver. Various options are allowed for each as controlled by the user interface. See the entries below. To use a default preconditioner based on the solution type, set this to Analysis Default. Consult the Nastran Quick Reference Guide for more details as to which defaults are used for each solution type.
Maximum Number of Iterations
Leave this blank to accept the default. Otherwise specify the maximum number of iterations allowed.
Diagonal Scaling
The Jacobi and Cholesky preconditioners allow diagonal scaling.
Reduced
Turn this toggle on to invoke the reduced incomplete Cholesky preconditioner as opposed to just the incomplete Cholesky. This can be combined with or without diagonal scaling.
Block
Turn this toggle on to invoke the block incomplete Cholesky preconditioner. You must specify real or complex also.
Real / Complex
This is only used for the block incomplete Cholesky preconditioner.
p-version
For p-element analysis, you can turn this toggle on to invoke the Jacobi, Cholesky or combined Cholesky/Jacobi preconditioner. This cannot be combined with any other options.
Padding
Specify the padding value for reduced incomplete Cholesky with any of its options. Leave this blank to specify the defaults. Each option has its own default, therefore it is recommended that you leave this blank.
Extraction
Specify the extraction level for reduced or block incomplete Cholesky preconditioner. The default is zero.
Geometric Progression Turn this toggle on if you wish to use geometric progression convergence criterion. Epsilon
This is a user-given convergence parameter. Default is 1e-6. If present, the solver will use additional external convergence criterion. See the Nastran Quick Reference Guide for more details. Blank this field out if only the internal convergence criterion is required.
Print Messages for each Iteration
Off by default. Turn ON if you want more diagnostics for each iteration. Otherwise only minimal messaging is given.
Terminate Early (Resource Estimate Only)
Turn this toggle ON if you want the run to terminate with only a resource estimation.
Chapter 3: Running an Analysis 407 Subcase Parameters
DDAM Subcase Parameters This subform defines the parameters for a SOL 187 DDAM analysis subcase
408
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Spectrum Source
Select File for a user-defined spectrum, or Coef for a DDAM style coefficient equation. If you select File, a button appears to the right to let you select the file where the spectrum is defined. If you select Coef, two other buttons appear:
Coef Source
Select File for a user-written coefficient file, or Default to use the coefficients built into the Fortran program. Note that the built-in coefficients we deliver in the program are NOT the DDS-072 coefficients. If you use this option for a real DDAM analysis, the Fortran file must be edited and recompiled. If you select File, a button appears to the right to let you choose the file where the coefficient data is stored.
F(x) Type
Choices are NRL 1396 and DDS 072. This option toggles between the old NRL 1396 style equations, and the current DDS-072 style equations used for DDAM.
Coefficient Options • Ship Type
Select Surface or Submerged
• Mount Location
Choice of Deck, Hull, or Shell.
• Elastic/Plastic
Select Elastic or Plastic. Choosing Plastic uses the Elastic/Plastic coefficients; Elastic uses the elastic coefficients.
Weight Cutoff
Default uses the default value compiled into the PCL code, which is 80%. If you choose Enter Value the text box becomes available and you can enter a percentage manually. The number entered is the percentage, not the fraction, so 100% of the modal mass is entered as 100.
Minimum G Level
If you select N/A, no minimum G value is used. If you enter a value, all modal accelerations below the minimum are set to the minimum.
Fore/Aft Axis
It is necessary to have the model oriented orthogonal to a global cartesian axis system, although not necessarily in one particular orientation. This toggle identifies which global axis is to be interpreted as Fore/Aft.
Vertical Axis
This identifies the axis that is in the vertical direction.
Modal Analysis • Number of Desired Roots • Lower • Upper
These are the limits that control the eigenvalue analysis and are the values from the Nastran EIGRL entry. ND is the number of desired roots, V1 is the lower frequency limit, V2 is the upper frequency limit. For the effects of using one of more of these, see the EIGRL section of the MD Nastran Quick Reference Guide.
Chapter 3: Running an Analysis 409 Subcase Parameters
Explicit Nonlinear Subcase Parameters This subordinate form appears when the Subcase Parameters button is selected on the Subcases form when the solution type is Explicit Nonlinear. All of the data is part of the TSTEPNL Bulk Data entry
Defines TSTEPNL. Similar to SOL 129, Nonlinear Transient
Defines BCTABLE. Similar to SOL 600 Implicit Nonlinear
Contact Table...
Activates, deactivates, and controls the behavior of contact bodies in the analysis.
410
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Selects the highest and lowest natural frequenc values to be extracted
Selects which Degrees of Freedom are used to determine the peaks Selects the output interval of accelerations, velocities, or displacements of the eigenvalues
The “Type of Response” menu specifies whether Acceleration, Velocity, or Displacement response will be used to select the modes.
Selects which Degrees of Freedom to be in the eigenvectors (3 for translations only, 6 for translations and rotations
The “Method of Normalization” menu specifies the method used to normalize the eigenvectors
Chapter 3: Running an Analysis 411 Subcase Parameters
Contact Table A contact table is used to control the behavior of contact bodies and to activate or deactivate, or in some cases, remove contact bodies from the analysis. This form defines the BCTABLE entry.
Additional Data...
Additional Contact Data for Explicit Nonlinear.
412
Patran Interface to MD Nastran Preference Guide Subcase Parameters
Additional Contact Data This subordinate form defines additional contact data for Explicit Nonlinear.
Chapter 3: Running an Analysis 413 Subcase Parameters
Adaptive Mesh Post-Processing Support has been added for adaptive mesh post-processing for airbag analysis. Below is an adapted mesh model as read in from the DBALL file and stored using offset ID’s in separate groups. The user can then select one or more time increments from the Quick Plot Results menu for postprocessing. The Quick Plot algorithm pulls up the mesh associated with the increment(s) selected for post-processing. Using this method a user can do a pseudo-animation to show the progression of the analysis. The model is loaded by a cylindrical rigid pin with a 200 lb load at the center.
Additional Information The following is also now supported for SOL 700 jobs: • Additional Properties • PBEAM71 • BPEAMD • PBELTD • PELAS1 • PLPLANE • PLSOLID • PSHELL1 • PSHELLD • PSPRMA
414
Patran Interface to MD Nastran Preference Guide Subcase Parameters
• GUI for time domain NVH • Many additional materials
Chapter 3: Running an Analysis 415 Output Requests
3.9
Output Requests This allows the definition of what data is desired from the analysis code in the form of results. For most solution sequences, the form consists of two formats: Basic and Advanced. The Basic form retains the simplicity of being able to specify the output requests over the entire model and uses the default settings of MD Nastran Case Control commands. There is a special set defined in Patran called ALL FEM. This set represents all nodes and elements associated with Object defined on the Analysis Form, 261. This default set is used for all output requests in the Basic Output Requests, 416 form. The Advanced version of this form allows the user to vary these default options. Since output requests have to be appropriate to the type of analysis, the form changes depending on the solution sequence. The Advanced Output Requests, 417 also adds the capability of being able to associate a given output request to a subset of the model using Patran groups. This capability can be used effectively in significantly reducing the results that are created for a model, optimizing the sizes and translation times of output files. The creation of Patran groups are documented in Group>Create (p. 263) in the Patran Reference Manual. The results types that will be brought into Patran due to any of these requests, are documented in Supported OUTPUT2 Result and Model Quantities, 502. In that chapter, tables are presented that correlate the MD Nastran results block, and the Patran primary and secondary results labels with the various output requests. Note:
Many of the output requests that can be defined on the Output Request forms currently apply only to the printed values in the MD Nastran output file; these result quantities cannot be imported and postprocessed in Patran. For guidance on specific quantities, review Supported OUTPUT2 Result and Model Quantities, 502.
MD Nastran Implicit Nonlinear (SOL 600) produces stress and strain results that differ from those results available with other solution sequences. A detailed discussion of the stress and strain measures for SOL 600 is given in Stress and Strain Measures for Nonlinear Analysis (Ch. 2) in the MSC.Nastran Implicit Nonlinear (SOL 600) User’s Guide.
416
Patran Interface to MD Nastran Preference Guide Output Requests
Basic Output Requests This form is used to select output requests with their default options. The set is always All FEM, which means results for all nodes or elements in the model. A default set of output requests is always preselected.
The available output requests depend on the active Solution Sequence as indicated by this value.
This option menu is used to switch between the advanced and basic versions of this form.
This listbox displays the appropriate result types that may be selected for the solution sequence indicated at the top of the form. The output requests are selected one at a time by clicking. This listbox displays the selected output requests for the subcase shown at the top of the form. The Delete button deletes the output request highlighted in the Output Requests listbox. The TITLE, SUBTITLE and LABEL are written to the MD Nastran output file.
Note:
The OK button accepts the output requests and closes the form. The Defaults button deletes all output requests and replaces them with defaults. The Cancel button closes the form without saving the output requests.
Chapter 3: Running an Analysis 417 Output Requests
Advanced Output Requests This form provides great flexibility in creating output requests. Output requests may be associated with different groups (SET options in MD Nastran) as well as different superelements1. The output requests available depend on the chosen Solution Types, 271, Solution Parameters, 277, and Translation Parameters, 265 . The Advanced Output Requests form is sensitive to the Result Type selected. The Form Type, Delete, OK, Defaults, and Cancel buttons operate exactly like on the Basic Output Requests, 416 form. A description of the output requests and their associated options are listed in Table 3-1 and Table 3-2.
1At the present time, superelement specifications are allowed only in the structured linear static solution
type (Solution Sequence 101).
418
Patran Interface to MD Nastran Preference Guide Output Requests
Use this listbox to select the result type to be created.
This listbox is used to select the group to which the output requests relate.
This databox appears for SOL 101 and 103 when the model contains p-elements. Other options will be presented, such as Percent of Step Output and Intermediate Output Options depending on conditions listed in Table 3-2.
Use this list box to select output requests that are to be modified or deleted.
These are the options that are appropriate to the highlighted result type. They also indicate the options that were selected for a highlighted output request. See Table 3-1.
Chapter 3: Running an Analysis 419 Output Requests
Table 3-1
Output Request Descriptions
Output Request
Case Control Command or Bulk Data Entry
Description
Acoustic Intensity
INTENSITY
Requests acoustic intensity for external acoustics analysis (frequency response).
Acoustic Power
ACPOWER
Requests acoustic power radiated from surface for external acoustics analysis (frequency response).
Acoustic Field Point Mesh
ACFPMRESULT
Requests acoustic field point mesh results for external acoustics analysis (frequency response). You are given a list of all acoustic field point meshes defined and groups with nodes. Each one selected is translated into its own BEGIN AFPM section in the bulk data.
Acoustic Velocities
VELOCITY
Requests nodal velocities. This is for acoustic velocities at the node points of Field Point Mesh.
Displacements
DISPLACEMENT
Requests nodal displacements.
Eigenvectors
VECTOR
Requests nodal eigenvectors.
Element Stresses
STRESS
Requests elemental stresses.
Constraint Forces
SPCFORCES
Requests forces of single- point constraints.
MultiPoint Constraint Forces
MPCFORCES
Requests forces of multipoint constraints (for versions 68 or higher).
Element Forces
FORCE
Requests elemental forces.
Applied Loads
OLOAD
Requests equivalent nodal applied loads.
Nonlinear Applied Loads
NLLOAD
Requests equivalent nonlinear applied loads. Sorting and format options are not allowed with this request.
Element Strain Energies
ESE
Requests elemental strain energies and energy densities. No options are allowed with this output request.
Element Strains
STRAIN
Requests elemental strains.
Grid Point Stresses
GPSTRESS
Requests stresses at grid points.
Velocities
VELOCITY
Requests nodal velocities.
420
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-1
Output Request Descriptions (continued) Case Control Command or Bulk Data Entry
Description
ACCELERATION
Requests nodal accelerations.
Grid Point Force Balance
GPFORCE
Requests grid point force balance at nodes. Sorting and format options are not allowed with this request.
Grid Point Stress Discontinuities
GPSDCON
Requests mesh stress discontinuities based on grid point stresses.
Element Stress Discontinuity
ELSDCON
Requests mesh stress discontinuities based on element stresses.
Nonlinear Stress
NLSTRESS
Requests the form and type of nonlinear element stress output.
Contact Results
BOUTPUT
Requests contact regions for output.
Output Request Accelerations
Table 3-2
Options Sorting
Output Request Form Options
Label By Node/
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
SORT1
Elements
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/ SORT2
Elements
No
Output is presented as tabular listing of frequency or time for each node or element.
Element
Time Format
Tensor
Descriptions
Rectangular
REAL
Elements
No
Requests real and imaginary format for complex output.
Polar
PHASE
Elements
No
Requests magnitude and phase format for complex output.
Von Mises
VONMISES
Elements
No
Requests von Mises stresses or strains.
Maximum Shear
MAXS
Elements
No
Requests Maximum shear or Octahedral stresses or strains.
Chapter 3: Running an Analysis 421 Output Requests
Table 3-2
Options Element Points
Composite Plate Options
Output Request Form Options (continued)
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Cubic
CUBIC
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach with cubic bending correction.
Corner
CORNER
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center.
Center
CENTER
Elements
No
Requests QUAD4 stresses or strains at the center only.
Strain Gage
SGAGE
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using the strain gage approach.
Bilinear
BILIN
Elements
No
Requests QUAD4 stresses or strains at the corner grid points as well as the center using bilinear extrapolation.
Element Stresses
NOCOMPS= -1, LSTRN = 0 in Bulk Data
Elements: Surfaces
No
Composite element ply stresses and failure indices are suppressed. Element stresses for the equivalent homogeneous element are output.
Ply Stresses
NOCOMPS=1,LS Elements: TRN = 0 in Bulk Surfaces Data
No
Composite element ply stresses and failure indices are output. Model should contain PCOMP entry defining composites.
422
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued) Case Control or Bulk Data Options
Options
Label
Composite Plate Options
Ply Strains
NOCOMPS=1,LS Elements: TRN = 1 in Bulk Surfaces Data
No
Composite element ply strains and failure indices are output. Model should contain PCOMP entry defining composites.
Ply Element Stresses
NOCOMPS=0,LS Elements: TRN=0 in Bulk Surfaces Data
No
Composite element ply stresses and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Element and Ply Strains
NOCOMPS=0,LS Elements: TRN=1 in Bulk Surfaces Data
No
Composite element ply strains and failure indices as well as Element stresses for the equivalent homogeneous element are output. Model should contain PCOMP entry defining composites.
Plane Curv.
STRCUR
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains and curvatures are output at the reference plane for plate elements.
Fiber
FIBER
Elements: Surfaces
No
This option is available for Element Strains output requests only. Strains at locations Z1 and Z2 (specified under element properties) are output at the reference plane for plate elements.
By Node /Element
SORT1
Nodes
No
Output is presented as tabular listing of nodes/elements for each load, frequency, eigenvalue, or time.
By Frequency/ Time
SORT2
Nodes
No
Output is presented as tabular listing of frequency or time for each node or element.
Rectangular
REAL
Nodes
No
Requests real and imaginary format for complex output.
Polar
PHASE
Nodes
No
Requests magnitude and phase format for complex output.
Plate Strain Options
Sorting
Format
Groups
Multiple Select Allowed
Descriptions
Chapter 3: Running an Analysis 423 Output Requests
Table 3-2
Output Request Form Options (continued)
Options
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Yes
Selects the output coordinate frame for grid point stress output. Coord 0 is the basic coordinate frame.
Elements: Volumes
Yes
Requests direct stress, principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
PRINCIPAL
Elements: Volumes
Yes
Requests principal stresses, direction cosines, mean pressure stress and von Mises equivalent stresses to be output.
Direct
DIRECT
Elements: Volumes
Yes
Requests direct stress, mean pressure stress and von Mises equivalent stresses to be output.
Fiber
All
FIBER, ALL
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at all fibre locations, that is at Z1, Z2 and the reference plane. Z1 and Z2 distances are specified as element properties (default Z1=-thickness/2, Z2= +thickness/2).
Fiber
Mid
FIBER, MID
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at the reference plane.
Z1
FIBER, Z1
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z1 from the reference plane (default Z1=thickness/2).
Z2
FIBER, Z2
Elements: Surfaces
Yes
Specifies that grid point stresses will be output at distance Z2 from the reference plane (default Z2=+thickness/2).
Output Coordinate
Coord
COORD CID
Volume Output
Both
Blank
Principal
Elements: Surfaces, Volumes
424
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued)
Options Normal
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
X1
NORMAL X1
Elements: Surfaces,
Yes
Specifies the x-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X2
NORMAL X2
Elements: Surfaces
Yes
Specifies the y-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
X3
NORMAL X3
Elements: Surfaces
Yes
Specifies the z-axis of the output coordinate frame to be the reference direction for the positive fiber and shear stress output.
Topological
TOPOLOGI-CAL Elements: Surfaces
Yes
Specifies the topological method for calculating average grid point stresses. This is the default.
Geometric
GEOMETRIC
Elements: Surfaces
Yes
Specifies the geometric interpolation method for calculating average grid point stresses. This method should be used when there are large differences in slope between adjacent elements.
X-axis of Basic Coord
X1
AXIS, X1
Elements: Surfaces
Yes
Specifies that the x-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X-axis of Basic Coord
X2
AXIS, X2
Elements: Surfaces
Yes
Specifies that the y-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
X3
AXIS, X3
Elements: Surfaces
Yes
Specifies that the z-axis of the output coordinate frame should be used as the x-output axis and the local x-axis when geometric interpolation method is used.
Method
Chapter 3: Running an Analysis 425 Output Requests
Table 3-2
Output Request Form Options (continued)
Options Branch
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Break
BREAK
Elements: Surfaces
Yes
Treats multiple element intersections as stress discontinuities in the geometric interpolation method.
No Break
NOBREAK
Elements: Surfaces
Yes
Does not treat multiple element intersections as stress discontinuities in the geometric interpolation method.
Tolerance
0.0
TOL=0.0
Elements: Surfaces
Yes
Defines the tolerance to be used for interelement slope differences. Slopes beyond this tolerance will signify discontinuous stresses.
Percent of Step Output
100
NOi Field of TSTEP and TSTEPNL entry
All
Once per subcase
An integer ‘n’ that specifies the percentage of intermediate outputs to be presented for transient and nonlinear transient analyses.
Adaptive Cycle Output Interval
0
BY = n on OUTPUT Bulk Data entry
p-elements Once per subcase
An integer ‘n’ that requests intermediate outputs for each nth adaptive cycle. For n=0, only the last adaptive cycle results are output. This is available for SOLs 101 and 103 for versions 68 and higher.
Intermediate Yes Output Options
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed load increment. Applicable for nonlinear static solution type only.
No
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for the last load of the subcase. Applicable for nonlinear static solution type only.
All
INTOUT field of NLPARM Bulk Data entry
All
Once per subcase
Intermediate outputs are requested for every computed and userspecified load increment. Applicable for nonlinear static solution type only.
426
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-2
Output Request Form Options (continued)
Options
Label
Case Control or Bulk Data Options
Groups
Multiple Select Allowed
Descriptions
Suppress Print for Result Type
N/A
Specifies PLOT option instead of PRINT on the Case Control Output request entry.
All
Yes
Print to the .f06 file is suppressed for the result type when this is selected.
Output Device Options
Specifies PRINT on a Case Control request entry, e.g. DISPL.
All
Yes
The printer will be the output medium for the .f06 file.
Punch
Specifies PUNCH All on a Case Control request entry, e.g. DISPL.
Yes
The punch file will be the output medium.
Both
Specifies both PRINT and PUNCH.
Yes
The printer and punch file will be the output medium.
All
Edit Output Requests Form Use this form to edit the outputs request associated with selected subcases. To access this form, select the Output Requests button on the Subcases form with the Action set to Global Data.
Chapter 3: Running an Analysis 427 Output Requests
Selecting the Default button when a single cell is selected resets the selected output request to its default setting.
The row labels for the spreadsheet are the selected subcases from the parent form. The Output Requests for each subcase are stored in cells of the spreadsheet.
Clears the selected cells. You can select individual cells, multiple cells in a column, entire columns, or entire rows. Inactive (greyed out) until a subcase label (column Closes the form and saves the selected changes. To apply the 1) is selected. When this button is selected, the top new output requests, you must select Apply on the parent half of the form will become inactive, and the default Subcases/Global Data form. output request function (named user_change_default_out_req) will be called. This will load user defined defaults or the system defined defaults if user ones do not exist.
Notes: • The Edit Output Requests form opens with focus in the first result type of the first subcase. • The top half of the Edit Output Requests form is similar to the Advanced Output Request form. • The spreadsheet column labels are the result types for the current solution type. • Putting focus in a cell causes the top half of the form to reflect the current setting, just like the
current advanced output request form. This means that the databox RESULT TYPE: gets updated with the result type of the currently selected cell. The OUTPUT REQUESTS: databox is also updated to show the actual content of the cell.
428
Patran Interface to MD Nastran Preference Guide Output Requests
• If a cell is initially empty, selecting it will cause the top half of the form to display the
appropriate default setting for the selected result type (i.e., column). • Selecting a column header will allow you to change all subcase output requests of a particular
type. The top half of the Edit Output Requests form will set to the default request of the particular result type. • When you select a set of contiguous column cells, the top half of the form will configure to the
upper most selected cell. • You cannot select multiple columns.
Default Output Request Information In order to make use of this new feature you will need to create a PCL file that contains the function user_change_default_out_req which will overwrite the existing default file in Patran. This new PCL file will need to be compiled and then the resulting library (.plb) will need to be loaded into Patran. This can be done using the p3midilog.pcl or the p3epilog.pcl file. The user_change_default_out_req function makes use of the mscn_user_add_out_req and the mscn_user_del_out_req functions to add and delete default Output Request types. These two functions are defined as follows:
mscn_user_add_out_req
(or_num, or_value)
Description: This function adds either a specified version or a default version of an Output Request type to the list of default Output Requests. Input: INTEGER or_num The OR number of the output request type to add (See Table 3-3). STRING or_value The value of the selected output request type. Blank implies the default value.
mscn_user_del_out_req
(or_num)
Description: This function deletes the specified Output Request type from the list of default Output Requests. Input: INTEGER or_num The OR number of the Output Request type to delete (See Table 3-3). Code Sample
FUNTION user_change_default_out_req(sol_seq) INTEGER sol_seq IF (sol_seq == 101 || sol_seq == 106) THEN
Chapter 3: Running an Analysis 429 Output Requests
/* This will add this version of the Output Request type to the list of default */ /* Output Requests for solution 101 and 106. */ mscn_user_add_out_req (4,”MPCFORCES(SORT2,REAL)=ALL FEM”) /* This will add the default version of these Output Request types from the list */ /* of default Output Requests for solution 101 and 106. */ mscn_user_add_out_req (10,“ ”) mscn_user_add_out_req (6,“ ”) /* This will delete these Output Request types from the list of default */ /* Output Requests for solution 101 and 106. */ mscn_user_del_out_req (1) mscn_user_del_out_req (2) mscn_user_del_out_req (3) END IF END FUNCTION The following is a table that shows the current predefined default Output Requests (those marked with an X) and the allowed options (those marked with an O) for the various solution sequences. Table 3-3
Result ID Number OR Number
Result ID Number (Solution Sequence )
1
2
3
4
5
6
101
x
x
x
o
o
o
103
o
o
x
o
o
105
x
o
x
o
o
o
106
x
x
x
o
o
107
o
o
x
o
o
108
x
o
x
o
o
o
109
x
o
x
o
o
o
110
o
o
x
o
o
111
x
o
x
o
o
o
112
x
o
x
o
o
o
114
x
x
x
o
o
o
115
o
o
x
o
o
129
x
o
x
153
o
o
o
159
o
o
o
400
o
7
8
9
10 11 12 13 14 15 16 17 18 19 20 21
o
o
o
o
o
o
o
o o
o o
o
o o
o
o
o
o
o
x
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
o
x
o
o
o
o
o
o
o
o o
x
x
x
o
o
o
o
o o
o
24
x
o o
o
23
x
o o
o
22
o
o
o
o
o
x
x
o
o
o
x
x
o
o
o o
o
o x
x
430
Patran Interface to MD Nastran Preference Guide Output Requests
Table 3-3
Result ID Number x
600
x
700
o
x
o
o
o
o
o
o
o
x
1 = Displacement, 2 = stress, 3 = spcforces, 4 = mpcforces, 5 = forces, 6 = oload, 7 = nlload, 8 = ese, 9 = strain, 10 = gpstress, 11 = velocity, 12 = acceleration, 13 = gpforce, 14 = gpsdcon, 15 = elsdcon, 16 = vector, 17 = thermal, 18 = flux, 19 = ht_oload, 20 = ht_spcforces, 21 =enthalpy, 22 = hdot
OR #
Default Value 1
DISPLACEMENT(SORT1,REAL)=All FEM
2
STRESS(SORT1,REAL,VONMISES,BILIN)=All FEM;PARAM,NOCOMPS,-1
3
SPCFORCES(SORT1,REAL)=All FEM
4
MPCFORCES(SORT1,REAL)=All FEM
5
FORCE(SORT1,REAL,BILIN)=All FEM
6
OLOAD(SORT1,REAL)=All FEM
7
NLLOAD=All FEM
8
ESE=All FEM
9
STRAIN(SORT1,REAL,VONMISES,STRCUR,BILIN)=All FEM
10
GPSTRESS=All FEM; VOLUME # SET,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL,BRANCH BREAK
11
VELOCITY(SORT1,REAL)=All FEM
12
ACCELERATION(SORT1,REAL)=All FEM
13
GPFORCE=All FEM
14
GPSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
15
ELSDCON=All FEM; VOLUME # SET #,PRINCIPAL,SYSTEM Coord 0; SURFACE # SET #,FIBRE ALL,SYSTEM Coord 0, AXIS X1,NORMAL R, TOPOLOGICAL 0.,BRANCH BREAK
16
VECTOR(SORT1,REAL)=All FEM
17
THERMAL=(SORT1,PRINT)=All FEM
18
FLUX(SORT1,PRINT)=All FEM
19
OLOAD(SORT1,PRINT)=All FEM
20
SPCFORCES(SORT1,PRINT)=All FEM
21
ENTHALPY(SORT1,PRINT)=All FEM
22
HDOT(SORT1,PRINT)=All FEM
Chapter 3: Running an Analysis 431 Output Requests
23
NLSTRESS
24
BCCONTACT
Note:
In SOL 109, 112 & 159 will have SORT2 as the default in some versions of Patran.
