Marc 2008 R1 Volume C: Program Input

Marc 2008 r1 ®

Volume C: Program Input

Main Index

Corporate MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 Telephone: (800) 345-2078 FAX: (714) 784-4056

Europe MSC.Software GmbH Am Moosfeld 13 81829 Munich GERMANY Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6

Asia Pacific 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 User Documentation: Copyright © 2008 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved. This document, and the software described in it, are furnished under license and may be used or copied only in accordance with the terms of such license. Any reproduction or distribution of this document, in whole or in part, without the prior written authorization of MSC.Software Corporation is strictly prohibited. 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 document are for illustrative and educational purposes only and are not intended to be exhaustive or to apply to any particular engineering problem or design. THIS DOCUMENT IS PROVIDED ON AN “AS-IS” BASIS AND ALL EXPRESS AND IMPLIED CONDITIONS, REPRESENTATIONS AND WARRANTIES, INCLUDING ANY IMPLIED WARRANTY OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE, ARE DISCLAIMED, EXCEPT TO THE EXTENT THAT SUCH DISCLAIMERS ARE HELD TO BE LEGALLY INVALID. MSC.Software logo, MSC, MSC., MD Nastran, Adams, Dytran, Marc, Mentat, and Patran are trademarks or registered trademarks of MSC.Software Corporation or its subsidiaries in the United States and/or other countries. NASTRAN is a registered trademark of NASA. Python is a trademark of the Python Software Foundation. LS-DYNA is a trademark of Livermore Software Technology Corporation. All other trademarks are the property of their respective owners. This software may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. METIS is copyrighted by the regents of the University of Minnesota. HP MPI is developed by Hewlett-Packard Development Company, L.P. MS MPI is developed by Microsoft Corporation. PCGLSS 6.0, copyright © 1992-2005 Computational Applications and System Integration Inc. MPICH Copyright 1993, University of Chicago and Mississippi State University. MPICH2 copyright © 2002, University of Chicago. Use, duplication, or disclosure by the U.S. Government is subject to restrictions as set forth in FAR 12.212 (Commercial Computer Software) and DFARS 227.7202 (Commercial Computer Software and Commercial Computer Software Documentation), as applicable.

MA*V2008r1*Z*Z*Z*DC-VOL-C

Main Index

Contents Marc Volume C: Program Input

Contents

Preface About this Manual, 26 Who Should Read this Manual, 26 Other Marc Manuals, 26 Chapter Contents, 26

1

Introduction Formats in Marc, 30 Fixed Field, 30 Free Field, 30 Input of List Items, 31 Examples, 33 Edges and Faces, 33 Guide to Organization of Marc Input Data, 40 Typical Marc Problem Data Files, 41 Marc Input for New Users, 42 Discussion of Marc Output for New Users, 51

2

Parameters List

2

Parameters Basic Input Requirements, 71 TITLE — Output Title Definition, 72 ALLOCATE — Initial Workspace Definition, 73 SIZING — Working Space Definition, 74 PREALLOC — Initial Workspace Allocation, 75 ELEMENTS — Element Type Selection, 76 VERSION — Indicate the Version of the Marc Input Data File, 77 FEATURE — Specification of the Behavior of a Feature, 78 PROCESSOR — Parallelization Control, 80 UNIT — Invoke Unit System Definition, 82 $NO LIST — No Listing of Input Data, 83

Main Index

4 Marc Volume C: Program Input

EXTENDED — Extended Precision of Reading in Data, 84 END — End of Parameter Section, 85 Analysis Types, 87 ELASTIC — Elastic Analysis with Multi-loads, 88 DESIGN SENSITIVITY — Perform Sensitivity Analysis Only, 89 DESIGN OPTIMIZATION — Perform Design Optimization, 90 ADAPTIVE — Adaptive Mesh Refinement, 91 LINEAR — Matrices Saved for Linear Analysis, 93 FOURIER — Arbitrary Loading of Axisymmetric Structures, 94 DYNAMIC — Dynamic Analysis, 95 HARMONIC — Frequency Response Analysis, 97 SS-ROLLING — Steady State Transport Analysis, 98 RESPONSE — Spectrum Response Analysis, 99 R-P FLOW — Rigid-Plastic Flow, 100 SPFLOW — Superplastic Forming Analysis, 101 LARGE DISP — Large Displacement or Buckling, 102 LARGE STRAIN — Large Strain Analysis with Updated Lagrange Formulation, 103 UPDATE — Updated Lagrange Procedure, 105 FINITE — Finite Strain Plasticity, 106 CONSTANT DILATATION — Define That Elements Are to Use Constant Dilatation Formulation, 107 ASSUMED STRAIN — Improved Bending Behavior, 108 ELASTICITY — Elasticity Procedure, 109 PLASTICITY — Plasticity Procedure, 110 FOLLOW FOR — Follower Forces: Distributed and Point Load Application on Current Geometry – Application of Total Boundary Condition, 111 BUCKLE — Buckling Load Estimation via Eigenvalue Analysis, 113 CREEP — Creep Analysis, 114 VISCO ELAS — Visco Elastic Analysis (Kelvin Model), 115 STRUCTURAL — Mechanical Analysis, 116 COUPLE — Coupled Thermal-Stress Analysis, 117 DECOUPLING — Set Control for Contact Decoupling Analysis, 118 FLUID — Fluid, Fluid-Thermal, Fluid-Solid, and Fluid-Thermal-Solid Analysis, 119 PORE — Soil Analysis, 121 T-T-T — Time-Temperature-Transformation, 122 HEAT — Heat Transfer (Conduction) Analysis, 123 JOULE — Joule Heating (Coupled Thermo-Electrical) Analysis, 124 DIFFUSION — Diffusion Analysis, 125 ABLATION — Specify Ablation Occurrence, 126 PYROLYSIS — Indicates Thermo-poro-ablative Model Analysis, 127 CURING — Curing Analysis Parameter Definition, 128 BEARING — Bearing Analysis, 129 ELECTRO — Electrostatic Analysis, 130 MAGNETO — Magnetostatic Analysis, 131 EL-MA — Perform Electromagnetic Analysis, 132

Main Index

5

PIEZO — Activate Piezoelectric Analysis, 133 ACOUSTIC — Acoustic Analysis, 134 RADIATION — Radiation Analysis, 135 CAVITY — Volume-dependant Pressure Load for Cavities, 138 RBE — Rigid Body Elements, 139 MACHINING — NC Machining (Metal Cutting) Process Analysis, 140 Rezoning and Substructure Parameters, 141 REZONING — Allow Rezoning, 142 MNF — MD ADAMS Modal Neutral File Options, 143 SUPER — Super Element Input, 144 USER — Create User-defined Element, 145 Additional Flags for Various Analyses, 147 CENTROID — State Storage at Centroid Only, 148 ALL POINTS — State Storage at All Points, 149 LOAD COR — Residual Load Correction, 150 NO LOADCOR — Suppression of Load Correction, 151 SCALE — Scaling to First Yield, 152 THERMAL — Thermal Stress Analysis, 153 ISTRESS — Define Initial Stress, 154 LUMP — Lumped Mass or Specific-Heat Matrix, 155 APPBC — Application of Boundary Conditions, 156 ACCUMULATE — Accumulation of Strain and Displacements, 157 ALIAS — Define Aliases, 158 Program Function and I/O Controls, 159 NEW — Use New Format, 160 TABLE — Indicate How Tables are to be used, 161 COMMENT — Define Comment, 162 PRINT — Debug Printout, 163 STOP — Exit following Workspace Allocation, 166 NOTES — Print Notes and Updates, 167 INPUT TAPE — Specify Device for Model Definition Data, 168 ELSTO — Out-of-Core Storage of Elements, 169 OOC — Out-of-core Solver, 170 IBOOC — Out-of-core Storage of Incremental Backup Data, 171 NO ECHO — Suppress Echo, 172 INCLUDE — Insert File into the Input File, 173 Modifying Default Values, 174 STATE VARS — Define Number of State Variables, 175 DIST LOADS — Distributed Loads or Point Loads, 176 FLUXES — Distributed Fluxes or Point Fluxes, 177 FILMS — Film Coefficients, 178 RESTRICTOR — Restrictor Input in Lubrication Analysis, 179 WELDING — Welding Analysis, 180

Main Index

6 Marc Volume C: Program Input

BOUNDARY CONDITIONS — Specify Maximum Number of Boundary Conditions to be Defined, 181 SHELL SECT — Define Number of Layer Through Shell Thickness, 182 TSHEAR — Transverse Shear for Elements 22, 45, 75, 140, and 185, 183 TIE — Define Tying Data, 184 MPC-CHECK — Multi-point Constraint Checking Parameter, 185 AUTOMSET — Modify Relationship Between Tied and Retained Nodes, 186 AUTOSPC — Automatically Apply Constraints to Eliminate Rigid Body Modes, 188 IO-DEACTIVATE — Deactivate Element if it goes Inside-out, 189 Defining Cross-sections of Beam Elements, 190 BEAM SECT — Beam Section Definition, 191

3

Model Definition Options List

3

Model Definition Options MESH2D, 215 Two-dimensional Mesh Generator, 215 MESH2D — Define a Two-dimensional Mesh, 216 BLOCKS — Define Working Size, 217 DEFINE (Mesh2D Block Type) — Define Block Type, 218 MANY TYPES — Define Multiple Elements, 219 START NUMBER — Specify Starting Element, 220 BOUNDARY — Define Boundary Nodes, 221 SPECIFIED NODES — Specify Node Coordinates, 222 MAPPER — Invoke User Subroutine MAP2D, 223 CONSTRAINT — Generate Boundary Condition Constraints, 224 MERGE (Model Definition) — Specify Minimum Distance Between Nodes, 225 MERGE SELECTIVE — Specify Minimum Distance Between Nodes by Block, 226 CONNECT — Connect or Disconnect Mesh Blocks, 227 PRTCONNECT — Print Out Block Connections, 228 SYMMETRY — Define Axis of Symmetry, 229 GENERATE — End of Mesh Generation Data, 230 Mesh Definition, 231 NEW (Model Definition) — Use New Format, 232 DEFINE (Sets) — Define Sets, 233 CONNECTIVITY — Specify Element Connectivity, 236 CONN FILL — Specify Element Connectivity Interpolator, 238 CONN GENER — Copy Element Connectivity Data, 239 UFCONN — Invoke the UFCONN User Subroutine, 241 COORDINATES — Enter Node Coordinates, 242 INCLUDE (Model Definition) — Insert File into the Input File, 244 FXORD — Coordinate Generation and Transformation Coordinates, 245 NODE CIRCLE — Generate Coordinates for Circular Arcs, 248

Main Index

7

NODE FILL — Coordinate Interpolation for Incremental Mesh Generation, 249 NODE GENER — Generate Node Coordinates, 250 NODE MERGE — Merge Duplicate Nodes, 251 UFXORD — Invoke the UFXORD User Subroutine, 252 CYLINDRICAL — Define Cylindrical Coordinate System, 253 WRITE — Write Connectivity and Coordinates, 255 ADAPTIVE — Define Error Criteria Used in Adaptive Analysis, 256 ADAPT GLOBAL (Model Definition) — Define Meshing Parameters Used in Global Remeshing, 264 POINTS — Define Geometric Points, 274 CURVES — Define Geometric Curves, 275 SURFACES — Define Geometrical Surfaces, 280 STRING — Define Curves Forming a String for Arc Length Calculation, 286 ATTACH NODE — Define the Nodes Attached to Surfaces, 288 ATTACH EDGE — Define the Element Edges Which are Attached to Curves, 290 ATTACH FACE — Define the Element Faces which are attached to Surfaces, 291 GEOMETRY — Specify Geometrical Data, 292 NODAL THICKNESS — Define Nodal Thickness, 296 ACTUATOR — Define the Length of the Actuator Link, 297 TRANSFORMATION — Define Nodal Coordinates for Transformation, 298 COORD SYSTEM — Define Coordinate System for Nodal Coordinates and Degrees of Freedom, 301 SHELL TRANSFORMATION — Define Shell Transformation, 308 UTRANFORM — Invoke User Subroutine UTRANS, 309 CYCLIC SYMMETRY — Enter Data for a Cyclic Symmetric Structure, 310 TYING — Define Tying Constraints, 313 SERVO LINK — Input Homogeneous Linear Constraints, 321 RBE2 — Define MD Nastran RBE2 Element, 323 RBE3 — Define MD Nastran RBE3 Element, 325 RROD — Rigid 2-node Constraint, 328 PIN CODE — Define Pin Code for Beam Element, 329 INSERT — Define Host Bodies and List of Elements or Nodes to be Inserted, 330 SPRINGS — Input Linear or Nonlinear Spring (Dashpot), 332 PBUSH — Input Data for Cbush Elements, 336 CFAST — Shell Patch Fastener Connection, 344 PFAST — CFAST Fastener Property, 347 CWELD — Weld or Fastener Element Connection, 349 PWELD — Connector Element Property, 357 SWLDPRM — Parameters for CWELD Connectors, 359 SUPERELEM (Model Definition) — Perform Craig-Bampton Analysis for MD Adams MNF Interface, 365 SUPERELEM (DMIG Applications - Model Definition) — Create DMIG of Substructure, 367 DMIG-OUT (Model Definition) — Output Control of Matrices, 370 DMIG — Direct Matrix Input, 375 K2GG, K2PP (Model Definition) — Selects Direct Input Stiffness Matrix, 378

Main Index

8 Marc Volume C: Program Input

M2GG, M2PP (Model Definition) — Selects Direction Input Mass Matrix, 379 B2GG, B2PP (Model Definition) — Selects Direction Input Damping Matrix, 380 P2G (Model Definition) — Selects Direction Input Load Vector, 381 BACKTOSUBS (Model Definition) — Recover Substructure Output, 382 MNF UNITS — MD Adams Modal Neutral File Units, 383 STIFSCALE — Define Stiffness Scaling Factor, 385 COEFFICIENT — Define Scaling Coefficients for Matrices, 386 DEACTIVATE (Model Definition) — Deactivate Elements, 389 ERROR ESTIMATE — Create Error Estimation, 390 USDATA — Invoke USDATA User Subroutine for Initialization, 391 Program Control, 393 CASE COMBIN — Combine Load Cases, 394 SOLVER (Model Definition) — Specify Direct or Iterative Solver, 396 OPTIMIZE — Invoke Bandwidth Optimizers, 399 POST (Model Definition) — Create File for Postprocessing, 401 LOADCASE (Model Definition) — Define Loadcase, 418 TRACK — Enter a List of Points to be Tracked, 421 FLOW LINE — Define a Flow Line Grid, 422 IRM — Intergraph Interface, 424 SDRC — SDRC I-DEAS™ Interface, 430 HYPERMESH — HyperMesh Interface, 433 PRINT CHOICE (Model Definition) — Specify Output, 435 PRINT ELEMENT (Model Definition) — Specify Elements to be Included in Output, 437 PRINT NODE (Model Definition) — Specify Nodes to be Included in Output, 440 NO PRINT (Model Definition) — Suppress Elements and Nodes in Output, 442 PRINT SPRING (Model Definition) — Controls the Print Out of Springs, 443 NO PRINT SPRING (Model Definition) — Deactivates the Printing of All Springs, 444 PRINT CONTACT (Model Definition) — Prints the Contact Body Summary, 445 NO PRINT CONTACT (Model Definition) — Suppresses the Contact Body Summary Printout, 446 GRID FORCE (Model Definition) — Nodal Force Output at Element or Node Level, 447 PRINT VMASS (Model Definition) — Print Element Volumes, Masses, Costs, and Strain Energies, 449 REAUTO — Interrupt/Modify Load Sequence from Previous Analysis, 450 RESTART — Set Flags for Restart, 452 RESTART LAST — Use Condensed Restart File, 455 UDUMP — Specify Nodes and Element for Postprocessing, 457 SUMMARY (Model Definition) — Create Summary Report, 458 NO SUMMARY (Model Definition) — Do Not Create Summary, 459 ELEMENT SORT (Model Definition) — Sort Element Results, 460 NO ELEM SORT (Model Definition) — Do Not Create Report Sorted by Element, 462 NODE SORT (Model Definition) — Sort Nodal Results, 463 NO NODE SORT (Model Definition) — Cancel Report Sorted by Nodes, 465 DESIGN OBJECTIVE — Define Objective Function to be Optimized, 466 DESIGN VARIABLES — Define Variable Design Parameters, 467

Main Index

9

DESIGN DISPLACEMENT CONSTRAINTS — Define Limits on Displacement Response, 469 DESIGN STRESS CONSTRAINTS — Define Limits on Stress Response, 471 DESIGN STRAIN CONSTRAINTS — Define Limits on Strain Response, 473 DESIGN FREQUENCY CONSTRAINTS — Define Limits on Eigenfrequency Response, 475 Mechanical Analysis, 477 CONTROL (Mechanical - Model Definition) — Control Option for Stress Analysis, 478 PARAMETERS (Model Definition) — Definition of Parameters used in Numerical Analysis, 484 FIXED DISP (with TABLE Input - Mechanical) — Define Fixed Displacement, 488 FIXED DISP (Mechanical) — Define Fixed Displacement, 492 DIST LOADS (with TABLE Input - Model Definition) — Define Distributed Loads, 494 DIST LOADS (Model Definition) — Define Distributed Loads, 499 FACE IDS — Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations, 504 POINT LOAD (with TABLE Input - Model Definition) — Define Nodal Point Loads, 509 POINT LOAD (Model Definition) — Define Nodal Point Loads, 513 HOLD NODES — Neglect Incremental Displacement, 516 INERTIA RELIEF (Model Definition) — Define Inertia Relief, 517 ROTATION A — Define Rotational Axis, 519 CORNERING AXIS — Define Cornering Axis in Steady State Rolling Analysis, 520 FLUID DRAG — Define Fluid Drag, 521 CAVITY — Define Constants and Reference Values for Structures with Internal Cavities, 523 PRE STATE — Transfer History Data from Previous Analysis to the Current Analysis as the Initial State, 524 AXITO3D (Model Definition) — Transfer Data from Axisymmetric Analysis to 3-D Analysis, 529 GLOBALLOCAL — Structural Zooming Analysis, 533 INIT STRESS (with TABLE Input) — Define Initial Stress, 537 INIT STRESS — Define Initial Stress, 539 INITIAL PLASTIC STRAIN (with TABLE Input) — Define Initial Strain, 543 INITIAL PLASTIC STRAIN — Define Initial Plastic Strain, 545 INITIAL STATE (with TABLE Input) — Initialize State Variables, 548 INITIAL STATE — Initialize State Variables, 551 CHANGE STATE (with TABLE Input - Model Definition) — Redefine State Variables, 554 CHANGE STATE (Model Definition) — Redefine State Variables, 558 THERMAL LOADS (Model Definition) — Input Temperature Data, 562 INITIAL TEMP (with TABLE Input - Thermal Stress) — Define Initial Temperatures, 564 INITIAL TEMP (Thermal Stress) — Define Initial Temperatures, 566 POINT TEMP (with TABLE Input - Model Definition) — Define Point Temperatures, 568 POINT TEMP (Model Definition) — Define Point Temperatures, 570 FORCDT — Input Displacement or Load Histories, 572 FOUNDATION (with TABLE Input - Model Definition) — Input Elastic Foundation Data, 573 FOUNDATION (Model Definition) — Input Elastic Foundation Data, 576 FOURIER — Describe Fourier Coefficients, 577 J-INTEGRAL — Define Path for J-Integral Estimation, 579 LORENZI — Define Path for Modified J-Integral, 580 VCCT — Virtual Crack Closure Technique, 583

Main Index

10 Marc Volume C: Program Input

DELAMINATION — , 587 ISLAND REMOVAL — Deactivate Islands of Connected Elements, 588 Contact, 589 Deformable and Rigid Surfaces, 589 Motion of Surfaces, 589 Cautions, 590 Control Variables and Option Flags, 590 Contact/Penetration, 591 Separation, 591 Optional Heat Transfer Data, 592 Optional Electrical Data (Joule Heating Analysis), 592 Time Step Control, 593 Dynamic Contact - Impact, 593 Two-dimensional Rigid Surfaces, 593 Three-dimensional Rigid Surfaces, 597 Selective Contact Surfaces, 608 User Subroutines, 608 Contact with Adaptive Meshing or Rezoning, 610 Spring-Back Analysis, 610 Contact Tolerance, 610 Corner Conditions, 611 Friction, 611 CONTACT with TABLES (2-D) — Define Two-dimensional Contact Surface, 615 CONTACT (2-D) — Define Two-dimensional Contact Surface, 627 CONTACT with TABLES (3-D) — Define Three-dimensional Contact Surface, 637 CONTACT (3-D) — Define Three-dimensional Contact Surface, 653 CONTACT TABLE with TABLES (Model Definition) — Define Contact Table, 667 CONTACT TABLE (Model Definition) — Define Contact Table, 676 SPLINE (Model Definition) — Analytical Surface used to Represent a Deformable Body, 683 UMOTION — Invoke User Subroutine to Prescribe Surface Motion, 687 UFRICTION — Invoke User Subroutine to Define Surface Friction Behavior, 688 UHTCOEF — Invoke User Subroutine to Define Surface/Environment Thermal Behavior, 689 UHTCON — Invoke User Subroutine to Define Surface to Surface Behavior, 690 CONTACT NODE (Model Definition) — Define Nodes for Surface Contact, 691 DEACT GLUE (Model Definition) — Define Deact Glue for Nodes in Glued Contact, 692 EXCLUDE (Model Definition) — Ignore Contact with Certain Regions, 693 Material Properties, 695 A. Elastic Behavior, 695 B. Elastic-Plastic Behavior, 698 C. Temperature Dependent Material Properties, 700 D. Relative Density Dependent Material Properties, 700 E. Low Tension Material, 700 F. Soil Materials, 700 G. Material Dependent Failure Criteria, 700 H. Characterization of Gap Elements, 701

Main Index

11

I. Laminated Composite, 701 J. Material Preferred Direction, 701 K. Material Property (Element) Coordinate Systems in Marc, 701 ISOTROPIC (with TABLE Input - Stress) — Define Mechanical Data for Isotropic Materials, 709 ISOTROPIC (Stress) — Define Mechanical Data for Isotropic Materials, 717 ORTHOTROPIC (with TABLE Input - Mechanical) — Define Mechanical Data for Orthotropic Materials, 723 ORTHOTROPIC (Mechanical) — Define Mechanical Data for Orthotropic Materials, 729 ANISOTROPIC (with TABLE Input - Mechanical) — Stress or Coupled-Thermal Stress Analysis, 733 ANISOTROPIC (Mechanical) — Stress or Coupled-Thermal Stress Analysis, 740 HYPOELASTIC (with TABLE Input) — Define Data for Hypoelastic Materials, 744 HYPOELASTIC — Define Data for Hypoelastic Materials, 746 MOONEY (with TABLE Input) — Define Data for Mooney-Rivlin Materials, 748 MOONEY — Define Data for Mooney-Rivlin Materials, 752 ARRUDBOYCE (with TABLE Input) — Define Data for Arruda-Boyce Model, 755 ARRUDBOYCE — Define Data for Arruda-Boyce Model, 759 GENT (with TABLE Input) — Define Data for the Gent Model, 762 GENT — Define Data for the Gent Model, 766 OGDEN (with TABLE Input) — Define Data for Ogden or Principal Stretch Based Material Model, 769 OGDEN — Define Data for Ogden or Principal Stretch Based Material Model, 773 NLELAST — Simplified Nonlinear Elastic Models Input, 776 FOAM (with TABLE Input) — Define Data for Foam Material Model, 781 FOAM — Define Data for Foam Material Model, 785 GASKET — Define Material Data for Gasket Materials, 788 TABLE — Define Table, 791 STRAIN RATE (Material Properties) — Define Strain Rate Dependent Yield Stress, 799 FORMING LIMIT — Forming Limit Properties, 801 WORK HARD — Define Workhardening Data, 803 TEMPERATURE EFFECTS (Stress) — Define Effects of Temperature, 806 TEMPERATURE EFFECTS (Coupled Thermal-Stress) — Temperature Effects in Coupled Thermal-Stress Analysis, 811 ORTHO TEMP (Structural) — Define Temperature Effects for Orthotropic Materials, 818 TIME-TEMP — Define Effects of Time/Temperature Transformation, 828 SHAPE MEMORY (with TABLE Input) — Define the Properties of Shape Memory Model, 832 SHAPE MEMORY — Define the Properties of Shape Memory Model, 838 CRACK DATA (with TABLE Input) — Define Material Properties for Concrete Cracking, 842 CRACK DATA — Define Material Properties for Concrete Cracking, 844 FAIL DATA (with TABLE Input) — Define Failure Criteria Data, 845 FAIL DATA — Define Failure Criteria Data, 859 MATERIAL DATA — Define Additional Material Data Constants, 870 GRAIN SIZE — Define Grain Size Growth Model, 871 DAMAGE — Define Properties for Damaging Materials, 873

Main Index

12 Marc Volume C: Program Input

GAP DATA — Define Data for Gap Elements, 880 COMPOSITE — Define Properties for Laminated Composite Materials, 882 MIXTURE — Define Constituents of Composite Material in Original and Potentially Damaged State, 885 COHESIVE (with TABLE Input) — Define Material Data for Interface Elements, 888 COHESIVE — Define Mechanical Data for Cohesive Materials, 891 PSHELL — Shell Element Property, 894 REBAR — Define Rebar Positions, Areas, and Orientations, 897 ORIENTATION — Define Orientation of Elements, 904 POWDER (with TABLE input) — Define Powder Material Model, 912 POWDER — Define Powder Material Model, 915 DENSITY EFFECTS — Define Effects of Density on Powder Materials, 918 RELATIVE DENSITY — Define Initial Relative Density for Stress or Coupled Thermal Stress Analysis, 921 SOIL (with TABLE Input) — Define Material Properties for Soil Analysis, 922 SOIL — Define Material Properties for Soil Analysis, 926 INITIAL POROSITY (with TABLE input) — Define Initial Porosity, 929 INITIAL POROSITY — Define Initial Porosity, 931 POROSITY CHANGE (with TABLE Input - Model Definition) — Define Changes in Porosity for Nonsoil Analysis, 932 INITIAL VOID RATIO (with TABLE Input) — Define Initial Void Ratio for Soil or Diffusion Analysis, 934 INITIAL VOID RATIO — Define Initial Void Ratio for Soil or Diffusion Analysis, 936 VOID CHANGE (with TABLE Input - Model Definition) — Define Changes in Void Ratio for Nonsoil Analysis, 937 INITIAL PC (with TABLE Input) — Define Initial Preconsolidation Pressure, 939 INITIAL PC — Define Initial Preconsolidation Pressure, 941 SPECIFIC WEIGHT — Define Specific Weight Constant for Soil Analysis, 942 INITIAL PORE (with TABLE Input) — Define Initial Pore Pressure for Soil Analysis, 943 INITIAL PORE — Define Initial Pore Pressure for Soil Analysis, 945 CHANGE PORE (with TABLE Input - Model Definition) — Define Pore Pressure for Uncoupled Soil Analysis, 948 CHANGE PORE (Model Definition) — Define Pore Pressures for Uncoupled Soil Analysis, 950 PRESS FILM (with TABLE Input) — Define Pressure Film Boundary Conditions, 953 PRESS FILM (Model Definition) — Define Pressure Film Coefficient Input, 956 Rate Effects, 957 CREEP (with TABLE Input) — Define Creep Constitutive Data, 959 CREEP — Define Creep Constitutive Data, 962 PHI-COEFFICIENTS — Define Phi-Coefficients for Rubber Viscoelastic Model, 967 VISCELPROP — Define Properties for Isotropic Viscoelastic Materials, 968 VISCELORTH — Define Properties for Viscoelastic Orthotropic Materials, 969 VISCELMOON — Define Properties for Large Strain Viscoelastic Materials, 971 VISCELOGDEN — Define Properties for Large Strain Viscoelastic Ogden Materials, 972 VISCELFOAM — Define Properties for Large Strain Viscoelastic Materials, 973

Main Index

13

SHIFT FUNCTION — Define Properties for Thermo-rheologically Simple Viscoelastic Materials, 974 VISCEL EXP — Viscoelastic Thermal Expansion, 976 Dynamic Analysis, 977 DAMPING — Define Damping Factors, 978 FLUID SOLID — Define Fluid-Solid Interface, 980 INITIAL DISP (with TABLE Input) — Define Initial Displacements, 981 INITIAL DISP — Define Initial Displacements, 984 INITIAL VEL (with TABLE Input) — Define Initial Velocity, 985 INITIAL VEL — Define Initial Velocity, 987 FIXED ACCE — Define Fixed Acceleration, 988 MASSES — Define Concentrated Masses, 989 CONM1 — Define a General Concentrated Mass, 990 CONM2 — Define a Diagonal Mass/Moment of Inertia, 996 RESPONSE SPECTRUM — Define Density for Spectral Response, 998 MODAL INCREMENT — Define Increments for Eigenvalue Extraction, 999 BUCKLE INCREMENT — Define Increments for Buckling Analysis, 1001 Heat Transfer Analysis, 1003 FIXED TEMPERATURE (with TABLE Input) — Define Fixed Temperature, 1004 FIXED TEMPERATURE — Define Fixed Temperature, 1007 FILMS (with TABLE Input - Model Definition) — Define Thermal Boundary Conditions, 1009 FILMS (Model Definition) — Define Convection Film Coefficient Input, 1013 SINK POINTS (with TABLE Input - Model Definition) — Define Sink Points, 1014 DIST FLUXES (with TABLE Input - Model Definition) — Define Distributed Fluxes, 1016 DIST FLUXES (Model Definition) — Define Distributed Fluxes, 1019 POINT FLUX (with TABLE Input - Model Definition) — Define Point Fluxes, 1020 POINT FLUX (Model Definition) — Define Point Fluxes, 1023 QVECT (with TABLE Input - Model Definition) — Define Thermal Vector Flux Boundary Conditions, 1024 WELD FLUX (with TABLE Input - Model Definition) — Define Motion and Flux Parameters for Weld Heat Source, 1028 WELD FLUX (Model Definition) — Define Motion and Flux Parameters for Weld Heat Source, 1032 WELD PATH (Model Definition) — Define Path and Arc Orientation for Weld Heat Source, 1036 WELD FILL (Model Definition) — Define Parameters for Weld Filler Elements, 1042 THERMAL CONTACT with TABLES (2-D) — Define Two-dimensional Thermal or Electrical Contact Conditions, 1045 THERMAL CONTACT (2-D) — Define Two-dimensional Thermal or Electrical Contact Conditions, 1053 THERMAL CONTACT with TABLES (3-D) — Define Three-dimensional Thermal or Electrical Contact Conditions, 1059 THERMAL CONTACT (3-D) — Define Three-dimensional Thermal or ElectricalContact Conditions, 1070 INITIAL TEMP (with TABLE Input - Heat Transfer) — Define Initial Temperatures, 1079