Subcases Direct Text Input This form is used to directly enter entries into the Case Control section for the defined subcase. Directly entered entries may potentially conflict with those created by the interface. Writing these entries to the file can be controlled with this toggle.
Saves the current setting and data for the four sections and closes the form.
Clears the current form.
Resets the form back to the data values it had at the last OK.
Resets all four forms back to its previous value and closes the form.
432
Patran Interface to MD Nastran Preference Guide Output Requests
SOL 600 Output Requests This subform defines the output data for a SOL 600 analysis subcase
Echo Marc Input File
Produces an echo of the input file.
Results in Marc Print File
Writes results to a print file.
Results (POST) File Options • Increments between Writing Results
Defines the number of increments between writing results to the MD Nastran results file after the first increment of the analysis. The default is one (1) for every increment. Note: You can select a fixed number of increments of output on the subcase parameters-load increments parameters form.
• Select Nodal Results...
Brings up a subform for selecting nodal results
• Select Element Results...
Brings up a subform for selecting elemental results.
Output requests for all subcases.
Chapter 3: Running an Analysis 433 Output Requests
Select Nodal Results
This subform controls which nodal result quantities are returned from the analysis.
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers, that will be specified on the MARCOUT entry
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
434
Patran Interface to MD Nastran Preference Guide Output Requests
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis. Nodal Result
Postcode
Default(?)
DISPLACEMENT
1
YES
ROTATION
2
no
EXTERNAL FORCE
3
no
EXTERNAL MOMENT
4
no
REACTION FORCE
5
YES
REACTION MOMENT
6
no
PORE PRESSURE
23
no
VELOCITY
28
no
ROTATIONAL VELOCITY
29
no
ACCELERATION
30
no
ROTATIONAL ACCELERATION
31
no
MODAL MASS
32
no
ROTATION MODAL MASS
33
no
CONTACT NORMAL STRESS
34
no
CONTACT NORMAL FORCE
35
no
FRICTION STRESS
36
no
FRICTION FORCE
37
no
CONTACT STATUS
38
no
CONTACT TOUCHED BODY
39
no
HERRMANN VARIABLE
40
no
POST CODE, No. -11
-11 thru -16
no
POST CODE, No. -22
-21 thru -23
no
POST CODE, No. -31
-31
no
POST CODE, No. -41
-41
no
POST CODE, No. -51
-51
no
Note:
The POST CODE (<0) are for user-defined quantities via user subroutine UPSTNO.
Chapter 3: Running an Analysis 435 Output Requests
Element Output Requests
This subform controls which element result quantities are returned from the MSC.Marc analysis.
436
Patran Interface to MD Nastran Preference Guide Output Requests
Available Result Types
Lists all of the available result types for the analysis. The numbers in parentheses are the MSC.Marc POST code numbers.
Selected Result Types
Shows the set of result types that have been selected to be returned in the analysis.
Element X-section Results
Defines the number of layer points to use through the cross section of homogeneous shells, plates and beams. This number must be odd if not a composite.
Note:
If no changes are made to the default output requests, no MARCOUT entry will be written and MD Nastran will determine the appropriate output.
The following table shows the post codes that may be selected for a SOL 600 structural nonlinear analysis. Elemental Result
Postcode
Solutions
Default(?)
STRAIN, TOTAL COMPONENTS
301
nonlinear only
YES
STRAIN, TOTAL COMPONENTS (defined system)
461
nonlinear only
no
STRAIN, ELASTIC COMPONENTS
401
any
no
STRAIN, ELASTIC COMPONENTS (global system)
421
any
no
STRAIN, ELASTIC EQUIVALENT
127
any
no
STRAIN, PLASTIC COMPONENTS
321
nonlinear only
no
STRAIN, PLASTIC COMPONENTS (global system)
431
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT
27
nonlinear only
no
STRAIN, PLASTIC EQUIVALENT (from rate)
7
nonlinear only
no
STRAIN, CRACKING COMPONENTS
381
nonlinear only
no
STRAIN, CREEP COMPONENTS
331
creep only
no
STRAIN, CREEP COMPONENTS (global system)
441
creep only
YES
STRAIN, CREEP EQUIVALENT
37
creep only
no
STRAIN, CREEP EQUIVALENT (from rate)
8
creep only
no
STRAIN, THERMAL
371
any
no
STRAIN, THICKNESS
49
any
no
STRAIN, VELOCITY
451
nonlinear only
no
Chapter 3: Running an Analysis 437 Output Requests
Elemental Result
Postcode
Solutions
Default(?)
STRESS, COMPONENTS
311
any
no
STRESS, COMPONENTS (defined system)
391
an
no
STRESS, COMPONENTS (global system)
411
any
YES
STRESS, EQUIVALENT YIELD
59
nonlinear only
no
STRESS, EQUIVALENT MISES
17
any
no
STRESS, MEAN NORMAL
18
any
no
STRESS, INTERLAMINAR SHEAR No. 1
108
any
no
STRESS, INTERLAMINAR SHEAR No. 2
109
any
no
STRESS, INTERLAMINAR COMPONENTS
501,511
any
no
STRESS, CAUCHY COMPONENTS
341
nonlinear only
no
STRESS, CAUCHY EQUIVALENT
47
nonlinear only
no
STRESS, HARMONIC COMPONENTS
351 (real) 361(imag)
harmonic only
no
STRESS, REBAR UNDEFORMED
471
any
no
STRESS, REBAR DEFORMED
481
any
no
FORCES, ELEMENT
264-269
any
no
BIMOMENT
270
any
no
STRAIN RATE, PLASTIC
28
nonlinear only
no
STRAIN RATE, EQUIVALENT VISCOPLASTIC
175
any
no
STATE VARIABLE, SECOND
29
any
no
STATE VARIABLE, THIRD
39
any
no
TEMPERATURE, ELEMENT TOTAL 9
any
no
TEMPERATURE, ELEMENT INCREMENTAL
any
no
STRAIN ENERGY DENSITY, TOTAL 48
nonlinear only
no
STRAIN ENERGY DENSITY, ELASTIC
58
any
no
STRAIN ENERGY DENSITY, PLASTIC
68
nonlinear only
no
THICKNESS, ELEMENT
20
any
no
10
438
Patran Interface to MD Nastran Preference Guide Output Requests
Elemental Result
Postcode
Solutions
Default(?)
VOLUME, ELEMENT
78
any
no
VOLUME, VOID FRACTION
177
any
no
GRAIN SIZE
79
any
no
FAILURE, INDEX No. 1-7
91-103
any
no
DENSITY, RELATIVE
179
any
no
POST CODE, No. 19
19
any
no
POST CODE, No. 38
38
any
no
POST CODE, No. -11
-11 thru -16
any
no
POST CODE, No. -21
-21 thru -23
any
no
POST CODE, No. -31
-31
any
no
POST CODE, No. -41
-41
any
no
POST CODE, No. -51
-51
any
no
DDAM Output Requests The output requests form has been altered for the DDAM solution. Because the program performs an NRL sum and has no explicit constraints, only a few result quantities are available: Nodal Results: Displacement Velocity Accelerations Element Results: Stress Force The results reported in the .f06 file are printed sequentially, first x-shock results, then y, then z, but all are labeled as TIME = 0.000000E+00. To differentiate these in the file, there is a small header printer prior to the results for each shock direction that looks something like this: ^^^ ^^^ *************************************** ^^^ ^^^ SUMMED MODAL RESPONSES IN X-DIRECTION ^^^ ^^^ *************************************** ^^^
Chapter 3: Running an Analysis 439 Output Requests
If you need to find the start of the X-shock results, search for X-DIRECTION to find this header and proceed from there. It is necessary to specify that Patran calculate the combined stresses on a mode-by-mode basis, and NRL sum the combined results. See Defining Translation Parameters for DDAM (SOL 187) (Ch. 4). Mode by Mode Output You can use the Direct Text Input section of Patran Analysis forms to obtain more data. Using the parameters XBYMODE, YBYMODE and ZBYMODE you can get mode by mode data for the selected direction. To get this data, enter the following lines into the Bulk Data direct text area: PARAM,XBYMODE,YES PARAM,YBYMODE,YES PARAM,ZBYMODE,YES You can select one or more of these parameters. Keep in mind that this generates a lot of data for an analysis with a lot of modes, and that you must have an output request for the corresponding data – e.g., if you want mode-by-mode displacements, you must have a DISPLACEMENT request as chosen above. Each of these parameters outputs the data to the .f06 file if you have the (PRINT) option on, or an .op2 file if the (PLOT) option is on. Both are on by default when you specify something like: DISPLACEMENT = ALL Alternately, DISPLACEMENT(PLOT) = ALL DISPLACEMENT(PRINT) = ALL plots or prints the results. If unassigned, the mode-by-mode results outputs to generic Fortran files (like fort.42), so it is necessary to add an ASSIGN statement to the file if you wish to have these files named appropriately. To do this, use the FMS section in the Direct Text Input form, and add lines like: ASSIGN OUTPUT2=’jobname_mbmx.op2’, UNIT=41, DELETE ASSIGN OUTPUT2=’jobname_mbmy.op2’, UNIT=42, DELETE ASSIGN OUTPUT2=’jobname_mbmz.op2’, UNIT=43, DELETE In the .f06 file, the mode-by-mode results are labeled with their own header prior to the section: ^^^ ^^^ ************************************************** ^^^ ^^^ INDIVIDUAL SCALED MODAL RESPONSES IN Y-DIRECTION ^^^ ^^^ ************************************************** ^^^
440
Patran Interface to MD Nastran Preference Guide Output Requests
Since the mode-by-mode velocities and accelerations are calculated by multiplying the displacements by the frequency (omega and omega2), MD Nastran labels them as Eigenvectors. If you ask for displacement, velocity, and acceleration for three modes, you will find nine Eigenvectors in the .f06 file with repeating frequencies – the first three (1-3) are displacements, the next three (4-6) velocities, and the last three (7-9) the accelerations. The .op2 files are similar, reporting the three as Eigenvectors with repeating frequencies. The magnitude of the values should be a clue as to what you are looking at for all but the lowest frequencies. The Fortran Driver File (jobname.ddd)
Some of the options you choose on the Subcase Parameters form are written to an external file that is read by the Fortran file when it calculates the spectrum. While you do not have the ability to edit this file when using MSC.FEA, the file is a hardcopy ASCII record of what options were used when running the DDAM analysis. The file is small and has just a few lines that comprise the answers to questions that the ddam.exe program asks if it is run interactively. File Format (varies depending on chosen options on the first record) Record 1 (user spectrum file) (user coef file) (DDS-072 format) user spectrum file= T (use a user defined spectrum) = F (use coefficients) user coef file = T (use an external coefficient file) = F (use the coefficients compiled into the Fortran) DDS-072 format = T (use DDS-072 style equations) = F (use NRL 1396 style equations) Record 1a (if either file option on record 1 was true) cp10 filename = name of either the spectrum file or coefficient file Record 2 (if using coefficients) nsurf nstruc nplast ship type mount location elastic/plastic
Record 3 pref pref
= 1 (surface ship equations) = 2 (submarine equations) = 1 (file mounted equipment) = 2 (hull mounted equipment) = 1 (use elastic factors) = 2 (use elastic/plastic factors)
= 0.0 (use default cutoff in program) = nnn.nn
Chapter 3: Running an Analysis 441 Output Requests
Record 4 Ming Ming
Record 5 (F/A axis) (Vert axis) F/A axis
Vert axis
= 0.0 (no minimum G) = n.n (use this minimum G value)
= X (F/A is along the X axis) = Y (F/A is along the Y axis) = Z (F/A is along the Z axis) = X (Vertical is along the X axis) = Y (Vertical is along the Y axis) = Z (Vertical is along the Z axis)
Record 6 .f11 filename .f11 filename
= name of the .f11 file
Record 7 .f13 filename .f13 filename
= name of the .f13 file
Record 8 .ver filename .ver filename
= name of the modal verification file
Depending on the chosen options, the file will look like one of the following: No special user options – coefficients from default source:
F F T nsurf nstruc nplast pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename
442
Patran Interface to MD Nastran Preference Guide Output Requests
User coefficient option:
F T T coef.dat filename nsurf nstruc nplast pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename User spectrum Option:
T F T spec.dat filename pref ming f/a_axis vert_axis .f11 filename .f13 filename .ver filename Note:
Note that capitalization is required. The file is read free-format, so spacing is not important. A sample file for a conventional analysis might look like: F F T 1 1 1 100. 1. X Z d1.f11 d2.f11 d1.ver
Chapter 3: Running an Analysis 443 Select Explicit MPCs...
3.10
Select Explicit MPCs... The Explicit MPCs created in the Element menu can be selected for a given subcase. The highlight of selected Explicit MPCs is supported when this form is displayed. The All MPCs toggle indicates that all the Explicit MPCs already created or created later will be used for the subcase being created. The All MPCs toggle should be turned OFF in order to select MPCs. ‘MPXADD SID’ is the ID used for identifying the selected MPCs for the subcase.
444
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
3.11
Non-Structural Mass Properties MSC Nastran non-structural mass (NSM and NSML) are now supported in Patran. Note:
NSM and NSML are used to define masses that affect the behavior of specific element types but are not directly part of the structure of the model. NSM and NSML support:
Line Element Types
Surface Element Types
Property Types
CBAR, CBEAM, CBEND, CONROD, CROD, CTUBE
CCONEAX, CQUAD4, CQUAD8, CQUADR, CRAC2D, CSHEAR, CTRIA3, CTRIA6, CTRIAR
CONROD, PBAR, PBARL, PBCOMP, PBEAM, PBEAML, PBEND, PCOMP, PCONEAX. PRAC2D, PROD, PSHEAR, PSHELL, PTUBE
NSM and NSML forms are available through the Tools menu.
Selecting NSM Properties displays the NSM Properties form. NSM Properties forms are MSC Nastran preference specific. NSM mass can be applied as Lumped or Distributed.
Chapter 3: Running an Analysis 445 Non-Structural Mass Properties
For a distributed NSM, the mass is spread evenly over all of the elements in the application region. For a lumped NSM, the applied mass is applied directly to each element in the application region.
446
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
Non-structural mass can be applied to elements or property sets.
Chapter 3: Running an Analysis 447 Non-Structural Mass Properties
A Select form has been added to allow for the selection of NSM properties. Multiple sets of NSMs can be defined in the model. Only the selected sets will be used in the analysis.
The following examples display results of applying lumped and distributed NSMs.
448
Patran Interface to MD Nastran Preference Guide Non-Structural Mass Properties
A lumped mass value of 20 is applied to 10 elements
A distributed mass value of 20 is applied to 10 elements.
Chapter 3: Running an Analysis 449 Select NSM Properties...
3.12
Select NSM Properties... This Subcases dependant form allows you to select the defined Nonstructural Mass sets. The Defined NSM Sets box lists all defined Nonstructural Mass property sets. Since it is possible to have up to four property sets with the same set name, the Distributed vs Lumped and Element vs Property attributes of the sets are listed in columns to the left of the property set name. Individual groupings of Nonstructural Mass property sets can be selected in the form and then applied with the Apply button. By default, all of the listed Nonstructural Mass property sets are selected by the case control code even if they are not shown as selected in the Defined NSM Sets box. Groups of Nonstructual Mass properties can be excluded from an analysis by not including that specific subcase in the analysis job. Individual Nonstructural Mass properties can be excluded from an analysis by setting the applied mass for that property set to zero (0).
450
Patran Interface to MD Nastran Preference Guide Select NSM Properties...
This subform appears when the Select NSM Properties... button is selected from the Subcases form.
Chapter 3: Running an Analysis 451 Subcase Select
3.13
Subcase Select This form appears when the Subcase Select button is selected on the Analysis form. This form is used to select a sequence of subcases associated with an analysis job.
Displays all the available subcases for the current solution sequence. The current solution sequence is displayed at the top of the form. For example, SOL 101 subcases lc1, lc2, and lc3.
Displays all subcases that have been associated with the current job name. For example, subcases lc1 and lc3 have been selected; for SOL 101 the Bulk Data will contain two Case Control section SUBCASEs, SUBCASE 1 and SUBCASE 2. For SOL 600 a single run will be performed with it having two steps, lc1 and lc3. For optimization jobs, the solution type will be appended at the begining of the subcase name.
For SOL 400 runs the Subcase Select form looks the same, except for the Select Steps for New Subcase button being un-greyed (it is pickable).
452
Patran Interface to MD Nastran Preference Guide Subcase Select
Displays all the available subcases for SOL 400. For example, subcases lc1, lc2, lc3, lc4, and lc5.
Displays all subcases that have been associated with the current job name. If the button Select Steps for New Subcase is not used, the job run will be the same as for SOL 600 , a single run will be performed with five steps, 1c1, ..., lc5, in the order shown in the GUI going from top to bottom.
When the Select Steps for New Subcase button is used the following form appears.
Chapter 3: Running an Analysis 453 Subcase Select
Notice that the selected steps (lc1, lc2, lc3, lc4, and lc5) match the selected subcases of the parent form. This indicates that some or all of these steps can be used in defining the new subcases. By selecting the steps lc1 and lc3, under Steps Selected, the names are entered under New Subcase Starting with Steps. This indicates that two subcases will be defined, “subcase_lc1” and “subcase_lc3”.
Displays the steps names that are to be used at the begining of the (new) subcases to be created. The subcases that are defined are “subcase_lc1” with steps lc1 and lc2, and “subcase_lc3” with steps lc3, lc4 and lc5: • Subcase, “subcase_lc1” • Steps: lc1, lc2 • Subcase, “subcase_lc3” • Steps: lc3, lc4, lc5
454
Patran Interface to MD Nastran Preference Guide Restart Parameters
3.14
Restart Parameters This format of the Analysis form appears when the Action is set to Analyze and the Object is Restart. Currently, restarts are only supported for the Linear Static (101), Nonlinear Static (106), and Normal Modes (103) Solution Sequences. Linear and Nonlinear Static jobs can be restarted as Linear or Nonlinear Static. Normal Modes jobs can be restarted as Frequency Response, or Transient Response. The DBALL and the MASTER files for the initial job must be present in the current directory when the restart job is submitted.The Restart Parameters button on the main analysis form allows the user to enter information about where to resume the analysis. The Patran Analysis Manager User’s Manual contains
Chapter 3: Running an Analysis 455 Restart Parameters
more information on how to submit restart jobs with Analysis Manager. Restart for SOL 600 jobs are described on (p. 315) and (p. 458).
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of names for existing analysis jobs. Select the jobname of the analysis to restart from.
List of names for existing restart jobs. Select the name of an existing restart job or enter the name for a new restart job in the databox below.
Name to use for the restart job. An existing restart job may be modified and/or resubmitted by making a selection from the Available Restart Jobs listbox.
456
Patran Interface to MD Nastran Preference Guide Restart Parameters
Linear Static/Normal Modes
This subordinate form appears when the Restart Parameters button is selected on the Analysis form and the solution type of the initial job is Linear Static or Normal Modes.
Defines the version number from which to restart. This is the VERSION field on the RESTART file management statement.
Requests that the restart data for the specified version be saved. This results in a KEEP option on the RESTART File Management statement.
Chapter 3: Running an Analysis 457 Restart Parameters
Nonlinear Static
This subordinate form appears when the Restart Parameters button is selected on the Analysis form and the solution type is Nonlinear Static.
Defines the version number to restart the analysis from. This is the VERSION field on the RESTART File Management statement.
Defines the increment number to start the analysis from. This is the value of the PARAM,LOOPID Bulk Data entry.
Defines the subcase number to start from in the list of subcases for this job. The value entered should be one greater than the SUBID from the initial job’s print file (*.f06). This is the value of the PARAM,SUBID Bulk Data entry. Requests that the restart data for the specified version be saved. This results in a KEEP option on the RESTART File Management statement.
458
Patran Interface to MD Nastran Preference Guide Restart Parameters
SOL 600
This subordinate form appears when the Restart Parameters button is selected on the Solution Parameters form.
Set Restart Parameters Restart Parameters: None
Restart Type: Create Continuous Results File Last Converged Increment
Reauto
Restart from Increment =
Increments between Writing Data =
Select Restart File...
OK
Parameter
Cancel
Description
Restart Type
You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File
If, when restarting a job, you wish the results form the previous run to be copied into the new .t16 file, then turn this ON. Otherwise MSC.Marc will not copy the results to the new .t16 file. If you turn this ON, you must have a restarname.marc .t16 and/or restartname.marc.t19 file in your local directory or the MSC.Marc analysis will fail.
Last Converged Increment
Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto
OFF by default. This places a REAUTO option in the MSC.Marc input file. Any additional data needed for the REAUTO option are extracted from the first Subcase information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user.
Chapter 3: Running an Analysis 459 Restart Parameters
Parameter
Description
Restart from Increment
Defines the increment to be read from the file specified in the Select Restart File form. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing
Defines the number of increments between writing data to the restart file. It is only requested when Restart Type is set to Write or Read and Write.
Select Restart File...
This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write.
460
Patran Interface to MD Nastran Preference Guide Optimize
3.15
Optimize When preparing for an optimization analysis run, select Optimize as the Action on the Analysis application form. This allows setup and submission of SOL 200 jobs. The functionality is similar and in many cases identical to running a normal analysis as described in Review of the Analysis Form, 260 and other sections in this chapter. Each button and its subordinate form that appears when the Action is set to Optimize is explained briefly below. Use the Optimize action for sizing optimization and combined sizing and topology optimization. For pure topology, topography and topometry optimization, use the Toptomize action explained in Toptomize, 462.
Button/Subordinate Form:
Description:
Design Study Select...
From this form, select the design study of interest. Design studies can contain multiple design objectives, responses, constraints, and variables. Any particular job can only have one design objective. The specific objective and constraints to be used in an optimization job are selected in the Global Objective / Constraint Select form or they are associated to a solution specific subcase. Design Studies are setup under the Design Study tool under the Tools pull down menu. A Default design study is present if none are previously created, however a design study without any design variable defined will not run through Nastran properly.
Global Obj/Constr Select...
Once a design study has been selected, you may select from this form the specific global design objective and constraints to be active for this job. You can only have one objective in an optimization job. A global objective will override any other objective associated to a solution specific subcase that may be associated to this job, therefore it is not necessary to select a global objective or constraints when defined at the subcase level.
Translation Parameters...
These parameters are described in Translation Parameters, 265 and are not specific to optimization.
Optimization Parameters...
This form is used to define optimization parameter for the job. Parameters set in this form and its subordinate form define some of the values on the DOPTPRM entry. These are explained in the MSC Nastran Quick Reference Guide under this entry and the user if referred there for details. Results file formats can also be set in this form as described in Results Output Format, 348.
Direct Text Input...
Use of this form is described in Direct Text Input, 276.
Select Superelements...
Use of this form is described in Select Superelements, 352.
Subcases...
Use of this form is described in Subcases, 354. There are two differences that are significant to this form, however. For optimization, subcases are created based on solution sequence, e.g. Statics 101, Normal Modes 103, etc. You must set the solution sequence on this form before creating the subcase, otherwise the default 101 will be used. Secondly, an additional subordinate form allows you to select existing constraint sets and an objective for the particular subcase being created if necessary. Objectives and constraints are created using the Design Study tool under the Tools pull down menu. Note that not all subcase parameters are identical between a normal analysis and an optmization analysis. Also see the note on Contact below: page 461.
Chapter 3: Running an Analysis 461 Optimize
Button/Subordinate Form:
Description:
Subcase Select...
Use of this form is described in Subcase Select, 451. One difference is that for optimization you must set the solution type to see the subcases defined for a particular solution sequence. Otherwise by default only SOL 101 subcases are displayed. A selected subcase will display the associated solution sequence number in front of its label.
Analysis Manager...
This gives access to the Analysis Manager for submitting, monitoring, aborting and generally managing a Nastran job. This button will not appear if the Analysis Manager is not installed or licensed.
Note:
Using Contact Bodies in Optmization Jobs: Linear contact is supported in optimization jobs (SOL 200). If contact bodies are present in the model and included in the load cases associated to the the subcases created, then the contact bodies will be written to the deck. The most common scenario is using linear contact in optimization jobs to glue noncongruent meshes together. When this feature is used, you must “glue” the bodies together, which requires that you set up the proper contact tables to define body pairs that are properly glued. Usage of the contact table is described in Contact Table, 396.
462
Patran Interface to MD Nastran Preference Guide Toptomize
3.16
Toptomize When preparing for a pure topology, topometry, or topography optimization analysis run, select Toptomize as the Action on the Analysis application form. This allows setup and submission of SOL 200 jobs. The functionality is similar and in many cases identical to running a normal analysis as described in Review of the Analysis Form, 260 and other sections in this chapter. Each button and its subordinate form that appears when the Action is set to Toptomize is explained briefly below. Use the Optimize action for sizing optimization and combined sizing and topology optimization as explained in Optimize, 460. Button/Subordinate Form: Translation Parameters...
Description: These parameters are described in Translation Parameters, 265 and are not specific to optimization.
Optimization Parameters... This form is used to define optimization parameter for the job.
Parameters set in this form and its subordinate form define some of the values on the DOPTPRM entry. These are explained in the MSC Nastran Quick Reference Guide under this entry and the user if referred there for details. Note that no DOPTPRM entry is written if all values are default values. Results file formats can also be set in this form as described in Results Output Format, 348.
Objectives & Constraints... This form allows you to define the objective and constraints for the topology, topometry or topography optimization run. Please see Objectives & Constraints, 463 below.
Optimization Controls...
This form allows you to define various controls and settings necessary for topology, topometry, or topography optimization jobs. Please see Optimization Control, 464 below.
Design Domain...
This form allows you to select the property sets that define the active design domain. Manufacturing constraints are defined via this form also. Please see Design Domain, 466 below.
Direct Text Input...
Use of this form is described in Direct Text Input, 276.
Subcases...
Use of this form is described in Subcases, 354. There are two differences that are significant to this form, however. For optimization, subcases are created based on solution sequence, e.g. Statics 101, Normal Modes 103, etc. You must set the solution sequence before creating the subcase, otherwise the default 101 will be used. Secondly, an additional subordinate form allows you to select existing constraint sets and an objective for the particular subcase being created if necessary. Objectives and constraints are created using the Design Study tool under the Tools pull down menu. Note that not all subcase parameters are identical between a normal analysis and an optmization analysis. Also see the note on Contact above: page 461.
Subcase Select...
Use of this form is described in Subcase Select, 451. One difference is that for optimization you must set the solution type to see the subcases defined for a particular solution sequence. Otherwise by default only SOL 101 subcases are displayed. A selected subcase will display the associated solution sequence number in front of its label.
Analysis Manager...
This gives access to the Analysis Manager for submitting, monitoring, aborting and generally managing a Nastran job. This button will not appear if the Analysis Manager is not installed or licensed.
Chapter 3: Running an Analysis 463 Toptomize
Objectives & Constraints This form is used to define the optimization type and select the objective and constraints of the optimization run. All widgets on this form are explained in the table below. Widget Parameter:
Description:
Type
Select the optimization type for job to be set up, either Topology, Topometry, or Topography. Topology is the default.
Objective Function(s):
The objective of the optimization is set with the widgets in this frame. The default is to Minimize Compliance. Multiple static subcases are allowed.
Minimize Compliance Maximize Frequency Track Modes Mode Numbers
Optionally you can also maximize frequency (or eigenvalue). You specify the mode number in the provided databox. If the provided mode is not the first mode or you provide modes such as 1 5 and 6, you can turn on the Track Modes toggle. This is recommended as modes can change with each design cycle. The MODTRAK case and bulk data entries are written in this case using the number of modes called out for extraction as set up in the modal subcase. Multiple modal subcases are allowed. A DESOBJ case control entry is written to the deck which calls out the appropriate DRESP1 and/or DRESP2 entries with the COMP, FREQ, or EIGN options. Multiple DRESP1 entries are written when the Constraint Target is Mass Fraction with multiple property sets selected and subsequently referenced or combined using an average function on the DRESP2 entry. Only one objective is allowed, however you can specify to Minimize Compliance and Maximize Frequency in which case you need to also specify a single Frequency Constraint Target. This target along with the compliance minimization objective is combined onto a DRESP2 entry using a DEQATN entry to formulate the objective relationship. In this case a single modal subcase is required. Note that when multiple static subcases are selected, a DRSPAN entry is written to each subcase as necessary to ensure the objective function properly spans all subcases.
464
Patran Interface to MD Nastran Preference Guide Toptomize
Widget Parameter: Frequency Constraint Targets
Description: Specify the mode number(s) and corresponding frequencies to be constrained in the optimization run. At least one modal subcase is required. This is typically used when the Objective Function is set to Maximize Frequency. If the Objective Function is set to both Minimize Compliance and Maximize Frequency, then a singe mode frequency target is required and only one modal subcase is allowed. A DESSUB case control is written to the deck which calls out the appropriate DCONSTR and DRESP1 entries. This constraint because part of the objective if both Minimize Compliance and Maximize Frequency objective functions are specified and is incorporated via a DEQATN entry referenced on a DRESP2 entry called out by a DESOBJ case control.
Constraint Target
Specify the constraint target. For Topology, only Mass Fraction is allowed. For Topography, only Weigh or Volume is allowed. For Topometry, either of the three are allowed. You must specify the mass fraction, weight or volume target. By default, the mass fraction is 0.4 (40% of the original mass). However, volume and weight have no defaults. If the Objective Function is set to only Maximize Frequency, then a Constraint Target is not required (can be set to None) for Topometry and Topography only. A DESGLB case control is written, which calls out the appropriate DCONSTR and DRESP1 entries. For Weight and Volume, only a single DCONSTR/DRESP1 entry combination is written as the entire design domain can only have one weight or volume constraint. For Mass Fraction, multiple combinations are written with the same DCONSTR ID.
Optimization Control Use this form to set various controls used during the optimization run. They are briefly described here but the user is referred to the MSC Nastran Quick Reference Guide for further information. Leaving a field blank will trigger usage of the default in most cases. Some parameters must be provided or the analysis cannot proceed. Setting the Maximum Design Cycles is the most common usage of this form to limit the analysis to something reasonable. Each optimization type has different settings: Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Initial Design (XINIT)
Required. Initial value. It is recommended that this match the mass target constraint. This value defaults to the mass value target constraint set on the Objectives and Constraints form.
Lower Bounds (XLB)
Optional. Lower bound to prevent the singularity of the stiffness matrix. Leave blank to use Nastran default of 0.001. Real 0.0 < XLB <= 0.1
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Penalty Factor (POWER)
Optional. A penalty factor used in the relation between topology design variables and element Young’s modulus. Leave blank to use Nastran default of 3.0. Real 1.0 <= POWER <= 6.0
Chapter 3: Running an Analysis 465 Toptomize
Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Minimum Member Size (TDMIN)
Optional. Indicates the minimum member size. No default. No minimum is used if not specified. Recommendation is that it be set to three times a representative element dimension. Real > 0.0. This is written to the DOPTPRM entry and is for 2D and 3D elements only.
Checkboard-Free Method (TCHECK)
Optional. On by default. Turns on/off topology filtering (allows of minimizes checker boarding effects). This is written to the DOPTPRM.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
Topometry Parameters:
Description: (all values written to the TOMVAR entry unless otherwise indicated)
Initial Design (XINIT)
Required. Initial design value of property to optimize. Optimization job will not proceed without this value defined. Real > 0.0
Lower Bounds (XLB)
Optional. Lower bound of the property to optimize. Leave blank to use Nastran default of XLB=0.5*XINIT. Real > 0.0.
Upper Bounds (ULB)
Optional. Upper bound of the property to optimize. Leave blank to use Nastran default of XUB=1.5*XINIT. Real > 0.0.
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Property to Optimize (PNAME)
Required. The property to optimize. No Nastran default. This is dependent on the model dimensionality is some cases. Default is set to Thickness for 2d problems but is not appropriate for 1D models where cross sectional Area would be the most common choice.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
466
Patran Interface to MD Nastran Preference Guide Toptomize
Topography Parameters:
Description: (all values written to the BEADVAR entry unless otherwise indicated)
Lower Bounds (XLB)
Optional. Lower bound on the bead height. Leave blank to use Nastran default of 0.0. See the Upper Bounds (XUB) description.
Upper Bounds (XUB)
Optional. Upper bound on the bead height. Leave blank to use Nastran default of 1.0. To force grids to move only the positive bead vector direction (one side of the surface), use XLB = 0.0. To force grids to move only in the negative bead vector direction (the other side of the surface), use XUB = 0.0. To allow grids to move in both positive and negative bead vector directions, use XLB < 0.0 and XUB > 0.0.
Maximum Design Cycles (DESMAX)
This is the maximum number of design cycles after which the optimization run is forced to quit. This is written on the DOPTPRM entry. Default is 30. This option is not written if default is used. The entire DOPTPRM entry is not written if all options are defaulted.
Move Limit (DELXV)
Optional. Fractional change allowed for the design variable during approximate optimization. Leave blank to use Nastran default of 0.2. Real > 0.0 Note that if this is left blank and DELX is specified on the DOPTPRM entry (Optimization Parameters form), Nastran will use that value in place of this one.
Tolerance of Convergence (CONV1)
Optional. Relative criterion to detect convergence. If the relative change in objective between two optimization cycles is less then CONV1, then optimization is terminated. Leave blank to use Nastran default of 0.0001. Real > 0.0. This is written to the DOPTPRM entry.
Minimum Bead Width (MW)
Required. Minimum bead width. There is no default. This controls the width of beads and the recommended value is 1.5 to 2.5 times the average element width. Real > 0.0
Maximum Bead Height (MH)
Required. Maximum bead height. There is no default. This controls the maximum height of beads when XUB = 1.0 (or left blank). Real > 0.0
Draw Angle (ANG)
Required. Draw angle in degrees. This controls the angel of the sides of the beads and the recommended values is between 60 and 75 degrees.
Buffer Zone (BF)
Optional. Buffer zone. This parameter creates a buffer zone between elements in the topography design region and elements outside the design region when turned on, which is the default.
Exclude from Design (SKIP)
Optional. Boundary skip. This indicates which element nodes are excluded from the design region. Constraints indicates all constrained nodes and Loads indicates all nodes referenced by forces, moments and enforced displacements. Both are on by default.
Results Output Format
Results file formats can also be set in this form as described in Results Output Format, 348.
Design Domain The property sets that define the intended design domain are set on this form as well as manufacturing constraints. The form works by clicking on a valid property set (row) in the top spread sheet. This action adds the selected row to the bottom spread sheet, which are the active domains during the optimization run. To remove domains, click on the rows of interest in the bottom spread sheet and press the Remove Selected Rows button.
Chapter 3: Running an Analysis 467 Toptomize
From this form you can also define manufacturing constraints to impose on the topology optimization. Each property set is written to a TOPVAR, TOMVAR, or BEADVAR entry in the input file depending on the optimization Type set in the Objectives & Constraints form. The values of various parameters on these entries can be different for each property set. It is recommended that you review the settings for each property set defined in the design domain before submitting the job. When a property set is added to the selected design domain properties spreadsheet, some of the values are set in the various columns from the settings on the Optimization Control form. To change these settings for an individual property set, simply click on the cell to be changed. A widget will appear above the spreadsheet allowing you to change the value. Use the Enter key to accept the new value into the spreadsheet. The same can be done when opening the Manufacturing Constraints form. The values set in the Manufacturing Constraint forms will correspond only to the property sets that are selected from the Design Domain spreadsheet. If you do not select any rows in the Design Domain spreadsheet, then any change made on the Manufacturing Constraints form will be applied to all property sets in this spreadsheet. For this reason, care should be taken to verify all changes are what is intended. The tables below indicate the parameters that can be set for each property set of the design domain. Any parameter set on this form overrides any global setting of that parameter that may be defined under the Objective & Constraints form or the Optimization Control form. For more information on each parameter, the user is directed to the MSC Nastran Quick Reference Guide. Topology Parameters:
Frac Mass Target (FRMASS)
Description: (all values written to the TOPVAR entry unless otherwise indicated) The fraction mass target for the specified property set. The initial value is picked up from the setting on the Objectives & Constraints form. If one of these cells is set, all rows must be set. You can remove the values from all rows and the value from the Objectives & Constraints form will be used. Otherwise these values override the value from the Objectives and Constraints form. Values in these cells are also written the corresponding DCONSTR/DRESP1 entries with FRMASS option as well as the TOPVAR entry.
468
Patran Interface to MD Nastran Preference Guide Toptomize
Topology Parameters:
Description: (all values written to the TOPVAR entry unless otherwise indicated)
Lower Bounds (XLB)
Lower Bounds. The original value is picked up from the setting on the Optimization Control form. Typically these cells are blank by default. If one of these cells is set, all rows must be set. You can remove the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Manufacturing Constraints:
These are accessed from the Manufacturing Constraints form.
Ref. Coordinate System Minimum Member Size Symmetric Constraints Extrusion Constraints Casting Constraints
Topometry Parameters:
Any direction, plane, or axis specified for the constraints will be in the Reference Coordinate Frame specified. By default all constraints are off. You may turn any on that are applicable. Some combinations are not possible in Nastran and the interface should indicate if an incompatible combination is selected. Note that all of these values can differ for each selected design domain from the Design Domain form (bottom spreadsheet). By selecting a row from the spreadsheet, you can see the settings change on the Manufacturing Constraints form if there are differences. If multiple rows are selected, only the settings for the top row are displayed on the Manufacturing Constraints from. If a change is made to a value with multiple rows selected, the new value is associated to all the selected property sets. If no property sets are selected, it is the same as if all are selected. So care should be taken when changing values on this form to ensure only the property sets of interest are being affected.
Description: (all values written to the TOMVAR entry unless otherwise indicated)
Property to Optimize (PNAME)
The property to optimize. The original value is picked up from the setting on the Optimization Control form. If one of these cells is set, all rows must be set. You can clear the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Initial Design (XINIT)
Initial Value on the property value to optimize. Operates similar to Property to Optimize above.
Lower Bounds (XLB)
Lower Bounds on the property value to optimize. Operates similar to Initial Value above
Upper Bounds (ULB)
Upper Bound on the property value to optimize. Operates similar to Lower Bound above.
Manufacturing Constraints:
Not supported for Topometry.
Chapter 3: Running an Analysis 469 Toptomize
Topography Parameters:
Description: (all values written to the BEADVAR entry unless otherwise indicated)
Minimum Bead Width (MW)
Minimum bead width. The original value is picked up from the setting on the Optimization Control form. If one of these cells is set, all rows must be set. You can clear the values from all rows and the value from the Optimization Control form will be used. Otherwise these values override the value from the Optimization Control form.
Maximum Bead Height (MH)
Maximum bead height. Operates similar to Minimum Bead Width.
Draw Angle (ANG)
Draw angle in degrees. Operates similar to the above parameters.
Lower Bounds (XLB)
Lower bound on the bead height. Operates similar to the above parameters.
Upper Bounds (XUB)
Upper bound on the bead height. Operates similar to the above parameters.
Buffer Zone (BF)
Buffer zone. Operates similar to the above parameters.
Exclude from Design (SKIP)
Boundary skip. Operates similar to the above parameters.
Manufacturing Constraints:
These are accessed from the Manufacturing Constraints form.
Ref. Coordinate Frame Extrusion Direction Nodes to Exclude/Include
Any vector specified for the draws direction of the beads will be in the Reference Coordinate Frame specified. By default the Extrusion Direction is Normal to the surface. If Vector is specified, a user defined vector can be specified in any acceptable manner with the select mechanism. Optionally the user may select a group of nodes to include or exclude from the design domain. Note that all of these values can differ for each selected design domain from the Design Domain form (bottom spreadsheet). By selecting a row from the spreadsheet, you can see the settings change on the Manufacturing Constraints form if there are differences. If multiple rows are selected, only the settings for the top row are displayed on the Manufacturing Constraints from. If a change is made to a value with multiple rows selected, the new value is associated to all the selected property sets. If no property sets are selected, it is the same as if all are selected. So care should be taken when changing values on this form to ensure only the property sets of interest are being affected.
Postprocessing Postprocessing topology optimization results requires that you read element density values (the new mesh from optimization) using the Nastran results .xdb file (e.g. jobname.xdb) or .des file (e.g. jobname.des) through the Tools | Design Study | Postprocessing menu and use that application to view the results rather than through the Patran Results application. See Tools>Design Studies>PostProcess (p. 546) in the Patran Reference Manual.
470
Patran Interface to MD Nastran Preference Guide Interactive Analysis
3.17
Interactive Analysis The Patran Preference for MD Nastran has a new capability that enables the user to perform visual interactive modal frequency response analysis. The process begins by creating a good modal analysis solution with MD Nastran. The interactive modal frequency response solution is then directed from a special set of Patran menus (wizard). The wizard assists the user in applying the desired loads, specifying damping, selecting result entities, and defining solution criteria for an automated fast restart in Nastran effected from the modal database selected. Patran running as the client spawns a fast restart job to Nastran functioning as a server. Solution results are automatically returned to the client for visualization. This procedure suggests that there might be several benefits to using this product. The wizard provides a guide for problem definition, minimizing confusion associated with general-purpose menu structures. The fast restart, as the name suggests, is fast, and is executed automatically, as are the client-server connections and the data transmission. The reduced solution space of the fast restart minimizes the amount of result data that is calculated, stored, transmitted, and displayed. The net result is the ability to quickly apply discrete loads to the structure and immediately visualize the response at select grids or elements of the model. The real time solution paradigm of the interactive scheme does not provide fringe or contour plots of the global structural response. Assumptions Interactive modal frequency response requires that a normal modes analysis of the structure has been completed using Nastran, and that a .DBALL/MASTER database exists containing the model data and the normal modes solution. Currently, the interactive paradigm presumes the Nastran executable, the modal database, and the Patran executable are all located in the same directory. To maintain optimal performance, licensing and security should be local also. Given these initial conditions, the following scenarios exist for performing interactive frequency response. Scenario 1 If the initial normal modes analysis was modeled in Patran, then that Patran database should be selected under File/Open when starting Patran. This provides the user with the model from which to exercise the interactive frequency response wizard, provided the correct flag was set to precondition the Nastran normal modes database for this purpose. This is done in Patran by going to Analysis/Solution Type/Interactive Modal Analysis, and activating the check box. Scenario 2 The normal modes model may have been built and run without using Patran. If the user intends to use the MSC integrated product to proceed with interactive frequency response, then special care must be taken when preparing the NASTRAN input file for the normal modes analysis. Specifically, the Nastran normal modes input file must contain the following statement just before the CEND delimiter: include `SSSALTERDIR:run0.V2001` Note that both “ticks” are right handed and that SSSALTERDIR must be capitalized. Nastran then creates an environment variable called SSSALTERDIR which points to where the sssalters are located when performing a standard installation.
Chapter 3: Running an Analysis 471 Interactive Analysis
If the user does not have a standard Nastran installation, then he will be required to specify the full directory path. For example, if the file run0.V2001 is located in the directory /scr2/mike/tmp, then he must include the following statement just prior to the CEND delimiter: include `/scr2/mike/tmp/run0.V2001` This include statement provides the DMAP alter required to precondition the large modal database. This conditioning enables efficient data manipulation during the interactive frequency response solution phase. Under this scenario, the model data will need to be imported by starting Patran and requesting “Read Input File” from the Analysis Menu. This procedure is described in greater detail in Chapter 5 of this user’s guide, and constitutes reading a NASTRAN Input File for the model data. Once the model data is placed in the Patran database, interactive frequency response can proceed. The Process Scenario 1 or 2 above can be followed to provide a Patran database with a data model suitable for performing interactive frequency response. The Analysis menu shown below controls the interactive analysis process. Submenus for Select NASTRAN .DBALL, Create Loading, Output Requests, Create a Field, and Define Frequencies are discussed. Solution Type--Is currently fixed to Frequency Response (Modal Frequency Response) as the only solution available in interactive analysis format. Subsequent versions of Nastran and Patran may expand this capability to other solution types. Loading Menu--The loading menu provides a spreadsheet to guide the user through load and boundary condition application. Miscellaneous The Interactive Modal Frequency response solution process is staged, in the sense that a normal mode solution is performed first to create what we refer to as the large database (so named for obvious reasons), and then a fast restart procedure is used to develop the frequency response. The normal modes solution is where the user specifies any weight to mass conversion quantities (see PARAM, WTMASS) as well as a specification of the mass matrix formulation desired (see PARAM, COUPMASS). The mass units and desired mass matrix formulation then, are automatically accounted for in the subsequent determination of the frequency response quantities calculated.
472
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Analysis Form
Every interactive solution will have a user assigned job name associated with it. This provides a record of applied loads, enforced motion boundary conditions, solution frequencies requested, structural damping definition, and output request entities. In a Nastran sense, each job represents a “loading condition” which reflects application of a number of loads and load types distributed on the structure. Maintaining a record of the interactive run provides a starting point for subsequent analyses whether they are done in the current session, or a subsequent session. Specifically, if a user wanted to change only a frequency dependent load function or damping function, the interactive job storage capacity makes this a simple procedure.
Each Interactive Analysis will have its solution specifications stored with a job name (Interactive Name). This allows recovery of all specifications required for performing that particular analysis : loading, damping, solution frequencies, and output entities. If an existing Interactive Job is selected, those input requirements automatically populate the interactive menus. If we want to rerun that analysis, all that is required is to hit APPLY on the Analysis Menu. When the calculations are finished in Nastran, the interactive system automatically positions the user in the Interactive Results section where XY plot requests can be made. Plot requests are not saved in the jobs data.