Main Index

14 Marc Volume C: Program Input

INITIAL TEMP (Heat Transfer) — Define Initial Temperatures, 1082 ISOTROPIC (with TABLE Input - Thermal) — Define Thermal Properties for Isotropic Materials, 1084 ISOTROPIC (Heat Transfer) — Define Thermal Properties for Isotropic Materials, 1086 ORTHOTROPIC (with TABLE Input - Thermal) — Define Thermal Properties for Orthotropic Materials, 1088 ORTHOTROPIC (Thermal) — Define Thermal Properties for Orthotropic Materials, 1091 ANISOTROPIC (with TABLE Input - Thermal) — Model Definition Option for Heat Transfer Analysis, 1093 ANISOTROPIC (Thermal) — Model Definition Option for Heat Transfer Analysis, 1096 LATENT HEAT — Define Latent Heat, 1098 TEMPERATURE EFFECTS (Heat Transfer) — Define Variation of Material Properties in Heat Transfer Analysis, 1099 ORTHO TEMP (Thermal) — Define Variation of Orthotropic Thermal Properties, 1102 CONTROL (Heat Transfer - Model Definition) — Define Control Parameters for Heat Transfer Analysis, 1107 CONVERT — Define Conversion Factors, 1109 CONRAD GAP — Define Convection/Radiation Gap, 1110 CHANNEL — Define Fluid Channel Input, 1111 VIEW FACTOR — Read in Radiation View Factors, 1112 RADIATING CAVITY — Define Outline of Radiating Cavity, 1113 RAD-CAVITY — Define Radiation Cavity, 1114 CAVITY DEFINITION — Define Geometry of a Cavity, 1116 EMISSIVITY — Define Emissivity, 1119 VELOCITY (with TABLE Input - Convective Heat Transfer) — Define Nodal Velocity Components, 1122 VELOCITY (Convective Heat Transfer) — Define Nodal Velocity Components, 1124 CURE RATE — Cure Kinetics, 1126 INIT CURE (with TABLE Input) — Define Initial Degree of Cure, 1130 INIT CURE — Define Initial Degree of Cure, 1132 CURE SHRINKAGE — Shrinkage Property of Resin Material, 1133 THERMO-PORE — Define Properties of Thermal Degrading Material, 1136 SURFACE ENERGY — Define Surface Energy, 1141 RECEDING SURFACE — Define Areas where Surface Recedes Due to Thermo-chemical Erosion or Wear Behavior, 1147 THROAT — Define Coordinates of Throat, 1150 INITIAL PYROLYSIS — Define Initial Pyrolysis, 1151 INITIAL DENSITY (Heat Transfer) — Define Initial Density, 1153 STREAM DEFINITION — Define Stream Definition, 1155 PRINT STREAMLINE — Control Output of Results along a Streamline, 1157 TRACK STREAMLINE — Track Behavior of a Point along a Streamline, 1158 Joule Heating Analysis, 1159 JOULE — Define Conversion Factor for Joule Heating Analysis, 1160 DIST CURRENT (with TABLE Input - Joule Heating) — Define Distributed Currents, 1161 DIST CURRENT (Joule Heating - Model Definition) — Define Distributed Current, 1164

Main Index

15

POINT CURRENT (with TABLE Input - Joule Heating) — Define Point Currents, 1165 POINT CURRENT (Joule - Model Definition) — Define Nodal Point Current, 1167 FIXED VOLTAGE (with TABLE Input - Joule Heating) — Define Fixed Voltage, 1168 FIXED VOLTAGE — Define Nodal Fixed Voltage, 1171 Diffusion Analysis, 1172 INITIAL PRESSURE (with TABLE Input - Diffusion) — Define Initial Pressure, 1173 FIXED PRESSURE (with TABLE Input - Diffusion) — Define Fixed Pressure, 1175 DIST MASS (with TABLE Input - Diffusion) — Define Distributed Mass Flux, 1177 POINT MASS (with TABLE Input - Diffusion) — Define Nodal Mass Flux, 1180 ISOTROPIC (with TABLE Input - Diffusion) — Define Diffusion Properties for Isotropic Materials, 1182 ORTHOTROPIC (with TABLE Input - Diffusion) — Define Diffusion Properties for Orthotropic Materials, 1184 ANISOTROPIC (with TABLE Input - Diffusion) — Model Definition Option for Diffusion Analysis, 1186 Hydrodynamic Bearing Analysis, 1189 VELOCITY (with TABLE Input - Hydrodynamic) — Define Nodal Velocity Components, 1190 VELOCITY (Hydrodynamic) — Define Nodal Velocity Components, 1192 THICKNESS (with TABLE Input - Model Definition) — Define Lubrication Thickness, 1194 THICKNESS — Define Lubrication Thickness, 1196 RESTRICTOR (with TABLE Input - Model Definition) — Coefficient Input for Bearing Analysis, 1197 RESTRICTOR — Coefficient Input for Bearing Analysis, 1199 CONTROL (Hydrodynamic) — Define Maximum Number of Increments for Bearing Analysis, 1200 ISOTROPIC (with TABLE Input - Hydrodynamic) — Define Lubricant Material Properties, 1201 ISOTROPIC (Hydrodynamic) — Define Lubricant Material Properties, 1203 TEMPERATURE EFFECTS (Hydrodynamic) — Define Effect of Temperature in Bearing Analysis, 1204 Acoustic Analysis, 1207 FIXED PRESSURE (with TABLE Input - Acoustic) — Define Fixed Pressure, 1208 FIXED PRESSURE (Acoustic) — Define Nodal Fixed Pressure, 1211 DIST SOURCES (with TABLE Input - Acoustic) — Define Distributed Sources, 1213 DIST SOURCES (Acoustic - Model Definition) — Define Distributed Sources, 1216 POINT SOURCE (with TABLE Input - Acoustic) — Define Point Source, 1217 POINT SOURCE (Acoustic - Model Definition) — Define Point Sources, 1220 ISOTROPIC (with TABLE Input - Acoustic) — Define Properties for Acoustic Cavity, 1221 ISOTROPIC (Acoustic) — Define Properties for Acoustic Cavity, 1222 ACOUSTIC (with TABLE Input - Acoustic) — Define Material Properties for Acoustic Analysis, 1223 ACOUSTIC — Define Material Properties for Acoustic Analysis, 1224 Electrostatic Analysis, 1225 FIXED EL-POT (with TABLE Input - Electrostatic) — Define Fixed Potential, 1226

Main Index

16 Marc Volume C: Program Input

FIXED EL-POT (Electrostatic) — Define Fixed Nodal Potential, 1229 FIXED POTENTIAL (with TABLE Input - Electrostatic) — Define Fixed Potential, 1231 FIXED POTENTIAL (Electrostatic) — Define Fixed Nodal Potential, 1234 DIST CHARGES (with TABLE Input - Electrosatatic) — Define Distributed Charges, 1236 DIST CHARGES (Electrostatic) — Define Distributed Charges, 1239 POINT CHARGE (with TABLE Input - Electrostatic) — Define Point Charges, 1240 POINT CHARGE — Define Nodal Point Charges, 1242 ISOTROPIC (with TABLE Input - Electrostatic) — Define Electrical Properties for Isotropic Materials, 1243 ISOTROPIC (Electrostatic) — Define Electrical Properties for Isotropic Materials, 1244 ORTHOTROPIC (with TABLE Input - Electrostatic) — Define Electrical Properties for Orthotropic Materials, 1245 ORTHOTROPIC (Electrical) — Define Electrical Properties for Orthotropic Materials, 1247 Piezoelectric Analysis, 1249 FIXED POTENTIAL (with TABLE Input - Piezoelectric) — Define Fixed Potential, 1250 FIXED POTENTIAL (Piezoelectric - Model Definition) — Define Fixed Nodal Potential, 1253 DIST CHARGES (with TABLE Input - Piezoelectric) — Define Distributed Charges, 1254 DIST CHARGES (Piezoelectric - Model Definition) — Define Distributed Charges, 1257 POINT CHARGE (with TABLE Input - Piezoelectric) — Define Point Charges, 1258 POINT CHARGE (Piezoelectric - Model Definition) — Define Nodal Point Charges, 1260 PIEZOELECTRIC (with TABLE Input - Piezoelectric) — Define Electrical Data for Piezoelectric Analysis, 1261 PIEZOELECTRIC (Piezoelectric - Model Definition) — Define Electrical Data for Piezoelectric Analysis, 1264 Magnetostatic Analysis, 1267 FIXED MG-POT (with TABLE Input - Magnetostatic) — Define Fixed Potential, 1268 FIXED MG-POT (Magnetostatic) — Define Nodal Fixed Potential, 1271 FIXED POTENTIAL (with TABLE Input - Magnetostatic) — Define Fixed Potential, 1273 FIXED POTENTIAL (Magnetostatic) — Define Nodal Fixed Potential, 1276 DIST CURRENT (with TABLE Input - Magnetostatic) — Define Distributed Currents, 1278 DIST CURRENT (Magnetostatic) — Define Distributed Current, 1281 POINT CURRENT (with TABLE Input - Magnetostatic) — Define Nodal Point Current, 1282 POINT CURRENT (Magnetostatic) — Define Nodal Point Current, 1284 ISOTROPIC (with TABLE Input - Magnetostatic) — Define Magnetic Properties for Isotropic Materials, 1285 ISOTROPIC (Magnetostatic) — Define Magnetic Properties for Isotropic Materials, 1287 ORTHOTROPIC (with TABLE Input - Magnetostatic) — Define Magnetic Properties for Orthotropic Materials, 1288 ORTHOTROPIC (Magnetostatic) — Define Magnetic Properties for Orthotropic Materials, 1292 B-H RELATION (Magnetostatic) — Define Magnetization Curve for Nonlinear Magnetic Material, 1294 PERMANENT (with TABLE Input - Magnetostatic) — Define Permanent Magnet, 1296 PERMANENT (Magnetostatic) — Define Permanent Magnet, 1298 CONTROL (Magnetostatic) — Control for Magnetostatic Analysis, 1300

Main Index

17

Electromagnetic Analysis, 1301 FIXED POTENTIAL (with TABLE Input - Electromagnetic) — Define Fixed Potential, 1302 FIXED POTENTIAL (Electromagnetic) — Define Nodal Fixed Potential, 1305 DIST CURRENT (with TABLE Input - Electromagnetic) — Define Distributed Currents, 1307 DIST CURRENT (Electromagnetic - Model Definition) — Define Distributed Currents, 1310 DIST CHARGES (with TABLE Input - Electromagnetic) — Define Distributed Charges, 1311 DIST CHARGE (Electromagnetic - Model Definition) — Define Distributed Charges, 1314 POINT CURRENT-CHARGE (with TABLE Input - Electromagnetic) — Define Point Fluxes, 1315 POINT CURRENT-CHARGE — Define Nodal Point Currents and Point Charges, 1317 ISOTROPIC (with TABLE Input - Electromagnetic) — Define Electromagnetic Properties for Isotropic Materials, 1318 ISOTROPIC (Electromagnetic) — Define Electromagnetic Properties for Isotropic Materials, 1320 ORTHOTROPIC (with TABLE Input - Electromagnetic) — Define Electromagnetic Properties for Orthotropic Materials, 1322 ORTHOTROPIC (Electromagnetic) — Define Electromagnetic Properties for Orthotropic Materials, 1325 B-H RELATION (Electromagnetic) — Define Magnetization Curve for Nonlinear Magnetic Material, 1327 PERMANENT (Electromagnetic) — Define Permanent Magnet, 1329 CONTROL (Electromagnetostatic) — Control for Electromagnetostatic Analysis, 1331 Fluid Analysis, 1333 REGION (Fluid) — Define Elements in a Region, 1335 COUPLING REGION — Define Coupling Regions, 1336 FIXED DISP (Fluid) — Define Fixed Displacement, 1340 FIXED VELOCITY (with TABLE Input - Fluid) — Define Fixed Velocity, 1342 FIXED VELOCITY — Define Fixed Velocity, 1345 ISOTROPIC (with TABLE Input - Fluid) — Define Material Properties for Fluid Analysis, 1347 ISOTROPIC (Fluid) — Define Material Properties for Fluid Analysis, 1349 STRAIN RATE (Fluid) — Define Strain Rate Dependent Viscosity, 1351 TEMPERATURE EFFECTS (Coupled Fluid-Thermal) — Temperature Effects in Coupled Fluid-Thermal Analysis, 1354 CONTROL (Fluid) — Control Option for Fluid Analysis or Fluid-Thermal Analysis, 1357 CONTROL (Fluid-Solid) — Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis, 1360 END OPTION — Model Definition Data End, 1365

4

History Definition Options List

4

History Definition Options Elastic Analysis, 1374 Mechanical, Acoustic, Piezoelectric or Electrostatic-Structural or Electromagnetic Analyses, 1374

Main Index

18 Marc Volume C: Program Input

Heat Transfer Analysis, 1374 Hydrodynamic Bearing Analysis, 1374 Electrostatic Analysis, 1375 Magnetostatic Analysis, 1375 Table Driven Boundary Conditions, 1375 Restart Considerations, 1375 General Controls, 1376 COMMENT — Enter Comments, 1377 TITLE — Output Title Definition, 1378 NEW (History Definition) — Use New Format, 1379 INCLUDE (History Definition) — Insert File into the Input File, 1380 PRINT CHOICE (History Definition) — Define Data to be Printed, 1381 PRINT ELEMENT (History Definition) — Specify Elements to be Included in Output, 1383 PRINT NODE (History Definition) — Define Nodes and Nodal Quantities to be Printed, 1385 NO PRINT (History Definition) — Suppress Printing, 1387 PRINT CONTACT (History Definition) — Prints the Contact Body Summary, 1388 NO PRINT CONTACT (History Definition) — Suppresses the Contact Body Summary Printout, 1389 PRINT SPRING (History Definition) — Controls the Print Out of Springs, 1390 NO PRINT SPRING (History Definition) — Deactivates the Printing of All Springs, 1391 GRID FORCE (History Definition) — Nodal Force Output at Element or Node Level, 1392 SUMMARY (History Definition) — Create Summary Report, 1394 NO SUMMARY (History Definition) — Suppress Summary, 1395 ELEMENT SORT (History Definition) — Sort Elements for Report, 1396 NO ELEM SORT (History Definition) — Do Not Create Report Sorted by Element, 1398 NODE SORT (History Definition) — Sort Nodal Results, 1399 NO NODE SORT (History Definition) — Cancel Report Sorted by Nodes, 1401 PRINT VMASS (History Definition) — Print Element Volumes, Masses, Costs, and Strain Energies, 1402 CONTROL (Mechanical - History Definition) — Control Option for Stress Analysis, 1403 PARAMETERS (History Definition) — Definition of Parameters used in Numerical Analysis, 1409 SOLVER (History Definition) — Specify Direct or Iterative Solver, 1413 POST (History Definition) — Create File for Postprocessing, 1416 POST INCREMENT — Define Increments between Writing on Post File, 1431 RESTART INCREMENT — Define Increments between Writing on Restart File, 1433 ADAPT GLOBAL (History Definition) — Define Meshing Parameters Used in Global Remeshing, 1434 LOADCASE (History Definition) — Define Loadcase, 1444 DMIG-OUT (History Definition) — Output Control of Matrices, 1447 K2GG, K2PP (History Definition) — Selects Direct Input Stiffness Matrix, 1452 M2GG, M2PP (History Definition) — Selects Direction Input Mass Matrix, 1454 B2GG, B2PP (History Definition) — Selects Direction Input Damping Matrix, 1455

Main Index

19

P2G (History Definition) — Selects Direction Input Load Vector, 1456 READ FILE — Read Data Transfer File Used in Contact Decoupled Analysis, 1457 WRITE FILE — Write Data Transfer File Used in Contact Decoupled Analysis, 1458 Static, Dynamic, Creep Analysis, 1459 DISP CHANGE — Define Displacement Boundary Conditions, 1460 RELEASE NODE — Define Nodes for which the Boundary Condition is Gradually Released, 1463 GAP CHANGE — Redefine Data for Gap Elements, 1464 TYING CHANGE — Define Tying Constraints, 1466 DIST LOADS (History Definition) — Define Distributed Loads, 1467 POINT LOAD (History Definition) — Define Point Loads, 1472 AUTO LOAD — Define Equal Load Increments, 1474 INERTIA RELIEF (History Definition) — Define Inertia Relief, 1476 BEGIN SEQUENCE — Initiate a Series of Repeated Load Cases, 1478 END SEQUENCE — Terminates a Series of Repeated Load Cases, 1479 PROPORTIONAL INCREMENT — Define Proportional Increments, 1480 AUTO INCREMENT — Define Automatic Load Stepping, 1481 AUTO STEP — Adaptive Load Step Control, 1486 TERMINATE — Terminate Loadcase, 1493 SUPERPLASTIC — Superplastic Forming Analysis, 1495 THERMAL LOADS (History Definition) — Define Thermal Loads, 1497 AUTO THERM — Specify Data for Automatic Thermal Loading, 1499 CHANGE STATE (History Definition) — Change State Variables, 1501 POINT TEMP (History Definition) — Define Point Temperatures, 1506 CHANGE PORE (History Definition) — Define Pore Pressures for Uncoupled Soil Analysis, 1508 TIME STEP — Define Time Step, 1511 RESET TIME — Resets Time to Zero, 1512 BUCKLE — Specify Buckling Analysis, 1513 SUPERELEM (History Definition) — Perform Craig-Bampton Analysis for MD Adams MNF Interface, 1515 SUPERELEM (DMIG Applications - History Definition) — Create DMIG of Substructure, 1517 ASSEM LOAD — Assemble Equivalent Nodal Force Vector, 1520 ACTIVATE — Activate Elements, 1521 DEACTIVATE (History Definition) — Deactivate Elements, 1522 FOUNDATION (History Definition) — Define Foundation Spring Force for Elements, 1525 CHANGE RIGID — Define New Geometry For a Rigid Contact Surface, 1526 ADD RIGID with TABLES (2-D) — Define a New Two-dimensional Rigid Contact Surface, 1534 ADD RIGID (2-D) — Define a New Two-dimensional Rigid Contact Surface, 1540 ADD RIGID with TABLES (3-D) — Define a New Three-dimensional Rigid Contact Surface, 1545 ADD RIGID (3-D) — Define a New Three-dimensional Rigid Contact Surface, 1554 CONTACT TABLE with TABLES (History Definition) — Define Contact Table, 1563 CONTACT TABLE (History Definition) — Define Contact Table, 1572

Main Index

20 Marc Volume C: Program Input

CONTACT NODE (History Definition) — Define Nodes for Surface Contact, 1579 MOTION CHANGE — Define Motion of Rigid Surfaces, 1580 SS-ROLLING — Define the Parameters for Steady State Transport, 1582 RELEASE — Define Release Data, 1585 APPROACH — Move Rigid Surfaces into Position, 1586 MOVE (History Definition) — Perform Rigid Body Motion on Model, 1587 ANNEAL — Modify State of Material, 1589 SYNCHRONIZED — Move Rigid Surfaces into Position, 1590 SPLINE (History Definition) — Analytical Surface used to Represent a Deformable Body, 1591 EXCLUDE (History Definition) — Ignore Contact with Certain Regions, 1593 ACTUATOR — Define the Length of the Actuator Link, 1594 Rate Dependent Analysis, 1595 CREEP INCREMENT — Define Creep Increment, 1596 AUTO CREEP — Control Transient Creep, 1597 ACCUMULATE — Specify Accumulation Option, 1599 EXTRAPOLATE — Specify Extrapolation Option, 1600 AUTO THERM CREEP — Automatic, Thermally-Loaded Elastic-Creep Analysis, 1601 Dynamic Analysis, 1605 MODAL SHAPE — Define Modal Shape, 1606 RECOVER — Recover Option, 1608 DYNAMIC CHANGE (Dynamic) — Define Integration in Time, 1610 SPECTRUM — Initiate Spectral Response Analysis, 1611 HARMONIC (Dynamic) — Define Excitation Frequency, 1612 ACC CHANGE — Define Acceleration Boundary Conditions, 1613 — , 1614 Heat Transfer Analysis, 1615 TRANSIENT — Specify Transient or Steady-State Heat Transfer Analysis, 1616 STEADY STATE (Heat Transfer) — Specify Steady-State Heat Transfer Analysis, 1618 DIST FLUXES (History Definition) — Define Distributed Fluxes, 1619 — , 1620 POINT FLUX (History Definition) — Define Point Fluxes, 1621 WELD FLUX (History Definition) — Define Motion and Flux Parameters for Weld Heat Source, 1622 WELD PATH (History Definition) — Define Path and Arc Orientation for Weld Heat Source, 1626 WELD FILL (History Definition) — Define Parameters for Weld Filler Elements, 1632 CONTROL (Heat Transfer - History Definition) — Define Controls for Heat Transfer Analysis, 1635 TEMP CHANGE — Specify or Change Fixed Temperatures, 1637 FILMS (History Definition) — Define Film Coefficients and Sink Temperatures, 1639 VELOCITY CHANGE — Modify Nodal Velocity Components, 1640 Joule Heating Analysis, 1643 EMRESIS —. Select Conducting Bodies to be used in a Resistance Calculation, 1644 DIST CURRENT (Joule Heating - History Definition) — Define Distributed Current, 1645

Main Index

21

POINT CURRENT (Joule - History Definition) — Define Nodal Point Current, 1646 VOLTAGE CHANGE — Define or Change Voltage for Joule Heating Analysis, 1647 Diffusion Analysis, 1649 POROSITY CHANGE — Define Changes in Porosity for Nonsoil Analysis, 1650 VOID CHANGE — Define Changes in Void Ratio for Nonsoil Analysis, 1652 DIST MASS (Diffusion) — Define Distributed Mass Flux, 1654 POINT MASS (Diffusion) — Define Nodal Mass Flux, 1657 Hydrodynamic Bearing Analysis, 1659 THICKNS CHANGE — Define Thickness Variations, 1660 DAMPING COMPONENTS — Define Damping Coefficients, 1661 STIFFNS COMPONENTS — Define Stiffness Coefficients, 1662 Acoustic Analysis, 1663 PRESS CHANGE — Define Fixed Pressures, 1664 DIST SOURCES (History Definition) — Define Incremental Distributed Sources, 1666 POINT SOURCE (Acoustic - History Definition) — Define Incremental Nodal Point Sources, 1667 HARMONIC (Acoustic - History Definition) — Define Excitation Frequency, 1668 Electrostatic Analysis, 1669 STEADY STATE (Electrostatic) — Specify Steady-State Electrostatic Analysis, 1670 EMCAPAC — Select Conducting Bodies to be used in a Capacitance Calculation, 1671 Piezoelectric Analysis, 1672 POTENTIAL CHANGE (Piezoelectric - History Definition) — Define Potential Boundary Conditions, 1673 POINT CHARGE (Piezoelectric - History Definition) — Define Nodal Point Charges, 1675 DIST CHARGE (Piezoelectric - History Definition) — Define Distributed Charges, 1676 Magnetostatic Analysis, 1678 STEADY STATE (Magnetostatic) — Specify Steady-State Magnetostatic Analysis, 1679 DIST CURRENT (Magnetostatic) — Define Distributed Current, 1680 Electromagnetic Analysis, 1682 HARMONIC (Electromagnetic - History Definition) — Define Excitation Frequency, 1683 DYNAMIC CHANGE (Electromagnetic - History Definition) — Define Dynamic Change, 1684 POTENTIAL CHANGE — Define or Redefine Potential Boundary Conditions, 1685 POINT CURRENT (Electromagnetic - History Definition) — Define Point Current and/or Charge, 1687 DIST CURRENT (Electromagnetic - History Definition) — Define Distributed Current, 1688 DIST CHARGE (Electromagnetic - History Definition) — Define Distributed Charges, 1690 CONTINUE (History Definition) — End Loadcase, 1692

Main Index

22 Marc Volume C: Program Input

5

Rezoning Options List

5

Rezoning Options Rezoning Options, 1697 REZONE — Specify Rezoning Input, 1698 SPLIT BODIES — Defines Rezoned Data of Contact Nodes, 1699 SECTIONING (Rezoning) — Define Sections for Rezoning, 1700 CONNECTIVITY CHANGE — Define or Change Connectivity, 1702 GEOMETRY CHANGE — Specify New Geometry, 1703 ORIENTATION CHANGE — Redefine Orientation, 1707 GAP DATA CHANGE — Redefine Gap Data, 1709 COORDINATE CHANGE — Redefine Node Coordinates, 1711 UFRORD — Use Subroutine UFRORD, 1712 MOVE (Rezoning) — Redefine Node Coordinates, 1713 CONTACT CHANGE — Change Surface Contact after Rezoning, 1714 PRINT CHOICE (Rezoning) — Select Print Settings, 1720 URCONN — Invoke User Subroutine URCONN, 1722 CONTINUE (Rezoning) — End Rezoning Input, 1723 END REZONE — End Input for Rezoning Increment, 1724

A

Program Messages Marc Exits, 1726 Exit Numbers 1-1000, 1726 Exit Numbers 1001-2000, 1732 Exit Numbers 2001-3000, 1734 Exit Numbers 3001-4000, 1737 Exit Numbers 4001-5000, 1740 Exit Numbers 5001-6000, 1741 Exit Numbers 6001-7000, 1743 Exit Numbers 9001-10000, 1744

B

Workspace Definition and the Sizing Option Estimating Workspace Sizes for Marc Jobs, 1746 I/O With Marc, 1747 Estimating File Sizes, 1748 Running Marc, 1750

C

Default File Parameters, 1760 Model Definition Options, 1760

Main Index

23

D

Control File

E

Environment Variables

F

Material Database

G

Flow Line File Format

H

3-D Remeshing Files

I

Units Tables of Units, 1776

J

Parameters List

K

Options List

Main Index

24 Marc Volume C: Program Input

Main Index

Marc Volume C: Program Input Preface

Preface

Main Index

J

About this Manual

J

Who Should Read this Manual

J

Other Marc Manuals

J

Chapter Contents

26

26 26

26

26 Marc Volume C: Program Input About this Manual

About this Manual This document describes the file format of the Marc input file. Its chapters and sections roughly parallel the organization of that file. Appendices describe Marc program messages and provide an alphabetical list of parameters and options for easy reference. Plus, at the beginning of each chapter is a list of the parameters or options discussed in that particular chapter.

Who Should Read this Manual This document is intended for current and new users of Marc. It does not purport to teach the use of Marc, but is a reference to its specific functioning. Other Marc documents are listed below.

Other Marc Manuals The Marc Reference Library includes: Marc Volume A: Theory and User Information Marc Volume B: Element Library Marc Volume C: Program Input Marc Volume D: User Subroutines and Special Routines Marc Volume E: Demonstrations Problems

Marc User’s Guide Marc Python Tutorial and Reference Manual Marc Mentat Help Reference

Chapter Contents

Main Index

Chapter 1

Introduction

introduces basic concepts of Marc program input.

Chapter 2

Parameters

describes the options that are used in the parameter section of the Marc input files.

Chapter 3

Model Definition Options

describes the options that are used in the model definition section of the Marc input files.

Chapter 4

History Definition Options

describes the options that are used for displaying the results of the analysis.

Chapter 5

Rezoning Options

describes the options that are used in Marc input files to specify load history information.

Preface 27 Chapter Contents

Appendix A Program Messages

describes the messages one might see upon termination of Marc.

Appendix B Workspace Definition and the Sizing Option

details the running of Marc on supported computers.

Appendix C Default File

lists the most commonly used parameters and options put into a default file.

Appendix D Control File

describes how to create and use a control file.

Appendix E Environment Variables

introduces user-controlled environment variables.

Appendix F Material Database

describes how to enter new material into the database.

Appendix G Flow Line File Format

provides the flow line format.

Appendix H 3-D Remeshing Files

provides how to view files within the GUI for remeshing observation.

Appendix I

Units

provides tables for the International System (SI) of units and conversation tables for Imperial units from US units.

Appendix J

Parameters List

provides a complete alphabetical list of all parameters and their associated page numbers.

Appendix K Options List

Main Index

provides a complete alphabetical list of all program options and their associated page numbers.

28 Marc Volume C: Program Input Chapter Contents

Main Index

Chapter 1 Introduction Marc Volume C: Program Input

1

Main Index

Introduction

J

Formats in Marc

J

Input of List Items

J

Guide to Organization of Marc Input Data

40

J

Discussion of Marc Output for New Users

51

30 31

30 Marc Volume C: Program Input Formats in Marc

This chapter contains a brief outline of the various data input options and problem solution setups which are available to a Marc user. It highlights only a small segment of the total problem solution capability available. You only have to select the options required for the solution of your problem. In addition, you can further elect to use the many default and built-in conditions which have been provided in these options. This user-selection feature forms the basis for Marc and input data organization. Marc then provides a solution capability based on your selection of options. Further details on Marc’s organization can be found in Marc Volume A: Theory and User Information. Formats used by Marc are discussed in this chapter. A short description of the organization of the input data is given, followed by an illustrative example particularly useful for new users. Selected portions of the output generated by Marc are shown and discussed. The last section of this chapter summarizes the input requirements for different classes of analyses.

Formats in Marc Marc is written in FORTRAN, but does its own data conversion to avoid system aborts due to user data errors. All input data files are read as alphanumeric and are converted to integer, floating point, or keywords, as necessary. Marc issues error messages and displays the illegal image if it cannot interpret the data field according to the specifications given in the manual. When such errors occur, Marc attempts to scan the remainder of the data files and ends the run with an exit error message at the END OPTION (or end file). Two conventions are allowed for input format control—fixed and free format. Fixed and free format can be mixed within a data file, but on a single data line, only one type of format can be entered. The syntax rules for each format type are as follows:

Fixed Field 1. Integers must be right-justified (right blank fill) in their fields. 2. Floating point numbers can be given with or without exponent. In either case, the mantissa must contain a decimal point. If an exponent is given, it must be preceded by the character E or D and must be right justified. The size of the number must lie in the range 10-72 to 1072. Note that, in the this manual, integer fields are indicated as “I” and floating point numbers are indicated as “E” or “F” and the allowable column field is specified.

Free Field Data can be input in free field under the following syntax rules: 1. Each data block must contain the same number of data items that it would contain under standard fixed format control as documented in this manual. Thus, for example, the 3rd data block of the CONNECTIVITY option is given as (16I5); therefore, no more than 16 numbers can appear on a data line in this data block under fixed or free field format. This syntax rule allows mixing of fixed-field and free-field data in the data file, since the number of data blocks needed to input any data list is the same in both cases.

Main Index

Chapter 1 Introduction 31 Input of List Items

2. Data items on a data line must be separated by a comma. This separator can be surrounded by an arbitrary number of blanks. Within the data item itself, no embedded blanks can appear. 3. Floating point numbers can be given with or without exponent. In either case, the mantissa must contain a decimal point. If an exponent is given, it must be preceded by the character E or D and must immediately follow the mantissa (no embedded blanks). The size of the number must lie in the range 10-35 to 1035. 4. Keywords must be typed exactly as written in the manual. Embedded blanks do not count as separators here (for example, BEAM SECT is one word only). 5. Note that you must distinguish between a real and integer zero when entering data; the floating point zero must contain a decimal point, as in Rule 3, above. 6. If a data line contains only one free-field data item, that item must be followed by a comma. Thus, “1” must be entered as “1,” if it is the only data item on a data line.