Load types include: Acoustic (Pressure), Force, Displacement, Velocity, or Acceleration.
Chapter 3: Running an Analysis 473 Interactive Analysis
Select Modal Results .DBALL The following form appears when you select Select Nastran .DBALL from the Analysis form. This form provides the pointer to the Nastran database which contains the preconditioned normal modes solution. Some additional data is retrieved from this database for use in Patran. Specifically, the Nastran modal constraint data is provided to Patran to guarantee that the allowable degrees of freedom available for enforced motion are exposed in the Loading Menu. (Application of enforced motion in modal frequency response requires that the effected degrees of freedom were constrained in the normal modes analysis.)
474
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Loading Form This form allows you to create loading sets. The following is the default form.
Load types include: Acoustic (Pressure), Force, Displacement, Velocity, or Acceleration.
The following shows the Loading Form filled out with a few different load conditions. If Load Type = Acoustic, Load Entity can only reference elements and the default direction for the load application is relative to the element normal regardless of the Coord Frame selection. The Basic coordinate system is the default reference (COORD 0), unless, the element was defined in a local coordinate system, in which case that Coord ID will appear in the Coord Frame column. If the user changes the Direction from NORMAL to a specific direction vector, then the applied pressure direction is relative to the Coord Frame referenced. If Load Type = Force, Load Entity can only reference nodes (grid points), and a direction vector is input to define application direction relative to the coordinate frame reference. If no coordinate reference frame is specified, the default becomes the Basic Coordinate system (Coord 0). If Load Type = Displacement, Velocity, or Acceleration, Load Entity can only be selected from nodes that will appear in the Load Entities list box. These nodes represent the set of all possible nodes to which enforced motion can be applied, and is limited to nodes that were constrained during the normal modes analysis. The Basic coordinate system is the default reference (COORD 0), unless, the node was defined in a local coordinate frame, in which case that Coord ID will appear in the Coord Frame column. When Load Type = Displacement, Velocity, or Acceleration, and a specific node has been selected in Load Entities, the Direction specification will indicate which directions are available X, Y, and / or Z in
Chapter 3: Running an Analysis 475 Interactive Analysis
the reference coordinate frame. When an enforced motion is defined for a selected degree of freedom, it is eliminated from the available enforced motion set. Only one enforced motion boundary condition per degree of freedom can be applied to a given node. (Enforced motion cannot be applied to rotational degrees of freedom for interactive analysis).
476
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Create a Field Form This form appears when you select the Create New Field/Table... button from the Loading Form.
Chapter 3: Running an Analysis 477 Interactive Analysis
Output Selection Form This form will allow the user to select nodes and elements for output, and allow him to select the frequencies which interest him in the analysis. The frequency selection form is the same form that is used in standard analysis for sol 111 subcase parameters.
Define Frequencies prompts a spreadsheet for defining the desired solution frequencies for which output will be available. Output Selection also provides for selecting Nodes / Grids and Elements for which output response is desired. Selection can be made to create output response for complex quantities in either Real / Imaginary or Magnitude / Phase formats. For Interactive Analysis, the output quantities are preset. Close the Output Selection menu.
Define Frequencies Form This form allows the user to define the frequencies of interest in the most complete way. This form allows the users access to FREQ, FREQ1, FREQ2, FREQ3, FREQ4, FREQ5.
478
Patran Interface to MD Nastran Preference Guide Interactive Analysis
Chapter 4: Read Results Patran Interface to MD Nastran Preference Guide
4
Read Results
Accessing Results
492
Supported OUTPUT2 Result and Model Quantities
Supported T16/T19 Results Quantities
Supported MSC.Access Result Quantities
Supported 3dplot Results Quantities
511
543
516
502
492
Patran Interface to MD Nastran Preference Guide Accessing Results
4.1
Accessing Results This form appears when the Analysis toggle is selected on the main menu and the Action is set to Access Results. The Object you select defines the type of results file to be read or accessed from the analysis. The following file types are available: XDB, Output2, MASTER, T16/T19 and 3dplot (for SOL 700). The Method choices are: Result Entities, Model Data, or Both.
When the Object selected is Result Entities, the model data must already exist in the database. No results can be read into Patran if the associated node or element does not already exist. Model Data only reads the model data that exists in the results file. Both will first read the model data, then the result entities. If Model Data or Both are selected, it is up to the user to ensure that there will not be any ID conflicts with existing model entities.
Defines the job name to be used for this job. The same job name used for the Analysis menu should be used for the Read Results menu. This will allow Patran to load the results directly into the load cases that were used for the analysis.
Defines the results file to be read. The form that is called up lists all files recognized as being analysis code results files. By default this is all files with an op2 extension on them. This can be changed with the filter. If you are attaching a T16/T19 file that has the same jobname as your current database, you do not have to select the file. Patran automatically attaches the T16/T19 file that matches the database jobname. Defines any parameters used to control the results or model translation from the analysis code results file.
Chapter 4: Read Results 493 Accessing Results
Results File Formats Output2 Formats The Patran MD Nastran interface supports several different OUTPUT2 file formats. The interface, running on any platform can read a binary format OUTPUT2 file produced by MSC. Nastran running on any of these same platforms. For example, a binary OUTPUT2 file produced by MD Nastran running on an IBM RS/6000 can be read by Patran running on DEC Alpha. Patran may be able to read binary format OUTPUT2 files from other platforms if they contain 32 bit, IEEE format entities (either Big or Little Indian). For platforms that do not produce OUTPUT2 files in these formats, Patran MD Nastran can read OUTPUT2 files created with the FORM=FORMATTED option in MD Nastran. This option can be selected from the Analysis/Translation Parameters form in Patran and directs MD Nastran to produce an ASCII format OUTPUT2 file that can be moved between any platforms. The Patran MD Nastran interface detects this format when the OUTPUT2 file is opened, automatically converts it to the binary format, and then reads the model and/or results into the Patran database. An OUTPUT2 file is created by MD Nastran by placing a PARAM,POST,-1 in the bulk data portion of the input file. The formatted or unformatted OUTPUT2 file is specified in the FMS section using an ASSIGN OUTPUT2 = filename, UNIT=#, FORM=FORMATTED (or UNFORMATTED). See Translation Parameters, 265. XDB Formats The same basic issues exist for MSC.Access databases as for OUTPUT2 files. For example, the MSC.Access database (xdb file) may be exchanged between computer Systems that have binary compatibility. That is, an XDB file generated on a SUN Machine may be used on an IBM/AIX, HPUX or SGI computers. However, in order to exchange the XDB file on binary incompatible machines, one needs to use the TRANS and RECEIVE utilities delivered with every installation of MD Nastran. TRANS converts an XDB file generated by MD Nastran to an “equivalent” character, i.e. ASCII, file which can be transported to another computer across the network via ftp or rcp. RECEIVE converts the character file back into the XDB format for postprocessing. For more information on TRANS and RECEIVE utilities, please consult the “Configuration and Operations Guide” for V70 of MSC.Nastran. A MSC.Access XDB database is created by MD Nastran by placing a PARAM,POST,0 in the bulk data portion of the input file. See Translation Parameters, 265. In this release of the product, it is assumed that the Geometry, loads and results output all reside in the same physical XDB file. That is, "split" XDB databases are not supported.
494
Patran Interface to MD Nastran Preference Guide Accessing Results
MASTER Formats Using the MASTER format, you can attach to the MD Nastran database directly saving the extra step of creating alternate form of MD Nastran model and results data, i.e. OP2 and/or XDB. Because the model and results data in the MD Nastran database tends be sequential in nature, an index provides fast “direct” access to the data. The indexing is accomplished by two indexing modules in MD Nastran named: ifpindx and ofpindx. The DRA/DBALL capability uses the MD Nastran toolkit, i.e. MNT, capability. The MNT interfaces with the MD Nastran executable in a client-server. This means that in order to use the DRA/DBALL feature one needs to have access to MD Nastran installation. If you do not have access to a MD Nastran installation you will need to use the MD Nastran mini server that is delivered with Patran to import DRA/DBALL files. To point to a MD Nastran installation, the location of the MD Nastran executable is set in the following files: p3_trans.ini(NT), .site_setup(UNIX,LINUX). On Windows NT, the “ACommand20xx” must be set to the MD Nastran executable. On UNIX, on the other hand, “MSP_NASTRAN_CMD20xx” needs to be set to the MD Nastran executable. To point to a MD Nastran mini server, the location of the MD Nastran mini server executable must be set on Windows with the “AcommandNasServer” environment variable. On UNIX, you must set the environment variable “MSCP_NASTRAN_SERVER” . By default the MD Nastran mini server is located in $P3_Home/mscnastran_files/servermode/nastran.exe. Note that you are required to point to a V2004 or later version of MD Nastran. If you specify an MSC.Nastran executable earlier than V2004 you will be presented with a modal form preventing you from using this capability. However, you may bypass this restriction by setting the “DRA_NAST_NOVEDRCHK” environment variable. The DRA/MASTER functionality only supports static analysis (SOL101). This includes the support of Superelements, grid point forces and other result types available in the OP2 or XDB translators. This capability supports importing the model data into Patran database. Moreover, since this capability reuses the import/bdf functionality all of the model information available in the database shall be imported including Nodes, Elements, Coordinate systems, material properties, physical properties, loads and boundary conditions, load cases, parameters and etc... The “indexing” modules are tied to a system cell. That is, an MD Nastran database is indexed and saved by MD Nastran by setting system cell “316” to a value “7”. This system cell tells MD Nastran executable to create index files for IFP and OFP datablocks and move the indexed datablocks to the “MASTER” file. This means that one can even delete the “DBALL” file after the MD Nastran run completes. For example, if you would like to get an Indexed MASTER data file for the job some_job.bdf, the following must be executed: < ...>/nastran some_job.bdf sys316=7 scr=no sdir=/tmp This example generates a “some_job.MASTER and some_job.DBALL database files. You can delete the *.DBALL file because it does not contain any results or model data of importance. However, if you would like to perform a restart from the run then the DBALL file must be kept for future use but the “Master” file may be moved to other directories at will.
Chapter 4: Read Results 495 Accessing Results
The MD Nastran toolkit environment is derived from the MD Nastran installation via the use of the “rc” files which is documented in the MSC.Nastran (p. 1) in the MSC.Nastran 2004 Installation and Operations Guide. For example, you can set the amount of memory used by the MD Nastran to 20 megawords by setting the “memory=20MW” in one of the “rc” files, i.e. nastran.rcf file in the current working directory on the NT platform. This setting can be double checked using the MD Nastran “whence” command as follows: < ...>/nastran some_job.bdf whence=mem The same basic issues exist for attaching to an Indexed MD Nastran database as attaching an XDB database. That is, the MD Nastran database (MASTER file) may be exchanged among computer Systems that have binary compatibility. That is, a MASTER file generated on a SUN Machine can not be used on an IBM/AIX, HPUX or SGI computers. However, at this time it is not possible to exchange the MASTER file on binary incompatible machines. T16/T19 Formats The T16 file is the MSC.Marc binary results file and the T19 file is the MSC.Marc ASCII results (POST) file that are created by a SOL 600 analysis, the contents of which can be imported or attached for postprocessing. When domain decomposition is used, multiple files are produced where # is the domain number. This file format is recommended for post-processing SOL 600 runs since it has more information, such as contact info and additional nonlinear analysis information, then the xdbor OP2 formats. These results file types are used for accessing SOL 600 results. 3dplot Formats The 3dplot ptf file is the LS-Dyna binary results file that are created by a SOL 700 analysis, the contents of which can be attached for postprocessing. This option is available only for Explicit Nonlinear.
496
Patran Interface to MD Nastran Preference Guide Accessing Results
Translation Parameters OUTPUT2 This subordinate form appears when the Translation Parameters button is selected and Read Output2 is the selected Object. When reading results there are three Method options that may be selected: Result Entities, Model Data or Both. This form affects import of all these objects as noted below
Tolerances • Division • Numerical
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available.
Chapter 4: Read Results 497 Accessing Results
MSC.Nastran Version
Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation.
• P-element P-order Field
Creates a field that describes the polynomial orders in all p-elements in the model at the end of an adaptive cycle.
Element Results Positions
If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
Defining Translation Parameters for DDAM (SOL 187) Patran calculates combined stresses (like bar stresses, principal stresses and von Mises stresses by default, rather than reading these values from the OP2 files. If Patran does this, the combined stresses will be incorrectly calculated from summed results. It is necessary to calculate the combined stresses on a mode-by-mode basis, and NRL sum the combined results. To obtain correct results, it is necessary to explicitly tell Patran to read the combined values. Select the Translation Parameters button on the Analysis form when reading results in. On the form, you can select the box labeled Stress/Strain Invariants. This produces a number of additional results for each result case. These additional results are the correct von Mises and Principal stresses. The ones that Patran displays when you choose Stress Tensor are the incorrect values.
498
Patran Interface to MD Nastran Preference Guide Accessing Results
XDB This subordinate form appears when the Translation Parameters button is selected and Result Entities is the selected Object.
Tolerances • Division • Numerical
MSC.Nastran Version
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available. Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Chapter 4: Read Results 499 Accessing Results
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Element Results Positions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation. If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
MASTER This subordinate form appears when the Translation Parameters... button is selected and MASTER is the selected Object.
500
Patran Interface to MD Nastran Preference Guide Accessing Results
Tolerances • Division • Numerical
MSC.Nastran Version
Defines the tolerances used during translation. The division tolerance is used to prevent division by zero errors. The numerical tolerance is used when comparing real values for equality. When the Object is set to Model Data, only these tolerances are available. Specifies the version of MSC .Nastran that created the OUTPUT2 file to be read. Solid Element orientation differs between versions less than 67 and version 67 and above. Elementally oriented Solid element results may be translated incorrectly if the wrong version is specified.
Additional Results to be Imported • Rotational Nodal Results • Stress/Strain Invariants • Principal Directions
Indicates which results categories are to be filtered out during translation. Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Principal Direction Results can be skipped during translation. Items selected will be translated. Items not selected will be skipped. By default, Rotational Nodal Results, Stress and Strain Invariants, and Stress and Strain Tensor Principal Directions are ignored during translation.
• P-element P-order Field
Creates a field that describes the polynomial orders in all p-elements in the model at the end of an adaptive cycle.
Element Results Positions
If an element has results at both the centroid and at the nodes, this filter will indicate which results are to be included in the translation.
Chapter 4: Read Results 501 Accessing Results
T16/T19 This subordinate form appears when the Translation Parameters... button is selected and T16/T19 is the selected Object.
Model Import Options • Create Groups by PIDs
Creates groups for each element type encountered in the model.
• Geometry Import
Imports any NURB based rigid geometry found in the POST file into the database.
Select Mesh
Pertains to importing results and model data from adaptive meshing analyses. In order for this toggle to be active, a results file must have been selected first in which case it is scanned to show the available meshes and to which load increments they are associated. You can select which meshes/increments are imported in the provided list box. Adaptive meshing is not supported in MSC.Nastran 2004.
Available Increments
Defines the increments available for import from the results file.
502
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
4.2
Supported OUTPUT2 Result and Model Quantities The following table indicates all the possible results quantities that can be loaded into the Patran database during results translation from MD Nastran. The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor, and determines which postprocessing techniques are available to view the results quantity. Data Block indicates which MD Nastran OUTPUT2 data block the data comes from. The Description gives a brief discussion about the results quantity, such as if it is only for certain element types, and what Output Request selection will generate this data block. For design optimization, all of the listed results can be loaded as a function of design cycle. Results
Primary Label
Secondary Label
Type
DataBlocks
Description
Acoustic
Intensity
Scalar
OAIG1
Acoustic intensity on surface in contact with fluid.
Acoustic
Radiated Power
Scalar
OARPWR1
Acoustic power radiated from surface in contact with fluid.
Acoustic
Field Point Mesh
Vector
OUGFP1
Acoustic results for Field Point Mesh.
Acoustic
Velocity @ FPM Grids
Vector
OVGFP1
Acoustic velocities at the node points of Field Point Mesh.
Bar Forces
Rotational
Vector
OEF1
Bar moments
Translational
Vector
OEF1
Bar forces
Warping Torque
Scalar
OEF1
Warping torque
Axial Safety Margin
Scalar
OSTR1
Axial safety margin
Compression Safety Margin
Scalar
OSTR1
Safety margin in compression
Maximum Axial
Scalar
OSTR1
Maximum axial strain
Minimum Axial
Scalar
OSTR1
Minimum axial strain
Tension Safety Margin
Scalar
OSTR1
Safety margin in tension
Torsional Safety Margin
Scalar
OSTR1
Safety margin in torsion
Axial Safety Margin
Scalar
OES1
Axial safety margin
Compression Safety Margin
Scalar
OES1
Safety margin in compression
Maximum Axial
Scalar
OES1
Maximum axial stress
Minimum Axial
Scalar
OES1
Minimum axial stress
Tension Safety Margin
Scalar
OES1
Safety margin in tension
Torsional Safety Margin
Scalar
OES1
Safety margin in torsion
Bar Strains
Bar Stresses
Chapter 4: Read Results 503 Supported OUTPUT2 Result and Model Quantities
Primary Label Grid Point Stresses
Secondary Label
Type
DataBlocks
Description
Stress Tensor
Tensor
OGS1
Stress tensor
Zero Shear Angle
Scalar
OGS1
Zero shear angle
Major Principal
Scalar
OGS1
Major principal
Minor Principal
Scalar
OGS1
Minor principal
Maximum Shear
Scalar
OGS1
Maximum shear
von Mises
Scalar
OGS1
von mises
Displacement
Vector
OEF1 or OES1
Gap element displacement
Force
Vector
OEF1 or OES1
Gap element force
Slip
Vector
OEF1 or OES1
Gap element slip
Creep Strain
Scalar
OESNL1
Creep strain
Plastic Strain
Scalar
OESNL1
Plastic strain
Strain Tensor
Tensor
OESNL1
Strain tensor
Nonlinear Stresses
Equivalent Stress
Scalar
OESNL1
Equivalent stress
Stress Tensor
Tensor
OESNL1
Stress tensor
Principal Strain Direction
1st Principal x cosine
Scalar
OSTR1
1st Principal x cosine
1st Principal y cosine
Scalar
OSTR1
1st Principal y cosine
1st Principal z cosine
Scalar
OSTR1
1st Principal z cosine
2nd Principal x cosine
Scalar
OSTR1
2nd Principal x cosine
2nd Principal y cosine
Scalar
OSTR1
2nd Principal y cosine
2nd Principal z cosine
Scalar
OSTR1
2nd Principal z cosine
3rd Principal x cosine
Scalar
OSTR1
3rd Principal x cosine
3rd Principal y cosine
Scalar
OSTR1
3rd Principal y cosine
3rd Principal z cosine
Scalar
OSTR1
3rd Principal z cosine
Zero Shear Angle
Scalar
OSTR1
Zero shear angle
Gap Results
Nonlinear Strains
504
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Principal Stress Direction
Shear Panel Forces
Shear Panel Strains
Shear Panel Stresses
Shell Forces
Secondary Label
Type
DataBlocks
Description
1st Principal x cosine
Scalar
OES1
1st Principal x cosine
1st Principal y cosine
Scalar
OES1
1st Principal y cosine
1st Principal z cosine
Scalar
OES1
1st Principal z cosine
2nd Principal x cosine
Scalar
OES1
2nd Principal x cosine
2nd Principal y cosine
Scalar
OES1
2nd Principal y cosine
2nd Principal z cosine
Scalar
OES1
2nd Principal z cosine
3rd Principal x cosine
Scalar
OES1
3rd Principal x cosine
3rd Principal y cosine
Scalar
OES1
3rd Principal y cosine
3rd Principal z cosine
Scalar
OES1
3rd Principal z cosine
Zero Shear Angle
Scalar
OES1
Zero shear angle
Force12
Scalar
OEF1
Shear force from nodes 1 to 2
Force14
Scalar
OEF1
Shear force from nodes 1 to 4
Force21
Scalar
OEF1
Shear force from nodes 2 to 1
Force23
Scalar
OEF1
Shear force from nodes 2 to 3
Force32
Scalar
OEF1
Shear force from nodes 3 to 2
Force34
Scalar
OEF1
Shear force from nodes 3 to 4
Force41
Scalar
OEF1
Shear force from nodes 4 to 1
Force43
Scalar
OEF1
Shear force from nodes 4 to 3
Kick
Scalar
OEF1
Kick forces
Rotational
Vector
OEF1
Moments at nodes
Shear
Scalar
OEF1
Shear force in panel
Translational
Vector
OEF1
Forces at nodes
Average Shear
Scalar
OSTR1
Average shear strain in panel
Maximum Shear
Scalar
OSTR1
Maximum shear strain in panel
Safety Margin
Scalar
OSTR1
Shear safety margin of panel
Average Shear
Scalar
OES1
Average shear stress in panel
Maximum Shear
Scalar
OES1
Maximum shear stress in panel
Safety Margin
Scalar
OES1
Shear safety margin of panel
Force Resultant
Tensor
OEF1
Force resultants and moment resultants
Moment Resultant
Tensor
OEF1
Moment stress resultants
Chapter 4: Read Results 505 Supported OUTPUT2 Result and Model Quantities
Primary Label Strain Curvatures
Secondary Label
Type
DataBlocks
Description
Strain Tensor
Tensor
OSTR1
Strain curvatures of a plate
1st Principal
Scalar
OSTR1
Curvature of strain 1st principal
2nd Principal
Scalar
OSTR1
Curvature of strain 2nd principal
Maximum Shear
Scalar
OSTR1
Curvature of maximum shear strain
von Mises
Scalar
OSTR1
Curvature of von Mises strain
Zero Shear Angle
Scalar
OSTR1
Curvature of zero shear angle
Energy
Scalar
ONRGY1
Element’s total strain energy
Energy Density
Scalar
ONRGY1
Element’s strain energy density
Percent of Total
Scalar
ONRGY1
Element’s percentage of total strain density
1st Principal
Scalar
OSTR1
Strain 1st principal
2nd Principal
Scalar
OSTR1
Strain 2nd principal
3rd Principal
Scalar
OSTR1
Strain 3rd principal
Maximum Shear
Scalar
OSTR1
Maximum shear strain
Mean Pressure
Scalar
OSTR1
Mean strain pressure
Octahedral Shear
Scalar
OSTR1
Octahedral shear strain
von Mises
Scalar
OSTR1
von Mises equivalent strain
Strain Tensor
NONE
Tensor
OSTR1
Strain tensor
Stress Invariants
1st Principal
Scalar
OES1
Stress 1st Principal
2nd Principal
Scalar
OES1
Stress 2nd Principal
3rd Principal
Scalar
OES1
Strain 3rd Principal
Maximum Shear
Scalar
OES1
Maximum shear stress
Mean Pressure
Scalar
OES1
Mean stress principal
Octahedral Shear
Scalar
OES1
Octahedral shear stress
von Mises
Scalar
OES1
von Mises equivalent stress
Stress Tensor
NONE
Tensor
OES1
Stress tensor
Accelerations
Rotational
Vector
OUGV1
Nodal angular accelerations
Translational
Vector
OUGV1
Nodal translational accelerations
Rotational
Vector
OPG1
Nodal equivalent applied moments
Translational
Vector
OPG1
Nodal equivalent applied forces
Strain Energy
Strain Invariants
Applied Loads
506
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Constraint Forces
Displacements
Eigenvectors Nonlinear Applied Loads
Secondary Label
Type
DataBlocks
Description
Rotational
Vector
OQG1
Nodal moments of single-point constraints
Translational
Vector
OQG1
Nodal forces of single-point constraint
Rotational
Vector
OUGV1
Nodal rotational displacements
Translational
Vector
OUGV1
Nodal translational displacements
Rotational
Vector
OPHIG
Nodal rotational eigenvectors
Translational
Vector
OPHIG
Nodal translational eigenvectors
Rotational
Vector
OPNL1
Nodal nonlinear applied moments
Chapter 4: Read Results 507 Supported OUTPUT2 Result and Model Quantities
Primary Label
Secondary Label
Type
DataBlocks
Description
Translational
Vector
OPNL1
Nodal nonlinear applied forces
Rotational
Vector
OUGV1
Nodal angular velocity
Translational
Vector
OUGV1
Nodal translational velocity
Error
Estimate
Scalar
ERROR
Elemental error in adaptive analysis
Grid Point Forces
Elements
Vector
OGPFB1*
Internal nodal force contribution by element
Applied Loads
Vector
OGPFB1*
Nodal equivalent applied forces
Constraint Forces
Vector
OGPFB1*
Nodal equivalent constraint forces
Total
Vector
OGPFB1*
Total nodal equivalent forces due to internal loads, applied loads and constraint forces.