Input of List Items Marc requests that you input a list of items in association with certain program functions. These items, as an example, can be a set of elements as in conjunction with the ISOTROPIC option, or a set of nodes as in conjunction with the POINT LOAD option. There are 12 types of items that can be requested: Element numbers

Points

Node numbers

Curves

Degree of freedom numbers

Surfaces

Integration point numbers

Bodies

Layer numbers

Edges

Increment numbers

Faces

A set of items can be expressed as a combination of one or more subsets. These subsets can be specified in three different forms, depending on your convenience. The operations that can be performed between subsets are: AND INTERSECT EXCEPT

In forming a set, subsets are combined in binary operations going from left to right. Hence, a set can be formed as: 1. SUBLIST1 AND SUBLIST2

which implies all items in SUBLIST1 AND SUBLIST2. Duplicate items are eliminated and the resultant set is sorted. 2. SUBLIST1 INTERSECT SUBLIST2

which implies only those items occurring both in SUBLIST1 and SUBLIST2.

Main Index

32 Marc Volume C: Program Input Input of List Items

3. SUBLIST1 EXCEPT SUBLIST2

which implies all items in SUBLIST1 except those which occur in SUBLIST2. 4. SUBLIST1 AND SUBLIST2 EXCEPT SUBLIST3 INTERSECT SUBLIST4

which implies take the items in SUBLIST1 and SUBLIST2 and remove those items that occur in SUBLIST3. Then, if these items also occur in SUBLIST4, include them in the set. The SUBLISTS can have the form: 1. A range of items can be specified as: l TO m BY n

or 1 THROUGH M BY n

which implies items l through m by n; if BY n is not included, it is assumed to be BY 1. Note that the range can be either increasing or decreasing. 2. A string of items can be specified as: a1 a2 a3 ... an

which implies that n items are to be included. If continuation data is necessary, a “C” or CONTINUE should be the last item on the data line. 3. A setname can be specified as: MYSET

which implies that all items previously specified to be in the set MYSET are to be used. The items in a set are specified using the DEFINE option. In a list, edges and faces are entered as pairs (i:j) where i is the user element id and j is the edge id or face id. The edge id/face id for the different element classes is given beginning on page 33. There are two types of edge and face sets; those expressed in Marc convention or the Marc Mentat convention. The edge/face id in Marc convention is one greater than the Marc Mentat convention. For example, to specify edge 1 on elements 1 to 20, one would use: 1:1 TO 20:1

Sorted vs. Unsorted Lists In Marc, most lists are sorted lists. That is, regardless of the order of the list items on the list line, Marc returns these items sorted from lowest to highest. Unsorted lists are required in several places, however. These places are: 1. List of nodes in the TYING option. 2. List of nodes in the SUPERINPUT and SUBSTRUCTURE option. 3. List of degrees of freedom in the FIXED DISP option. When defining unsorted lists, the sublist connectors EXCEPT and INTERSECT cannot be used. Setnames can be used as long as the sets themselves are unsorted. In Marc, degree of freedom sets are always

Main Index

Chapter 1 Introduction 33 Edges and Faces

unsorted. Unsorted node sets can be defined by using set type NDSQ (for “node sequence”) rather than set type NODE (see the DEFINE model definition option).

Examples Define subsets FLOOR, NWALL, WWALL DEFINE NODE SET FLOOR 1 TO 5 (i.e. NODES 1,2,3,4,5) DEFINE NODE SET NWALL 5 TO 15 BY 5 AND 20 to 22 (i.e. NODES 5,10,15,20,21,22) DEFINE NODE SET WWALL 11 TO 20 (i.e. NODES 11,12,13,14,15,16,17,18,19,20)

Possible lists can be: 1. NWALL AND WWALL, which would contain nodes 5 16

10 17

11 18

12 19

13 20

14 21

15 22

2. NWALL INTERSECT WWALL, which would contain node 15

20

3. NWALL AND WWALL EXCEPT FLOOR, which would contain nodes: 10 16

11 17

12 18

13 19

14 20

15 21

22

Edges and Faces Marc 2003 introduces the concept of edge ids and face ids that are used with the ATTACH EDGE, ATTACH FACE, and edge and face sets. The edge and face ids follow two different conventions - either Marc or Marc Mentat. The difference is that the Marc Mentat number is equal to the Marc number minus one. The edge and face ids are dependent upon the element geometry and are shown below. 1-D 2-Node Elements y 2 1

x

Main Index

EDGE ID 1

NODES 1–2

34 Marc Volume C: Program Input Edges and Faces

1-D 3-Node Elements 3

EDGE ID 1

NODES 1–2–3

2 1 2-D 4-Node Quadrilateral Elements 4

3 EDGE ID 1 2 3 4

1

NODES 1–2 2–3 3–4 4–1

2

Load shown on EDGE ID 1 2-D 8-Node Quadrilateral Elements 4

7

8

1

Main Index

3

6

5

2

EDGE ID 1 2 3 4

NODES 1–5–2 2–6–3 3–7–4 4–8–1

Chapter 1 Introduction 35 Edges and Faces

2-D 3-Node Triangle 3

1

EDGE ID 1 2 3

NODES 1–2 2–3 3–1

EDGE ID 1 2 3

NODES 1–4–2 2–5–3 3–6–1

2

2-D 6-Node Triangle 3

6

5

1

4

2

3-D 4-Node Tetrahedral 4 3

1 2

Main Index

EDGE ID 1 2 3 4 5 6

NODES 1–2 2–3 3–1 1–4 2–4 3–4

36 Marc Volume C: Program Input Edges and Faces

3-D 6-Node Pentahedral 6 4

5

3 1 2

EDGE ID 1 2 3 4 5 6 7 8 9

NODES 1–2 2–3 3–1 4–5 5–6 6–4 1–4 2–5 3–6

EDGE ID 1 2 3 4 5 6 7 8 9 10 11 12

NODES 1–2 2–3 3–4 4–1 5–6 6–7 7–8 8–5 1–5 2–6 3–7 4–8

3-D 8-Node Brick 8 7

5 6 4 1

3 2

3-D 10-Node Tetrahedral 4 8

10 3

9 7 6

1 5 2

Main Index

EDGE ID 1 2 3 4 5 6

NODES 1–2– 5 2–3– 6 3–1– 7 1–4– 8 2–4– 9 3 – 4 – 10

Chapter 1 Introduction 37 Edges and Faces

3-D 20-Node Brick 8 16

15

EDGE ID 1 2 3 4 5 6 7 8 9 10 11 12

7

5

20

13

14

6 17

19

4 12

11 18

1

3 9

10 2

NODES 1–2– 9 2 – 3 – 10 3 – 4 – 11 4 – 1 – 12 5 – 6 – 13 6 – 7 – 14 7 – 8 – 15 8 – 5 – 16 1 – 5 – 17 2 – 6 – 18 3 – 7 – 19 4 – 8 – 20

3-D 3-Node Shell z

3

FACE ID 1

NODES 1–2–3

1 y x

2

3-D 4-Node Shell/Membrane 4

P FACE ID 1 3

1 2

Main Index

NODES 1–2–3–4

38 Marc Volume C: Program Input Edges and Faces

3-D 6-Node Shell 3 P

FACE ID 1

6

NODES 1–2–3–4–5–6

5

1

4

2

3-D 4-Node Tetrahedral 4 3

FACE ID 1 2 3 4

NODES 1–2–4 2–3–4 3–1–4 1–2–3

1 2 3-D 6-Node Pentahedral 6 4

5

3 1 2

Main Index

FACE ID 1 2 3 4 5

NODES 1–2–5–4 2–3–6–5 3 –1 – 4 – 6 1–3–2 4–5–6

Chapter 1 Introduction 39 Edges and Faces

3-D 8-Node Brick 8 7

5 6 4 1

FACE ID 1 2 3 4 5 6

NODES 1–2–6–5 2–3–7–6 3–4–8–7 4–1–5–8 1–2–3–4 6–5–8–7

3 2

3-D 10-Node Tetrahedral 4

10

8

FACE ID 1 2 3 4

3

9 7 6

NODES 1 – 2 – 4 – 5 – 09 – 08 2 – 3 – 4 – 6 – 10 – 09 3 – 1 – 4 – 7 – 08 – 10 1 – 2 – 3 – 5 – 06 – 07

1 5 2 3-D 15-Node Pentahedral 3 15

FACE ID 1 2 3 4 5

6 8

9 11

12

7

1

2

13 4

Main Index

14 10

5

NODES 1 – 2 – 5 – 04 – 07 – 14 – 10 – 13 2 – 3 – 6 – 05 – 08 – 15 – 11 – 14 3 – 1 – 4 – 06 – 09 – 13 – 12 – 15 3 – 2 – 1 – 08 – 07 – 09 4 – 5 – 6 – 10 – 11 – 12

40 Marc Volume C: Program Input Guide to Organization of Marc Input Data

3-D 20-Node Brick 8 16

15 7

5

20

13

14

6 17

19

4 12

11 18

1

FACE ID 1 2 3 4 5 6

NODES 1 – 2 – 6 – 5 – 09 – 18 – 13 – 17 2 – 3 – 7 – 6 – 10 – 19 – 14 – 18 3 – 4 – 8 – 7 – 11 – 20 – 15 – 19 4 – 1 – 5 – 8 – 12 – 17 – 16 – 20 1 – 2 – 3 – 4 – 09 – 10 – 11 – 12 6 – 5 – 8 – 7 – 13 – 16 – 15 – 14

3 9

10 2

Guide to Organization of Marc Input Data The input data for Marc is organized into three basic groups. These groups form a natural subdivision of the data. Each group is then subdivided into various optional blocks of input data. The optional blocks of data within each group have been organized to minimize the input of unnecessary data. The main idea is to enable you to specify only the data for the optional blocks needed to define your problem. The various blocks of input are referred to here as optional in the sense that many have built-in default values which can be used and does not imply that they are optional in all cases. The input data is divided into the following three groups: Parameter Data This group of data is used to allocate the necessary working space for the problem and to set up initial switches which control the flow of Marc through the desired analysis. This set of input data is terminated with END parameter data. Model Definition Data This set of data is used to read in the initial loading, geometry, and material data of the model. It also provides nodal point data such a boundary conditions. In general, the initial model data is provided in this group and control restart. Print options can also be specified here for further Marc processing. This data provides Marc with the necessary information for determination of an initial elastic solution (zero increment solution in Marc terminology). This group of data is terminated with END OPTION data. History Definition Data This group of data provide the load incrementation and control of Marc after the initial elastic analysis. The group also includes blocks which allow changes in the initial model specifications. Each set of load incrementation data is terminated with CONTINUE data. This data sends Marc back for another increment or series of increments if the auto incrementation features are requested.

Main Index

Chapter 1 Introduction 41 Guide to Organization of Marc Input Data

Input data file organization for Marc is shown in Figure 1-1.

Linear Analysis

Linear and Nonlinear Analysis Requiring Incrementation

Proportional Increment Auto Load Etc.

Connectivity Coordinates Fixed Displacements Etc.

Title Sizing Etc.

Figure 1-1

Model Definition

Parameter

Marc Input Data File

Typical Marc Problem Data Files Marc Parameter Data END Data

Marc Model Definition Data (Zero Increment) END OPTION Data

Marc History Definition Data for the First Increment CONTINUE Data

(Additional History Definition Data for the 2nd, 3rd, ..., Increments)

Main Index

History Definition

42 Marc Volume C: Program Input Guide to Organization of Marc Input Data

Marc Input for New Users Marc input format is designed to allow the input of very complex problems. The new user is, however, faced with gaining familiarity with the system and its conventions. At the outset, therefore, you should adopt a systematic approach to the preparation of input data. One approach is to follow the construction of Marc and adopt the procedure of preparing input for each of the data blocks (parameter, model definition, and history definition options) in turn. We shall illustrate our discussion by preparing input for the analysis of a thin plate with hole subjected to pressure loading. The problem, as shown in Figure 1-2, is a well-known one so that the results can be compared to the exact solution (Timoshenko, Theory of Elasticity). The hole/plate size ratio is chosen to approximate an infinite plate. A procedure preparing Marc input takes the following steps: Finite Element Modeling The plate has an outside dimension of 10 inches x 10 inches with a central hole of 1 inch radius. The thickness of the plate is assumed to be 0.1 inches and the material property is assumed to be isotropic and linear elastic. The Young’s modulus is 30 x 106 pounds per square inch (psi) with Poisson’s ratio of 0.3. These quantities are sufficient to define the behavior of an isotropic, linear-elastic material. σ = 1.0 psi

10 in.

R = 1.0 in.

10 in. Plate Thickness = 0.1 in. E = 30 X 106 psi ν = 0.3

Figure 1-2

Plate with Hole

As shown in Figure 1-2, due to symmetry conditions, only a quarter of the plate is analyzed. Prescribed displacement boundary conditions exist along the lines of symmetry (that is, u = 0 at line x = 0; v = 0 at line y = 0) and traction (pressure) boundary condition exits at the top of the plate.

Main Index

Chapter 1 Introduction 43 Guide to Organization of Marc Input Data

This quarter plate is approximated by a finite element mesh consisting of twenty 8-node plane stress elements with appropriate loading and boundary conditions. The element (Marc type 26) is a secondorder, isoparametric two-dimensional element for plane stress. There are eight nodes with two translational degrees of freedom at each node. A description of element type 26 can be found in Marc Volume B: Element Library. This example uses a coarse mesh for demonstration purposes only. The analyst must anticipate the sharp stress gradients in this problem and design the mesh accordingly. This is achieved in this problem by using progressively smaller elements as the hole is approached. If necessary, further mesh refinement can be achieved by adding elements to the mesh. The preparation of parameter, model definition, and history definition data for this example is demonstrated as follows: Parameter Data The analysis to be carried out in this example is a linear elastic analysis with plots. Consequently, only five parameters are needed for the input data: TITLE ELEMENTS SIZING END

In this example, the title, Elastic Analysis of a Thin Plate with Hole, is chosen for the problem and entered through the TITLE parameter. The selected Marc element type 26 is entered through the ELEMENTS parameter. No data is required on the SIZING parameter: Finally, the parameters are completed with an END parameter. At this stage, the input data is: TITLE ELASTIC ANALYSIS OF A THIN PLATE WITH HOLE SIZING ELEMENTS,26, END Model Definition Data The model definition data contains the bulk data for the analysis. The data entered here concerns: 1. the topology of the model (finite element mesh in terms of element connectivity and nodal coordinates, as well as plate thickness), 2. material property (Young’s modulus and Poisson’s ratio),

Main Index

44 Marc Volume C: Program Input Guide to Organization of Marc Input Data

3. pressure loading and prescribed displacement boundary conditions, and 4. plotting and output controls. A list of the model definition options can be found in Chapter 3 of this document. 1. Topology of the Model The topology of the plate model is numerically defined by the following model definition options: CONNECTIVITY COORDINATES GEOMETRY

In this example, the mesh consists of 20 elements and 79 nodes. The data required for element connectivity and nodal coordinates are: CONNECTIVITY 20 1 26 1 2 26 3 3 26 9 4 26 11 5 26 5 6 26 3 7 26 30 8 26 32 9 26 38 10 26 40 11 26 1 12 26 47 13 26 9 14 26 53 15 26 49 16 26 47 17 26 30 18 26 69 19 26 38 20 26 75 COORDINATES 0 0 1 1.4000 2 1.5500 3 1.7000 . . . 77 0.0000 78 0.4931 79 0.0000

3 5 11 13 3 1 32 34 40 42 9 53 17 59 64 66 38 75 29 66

11 13 19 21 27 29 40 42 27 25 53 55 59 61 66 29 75 77 66 64

9 11 17 19 25 27 38 40 29 27 47 49 53 55 47 1 69 71 75 77

2 4 10 12 4 2 31 33 39 41 6 50 14 56 62 63 35 72 43 78

7 8 15 16 23 24 36 37 44 45 52 54 58 60 65 67 74 76 67 65

10 12 18 20 26 28 39 41 28 26 50 51 56 57 63 24 72 73 78 79

6 7 14 15 22 23 35 36 43 44 46 48 52 54 48 46 68 70 74 76

1.4000 1.0500 0.7000

1.2500 1.1910 1.3750

The data in the CONNECTIVITY option consists of element numbers (1,2,...,19,20), element type (26), and for each element, four corner node numbers and four midside node numbers.

Main Index

Chapter 1 Introduction 45 Guide to Organization of Marc Input Data

The data in the COORDINATES option consists of the node number (1); and coordinates (x = 1.4, y = 1.4) of node 1 in the global coordinate system (x, y). Finally, the plate thickness is entered through GEOMETRY as: GEOMETRY 0, 0.1, 1 TO 20 A thickness of 0.1 inches is assumed for all twenty (1 to 20) elements. 2. Material Property Material properties of the plate are entered through the ISOTROPIC option. For our problem, the only data required for a linear elastic analysis are Young’s modulus and Poisson’s ratio. The same material is used for the whole mesh (from Element No. 1 to Element No. 20). This is given a material ID of 1. The data in ISOTROPIC is: ISOTROPIC 1, 1, 30.E6,0.3, 1 TO 20 3. Pressure Loading and Prescribed Displacement Boundary Conditions As shown in Figure 1-3, the pressure loading is acted on two elements (elements 13 and 14), along the lines 61-60-59 and 59-58-17. From CONNECTIVITY, we observe that these lines represent the 2-6-3 face of the elements. As a result, a distributed load type of 8 can be determined for the pressure loading from the QUICK REFERENCE of element 26 in Marc Volume B: Element Library. "LOAD TYPE (IBODY)=8 FOR UNIFORM PRESSURE ON 2-6-3 FACE" In addition, as shown in Figure 1-4, the sign conversion of the pressure loading is that a negative magnitude represents a tensile distributed load. Consequently, the input for the one pound tensile distributed loading (DIST LOADS) acting on elements 13 and 14 takes the following form: DIST LOADS 0, 8,-1., 13,14,

Main Index

46 Marc Volume C: Program Input Guide to Organization of Marc Input Data

60

61

59

58

14

57

17

13 16

55

3

12

51

11

19

49 62 64 79 77 73 71

1

15 16 20 18 19 17 9 7 8 10

y

20

6

5 in.

4 5

34 37424525 22 5

2 5 in. 8

13

16

21

Radius of the hole = 1 in. x

1

Figure 1-3 4

8

Mesh Layout for Plate with Hole 7

3

7

8

9

4

5

6

1

2

3

1

5

Figure 1-4

6

2

Integration Points of Eight-Node, 2-D Element

The FIXED DISP option is used for the input of prescribed displacement boundary conditions at the lines of symmetry (x = 0, y = 0). As indicated in the QUICK REFERENCE of element 26, the nodal degrees of freedom are as follows: dof 1 = u = global x-direction displacement dof 2 = v = global y-direction displacement.

Main Index

Chapter 1 Introduction 47 Guide to Organization of Marc Input Data

In this example, the symmetry conditions require that: dof 1 = u = 0 for nodes (71, 73, 77, 79, 64, 62, 49, 51, 55, 57, 61) along the line x=0.

and dof 2 = v = 0 for nodes (34, 37, 42, 45, 25, 22, 5, 8, 13, 16, 21) along the line y=0.

The input data takes the following format: FIXED DISP 2, 0., 2, 34,37,42,45,25,22,5,8,13,16,21, 0., 1, 71,73,77,79,64,62,49,51,55,57,61, 4. Bandwidth Optimization and Output Controls Although the bandwidth in this sample problem cannot be extremely large, the use of the OPTIMIZE model definition option demonstrates the bandwidth optimization capabilities in Marc. This option can reduce considerable computing costs in larger problems. The bandwidth optimization option creates an internal node numbering different from your node numbering, but all data input and output is in your node numbering system. There are a number of options available to you for bandwidth optimization. The option number 2 (Cuthill-McKee algorithm) with a maximum of ten iterations is selected for this example. OPTIMIZE,2,0,0,1, 10, In order to minimize the output quantity (number of printed pages), the PRINT ELEMENT option is used for printing out stresses and strains at a few integration points of a number of elements. The elements to be printed are: From Element

to

Element

2

2

4

5

8

8

10

10

Only two integration points (numbers 4 and 6) where stresses and strains are to be printed. Nodal quantities (displacement, reactions, etc.) are printed for all nodes (from node 1 to node 79). The input data of PRINT ELEMENT is: PRINT ELEMENT 1,

Main Index

48 Marc Volume C: Program Input Guide to Organization of Marc Input Data

STRESS STRAIN 2,4,5,8,10 4,6, The SUMMARY option produces summary tables containing maximum and minimum values of stresses and strains. The model definition data is completed with an END OPTION. History Definition Data This following example is a linear-elastic analysis which requires no incrementation data. title elastic analysis of a thin plate with hole sizing elements 26 end connectivity 20 1 26 1 3 11 9 2 7 10 6 2 26 3 5 13 11 4 8 12 7 3 26 9 11 19 17 10 15 18 14 4 26 11 13 21 19 12 16 20 15 5 26 5 3 27 25 4 23 26 22 6 26 3 1 29 27 2 24 28 23 7 26 30 32 40 38 31 36 39 35 8 26 32 34 42 40 33 37 41 36 9 26 38 40 27 29 39 44 28 43 10 26 40 42 25 27 41 45 26 44 11 26 1 9 53 47 6 52 50 46 12 26 47 53 55 49 50 54 51 48 13 26 9 17 59 53 14 58 56 52 14 26 53 59 61 55 56 60 57 54 15 26 49 64 66 47 62 65 63 48 16 26 47 66 29 1 63 67 24 46 17 26 30 38 75 69 35 74 72 68 18 26 69 75 77 71 72 76 73 70 19 26 38 29 66 75 43 67 78 74 20 26 75 66 64 77 78 65 79 76 coordinates 0 0 1 1.4000 1.4000 2 1.5500 1.0500 3 1.7000 0.7000 4 1.8500 0.3500 5 2.0000 0.0000 6 2.3000 2.3000 7 2.5250 1.1500 8 2.7500 0.0000 9 3.2000 3.2000 10 3.2750 2.4000 11 3.3500 1.6000 12 3.4250 0.8000 13 3.5000 0.0000

Main Index

Chapter 1 Introduction 49 Guide to Organization of Marc Input Data

14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67

Main Index

4.1000 4.1750 4.2500 5.0000 5.0000 5.0000 5.0000 5.0000 1.7500 1.4900 1.2300 1.5000 1.3900 1.2800 1.1700 1.0600 0.7070 0.8315 0.9238 0.9810 1.0000 0.7953 1.0129 1.1250 0.8835 1.0008 1.1019 1.1855 1.2500 0.9718 1.1910 1.3750 1.0500 0.7000 0.3500 0.0000 1.1500 0.0000 2.4000 1.6000 0.8000 0.0000 2.0500 0.0000 3.7500 2.5000 1.2500 0.0000 0.0000 0.6150 0.0000 0.2650 0.5300 0.7950

4.1000 2.0500 0.0000 5.0000 3.7500 2.5000 1.2500 0.0000 0.0000 0.6150 1.2300 0.0000 0.2650 0.5300 0.7950 1.0600 0.7070 0.5557 0.3825 0.1948 0.0000 0.7953 0.4194 0.0000 0.8835 0.6753 0.4562 0.2299 0.0000 0.9718 0.4931 0.0000 1.5500 1.7000 1.8500 2.0000 2.5250 2.7500 3.2750 3.3500 3.4250 3.5000 4.1750 4.2500 5.0000 5.0000 5.0000 5.0000 1.7500 1.4900 1.5000 1.3900 1.2800 1.1700

50 Marc Volume C: Program Input Guide to Organization of Marc Input Data

68 0.5557 0.8315 69 0.3825 0.9238 70 0.1948 0.9810 71 0.0000 1.0000 72 0.4194 1.0129 73 0.0000 1.1250 74 0.6753 1.0008 75 0.4562 1.1019 76 0.2299 1.1855 77 0.0000 1.2500 78 0.4931 1.1910 79 0.0000 1.3750 geometry 1 0.1 1 to 20 isotropic 1 1 30000000. .3 1 to 20 dist loads 1 8 -1. 13 14 fixed displacement 2 0.0000e+00 2 34 37 42 45 25 0.0000e+00 1 71 73 77 79 64 optimize,2,0,0,1, 10, print element 1 stress strain 2 4 5 8 10 4 6 end option

Main Index

22

5

8

13

16

21

62

49

51

55

57

61

Chapter 1 Introduction 51 Discussion of Marc Output for New Users

Discussion of Marc Output for New Users Selected portions of the output for this problem are shown in the following. The small type on the output are the author’s comments and gives a further explanation. Marc first gives a notes section which identifies the version of Marc being used. This is followed by an echo of the input data and a summary of program sizing and options requested. W W MMMMM MMMMM WWWWW WWWWW MMMMMMMMM MMMMMMMMM WWWWWWWWW WWWWWWWWW MMMMMMMMMMMMM MMMMMMMMMMMMM WWWWWWWWWWWWW WWWWWWWWWWWWW MMMMMMMMMMMMMMMMMMMMMMMMMMMMMMMMM WWWWWWWWWWWWWWWWWWWWWWWWWWWWWWWWW MMMMMMMM MMMMMMMMMMMMMMM MMMMMMMM WWWWWWWW WWWWWWWWWWWWWWW WWWWWWWW MMMMMM MMMMMMMMMMM MMMMMM WWWWWW WWWWWWWWWWW WWWWWW MMMM MMMMMMM MMMM WWWW WWWWWWW WWWW MM MMM MM WW WWW WW M M M W W W MM MMM MM WW WWW WW MMMM MMMMMMM MMMM WWWW WWWWWWW WWWW MMMMMM MMMMMMMMMMM MMMMMM WWWWWW WWWWWWWWWWW WWWWWW MMMMMMMM MMMMMMMMMMMMMMM MMMMMMMM WWWWWWWW WWWWWWWWWWWWWWW WWWWWWWW MMMMMMMMMMMMMMMMMMMMMMMMMMMMMMMMM WWWWWWWWWWWWWWWWWWWWWWWWWWWWWWWWW MMMMMMMMMMMMM MMMMMMMMMMMMM WWWWWWWWWWWWW WWWWWWWWWWWWW MMMMMMMMM MMMMMMMMM WWWWWWWWW WWWWWWWWW MMMMM MMMMM WWWWW WWWWW M M Marc REVISION 2008 MSC.SOFTWARE CORPORATION machine type: NT (c) COPYRIGHT 2008 MSC.Software Corporation, all rights reserved

Marc - N T

Main Index

52 Marc Volume C: Program Input Discussion of Marc Output for New Users

i n p u t p a g e

d a t a

1

5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 -----------------------------------------------------------------------------title prob e2.9 elastic analysis title plate with hole title prob e2.9 elastic analysis - elmt 26 sizing card 5 elements,26, processor,1,1,1, version,10, end connectivity card 10 20 1 26 1 3 11 9 2 7 10 6 2 26 3 5 13 11 4 8 12 7 3 26 9 11 19 17 10 15 18 14 4 26 11 13 21 19 12 16 20 15 card 15 5 26 5 3 27 25 4 23 26 22 6 26 3 1 29 27 2 24 28 23 7 26 30 32 40 38 31 36 39 35 8 26 32 34 42 40 33 37 41 36 9 26 38 40 27 29 39 44 28 43 card 20 10 26 40 42 25 27 41 45 26 44 11 26 1 9 53 47 6 52 50 46 12 26 47 53 55 49 50 54 51 48 13 26 9 17 59 53 14 58 56 52 14 26 53 59 61 55 56 60 57 54 card 25 15 26 49 64 66 47 62 65 63 48 16 26 47 66 29 1 63 67 24 46 17 26 30 38 75 69 35 74 72 68 18 26 69 75 77 71 72 76 73 70 19 26 38 29 66 75 43 67 78 74 card 30 20 26 75 66 64 77 78 65 79 76 coordinates 2 79 1 1.4000 1.4000 2 1.5500 1.0500 card 35 3 1.7000 0.7000 4 1.8500 0.3500 5 2.0000 0.0000 6 2.3000 2.3000 7 2.5250 1.1500 card 40 8 2.7500 0.0000 9 3.2000 3.2000 10 3.2750 2.4000 11 3.3500 1.6000 12 3.4250 0.8000 card 45 13 3.5000 0.0000 -----------------------------------------------------------------------------5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 p a g e

2

5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 -----------------------------------------------------------------------------14 4.1000 4.1000 15 4.1750 2.0500 16 4.2500 0.0000 17 5.0000 5.0000 card 50 18 5.0000 3.7500 19 5.0000 2.5000 20 5.0000 1.2500 21 5.0000 0.0000 22 1.7500 0.0000

Main Index

Chapter 1 Introduction 53 Discussion of Marc Output for New Users

card

55

23 1.4900 0.6150 24 1.2300 1.2300 25 1.5000 0.0000 26 1.3900 0.2650 27 1.2800 0.5300 card 60 28 1.1700 0.7950 29 1.0600 1.0600 30 0.7070 0.7070 31 0.8315 0.5557 32 0.9238 0.3825 card 65 33 0.9810 0.1948 34 1.0000 0.0000 35 0.7953 0.7953 36 1.0129 0.4194 37 1.1250 0.0000 card 70 38 0.8835 0.8835 39 1.0008 0.6753 40 1.1019 0.4562 41 1.1855 0.2299 42 1.2500 0.0000 card 75 43 0.9718 0.9718 44 1.1910 0.4931 45 1.3750 0.0000 46 1.0500 1.5500 47 0.7000 1.7000 card 80 48 0.3500 1.8500 49 0.0000 2.0000 50 1.1500 2.5250 51 0.0000 2.7500 52 2.4000 3.2750 card 85 53 1.6000 3.3500 54 0.8000 3.4250 55 0.0000 3.5000 56 2.0500 4.1750 57 0.0000 4.2500 card 90 58 3.7500 5.0000 59 2.5000 5.0000 60 1.2500 5.0000 61 0.0000 5.0000 62 0.0000 1.7500 card 95 63 0.6150 1.4900 -----------------------------------------------------------------------------5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 p a g e

3

5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 -----------------------------------------------------------------------------64 0.0000 1.5000 65 0.2650 1.3900 66 0.5300 1.2800 67 0.7950 1.1700 card 100 68 0.5557 0.8315 69 0.3825 0.9238 70 0.1948 0.9810 71 0.0000 1.0000 72 0.4194 1.0129 card 105 73 0.0000 1.1250 74 0.6753 1.0008 75 0.4562 1.1019 76 0.2299 1.1855 77 0.0000 1.2500 card 110 78 0.4931 1.1910 79 0.0000 1.3750 isotropic card

Main Index

115

1 0.300e+08 0.300e+00 0.000e+00 0.000e+00 0.100e+21 0.000e+00

54 Marc Volume C: Program Input Discussion of Marc Output for New Users

1

card

120

card

125

card

130

2

3 16

4 17

5 18

6 19

7 20

8

9

10

11

12

13

14

geometry 1 1. 1 to 20 fixed displacement 0.0000e+00 2 34 37 42 0.0000e+00 1 71 73 77 dist loads

45

25

22

5

8

13

16

21

79

64

62

49

51

55

57

61

8 -1.000 13 14 summary card 135 optimize,2,0,0,1, 10, print element 1 stress strain card 140 2 4 5 8 10 4 6 post 16 17 2 0 19 17 equivalent von mises stress card 145 11 1st comp of total stress -----------------------------------------------------------------------------5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 p a g e

4

5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 -----------------------------------------------------------------------------12 2nd comp of total stress 13 3rd comp of total stress end option -----------------------------------------------------------------------------5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 ----------------------------------------------------------------------------------------------------------------------------------------------------------************************************************* ************************************************* program sizing and options requested as follows

element type requested************************* number of elements in mesh********************* number of nodes in mesh************************ max number of elements in any dist load list*** maximum number of point loads****************** load correction flagged or set************ number of lists of distributed loads*********** values stored at all integration points**** tape no.for input of coordinates + connectivity no.of different materials 1 max.no of slopes number of points on shell section ************* new style input format will be used********* maximum number of set names is***************** number of processors used ********************* Marc input version ************************

Main Index

26 20 79 2 0 3 5 5 11 50 1 10

15

c

Chapter 1 Introduction 55 Discussion of Marc Output for New Users

end of parameters and sizing ************************************************* *************************************************

At this stage, Marc attempts to allocate core for input of the model definition data and assembly of the element stiffness matrix. Marc first prints out the key to strain, stress, and displacement output for each element type chosen. Column numbers identifying output quantities are referenced to the appropriate components of stress, strain, or displacement. Then, the required number of words is printed out followed by a list of the internal core allocation parameters. They reflect the maximum requirements imposed by different elements. The internal element variables are different for each element type and are repeated for each element type used in a given analysis. key to stress, strain and displacement output

element type

26

8-node isoparametric plane stress quadrilateral stresses and strains in global directions 1=xx 2=yy 3=xy displacements in global directions 1=u global x direction 2=v global y direction workspace needed for input and stiffness assembly internal core allocation parameters degrees of freedom per node (ndeg) 2 max. number of coordinates per node 2 max. nodes per element (nnodmx) 8 max. invariants per int. points (neqst) 1 max.stress components per int. point (nstrmx) strains per integration point (ngens) 3

3

flag for element storage (ielsto) 0 elements in core, words per element (nelsto) total space required vectors in core, total space required

1046 20920 6004

words per record on disk set to

40960

internal element variables

internal element number

Main Index

53059

1

library code type 26

56 Marc Volume C: Program Input Discussion of Marc Output for New Users

number of nodes= 8 stresses stored per integration point = 3 direct continuum components stored = 2 shear continuum components stored = 1 shell/beam flag = 0 curvilinear coord. flag = 0 int.points for elem. stiffness 9 number of local inertia directions 2 int.point for print if all points not flagged 5 int. points for dist. surface loads (pressure) 3 library code type = 26 large disp. row counts 4 4 7 residual load correction is invoked

For nonlinear problems, it is important to note if the residual load correction was turned on. this is automatically done in the current version. This is followed by the model definition data; how it is read and interpreted by Marc. Marc then calculates the bandwidth of the stiffness matrix and optimizes it if the OPTIMIZE model definition option is included. The original bandwidth (try 0) and the optimized bandwidth (try 10). direct symmetric profile solver is invoked for region maximum connectivity in stiffness matrix is

1

17 at node

75

workspace needed for optimizing = 45562 maximum sky-line including fill-in is526at try 0(forward numbering) maximum sky-line including fill-in is1128at try10(backward numbering) maximum sky-line including fill-in is1307at try10(forward numbering) maximum sky-line including fill-in is900at try10(backward numbering) maximum connectivity in stiffness matrix is

maximum half-bandwidth is

26

14 at node

between nodes

21

40

and

number of profile entries including fill-in is

900

number of profile entries excluding fill-in is

546

total workspace needed with in-core matrix storage =

61121

load increments for each degree of freedom summed over the whole model from distributed loads dist. loads on undeformed configuration - increments for dist. loads increments for point loads 0.000000E+00 5.000000E+00 point loads 0.000000E+00

0.000000E+00

start of assembly

Main Index

cycle number is

0

46

Chapter 1 Introduction 57 Discussion of Marc Output for New Users

wall time =

2.00

start of matrix solution wall time = 2.00 singularity ratio

1.8140E-01

end of matrix solution wall time = 2.00

element with highest stress relative to yield is where equivalent stress is 3.091E-20 of yield

NT version Marc 2008 output for increment

8

0. "prob e2.9 elastic analysis - elmt 26"

total strain energy within which: elastic strain energy plastic strain energy total ext-force work within which: work by appl. force/disp. work by contact forces work by frictional forces

is

4.60569E-07

is is is

4.60569E-07 0.00000E+00 4.60569E-07

is is is

4.60569E-07 0.00000E+00 0.00000E+00

After the bandwidth calculation (and optimization), Marc assigns the necessary workspace for the in-core solution of this matrix. maximum connectivity is 14 at node 40 maximum half-bandwidth is 26 between nodes 21 and 46 number of profile entries including fill-in is 900 number of profile entries excluding fill-in is 546 total workspace needed with in-core matrix storage = 60117

Marc then calculates the loading and sums the load applied to each degree of freedom for distributed loads and point loads. This information provides for a valuable check on the total loads in the different degrees of freedom. load increments associated with each degree of freedom summed over the whole model distributed loads 0.000e+00 5.000e-01 point loads 0.000e+00 0.000e-00 load increments associated with each degree of freedom summed over the whole model distributed loads 0.000e+00 5.000e-01

Main Index

58 Marc Volume C: Program Input Discussion of Marc Output for New Users

point loads 0.000e+00 0.000e-00

Then it prints the time (system billing units) at the start of assembly measured from the start of the job. It then prints out the bandwidth which might have changed due to optimization of the nodal numbering (if specified by you). This is followed by a printout of the time at the start of the matrix solution start time start time

of assembly = 0.18 of matrix solution = 0.24

If the out-of-core solver is used, a figure representing the profile of the global stiffness matrix is shown. It then prints the following message which gives an estimate of the conditioning of the matrix. If the singularity is of the order of the accuracy of the machine (10 for 64 bits), the equations can be considered singular and the solution unreliable. For nonlinear problems, incremental changes in the singularity ratio reflects approaching instabilities. Marc then prints the time at the end of the matrix solution. This is the time at the end of matrix triangularization.

singularity ratio 1.8140e-01 end of matrix solution time = 0.25 At this stage, Marc enters a back substitution for the displacements. This is followed by calculation of element stress values. Default yield stress is set by Marc for a linear elastic analysis.

MARC 2008, 01/03/07, output for increment 0. plate with hole element with highest stress relative to yield is 0.309e-19 of yield

elastic analysis of a thin 8

where equivalent stress is

A heading is printed next. The Tresca Intensity is output for application in ASME code applications. The Mises intensity is the equivalent yield stress. Principal stress and strain values are output. This is followed by individual stress and strain components. The number of each column is to be used with the key printed at the beginning of the analysis. tresca mises mean p r i n c i p a l v a l u e s o m p o n e n t s intensity intensity normal minimum intermediate maximum 1 5 6

p h y s i c a l 2

3

c

4

intensity element 20 point 4 integration pt. coordinate= 0.234e+00 0.121e+01 section thickness = 0.100e+00 engsts 5.802e-01 5.413e-01-1.342e-01-4.914e-01 0.000e+00 8.880e-02-4.531e-01 5.052e-02-1.440e-01 engstn 2.514e-08 1.550e-08-3.131e-09-1.727e-08 0.000e+00 7.874e-09-1.561e-08 6.215e-09-1.248e-08 element 20 point 6 integration pt. coordinate= 0.261e+00 0.137e+01 section thickness = 0.100e+00 engsts 6.055e-01 5.255e-01-2.275e-02-3.369e-01 0.000e+00 2.686e-01-2.677e-01 1.995e-01-1.926e-01 engstn 2.624e-08 1.518e-08-5.307e-10-1.391e-08 0.000e+00 1.232e-08-1.092e-08 9.326e-09-1.669e-08

The stress and strain results are followed by the increment of displacements and the total displacements for all the nodes. If it is requested to print and store all stress points, a printout of the reaction forces would follow the displacement output.

Main Index

Chapter 1 Introduction 59 Discussion of Marc Output for New Users

n o d a l

p o i n t

i n c r e m e n t a l 1 -2.17163e-08

7.15861e-08

4 -4.76926e-08 7 -4.39062e-08

1.49932e-08 4.43055e-08

d a t a

d i s p l a c e m e n t s

2 -3.08177e-08

5.15029e-08

3 -4.07290e-08

3.20392e-

08 5 -5.04297e-08 8 -5.45603e-08

t o t a l 1 -2.17163e-08

7.15861e-08

4 -4.76926e-08 7 -4.39062e-08

1.49932e-08 4.43055e-08

0. 0.

6 -2.76616e-08 9 -3.22702e-08

9.27126e-08 1.16274e-07

d i s p l a c e m e n t s 2 -3.08177e-08

5.15029e-08

3 -4.07290e-08

3.20392e-

08 5 -5.04297e-08 8 -5.45603e-08

0. 0.

6 -2.76616e-08 9 -3.22702e-08

9.27126e-08 1.16274e-07

total equivalent nodal forces (distributed plus point loads) 1 4 7

0. 0. 0.

0. 0. 0.

2 5 8

0. 0. 0.

0. 0. 0.

3 6 9

0. 0. 0.

0. 0. 0.

reaction forces at fixed boundary conditions, residual load correction elsewhere 1

1.21431e-17 -3.61690e-16

2

1.24033e-16 -1.11022e-16

3 -1.86483e-16

9.54098e-

4

1.31839e-16

1.42247e-16

5 -4.68375e-17 -4.27307e-02

6 -7.19910e-17

1.66533e-

7 -5.20417e-18

1.11022e-16

17 16 8 -3.96005e-17 -0.11445

9 -1.72388e-17

1.04083e-16

summary of externally applied loads 0.00000e+00

0.50000e+00

-0.72045e-17

-0.50000e+00

summary of reaction/residual forces

The results are concluded with an indication of the magnitude of distributed loads.

distributed load list number 1

type 8

current magnitude -1.000

0.

0.

The SUMMARY model definition option prompts Marc to print summary tables of stresses and strains as follows:

************************************************************************ ************************************************************************ * * * elastic analysis of a thin plate with hole * * * * increment 0 MARC 2008 * * *

Main Index

60 Marc Volume C: Program Input Discussion of Marc Output for New Users

************************************************************************ * * * * * * * quantity * value * elem.* int.*layer* * * *number*point* * * * * * * * ************************************************************************ * * * * * * * max first comp. of stress * 0.52712e+00 * 7 * 2 * 1 * * min first comp. of stress * -0.11257e+01 * 18 * 7 * 1 * * * * * * * * * * * * * * max second comp. of stress * 0.31370e+01 * 8 * 3 * 1 * * min second comp. of stress * -0.75958e-01 * 18 * 4 * 1 * * * * * * * * * * * * * * max third comp. of stress * 0.15887e+00 * 18 * 1 * 1 * * min third comp. of stress * -0.84812e+00 * 7 * 3 * 1 * * * * * * * * * * * * * * max equivalent stress * 0.30910e+01 * 8 * 3 * 1 * * min equivalent stress * 0.26979e+00 * 17 * 4 * 1 * * * * * * * * * * * * * * max mean stress * 0.10821e+01 * 8 * 3 * 1 * * min mean stress * -0.38696e+00 * 18 * 7 * 1 * * * * * * * * * * * * * * max tresca stress * 0.31419e+01 * 8 * 3 * 1 * * min tresca stress * 0.29647e+00 * 17 * 4 * 1 * * * * * * * * * * * * * * max first comp. of total strain * 0.58578e-08 * 7 * 1 * 1 * * min first comp. of total strain * -0.37172e-07 * 18 * 7 * 1 * * * * * * * * * * * * * * max second comp. of total strain * 0.10347e-06 * 8 * 3 * 1 * * min second comp. of total strain * 0.34023e-08 * 17 * 7 * 1 * * * * * * * * * * * * * * max third comp. of total strain * 0.13769e-07 * 18 * 1 * 1 * * min third comp. of total strain * -0.73504e-07 * 7 * 3 * 1 * * * * * * * * * * * * * * max equivalent total strain * 0.87678e-07 * 8 * 3 * 1 * * min equivalent total strain * 0.77458e-08 * 17 * 4 * 1 * * * * * * * * * * * * * * max mean total strain * 0.00000e+00 * 1 * 1 * 1 * * min mean total strain * 0.00000e+00 * 1 * 1 * 1 * * * * * * * ************************************************************************

The message end of increment 0 signifies the end of analysis for 0th increment. Additional output concerns only with post plottings. The output is finally concluded by plot messages, since plotting was requested.

************************************************************************ ************************************************************************ * * * elastic analysis of a thin plate with hole * * * * increment 0 MARC 2008 * * * ************************************************************************

Main Index

Chapter 1 Introduction 61 Discussion of Marc Output for New Users

* * * * * * * quantity * value * elem.* int.*layer* * * *number*point* * * * * * * * ************************************************************************ * * * * * * * max tresca total strain * 0.13162e-06 * 8 * 3 * 1 * * min tresca total strain * 0.12847e-07 * 17 * 4 * 1 * * * * * * * * * * * * * * max temperature * 0.00000e+00 * 1 * 1 * 1 * * min temperature * 0.00000e+00 * 1 * 1 * 1 * * * * * * * ************************************************************************ ************************************************************************ ****************************************************************** ****************************************************************** * * * elastic analysis of a thin plate with hole * * increment 0 Marc 2008 * * * ****************************************************************** * * * * * quantity * value * node * * * * number * * * * * ****************************************************************** * * * * * max first comp. of incremental disp * -0.19968e-08 * 48 * * min first comp. of incremental disp * -0.73223e-07 * 21 * * * * * * * * * * max second comp. of incremental disp * 0.20382e-06 * 61 * * min second comp. of incremental disp * 0.14872e-07 * 26 * * * * * * * * * * max first comp. of total disp. * -0.19968e-08 * 48 * * min first comp. of total disp. * -0.73223e-07 * 21 * * * * * * * * * * max second comp. of total disp. * 0.20382e-06 * 61 * * min second comp. of total disp. * 0.14872e-07 * 26 * * * * * * * * * * max first comp. of reaction force * 0.12293e-01 * 73 * * min first comp. of reaction force * -0.13867e-01 * 57 * * * * * * * * * * max second comp. of reaction force * -0.13839e-01 * 34 * * min second comp. of reaction force * -0.11445e+00 * 8 * * * * * ****************************************************************** ******************************************************************

e n d o f time =

i n c r e m e n t 1.17

0

The Marc exit number 3004 indicates the problem is completed.

Main Index

62 Marc Volume C: Program Input Discussion of Marc Output for New Users

Main Index

Marc Volume C: Program Input Chapter 2 Parameters List

2

Parameters List

Parameter

Main Index

Page

$NO LIST

83

ABLATION

126

ACCUMULATE

157

ACOUSTIC

134

ADAPTIVE

91

ALIAS

158

ALL POINTS

149

ALLOCATE

73

APPBC

156

ASSUMED STRAIN

108

AUTOMSET

186

AUTOSPC

188

BEAM SECT

191

BEARING

129

BOOC

171

64 Marc Volume C: Program Input

Parameter BOUNDARY CONDITIONS

181

BUCKLE

113

CAVITY

138

CENTROID

148

COMMENT

162

CONSTANT DILATATION

107

COUPLE

117

CREEP

114

CURING

128

DECOUPLING

118

DESIGN OPTIMIZATION

90

DESIGN SENSITIVITY

89

DIFFUSION

125

DIST LOADS

176

DYNAMIC

95

ELASTIC

88

ELASTICITY

109

ELECTRO

130

ELEMENTS

Main Index

Page

76

EL-MA

132

ELSTO

169

END

85

EXTENDED

84

FEATURE

78

FILMS

178

FINITE

106

FLUID

119

Chapter 2 Parameters List 65

Parameter FLUXES

177

FOLLOW FOR

111

FOURIER

94

HARMONIC

97

HEAT

123

INCLUDE

173

INPUT TAPE

168

IO-DEACTIVATE

189

ISTRESS

154

JOULE

124

LARGE DISP

102

LARGE STRAIN

103

LINEAR

Main Index

Page

93

LOAD COR

150

LUMP

155

MACHINING

140

MAGNETO

131

MNF

143

MPC-CHECK

185

NEW

160

NO ECHO

172

NO LOADCOR

151

NOTES

167

OOC

170

66 Marc Volume C: Program Input

Parameter PIEZO

133

PLASTICITY

110

PORE

121

PREALLOC PRINT PROCESSOR

75 163 80

PYROLYSIS

127

RADIATION

135

RBE

139

RESPONSE

99

RESTRICTOR

179

REZONING

142

R-P FLOW

100

SCALE

152

SHELL SECT

182

SIZING SPFLOW

74 101

SS-ROLLING

98

STATE VARS

175

STOP

166

STRUCTURAL

116

SUPER

144

TABLE

161

THERMAL

153

TIE

184

TITLE

Main Index

Page

72

TSHEAR

183

T-T-T

122

Chapter 2 Parameters List 67

Parameter UNIT

82

UPDATE

105

USER

145

VERSION

Main Index

Page

77

VISCO ELAS

115

WELDING

180

68 Marc Volume C: Program Input

Main Index

Chapter 2: Parameters Marc Volume C: Program Input

2

Main Index

Parameters

J

Basic Input Requirements

J

Analysis Types

J

Rezoning and Substructure Parameters

J

Additional Flags for Various Analyses

J

Program Function and I/O Controls

J

Modifying Default Values

J

Defining Cross-sections of Beam Elements

71

87 141 147 159

175 191

70 Marc Volume C: Program Input

This chapter describes the parameter section of the Marc input file. It is the first section of the file. The parameter section is used to specify the title of the file, the work space requirements, the elements to be used in the analysis, and the type of analysis to be performed. It is organized according to loosely defined categories of parameter types, as shown in the above list. Only the TITLE, ELEMENTS, and END parameters are required. Optional parameters flag the use of certain elements, analysis capabilities, or change the default values. The first ten columns of the parameter data are reserved for the key words which control the input of the parameters. These key words must be entered as left justified. Some options are set by the order in which data is input.

Main Index

Chapter 2: Parameters 71 Basic Input Requirements

Basic Input Requirements

Main Index

72 TITLE Output Title Definition

TITLE

Output Title Definition

This parameter is REQUIRED. Description This required parameter defines the output title. There is no limit to the number of the title data read in as long as the word TITLE appears in the first field. However, only the last TITLE data is used as an output header. Due to the free-format processor, do not place commas within the TITLE data (Columns 11-80). Format Format Fixed

Main Index

Free

Data Type Entry

1-10

1st

A

Enter the word TITLE.

11-80

2nd

A

Enter the title to be output with results.

ALLOCATE 73 Initial Workspace Definition

ALLOCATE

Initial Workspace Definition

Description This parameter allows the specification of memory to be allocated at the start of the job. Marc uses additional memory if necessary and it is available. See Appendix B Workspace Definition and the Sizing Option for more details. Values which are too large waste memory. The initial allocation can be done for the following parts. General memory: This specifies the initial allocation of the so-called general memory. This is used for boundary condition data, material data, storing element stiffness matrices, and part or all of the assembled global stiffness matrix among other things. Please note that element data like stresses and strains are no longer part of the general memory starting with the 2005r3 release. Solver 0 also uses the general memory area for the decomposition of the stiffness matrix. Initial allocation of the general memory can be used for avoiding reallocation (increase of the workspace). For parallel processing, the amount specified is the total for the job. It is divided by the number of domains used. Matrix solver: This specifies the initial allocation of memory for solver 8. By giving a value that is more than the maximum used during the run, one avoids that the solver workspace is increased (reallocated). This can be particularly useful for large contact jobs, where additional memory may be allocated due to contact. If the given workspace is less than what is needed, it is automatically increased. This option is only for use with solver type 8. No check is done to see if solver type 8 is used in the job. For parallel processing, the amount specified is the total for the job. It is divided by the number of domains used. Format Format Free

Main Index

Fixed

Data Type Entry

1-8

1st

A

Enter the word ALLOCATE.

11-15

2nd

I

Size of workspace in MByte for general memory.

16-20

3rd

I

Size of workspace in MByte for solver memory.

74 SIZING Working Space Definition

SIZING

Working Space Definition

Description This parameter can be used to specify the maximum number of nodes and elements. The values for the maximum number of elements and nodes should be set to an upper-bound if a manual rezoning analysis is performed. In general for other cases, they are not needed. If the number of elements or nodes in the model is greater than the value of MAXNUM in the include file located in the tools directory, then either the value of MAXNUM should be increased or the number of elements and nodes should be given on the SIZING parameter. The default value for MAXNUM is one million. The value of MAXNUM may also be set using the environment value of MSC_MMEM. This is often preferable to changing the include file. Format Format Fixed

Main Index

Free

Data Type Entry

1-10

1st

A

Enter the word SIZING.

11-20

2nd

I

Not used; enter 0.

21-25

3rd

I

Maximum number of elements.

26-30

4th

I

Maximum number of nodal points.

PREALLOC 75 Initial Workspace Allocation

PREALLOC

Initial Workspace Allocation

Description This parameter allows the specification of memory to be allocated at the start of the job. The workspace for solver 8, given in the second field, is used for allocating the workspace for the solver before any other memory is allocated. By giving a value that is more than the maximum used during the run, one avoids that the solver workspace is increased (reallocated). This can be particularly useful on 32 bit systems for large jobs. If the given workspace is less than what is needed, it is automatically increased. This option is only for use with solver type 8. No check is done to see if solver type 8 is used in the job. In a job using parallel processing, the allocation applies to the local domain and is the same on all domains. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word PREALLOC.

11-20

2nd

I

Size of workspace in words for solver type 8 (Multifrontal Direct Sparse Solver).

76 ELEMENTS Element Type Selection

ELEMENTS

Element Type Selection

This parameter is REQUIRED. Description This required parameter is used to identify the elements used in the analysis. Element codes for all the allowable element types are found in Marc Volume B: Element Library. This data can be repeated as often as necessary. Note that the ALIAS parameter is available to change element library code descriptions on the CONNECTIVITY model definition option. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word ELEMENTS.

11-15

2nd

I

Library code of the first type of element selected.

16-20

3rd

I

Library code of the second type of element selected.

21-25

4th

I

Library code of the third type of element selected.

Etc.

Etc.

I

Etc. up to 14 element types.

VERSION 77 Indicate the Version of the Marc Input Data File

VERSION

Indicate the Version of the Marc Input Data File

Description This parameter is used to control which version of the program to use from an input perspective and a defaults perspective. The following numbers are appropriate. 9

– defaults and input associated with MSC.Marc 2001

10

– defaults and input associated with MSC.Marc 2003

11

– defaults and input associated with MSC.Marc 2005

12

– defaults and input associated with Marc 2007

Note:

If this parameter is not included or is given a value of zero, it is automatically set to nine.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word VERSION.

11-15

2nd

I

Enter the input/analysis version to be used.

78 FEATURE Specification of the Behavior of a Feature

FEATURE

Specification of the Behavior of a Feature

Description This parameter allows the user to specify that a particular feature is to be defined in a selected data style. This permits data files to maintain compatibility with older versions of the program while still utilizing the latest technology. Currently, the following options used this capability:

Option

Consequence

DIST LOADS

203

Do not apply distributed load to a face or an edge if all nodes on the face or edge are in contact.

RADIATION

3301

Radiation viewfactor cut-off is relative; default for before version 11.

RADIATION

3302

Radiation viewfactor cut-off is relative; default for version 11.

MOONEY, ARRUDBOYCE, GENT, OGDEN

3402

use mixed J, u, p formulation for updated Lagrange rubber formulations and permits use of series representation of volumetric strain energy function.

5700

Set absolute rigid link rotation tolerance to 0.001; this is the default.

5701

Do not set absolute rigid link rotation tolerance by default; instead, read off the CONTROL option.

5800

Conventional element type 140.

5801

Add the enhanced strain contribution to improve the shell element performance especially for distorted meshes (linear analysis only).

5802

Extensions to 5801 for nonlinear analysis.

1002

Contact tolerance is based upon edge length of boundary elements only.

4401

Skip recycle due to body-body contact; generally reduces computational costs.

5301

Use double-sided tying in contact - this sometimes improves behavior for self contact, but often leads to increase costs. It should only be used if no other method resolves penetration problems.

6601

Remove deactivated deformable bodies from the post file.

8201

Activates improvements for force based friction models.

CONTROL

CONTACT

Main Index

Feature ID (ifeat)

FEATURE 79 Specification of the Behavior of a Feature

Feature ID (ifeat)

Option

Consequence

PIN CODE

6901

Use static condensation to remove pin code degrees of freedom. This is not recommended for dynamics.

HEAT

7001

Switch off Lobatto integration for convective boundary conditions to improve compatibility with 2005 r3.

7902

Used for higher order tetrahedral elements 127, 130 and 133: check inside-out condition based upon 16 integration points.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word FEATURE.

11-15

2nd

I

Enter the feature ID.

This parameter may be repeated as often as necessary, or you can enter 14 feature IDs per line.

Main Index

80 PROCESSOR Parallelization Control

PROCESSOR

Parallelization Control

Description This parameter may be used to specify the decomposition of the model when the single input DDM procedure is used. It is necessary to start the analysis using the -nps command line argument. For more details, see Table 2-3: Keyword Descriptions in Marc Volume A: Theory and User Information, Chapter 2: Program Initiation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PROCESSOR.

11-15

2nd

I

Not used; enter 0.

16-20

3rd

I

Not used; enter 0.

21-25

4th

I

Not used; enter 0.

26-30

5th

I

Not used; enter 0.

31-35

6th

I

Enter 1 to use DDM single input file.

36-40

7th

I

Decomposition method: Enter 11 to use Metis Best decomposition; default. Enter 12 to use Metis Element-Based decomposition. Enter 13 to use Metis Node-Based decomposition. Enter 14 to use Vector decomposition. Enter 15 to use Radial decomposition. Enter 16 to use Angular decomposition.

41-45

8th

I

Enter 1 to use out-of-core storage for DDM single input file.

46-50

9th

I

Flag for Additional Domain Decomposition Information (Default 0) 0 - No additional input 1 - Additional Input (Data Blocks 2 and 3 required)

2nd data block 1-5

1st

I

Island Removal Flag for Domain Decomposition (Default is 0) 0 - Do not attempt to remove Islands 1 - Attempt to remove Islands

Main Index

PROCESSOR 81 Parallelization Control

Format Fixed

Free

Data Entry Entry 2 - Detect contact during Decomposition; do not attempt to remove Islands 3 - Detect contact during Decomposition; attempt to remove Islands

6-10

2nd

I

Fine Graph Flag for Domain Decomposition (Default is 0) 0 - Coarse Graph 1 - Fine Graph

11-15

3rd

I

Control of point on axis of rotation for Radial/Angular Decompositions. 0 - Use Centroid of the Bounding Box of the model 1 - User-supplied point; defined in 4th, 5th, and 6th fields of 3rd data block.

16-25

4th

F

Element coefficient weight - Controls balance between computational cost of domains. Range <0.,1.0>. Default is 1.0 (use full element weight). 0 means do not use element weight.

3rd data block

Main Index

1-10

1st

F

First direction cosine of vector used for Decomposition method 14, 15, or 16.

11-20

2nd

F

Second direction cosine of vector used for Decomposition method 14, 15, or 16.

21-30

3rd

F

Third direction cosine of vector used for Decomposition method 14, 15, or 16.

31-40

4th

F

x-coordinate of point on axis.

41-50

5th

F

y-coordinate of point on axis.

51-60

6th

F

z-coordinate of point on axis.

82 UNIT Invoke Unit System Definition

UNIT

Invoke Unit System Definition

Description This parameter allows users to specify the unit system used in the analysis. The material data read in from the material data base or from the ISOTROPIC, WORK HARD, TEMPERATURE EFFECTS, MATERIAL DATA, GRAIN SIZE, and PARAMETERS options are converted to this set of units where appropriate. The output indicates both the user-defined quantity and the converted value. Note that if the material data is entered through a user subroutine, it must be consistent with the unit type specified here. This option is not applied to data entered through the TABLE option. Hence, the data must be consistent with the unit type entered here. For material data, it is advantageous to enter data normalized with respect to the reference value to avoid this problem. If this parameter is not included, no conversions are performed. If this parameter is included, the display of the results indicate the unit of the resultant quantity. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word UNIT.

11-15

2nd

I

Enter 1 for SI-meter unit. Enter 2 for SI-millimeter unit. Enter 3 for US-inch unit.

Notes:

For the unit definition and conversions, see Appendix I: Units. The unit is assumed to be SI-mm if this parameter is not used.

Main Index

$NO LIST 83 No Listing of Input Data

$NO LIST

No Listing of Input Data

Description Using this parameter results in the suppression of the printout of the remainder of the input file. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words $NO LIST.

84 EXTENDED Extended Precision of Reading in Data

EXTENDED

Extended Precision of Reading in Data

Description This parameter is used to indicate that models are to be in extended precision and/or a large number of elements or nodes exist in the model. If this option is included, the width of all the data fields described in this manual must be doubled. For example, all I5 integer fields change to I10. If this parameter is included, all input lines must be in this format. Note that the post file is written in 32 bit integer mode so the largest element of node ID is still limited to about one billion. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word EXTENDED.

END 85 End of Parameter Section

END

End of Parameter Section

This parameter is REQUIRED. Description This required parameter terminates the input of parameter data, signaling the end of the parameter section. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word END.

86

Main Index

Chapter 2: Parameters 87 Analysis Types

Chapt Analysis Types er 2: Para meter s

Main Index

88 ELASTIC Elastic Analysis with Multi-loads

ELASTIC

Elastic Analysis with Multi-loads

Description When this option is invoked, each load case is independent. Total loads must be input with the POINT LOAD, DIST LOADS, or CHANGE STATE/THERMAL LOADS model definition options after END OPTION. If the direct solver is invoked, the decomposed stiffness matrix is used for each load case and only a back substitution on a series of load vectors is performed. When the ADAPTIVE meshing option is used in conjunction with this parameter, only the loads before the END OPTION (increment zero) are considered. This load is then re-analyzed until the error criteria is satisfied. Notes:

This data should never be used with any data which flags nonlinear analysis or which change the stiffness matrix; for example, the LARGE DISP parameter or the DISP CHANGE option. If temperature dependent material properties are included, then a new assembly is performed (if temperature loading is on).