Elements
Vector
OGPFB1*
Internal nodal moment contribution by element
Applied Loads
Vector
OGPFB1*
Nodal equivalent applied moments
Constraint Forces
Vector
OGPFB1*
Nodal equivalent constraint moments
Total
Vector
OGPFB1*
Total nodal equivalent moments due to internal loads, applied loads and constraint forces.
None
Vector
GEOMIN
In a shape optimization run, this is the new shape displayed as a deformation of the original shape.
Velocities
Grid Point Moments
Shape Change
508
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
Primary Label Active Constraints
Secondary Label
Type
DataBlocks
Description
Element Stress
Scalar
R1TABRG
Element stress
Element Strain
Scalar
R1TABRG
Element strain
Element Force
Scalar
R1TABRG
Element force
Element Ply Failure
Scalar
R1TABRG
Element ply failure
Translational Displacement
Vector
R1TABRG
Nodal translational displacement
Rotational Displacement
Vector
R1TABRG
Nodal rotational displacement
Translational Velocity
Vector
R1TABRG
Nodal translational velocity
Rotational Velocity
Vector
R1TABRG
Nodal rotational velocity
Translational Acceleration
Vector
R1TABRG
Nodal translational acceleration
Rotational Acceleration
Vector
R1TABRG
Nodal rotational acceleration
Translational SPC
Vector
R1TABRG
Nodal translational SPC force
Rotational SPC
Vector
R1TABRG
Nodal rotational SPC force
Global Variables In addition to standard results quantities, a number of Global Variables can be created. This table outlines Global Variables that may be created. Global Variables are results quantities where one value is representative of the entire model. Labels
Type
DataBlocks
Description
Critical Load Factor
S
Oxxx
Value of buckling load for the given buckling mode.
Time
S
Oxxx
Time value of the time step.
Frequency
S
Oxxx
Frequency value of the frequency step or for the normal mode.
Damping Ratio
S
Oxxx
Damping ratio value of a complex eigenvalue analysis.
Eigenvalue
S
Oxxx
Eigenvalue for normal modes or complex eigenvalue analysis.
Percent of Load
S
Oxxx
Percent of load value for a nonlinear static analysis.
Adaptive Cycle
S
Oxxx
Cycle number in p-adaptive analysis.
Design Cycle
S
Oxxx
Cycle number in an optimization run (SOL 200).
Design Variable
S
DESTAB HISADD
Design Variable for optimization (Label from DESTAB, value from HISADD).
Maximum Constraint Value
S
HISADD
Maximum constraint value for optimization.
Objective Function
S
HISADD
Objective function for optimization.
Chapter 4: Read Results 509 Supported OUTPUT2 Result and Model Quantities
Coordinate Systems In some cases, the elemental stresses and strains are transformed from one coordinate frame to another when imported into the Patran database. The following describes the coordinate systems for these element results after they are imported into the Patran database. The coordinate system names referred to are described in the Patran or the MD Nastran documentation. CTRIA3
Table 4-1 Results are in the MD Nastran system which coincides with the Patran IJK system. At the user’s request during postprocessing, these results can be transformed by Patran to alternate coordinate systems. If the user selects a component of a stress or strain tensor to be displayed, by default, the Results application transforms the tensor to a projected global system (Projected Global System).
CQUAD4
Table 4-2 Results are in the MD Nastran “bisector” coordinate system but may be transformed by Patran to alternate coordinate systems (e.g., global) during postprocessing. If the user selects a component of a stress or strain tensor to be displayed, by default, the Results application transforms the tensor to a projected global system (Projected Global System). Import of results when this element is used in a hyperelastic analysis is not currently supported.
CHEXA, CPENTA, CTETRA
Table 4-3 The user can request that MD Nastran compute element results in either a local element or alternate coordinate system via the PSOLID entry. If the element results are in the local element system, these are converted to the Patran IJK system on import. If the results are in a system other than local element, they are imported in this system. These results may be transformed to alternate systems during postprocessing.
CQUAD8, CTRI6
Table 4-4 The elemental coordinate system, used by MD Nastran for results, is described in the MD Nastran documentation. These results are imported into the Patran database “asis”. These results can be postprocessed in Patran using the “As Is” options, but they cannot be transformed to alternate coordinate systems. Projected Global System The projected system is defined as follows. First, the normal to the shell surface is calculated. This varies for curved elements and is constant for flat elements. If the angle between the normal and the global xaxis is greater than .01 radians, the global x-axis is projected onto the shell surface as the local x-axis. If the angle is less than .01 radians, either the global y-axis or the z-axis (whichever makes the largest angle with the normal) is defined to be the local x-axis. The local y-axis is perpendicular to the plane defined by the normal and the local x-axis. XY Plots For results from MD Nastran design optimization solution 200 runs, three XY Plots are generated, but not posted, when the Read OUTPUT2 option is selected: 1. Objective Function vs. Design Cycle. 1. Maximum Constraint Value vs. Design Cycle. 1. Design Variable vs. Design Cycle.
510
Patran Interface to MD Nastran Preference Guide Supported OUTPUT2 Result and Model Quantities
These plots can be viewed under the XY Plot option in (p. 1) in the MSC.Patran User’s Guide. When they are initially posted, you will have to expand their windows to view them properly. Model Data The following table outlines all the data that will be created in the Patran database when reading model data from an MD Nastran OUTPUT2 file and the location in the OUTPUT2 file from where it is derived. This is the only data extracted from the OUTPUT2 file. This data should be sufficient for evaluating results values. Item Nodes
Block GEOM1
Description Node ID Nodal Coordinates Reference Coordinate Frame Analysis Coordinate Frame
Coordinate Frames
GEOM1
Coordinate Frame ID Transformation Matrix Origin Can be Rectangular, Cylindrical, or Spherical
Elements
GEOM2
Element ID Topology (e.g., Quad/4 or Hex20) Nodal Connectivity
Chapter 4: Read Results 511 Supported T16/T19 Results Quantities
4.3
Supported T16/T19 Results Quantities The following table indicates all the possible result quantities which can be loaded into the Patran database from the t16 file. The Primary and Secondary Labels are items selected from the postprocessing menus. The Type indicates whether the results are Scalar, Vector, or Tensor. These types will determine which postprocessing techniques will be available in order to view the results quantity. Postcodes indicates which MSC.Marc element postcodes (selected automatically or by MD Nastran Bulk Data entry MARCOUT) the data comes from. The Description gives a brief discussion about the results quantity. The Output Request forms use the actual primary and secondary labels which 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.
Primary Label
Secondary Label
Type
Postcodes
Description
Displacement
Translation
Vector
1 (nodal)
Translational displacements at nodes from a structural analysis.
Displacement
Rotation
Vector
2 (nodal)
Rotational displacements at nodes from a structural analysis.
Velocity
Translation
Vector
28 (nodal)
Translational velocities at nodes from a dynamic analysis.
Velocity
Rotation
Vector
29 (nodal)
Rotational velocities at nodes.
Acceleration
Translation
Vector
30 (nodal)
Translational accelerations at nodes from a dynamic analysis.
Acceleration
Rotation
Vector
31 (nodal)
Rotational accelerations at nodes from a dynamic analysis.
Force
Nodal External Applied
Vector
3 (nodal)
Forces applied to the model in a structural analysis.
Force
Nodal Reaction
Vector
5 (nodal)
Reaction forces at boundary conditions from a structural analysis.
Moment
Nodal External Applied
Vector
4 (nodal)
Moments applied to the model in a structural analysis.
Moment
Nodal Reaction
Vector
6 (nodal)
Reaction moments at boundary conditions from a structural analysis.
Modal Mass
Translation
Vector
32 (nodal)
Translational modal masses from modal extractions.
Modal Mass
Rotation
Vector
33 (nodal)
Rotational modal masses from modal extractions.
Temperature
Nodal
Scalar
14 (nodal)
Temperature at nodes from a thermal analysis.
Velocity
Fluid
Vector
7 (nodal)
Fluid Velocity
512
Patran Interface to MD Nastran Preference Guide Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Flux
Nodal
Scalar
15 (nodal)
Heat Flux applied to the model in a thermal analysis.
Pressure
Fluid
Scalar
8 (nodal)
Fluid Pressure
Force
External Fluid
Vector
9 (nodal)
External Fluid Force
Force
Reaction Fluid
Vector
10 (nodal)
Reaction Fluid Force
Pressure
Sound
Scalar
11 (nodal)
Sound Pressure
Source
External Sound
Scalar
12 (nodal)
External Sound Source
Source
Reaction Sound
Scalar
13 (nodal)
Reaction Sound Source
Flux
Nodal Reaction
Scalar
16 (nodal)
Nodal Reaction Flux
Potential
Electric
Scalar
17 (nodal)
Electric Potential
Charge
External Electric
Scalar
18 (nodal)
External Electric Charge
Charge
Reaction Electric
Scalar
19 (nodal)
Reaction Electric Charge
Potential
Magnetic
Scalar
20 (nodal)
Magnetic Potential
Current
External Electric
Scalar
21 (nodal)
External Electric Current
Current
Reaction Electric
Scalar
22 (nodal)
Reaction Electric Current
Pressure
Pore
Scalar
23 (nodal)
Pore Pressure
Flux
External Mass
Scalar
24 (nodal)
External Mass Flux
Flux
Reaction Mass
Scalar
25 (nodal)
Reaction Mass Flux
Pressure
Bearing
Scalar
26 (nodal)
Bearing Pressure
Force
Bearing
Scalar
27 (nodal)
Bearing Force
Stress
Contact Normal
Vector
34 (nodal)
Contact Normal Stress
Force
Contact Normal
Vector
35 (nodal)
Contact Normal Force
Stress
Friction
Vector
36 (nodal)
Friction Stress
Force
Friction
Vector
37 (nodal)
Friction Force
Contact
Status
Scalar
38 (nodal)
Contact Status
Contact
Touched Body
Scalar
39 (nodal)
Touched Body Contact
Variable
Herrmann
Scalar
40 (nodal)
Herrmann Variable
Post Code
No. -11 through -16
Tensor
-11 thru -16, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -21 through -23
Vector
-21 thru -23, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -31
Scalar
-31, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Chapter 4: Read Results 513 Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Post Code
No. -41
Scalar
-41, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Post Code
No. -51
Scalar
-51, (nodal)
User defined nodal quantities via user subroutine UPSTNO.
Strain
Cracking
Tensor
81-86 or 381
Cracking strain from a nonlinear structural analysis.
Strain
Creep
Tensor
31-36 or 331
Creep strain from a nonlinear structural analysis.
Strain
Creep Equivalent
Scalar
37
Equivalent creep strain from a nonlinear structural analysis.
Strain
Creep Equivalent (from rate)
Scalar
8
Equivalent creep strain determined from rate from a nonlinear structural analysis.
Strain
Elastic
Tensor
121-126 or 401
Elastic strain from a structural analysis.
Strain
Elastic Equivalent
Scalar
127
Equivalent elastic strain from a structural analysis.
Strain
Plastic
Tensor
21-26 or 321
Plastic strain from a nonlinear structural analysis.
Strain
Plastic Equivalent
Scalar
27
Equivalent plastic strain from a nonlinear structural analysis.
Strain
Plastic Equivalent (from rate)
Scalar
7
Equivalent plastic strain determined from rate from a nonlinear structural analysis.
Strain
Plastic Equivalent Rate
Scalar
28
Equivalent plastic strain rate from a nonlinear structural analysis.
Strain
Thermal
Tensor
71-76 or 371
Thermal strain from a structural analysis.
Strain
Thickness
Scalar
49
Thickness strain from a structural analysis.
Strain
Total
Tensor
1-6 or 301
Total strain from a structural analysis.
Temperature
Element
Scalar
9
Element temperature from a thermal or structural analysis.
Temperature
Element Gradient
Vector
181-183
Element temperature gradient from a thermal analysis.
Temperature
Element Incremental Scalar
10
Incremental element temperature from a thermal or structural analysis.
Tensor
11-16 or 311
Stress from a structural analysis.
Tensor
41-46 or 341
Cauchy stress from a nonlinear structural analysis.
Stress Stress
Cauchy
514
Patran Interface to MD Nastran Preference Guide Supported T16/T19 Results Quantities
Primary Label
Secondary Label
Type
Postcodes
Description
Stress
Cauchy Equivalent Mises
Scalar
47
Equivalent Cauchy stress from a nonlinear structural analysis.
Stress
Equivalent Mises
Scalar
17
Equivalent (von mises) stress from a structural analysis.
Stress
Hydrostatic
Scalar
18
Hydrostatic stress from a structural analysis.
Stress
Interlaminar Shear No. 1
Scalar
108
Interlaminar shear in one direction from a structural analysis.
Stress
Interlaminar Shear No. 2
Scalar
109
Interlaminar shear in two direction from a structural analysis.
Energy Density
Elastic
Scalar
48
Elastic strain energy density from a structural analysis.
Energy Density
Plastic
Scalar
58
Plastic strain energy density from a nonlinear structural analysis.
Energy Density
Total
Scalar
68
Total strain energy density from a structural analysis.
Flux
Element
Vector
184-186
Element heat flux from a thermal analysis.
State Variable
Second
Scalar
29
Second state variable from a nonlinear thermal or structural analysis.
State Variable
Third
Scalar
39
Third state variable from a nonlinear thermal or structural analysis.
Failure
Index No. 1
Scalar
91
Failure index one from a structural analysis.
Failure
Index No. 2
Scalar
92
Failure index two from a structural analysis.
Failure
Index No. 3
Scalar
93
Failure index three from a structural analysis.
Failure
Index No. 4
Scalar
94
Failure index four from a structural analysis.
Failure
Index No. 5
Scalar
95
Failure index five from a structural analysis.
Failure
Index No. 6
Scalar
96
Failure index six from a structural analysis.
Failure
Index No. 7
Scalar
97
Failure index seven from a structural analysis.
Thickness
Scalar
20
Element thickness from a thermal or structural analysis.
Volume
Scalar
78
Element Volume from a thermal or structural analysis.
Chapter 4: Read Results 515 Supported T16/T19 Results Quantities
In addition to these standard results quantities, several Global Variable results can be created. Global Variables are results quantities where one value is representative of the entire model. The following table defines the Global Variables which may be created. Global Variable Label
Type
Description
Increment
Scalar
Increment of the analysis.
Time
Scalar
Time of the analysis.
Buckling Mode
Scalar
Buckling mode number.
Critical Load Factor
Scalar
Critical load factor for buckling analysis.
Dynamic Mode
Scalar
Dynamic mode number from modal extraction.
Frequency (radians/time)
Scalar
Frequency in radians per unit time for modal extraction.
516
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
4.4
Supported MSC.Access Result Quantities The following tables list the currently supported quantities from the MSC.Access database (xdb file).To get further information on the MSC.Access, i.e. XDB, objects supported in Patran, please use the ddlprt and ddlqry utilities delivered with every installation of MD Nastran. ddlprt is MSC.Access' on-line documentation. ddlqry is MSC.Access’ Data Definition Language (DDL) browser. See “Configuration and Operations Guide” for MSC.Nastran V70. Nodal Results
Primary Label Displacements
Eigenvectors
Velocities
Secondary Label
Type
Objects
Translational
VECTOR
DISPR
Rotational
VECTOR
DISPR
Translational
VECTOR
DISPRI
Rotational
VECTOR
DISPRI
Translational
VECTOR
DISPMP
Rotational
VECTOR
DISPMP
Translational
VECTOR
DISPR
Rotational
VECTOR
DISPR
Translational
VECTOR
DISPRI
Rotational
VECTOR
DISPRI
Translational
VECTOR
DISPMP
Rotational
VECTOR
DISPMP
Translational
VECTOR
VELOR
Rotational
VECTOR
VELOR
Translational
VECTOR
VELORI
Rotational
VECTOR
VELORI
Translational
VECTOR
VELOMP
Rotational
VECTOR
VELOMP
Chapter 4: Read Results 517 Supported MSC.Access Result Quantities
Primary Label Accelerations
Constraint Forces
Applied Loads
Grid Point Stresses
Secondary Label
Type
Objects
Translational
VECTOR
ACCER
Rotational
VECTOR
ACCER
Translational
VECTOR
ACCERI
Rotational
VECTOR
ACCERI
Translational
VECTOR
ACCEMP
Rotational
VECTOR
ACCEMP
Translational
VECTOR
SPCFR
Rotational
VECTOR
SPCFR
Translational
VECTOR
SPCFRI
Rotational
VECTOR
SPCFRI
Translational
VECTOR
SPCFMP
Rotational
VECTOR
SPCFMP
Translational
VECTOR
LOADR
Rotational
VECTOR
LOADR
Translational
VECTOR
LOADRI
Rotational
VECTOR
LOADRI
Translational
VECTOR
LOADMP
Rotational
VECTOR
LOADMP
Stress Tensor
TENSOR
SGSVR
Zero Shear Angle
SCALAR
SGSVR
Major Principal
SCALAR
SGSVR
Minor Principal
SCALAR
SGSVR
Maximum Shear
SCALAR
SGSVR
Von Mises
SCALAR
SGSVR
518
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Grid Point Stresses
Grid Point Strains
Secondary Label
Type
Objects
Stress Tensor
TENSOR
SGVVR
Mean Pressure
SCALAR
SGVVR
Octahedral Shear
SCALAR
SGVVR
Major Principal
SCALAR
SGVVR
Intermediate Principal
SCALAR
SGVVR
Minor Principal
SCALAR
SGSVR
Major Prin x cosine
SCALAR
SGSVR
Intermed Prin x cosine
SCALAR
SGSVR
Minor Prin x cosine
SCALAR
SGSVR
Major Prin y cosine
SCALAR
SGSVR
Intermed Prin y cosine
SCALAR
SGSVR
Minor Prin y cosine
SCALAR
SGSVR
Major Prin z cosine
SCALAR
SGSVR
Intermed Prin z cosine
SCALAR
SGSVR
Minor Prin z cosine
SCALAR
SGSVR
Strain Tensor
TENSOR
EGSVR
Zero Shear Angle
SCALAR
EGSVR
Major Principal
SCALAR
EGSVR
Minor Principal
SCALAR
EGSVR
Maximum Shear
SCALAR
EGSVR
Von Mises
SCALAR
EGSVR
Chapter 4: Read Results 519 Supported MSC.Access Result Quantities
Primary Label Grid Point Strains
GPS discontinunities
Secondary Label
Type
Objects
Strain Tensor
TENSOR
EGVVR
Mean Pressure
SCALAR
EGVVR
Octahedral Shear
SCALAR
EGVVR
Major Principal
SCALAR
EGVVR
Intermediate Principal
SCALAR
EGVVR
Minor Principal
SCALAR
EGSVR
Major Prin x cosine
SCALAR
EGSVR
Intermed Prin x cosine
SCALAR
EGSVR
Minor Prin x cosine
SCALAR
EGSVR
Major Prin y cosine
SCALAR
EGSVR
Intermed Prin y cosine
SCALAR
EGSVR
Minor Prin y cosine
SCALAR
EGSVR
Major Prin z cosine
SCALAR
EGSVR
Intermed Prin z cosine
SCALAR
EGSVR
Minor Prin z cosine
SCALAR
EGSVR
Stress Tensor
TENSOR
SGSDTR
Major Principal
SCALAR
SGSDTR
Minor Principal
SCALAR
SGSDTR
Maximum Shear
SCALAR
SGSDTR
Von Mises
SCALAR
SGSDTR
Error Estimate
SCALAR
SGSDTR
Stress Tensor
TENSOR
SGVDTR
Mean Pressure
SCALAR
SGVDTR
Octahedral Shear
SCALAR
SGVDTR
Major Principal
SCALAR
SGVDTR
Intermediate Principal
SCALAR
SGVDTR
Minor Principal
SCALAR
SGVDTR
Error Estimate Direct
SCALAR
SGVDTR
Error Estimate Principal
SCALAR
SGVDTR
520
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Elem Stress discontinunities Stress Tensor
MPC Constraint Forces
Type
Objects
TENSOR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Major Principal
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Minor Principal
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Maximum Shear
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Von Mises
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Error Estimate
SCALAR
DQD4VR, DQD8VR, DQDRVR, DTR6VR, DTRRVR
Stresss Tensor
TENSOR
DHEXVR, DPENVR, DTETVR
Mean Pressure
SCALAR