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word ELASTIC.

11-15

2nd

I

Element storage parameter, to reduce storage in elastic analysis. Set to 1, so that creep, swelling, plastic, incremental strains, plastic strain rates, and incremental stresses are not stored. Set to 2, so that strain energies, thermal strains, and elastic strains are not stored. Note:

Main Index

If you request these items on the post file and they are not stored, the information is incorrect.

DESIGN SENSITIVITY 89 Perform Sensitivity Analysis Only

DESIGN SENSITIVITY

Perform Sensitivity Analysis Only

Description This parameter invokes the design sensitivity capability in Marc. In this release, the capability is restricted to linear static structural analysis and eigenvalue analysis. This option requires the model definition options: DESIGN VARIABLES and at least one of DESIGN DISPLACEMENT CONSTRAINTS, DESIGN STRESS CONSTRAINTS, DESIGN STRAIN CONSTRAINTS, or DESIGN FREQUENCY CONSTRAINTS. If multiple load cases are to be evaluated, the ELASTIC parameter should be included. Format Format Fixed

Free

Data Entry Entry

1-18

1st

A

Enter the words DESIGN SENSITIVITY. Fixed field can be truncated to 12 characters

N/A

2nd

A

Enter the word SORT* if you desire to sort the constraints by degree of criticalness (optional), and also optionally to limit the number of constraints to be analyzed (see third field).

N/A

3rd

I

Only if SORT* is invoked, enter the number of most critical constraints to be analyzed. If no number is entered, the default number (100) of most critical constraints are isolated by sorting and are subjected to sensitivity analysis.

*If there are any eigenvalue constraints in the sorted group, these will be output before any static response constraints. Thus, the first constraint to be output may not always be the most critical one.

Main Index

90 DESIGN OPTIMIZATION Perform Design Optimization

DESIGN OPTIMIZATION

Perform Design Optimization

Description This parameter invokes the design optimization capability in Marc. In this release, the capability is restricted to linear static structural analysis and eigenvalue analysis. This option requires the model definition options: DESIGN OBJECTIVE, DESIGN VARIABLES and at least one of DESIGN DISPLACEMENT CONSTRAINTS, DESIGN STRESS CONSTRAINTS, DESIGN STRAIN CONSTRAINTS, or DESIGN FREQUENCY CONSTRAINTS. The DESIGN OBJECTIVE option is used to define the objective function. If multiple load cases are to be evaluated, the ELASTIC parameter should be included. Format Format Fixed

Free

Data Entry Entry

1-19

1st

A

Enter the words DESIGN OPTIMIZATION. Fixed field can be truncated to 12 characters.

N/A

2nd

A

Enter the word ACTIVESET (optional).

N/A

3rd

I

Only if ACTIVESET is invoked, enter the maximum number of constraints for the active set. This does not limit the number of constraints that can be prescribed by you. Default is 100.

N/A

4th

A

Enter the word CYCLES (optional).

N/A

5th

I

Only if CYCLES is invoked, enter the maximum number of design optimization cycles (including analyses). Default is 20. The order of the ACTIVESET and CYCLES can be reversed; for example, Free Formats 4th and 5th become 2nd and 3rd while Free Formats 2nd and 3rd become 4th and 5th.

Main Index

ADAPTIVE 91 Adaptive Mesh Refinement

ADAPTIVE

Adaptive Mesh Refinement

Description This parameter is required when either a local adaptive meshing or global adaptive meshing is to be used to improve the accuracy and/or mesh quality. The parameter indicates whether fixed bounds are set on the number of elements and nodes or whether dynamic memory should be used. Local Adaptive Meshing The criteria for determining when local remeshing should occur is provided in the ADAPTIVE model definition option.Local remeshing is available for lower-order shell and continuum elements including triangular, quadrilateral, tetrahedral, and brick elements. In an elastic analysis, Marc iterates based upon the excitation given to satisfy an error tolerance. The ELASTIC parameter must be included. In a steady-state heat transfer, electrostatic, or magnetostatic

analysis, Marc iterates until the error criteria is satisfied. In a nonlinear incremental analysis, Marc adapts the mesh at each increment, or user controlled frequency to improve the solution. New elements are created as described in Marc Volume A: Theory and User Information. Global Adaptive Meshing The criteria for determining when global remeshing is to occur is provided in the ADAPT GLOBAL model or history definition option. This option also indicates which remeshing procedure is to be used. Additionally, the REZONING,1 parameter must be used. Global adaptive meshing is available for lower-order triangular, quadrilateral, and tetrahedral, continuum, and shell elements in Marc. Format Format Fixed

Main Index

Free

Data Entry Entry

1-8

1st

A

Enter the word ADAPTIVE.

11-15

2nd

I

Enter an upper bound to the number of elements in the mesh.

16-20

3rd

I

Enter an upper bound to the number of nodes in the mesh.

21-25

4th

I

Enter 1 to continue to perform an incremental analysis. If the number of nodes or elements created exceeds the maximums specified, the previous mesh is used.

92 ADAPTIVE Adaptive Mesh Refinement

Format Fixed

Main Index

Free

Data Entry Entry

26-30

5th

I

Enter 1 if analysis is to be stopped when upper-bound is reached; otherwise, dynamically allocate more space.

Note:

If only the word ADAPTIVE is entered, the program dynamically allocates memory for the new elements and nodes (there is no limit to the number of elements or nodes unless all memory is exceeded).

LINEAR 93 Matrices Saved for Linear Analysis

LINEAR

Matrices Saved for Linear Analysis

Description This parameter allows additional values to be stored rather than being recalculated during subsequent increments. This means an increase in the overall size of the workspace used for the problem, but can actually result in a reduced computation time. The efficiency of this parameter is highly dependent upon the analysis data and the machine on which the problem is computed. It has proven very effective in reducing computation time for linear elastic and small displacement dynamic problems. When set to 0, the parameter has also been used effectively on nonlinear problems such as rigid plastic flow. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word LINEAR.

11-15

2nd

I

Enter 0 (default) to save BETA matrix (Strain-Displacement). Enter 1 to save the BETA matrix and the stress-strain law.

Main Index

94 FOURIER Arbitrary Loading of Axisymmetric Structures

FOURIER

Arbitrary Loading of Axisymmetric Structures

Description This parameter governs the analysis of axisymmetric structures under arbitrary loading by means of the Fourier series expansion technique. See Marc Volume A: Theory and User Information for a description of this analysis technique. To perform a modal Fourier analysis, you must include a DYNAMIC parameter. To perform a Fourier buckling analysis, you must include a BUCKLE parameter. Note:

Fourier analysis is not supported with the table driven input format in Version 2005.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word FOURIER.

11-15

2nd

I

Total number of FOURIER series expansions needed for characterizing the circumferential variation of tractions, thermal loads and boundary conditions.

16-20

3rd

I

Maximum number of harmonics in any of the series. The number of series terms is two times the number of harmonics plus one.

21-25

4th

I

Total number of nodal degrees of freedom that are loaded by concentrated forces or restrained by nonzero boundary conditions described by a FOURIER series expansion.

26-30

5th

I

If only symmetric (cos) terms are present in all expansions used, set this flag to 1. For strictly antisymmetric (sin) expansions, set this flag to 2. Default is 0 which allows for the full expansion containing sine and cosine terms. To skip increments 0 and 1 for symmetric terms only, set this flag to -1. To skip increments 0, 1 and 2 for antisymmetric terms only, set this flag to -2. A negative value of this flag means that no constant loading or constant nonzero boundary condition around the circumference are present.

Main Index

31-35

6th

I

Maximum number of stations around circumference used for printout during the superposition using CASE COMBIN option. Default is 24.

36-40

7th

I

Enter 1 if the initial stress stiffness is to be included in modal Fourier calculation.

DYNAMIC 95 Dynamic Analysis

DYNAMIC

Dynamic Analysis

Description This parameter sets the flags for one of several possible dynamic analysis methods. Any of several optional data blocks can be required. See Marc Volume A: Theory and User Information. The MODAL SHAPE history definition option or the MODAL INCREMENT model definition option controls the eigenvalue extraction. The DYNAMIC CHANGE or AUTO STEP history definition options control the time steps. The RECOVER history definition option allows for modal stress recovery or storing eigenvectors on the post file. Eigenvectors can also be stored on the post file with the MODAL INCREMENT option. Notes:

1) The single step Houbolt procedure is the recommended method for nonlinear transient analysis. 2) The Lanczos method is the recommended method for extracting eigenvalues. 3) The central difference operator do not work with zero mass at any degrees of freedom. 4) The direct integration operators automatically use residual load correction, and this cannot be overridden. The CENTROID parameter should not be used. 5) The Houbolt (IDYN=3)and central difference (IDYN=4) operators can only be used with constant time step. If the time step is changed during analysis, results are in error. The Newmark-beta (IDYN=2), fast central difference operator (IDYN=5), and Single Step Houbolt (IDYN=6) can use a variable time step. 6) Rigid body modes can be handled by the inverse power sweep or Lanczos method. Use the flag in the CONTROL option for solving a singular equation. 7) The fast central difference operator can be used with element types (2, 3, 5, 6, 7, 9, 10, 11, 18, 19, 20, 52, 64, 75, 98, 114, 115, 116, 117, 118, 119, 120). 8) The Newmark-beta method is unconditionally stable for linear analysis, with β = 0.25, γ = 0.50. These parameters can be reset through the PARAMETERS option. 9) The central difference (IDYN = 4) operator does not consider the term of damping.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word DYNAMIC.

11-15

2nd

I

Enter the dynamic operator type (IDYN). Set to 1 for modal superposition dynamic response. Set to 2 for Newmark direct integration.

Main Index

96 DYNAMIC Dynamic Analysis

Format Fixed

Free

Data Entry Entry Set to 3 for Houbolt direct integration. Set to 4 for explicit direct time integration using central difference. Set to 5 for fast explicit direct integration. Set to 6 for Single Step Houbolt integration (preferred for implicit dynamic analysis with contact). Set to 8 for generalized alpha method direct integration.

16-20

3rd

I

Maximum number of modes to be used in the modal superposition dynamic option. If the inverse power sweep method is used for eigenvalue analysis, it is also the number of mode shapes and frequencies to be extracted.

21-25

4th

I

Set to 0 for Inverse power sweep with double eigenvalue extraction. Set to 1 to for the Lanczos method. Set to 3 for Inverse power sweep with single eigenvalue extraction.

Main Index

26-30

5th

I

Enter 1 if modal stress recovery or storing eigenvectors on post tape is to be performed in this analysis.

31-35

6th

I

Not used; enter 0.

36-40

7th

I

Used only if the 2nd field is 8. Enter 0 (default) if the parameters of the generalized alpha method are optimized for an analysis involving dynamic contact; enter 1 if these parameters are optimized for an analysis without dynamic contact. Note that user-defined values can be entered on the PARAMETERS model definition or history definition option.

HARMONIC 97 Frequency Response Analysis

HARMONIC

Frequency Response Analysis

Description The HARMONIC parameter allows the frequency response analysis to be superimposed upon the deformed configuration. This parameter can also be used in conjunction with the EL-MA parameter for electromagnetic (harmonic) analysis or ACOUSTIC parameter for acoustic analysis or PIEZO parameter for piezoelectric analysis. Note that the 3rd through 5th fields are not required if the table input format is used. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word HARMONIC.

11-15

2nd

I

Enter 1 if complex damping matrix is used. Default is no complex damping.

16-20

3rd

I

Maximum number of excitation boundary conditions.

21-25

4th

I

Maximum number of excitation distributed load lists.

26-30

5th

I

Maximum number of elements in any excitation distributed load list.

31-35

6th

I

Enter 1 to include inertia effects in the calculation of the harmonic reaction force. Note that if damping is used, the mass proportional part of the damping matrix also contributes to the inertia effects.

98 SS-ROLLING Steady State Transport Analysis

SS-ROLLING

Steady State Transport Analysis

Description This flag activates steady state rolling analysis. No additional data is needed for this parameter. Using this procedure, an Eulerian/Lagrange analysis is performed on a body that is spinning about an axis, which may also be rotating. This is typically applied to tire models, see Marc Volume A: Theory and User Information for more detail. Model definition options ROTATION A and CORNERING AXIS are used to define rotation and cornering axes in a steady state rolling analysis. History definition option, SS-ROLLING, is used to define parameters such as spinning velocity, cornering velocity, and translational velocities. See the options descriptions for more details. Only three-dimensional solid elements are supported in the current release. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter SS-RO.

RESPONSE 99 Spectrum Response Analysis

RESPONSE

Spectrum Response Analysis

Description This parameter allows you to perform a spectrum response analysis. See Marc Volume A: Theory and User Information for detailed directions. The modes used are specified in the SPECTRUM response load incrementation data. To perform a SPECTRUM response calculation, it is also necessary to include the DYNAMIC parameter and either the MODAL INCREMENT or MODAL SHAPE option. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word RESPONSE.

11-15

2nd

I

Enter the number of data points used to specify spectral density function. Enter 0 to use the USSD user subroutine.

Main Index

100 R-P FLOW Rigid-Plastic Flow

R-P FLOW

Rigid-Plastic Flow

Description This parameter is used to specify a rigid, perfectly-plastic flow analysis. See Marc Volume A: Theory and User Information for an introduction to this technique. This parameter is used either with the Herrmann elements or with conventional elements. In the latter case, a penalty function is used to apply the incompressibility constraint. The penalty factor is defined through the PARAMETERS history definition option. This parameter has two modes. In the first mode, a steady state solution is obtained. This parameter can also be used for the analysis of laminar fluid flow problems. See the UNEWTN user subroutine in Marc Volume D: User Subroutines and Special Routines. This method requires iteration on the velocity field for convergence; convergence controls are input in the CONTROL option. In the second mode, a transient solution is obtained. This mode is always used in contact problems. This method required iteration on the incremental displacements. Increment 0 is suppressed. In this formulation, if the strain rate falls below a certain value, the material is effectively rigid. This cutoff value is specified through the PARAMETERS history definition option. Format Format Fixed

Free

Data Entry Entry

1-8

1st

A

Enter the words R-P FLOW.

11-15

2nd

I

Enter 1 for steady state procedure. Enter 2 for transient procedure.

16-20

3rd

I

Enter 1 for constant penalty factor. Option 2 is not available. Enter 3 for variable penalty factor (adjusted to limit volume loss).

Main Index

SPFLOW 101 Superplastic Forming Analysis

SPFLOW

Superplastic Forming Analysis

Description This parameter specifies the use of data for superplastic forming analysis. Use of this parameter automatically turns on the FOLLOW FOR,1 parameter. See ISOTROPIC model definition option for use of power law and rate power law hardening models (only available hardening rules for superplastic forming) and SUPERPLASTIC history definition option for control parameters in this document for more information. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word SPFLOW.

102 LARGE DISP Large Displacement or Buckling

LARGE DISP

Large Displacement or Buckling

Description This parameter is used to specify large displacement or buckling analysis. It signals Marc to calculate the geometric stiffness matrix and the initial stress stiffness matrix. This parameter automatically switches on the residual load correction option and switches off the scaling option. Default is no large displacement terms. See Marc Volume A: Theory and User Information for more information about large displacement and buckling analysis. Note:

The CENTROID parameter should not be used in conjunction with this parameter.

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words LARGE DISP.

LARGE STRAIN 103 Large Strain Analysis with Updated Lagrange Formulation

LARGE STRAIN

Large Strain Analysis with Updated Lagrange Formulation

Description This option specifies large strain analysis within the framework of updated Lagrange formulation. With this option, the Marc program calculates the geometric stiffness matrix and the initial stress stiffness matrix based upon the current configuration. Updated Lagrange procedures are not supported by some element types (for example, rebar elements). If LARGE STRAIN is specified, Marc internally switches to the total Lagrange formulation for the unsupported elements. For a list of elements not supported by updated Lagrange, refer to the Marc Volume B: Element Library

Note:

LARGE STRAIN must not be used with the CENTROID parameter due to nonlinearities in a large strain analysis.

For large strain analysis of rubber-like materials with incompressibility (such as materials defined with MOONEY, OGDEN, GENT, and ARRUDBOYCE model definition options), Marc uses a mixed formulation, in which both the displacement and the hydrostatic pressure are independent variables. For compressible hyperelastic materials defined with FOAM model definition option, Marc uses conventional displacement formulation. For large strain elastic-plastic analysis, the default procedure in Marc uses a procedure based on an additive decomposition of strain into an elastic part and a plastic part. In this case, volumetric strain is assumed to be constant for von Mises plasticity in a lower-order plane strain, axisymmetric, or a 3-D brick element. For elastic-plastic analysis using Herrmann elements, Marc internally switches to a procedure based on a multiplicative decomposition of deformation gradient into an elastic part and a plastic part. A mixed formulation is used to treat the incompressibility constraint. Herrmann elements have additional pressure degrees of freedom which result in increased computational times; hence, it is generally more efficient to use displacement-based elements.

In an elastic-plastic analysis, you can indicate the preferred algorithm for displacement-based elements. The obtained strain and stress with updated Lagrange formulation is logarithmic strain and Cauchy stress. Tables 3-12 and 3-13 (Chapter 3: Model Definition Options, Material Properties section) show the consequences of this option with different material types and element selections.

Main Index

104 LARGE STRAIN Large Strain Analysis with Updated Lagrange Formulation

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word LARGE STRAIN.

11-15

2nd

I

Flag to define preferred elasticity-plasticity procedure in an elastic-plastic analysis. = 1 Hypoelasticity and additive plasticity with mean normal return mapping (default) =2 Hyperelasticity and multiplicative plasticity with radial return mapping.

Main Index

UPDATE 105 Updated Lagrange Procedure

UPDATE

Updated Lagrange Procedure

Description This parameter flags the use of the classical updated Lagrange procedure for elastic-plastic materials, the elements for which such a formulation can be applied. The use of the procedure has two consequences. First, the element stiffnesses are assembled in the current configuration of the element. Second, the stress and strain output is given in the coordinate system which is applicable in the updated configuration of the element. The procedure is useful for analysis of shell and beam structures where rotations are large and the nonlinear terms in the curvature expressions can no longer be neglected. The updated Lagrange procedure can be used with or without the LARGE DISP parameter. With the LARGE DISP parameter invoked, the effect of the internal stresses on the stiffness is taken into account. Also, the strain increment is calculated to second order accuracy and, hence, large rotation increments might be allowed. Refer to Marc Volume B: Element Library for a list of the elements that can be used in an updated Lagrangian analysis. Instead of invoking the LARGE DISP parameter, the 4th entry of the UPDATE parameter can be set to 1. When the UPDATE parameter is used in conjunction with a coupled thermal-stress analysis, the element conductivity is assembled based on the current configuration of the element. Format Format Fixed

Main Index

Free

Data Entry Entry

1-6

1st

A

Enter the word UPDATE.

11-15

2nd

I

Not used; enter 0.

16-20

3rd

I

Enter 2 to allow large incremental rotations for beam elements. This is available for beam element types 52, 76, 77, 78, 79, and 98.

21-25

4th

I

Enter 1 to account for the effect of the internal stresses on the stiffness.

106 FINITE Finite Strain Plasticity

FINITE

Finite Strain Plasticity

Description This parameter flags the use of the large strain plasticity option. With this option invoked, the effects of the change in metric due to large inelastic deformations is included. This results in a different stiffness of the structure as well as in a modified calculation of stresses and inelastic strains. This parameter is only used for the elements which are formulated in terms of the updated Lagrange procedure. When using this parameter, true stresses are printed out. The UPDATE parameter must be included in all cases when this parameter is invoked. When the FINITE parameter is used, the work hardening slope for plasticity is defined as the rate of true stress versus the true plastic strain rate. Hence, the work hardening curve must be entered as the true stress versus logarithmic plastic strain curve in a uniaxial tension test. The anisotropic plasticity formulation cannot be used with this option. The finite strain option in Marc is written such that fairly large strain increments (up to 3%) can be allowed. However, large increments can result in many recycles as well as in decreased accuracy. Format Format Fixed 1-6

Main Index

Free 1st

Data Entry Entry A

Enter the word FINITE.

CONSTANT DILATATION 107 Define That Elements Are to Use Constant Dilatation Formulation

CONSTANT DILATATION

Define That Elements Are to Use Constant Dilatation Formulation

Description When performing nearly incompressible analysis with displacement based elements, the conventional isoparametric interpolation methods result in poor behavior for lower order elements. This results in overly stiff behavior when using element type 7, 149 (brick), type 10, 152 (axisymmetric), type 11, 151 (plane strain), type 19 (generalized plane strain), type 20 (axisymmetric with twist), or 136 (pentahedral). When this option is included, all elements of these types are modified to use the constant dilatation formulation. This is recommended for elastic-plastic analysis and creep analysis because of the potentially nearly incompressible behavior. Format Format Fixed 1-8

Main Index

Free 1st

Data Entry Entry A

Enter the word CONSTANT.

108 ASSUMED STRAIN Improved Bending Behavior

ASSUMED STRAIN

Improved Bending Behavior

Description The bending behavior can be improved by using the assumed strain formulation for element type 3, 160 (plane stress), type 11, 161 (plane strain), and type 7, 163 (brick). This procedure replaces the standard linear interpolation functions with an enriched group that is able to represent pure bending behavior. This formulation results in improved accuracy for isotropic behavior, but it should be noted that the computational costs increase. Note:

This option may not be used with all material behavior and is deactivated for those elements for which it is not applicable.

Format Format Fixed 1-7

Main Index

Free 1st

Data Entry Entry A

Enter the word ASSUMED.

ELASTICITY 109 Elasticity Procedure

ELASTICITY

Elasticity Procedure

Description This option can be used to define which formulation is used for large strain elasticity, including rubber and foam materials. The default is total Lagrange elasticity procedure. For rubber materials, either total (using Herrmann elements) or updated Lagrange (using either Herrmann or displacement elements) can be used. For foam, either total or updated Lagrange procedure is supported using the displacement based elements. The updated Lagrange procedure does not support plane stress elements and switches to total Lagrange procedure for these elements. For more details, see Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word ELASTICITY.

11-15

2nd

I

Enter 1 for total Lagrange formulation. Enter 2 for updated Lagrange formulation.

Main Index

110 PLASTICITY Plasticity Procedure

PLASTICITY

Plasticity Procedure

Description This option can be used to define the plasticity procedure that is used in Marc. The default is the mean normal procedure for satisfying the yield criteria and the additive decomposition of the incremental strains into elastic and plastic parts. For problems which have large elastic and plastic strains, the multiplicative decomposition is more accurate. The multiplicative decomposition implementation requires that the elasticity is isotropic. For more details, see Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word PLASTICITY.

11-15

2nd

I

Enter 1 for additive decomposition using the mean normal method; small strain formulation. Enter 2 for additive decomposition using the radial return method; small strain formulation. Enter 3 for additive decomposition using the mean normal method; large strain formulation using the updated Lagrange procedure. Enter 4 for additive decomposition using the radial return method; large strain formulation using the updated Lagrange procedure. Enter 5 for multiplicative decomposition (FeFp) using the radial return method and the three field variational principle; large strain formulation using the updated Lagrange procedure.

Main Index

FOLLOW FOR 111 Follower Forces: Distributed and Point Load Application on Current Geometry – Application of Total Boundary Condition

FOLLOW FOR

Follower Forces: Distributed and Point Load Application on Current Geometry – Application of Total Boundary Condition

Description The FOLLOW FOR parameter is used for follower force (for example, pressure) problems. Separate flags under this parameter are used to control follower forces for distributed loads and point loads respectively. When this parameter is used with default values for the associated flags, all distributed loads are formed on the basis of current geometry. This parameter requires the use of the residual load correction and, therefore, forces the use of that option regardless of other parameters (for example, the NO LOADCOR parameter is ignored). Whenever FOLLOW FOR is used, the distributed load magnitude given in the FORCEM user subroutine must be the total magnitude to be reached after the current increment, and not the incremental magnitude. In a coupled thermal-stress analysis, the fluxes are based upon the current geometry. When the table driven input procedure is not used, boundary conditions in structural analysis are normally entered as incremental values. To specify total values, use the third field of this option. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the words FOLLOW FOR.

11-15

2nd

I

Enter 1 if follower force stiffness due to distributed loads is not required (default). Enter 2 if follower force stiffness due to distributed loads is to be included. Enter 3 if the follower force for distributed loads is based upon the displacement at the beginning of the increment, as opposed to the last iteration. Enter -1 if the undeformed geometry is required but total values of distributed loads are to be used.

Main Index

16-20

3rd

I

Enter 1 if total values of boundary conditions are to be entered on DISP CHANGE, POINT LOAD, and DIST LOADS options as opposed to the default incremental loads.

21-25

4th

I

point loads is not required (default). Enter 1 if follower force for point loads is to be considered. Enter 0 if follower force for

112 FOLLOW FOR Follower Forces: Distributed and Point Load Application on Current Geometry – Application of Total

Notes:

If the follower force stiffness is included, the use of the SOLVER option can be used to specify a nonsymmetric formulation. This improves convergence, but results in longer solver times. If the 2nd field is 0 and the 4th field is 0, follower force is turned on for all distributed loads in the model (this allows compatibility with previous versions). Setting the 4th field to 1 only allows the possibility that point loads can be follower forces. Individual point loads specified under the POINT LOAD model and history definition options are used to actually specify if the load is a follower force or not. Follower force stiffness is not currently available for point loads.

Follower force stiffness for distributed loads is available for element types (3, 7, 10, 11, 18, 72, 75, 80, 82, 84, 114, 115, 116, 117, 118, 119, 120, 139, 149, 151, 152, 159, 160, 161, 162, 163, and 185).

Main Index

BUCKLE 113 Buckling Load Estimation via Eigenvalue Analysis

BUCKLE

Buckling Load Estimation via Eigenvalue Analysis

Description This parameter specifies the use of buckling load estimation by eigenvalue analysis, based on a perturbation of the tangent stiffness. Multiple eigenvectors are allowed for the case where the closest root to the current load set is not pertinent. Either the inverse power sweep method or the Lanczos method can be used. The BUCKLE history definition option or the BUCKLE INCREMENT modal definition option controls the eigenvalue extraction. The RECOVER history definition option allows for modal stress recovery or storing eigenvectors on a post file. The LARGE DISP parameter should be included to obtain the nonlinear collapse load estimate. Format Format Fixed

Free

Data Entry Entry

1-6

1st

A

Enter the word BUCKLE.

11-15

2nd

I

Maximum number of buckling modes to be estimated at any time.

16-20

3rd

I

Number of buckling modes with positive eigenvalues to be estimated at any time. In many buckling problems, collapse modes corresponding to loads of opposite magnitude to those of interest exist. By specifying a larger number of modes (say 5) in Columns 11-15 and one or two modes in this field, you can ensure getting the one or two modes you are interested in. Marc stops the modal search when all these modes have been formed, or when all the modes requested in columns 11-15 have been formed, whichever occurs first. If this field is left blank, all modes asked for in columns 11-15 are formed regardless of sign.

21-25

4th

I

Enter 1 if modal stress recovery or storing eigenvectors on post tape is to be performed in this analysis.

26-30

5th

I

Enter 3 to perform non-axisymmetric Fourier buckling.

31-35

6th

I

Enter 1 to use inverse power sweep with single eigenvalue extraction.

36-40

7th

I

Enter 0 if inverse power sweep method is to be used (default). Enter 1 if Lanczos method is to be used.

Main Index

114 CREEP Creep Analysis

CREEP

Creep Analysis

Description This parameter specifies a creep analysis. For more information about creep analysis, see the Creep Constitutive Data block model definition option in the section of this manual and Marc Volume A: Theory and User Information. The Marc CRPLAW and VSWELL user subroutines, used with creep analysis, are explained in Marc Volume D: User Subroutines and Special Routines. Note:

When using the implicit Maxwell creep model, the stress dependence must be in exponential form, the CRPLAW user subroutine cannot be used.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word CREEP.

11-15

2nd

I

Enter the flag for type of explicit creep analysis. Default of 0, normal creep (Maxwell Model); 1, viscoplastic creep; 2, viscoplastic creep with nonassociative flow rule.

16-20

3rd

I

Enter 1 for explicit Kelvin Model. (This is identical to the VISCO ELAS parameter.)

21-25

4th

I

Enter 1 for implicit Maxwell creep or implicit viscoplastic model.

26-30

5th

I

For the implicit Maxwell creep model or implicit viscoplastic model: When using the implicit Maxwell creep model, the stress dependence must be in exponential form, the CRPLAW user subroutine cannot be used. Enter 0 for elastic tangent Enter 1 for secant tangent Enter 2 for radial return

Main Index

VISCO ELAS 115 Visco Elastic Analysis (Kelvin Model)

VISCO ELAS

Visco Elastic Analysis (Kelvin Model)

Description This parameter flags the use of the CRPVIS user subroutine to model generalized Kelvin material behavior using an explicit procedure. See Marc Volume A: Theory and User Information for details. This parameter automatically flags the CREEP option as well, so that Maxwell behavior (VSWELL, CRPLAW user subroutines can be included with CRPVIS). Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words VISCO ELAS.

116 STRUCTURAL Mechanical Analysis

STRUCTURAL

Mechanical Analysis

Description This parameter is used in multi-physics analyses if one of the physics types is structural. It is used in combination with other parameters such as HEAT or ELECTRO. The inclusion of both the STRUCTURAL and ELECTRO parameters results in a coupled electrostatic-structural analysis. In such a multi-physics analysis, one pass will be a mechanical analysis and subjected to boundary conditions defined in the FIXED DISP, POINT LOAD, DIST LOADS, FOUNDATION, and CONTACT options. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word STRUCTURAL.

COUPLE 117 Coupled Thermal-Stress Analysis

COUPLE

Coupled Thermal-Stress Analysis

Description This parameter allows a coupled thermal-stress analysis. In these problems, the independent variables are displacements and temperatures. If you define displacement elements in the connectivity, heat transfer capabilities are included for these elements. To obtain the coupling between plastic work and internal heat generated, a DIST FLUXES model definition option with a flux type of 101 must be included. The CUPFLX user subroutine can be used to define an alternative model for internal heat generation. Care must be taken in defining the factor used to convert inelastic mechanical energy to thermal energy (see the CONVERT model definition option). If shell elements are present or latent heats are used, the HEAT parameter might also be required. For a coupled thermo-mechanical-electrical problem, it is also necessary to include a JOULE parameter. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word COUPLE.

118 DECOUPLING Set Control for Contact Decoupling Analysis

DECOUPLING

Set Control for Contact Decoupling Analysis

Description This parameter allows users to manually analyze contact between the workpiece and deformable tools in a decoupled manner. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word DECOUPLING.

11-15

2nd

I

Enter 1 for mechanical-only analysis.The deformable tools are treated as rigid bodies. Enter 2 for coupled analysis. The deformable tools are treated as rigidthermal bodies. Enter 3 for tool stress analysis only.

Notes:

Using contact decoupling assumes that the deformation in deformable tool is small compared to the workpiece deformation. No remeshing is allowed in the deformable tools. Typically, a decoupling analysis is run through the run_marc command: -dcoup. However, you can use the control here to run the analysis manually. The data transfer file is defined through READ FILE and WRITE FILE history options or, by default, using jid.t70 in the current directory.

Main Index

FLUID 119 Fluid, Fluid-Thermal, Fluid-Solid, and Fluid-Thermal-Solid Analysis

FLUID

Fluid, Fluid-Thermal, Fluid-Solid, and Fluid-Thermal-Solid Analysis

Description This parameter controls the procedure when performing a fluid analysis. In this release, Marc provides the ability to solve the Navier Stokes equations, excluding turbulence for incompressible fluids. Marc offers either weakly (staggered method) or strongly (simultaneous method) procedures in multi-physics type problems. Using the weak formulation, more iterations might be necessary, but overall computation costs might be less. For fluid-thermal problems, the strongly coupled procedure is recommended; while for fluid-solid problems, the weakly coupled procedure should be used. Furthermore, you can select how the fluid incompressibility conditions are to be satisfied. Either a mixed method, with degrees of freedom of velocity and pressure or a penalty method with degrees of freedom of velocity can be used with the continuum elements. The penalty factor can be entered through the PARAMETERS option. For more details, see Marc Volume A: Theory and User Information. Caution:

Fluid analysis cannot be performed with element types 155 through 157.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word FLUID.

11-15

2nd

I

Enter one of the following codes: 10 – fluid analysis – mixed method 11 – fluid analysis – penalty method 12 – fluid-thermal – mixed method – strong coupling 13 – fluid-thermal – penalty method – strong coupling 2 – fluid-thermal – mixed method – weak coupling 3 – fluid-thermal – penalty method – weak coupling 40 – fluid-solid – mixed method – weak coupling 41 – fluid-solid – penalty method – weak coupling 42 – fluid-thermal-solid – mixed method – strong – weak coupling 43 – fluid-thermal-solid – penalty method – strong – weak coupling 44 – fluid-thermal-solid – mixed method – weak – weak coupling 45 – fluid-thermal-solid – penalty method – weak – weak coupling

Main Index

120 FLUID Fluid, Fluid-Thermal, Fluid-Solid, and Fluid-Thermal-Solid Analysis

Format Fixed 16-20

Free 3rd

Data Entry Entry I

Enter 1 to obtain gradients and fluxes at integration points. Enter 2 to obtain in addition external flux values at nodal points. If this field is left blank, only temperatures at integration points and nodal temperatures are printed.

Main Index

PORE 121 Soil Analysis

PORE

Soil Analysis

Description This parameter sets the flags for one of several possible soil analysis. It is possible to perform either a pore pressure calculation (transient or steady state), a soil analysis (including the effects of previously obtained pore pressures), or a coupled pore-soil plasticity analysis. For information about soil analyses, see Marc Volume A: Theory and User Information. Notes:

If only a pore pressure calculation is be performed, use element types 41, 42 or 44. If an uncoupled soil calculation is to be performed, use element types 27, 28 or 21. If a coupled fluid-soil analysis is to be performed, use element types 32, 33 or 35.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word PORE.

11-15

2nd

I

Enter 0 if pore pressure data is to be entered. Enter 1 if a steady state pore pressure calculation is to be performed. Enter 2 if a transient pore pressure calculation is to be performed.

16-20

3rd

I

Enter 0 if only the pore pressure is to be calculated; for example, no stress analysis. Enter 1 if a stress analysis is to be performed.

Example If a fully coupled analysis is required, enter: PORE, 2, 1

Main Index

122 T-T-T Time-Temperature-Transformation

T-T-T

Time-Temperature-Transformation

Description This parameter allocates storage for the time-temperature-phase dependent properties. The properties themselves are defined using the TIME-TEMP model definition option. Most materials, when quenched or air cooled from a sufficiently high temperature, exhibit a change in mechanical or thermal properties. At any stage during the cooling process, these properties are usually dependent not only on the current temperature but also on the previous thermal history. This is due to the fact that the properties are influenced by the internal microstructure of the material and this in turn usually depends on the rate at which the temperature changes. Only in instances where the temperature is changed very gradually does the material respond in an equilibrium manner where properties are simply a function of the current temperature. In addition, during the cooling process, certain solid-solid phase transformations can occur. These represent another form of change in the material microstructure which can influence the mechanical or thermal properties. This parameter allows you to account for the timetemperature-transformation interrelationships of what are generally termed thermomechanical effects. For more information about this type of analysis, see the Marc Volume A: Theory and User Information. Format Format Fixed

Main Index

Free

Data Entry Entry

1-5

1st

A

Enter the expression T-T-T.

11-15

2nd

I

Enter the maximum number of material groups with time-temperaturetransformation dependent material properties (default is 1).

16-20

3rd

I

Enter the maximum number of cooling rates used to define any one property of any material group (see Marc Volume A: Theory and User Information for details). Default is 3.

21-25

4th

I

Enter the maximum number of temperature points at which a property value is specified for any cooling rate. Default is 5.

25-30

5th

I

If the thermal coefficient of expansion for any material group is to be expressed in terms of polynomial expansions in temperature, enter the maximum number of temperature points at which an expansion is defined for any cooling rate.

HEAT 123 Heat Transfer (Conduction) Analysis

HEAT

Heat Transfer (Conduction) Analysis

Description This parameter specifies a heat transfer (conduction) analysis instead of displacement/stress analysis. Convection can be included if the velocities are known or in a steady-state rigid plastic analysis. For the solution of the coupled thermal/flow problem, the FLUID parameter should be used. For more information about heat transfer capabilities in Marc, see Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1-4

1st

A

Enter the word HEAT.

11-15

2nd

I

Temperature distribution in thickness direction of heat transfer shell elements 50, 85, 86, 87, and 88. Enter 0 for linear temperature distribution in thickness direction. Enter 1 for quadratic temperature distribution in thickness direction. Default is 0.

16-20

3rd

I

Maximum number of latent heats associated with any material type. Default is 0.

21-25

4th

I

Enter 1 to obtain gradients and fluxes at integration points. Enter 2 to obtain in addition external flux values at nodal points. If this field is left blank, only temperatures at integration points and nodal temperatures are printed.

26-30

5th

I

Enter 2 to include convective terms. This automatically initiates the nonsymmetric solver. The velocity must be prescribed.

31-35

6th

I

Enter the number of heat transfer layers for composite shell elements. Default is 1.

36-40

7th

I

Enter 1 to linearize calculation of surface energy and receding surface data (default). Enter 2 to not linearize calculation.

41-45

Main Index

8th

I

Set to 1 to store value of nonhomogeneous density for postprocessing only. This is only applicable in a pyrolysis simulation.

124 JOULE Joule Heating (Coupled Thermo-Electrical) Analysis

JOULE

Joule Heating (Coupled Thermo-Electrical) Analysis

Description This parameter allows you to perform a coupled thermoelectrical (Joule heating) problem or a coupled thermo-mechanical-electrical problem. The coupling between the electrical problem and the thermal problem is because: (1) the resistance in the electric problem is dependent on temperatures and (2) the internal heat generation in the thermal problem is a function of the electric flow. For more information about the finite element formulation of Joule heating problems, see Marc Volume A: Theory and User Information. In the analysis of Joule heating, the model definition options JOULE, VOLTAGE, DIST CURRENT and POINT CURRENT must be used for the definition of electric problems. However, options for the heat transfer analysis remain unchanged. For a coupled thermo-mechanical-electrical problem, it is necessary to have either a COUPLE or a STRUCTURAL parameter. In such problems, there is additional coupling because of the change in boundary conditions through the CONTACT option which changes both the thermal and electrical behavior. Heat is generated not only by electrical resistance (Joule heating), but also by heat generated due to inelastic behavior. Note:

Joule heating is not applied to shell elements, conventional heat transfer will be applied in these regions.

Format Format Fixed

Free

Data Entry Entry

1-5

1st

A

Enter the word JOULE.

11-15

2nd

I

Enter 1 for conventional model Enter 2 if electrical properties are a strong function of temperature.

Main Index

DIFFUSION 125 Diffusion Analysis

DIFFUSION

Diffusion Analysis

Description This parameter indicates that a diffusion analysis is to be performed. The boundary conditions are applied using the FIXED PRESSURE, DIST MASS, and POINT MASS options. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word DIFFUSION.

126 ABLATION Specify Ablation Occurrence

ABLATION

Specify Ablation Occurrence

Description This parameter is used to specify that ablation is to occur. It is normally used in conjunction with the PYROLYSIS parameter. The surface to be ablated is specified via the RECEDING SURFACE option. Data used to control the ablation is entered via the SURFACE ENERGY option for the advanced model. Note:

Ablation is not applied to shell elements.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter word ABLATION.

11-15

2nd

I

Enter 1 to use normal based upon all surfaces. Enter 2 to use normal based upon surfaces given by RECEDING SURFACE data (default).

Enter 3 to use normal based upon direction of streamline. Enter 4 to use normal based upon direction of streamline with projected magnitude. 16-20

3rd

I

The following is used only with the shaver mesher: Enter 1 if new surface node coordinate is equal to old, shaved coordinate (default). Enter 2 if new surface node coordinate is projected coordinate.

21-25

4th

I

Enter the frequency to write the recession information to jid.rec file, default is write every increment.

26-30

5th

i

Enter 0, if Enter 1 if

Main Index

s· s·

calculated at surface integration points (default). calculated at the nodal point.

PYROLYSIS 127 Indicates Thermo-poro-ablative Model Analysis

PYROLYSIS

Indicates Thermo-poro-ablative Model Analysis

Description This parameter is used to indicate that a thermo-poro-ablative model is being analyzed. The region which can undergo pyrolysis is defined either via the THERMAL CONTACT or STREAM DEFINITION option. If the simplified streamline fluid flow model is used, the STREAM DEFINITION option is required. Note:

Pyrolysis is not applied to shell elements, conventional heat transfer will be applied in these regions.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter word PYROLYSIS.

11-15

2nd

I

Enter 1 for no fluid generation (default). Enter 2 for streamline fluid flow model. Enter 3 for D’Arcy fluid flow model.

16-20

3rd

I

Enter 1 to linearize calculation of surface energy and receding surface data (default). Enter 2 to not linearize system.

21-25

4th

I

Enter 1 to symmetrize convective terms (default). Enter 2 to use nonsymmetric formulation.

26-30

5th

I

Enter 0 or 1 if magnitude of

m· m· ˜

used in the surface energy or recession calculation is the .

Enter 2 if in used in the surface energy or recession calculation is the projection of m· ⋅ n . ˜

31-35

6th

I

Enter 1 for

φ

Enter 2 for

φ2

in rate term.

Enter -1 for no 36-40

Main Index

7th

I

˜

in rate term (default).

φ

in rate term.

Enter 1 to include divergence in

· ρg

Enter 2 to exclude divergence in

· ρg .

(default).

128 CURING Curing Analysis Parameter Definition

CURING

Curing Analysis Parameter Definition

Description The parameter flags the capability to take into account the curing effect on either the heat transfer or structural analysis. In a heat transfer analysis, the cure reaction heat flux is calculated and coupled into the heat transfer equation system. In a structural analysis, the cure induced volumetric shrinkage can also be incorporated. Notes:

The CURING parameter works in two analysis types: (a) Heat transfer analysis (b) Thermal-mechanical coupled analysis

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word CURING.

BEARING 129 Bearing Analysis

BEARING

Bearing Analysis

Description This parameter activates the bearing analysis facility for the analysis of lubrication problems. For more information about Marc’s bearing analysis capabilities, see Marc Volume A: Theory and User Information. In a bearing analysis, the model definition options VELOCITY, THICKNESS, RESTRICTOR, ISOTROPIC, FIXED PRESSURE, DAMPING COMPONENTS, STIFFNS COMPONENTS, and THICKNS CHANGE can be used to define the problem. Format Format Fixed

Main Index

Free

Data Entry Entry

1-7

1st

A

Enter the word BEARING.

11-15

2nd

I

Enter the maximum number of subincrements. Default is 4.

130 ELECTRO Electrostatic Analysis

ELECTRO

Electrostatic Analysis

Description This parameter allows an electrostatic analysis to be performed. The ISOTROPIC and ORTHOTROPIC model definition options are used to define the material properties. The FIXED POTENTIAL, DIST CHARGES, and POINT CHARGE options are used to prescribe the boundary conditions while the history definition option STEADY STATE is used for the steady state solution. For more information about the electrostatic analysis capability in Marc, see Marc Volume A: Theory and User Information. For information about elements used in electrostatic analysis, see Marc Volume B: Element Library. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word ELECTRO.

11-15

2nd

I

Potential distribution in thickness direction of shell elements 50, 85, 86, 87, and 88. Enter 0 for linear potential distribution in thickness direction. Enter 1 for quadratic potential distribution in thickness direction. Default is 0.

16-20

3rd

I

Flag to indicate which method for Coulomb Force calculation is used in a coupled electrostatic analysis. Enter 0 for using the electric field intensity based calculation. Use this when the distance between charged bodies is small. Enter 1 for the nodal charge based calculation. Use this when the distance between charged bodies is large. See Marc Volume A: Theory and User Information for details). Default is 0.

Main Index

MAGNETO 131 Magnetostatic Analysis

MAGNETO

Magnetostatic Analysis

Description This parameter specifies a magnetostatic analysis. The ISOTROPIC and ORTHOTROPIC model definition options are used for the input of isotropic or orthotropic magnetic permeabilities. The model definition options FIXED POTENTIAL, POINT CURRENT, and DIST CURRENT are used for prescribed potential and current boundary conditions; B-H RELATION is used for the input of the variation of magnetic permeability with either the magnetic field density or the magnetic field vector. Permanent magnets can be introduced by using the PERMANENT model definition option. The STEADY STATE history definition option is used for the steady state option. For more information about the magnetostatic analysis capability in Marc, see Marc Volume A: Theory and User Information. For information about elements used in magnetostatic analysis, see Marc Volume B: Element Library. Format Format Fixed 1-6

Main Index

Free 1st

Data Entry Entry A

Enter the word MAGNETO.

132 EL-MA Perform Electromagnetic Analysis

EL-MA

Perform Electromagnetic Analysis

Description This parameter activates the capability in Marc to perform an electromagnetic analysis. The electromagnetic analysis can be either a harmonic or a transient analysis. The ISOTROPIC and ORTHOTROPIC model definition options are used to define the material properties. The FIXED POTENTIAL, DIST CURRENT, and POINT CURRENT-CHARGE options are used to prescribe the boundary conditions while the HARMONIC and DYNAMIC CHANGE history definition options are used for the harmonic and transient solutions, respectively. Refer to Marc Volume A: Theory and User Information for a description of the electromagnetic analysis capability in Marc. An electromagnetic analysis can be performed with element types 111, 112, or 113. See Marc Volume B: Element Library for further details. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word EL-MA.

11-15

2nd

I

Set to 0 for transient electromagnetic analysis. Set to 1 for harmonic electromagnetic analysis. Default is 0.

16-20

3rd

I

Set to 0 for transient electromagnetic analysis using Newmark beta procedure. Set to 1 for transient electromagnetic analysis using backward Euler procedure; preferred for low-frequency simulations.

Main Index

PIEZO 133 Activate Piezoelectric Analysis

PIEZO

Activate Piezoelectric Analysis

Description This parameter activates a piezoelectric analysis. Possible analysis types are static, modal, transient dynamic, harmonic, or buckling. A description of the piezoelectric capabilities is included in Marc Volume A: Theory and User Information. Piezoelectric analysis may be performed with the following element types: 160

4-node plane stress

161

4-node plane strain

162

4-node axisymmetric

163

8-node brick

164

4-node tetrahedron

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word PIEZO.

134 ACOUSTIC Acoustic Analysis

ACOUSTIC

Acoustic Analysis

Description This parameter activates the capability to perform an acoustic analysis. The ACOUSTIC model definition option is used to prescribe the material behavior of the fluid. The FIXED PRESSURE, DIST SOURCES, and POINT SOURCE model definition options are used to prescribe boundary conditions. For Modal Acoustic analysis, Marc calculates the fundamental frequencies when the MODAL SHAPE option is encountered. A transient analysis can be performed using the DYNAMIC CHANGE option. This option can only be used in combination with cavities with rigid reflecting surfaces For Harmonic Acoustic analysis, Marc calculates the response of the coupled acoustic-solid system. The coupling is done via the CONTACT option. The frequency range is specified using the HARMONIC history definition option. Reactive boundary conditions can be given via the CONTACT TABLE option. For more information about the acoustic analysis capability in Marc, see Marc Volume A: Theory and User Information. For information about elements used in acoustic analysis, see Marc Volume B: Element Library. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word ACOUSTIC.

11-15

2nd

I

Maximum number of modes to be used in the modal superposition DYNAMIC parameter. If the inverse power sweep method is used for eigenvalue analysis, it is also the number of mode shapes and frequencies to be extracted. Only needed for modal acoustics.

16-20

3rd

I

Flag to indicate the Lanczos method is used. Set to 1 to force the Lanczos method. Only needed for modal acoustics.

21-25

4th

I

Enter 1 if modal stress recovery or storing eigenvectors on post file is to be performed in this analysis. Only needed for modal acoustics.

26-30

5th

I

Flag to indicate whether modal acoustics or harmonic acoustic analysis is used. 1 = modal acoustics (default) 2 = harmonic acoustics

Main Index

RADIATION 135 Radiation Analysis

RADIATION

Radiation Analysis

Description This parameter activates the radiation analysis capabilities in heat transfer and coupled analyses. This parameter selects the method to evaluate the viewfactors and controls the accuracy of the calculation of the vivisectors, and the resulting thermal radiation calculation as well. Depending on which method is chosen different model definition options are required to define the cavity and the specification of the emissivity as defined below. If spectral dependent emissivity is defined it is also necessary to use the PARAMETERS model definition option to specify the speed of light in the cavity medium. Format Format Fixed

Free

Data Entry Entry

1-9

1st

A

Enter the word RADIATION.

11-15

2nd

I

View factor calculation flag (IRADFL). Set to 0 to calculate viewfactors once using the direct integration method. The RADIATING CAVITY model definition option defines the cavity. This procedure is only available for axisymmetric cavities. The emissivity is defined with other material data through the ISOTROPIC, ORTHOTROPIC, etc. options. Set to 1 to read viewfactors from a file created by the direct integration approach. The emissivity is defined with other material data through the ISOTROPIC, ORTHOTROPIC, etc. options. Set to 2 to read view factor file created by Marc Mentat using the Monte Carlo method. They are read from a file jid.vfs. This procedure also requires the use of the VIEW FACTOR model definition option. The emissivity is defined with other material data through the ISOTROPIC, ORTHOTROPIC, etc. options. Set to 3 to calculate viewfactors by the hemi-cube projection method, and the view factor file will be in ascii format. The CAVITY DEFINITION option defines the cavity. The thermal radiation calculation is only active if the RAD-CAVITY option indicates that the cavity is used in a boundary condition, and the LOADCASE option is used to indicate that the boundary condition is active. The emissivity is defined either with other material data through the ISOTROPIC, ORTHOTROPIC, etc. options, or through the EMISSIVITY (preferred) option.

Main Index

136 RADIATION Radiation Analysis

Format Fixed

Free

Data Entry Entry Set to 4 to calculate viewfactors by the hemi-cube projection method, and the view factor file will be in binary format. The CAVITY DEFINITION option defines the cavity. The thermal radiation calculation is only active if the RAD-CAVITY option indicates that the cavity is used in a boundary condition, and the LOADCASE option is used to indicate that the boundary condition is active. The emissivity is defined either with other material data through the ISOTROPIC, ORTHOTROPIC, etc. options, or through the EMISSIVITY (preferred) option. Default is 0

16-20

3rd

I

Only used if IRADFL is 0 or 1. Enter the file number (IFILVF) for viewfactors. Viewfactors are written if IRADFL = 0, and are read if IRADFL = 1. When IRADFL = 0 and IFILVF = 0, the viewfactors are not saved. Default is 0.

21-25

4th

I

Temperature unit flag. Set to 0 to use offset temperature entered in PARAMETERS option. (Default) Set to 1 if user input is in degrees Celsius. Set to 2 if user input is in degrees Kelvin. Set to 3 if user input is in degrees Fahrenheit. Caution: Do not enter temperatures in degrees Rankine.

26-35

5th

F

Enter the Stefan-Boltzmann constant in the correct units. Default is the value given in PARAMETERS option, 5.67051 x 10-8W/m2K4.

For the direct integration approach. 36-40

6th

I

Number of divisions used in view factor calculation. Default is 3.

41-45

7th

I

Number of Gauss points used in each subdivision. Default is 3.

46-50

8th

I

Enter unit number for debug printout.

51-55

9th

I

Enter 4 for alternative (K4) method for calculation of view factors.

For the Monte Carlo approach (IRADFL=2) the 6th, 7th, 8th, and 9th fields are zero. For the hemi-cube approach (IRADFL=3 or IRADFL=4).

Main Index

36-40

6th

I

Enter the number of pixels (default is 500).

41-45

7th

I

Enter 1 to possibly re-evaluate the viewfactors based upon the motion of the structure. Only available in a coupled analysis using the updated Lagrange method, or in an analysis with ABLATION.

46-50

8th

I

For axisymmetric cavities, enter the number of divisions around circumference. Default is 36.

51-55

9th

I

Not used; enter 0.

RADIATION 137 Radiation Analysis

Format Fixed

Free

Data Entry Entry

For either the Monte Carlo or hemi-cube method.

Main Index

56-65

10th

E

Enter the fraction of the maximum view factor that is to be used as a cutoff. Viewfactors read in or calculated below this cutoff are ignored. Default is 0.0001.

66-75

11th

E

Enter the fraction of the maximum view factor that is to be treated implicitly (contribute to operator matrix). View factor values smaller than this cutoff are treated explicitly. Default is 0.01.

138 CAVITY Volume-dependant Pressure Load for Cavities

CAVITY

Volume-dependant Pressure Load for Cavities

Description This parameter governs the analysis of structures with internal cavities. When using the CAVITY parameter, the FOLLOW FOR parameter is automatically switched on. Note:

This capability is not available if the table input option is used.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word CAVITY.

11-15

2nd

I

Enter an upper bound to the number of cavities. Maximum is 1000.

16-20

3rd

I

Enter an upper bound to the number of segments in the cavity.

21-25

4th

I

Enter the number of nodes per segment. Enter 2 for low-order 2-D elements. Enter 3 for high-order 2-D elements. Enter 3 or 4 for low-order 3-D elements. Enter 6 or 8 for high-order 3-D elements. Default is 8.

Main Index

RBE 139 Rigid Body Elements

RBE

Rigid Body Elements

Description This option can be used to define the number of degrees of freedom for a reference node used in the RBE2 or RBE3 model definition option. This might be necessary in cases where the number of degrees of freedom for all other nodes in the structure is smaller than the required number of degrees of freedom for the reference node. This, for example, happens if the RBE2 or RBE3 option is used in an analysis with continuum elements only. It can also be used to set special features of RBE2 and RBE3. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word RBE.

11-15

2nd

I

Enter 3 for a 2-D analysis. Enter 6 for a 3-D analysis. Note:

16-20

3rd

I

Values other than 3 or 6 are not allowed.

Enter 1 to use large displacement formulation of RBE2 based upon a fixed coordinate system. Enter 3 to deactivate automatic convergence test by the RBE2 module.

21-25

4th

I

Enter 1 to use large displacement formulation of RBE3 based on small rotational increment assumption. Enter 2 to activate non-normalized rotation constraint coefficient of RBE3.

Main Index

140 MACHINING NC Machining (Metal Cutting) Process Analysis

MACHINING

NC Machining (Metal Cutting) Process Analysis

Description This parameter flags the capability to simulate the NC machining (that is, Metal Cutting or Material Removing) processes. With this option invoked, the deactivation of elements can be done according to the cutter path defined by either the APT source or CL files. The DEACTIVATE model or history definition option must be used in order to apply this capability during the course of analysis. Format Format Fixed 1-9

Main Index

Free 1st

Data Entry Entry A

Enter the word MACHINING.

Chapter 2: Parameters 141 Rezoning and Substructure Parameters

Chapt Rezoning and Substructure Parameters er 2: Para meter s

Main Index

142 REZONING Allow Rezoning

REZONING

Allow Rezoning

Description This parameter is used to indicate that rezoning can occur during this run. During rezoning, it is possible to add and/or delete elements and/or nodal points. If elements and/or nodal points are added, there should be enough elements and nodes allocated with the SIZING parameter in the initial run. The REZONING parameter can be used with all continuum displacement elements, shell elements 22, 75, 138, 139, and 140 and Herrmann elements 80 through 84 as well as elements 155 through 157. If the second field is entered as 1 or 2, automatic remeshing followed by rezoning is activated. In this case, use the ADAPTIVE parameter to define the upper-bound of the number of elements and nodes in the mesh and the ADAPT GLOBAL history definition option to define the criteria in global remeshing. Automatic remeshing with rezoning can only be used with the updated Lagrangian formulation, and with continuum (displacement or Herrmann) element. Marc switches to updated Lagrangian framework if the total Lagrangian formulation is specified in the input file. Global adaptive remeshing is available for lower-order triangular, quadrilateral continuum elements in 2-D and lower-order tetrahedral, lower-order triangular, or quadrilateral shell elements in 3-D. Note:

If rezoning is to be performed in this analysis, this parameter must be included from the very beginning. It cannot be added upon restart.

Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word REZONING.

11-15

2nd

I

Enter 0 for user supplied mesh for rezoning (default). Enter 1 for 2-D automatic remeshing followed by rezoning. Enter 2 for 3-D automatic remeshing followed by rezoning.

Main Index

MNF 143 MD ADAMS Modal Neutral File Options

MNF

MD ADAMS Modal Neutral File Options

Description This optional parameter allows the user to request that stress and/or strain modes be computed and exported to the MNF. It also allows the user to pick the layer number for shell elements. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word MNF.

11-15

2nd

I

Enter 1 to compute and export stress modes to MNF.

16-20

3rd

I

Enter 1 to compute and export strain modes to MNF.

21-25

4th

I

Enter the shell layer: 0: continuum elements. 1: shell top layer. 2: shell middle layer. 3: shell bottom layer.

Main Index

144 SUPER Super Element Input

SUPER

Super Element Input

Description This parameter allows the user to define an upper-bound to the number of degrees of freedom per node when DMIGs are used to define superelements. Format Format Fixed

Main Index

Free

Data Entry Entry

1-5

1st

A

Enter the word SUPER.

11-15

2nd

I

Not used; enter 0.

16-20

3rd

I

Not used; enter 0.

21-25

4th

I

Enter the maximum number of degrees of freedom per node number in any super element.

USER 145 Create User-defined Element

USER

Create User-defined Element

Description You can define your own stiffness or mass matrix using this parameter and user subroutine USELEM to specify equivalent nodal loads, stiffness matrix, mass matrix, stress recovery, and internal force. When using this capability, the element type given on the CONNECTIVITY model definition option and the ELEMENTS parameter is a negative number. This parameter can be used repeatedly to define different element types. For a thermo-mechanically coupled analysis, a user-defined element for the stress pass can be associated with a regular Marc element or a user-defined element for the heat transfer pass. In the latter case, note that USER parameter should be defined for all the user-defined stress elements first followed by USER parameters for the associated heat transfer elements in the same order. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word USER.

11-15

2nd

I

Enter the element type; must be a negative number.

16-20

3rd

I

Number of degrees of freedom per node.

21-25

4th

I

Maximum number of stress quantities to be stored per “integration” point; can be 0.

26-30

5th

I

Number of nodes per element; must be less than 101.

31-35

6th

I

Number of generalized strains; can be 0.

36-40

7th

I

Number of coordinates per node.

41-45

8th

I

Number of integration points per element; can be 0.

46-50

9th

I

Number of direct components of stress; can be 0.

51-55

10th

I

Number of shear components of stress; can be 0.

56-60

11th

I

Enter the element class based upon:

Conventional Marc Element Classes

Main Index

0 = Pipe

8 = 3-D solid (brick, tet)

1 = Truss

9 = Fourier

2 = Shell

10 = Axisymmetric solid with twist

3 = Plate

11 = Axisymmetric shell

4 = Plane stress

12 = Open section beam

146 USER Create User-defined Element

Conventional Marc Element Classes 5 = Plane strain

13 = Closed section beam

6 = Generalized plane strain

14 = Membrane

7 = Axisymmetric solid

15 = Gap

61-65

12th

I

Heat transfer flag; 0 = Stress element 1 = Heat transfer element

66-70

13th

I

Associated heat transfer element if this is a stress element and the analysis is coupled. This can be a positive normal Marc element type or another negative user element type.

71-75

14th

I

Enter the topology class based upon: Conventional Marc Topology Classes

11 = 2-node line (linear)

41 = 4-node tetrahedral (linear)

12 = 3-node line (quadratic)

42 = 5-node tetrahedral (4+1) (linear)

21 = 3-node triangle (linear)

43 = 10-node tetrahedral (quadratic)

22 = 4-node triangle (3+1) (linear+bubble)

51 = 6-node pentahedral

23 = 6-node triangle (quadratic)

52 = 15-node pentahedral

31 = 4-node quadrilateral (linear)

61 = 8-node hexahedral (linear)

32 = 5-node quadrilateral (4+1) Lagrange multiplier)

62 = 9-node hexahedral (8+1) (linear + Lagrange multiplier)

33 = 6-node quadrilateral

63 = 12-node hexahedral

34 = 8-node quadrilateral (quadratic serendipity)

64 = 20-node hexahedral (quadratic - serendipity)

35 = 9-node quadrilateral (8+1) (quadratic Lagrange)

Main Index

Chapter 2: Parameters 147 Additional Flags for Various Analyses

Chapt Additional Flags for Various Analyses er 2: Para meter s

Main Index

148 CENTROID State Storage at Centroid Only

CENTROID

State Storage at Centroid Only

Description This parameter is used for calculation and storage of stress and strain (or, for heat transfer, temperature) at the centroid of each element only. The CENTROID parameter reduces the storage requirements, and the computational costs. However, it is not recommended for nonlinear analysis because it reduces the accuracy of the solution. If this parameter is used, the residual load correction should be switched off by using the NO LOADCOR parameter. Note:

The POST option may be used to specify that output is at the CENTROID while insuring an accurate analysis.

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word CENTROID.