DHEXVR, DPENVR, DTETVR
Octahedral Shear
SCALAR
DHEXVR, DPENVR, DTETVR
Major Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Intermediate Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Minor Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Error Estimate Direct
SCALAR
DHEXVR, DPENVR, DTETVR
Error Estimate Principal
SCALAR
DHEXVR, DPENVR, DTETVR
Translational
VECTOR
MPCFR, MPCFRI, MPCFMP
Rotational
VECTOR
MPCFR, MPCFRI, MPCFMP
Chapter 4: Read Results 521 Supported MSC.Access Result Quantities
Primary Label Grid Point Forces
Secondary Label
Type
Objects
Applied Loads
VECTOR
GPFV
Constraint Forces
VECTOR
GPFV
MPC Forces
VECTOR
GPFV
Elements
VECTOR
GPFV
Total
VECTOR
GPFV
Applied Loads
VECTOR
GPFV
Constraint Forces
VECTOR
GPFV
MPC Forces
VECTOR
GPFV
Elements
VECTOR
GPFV
Total
VECTOR
GPFV
Bushing Forces
Translational, Rotational
VECTOR
FBSHR, FBSHRI, FBSHMP
Bushing Stresses
Translational, Rotational
VECTOR
SBSHR, SBSHRI, SBSHMP
Bushing Strains
Translational, Rotational
VECTOR
EBSHR, EBSHRI, EBSHMP
Bushing 1-D Results
Axial Stress, Axial Strain, Axial Force, Axial Displacement
SCALAR
SBS1R, SBS1RI, SBS1MP
Nonlinear Bushing Force
Axial Stress, Axial Strain, Axial Force, Axial Displacement
SCALAR
NBS1R, NBS1RI, NBS1MP
Temperature
SCALAR
THERR
Enthalpies
SCALAR
ENTHR
Rates of Enthalpy Change
SCALAR
ENRCR
Constraint Heats
SCALAR
HTFFR
Applied Loads
SCALAR
HTFLR
Boundary Heat Flux
Applied Loads
SCALAR
QHBDY
Free Convection
SCALAR
QHBDY
Forced Convection
SCALAR
QHBDY
Radiation
SCALAR
QHBDY
Total
SCALAR
QHBDY
Grid Point Moments
522
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Heat Fluxes
VECTOR
QBARR, QBEMR,QCONR, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R
Temperature Gradients
VECTOR
QBARR, QBEMR, QCONR, QHEXR,QPENR, QQD4R, QQD8R, QRODR, QTETR, QTUBR, QTX6R
Chapter 4: Read Results 523 Supported MSC.Access Result Quantities
Elemental Results Primary Label Bar Forces
Secondary Label
Type
Objects
Translational
VECTOR
FBEMR
Rotational
VECTOR
FBEMR
Warping Torque
SCALAR
FBEMR
Translational
VECTOR
FBEMRI
Rotational
VECTOR
FBEMRI
Warping Torque
SCALAR
FBEMRI
Translational
VECTOR
FBEMMP
Rotational
VECTOR
FBEMMP
Warping Torque
SCALAR
FBEMMP
Translational
VECTOR
FTUBR
Rotational
VECTOR
FTUBR
Translational
VECTOR
FTUBRI
Rotational
VECTOR
FTUBRI
Translational
VECTOR
FTUBMP
Rotational
VECTOR
FTUBMP
Translational
VECTOR
FCONR
Rotational
VECTOR
FCONR
Translational
VECTOR
FCONRI
Rotational
VECTOR
FCONRI
Translational
VECTOR
FCONMP
Rotational
VECTOR
FCONMP
Translational
VECTORs
FELSR FELSRI FELSMP FDMPR FDMPRI FDMPMP
Rotational
VECTOR
FBARR
Translational
VECTOR
FBARR
Rotational
VECTOR
FBARRI
Translational
VECTOR
FBARRI
524
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Bar Forces (continued
Shear Panel Forces
Secondary Label
Type
Objects
Rotational
VECTOR
FBARMP
Translational
VECTOR
FBARMP
Translational
VECTOR
FBRXR
Rotational
VECTOR
FBRXR
Force41
SCALAR
FSHRR
Force21
SCALAR
FSHRR
Force12
SCALAR
FSHRR
Force32
SCALAR
FSHRR
Force23
SCALAR
FSHRR
Force43
SCALAR
FSHRR
Force34
SCALAR
FSHRR
Force14
SCALAR
FSHRR
Kick
SCALAR
FSHRR
Shear
SCALAR
FSHRR
Force41
SCALAR
FSHRRI
Force21
SCALAR
FSHRRI
Force12
SCALAR
FSHRRI
Force32
SCALAR
FSHRRI
Force23
SCALAR
FSHRRI
Force43
SCALAR
FSHRRI
Force34
SCALAR
FSHRRI
Force14
SCALAR
FSHRRI
Kick
SCALAR
FSHRRI
Shear
SCALAR
FSHRRI
Force41
SCALAR
FSHRMP
Force21
SCALAR
FSHRMP
Force12
SCALAR
FSHRMP
Force32
SCALAR
FSHRMP
Force23
SCALAR
FSHRMP
Force43
SCALAR
FSHRMP
Force34
SCALAR
FSHRMP
Force14
SCALAR
FSHRMP
Chapter 4: Read Results 525 Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Shear Panel Forces (continued)
Kick
SCALAR
FSHRMP
Shear
SCALAR
FSHRMP
Shell Forces
Force Resultant
TENSOR
FQD4R
Moment Resultant
TENSOR
FQD4R
Force Resultant
TENSOR
FQD4RI
Moment Resultant
TENSOR
FQD4RI
Force Resultant
TENSOR
FQD4MP
Moment Resultant
TENSOR
FQD4MP
Force Resultant
TENSOR
FQD8R
Moment Resultant
TENSOR
FQD8R
Force Resultant
TENSOR
FQD8RI
Moment Resultant
TENSOR
FQD8RI
Force Resultant
TENSOR
FQD8MP
Moment Resultant
TENSOR
FQD8MP
Force Resultant
TENSOR
FTRRR
Moment Resultant
TENSOR
FTRRR
Force Resultant
TENSOR
FTRRRI
Moment Resultant
TENSOR
FTRRRI
Force Resultant
TENSOR
FTRRMP
Moment Resultant
TENSOR
FTRRMP
Force Resultant
TENSOR
FTR3R
Moment Resultant
TENSOR
FTR3R
Force Resultant
TENSOR
FTR3RI
Moment Resultant
TENSOR
FTR3RI
Force Resultant
TENSOR
FTR3MP
Moment Resultant
TENSOR
FTR3MP
Force Resultant
TENSOR
FTR6R
Moment Resultant
TENSOR
FTR6R
Force Resultant
TENSOR
FTR6RI
Moment Resultant
TENSOR
FTR6RI
Force Resultant
TENSOR
FTR6MP
Moment Resultant
TENSOR
FTR6MP
526
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Shell Forces (continued)
Gap Results
Stress Tensor
Secondary Label
Type
Objects
Force Resultant
TENSOR
FQDRR
Moment Resultant
TENSOR
FQDRR
Force Resultant
TENSOR
FQDRRI
Moment Resultant
TENSOR
FQDRRI
Force Resultant
TENSOR
FQDRMP
Moment Resultant
TENSOR
FQDRMP
Force Resultant
TENSOR
FQD4XR
Moment Resultant
TENSOR
FQD4XR
Force Resultant
TENSOR
FQD4XRI
Moment Resultant
TENSOR
FQD4XRI
Force Resultant
TENSOR
FQD4XMP
Moment Resultant
TENSOR
FQD4XMP
Force
VECTOR
FGAPR
Displacement
VECTOR
FGAPR
Slip
VECTOR
FGAPR
Force
VECTOR
NGAPR
Displacement
VECTOR
NGAPR
Slip
VECTOR
NGAPR
NONE
TENSOR
SRODR
TENSOR
SRODRI
TENSOR
SRODMP
TENSOR
SBEMR
TENSOR
SBEMRI
TENSOR
SBEMMP
TENSOR
STUBR
TENSOR
STUBRI
TENSOR
STUBMP
TENSOR
SCONR
TENSOR
SCONRI
TENSOR
SCONMP
NONE NONE
NONE
Chapter 4: Read Results 527 Supported MSC.Access Result Quantities
Primary Label Stress Tensor (continued)
Secondary Label NONE
Type
Objects
TENSOR
SELSR
TENSOR
SELSRI
TENSOR
SELSMP
TENSOR
SQD4R
TENSOR
SQD4RI
TENSOR
SQD4MP
TENSOR
SBARR
TENSOR
SBARRI
TENSOR
SBARMP
TENSOR
STETR
TENSOR
STETRI
TENSOR
STETMP
NONE
TENSOR
STX6R
NONE
TENSOR
SQD8R
TENSOR
SQD8RI
TENSOR
SQD8MP
TENSOR
SHEXR
TENSOR
SHEXRI
TENSOR
SHEXMP
TENSOR
SPENR
TENSOR
SPENRI
TENSOR
SPENMP
TENSOR
STRRR
TENSOR
STRRRI
TENSOR
STRRMP
TENSOR
STR6R
TENSOR
STR6RI
TENSOR
STR6MP
TENSOR
STR3R
TENSOR
STR3RI
TENSOR
STR3MP
NONE
NONE
NONE
NONE
NONE
NONE
NONE
NONE
528
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Stress Tensor (continued)
Bar Stresses
Bar Strains
Secondary Label NONE
Type
Objects
TENSOR
SQDRR
TENSOR
SQDRRI
TENSOR
SQDRMP
NONE
TENSOR
TQD4R
NONE
TENSOR
TQD8R
NONE
TENSOR
TTR3R
NONE
TENSOR
TTR6R
NONE
TENSOR
SBRXR
NONE
TENSOR
SQD4XR
TENSOR
SQD4XRI
TENSOR
SQD4XMP
NONE
TENSOR
SBRXR
Maximum Axial
SCALAR
SBEMR
Minimum Axial
SCALAR
SBEMR
Maximum Axial
SCALAR
SBARR
Minimum Axial
SCALAR
SBARR
Tension Safety Margin
SCALAR
SBARR
Maximum Axial
SCALAR
SBRXR
Minimum Axial
SCALAR
SBRXR
Maximum Axial
SCALAR
SBRXR
Minimum Axial
SCALAR
SBRXR
Maximum Axial
SCALAR
EBEMR
Minimum Axial
SCALAR
EBEMR
Maximum Axial
SCALAR
EBARR
Minimum Axial
SCALAR
EBARR
Tension Safety Margin
SCALAR
EBARR
Compressive Safety Margin
SCALAR
EBARR
Maximum Axial
SCALAR
EBRXR
Minimum Axial
SCALAR
EBRXR
Maximum Axial
SCALAR
EBRXR
Minimum Axial
SCALAR
EBRXR
Chapter 4: Read Results 529 Supported MSC.Access Result Quantities
Primary Label Strain Tensor
Secondary Label NONE
NONE
NONE
NONE
NONE
NONE
NONE
NONE
Type
Objects
ENG_TENSOR
ERODR
ENG_TENSOR
ERODRI
ENG_TENSOR
ERODMP
ENG_TENSOR
EBEMR
ENG_TENSOR
EBEMRI
ENG_TENSOR
EBEMMP
ENG_TENSOR
ETUBR
ENG_TENSOR
ETUBRI
ENG_TENSOR
ETUBMP
ENG_TENSOR
ECONR
ENG_TENSOR
ECONRI
ENG_TENSOR
ECONMP
ENG_TENSOR
EELSR
ENG_TENSOR
EELSRI
ENG_TENSOR
EELSMP
ENG_TENSOR
EQD4R
ENG_TENSOR
EQD4RI
ENG_TENSOR
EQD4MP
ENG_TENSOR
EBARRI
ENG_TENSOR
EBARR
ENG_TENSOR
EBARMP
ENG_TENSOR
ETETR
ENG_TENSOR
ETETRI
ENG_TENSOR
ETETMP
ENG_TENSOR
EQD8R
ENG_TENSOR
EQD8RI
ENG_TENSOR
EQD8MP
530
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Tensor (continued)
Shear Panel Stresses
Shear Panel Strains
Secondary Label
Type
Objects
ENG_TENSOR
EQDRR
ENG_TENSOR
EQDRRI
ENG_TENSOR
EQDRMP
NONE
ENG_TENSOR
GQD4R
NONE
ENG_TENSOR
GQD8R
NONE
ENG_TENSOR
GTR3R
NONE
ENG_TENSOR
GTR6R
NONE
ENG_TENSOR
EBRXR
NONE
ENG_TENSOR
EQD4XR
ENG_TENSOR
EQD4XRI
ENG_TENSOR
EQD4XMP
NONE
ENG_TENSOR
EBRXR
Maximum Shear
SCALAR
SSHRR
Average Shear
SCALAR
SSHRR
Maximum Shear
SCALAR
SSHRRI
Average Shear
SCALAR
SSHRRI
Maximum Shear
SCALAR
SSHRMP
Average Shear
SCALAR
SSHRMP
Maximum Shear
SCALAR
SSHRR
Average Shear
SCALAR
SSHRR
Maximum Shear
SCALAR
SSHRRI
Average Shear
SCALAR
SSHRRI
Maximum Shear
SCALAR
SSHRMP
Average Shear
SCALAR
SSHRMP
Maximum Shear
SCALAR
ESHRR
Average Shear
SCALAR
ESHRR
Maximum Shear
SCALAR
ESHRRI
Average Shear
SCALAR
ESHRRI
Maximum Shear
SCALAR
ESHRMP
Average Shear
SCALAR
ESHRMP
NONE
Chapter 4: Read Results 531 Supported MSC.Access Result Quantities
Primary Label Principal Stress Direction
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
SQD4R
Major Prin x cosine
SCALAR
STETR
Minor Prin x cosine
SCALAR
STETR
Intermed Prin x cosine
SCALAR
STETR
Major Prin y cosine
SCALAR
STETR
Minor Prin y cosine
SCALAR
STETR
Intermed Prin y cosine
SCALAR
STETR
Major Prin z cosine
SCALAR
STETR
Minor Prin z cosine
SCALAR
STETR
Intermed Prin z cosine
SCALAR
STETR
Zero Shear Angle
SCALAR
SQD8R
Major Prin x cosine
SCALAR
SHEXR
Minor Prin x cosine
SCALAR
SHEXR
Intermed Prin x cosine
SCALAR
SHEXR
Major Prin y cosine
SCALAR
SHEXR
Minor Prin y cosine
SCALAR
SHEXR
Intermed Prin y cosine
SCALAR
SHEXR
Major Prin z cosine
SCALAR
SHEXR
Minor Prin z cosine
SCALAR
SHEXR
Intermed Prin z cosine
SCALAR
SHEXR
Major Prin x cosine
SCALAR
SPENR
Minor Prin x cosine
SCALAR
SPENR
Intermed Prin x cosine
SCALAR
SPENR
Major Prin y cosine
SCALAR
SPENR
Minor Prin y cosine
SCALAR
SPENR
Intermed Prin y cosine
SCALAR
SPENR
Major Prin z cosine
SCALAR
SPENR
Minor Prin z cosine
SCALAR
SPENR
Intermed Prin z cosine
SCALAR
SPENR
Zero Shear Angle
SCALAR
STRRR
Zero Shear Angle
SCALAR
STR6R
Zero Shear Angle
SCALAR
STR3R
532
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Principal Stress Direction (continued)
Stress Invariants
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
SQDRR
Zero Shear Angle
SCALAR
TQD4R
Zero Shear Angle
SCALAR
TQD8R
Zero Shear Angle
SCALAR
TTR3R
Zero Shear Angle
SCALAR
TTR6R
Zero Shear Angle
SCALAR
SQD4XR
Major Principal
SCALAR
SQD4R
Minor Principal
SCALAR
SQD4R
Maximum Shear
SCALAR
SQD4R
Major Principal
SCALAR
STETR
Mean Pressure
SCALAR
STETR
Minor Principal
SCALAR
STETR
Intermediate Principal
SCALAR
STETR
Octahedral Shear
SCALAR
STETR
Von Mises
SCALAR
STETR
Major Principal
SCALAR
STX6R
Maximum Shear
SCALAR
STX6R
Octahedral Shear
SCALAR
STX6R
Von Mises
SCALAR
STX6R
Major Principal
SCALAR
SQD8R
Minor Principal
SCALAR
SQD8R
Maximum Shear
SCALAR
SQD8R
Von Mises
SCALAR
SQD8R
Major Principal
SCALAR
SHEXR
Mean Pressure
SCALAR
SHEXR
Minor Principal
SCALAR
SHEXR
Intermediate Principal
SCALAR
SHEXR
Octahedral Shear
SCALAR
SHEXR
Von Mises
SCALAR
SHEXR
Major Principal
SCALAR
SPENR
Mean Pressure
SCALAR
SPENR
Minor Principal
SCALAR
SPENR
Chapter 4: Read Results 533 Supported MSC.Access Result Quantities
Primary Label Stress Invariants (continued)
Secondary Label
Type
Objects
Intermediate Principal
SCALAR
SPENR
Octahedral Shear
SCALAR
SPENR
Von Mises
SCALAR
SPENR
Major Principal
SCALAR
STRRR
Minor Principal
SCALAR
STRRR
Maximum Shear
SCALAR
STRRR
Von Mises
SCALAR
STRRR
Major Principal
SCALAR
STR6R
Minor Principal
SCALAR
STR6R
Maximum Shear
SCALAR
STR6R
Von Mises
SCALAR
STR6R
Major Principal
SCALAR
STR3R
Minor Principal
SCALAR
STR3R
Maximum Shear
SCALAR
STR3R
Von Mises
SCALAR
STR3R
Major Principal
SCALAR
SQDRR
Minor Principal
SCALAR
SQDRR
Maximum Shear
SCALAR
SQDRR
Von Mises
SCALAR
SQDRR
Major Principal
SCALAR
TQD4R
Minor Principal
SCALAR
TQD4R
Maximum Shear
SCALAR
TQD4R
Major Principal
SCALAR
TQD8R
Minor Principal
SCALAR
TQD8R
Maximum Shear
SCALAR
TQD8R
Major Principal
SCALAR
TTR3R
Minor Principal
SCALAR
TTR3R
Maximum Shear
SCALAR
TTR3R
Major Principal
SCALAR
TTR6R
Minor Principal
SCALAR
TTR6R
Maximum Shear
SCALAR
TTR6R
Major Principal
SCALAR
SQD4XR
534
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Stress Invariants (continued)
Principal Strain Direction
Secondary Label
Type
Objects
Minor Principal
SCALAR
SQD4XR
Maximum Shear
SCALAR
SQD4XR
Von Mises
SCALAR
SQD4XR
Zero Shear Angle
SCALAR
EQD4R
Major Prin x cosine
SCALAR
ETETR
Minor Prin x cosine
SCALAR
ETETR
Intermed Prin x cosine
SCALAR
ETETR
Major Prin y cosine
SCALAR
ETETR
Minor Prin y cosine
SCALAR
ETETR
Intermed Prin y cosine
SCALAR
ETETR
Major Prin z cosine
SCALAR
ETETR
Minor Prin z cosine
SCALAR
ETETR
Intermed Prin z cosine
SCALAR
ETETR
Zero Shear Angle
SCALAR
EQD8R
Major Prin x cosine
SCALAR
EHEXR
Minor Prin x cosine
SCALAR
EHEXR
Intermed Prin x cosine
SCALAR
EHEXR
Major Prin y cosine
SCALAR
EHEXR
Minor Prin y cosine
SCALAR
EHEXR
Intermed Prin y cosine
SCALAR
EHEXR
Major Prin z cosine
SCALAR
EHEXR
Minor Prin z cosine
SCALAR
EHEXR
Intermed Prin z cosine
SCALAR
EHEXR
Major Prin x cosine
SCALAR
EPENR
Minor Prin x cosine
SCALAR
EPENR
Intermed Prin x cosine
SCALAR
EPENR
Major Prin y cosine
SCALAR
EPENR
Minor Prin y cosine
SCALAR
EPENR
Intermed Prin y cosine
SCALAR
EPENR
Major Prin z cosine
SCALAR
EPENR
Minor Prin z cosine
SCALAR
EPENR
Intermed Prin z cosine
SCALAR
EPENR
Chapter 4: Read Results 535 Supported MSC.Access Result Quantities
Primary Label Principal Strain Direction (continued)
Strain Invariants
Secondary Label
Type
Objects
Zero Shear Angle
SCALAR
ETRRR
Zero Shear Angle
SCALAR
ETR6R
Zero Shear Angle
SCALAR
ETR3R
Zero Shear Angle
SCALAR
EQDRR
Zero Shear Angle
SCALAR
GQD4R
Zero Shear Angle
SCALAR
GQD8R
Zero Shear Angle
SCALAR
GTR3R
Zero Shear Angle
SCALAR
GTR6R
Zero Shear Angle
SCALAR
EQD4XR
Major Principal
SCALAR
EQD4R
Minor Principal
SCALAR
EQD4R
Maximum Shear
SCALAR
EQD4R
Major Principal
SCALAR
ETETR
Mean Pressure
SCALAR
ETETR
Minor Principal
SCALAR
ETETR
Intermediate Principal
SCALAR
ETETR
Octahedral Shear
SCALAR
ETETR
Von Mises
SCALAR
ETETR
Major Principal
SCALAR
EQD8R
Minor Principal
SCALAR
EQD8R
Maximum Shear
SCALAR
EQD8R
Von Mises
SCALAR
EQD8R
Major Principal
SCALAR
EHEXR
Mean Pressure
SCALAR
EHEXR
Minor Principal
SCALAR
EHEXR
Intermediate Principal
SCALAR
EHEXR
Octahedral Shear
SCALAR
EHEXR
Von Mises
SCALAR
EHEXR
Major Principal
SCALAR
EPENR
Mean Pressure
SCALAR
EPENR
Minor Principal
SCALAR
EPENR
Intermediate Principal
SCALAR
EPENR
536
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Invariants (continued)
Secondary Label
Type
Objects
Octahedral Shear
SCALAR
EPENR
Von Mises
SCALAR
EPENR
Major Principal
SCALAR
ETRRR
Minor Principal
SCALAR
ETRRR
Maximum Shear
SCALAR
ETRRR
Von Mises
SCALAR
ETRRR
Major Principal
SCALAR
ETR6R
Minor Principal
SCALAR
ETR6R
Maximum Shear
SCALAR
ETR6R
Von Mises
SCALAR
ETR6R
Major Principal
SCALAR
ETR3R
Minor Principal
SCALAR
ETR3R
Maximum Shear
SCALAR
ETR3R
Von Mises
SCALAR
ETR3R
Major Principal
SCALAR
EQDRR
Minor Principal
SCALAR
EQDRR
Maximum Shear
SCALAR
EQDRR
Von Mises
SCALAR
EQDRR
Major Principal
SCALAR
GQD4R
Minor Principal
SCALAR
GQD4R
Maximum Shear
SCALAR
GQD4R
Major Principal
SCALAR
GQD8R
Minor Principal
SCALAR
GQD8R
Maximum Shear
SCALAR
GQD8R
Major Principal
SCALAR
GTR3R
Minor Principal
SCALAR
GTR3R
Maximum Shear
SCALAR
GTR3R
Major Principal
SCALAR
GTR6R
Minor Principal
SCALAR
GTR6R
Maximum Shear
SCALAR
GTR6R
Major Principal
SCALAR
EQD4XR
Minor Principal
SCALAR
EQD4XR
Chapter 4: Read Results 537 Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Type
Objects
Strain Invariants (continued)
Maximum Shear
SCALAR
EQD4XR
Von Mises
SCALAR
EQD4XR
Nonlinear Stresses
Stress Tensor
TENSOR
NTETR
Equivalent Stress
SCALAR
NTETR
Stress Tensor
TENSOR
NTUBR
Equivalent Stress
SCALAR
NTUBR
Stress Tensor
TENSOR
NTR3R
Equivalent Stress
SCALAR
NTR3R
Stress Tensor
TENSOR
NRODR
Equivalent Stress
SCALAR
NRODR
Stress Tensor
TENSOR
NQD4R
Equivalent Stress
SCALAR
NQD4R
Stress Tensor
TENSOR
NPENR
Equivalent Stress
SCALAR
NPENR
Stress Tensor
TENSOR
NCONR
Equivalent Stress
SCALAR
NCONR
Stress Tensor
TENSOR
NHEXR
Equivalent Stress
SCALAR
NHEXR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Stress Tensor
TENSOR
NBEMR
Equivalent Stress
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NTETR
Plastic Strain
SCALAR
NTETR
Creep Strain
SCALAR
NTETR
Strain Tensor
ENG_TENSOR
NTUBR
Plastic Strain
SCALAR
NTUBR
Creep Strain
SCALAR
NTUBR
Nonlinear Strains
538
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Nonlinear Strains (continued)
Secondary Label
Type
Objects
Strain Tensor
ENG_TENSOR
NTR3R
Plastic Strain
SCALAR
NTR3R
Creep Strain
SCALAR
NTR3R
Strain Tensor
ENG_TENSOR
NRODR
Plastic Strain
SCALAR
NRODR
Creep Strain
SCALAR
NRODR
Strain Tensor
ENG_TENSOR
NQD4R
Plastic Strain
SCALAR
NQD4R
Creep Strain
SCALAR
NQD4R
Strain Tensor
ENG_TENSOR
NPENR
Plastic Strain
SCALAR
NPENR
Creep Strain
SCALAR
NPENR
Strain Tensor
ENG_TENSOR
NCONR
Plastic Strain
SCALAR
NCONR
Creep Strain
SCALAR
NCONR
Strain Tensor
ENG_TENSOR
NHEXR
Plastic Strain
SCALAR
NHEXR
Creep Strain
SCALAR
NHEXR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Strain Tensor
ENG_TENSOR
NBEMR
Plastic Strain
SCALAR
NBEMR
Creep Strain
SCALAR
NBEMR
Chapter 4: Read Results 539 Supported MSC.Access Result Quantities
Primary Label Strain Energy
Secondary Label
Type
Objects
Energy
SCALAR
URODR
Percent of Total
SCALAR
URODR
Energy Density
SCALAR
URODR
Energy
SCALAR
UBEMR
Percent of Total
SCALAR
UBEMR
Energy Density
SCALAR
UBEMR
Energy
SCALAR
UTUBR
Percent of Total
SCALAR
UTUBR
Energy Density
SCALAR
UTUBR
Energy
SCALAR
USHRR
Percent of Total
SCALAR
USHRR
Energy Density
SCALAR
USHRR
Energy
SCALAR
UCONR
Percent of Total
SCALAR
UCONR
Energy Density
SCALAR
UCONR
Energy
SCALAR
UELSR
Percent of Total
SCALAR
UELSR
Energy Density
SCALAR
UELSR
Energy
SCALAR
UDMPR
Percent of Total
SCALAR
UDMPR
Energy Density
SCALAR
UDMPR
Energy
SCALAR
UQD4R
Percent of Total
SCALAR
UQD4R
Energy Density
SCALAR
UQD4R
Energy
SCALAR
UBARR
Percent of Total
SCALAR
UBARR
Energy Density
SCALAR
UBARR
Energy
SCALAR
UGAPR
Percent of Total
SCALAR
UGAPR
Energy Density
SCALAR
UGAPR
Energy
SCALAR
UTETR
Percent of Total
SCALAR
UTETR
540
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label Strain Energy (continued)
Secondary Label
Type
Objects
Energy Density
SCALAR
UTETR
Energy
SCALAR
UTX6R
Percent of Total
SCALAR
UTX6R
Energy Density
SCALAR
UTX6R
Energy
SCALAR
UQD8R
Percent of Total
SCALAR
UQD8R
Energy Density
SCALAR
UQD8R
Energy
SCALAR
UHEXR
Percent of Total
SCALAR
UHEXR
Energy Density
SCALAR
UHEXR
Energy
SCALAR
UPENR
Percent of Total
SCALAR
UPENR
Energy Density
SCALAR
UPENR
Energy
SCALAR
UTRRR
Percent of Total
SCALAR
UTRRR
Energy Density
SCALAR
UTRRR
Energy
SCALAR
UTR3R
Percent of Total
SCALAR
UTR3R
Energy Density
SCALAR
UTR3R
Energy
SCALAR
UTR6R
Percent of Total
SCALAR
UTR6R
Energy Density
SCALAR
UTR6R
Energy
SCALAR
UQDRR
Percent of Total
SCALAR
UQDRR
Energy Density
SCALAR
UQDRR
Chapter 4: Read Results 541 Supported MSC.Access Result Quantities
Primary Label Cauchy Stresses
Secondary Label
Type TENSOR
Objects HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Logarithmic Strains
TENSOR
HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
542
Patran Interface to MD Nastran Preference Guide Supported MSC.Access Result Quantities
Primary Label
Secondary Label
Pressure
Type TENSOR
Objects HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Volumetric Strains
TENSOR
HHEXR, HPENR, HQD4R, HQDXR. HQUDR, HTETR, HTR3R, HTR6R, HTRXR
Topology Optimization
Element Density
SCALAR
DVHIST
Chapter 4: Read Results 543 Supported 3dplot Results Quantities
4.5
Supported 3dplot Results Quantities The following table indicates all the possible result quantities which can be loaded into the Patran database from the LS-Dyna’s ptf file.