ALL POINTS 149 State Storage at All Points

ALL POINTS

State Storage at All Points

Description This parameter is used for calculation and storage of stress and strain (or, for heat transfer, temperature) at all integration points of all elements. Output is obtained for each integration point of each element. For the integration point locations of Marc elements, see Marc Volume B: Element Library. If this parameter is switched off by the use of the CENTROID parameter, the state at each integration point of the element is set equal to the value at the centroid of the element. This is not important in small displacement elastic solutions and might not be significant where the mesh is very fine. However, the utility of the sophisticated elements lies in the use of integration point data with relatively few elements. Use of this parameter is recommended for any nonlinear analysis, particularly nonlinear shell and large displacement analysis. If this parameter is turned off, the residual load correction should be switched off (using the NO LOADCOR parameter) since an accurate stress distribution is necessary for this correction to be effective. In general, use of this feature increases the run time; however, this parameter allows the use of a coarser mesh, which can result in a lower overall cost for the analysis. Storage requirements are also higher. This also can affect THERMAL LOADS or CHANGE STATE input requirements. Note:

This parameter has the default value of “on” in the K2 and subsequent versions. This parameter has the default value of “off” in all versions previous to K2.

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words ALL POINTS.

150 LOAD COR Residual Load Correction

LOAD COR

Residual Load Correction

Description This parameter is used to ensure that the nonlinear solution is always in equilibrium. In versions subsequent to K2, this was the default option. It is recommended that the ALL POINTS parameter always be used in conjunction with residual load correction. The residual correction depends on integrating stress over the elements, and this can only be accurate if stresses are stored at all points. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words LOAD COR.

NO LOADCOR 151 Suppression of Load Correction

NO LOADCOR

Suppression of Load Correction

Description Residual load correction is automatically included for any analysis. This parameter is used to override any automatic setting. This parameter should be the last parameter given before the END parameter. Note:

Certain parameters (DYNAMIC and LARGE DISP) override this parameter and always turn the load correction on. The use of this parameter should be limited to linear elastic problems.

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words NO LOADCOR.

152 SCALE Scaling to First Yield

SCALE

Scaling to First Yield

Description This parameter causes scaling of the linear-elastic solution to first yield in the highest stressed element, for small displacement elastic-plastic analysis where element properties are not temperature dependent. Using this parameter causes all aspects of the initial solution (displacements, strains, stresses, temperature changes, loads) to be scaled. Thus, subsequent incrementation is built onto the scaled solution; for example, the PROPORTIONAL INCREMENT history definition set proportions the scaled load. Note:

This parameter cannot be used in dynamic, large disp, or coupled analysis.

Format Format Fixed 1-10

Free 1st

Data Entry Entry A

Enter the word SCALE. This entry automatically switches on the load correction. This flag is ignored if large displacement or dynamic analysis is flagged.

Main Index

THERMAL 153 Thermal Stress Analysis

THERMAL

Thermal Stress Analysis

Description This parameter specifies the use of thermal loading or temperature-dependent material properties in the analysis. See THERMAL LOADS, CHANGE STATE, INITIAL TEMP, POINT TEMP, and TEMPERATURE EFFECTS or TABLE model definitions in this document for more information. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word THERMAL.

154 ISTRESS Define Initial Stress

ISTRESS

Define Initial Stress

Description This parameter allows you to input an initial set of stresses. It is your responsibility to input a self-equilibrating set of stresses. These stresses should not produce any material nonlinearity. The stresses are input through the UINSTR user subroutine or through the INIT STRESS model definition option. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word ISTRESS.

11-15

2nd

I

0: Initial stress in element coordinate system (Default) 1: Initial stress in preferred material coordinate system (Default)

Main Index

LUMP 155 Lumped Mass or Specific-Heat Matrix

LUMP

Lumped Mass or Specific-Heat Matrix

Description This parameter lumps the mass matrix (for dynamics) or specific heat matrix (for heat transfer) into a diagonal matrix. Note:

LUMP can also be used for acoustics. However, it tends to lower the eigenfrequencies.

Use of this parameter is not recommended for second order elements (8-node quadrilateral or 20-node brick elements) or for shell type elements. Format Format Fixed

Main Index

Free

Data Entry Entry

1-4

1st

A

Enter the word LUMP.

5-10

2nd

I

If greater than or equal to zero, use lumped mass matrix.

11-15

3rd

I

If greater than zero, does not add mass to rotational degrees of freedom of the following shell elements: 22, 75, 138, 139, 140.

156 APPBC Application of Boundary Conditions

APPBC

Application of Boundary Conditions

Description The APPBC parameter specifies that the application of boundary conditions is performed by row-column elimination, forcing re-assembly if there are any nonzero applied displacements. If this option is not included, boundary conditions are applied using the penalty method. The penalty factor is entered through the PARAMETERS option. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word APPBC.

ACCUMULATE 157 Accumulation of Strain and Displacements

ACCUMULATE

Accumulation of Strain and Displacements

Description This parameter reserves workspace for the storage of accumulated total strains, plastic strains, creep strains, and total displacements. Such accumulated values can be used for purposes of extrapolation in nonlinear creep and/or plasticity analysis. In particular, it can be used in analysis of cyclic loading problems, where from one complete cycle the accumulated strains and displacements can be extrapolated to cover multiple loading cycles. Note:

This parameter must be used with extreme care. Because of the nature of extrapolation, the results can only be considered to be an estimate of the values that would have otherwise been obtained with complete analysis. After an extrapolation, the analysis can be continued in the usual way. See the ACCUMULATE and EXTRAPOLATE options in the history definition section of this manual for more information.

Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word ACCUMULATE.

158 ALIAS Define Aliases

ALIAS

Define Aliases

Description In many cases, you might wish to enter a different element type identification to the library element type given on the ELEMENTS parameter when the mesh is read from the CONNECTIVITY model definition set. A common example is the use of the same mesh for heat transfer and stress analysis. The library element code on the ELEMENTS parameter must be changed, but you might not wish to change the library code on the CONNECTIVITY option. This parameter defines the aliases corresponding to the library element types in this analysis. For example, if a heat transfer analysis is to be done with 4-node, axisymmetric quadrilateral (library code 40) but the mesh has been generated with element code type 10 (the corresponding stress analysis element) the alias is set up as 10 for library code type 40. Format Format Fixed

Free

Data Entry Entry

1-5

1st

A

Enter the word ALIAS.

11-15

2nd

I

Number of aliases to be entered. More than one alias can be used for any one element library code.

16-20

3rd

I

Alias for element library code (the type given on the CONNECTIVITY option).

21-25

4th

I

Actual library code for the above alias (the type given on the ELEMENTS parameter and the one to be used in the analysis). Etc.

Note:

Main Index

Alias correspondence pairs are continued in fields of I5 to column 75. Continuation blocks, if needed, are given in 16I5 format.

Chapter 2: Parameters 159 Program Function and I/O Controls

Chapt Program Function and I/O Controls er 2: Para meter s

Main Index

160 NEW Use New Format

NEW

Use New Format

Description This parameter can be used to switch from input in extended format to the default width or vice-versa. Input is interpreted to be in the format defined here until another NEW option is encountered. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word NEW.

11-15

2nd

I

Enter 1 if the default width of the data fields is used for input. This overrides the EXTENDED parameter. Enter 2 if the double width of the data fields is used for input.

Main Index

TABLE 161 Indicate How Tables are to be used

TABLE

Indicate How Tables are to be used

Description This option defines how many tables are included in the input data, and how are they to be used. Tables may currently be used for defining nonlinear material behavior, and boundary conditions and contact data. Format Format Fixed

Free

Data Entry Entry

1-5

1st

A

Enter the word TABLE.

6-10

2nd

I

Enter the maximum number of tables in model.

11-15

3rd

I

Enter the maximum number of data points associated with a table.

16-20

4th

I

Enter 0 if old style input is used for: FIXED DISP, etc. POINT LOAD, etc. DIST LOADS, etc. FOUNDATION or FILMS option

Enter 2 if new style input is used for: FIXED DISP, etc. POINT LOAD, etc. DIST LOADS, etc. FOUNDATION or FILMS option

21-25

5th

I

Enter 0 if old style input is used for: ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, MOONEY, OGDEN, FOAM, HYPOELASTIC, GENT, ARRUDBOYCE options.

Enter 1 if new style input is used for: ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, MOONEY, OGDEN, FOAM, HYPOELASTIC, GENT, ARRUDBOYCE options.

26-30

6th

I

Enter 0 if old style input is used for CONTACT option. Enter 1 if new style input is used for CONTACT option.

Main Index

162 COMMENT Define Comment

COMMENT

Define Comment

Description The COMMENT parameter is used to enter informative comments. This parameter can be used as often as desired within the model definition and history definition options. Use of this parameter does not affect the analysis. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word COMMENT.

11-80

2nd

A

User-entered comment.

Alternate Format Format Fixed

Main Index

Free

Data Entry Entry

1-1

1st

A

Enter the $ character.

3-80

2nd

A

User-entered comment.

PRINT 163 Debug Printout

PRINT

Debug Printout

Description This parameter allows printout of various items for debugging; however, the amount of output is increased accordingly. Default is no check printout. Multiple print flags can be set using columns 11 to 80. Format Format Fixed

Free

Data Entry Entry

1-5

1st

A

Enter the word PRINT.

11-80

2nd

I

Enter as many print codes as required. Enter 1 for output of element stiffness matrices (this also prints out the shell surface metric for doubly curved shells 4, 8, and 24), consistent mass matrix, and equivalent nodal loads. Caution: This produces significant output. Enter 2 for output of the matrices used in tying. (See TYING, SERVO LINK, UFORMS.)

Enter 3 to force the solution of a nonpositive definite matrix. This is only recommended for the AUTO INCREMENT option to pass collapse points in the collapse analysis. This can be entered on the CONTROL option. Enter 5 to obtain additional information concerning gap convergence. In contact analysis, set to 5 to obtain information concerning nodes touching or separating from surfaces and also to print out the maximum residual and reaction forces. Enter 6 to obtain output of nodal value array during rezoning. Enter 7 to obtain tying information in CONRAD GAP option and fluid element numbers in CHANNEL option which is used to define fluid channel input data in heat transfer analysis. Enter 8 to obtain incremental displacements in local system in contact problems. Enter 9 to obtain latent heat output. Enter 10 to obtain the stress-strain relation in the local coordinate system. Enter 11 to obtain additional information on the interlaminar stress calculation. Enter 12 to output the right-hand side and solution vector. Caution: This produces significant output.

Main Index

164 PRINT Debug Printout

Format Fixed

Free

Data Entry Entry Enter 13 to obtain additional information regarding CPU resources used. Enter 14 to obtain information regarding the mesh adapting process. Enter 15 to obtain additional information regarding surface energy balances. Enter 16 to obtain additional information regarding pyrolysis calculation. Enter 17 to obtain additional information regarding creation of streamlines. Enter 18 to obtain information about rezoning when using ADAPT GLOBAL option.

Enter 20 to obtain information regarding the evaluation of tables. Enter 21 to obtain information about application of kinematic boundary conditions when table input is used. Enter 22 to obtain information about distributed loads, point loads, films, foundations, and initial conditions when table input is used. Enter 23 to obtain information about ablation deformation. Enter 24 to print internal heat generated in coupled analysis. Enter 25 to print additional information regarding remeshing during ablation. Enter 26 to print additional information regarding sink points. Enter 27 to obtain reaction forces at tied nodes. Enter 28 to obtain additional information about convective terms in heat transfer and fluid analysis. Enter 29 to obtain additional information on the internal created domains (not supported yet). Enter 30 to obtain information on cavity pressure loading. Enter 31 to obtain information about the welding process. The total weld heat input for each weld flux and the filler element creation history are printed. Enter 33 to obtain nodes and elements that are cut. Enter 34 to print a description of what independent variables may be used with a physical quantity. Enter 35 to obtain detailed information on every call to a coupling region API routine (see Marc Volume D: User Subroutines and Special Routines, Chapter 12: Code Coupling Interface) Enter 36 to obtain CASI solver debug information (has the least details).

Main Index

PRINT 165 Debug Printout

Format Fixed

Free

Data Entry Entry Enter 37 to obtain CASI solver debug information (has more details). Enter 38 to obtain CASI solver debug information (has the most details). Enter 39 to obtain detailed information about memory allocation. Enter 40 to obtain information about Marc-Adams integration. Enter 42 to create a step on the post file containing the rezoned model before the next increment of the analysis. Enter 43 to obtain information about VCCT. Enter 44 to obtain information during progressive failure. Enter 46 to obtain information as to what subroutine caused the fatal error.

Main Index

166 STOP Exit following Workspace Allocation

STOP

Exit following Workspace Allocation

Description For large problems, you might desire to see the exact sizing requirements for running a job without actually executing the analysis. The insertion of this parameter causes Marc to exit normally following workspace allocation. The solution space allocated is based on the optimized bandwidth if you request the OPTIMIZE option in the model definition section. This is not the total memory required in the case of the hardware provided solver (solver type 6) or the CASI iterative solver (solver type 9). Format Format Fixed 1-4

Main Index

Free 1st

Data Entry Entry A

Enter the word STOP.

NOTES 167 Print Notes and Updates

NOTES

Print Notes and Updates

Description This parameter provides detailed, updated information about Marc (manual update, new program features, etc.) Format Format Fixed 1-5

Main Index

Free 1st

Data Entry Entry A

Enter the word NOTES.

168 INPUT TAPE Specify Device for Model Definition Data

INPUT TAPE

Specify Device for Model Definition Data

Description This parameter allows specification of a storage device which contains previously generated CONNECTIVITY and COORDINATES model definition data. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the words INPUT TAPE.

11-15

2nd

I

Unit number for main input of coordinates and connectivity. Default is unit 5. For larger problems, involving out-of-core options, you should avoid using unit 2, 3, 11, 12, 13, 14, or 15 for mesh input.

Main Index

ELSTO 169 Out-of-Core Storage of Elements

ELSTO

Out-of-Core Storage of Elements

Description This parameter is used to save core storage for large problems. All element quantities, strains, stresses, etc. are stored on an auxiliary storage device. If the number of words actually required is less than the buffer specified below, this option is turned off by Marc. Format Format FixeD

Free

Data Entry Entry

1-10

1st

A

Enter the word ELSTO. This stores element arrays on unit 3.

11-15

2nd

I

Buffer size for out-of-core element storage. The default is 40960 words. This buffer size is usually adequate unless shell elements are used with a large number of layers.

Main Index

170 OOC Out-of-core Solver

OOC

Out-of-core Solver

Description This parameter is used to indicate that the global stiffness matrix is assembled using auxiliary disk space and will not reside in memory. This is available for solver types 0, 2, 4, 8, and 9 only. It can be used to save memory. Additionally, for solver types 0 and 4, this parameter controls the decomposition of the matrix. Normally, Marc automatically switches to the out-of-core solver only when it is unable to dynamically allocate any more space, and the system is unable to fit into the real/virtual memory available. For solver type 8, Marc automatically switches to the out-of-core assembly when there is inadequate memory for the decomposition. Format Format FixeD

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word OOC.

11-15

2nd

I

Not used; enter 0.

16-20

3rd

I

Enter 1 to further reduce memory requirements. Available only for solver type 8. In this case, the memory needed for the nodal vectors will be partly used by the direct solver. Furthermore, the memory for the direct solver will be limited to almost the minimum needed by that solver. This will reduce the memory but might increase the I/O time.

IBOOC 171 Out-of-core Storage of Incremental Backup Data

I

IBOOC

Out-of-core Storage of Incremental Backup Data

Description During the Newton-Raphson iteration process, Marc makes a second copy of the solution space. Marc normally does this in memory unless sufficient memory is not available; in which case, it uses auxiliary disk space. This option can be used to force it to use disk space (file jobname.t29). This is often useful for large problems when the sparse solver (type 0) or the multifront sparse solver (type 8) is used, as this back-up copy is allocated before the decomposition memory is allocated. If the solver has insufficient memory to perform its function, the job fails prematurely. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word IBOOC.

172 NO ECHO Suppress Echo

NO ECHO

Suppress Echo

This parameter is used to limit echoing of certain input data to the output file during reading. Different codes are used to suppress different things. Format Format Fixed

Free

Data Entry Entry

1-7

1st

A

Enter the words NO ECHO.

11-80

2nd

I

Up to 19 codes in I5 or I10 format. Enter 1 to suppress echo on node and element lists. Only one line and a summary of the number of lines read are printed. Enter 2 to suppress echo of boundary condition summary. Only the number of boundary conditions is printed. Enter 3 to suppress echo of NURBS data. Enter 4 to suppress information about coordinate systems.

Main Index

INCLUDE 173 Insert File into the Input File

INCLUDE

Insert File into the Input File

Description Inserts an external file into the input file. The include statement may appear in either the parameter, model definition, or history definition section. In Marc, an include file may reference another include file up to a level of 10 deep. The total length of the file name, including the directory path is limited to 240 characters. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word INCLUDE.

11-80

2nd

A

Physical filename. If the file name is specified without a path, the file should be in the same directory as the input file. If a path is given, the file should be in the path relative to the current working directory. Also, note that the file name is case sensitive and blanks should not be included in the name.

Main Index

174 INCLUDE Insert File into the Input File

Main Index

Chapter 2: Parameters 175 Modifying Default Values

Modifying Default Values Chapter 2: Parameters

Main Index

176 STATE VARS Define Number of State Variables

STATE VARS

Define Number of State Variables

Description This parameter allows consideration of state variables in addition to that of temperature. The number of predefined state variables stored at each point of the structure can be increased from the default of one (temperature for heat transfer and lubricant pressure for bearing analysis) by the use of this parameter. In addition, additional storage can be allocated for user-defined global scalar quantities. For more information, see THERMAL LOADS, INITIAL STATE, or CHANGE STATE model definition data in this document and CREDE or NEWSV user subroutine in Marc Volume D: User Subroutines and Special Routines. Note:

In bearing analysis, the first state variable equals the lubricant pressure. For this reason, the number of state variables must be set to 2 if viscosity varies with temperature in this type of analysis.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the words STATE VARS.

11-15

2nd

I

Number of state variables to be stored per point.

16-20

3rd

I

Number of global variables to be stored.

DIST LOADS 177 Distributed Loads or Point Loads

DIST LOADS

Distributed Loads or Point Loads

Description This parameter allows for the input of the maximum number of different lists of distributed loads, the maximum number of elements in any particular distributed load list, and the maximum number of nodes with point loads applied. This parameter is only necessary if the number of different lists of distributed loads, or the maximum number of elements per list, or the number of point loads is increased in the history definition section. Note:

This parameter is not required if the table driven boundary conditions are used.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the words DIST LOADS.

11-15

2nd

I

Maximum number of different lists of distributed loads. The default is 3.

16-20

3rd

I

Maximum number of elements in any particular distributed load list.

21-25

4th

I

Enter the maximum number of nodes with point loads applied.

178 FLUXES Distributed Fluxes or Point Fluxes

FLUXES

Distributed Fluxes or Point Fluxes

Description This parameter allows for the input of the maximum number of different lists of distributed fluxes, the maximum number of elements in a particular distributed flux list, and the maximum number of nodes with point fluxes applied. This parameter is only necessary unless the number of different lists of distributed fluxes, or the maximum number of elements per list, or the number of point fluxes is increased in the history definition section. Note:

This parameter is not required if the table driven boundary conditions are used.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-6

1st

A

Enter the word FLUXES.

11-15

2nd

I

Maximum number of different lists of distributed fluxes. Default is 3.

16-20

3rd

I

Maximum number of elements in any particular distributed flux list.

21-25

4th

I

Enter the maximum number of nodes with point fluxes applied.

FILMS 179 Film Coefficients

FILMS

Film Coefficients

Description This parameter allows for the input of the maximum number of elements that have films. This parameter is only needed if the number of elements with films is increased in the history definition section. Note:

This parameter is not required if the table driven boundary conditions are used.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word FILMS.

11-15

2nd

I

Maximum number of elements that have films.

180 RESTRICTOR Restrictor Input in Lubrication Analysis

RESTRICTOR

Restrictor Input in Lubrication Analysis

Description This parameter must be included to allow the use of restrictors in lubrication analysis. See the RESTRICTOR model definition option section of this document for more information. Note:

This parameter is not required if the table driven boundary conditions are used.

Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word RESTRICTOR.

11-15

2nd

I

Number of element surfaces for which restrictor conditions are imposed.

WELDING 181 Welding Analysis

WELDING

Welding Analysis

Description This parameter can be used to define the maximum number of weld fluxes in the model and other related maximum quantities for welding processes. This parameter is recommended, in general, for any welding analysis, but is particularly required if the number of weld fluxes, weld paths, weld fillers and other related quantities are increased in the history definition section. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word WELDING.

11-15

2nd

I

Enter an upper bound to the number of welding heat sources.

16-20

3rd

I

Enter an upper bound to the number of elements associated with any weld heat source.

21-25

4th

I

Enter an upper bound to the number of weld paths.

26-30

5th

I

Enter an upper bound to the number of weld fillers.

31-35

6th

I

Enter an upper bound to the number of elements associated with any weld filler.

36-40

7th

I

Enter an upper bound to the number of curves associated with any weld path. This is set to 1 by the program if left undefined.

41-45

8th

I

Enter an upper bound to the number of points associated with any weld path curve. This is set to 2 by the program is left undefined.

182 BOUNDARY CONDITIONS Specify Maximum Number of Boundary Conditions to be Defined

BOUNDARY CONDITIONS

Specify Maximum Number of Boundary Conditions to be Defined

Description This option allows the user to specify the maximum number of boundary conditions (FIXED DISP., etc., DIST LOADS, etc., POINT LOAD, etc., FILMS or FOUNDATION) labels to be given. If all boundary conditions are specified before the END OPTION, this is not necessary. This is only necessary if the table driven style input is used for defining boundary conditions. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word BOUNDARY.

11-15

2nd

I

Enter the maximum number of boundary condition ids.

SHELL SECT 183 Define Number of Layer Through Shell Thickness

SHELL SECT

Define Number of Layer Through Shell Thickness

Description By default, all the shell and beam-in-a-plane elements in Marc use a Simpson rule for integration through the cross section. This numerical integration allows any material behavior at each layer; for example, the yielding of a nonlinear elastic-plastic shell can be followed through the section, from a fully elastic to a fully plastic section. The density of integration points through the thickness is chosen with this parameter. For purely linear material behavior, 1 point (the minimum) is required for exact integration across the section. For most nonlinear problems, 7 points are sufficient to describe the nonlinear material response exactly. For extremely nonlinear response, such as elastic-plastic dynamic problems, 11 points might be needed. The default if this parameter is not used is 11 points. If the COMPOSITE option is used for a group of elements, it controls the number of layers used, and the integration is performed using the trapezoidal rule. This option (4th field) may be used to control the procedure which can improve computational performance but limit materials selection. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the words SHELL SECT.

11-15

2nd

I

Number of points across the section for Simpson rule integration of stresses. The default is 11; minimum is 1. Must be an odd number.

16-20

3rd

I

Enter 1 if you are going to perform your own integration through the shell/beam thickness. This requires you to input a generalized stress-strain law through the GENSTR user subroutine.

21-25

4th

I

Enter the default method for integrating through the thickness of composite shell elements. If a value is given on the COMPOSITE option, it will be used for that particular material. Enter 1 (default) for conventional procedure, which supports all material behavior available for composite elements. Enter 2 if stiffness is to be fast-integrated through the thickness based upon classical laminate theory. This reduces the memory requirements and computational costs for elastic shells. Thermal strains and temperature dependent properties are not supported. Enter 3 if stiffness is to be fast-integrated through the thickness based upon classical laminate theory. This reduces the memory requirements and computational costs for elastic shells. This procedure uses more memory and computational time than method 2.

Main Index

184 TSHEAR Transverse Shear for Elements 22, 45, 75, 140, and 185

TSHEAR

Transverse Shear for Elements 22, 45, 75, 140, and 185

Description The default distribution of transverse shear strain through the thickness for thick shell element types 22, 75, and 140, and for thick beam 45, is a constant. With the inclusion of the TSHEAR parameter, a more parabolic beam-like distribution derived from a strength-of-materials approach is used. This distribution is exact for beam 45 but is only approximate for shells 22, 75, or 140 since it is based on the assumption that the stresses in perpendicular directions are independent of each other. For unstacked solid shell element, type 185, and 3D composite brick elements, type 149 and 150, the inclusion of the TSHEAR parameter results in an improved transverse shear distribution. For solid shell elements, if not used as a composite material, the shear correction factor should be entered in the GEOMETRY option. The interlaminar shear is printed only if the PRINT ELEMENT option is used. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word TSHEAR.

TIE 185 Define Tying Data

TIE

Define Tying Data

Description This allocates storage for tying data. See TYING and SERVO LINK model definition options in Chapter 3 of this manual. Also see the UFORMSN user subroutine in Marc Volume D: User Subroutines and Special Routines. This parameter is necessary only if TYING CHANGE is used to increase the number of constraints. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word TIE.

11-15

2nd

I

Not used; enter 0.

16-20

3rd

I

Not used; enter 0.

21-25

4th

I

Maximum number of retained nodes plus one involved in any tying type or servo link constraint.

26-30

5th

I

Not used; enter 0.

186 MPC-CHECK Multi-point Constraint Checking Parameter

MPC-CHECK

Multi-point Constraint Checking Parameter

Description This parameter allows the user to specify the amount of checking and ordering done by the program during the application of multi-point constraints arising from the model definition options: CONTACT, CYCLIC SYMMETRY, INSERT, RBE2, RBE3, SERVO LINK, and TYING. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the words MPC-CHECK.

11-15

2nd

I

1: Apply the MPCs in the default order: 1. MPCs obtained from SERVO LINK option. 2. MPCs obtained from INSERT option. 3. MPCs obtained from TYING, RBE2, or RBE3 options (the actual order follows from the order of these options in the model definition block of the data file). 4. MPCs obtained from CYCLIC SYMMETRY option. 5. MPCs obtained from CONTACT option. Print a warning message if a tied degree of freedom is being used by a subsequent MPC. 2: Same as 1, but instead of warning, a fatal error message is printed and the analysis will stop with exit 2011. 3: Try to rearrange the MPCs in such a way that a tied degree of freedom will not be used in a subsequent MPC. If this reordering cannot successfully be completed, print a fatal error message and stop the analysis with exit 2011. If the MPC-CHECK parameter is not present in the input file: For Version 10 or earlier, default is 1. For Version 11, default is 3.

Main Index

AUTOMSET 187 Modify Relationship Between Tied and Retained Nodes

AUTOMSET

Modify Relationship Between Tied and Retained Nodes

Description Without this option, a tied degree of freedom cannot be used as a tied degree of freedom in other tying constraints nor can it be used as a fixed degree of freedom in a single point constraint (for example, FIXED DISP/FIXED TEMPERATURE). When this option is used, the above is allowed as long as the number of constraints is not larger than the number of degrees of freedom. The program re-writes the tying constraint equation so that one of the retained degrees of freedom becomes the tied degree of freedom. If this option is activated, the MPC-CHECK parameter is ignored. Format Format Fixed

Free

1-10

1st

Data Entry Entry A

Enter the word AUTOMSET.

Examples Example 1 Xdisplacement of node 3 is tied to Xdisplacements of node 1 and node 2: Ux(3) = 0.5 * Ux(1) + 0.5 * Ux(2) Xdisplacement of node 3 is fixed to be 0.1: Ux(3) = 0.1 Without the AUTOMSET option, this is not allowed; with the AUTOMSET option, these two constraints are rewritten as: Ux(1) = 2*Ux(3) - Ux(2) Ux(3) = 0.1 Example 2 Xdisplacement of node 3 is tied to Xdisplacement of node 1 and node 2: Ux(3) = 0.5 * Ux(1) + 0.5 * Ux(2) Xdisplacement of node 3 are tied to Xdisplacement of node 4: Ux(3) = Ux(4) Xdisplacement of node 3 is fixed to be 0.1: Ux(3) = 0.1

Main Index

188 AUTOMSET Modify Relationship Between Tied and Retained Nodes

Without the AUTOMSET parameter, this is not allowed; with the AUTOMSET parameter, these two constraints are rewritten as: Ux(1) = 2*Ux(3) - Ux(2) Ux(4) = Ux(3) Ux(3)=0.1 The parameter is effective for constraints generated by the following options: TYING SERVO LINK RBE2 RBE3 RROD CONRAD GAP

It is not active for constraints generated by the following options: INSERT CONTACT INERTIA RELIEF

Main Index

AUTOSPC 189 Automatically Apply Constraints to Eliminate Rigid Body Modes

AUTOSPC

Automatically Apply Constraints to Eliminate Rigid Body Modes

Description The AUTOSPC option applies a constraint to multiple degrees of freedom to eliminate rigid body modes in the structure. This procedure can only be used with the direct solvers. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word AUTOSPC.

190 IO-DEACTIVATE Deactivate Element if it goes Inside-out

Chap IO-DEACTIVATE

Deactivate Element if it goes Inside-out

Description This parameter will result in the simulation continuing even if an element goes inside-out due to large deformation or material instability. The element that has gone inside-out will be deactivated from the model. This option is intended for use with damage models where the reduced stiffness of the element may result in these difficulties. It should be used with caution in the simulation, and it should be recognized that this will result in a decrease in mass in the system. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word IO-DEACT.

ter 2: Parameters 191 Defining Cross-sections of Beam Elements

ter 2: Defining Cross-sections of Beam Elements Para meter s

Main Index

192 BEAM SECT Beam Section Definition

BEAM SECT

Beam Section Definition

Description This parameter is used to define the sectional properties of beam sections used in the analysis. The format and exact data entered depends upon which elements are used. Formats for all available Marc beam elements are shown below. This parameter must be included if element 13, 77, or 79 is used, if 14, 25, 31, 76, or 78 is used with a noncircular section, or if element 52 or 98 is used with a nonprismatic section or if element 52 or 98 is used with numerical section integration. See Marc Volume B: Element Library for more information about individual elements. If used, the BEAM SECT parameter must directly follow the SIZING and ELEMENTS parameters. Each beam section used in the analysis must then be described. A LAST statement must follow the last beam section description to complete the BEAM SECT parameter definition. There are four methods in this option to define the beam cross section properties: a. For thin section open and closed beams b. Elastic non-integrated element types 31, 52, and 98 c. Numerically integrated standard solid section d. Numerically integrated non-standard solid section Format Format Fixed

Free

Data Entry Entry

For all beam elements, use the 1st and last data blocks described below. 1st data block 1-10

1st

A

Enter the words BEAM SECT.

. .

(Include all beam section definitions here.)

. Last data block 1-10

1st

A

Enter the word LAST.

Method A For elements 13, 14, 25, and 76 to 79, use data blocks 2a, 3a, 4a, 5a to define each beam section: 2a data block 1-10

Main Index

1st

A

Descriptive title of beam section.

BEAM SECT 193 Beam Section Definition

Format Fixed

Free

Data Entry Entry

3a data block for elements 13, 14, 25, and 76 - 79 1-5

1st

I

Number of branches used to input section.

6-10

2nd

I

Number of divisions in first branch. Must be an even number.

11-15

3rd

I

Number of divisions in second branch. Must be an even number.

Etc.

Etc.

I

Etc.