Global Variable Label
Type
Description
Displacement
Nodal
x, y, z displacements of nodes, in global coordinate frame.
Velocity
Nodal
x, y, z velocity of nodes, in global coordinate frame.
Acceleration
Nodal
x, y, z acceleration of nodes, in global coordinate frame.
Temperature
Nodal
Nodal temperature.
Forces
Nodal
Resultant beam forces and moments, in local beam coordinate.
Stress
Element
6 components of stress tensor, at element centre and gaussian points - top, middle, and bottom for shells.
Stress Resultants
Element
Stress Resultants at elements.
Strain
Element
6 components of strain tensor, at element centre and gaussian points - top, middle, and bottom for shells.
Eff. Plastic Strain
Element
Effective plastic strain, at element centre and gaussian points - top, middle, and bottom for shells.
Element Volume, Euler
Partition/ Element
Element of constant volume.
Mass, Euler
Partition/ Element
Mass of fluid in a partition (element of constant volume).
Density, Euler
Partition/ Element
Density of fluid in a partition (element of constant volume).
Specific Internal Energy, Euler
Partition/ Element
Specific internal energy of fluid in a partition (element of constant volume).
Total Energy, Euler
Partition/ Element
Total energy of fluid in a partition (element of constant volume).
Material Fraction, Euler
Partition/ Element
Material fraction of fluid * the volume uncovered fraction in a partition (element of constant volume).
Speed of Sound, Euler
Partition/ Element
Speed of sound of fluid in a partition (element of constant volume).
Momentum, Euler
Partition/ Element
Momentum of fluid in a partition (element of constant volume).
Volume Uncovered Fraction, Euler
Partition/ Element
Volume uncovered fraction of fluid in a partition (element of constant volume).
Mass Flow Rate, Euler
Partition/ Element
Mass flow rate of fluid in a partition (element of constant volume).
544
Patran Interface to MD Nastran Preference Guide Supported 3dplot Results Quantities
Global Variable Label
Type
Description
Total Mass Flow, Euler
Partition/ Element
Total mass flow over a given time of fluid in a partition (element of constant volume).
Heat Transfer Rate, Euler
Partition/ Element
Heat transfer rate for fluid in a partition (element of constant volume).
Total Heat Transfer, Euler
Partition/ Element
Total heat transfer over a given time of fluid in a partition (element of constant volume).
Velocity, Euler
Partition/ Element
Velocity of fluid in a partition (element of constant volume).
Chapter 5: Read Input File Patran Interface to MD Nastran Preference Guide
5
Read Input File
Review of Read Input File Form
Data Translated from the NASTRAN Input File
Conflict Resolution
565
546 554
546
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
5.1
Review of Read Input File Form The Analysis form will appear when the Analysis toggle, located on the Patran main menu, is chosen.
Read Input File as the selected Action on the Analysis form allows much of the model data from a MD Nastran input file to be translated into the Patran database. A subordinate File Selection form allows the user to specify the MD Nastran input file to translate. This form is described on the following pages.
Chapter 5: Read Input File 547 Review of Read Input File Form
Read Input File Form This form appears when the Analysis toggle is selected on the main menu. Read Input File, as the selected Action, specifies that model data is to be translated from the specified MD Nastran input file into the Patran database.
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of already existing jobs.
Name assigned to current translation job. This job name will be used as the base file name for the message file.
Activates a subordinate Entity Selection form which allows the user to specify the specific entry types to be read. Also defines ID offset values to be used during import.
Activates a subordinate File Select form which allows the user to specify the NASTRAN input file to be translated.
548
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
Entity Selection Form This subordinate form appears when the Entity Selection button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which MD Nastran entity types to import.
Highlighted entity types will be imported.
Activates the form to define ID offsets.
Select this button to create groups based on property sets and materials. Selecting this toggle will tell Patran to attempt to retrieve the names of properties and materials from the comments in the input file. This only applys to material and element properties names.
Chapter 5: Read Input File 549 Review of Read Input File Form
The following table shows the relation between the entity types listed above and the actual MD Nastran entry types effected. If an entity type is filtered out, it is treated as if those entries did not exist in the original input file. Entity Type
MD Nastran Cards
Nodes
GRID, GRDSET, SPOINT
Elements
BAROR, BEAMOR, CBAR, CBEAM, CBEND, CDAMP1, CDAMP2, CDAMP3, CDAMP4, CELAS1, CELAS2, CELAS3, CELAS4, CGAP, CHEXA, CMASS1, CMASS2, CMASS3, CMASS4, CONM1, CONM2, CONROD, CPENTA, CQUAD4, CQUAD8, CQUADR, CROD, CSHEAR, CTETRA, CTRIA3, CTRIA6, CTRIAR, CTRIAX6, CTUBE, CVISC, PLOTEL
Material Properties
MAT1, MAT2, MAT3, MAT8, MAT9
Element Properties
PBAR, PBCOMP, PBEAM, PBEND, PCOMP, PDAMP, PELAS, PGAP, PMASS, PROD, PSHEAR, PSHELL, PSOLID, PTUBE, PVISC
Coordinate Frames
CORD1C, CORD1R, CORD1S, CORD2C, CORD2R, CORD2S
Load Sets
FORCE, GRAV,MOMENT, PLOAD1, PLOAD2, PLOAD4, PLOADX1, RFORCE, TEMP, TEMPP1, TEMPRB, SPC, SPC1, SPCD
Subcases
LOAD, SPCADD, Case Control Section
MPC Data
MPC, RBAR, RBE1, RBE2, RBE3, RROD, RSPLINE, RTRPLT It should be noted that since the GRID entry is controlled with the Nodes filter, the grid.ps load set with the permanent single point constraint data will also be controlled by the Nodes filter.
550
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
Define Offsets Form This subordinate form appears when the Define Offsets button is selected on the Entity Selection form. It allows the user to specify the ID offsets used when reading a MD Nastran input file. If selected, the value in the Maximum column will be used as the offset for the selected rows.
Minimum and Maximum IDs currently found in the Patran database.
All offset data boxes can be selected at once by selecting this column header.
ID offset value to be used during import. The new ID value will be the ID found in the NASTRAN input file plus this offset value.
All references made in the input file will also be offset. If a node references a particular CID as its analysis frame, then the reference will be offset as well. If the coordinate frame is defined in the same input file, the proper references should be maintained. The preference will be properly maintained. If the coordinate frame existed in the file prior to the import, then it needs to be the offset CID. If a coordinate frame with that CID is not found in the database, an error message will be issued.
Chapter 5: Read Input File 551 Review of Read Input File Form
To determine which offset effects a particular MD Nastran entry type, refer to the table in the previous section. For Patran entities identified by integer IDs (nodes, elements, coordinate frames, and MPCs), the offset value is simply added to the MD Nastran ID to generate the Patran ID. For Patran entities identified by text names (materials, element properties, load sets, and load cases), the offset value is first added to the MSC Nastran ID. The new integer value is then used to generate the Patran name per the naming conventions described in later sections.
Selection of Input File This subordinate form appears when the Select Input File button is selected on the Analysis form and Read Input File is the selected Action. It allows the user to specify which MD Nastran input file to translate.
Summary Data Form This form appears after the import of the NASTRAN input file has completed. It displays the number of entities imported correctly, imported with warnings, or not imported due to errors. These figures reflect the number of Patran entities created. In some cases, there is not a one-to-one relation between the original MD Nastran entities and the generated Patran entities. For example, when material orientations on several CQUAD4s are defined using references to varying MCIDs while still referencing the same PID, Patran needs to create a unique property set for each different MCID reference.
552
Patran Interface to MD Nastran Preference Guide Review of Read Input File Form
When the OK button is selected, the newly imported data will be committed to the Patran database, and can not be undone. If there is any question as to whether or not this import was desired, review the graphics data prior to selecting OK on this form. If the import was not correct, select the undo button on the main menu bar before selecting OK on this form. NASTRAN Input File Import Summary Imported
Imported with Warning
Nodes Elements Coordinate Frames Materials Element Properties Load Sets Load Cases MPCs
Reject Cards...
OK
Not Imported
Chapter 5: Read Input File 553 Review of Read Input File Form
Reject Card Form During import of the NASTRAN input file, some entries types might not be understood by Patran. Those entries are brought into Patran in the direct text input data boxes. Selecting the Reject Cards button on the Summary Data form will bring up this Reject Card Form. You can review these entries here. Direct Text Import Bulk Data Section $ $CBEAM
215
MPCADD
100
213 101
214
0.
0.
1.
102
uu File Management Section
uu Case Control Section
uu Executive Control Section u Bulk Data Section OK
Only entry types not supported by Patran are sent to the reject entry blocks. (This includes comments.) Cards which are otherwise recognized, but can not be imported due to syntax or invalid data errors are not sent to the reject blocks. The rejected entries will have no characters in front of the command name. Commands preceded by the character $> are used by the MSC/AMS product to allow processing of comment lines. Note:
As long as you don not delete the reject casrd file, Patran will re-insert the rejected entries back into the input file if you use the same jobname.
554
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
5.2
Data Translated from the NASTRAN Input File The following sections describe which specific MD Nastran entry types can currently be read into Patran. The MD Nastran entries described in this document are the only entries read when importing a NASTRAN input file into Patran. All non-supported entries will be sent to the appropriate Direct Text Input data box for this job. When errors occur during the import of a supported entry type, the entry being processed may or may not be imported, depending on the severity of the problem encountered. An error message will be presented regardless of whether or not the offending entry is actually imported. Any references from supported entries to entries that were not imported (either due to not being a supported entry type or due to serious import errors) will still be attempted. If this reference is required in Patran for the entry currently being processed, it too will fail to import. For example, if there is a serious error on a GRID entry which causes it to not imported, then all elements attached to that GRID will also fail to import. Partial Decks This Patran function can read incomplete MD Nastran files (except where explicitly noted). However, if the BEGIN BULK command is missing, the program can get confused when trying to determine if a particular entry belongs to the case control or bulk data. If you experience any difficulties importing a file that does not have a BEGIN BULK command, add one to the top of the file. This should avoid any such confusion.
Coordinate Systems The following coordinate system definitions can be read into Patran. Command CORD1C CORD1R
Comments References to the GRIDs on these entries are lost. The locations of the referenced GRIDs are extracted, and those locations are used to create the Patran definition.
CORD1S CORD2C CORD2R CORD2S
References to RIDs are lost. The specified locations are converted to global cartesian for use in the Patran definitions. The original B and C points are not retained. Their values are recomputed when a new NASTRAN input file is created. The definition will be equivalent, but not identical.
Referential Integrity Coordinate systems and GRIDs which are referenced as part of a CORD definition must be in the same input file. If these are not found in the input file, the definition will be rejected.
Chapter 5: Read Input File 555 Data Translated from the NASTRAN Input File
References to coordinate frames other than for new coordinate frame definitions can be resolved with coordinate frames previously found in the Patran database. Chaining Due to limitations in the Patran definitions of coordinate systems, chained definitions (definitions based on other coordinate systems or grids) are modified during import. The resulting definitions are equivalent in global space, but are based on global cartesian coordinates rather than GRID references or coordinate locations in other systems. This change is carried through when a new NASTRAN input file is created. All coordinate systems will be created using CORD2 type definitions, and they will all reference global cartesian coordinates. These definitions will be different from, but equivalent to, the original definitions.
Grids and SPOINTs The MD Nastran GRID entry is read fully, except the SEID field. The CD and CP references are both maintained. The PS data is used to create a constraint set. The details of the created load set are defined in the load set import section. GRDSET data is merged into the GRID data during import. The data will be retained, but will appear directly on the GRID entry when a new NASTRAN input file is generated. SPOINTs SPOINTs are treated as GRIDs at the global origin. They are assumed to have their GRID CD and CP fields set to the basic system, and their PS field is set to permanently constrain degrees-of-freedom 2 through 6. Referential Integrity Coordinate frames referenced in the CP field must exist in the same input file. Coordinate frames referenced on the CD field can exist in either the same input file, or the Patran database prior to the import.
Elements and Element Properties The following MD Nastran elements and element properties can be read into Patran. Element CBAR
Property PBAR
Property Set Name pbar.
Comments Orientation and offset vectors are re-defined in global cartesian during import. (See BAROR comments below.)
PBARL
pbarl.
556
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element
Property
Property Set Name
Comments
CBARAO
New property sets are created for each occurrence of a CBAR entry referenced by a CBARAO entry
CBEAM
Orientation and offset vectors are re-defined in global cartesian during import. (See BEAMOR comments below.) PBEAM
pbeam.
PBEAML
pbeaml.
PBCOMP
pbcomp.
The MD Nastran documentation describes how the section data is used to create a complete set of lumped areas. The data imported into Patran is fully expanded, and therefore, is different from the data in the original input file. This definition is, however, fully equivalent to the original. The SO field is not currently supported. A YES is provided automatically when a new NASTRAN input file is created. Only the lumped areas definition is understood, If a uniform cross section is defined here, it will be converted to a lumped area definition, but no lumped areas will be defined.
CBEND
Patran only understands the GEOM = 1 orientation data. If other definitions are found, a vector will be computed to convert the definition to the GEOM = 1 format. If a GRID was referenced for GEOM other than 1, that reference will be lost. For the same reasons, the THETAB and RB data will also be lost since that data is not used for GEOM = 1 definitions. Orientation and offset vectors are re-defined in global cartesian during import. PBEND
CBUSH
PBUSH
pbend_g.
If standard cross section properties are found on the PBEND entry
pbend_p.
If the alternate format of the PBEND is used to define a pipe cross section.
pbush.
CDAMP1 CDAMP2
The grounded form of the PBUSH
PBUSHT
pbusht_1D.
PDAMP
pdamp.
For dampers connecting 2 GRIDs.
pdamp_g.
For grounded dampers attached to a single GRID.
cdamp2
For dampers connecting 2 GRIDs.
cdamp2_g
For grounded dampers attached to a single GRID.
Chapter 5: Read Input File 557 Data Translated from the NASTRAN Input File
Element CDAMP3
Property
Property Set Name
PDAMP
Treated identical to the CDAMP1 and CDAMP2 elements with the degree-of-freedom fields set to 1 (UX).
CDAMP4 CELAS1
PELAS
CELAS2 CELAS3
pelas.
For springs connecting 2 GRIDs.
pelas_g.
For grounded springs attached to a single GRID.
celas2
For springs connecting 2 GRIDs.
celas2_g
For grounded springs attached to a single GRID.
PELAS
Treated identical to the CELAS1 and CELAS2 elements with the degree-of-freedom fields set to 1 (UX).
CELAS4 CGAP
Orientation and offset vectors are re-defined in global cartesian during import. PGAP
CHBDYG
Comments
pgap.
For non-adaptive definitions on the PGAP entry.
pgap_a.
For adaptive definitions on the PGAP entry.
PHBDY
Note: The BDYOR command that may contain default values for CHBDY elements is not currently supported.
CHBDYP CHEXA
PSOLID
psolid.
CMASS1
PMASS
pmass.
For masses connecting 2 GRIDs.
pmass_g.
For masses attached to a single GRID.
cmass2
For masses connecting 2 GRIDs.
cmass2_g
For masses attached to a single GRID.
CMASS2 CMASS3
PMASS
Treated identical to the CMASS1 and CMASS2 elements with the degree-of-freedom fields set to 1 (UX).
CMASS4 CONM1
conm1
CONM2
conm2
CONROD
conrod
CPENTA
PSOLID
psolid.
CQUAD4
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp.
CQUAD8
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp.
558
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element CQUADR
Property
Property Set Name
Comments
PSHELL
pshellr.
(See PSHELL comments below.)
PCOMP
pcompr.
A new material named pcomp.
CROD
PROD
prod.
CSHEAR
PSHEAR
pshear.
CTETRA
PSOLID
psolid.
CTRIA3
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp.
CTRIA6
PSHELL
pshell.
(See PSHELL comments below.)
PCOMP
pcomp.
A new material named pcomp.
CTRIAR
PSHELL
pshellr.
(See PSHELL comments below.)
PCOMP
pcompr.
A new material named pcomp.
CTRIAX6
ctriax6
CTUBE
PTUBE
ptube.
CVISC
PVISC
pvisc.
PLOTEL
Tapered tubes are converted to an equivalent constant section definition. Creates the connectivity only. These elements are not assigned to any property set region. PLOTEL entries will not be written when a new input file is created.
MBOLTU S
Defines a bolt in the form of an Overclosure MPC.
Higher order elements (CQUAD8, CTRIA6, CTRIAX6, CHEXA, CPENTA, CTETRA) will generate linear elements in Patran if none of the mid-edge nodes are specified.
Chapter 5: Read Input File 559 Data Translated from the NASTRAN Input File
PSHELL Properties PSHELL properties can be imported as any one of five Patran property types. The MID1, MID2, MID3, 12I/T3, and TS/T property fields are used to determine which one to choose. If MID2 is -1 and MID3 is 0, then a Plane Strain property set is used. If MID2 and MID3 are both 0, then a Membrane property set is chosen. If MID1 and MID3 are 0, then a Bending property set is used. If MID1, MID2, and MID3 are all the same, and the MD Nastran defaults are used for 12I/T3 and TS/T, then a Homogeneous property set is used. If all else fails, then an Equivalent Section property set is chosen. BAROR and BEAMOR Definitions The BAROR and BEAMOR data is merged onto the CBAR and CBEAM entries using the proper MD Nastran conventions. The data is treated as if it had originally been defined on the CBAR and CBEAM entries. When a new NASTRAN input file is created, the data will remain with the CBAR and CBEAM entries. No BAROR or BEAMOR entries are generated. Fields If a field is required to store varying data, the field will have the same name as the property set, with the name of the specific property word appended to it. For example, if property set “pshell.101” has a varying thickness, the field will be named “pshell.101.Thickness”. Referential Integrity Nodes and coordinate frames referenced on elements or element properties must exist, but they do not need to be in the input file. They could also have been defined in the Patran database prior to the import. If a material is referenced, but can not be found, a new material with no properties will be created. A message will be issued indicating the creation of this material. If an element property set is referenced, but can not be found, a new property set with no properties will be created. A message will be issued indicating the creation of this property set. Set Name Extensions In some cases, the data found on the element can not be defined in Patran in a single property set. In those cases, multiple property sets will be created to define the distinct definitions. The table below defines extensions to the Property Set Names shown in the previous table. If the values on the specified field changes, a new property set with the indicated extension will be created. If all elements which reference a single PID can be stored in a single property set, then no extension will be added to the Property Set Name. Element CBAR
Field
Extension
PA
.pa
PB
.pb
Comments
560
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Element
Field
Extension
SA
.sa<SA>
SB
.sb<SB>
PA
.pa
PB
.pb
CDAMP1, CDAMP2,
C1
.ca
CELAS1, CELAS2,
C2
.cb
CDAMP3, CDAMP4,
C1
.ca1
CELAS3, CELAS4,
C2
.cb1
CGAP, CONM1, CONM2
CID
.c
CONROD, CTRIAX6
MID
.m<MID>
CQUAD4, CQUAD8,
MCID
.c<MCID>
CBEAM
Comments
CMASS1, CMASS2 These are automatically treated as component 1 (X translation).
CMASS3, CMASS4
CQUADR, CTRIA3, CTRIA6, CTRIAR
Materials The following MD Nastran material definitions can be read into Patran. Material Type
Material Name
Comments
CREEP MAT1
mat1.<mid>
The MCSID field is not currently supported. If the G field is blank in the input file, the MD Nastran default value will be filled in during import.
MATT1 MAT2
mat2.<mid>
MATT2 MAT3 MATT3 MAT4
mat3.<mid>
The MCSID field is not currently supported.
Chapter 5: Read Input File 561 Data Translated from the NASTRAN Input File
Material Type
Material Name
Comments
MATT4 MAT5 MATT5 MAT8
mat8.<mid>
MAT9
mat9.<mid>
MATT9
MPCs The following MD Nastran MPC and rigid element definitions can be read into Patran. Card Type MPC
MPC Type Explicit
Comments Unique MPC IDs will be assigned to these entities. Since Patran uses a slightly different basis MPC equation, the equation coefficients (Ai) will probably be scaled by a constant multiplier during import. The resulting equation will be equivalent, but not necessarily identical to the original definition in the NASTRAN input file.
RBAR
RBAR
RBE1
RBE1
RBE2
RBE2 Fixed
RBE3
RBE3
RROD
RROD
RSPLINE
RSPLINE
RSSCON
RSSCON
RTRPLT
RTRPLT MPCs in Patran are treated as elements and are not associated to load cases. As a result, all SUBCASE related data is lost. The MPCs are simply imported into the model and are no longer associated to a specific load case. MPCs can reference SPOINTs instead of GRIDs. If this is detected, the corresponding component field will be set to 1 (UX) to be consistent with the import of SPOINTs. The MPCADD command is not read since the MPCs are simply imported and no associated to a load case. The SID references on the MPC entry are also lost for the same reason. New MPC IDs are assigned to these elements during import.
562
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
Load Sets The following MD Nastran Loads and Boundary Condition definitions can be read into Patran. Card Type
LBC Set Name
FORCE
force.<sid>
GRAV
grav.<sid>
MOMENT
moment.<sid>
PLOAD1
pload1.<sid>
PLOAD2
pload2.<sid>
PLOAD4
pload4.<sid>
PLOADX1
ploadx1.<sid>
CONV
conv.
Comments
Only PLOAD1s applied to the entire length of an element can be read. If a load is applied only to a portion of an element, the load will be ignored, and a message will be presented indicating the problem. Only pressure loads normal to the surface can be imported. If a surface traction is detected, it will be ignored, and a message will be presented indicating the problem.
PCONV CONVM
convm.
PCONVM QBDYi
qbdyi.
QVECT
qvect.
QVOL
qvol.
RADBC
radbc.
RADCAV
radcav.
Note: ELEAMB field is not supported by Patran. The ambient element is added to the application region.
rforce.<sid>
If the G point is not at the origin of the referenced CID, a new CID will be created and referenced.
RADM RADMT RFORCE
The METHOD field is not read. It is automatically set to 1 when writing a new file. SLOAD
sload.
TEMP
temp.<sid>
TEMPP1
tempp1.<sid>
Only the average temperature and effective linear gradient data fields are used. The specified temperatures at the Z1 and Z2 locations are ignored.
Chapter 5: Read Input File 563 Data Translated from the NASTRAN Input File
Card Type
LBC Set Name
TEMPRB
temprb.<sid>
grid#
grid.ps
SPC
spc.<sid>
Comments Only the average temperature and effective linear gradient data fields are used. The specified temperatures at the stress recovery locations are ignored.
SPCADD SPC1
spc1.<sid>
SPCD
spcd.<sid>
The required SPC or SPC1 entries for the same Degree-of-Freedom are removed from the load case when a SPCD is found. They will automatically be re-generated when a new input file is created.
VIEW VIEW3D Fields If a field is required to store varying data, the field will have the same name as the load set, with the name of the specific data word appended to it. For example, if load set “force.101” has a varying force magnitude, the field will be named “force.101.Force”. Load cases are created in Patran from the SUBCASE definitions in the NASTRAN input file. Load sets not referenced by a SUBCASE definition are created as load sets in Patran, but are not associated to a load case. Load sets defined above the first SUBCASE command, plus any permanent single point constraint sets from the GRID entries, are associated to all load cases created during this import. If there is no case control data, then load sets will be created, but they will not be assigned to any load cases. The SPCADD and LOAD entries are used in creating load cases in Patran, but the SID of these entries is lost. The SIDs on the individual SPCx, FORCE, MOMENT, GRAV, PLOADx, RFORCE, and TEMPx entries are used in creating the names of the load sets. The name for the created load cases is derived from the subtitle of the SUBCASE. This is done for consistency with the forward PAT3NAS translation. A job is created during the import. The name of the created job is the basename of the file being read. MD Nastran allows load sets to be referenced in multiple places with different scale factors. This is not possible in Patran. Therefore, in some cases, multiple copies of the same load set need to be created with the only difference being the scale factor. The name of these load sets are modified to include the subcase ID to create unique names.
564
Patran Interface to MD Nastran Preference Guide Data Translated from the NASTRAN Input File
TABLES The following table types are supported during import of a NASTRAN input file. Note that some forms of the table commands are converted to an equivalent version supported by Patran. Card Type
Field Name
Comments
TABLED1
Field.
TABLED2
Field.
Converted to an equivalent TABLED1 when read into Patran by NIFIMP.
TABLED3
Field.
Converted to an equivalent TABLED1 when read into Patran by NIFIMP.
TABLEM1
Field.
TABLEM2
Field.
Converted to an equivalent TABLEM1 when read into Patran by NIFIMP.
TABLEM3
Field.
Converted to an equivalent TABLEM1 when read into Patran by NIFIMP.
SOL 600 entries
Note:A
Additional entries specific to SOL 600 can be read into Patran. For more details see MD Nastran Implicit Nonlinear (SOL 600), 14.
Chapter 5: Read Input File 565 Conflict Resolution
5.3
Conflict Resolution If an entity can not be imported into Patran because another entity already exists with that ID or name, then the conflict resolution logic is used. There are 2 different approaches taken, depending on whether the entity is identified by an ID or by a name.
Conflict Resolution for Entities Identified by IDs If a new definition conflicts with a definition already in the Patran database, you will be asked if you want the ID of the new definition offset. If you select YES, a new ID will be chosen. If you select YES FOR ALL, a new ID will be chosen for this definition, as well as for any others found to be in conflict. In this case, then all references to the ID in the original Patran database will still reference the old ID, but references to the ID from within the input file will be altered to reference the new ID. If you do not want the CID to be offset, then you will be asked if you want the new definition to overwrite the existing definition. If this is done, then all references to this ID from both the original Patran database and the input file will be referencing the same ID. The definition for that ID will be either the old or the new definition, depending on how this second question is answered.
Conflict Resolution for Entities Identified by Names The user is not asked what to do in cases where the conflicting entities are identified by names. The name for the new entity will be modified by appending an extension to the name. The new name will be “
566
Patran Interface to MD Nastran Preference Guide Conflict Resolution
Chapter 6: Delete Patran Interface to MD Nastran Preference Guide
6
Delete
Review of Delete Form
568
Deleting an MD Nastran Job
569
568
Patran Interface to MD Nastran Preference Guide Review of Delete Form
6.1
Review of Delete Form The Analysis form will appear when the Analysis toggle, located on the Patran main form, is chosen and the selected Action is Delete.
The Delete option under Action allows the user to delete jobs that have been created for the MD Nastran preference.
Chapter 6: Delete 569 Deleting an MD Nastran Job
6.2
Deleting an MD Nastran Job This format of the Analysis form appears when the Action is set to Delete. The user may delete job definitions that were created for the MD Nastran preference with this form.
Indicates the selected Analysis Code and Analysis Type, as defined in the Preferences>Analysis (p. 431) in the Patran Reference Manual.
List of already existing jobs. Select the jobs that are to be deleted.
Deletes the jobs selected in the Existing Jobs listbox.
570
Patran Interface to MD Nastran Preference Guide Deleting an MD Nastran Job
Chapter 7: Files Patran Interface to MD Nastran Preference Guide
7
Files
Files
572
572
Patran Interface to MD Nastran Preference Guide Files
7.1
Files The Patran MD Nastran interface uses or creates several files.The following table outlines each file and its uses. In the file name definition, jobname will be replaced with the jobname assigned by the user. File Name
Description
*.db
This is the Patran database. During an analyze pass, model data is read from this database and, during a Read Results pass, model and/or results data is written into it. This file typically resides in the current directory.
jobname.jbr
These are small files used to pass certain information between Patran and the independent translation programs during translation. There should never be a need to directly alter these files. These files typically reside in the current directory.
jobname.bdf
This is the NASTRAN input file created by the interface. This file typically resides in the current directory.
msc_v#_sol#.alt
These are a series of MD Nastran alters that are read during forward translation. These alters instruct MD Nastran to write information to the OUTPUT2 file that the results translation will be looking for. The forward translator searches the Patran file path for these files, but they typically reside in the
jobname.op2
This is the MD Nastran OUTPUT2 file, which is read by the Read Results pass. This file typically resides in the current directory and contains both model and results data. It is created by placing a PARAM,POST,-1 in the input file.
jobname.xdb
This is the MD Nastran XDB file or MSC.Access database, which is attached by the Read Results pass. This file typically resides in the current directory and contains results data. It is created by placing a PARAM, POST,0 in the input file.
jobname.marc.t16
SOL 600 file recommended for use in postprocessing SOL 600 analyses.
jobname.flat
This file may be generated during a Read Results pass. If the results translation cannot write data directly into the specified Patran database it will create this jobname flat file. This file typically resides in the current directory.
jobname.marc.xxx
File generated by a SOL 600 analysis. See the “MD Nastran Implicit Nonlinear (SOL 600) User’s Guide” for a complete list.
Chapter 7: Files 573 Files
File Name
Description
jobname.msg.xx
These message files contain any diagnostic output from the translation, either forward or reverse. This file typically resides in the current directory.
MscNastranExecute
This is a UNIX script file, which is called on to submit MD Nastran after translation is complete. This file might need customizing with site specific data, such as, host machine name and MD Nastran executable commands. This file contains many comments and should be easy to edit. Patran searches its file path to find this file, but it typically resides in the
574
Patran Interface to MD Nastran Preference Guide Files
Chapter 8: Errors/Warnings Patran Interface to MD Nastran Preference Guide
8
Errors/Warnings
Errors/Warnings
576
576
Patran Interface to MD Nastran Preference Guide Errors/Warnings
8.1
Errors/Warnings There are many error or warning messages that may be generated by the Patran MD.Nastran Interface. The following table outlines some of these. Message
Description
Unable to open a new message file " ". Translation messages will be written to standard output.
If the translation tries to open a message file and cannot, it will write messages to Standard Output. On most systems, the translator automatically writes messages to standard output and never tries to create a separate message file.
Unable to open the specified OUTPUT2 file "
The OUTPUT2 file was not found. Check the OUTPUT2 file specification in the translation control file.
".
The specified OUTPUT2 file " " is not in standard binary format and cannot be translated.
The OUTPUT2 file is not in standard binary format. Check the OUTPUT2 file specification in the translation control file.
Group " " does not exist in the database. Model data will not be translated.
The name of a nonexistent group was specified in the translator control file. No model data will be translated from the OUTPUT2 file.
Needed file specification missing! The full name of the job file must be specified as the first commandline argument to this program.
The translation control file must be specified as the first online argument to the translator.
Unable to open the specified database " ". Writing the OUTPUT2 information to the PCL command file " ".
If the translator cannot communicate directly to the specified database. It will write the results and/or model data to a PCL session file.
Unable to open either the specified database " PCL command file, " ". Unable to open the NASTRAN input file " Unable to open the specified database, "
", or a The naspat3 translator is unable to open any output file. Check file specification and directory protection. ".
".
The translator was unable to open a file to where the input file information will be written. The forward Patran MD.Nastran translator was unable to open the specified Patran database.
Alter file of the name " " could not be found. No The OUTPUT2 DMAP alter file, for this type of analysis, OUPUT2 alter will be written to the NASTRAN input could not be found. Correct the search path to include the file. necessary directory if you want the alter files to be written to the input file. No property regions are defined in the database. No elements or element properties can be translated.
Elements referenced by an element property region in the Patran database will not get translated by the forward Patran MD.Nastran translator. If no element regions are defined, no elements will be translated.
Chapter A: Preference Configuration and Implementation Patran Interface to MD Nastran Preference Guide
A
Preference Configuration and Implementation
Software Components in Patran MD Nastran
578
Patran MD Nastran Preference Components
579
Configuring the Patran MD Nastran Execute File
582
578
Patran Interface to MD Nastran Preference Guide Software Components in Patran MD Nastran
1.1
Software Components in Patran MD Nastran The Patran MD Nastran product includes the following items: • A PCL function contained in p3patran.plb that will add MD Nastran specific definitions to
any Patran database (not already containing such definitions) at any time. • A PCL library called mscnastran.plb and contained in the
directory. This library is used by the analysis forms to produce forms for analysis code specific translation parameter, solution parameter, etc. • A script file called MscNastranExecute, contained in the
directory. This script controls the operation of the interface and the submission of MD Nastran analyses. This script can be run independent of Patran but typically run from within Patran, transparent to the user. • Several MD Nastran alter files are included. These files are used when creating the NASTRAN
input file. They ask MD Nastran to produce the results file required by the NASPAT3 results translator. These files can be found in the
is also provided to allow the direct access to this information from within Patran.
Chapter A: Preference Configuration and Implementation 579 Patran MD Nastran Preference Components
1.2
Patran MD Nastran Preference Components The diagrams shown below indicate how the functions, scripts, programs, and files that constitute the Patran MD Nastran interface affect the Patran environment. Site customization, in some cases, is indicated. Figure A-1 shows the process of running an analysis. The mscnastran.plb library defines the Translation Parameter, Solution Type, Solution Parameter, and Output Request forms called by the Analysis form. When the Apply button is pushed on the Analyze form, the interface process is initiated. The interface reads data from the database and creates the NASTRAN input file. Status messages from the interface are recorded in the Patran session file. A series of MD Nastran alter files is provided. They may be used during the creation of the input file depending upon the selected solution type and solution parameters. These alter files are mostly used in support of older solution sequences. If the interface successfully produces a NASTRAN input file, and the user requests it, the MscNastranExecute script will then start MD Nastran.
Patran
p3patran.plb
Analysis mscnastran.plb
Analyze
MscNastranExecute Patran Database Alter Library
jobname.bdf
Figure A-1
MD Nastran
Forward Translation
Figure A-2 shows the process of reading information from an MD Nastran OUTPUT2 file. When the Apply button is selected on the Read Output2 form, a <jobname>.jbr file is created and the results translation is started. The results interface process reads the data from the MD Nastran OUTPUT2 file
580
Patran Interface to MD Nastran Preference Guide Patran MD Nastran Preference Components
and stores the results in the Patran database. Status messages from the interface are recorded in the Patran session file.
p3patran.plb Patran Analysis
mscnastran.plb
Read Output2
jobname.jbr Patran database
MD Nastran
Figure A-2
jobname.OP2
OUTPUT2 File Translation
Figure A-3 shows the process of translating information from a NASTRAN input file into a Patran database. The behavior of the main Analysis/Read Input File form and the subordinate file select form is
Chapter A: Preference Configuration and Implementation 581 Patran MD Nastran Preference Components
dictated by the mscnastran.plb PCL library. The Apply button on the main form activates the input file reader program, which reads the specified NASTRAN input file.
Patran p3patran.plb Analysis
Read Input File
mscnastran.plb
MD Nastran Input
Patran database
File Reader
NASTRAN Input File
input_file_name.error.* Figure A-3
NASTRAN Input File Translation
582
Patran Interface to MD Nastran Preference Guide Configuring the Patran MD Nastran Execute File
1.3
Configuring the Patran MD Nastran Execute File During the installation of the Patran MD Nastran analysis preference, the mscsetup utility creates a default site_setup file in the installation directory. This file sets environment variables relating to Patran. To custom configure this site_setup file consult Environment Variables (p. 48) in the Patran Installation and Operations Guide.
MSC.Fatigue Quick Start Guide
Index Patran Interface to MD Nastran Preference Guide
Numerics
3rd Order Invariant, 76 I n d e x
Pa tra n Int erf ac e to M
A
ACFPMRESULT, 419 ACPOWER, 419 Adaptive Meshing, 413 adaptive meshing, 501 alternate reduction, 278, 474 ALTERS, 578 Alters, 265 ALTRED, 278, 474 analysis coordinate frames, 23 analysis form, 261 analysis job definition, 263 analysis job submittal, 263 analysis preferences, 6 analyze, 260 Arruda-Boyce model, 78
B
BCBODY, 14 BCBOX, 14 BCHANGE, 14 BCMATL, 14 BCMOVE, 14 BCPARA, 14 BCPROP, 14 BCTABLE, 14 BEGIN AFPM, 178, 419 BEGIN BULK SUPER, 267, 352 BSURF, 14 buckling, 287 bulk data, 9 bulk data file, 546
C
CACINF3, 195
CACINF4, 195 case control, 9 CBAR, 103 CBEAM, 107, 115, 120 CBEND, 110, 113 CDAMP1, 98, 140 CELAS1, 97, 138 CGAP, 142 CHEXA, 206 CMASS1, 93, 145 complex Eigenvalue, 291 CONM1, 91 CONM2, 94 contact penetration, 308 contact bodies deformable surfaces defining in MSC.Patran, 241, 242 rigid surface defining in MSC.Patran, 243 slideline defining in MSC.Patran, 240 coordinate frames, 22, 510 analysis, 23 reference, 23 coordinates, 266 COUPMASS, 283 CPENTA, 206 CQUAD4, 155, 158, 161, 164, 167, 168, 171, 174, 177, 179, 183, 190, 191, 198, 200 CQUAD8, 155, 164, 168, 179, 190, 198 CQUADR, 181 CREEP, 84 CROD, 131, 134 CSHEAR, 204 CTETRA, 206 CTRIA3, 155, 161, 164, 168, 174, 177, 179, 183, 190, 198 CTRIA6, 155, 164, 168, 179, 190, 198 CTRIAR, 158, 167, 171, 181, 191, 200
584 Patran Interface to MD Nastran Preference Guide
CTRIAX, 187 CTRIAX6, 186 CTUBE, 136 CVISC, 142 CYAX, 48 cyclic symmetry, 30, 48, 278, 287, 296, 474 CYJOIN, 48 CYSYM, 48
D
DCONSTR, 479 degrees-of-freedom, 31 DESGLB, 479 DISPLACEMENT, 419 displacements, 226, 231 distributed load, 226 DOPTPRM, 470, 479 DPHASE, 231, 232 DRESP1, 479 DRESP2, 479 dynamic reduction, 286 DYNRED, 286
E
EIGB, 289 EIGC, 294 Eigenvalue extraction, 282, 287 buckling, 289 complex, 294 real, 284 EIGR, 284 EIGRL, 289 element properties, 87
elements, 510 2d solid, 190, 191 acoustic field point mesh, 177 axisymmetric solid, 186, 187 coupled point mass, 91 curved general section, 110 curved pipe, 113 gap, 142 general beam, 124 general section beam, 102 general section rod, 131, 134 grounded scalar damper, 98 grounded scalar mass, 93 grounded scalar spring, 97 infinite exterior acoustic, 195 lumped area beam, 115 lumped point mass, 94 p-formulation, 18, 209 P-Formulation bending panel, 183 P-Formulation Equivalent Section plate, 174 P-Formulation general section beam, 107 P-Formulation homogeneous plate, 161 P-Formulation Membrane, 201 P-Formulation Plane Strain Solid, 193 pipe section, 136 plotel, 146 revised bending panel, 181 revised equivalent section plate, 171 revised homogeneous plate, 158 revised laminate plate, 166 revised membrane, 199 revised plane strain solid, 191 scalar damping, 139 scalar mass, 144 scalar spring, 137 shear panel, 204 solid, 206 standard bending panel, 179 standard equivalent section plate, 168 standard homogeneous plate, 155 standard laminate plate, 163 standard membrane, 197 standard plane strain solid, 190 tapered beam, 119 viscous damper, 141 ELSDCON, 420
INDEX 585
Environment Variables ACommand20xx, 494 ACommandNasServer, 494 DRA_NAST_NOVEDRCHK, 494 MSCP_NASTRAN_SERVER, 494 MSP_NASTRAN_CMD20xx, 494 errors, 576 ESE, 419 executive control, 9
F
failure criteria, 81, 82 FEEDGE, 18 FEFACE, 20 files, 572 finite elements, 23, 24 FMS, 9 Foam model, 76 follower forces, 280 FORCE, 232, 233, 419 force, 226, 232 frequency response, 296
G
Gent model, 78 GEOM1, 510 GEOM2, 510 GMBC, 20 GMNURB, 14 GPFORCE, 420 GRAV, 236 GRDPNT, 283
I
inertia relief, 278, 474 inertial load, 236 initial conditions, 226, 237 initial load, 226 initial velocity, 226 input file, 546 INREL, 278, 474 INTENSITY, 419 IPSTRAIN, 14
ISTRESS, 14 iteration parameters, 391 iterations static nonlinear, 359
J
Jamus-Green-Simpson model, 75, 76
K
keywords POST, 315 REAUTO, 315, 461
L
large displacements, 280 LGDISP, 281 linear static, 277 linear surf-vol, 28 linear transient, 299 load cases, 246 loads and boundary conditions, 224
M
MARCIN, 14 MARCOUT, 14 Mass properties, non-structural (MSC.Nastran), 445 MAT1, 73, 81, 82 MAT2, 81, 82 MAT3, 73 MAT8, 73, 81, 82 MATEP, 14, 15, 78 materials, 59 2D anisotropic, 68, 73, 74 2D orthotropic, 65, 72 3D anisotropic, 68, 73, 74 3D orthotropic, 67, 72 composite, 68, 85 Fluid, 68 isotropic, 62, 69, 73, 74 MATF, 14, 15, 82 MATG, 14 MATHE, 14, 15, 75 MATORT, 14, 15, 73
586 Patran Interface to MD Nastran Preference Guide
MATS1, 74, 75, 78 MATTEP, 14, 15 MATTF, 82 MATTG, 14 MATTHE, 14, 15 MATTi, 73 MATTORT, 14 MATTVE, 14, 85 MATVE, 15, 85 MATVP, 15, 84 model data, 496 MOMENT, 232 Mooney-Rivlin model, 75, 76 MPC, 28, 31, 48 MSC.Nastran enhancements Non-structural mass properties, 445 MSC.Nastran version, 266, 267, 497, 498, 500 multi-point constraints, 27
N
Neo-Hookean, 76 NLAUTO, 15 NLDAMP, 15 NLLOAD, 419 NLPARM, 359 NLSTRAT, 15 nodes, 23, 266, 510 nonlinear elastic, 74 nonlinear statics, 279 nonlinear transient, 302 Non-Structural mass properties (MSC.Nastran), 445 normal nodes, 282 NSM and NSML forms (MSC.Nastran), 445 NTHICK, 15 numbering options, 268
O
OEF1, 502, 503 OESNL1, 503 Ogden model, 76 OLOAD, 419 ONRGY1, 505 OPG1, 505 OPHIG, 506
OPNL1, 506 optimize, 463 optimization parameters, 467 subcase create, 471 subcase parameters, 474 subcase select optimize, 475 topology optimization, 476 OSTR1, 502, 503 OUGV1, 505 output requests, 415 OUTPUT2, 265 OUTRCV, 20
P
PACINF, 195 PARAM, SNORM, 278, 283, 292, 297, 300, 324 PARAMARC, 15 PBAR, 103 PBCOMP, 115 PBEAM, 107, 120 PBEND, 110, 113 PCOMP, 82, 85, 164, 167 PDAMP, 98, 140 PELAS, 97, 138 penetration, 308 PGAP, 142 PLOAD4, 233 PLOADX1, 233 PMASS, 93, 145 POINT, 18 Postprocessing, 413 preferences, 6 pressure, 226, 233 PROD, 131 properties, 87 PSHEAR, 204 PSHELL, 155, 158, 168, 171, 179, 181, 190, 191, 198, 200 PSOLID, 206 PTUBE, 136 PVISC, 142
R
RBAR, 28, 34 rbar1, 50
INDEX 587
RBE1, 28, 36 RBE2, 29, 33, 38 RBE3, 29, 40 read input file, 546 reference coordinate frames, 23 RESTART, 15 restart file, 316, 462 results, 492 element, 436 nodal, 434 supported entities, 502, 516 types, 511 results output format, 348 RFORCE, 236 rjoint, 53 RLOAD1, 231 RROD, 29, 42 RSPLINE, 29, 44 RSSCON, 28 RTRPLT, 30, 46 rtrplt1, 51
S
SESET, 352 SETREE, 352 sliding surface, 30, 48 solution parameters, 277 SOL 109, 299 SOL 112, 299 SOL 27, 299 SOL 31, 299
solution sequences SOL 1, 272, 278 SOL 101, 272, 278 SOL 103, 273 SOL 105, 273, 287 SOL 106, 273, 279 SOL 107, 291 SOL 108, 273, 296 SOL 109, 273 SOL 110, 273, 291 SOL 111, 273, 296 SOL 112, 273 SOL 114, 272, 278 SOL 115, 273 SOL 118, 273, 296, 297 SOL 129, 273, 302 SOL 147, 273 SOL 26, 273, 296 SOL 27, 273 SOL 28, 273, 291 SOL 29, 273, 291 SOL 3, 273 SOL 30, 273, 296 SOL 37, 273 SOL 47, 272, 278 SOL 48, 273 SOL 5, 273, 287 SOL 600, 273, 304, 324, 326 SOL 66, 273, 279 SOL 77, 273, 287 SOL 99, 273, 302 solution types, 271 SPC1, 231 SPCD, 231 SPCFORCES, 419 SPCR, 232 static data, 226 STRAIN, 419, 420 STRESS, 419, 420 structural damping, 293, 301, 303 superelements, 267, 352 supported entities, 8
T
t16 file, 511, 543
588 Patran Interface to MD Nastran Preference Guide
TABLEDi, 231, 232 TABLEMi, 73 TABLES1, 75 TEMP, 235 temperature, 226, 235 TEMPP1, 235 TEMPRB, 235 TIC, 237 time dependent, 229 tolerances, 265, 496, 498, 500 TOPVAR, 479 translation parameters, 265, 496, 498 TSTEPNL, 362, 409
V
VECTOR, 419 VU mesh, 20
W
warnings, 576 WTMASS, 283
Related Documents
More Documents from "Kevin"
Resumen De La Exposicion De Regimen.docx
November 2019 7
What Is Hiv Lbl F.docx
May 2020 4
Centrobiblia
May 2020 1