Note that a beam section consisting of one straight branch has no stiffness against rotation along the branch direction. Data blocks 4a and 5a are given one pair per branch. (X, Y, and S are coordinates on the cross-section face.) See Marc Volume B: Element Library. Note that a branch with zero thickness does not contribute to the stiffness but is used to ensure that the branches form a connected path for open section beams. 4a data block 1-10

1st

F

X-Coordinate of beginning of branch.

11-20

2nd

F

Y-Coordinate of beginning of branch.

21-30

3rd

F

DX/DS at beginning of branch.

31-40

4th

F

DY/DS at beginning of branch.

41-50

5th

F

X-Coordinate of end of branch.

51-60

6th

F

Y-Coordinate of end of branch.

61-70

7th

F

DX/DS at end of branch.

71-80

8th

F

DY/DS at end of branch.

5a data block 1-10

1st

F

Length of branch.

11-20

2nd

F

Thickness of beginning branch.

21-30

3rd

F

Thickness of end branch. Default to thickness at beginning if left zero.

Method B For elastic non-integrated element types 31, 52, or 98, use data blocks 2b and 3b formats to define each beam section. 2b data block 1-10

1st

A

Descriptive title of section.

3b data block for element type 31, 52, or 98

Main Index

1-5

1st

I

Enter 0.

6-15

2nd

F

Area of cross section A.

16-25

3rd

F

Ixx Moment of inertia about local x-axis.

194 BEAM SECT Beam Section Definition

Format Fixed

Free

Data Entry Entry

26-35

4th

F

Iyy Moment of inertia about local y-axis.

36-45

5th

F

K Torsional stiffness factor. The torsional stiffness is calculated as EK --------------------2(1 + ν)

46-55

6th

F

A xs

.

Effective transverse shear area in x-direction (only applies to element

31 and 98). Default A xs = A.

56-65

7th

F

Effective transverse shear area in y-direction (only applies to element 31 and 98). Default A ys = A. A ys

Method C For elements 52 and 98 using the standard numerically integrated sections, use data blocks 2c, 3c, 4c, and 5c to define the beam section: 2c data block 1-10

1st

A

Descriptive title of beam section.

3c data block 1-5

1st

I

Enter 0 for the standard cross-section shapes (i.e., elliptical, rectangular, trapezoidal, or hexagonal).

6-15

2nd

F

Enter N sec t for the cross-section type. The negative value indicates the section is numerically integrated. The value is entered as a real number.

16-25

Main Index

3rd

F

N sec t

= -1 for an elliptical section

N sec t

= -2 for a rectangular section

N sec t

= -3 for a trapezoidal section

N sec t

= -4 for a hexagonal section

Enter a, the first dimension defining the cross section. if

N sec t

= -1: a is the diameter of the circle or the length of the ellispe in local x.

if

N sec t

= -2: a is the length of the square or the rectangle in local x.

if

N sec t

= -3: a is the width of the trapezoid in local x on minus local y side.

if

N sec t

= -4: a is the width of the hexagon in local x at y = 0.

BEAM SECT 195 Beam Section Definition

Format Fixed 26-35

36-45

Free 4th

5th

Data Entry Entry F

F

Enter b, the second dimension defining the cross-section. The default is a when blank or zero. if

N sec t

= -1: b is the height of the ellipse in local y.

if

N sec t

= -2: b is the height of the rectangle in local y.

if

N sec t

= -3: b is the height of the trapezoid in local y.

if

N sec t

= -4: b is the height of the hexagon in local y.

Enter c, the third dimension defining the cross section. The default is zero when blank. if

N sec t

= -1: c is not used. Leave blank or enter 0.

if

N sec t

= -2: c is not used. Leave blank or enter 0.

if

N sec t

= -3: c is the width of the trapezoid in local x on the plus local y side.

if

N sec t

= -4: c is the width of the hexagon in local x on either local y side.

4c data block 1-5

1st

I

For an elliptical section, enter the number of subdivisions in radial direction. The default is 3. For a rectangular or trapezoidal section, enter the order of the integration rule used in local x-direction. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is 5 and the order cannot be larger than 10. For a hexagonal section, enter the order of the integration rule used in local x-direction over each trapezoidal half. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is 5 and the order cannot be larger than 10.

6-10

2nd

I

For an elliptical section, enter the number of subdivisions in circumferential direction of a 90° sector. The default is 2. For a rectangular or trapezoidal section, enter the order of the integration rule used in local y-direction. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is what was entered in the first field and the order cannot be larger than 10.

Main Index

196 BEAM SECT Beam Section Definition

Format Fixed

Free

Data Entry Entry For a hexagonal section, enter the order of the integration rule used in local y-direction over each trapezoidal half. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is half the order in x-direction plus 1 and the order cannot be larger than 10. For non-Gauss rules, the points in the top row of the lower trapezoid coinciding with the points in the bottom row of the upper trapezoid (i.e., the points coinciding at y = 0) are merged together.

11-15

3rd

I

Enter one if the section is to be treated as a pre-integrated section. The default, when blank or zero, is not to treat it as a pre-integrated section and use numerical integration throughout the analysis. If a one is entered in this field, the input in the 1st and the 2nd field of this data block is ignored.

16-20

4th

I

Not used; leave blank or enter 0.

21-30

5th

F

Enter the normal stiffness factor

31-40

6th

F

Enter the bending stiffness factor

f2

for bending about local x.

41-50

7th

F

Enter the bending stiffness factor

f3

for bending about local y.

61-70

8th

F

Enter the shear stiffness factor

f4

for shear in local x.

71-80

9th

F

Enter the shear stiffness factor

f5

for shear in local y.

51-60

10th

F

Enter the torsional stiffness factor

f1 .

f6 .

Stiffness factors default to 1 when left blank or entered as 0. Entered stiffness factors must be positive 5c data block 1-10

1st

F

For a uniform change in cross section, enter the effective Poisson’s ratio. The default is zero when left blank. This datum is not used at this time and its value will be ignored.

Not more than 100 integration points can exist in any cross section. Note that pre-integrated sections do not allow746+5 stress and strain output in section integration points; only generalized stresses and strains can be requested for output. Method D For elements 52 and 98 using the more general numerically integrated sections that use quadrilateral segments as building blocks, use data blocks 2d, 3d, 4d, and 5d to define the beam section. 2d data block 1-10

Main Index

1st

A

Descriptive title of beam section.

BEAM SECT 197 Beam Section Definition

Format Fixed

Free

Data Entry Entry

3d data block 1-5

1st

I

Enter – N seg , the negative of the number of quadrilateral shaped segments. The negative number indicates the section is solid.

6-10

2nd

I

Enter the order of the integration rule used for each quadrilateral shaped segment in parametric ξ -direction. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is 5 and the order cannot be larger than 10.

11-15

3rd

I

Enter the order of the integration rule used for each quadrilateral shaped segment in parametric η -direction. If the number is positive and odd, a Simpson rule is used. If the number is positive and even, a Newton-Cotes rule is used. If the number is negative, a Gauss rule is used. The default is the same rule and order as in parametric ξ -direction and the order cannot be larger than 10.

16-20

4th

I

Enter a one if the section is to be treated as a pre-integrated section. The default, when blank or zero, is not to treat it as a pre-integrated section and use numerical integration throughout the analysis. If a 1 is entered in this field, the input in the 2nd and the 3rd field of this data block is ignored.

21-30

5th

F

Enter the normal stiffness factor

31-40

6th

F

Enter the bending stiffness factor

f2

for bending about local x.

41-50

7th

F

Enter the bending stiffness factor

f3

for bending about local y.

61-70

8th

F

Enter the shear stiffness factor

f4

for shear in local x.

71-80

9th

F

Enter the shear stiffness factor

f5

for shear in local y.

51-60

10th

F

Enter the torsional stiffness factor

f1 .

f6 .

Stiffness factors default to 1 when left blank or entered as 0. Entered stiffness factors must be positive Enter the 4d data block

N seg

times as follows (i.e., one data block for each quadrilateral segment.

4d data block

Main Index

1-10

1st

F

x-coordinate of the first corner of the segment.

11-20

2nd

F

y-coordinate of the first corner of the segment.

21-30

3rd

F

x-coordinate of the second corner of the segment.

31-40

4th

F

y-coordinate of the second corner of the segment.

41-50

5th

F

x-coordinate of the third corner of the segment.

198 BEAM SECT Beam Section Definition

Format Fixed

Free

Data Entry Entry

51-60

6th

F

y-coordinate of the third corner of the segment.

61-70

7th

F

x-coordinate of the fourth corner of the segment.

71-80

8th

F

y-coordinate of the fourth corner of the segment.

The corners are given in counterclockwise order with respect to the local x-y axis. 5d data block 1-10

1st

F

For a uniform change in cross section, enter the effective Poisson’s ratio. Default is zero when left blank. This data is not used at this time and its value will be ignored.

11-15

2nd

I

Enter 1 to have the principal axis associated with the largest area moment of inertia to be aligned with the local x-axis. Enter 2 to have the principal axis associated with the smallest area moment of inertia to be aligned with the local x-axis. Enter 3 to have the x-axis of the coordinate system for which the section is being defined to be aligned with the local x-axis is given in the GEOMETRY option. Default is 3 when left blank or zero.

16-25

3rd

F

Enter the x-coordinate of a point that, when projected, lies on the positive side of the local x-axis. If the principal moments of inertia are equal, this defines the x-coordinate of a point on the positive local x-axis. This coordinate defaults to X cg + 1 , where X cg is the x-coordinate of the center of gravity of the section in the coordinate system in which the section was entered. The default is used when this field is blank or zero or when the user point coincides with the center of gravity.

26-35

4th

F

Enter the y-coordinate of a point that, when projected, lies on the positive side of the local x-axis. If the principal moments of inertia are equal, this defines the y-coordinate of a point on the positive local x-axis. This coordinate defaults to Y cg , where Y cg is the y-coordinate of the center of gravity of the section in the coordinate system in which the section was entered. The default is used when this field is blank or zero or when the user point coincides with the center of gravity.

Not more than 100 integration points can exist in any cross section. Note that pre-integrated sections do not allow stress and strain output in section integration points; only generalized stresses and strains can be requested for output. A section not pre-integrated cannot have more than 100 segments; using single point integration each. For pre-integrated sections, there is no limit on the number of segments.

Main Index

Chapter 3 Model Definition Options List

3

Model Definition Options List

Model Dedinition Option ACOUSTIC (with TABLE Input - Acoustic)

1219

ACOUSTIC

1220

ACTUATOR

293

ADAPT GLOBAL

260

ADAPTIVE

252

ANISOTROPIC (Mechanical)

736

ANISOTROPIC (Thermal)

1092

ANISOTROPIC (with TABLE Input - Diffusion)

1182

ANISOTROPIC (with TABLE Input - Mechanical) ANISOTROPIC (with TABLE Input - Thermal)

Main Index

Page

729 1089

ARRUDBOYCE (with TABLE Input)

751

ARRUDBOYCE

755

ATTACH EDGE

286

ATTACH FACE

287

ATTACH NODE

284

AXITO3D

525

200

Model Dedinition Option B2GG, B2PP

376

BACKTOSUBS

378

B-H RELATION (Electromagnetic)

1323

B-H RELATION (Magnetostatic)

1290

BLOCKS

213

BOUNDARY

217

BUCKLE INCREMENT

997

CASE COMBIN

390

CAVITY DEFINITION

1112

CAVITY

520

CFAST

340

CHANGE PORE

946

CHANGE PORE (with TABLE Input)

944

CHANGE STATE

554

CHANGE STATE (with TABLE Input)

550

CHANNEL

Main Index

Page

1107

COEFFICIENT

382

COHESIVE (with TABLE Input)

884

COHESIVE

887

COMPOSITE

878

CONM1

986

CONM2

992

CONN FILL

234

CONN GENER

235

CONNECT

223

CONNECTIVITY

232

CONRAD GAP

1106

CONSTRAINT

220

CONTACT (2-D)

623

CONTACT (3-D)

649

CONTACT NODE

687

CONTACT TABLE

672

Chapter 3 Model Definition Options List 201

Model Dedinition Option CONTACT TABLE with TABLES

663

CONTACT with TABLES (2-D)

611

CONTACT with TABLES (3-D)

633

CONTROL (Electromagnetostatic)

1327

CONTROL (Fluid)

1353

CONTROL (Fluid-Solid)

1356

CONTROL (Heat Transfer)

1103

CONTROL (Hydrodynamic)

1196

CONTROL (Magnetostatic)

1296

CONTROL (Mechanical) CONVERT

474 1105

COORD SYSTEM

297

COORDINATES

238

CORNERING AXIS

517

COUPLING REGION

Main Index

Page

1332

CRACK DATA (with TABLE Input)

838

CRACK DATA

840

CREEP (with TABLE Input)

955

CREEP

958

CURE RATE

1122

CURE SHRINKAGE

1129

CURVES

271

CWELD

345

CYCLIC SYMMETRY

306

CYLINDRICAL

249

DAMAGE

869

DAMPING

974

DEACT GLUE

688

DEACTIVATE

385

DEFINE (Mesh2D Block Type)

214

DEFINE (Sets)

229

DELAMINATION

583

202

Model Dedinition Option DENSITY EFFECTS

914

DESIGN DISPLACEMENT CONSTRAINTS

465

DESIGN FREQUENCY CONSTRAINTS

471

DESIGN OBJECTIVE

462

DESIGN STRAIN CONSTRAINTS

469

DESIGN STRESS CONSTRAINTS

467

DESIGN VARIABLES

463

DIST CHARGE (Electromagnetic)

1310

DIST CHARGES (Electrostatic)

1236

DIST CHARGES (Piezoelectric)

1254

DIST CHARGES (with TABLE Input - Electromagnetic)

1307

DIST CHARGES (with TABLE Input - Electrosatatic)

1233

DIST CHARGES (with TABLE Input - Piezoelectric)

1251

DIST CURRENT (Electromagnetic)

1306

DIST CURRENT (Joule Heating)

1160

DIST CURRENT (Magnetostatic)

1277

DIST CURRENT (with TABLE Input - Electromagnetic)

1303

DIST CURRENT (with TABLE Input - Joule Heating)

1157

DIST CURRENT (with TABLE Input - Magnetostatic)

1274

DIST FLUXES

1015

DIST FLUXES (with TABLE Input)

1012

DIST LOADS

495

DIST LOADS (with TABLE Input)

490

DIST MASS (with TABLE Input - Diffusion)

1173

DIST SOURCES (Acoustic)

1212

DIST SOURCES (with TABLE Input - Acoustic)

1209

DMIG

370

DMIG-OUT

365

ELEMENT SORT

456

EMISSIVITY

1115

END OPTION

1361

ERROR ESTIMATE

Main Index

Page

386

Chapter 3 Model Definition Options List 203

Model Dedinition Option EXCLUDE

689

FACE IDS

500

FAIL DATA (with TABLE Input)

841

FAIL DATA

855

FILMS

1009

FILMS (with TABLE Input)

1005

FIXED ACCE FIXED DISP (Fluid)

984 1336

FIXED DISP (Mechanical)

488

FIXED DISP (with TABLE Input - Mechanical)

484

FIXED EL-POT (Electrostatic)

1226

FIXED EL-POT (with TABLE Input - Electrostatic)

1223

FIXED MG-POT (Magnetostatic)

1267

FIXED MG-POT (with TABLE Input - Magnetostatic)

1264

FIXED POTENTIAL (Electromagnetic)

1301

FIXED POTENTIAL (Electrostatic)

1231

FIXED POTENTIAL (Magnetostatic)

1272

FIXED POTENTIAL (Piezoelectric)

1250

FIXED POTENTIAL (with TABLE Input - Electromagnetic)

1298

FIXED POTENTIAL (with TABLE Input - Electrostatic)

1228

FIXED POTENTIAL (with TABLE Input - Magnetostatic)

1269

FIXED POTENTIAL (with TABLE Input - Piezoelectric)

1247

FIXED PRESSURE (Acoustic)

1207

FIXED PRESSURE (with TABLE Input - Acoustic)

1204

FIXED PRESSURE (with TABLE Input - Diffusion)

1171

FIXED TEMPERATURE (with TABLE Input)

1000

FIXED TEMPERATURE

1003

FIXED VELOCITY (with TABLE Input - Fluid)

1338

FIXED VELOCITY

1341

FIXED VOLTAGE (with TABLE Input - Joule Heating)

1164

FIXED VOLTAGE

1167

FLOW LINE

Main Index

Page

418

204

Model Dedinition Option FLUID DRAG

518

FLUID SOLID

976

FOAM (with TABLE Input)

777

FOAM

781

FORCDT

568

FORMING LIMIT

797

FOUNDATION

572

FOUNDATION (with TABLE Input)

569

FOURIER

573

FXORD

241

GAP DATA

876

GASKET

784

GENERATE

226

GENT (with TABLE Input)

758

GENT

762

GEOMETRY

288

GLOBALLOCAL

529

GRAIN SIZE

867

GRID FORCE

443

HOLD NODES

513

HYPERMESH

429

HYPOELASTIC (with TABLE Input)

740

HYPOELASTIC

742

INCLUDE

240

INERTIA RELIEF

514

INIT CURE (with TABLE Input)

1126

INIT CURE

1128

INIT STRESS (with TABLE Input)

533

INIT STRESS

535

INITIAL DENSITY (Heat Transfer)

Main Index

Page

1149

Chapter 3 Model Definition Options List 205

Model Dedinition Option INITIAL DISP (with TABLE Input)

977

INITIAL DISP

980

INITIAL PC (with TABLE Input)

935

INITIAL PC

937

INITIAL PLASTIC STRAIN (with TABLE Input)

539

INITIAL PLASTIC STRAIN

541

INITIAL PORE (with TABLE Input)

939

INITIAL PORE

941

INITIAL POROSITY (with TABLE input)

925

INITIAL POROSITY

927

INITIAL PRESSURE (with TABLE Input - Diffusion)

1169

INITIAL PYROLYSIS

1147

INITIAL STATE (with TABLE Input)

544

INITIAL STATE

547

INITIAL TEMP (Heat Transfer)

1078

INITIAL TEMP (Thermal Stress)

562

INITIAL TEMP (with TABLE Input - Heat Transfer)

1075

INITIAL TEMP (with TABLE Input - Thermal Stress)

560

INITIAL VEL (with TABLE Input)

981

INITIAL VEL

983

INITIAL VOID RATIO (with TABLE Input)

930

INITIAL VOID RATIO

932

INSERT

326

IRM

420

ISLAND REMOVAL

584

ISOTROPIC (Acoustic)

1218

ISOTROPIC (Electromagnetic)

1316

ISOTROPIC (Electrostatic)

1241

ISOTROPIC (Fluid)

1345

ISOTROPIC (Heat Transfer)

1082

ISOTROPIC (Hydrodynamic)

1199

ISOTROPIC (Magnetostatic)

1283

ISOTROPIC (Stress)

Main Index

Page

713

206

Model Dedinition Option ISOTROPIC (with TABLE Input - Acoustic)

1217

ISOTROPIC (with TABLE Input - Diffusion)

1178

ISOTROPIC (with TABLE Input - Electromagnetic)

1314

ISOTROPIC (with TABLE Input - Electrostatic)

1240

ISOTROPIC (with TABLE Input - Fluid)

1343

ISOTROPIC (with TABLE Input - Hydrodynamic)

1197

ISOTROPIC (with TABLE Input - Magnetostatic)

1281

ISOTROPIC (with TABLE Input - Stress) ISOTROPIC (with TABLE Input - Thermal)

J-INTEGRAL JOULE

K2GG, K2PP

LATENT HEAT

Main Index

Page

705 1080 575 1156 373 1094

LOADCASE

414

LORENZI

576

M2GG, M2PP

375

MANY TYPES

215

MAPPER

219

MASSES

985

MATERIAL DATA

866

MERGE

221

MERGE SELECTIVE

222

MESH2D

212

MIXTURE

881

MNF UNITS

379

MODAL INCREMENT

995

MOONEY (with TABLE Input)

744

MOONEY

748

NEW

228

Chapter 3 Model Definition Options List 207

Model Dedinition Option NLELAST

772

NO ELEM SORT

458

NO NODE SORT

461

NO PRINT

438

NO PRINT CONTACT

442

NO PRINT SPRING

440

NO SUMMARY

455

NODAL THICKNESS

292

NODE CIRCLE

244

NODE FILL

245

NODE GENER

246

NODE MERGE

247

NODE SORT

459

OGDEN (with TABLE Input)

765

OGDEN

769

OPTIMIZE

395

ORIENTATION

900

ORTHO TEMP (Structural)

814

ORTHO TEMP (Thermal)

1098

ORTHOTROPIC (Electrical)

1244

ORTHOTROPIC (Electromagnetic)

1321

ORTHOTROPIC (Magnetostatic)

1288

ORTHOTROPIC (Mechanical)

725

ORTHOTROPIC (Thermal)

1087

ORTHOTROPIC (with TABLE Input - Diffusion)

1180

ORTHOTROPIC (with TABLE Input - Electromagnetic)

1318

ORTHOTROPIC (with TABLE Input - Electrostatic)

1242

ORTHOTROPIC (with TABLE Input - Magnetostatic)

1284

ORTHOTROPIC (with TABLE Input - Mechanical) ORTHOTROPIC (with TABLE Input - Thermal)

P2G

Main Index

Page

719 1084 377

208

Model Dedinition Option PARAMETERS

480

PBUSH

332

PERMANENT (Electromagnetic)

1325

PERMANENT (Magnetostatic)

1294

PERMANENT (with TABLE Input - Magnetostatic)

1292

PFAST

343

PHI-COEFFICIENTS

963

PIEZOELECTRIC (Piezoelectric)

1261

PIEZOELECTRIC (with TABLE Input - Piezoelectric)

1258

PIN CODE

Main Index

Page

325

POINT CHARGE (Piezoelectric)

1257

POINT CHARGE (with TABLE Input - Electrostatic)

1237

POINT CHARGE (with TABLE Input - Piezoelectric)

1255

POINT CHARGE

1239

POINT CURRENT (Joule)

1163

POINT CURRENT (Magnetostatic)

1280

POINT CURRENT (with TABLE Input - Joule Heating)

1161

POINT CURRENT (with TABLE Input - Magnetostatic)

1278

POINT CURRENT-CHARGE (with TABLE Input - Electromagnetic)

1311

POINT CURRENT-CHARGE

1313

POINT FLUX

1019

POINT FLUX (with TABLE Input)

1016

POINT LOAD

510

POINT LOAD (with TABLE Input)

506

POINT MASS (with TABLE Input - Diffusion)

1176

POINT SOURCE (Acoustic)

1216

POINT SOURCE (with TABLE Input - Acoustic)

1213

POINT TEMP

566

POINT TEMP (with TABLE Input)

564

POINTS

270

POROSITY CHANGE (with TABLE Input)

928

POST

397

POWDER (with TABLE input)

908

Chapter 3 Model Definition Options List 209

Model Dedinition Option POWDER

911

PRE STATE

521

PRESS FILM

952

PRESS FILM (with TABLE Input)

949

PRINT CHOICE

431

PRINT CONTACT

441

PRINT ELEMENT

433

PRINT NODE

436

PRINT SPRING

439

PRINT STREAMLINE

Main Index

Page

1153

PRINT VMASS

445

PRTCONNECT

224

PSHELL

890

PWELD

353

QVECT (with TABLE Input)

1020

RAD-CAVITY

1110

RADIATING CAVITY

1109

RBE2

319

RBE3

321

REAUTO

446

REBAR

893

RECEDING SURFACE

1143

REGION (Fluid)

1331

RELATIVE DENSITY

917

RESPONSE SPECTRUM

994

RESTART LAST

451

RESTART

448

RESTRICTOR (with TABLE Input)

1193

RESTRICTOR

1195

ROTATION A

516

RROD

324

210

Model Dedinition Option SDRC

426

SERVO LINK

317

SHAPE MEMORY (with TABLE Input)

828

SHAPE MEMORY

834

SHELL TRANSFORMATION

304

SHIFT FUNCTION

970

SINK POINTS (with TABLE Input)

1010

SOIL (with TABLE Input)

918

SOIL

922

SOLVER

392

SPECIFIC WEIGHT

938

SPECIFIED NODES

218

SPLINE

679

SPRINGS

328

START NUMBER

216

STIFSCALE

381

STRAIN RATE (Fluid) STRAIN RATE (Material Properties) STREAM DEFINITION

1347 795 1151

STRING

282

SUMMARY

454

SUPERELEM (DMIG Applications)

363

SUPERELEM

361

SURFACE ENERGY

Main Index

Page

1137

SURFACES

276

SWLDPRM

355

SYMMETRY

225

TABLE

787

TEMPERATURE EFFECTS (Coupled Fluid-Thermal)

1350

TEMPERATURE EFFECTS (Coupled Thermal-Stress)

807

TEMPERATURE EFFECTS (Heat Transfer)

1095

TEMPERATURE EFFECTS (Hydrodynamic)

1200

Chapter 3 Model Definition Options List 211

Model Dedinition Option TEMPERATURE EFFECTS (Stress)

802

THERMAL CONTACT (2-D)

1049

THERMAL CONTACT (3-D)

1066

THERMAL CONTACT with TABLES (2-D)

1041

THERMAL CONTACT with TABLES (3-D)

1055

THERMAL LOADS

558

THERMO-PORE

1132

THICKNESS (with TABLE Input)

1190

THICKNESS

1192

THROAT

1146

TIME-TEMP TRACK STREAMLINE

824 1154

TRACK

417

TRANSFORMATION

294

TYING

309

UDUMP

453

UFCONN

237

UFRICTION

684

UFXORD

248

UHTCOEF

685

UHTCON

686

UMOTION

683

USDATA

387

UTRANFORM

305

VCCT

579

VELOCITY (Convective Heat Transfer)

1120

VELOCITY (Hydrodynamic)

1188

VELOCITY (with TABLE Input - Convective Heat Transfer)

1118

VELOCITY (with TABLE Input - Hydrodynamic)

1186

VIEW FACTOR

1108

VISCEL EXP

Main Index

Page

972

212

Model Dedinition Option

Main Index

Page

VISCELFOAM

969

VISCELMOON

967

VISCELOGDEN

968

VISCELORTH

965

VISCELPROP

964

VOID CHANGE (with TABLE Input)

933

WELD FILL

1038

WELD FLUX

1028

WELD FLUX (with TABLE Input)

1024

WELD PATH

1032

WORK HARD

799

WRITE

251

Chapter 3: Model Definition Options Marc Volume C: Program Input

3

Main Index

Model Definition Options

J

MESH2D

J

Mesh Definition

J

Program Control

J

Mechanical Analysis

J

Contact

J

Material Properties

J

Rate Effects

J

Dynamic Analysis

J

Joule Heating Analysis

J

Diffusion Analysis

J

Hydrodynamic Bearing Analysis

J

Acoustic Analysis

J

Electrostatic Analysis

1227

J

Piezoelectric Analysis

1251

J

Magnetostatic Analysis

J

Electromagnetic Analysis

J

Fluid Analysis

215 231 393 477

591 697

959 979 1161

1174

1209

1335

1269 1303

1191

214 Marc Volume C: Program Input

The model definition input consists of a series of optional blocks of data. These blocks define the geometry of the mesh, material properties, boundary conditions, and analysis controls. These options are read in by activating the respective option with an alphanumeric code word (a keyword), followed by sets of data. In this document, both fixed format and free input are described. This code word is given in capital letters at the top of each block of data in the following section. An END OPTION is used to signify the end of all the model definition input data. Note that each option can be exercised more than once. In general, there is no specific order required in reading the options; however, you should be aware that the same option flags can appear in different blocks and that the last data read controls that flag. The exceptions are as follows: 1. If the FXORD or UFXORD option is used, it must come after the COORDINATES option when it uses data read in the COORDINATES option; 2. If postprocessor and restart files are being used, the results are order dependent. See the POST option for more details. 3. If the MESH2D option is used, it must follow the END parameter. If the MESH2D option is used to write a mesh file containing connectivity, coordinates and optional boundary conditions, the file needs to be read in sequential order. The CONNECTIVITY option must appear before the COORDINATES option followed by BOUNDARY conditions if stored on mesh file. Other options can be in any sequence and the above options can be repeated in any sequence to read data from other files or data input. Information given in the last option overwrites any previous information, thus facilitating any minor corrections to the data. Any option not needed should be left out.

Main Index

Chapter 3: Model Definition Options 215 MESH2D

MESH2D Two-dimensional Mesh Generator This two-dimensional mesh generator generates a mesh composed of either triangular or quadrilateral elements. The results of the mesh generation are output on a specified file. This file can then be used as input for Marc. A detailed description of the capabilities of the MESH2D generation is contained in Marc Volume A: Theory and User Information. The call to the mesh generation feature is initialized by a block with MESH2D in the first six columns. This is followed by a series of optional sets of blocks; each of which has an alphanumeric keyword. The keywords are: • BLOCKS (Required as first set) • DEFINE • MANY TYPES • START NUMBER • BOUNDARY • SPECIFIED NODES • MAPPER • CONSTRAINT • MERGE • MERGE SELECTIVE • CONNECT • PRTCONNECT • SYMMETRY • GENERATE BLOCKS must be the first set input. GENERATE must terminate the mesh generation. BLOCKS defines the parameters and the working space for the mesh generation. GENERATE tells Marc to start generating the mesh, and then returns control to Marc. You should note that the generated mesh is written out on the specified file and must be read in from this file using the appropriate model definition data options (CONNECTIVITY and COORDINATES) described in a following section before plotting or optimization of the mesh can proceed.

When using the MESH2D option, divide the geometry into simpler regions called blocks. Marc meshes each block into nodes and elements, and finally combines the blocks to form the complete mesh. The MESH2D option can be used more than once in an analysis. Simply place the second group to be included after the previous GENERATE.

Main Index

216 MESH2D Define a Two-dimensional Mesh

MESH2D

Define a Two-dimensional Mesh

Description This option starts the call to the two-dimensional mesh generation feature. This data must follow the END of the parameters. Format Format Fixed 1-6

Main Index

Free‘ 1st

Data Entry Entry A

Enter the word MESH2D.

BLOCKS 217 Define Working Size

BLOCKS

Define Working Size

This option is required and must follow MESH2D. Description This option defines the parameters and the sizes of the working space for mesh generation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word BLOCKS.

2nd data block 1-5

1st

I

Number of blocks.

6-10

2nd

I

Number of principal boundary nodes defining the geometry of all blocks. Note that principal nodes should be continuous in their numbering.

11-15

3rd

I

Code number of element type for use with Marc series of programs.

16-20

4th

I

Set to 1 for generation of 4-node quadrilateral elements. Set to 0 for triangles. Set to 2 for 8-node quads.

Main Index

21-25

5th

I

Local file on which the output is written; to be used by the Marc series of programs.

26-30

6th

31-35

7th

I

Number of times the mesh is repeated due to use of the SYMMETRY option.

36-40

8th

I

Maximum number of degrees of freedom constrained during mesh generation. Default is 100.

41-45

9th

I

Number of degrees of freedom for each node. The default is two degrees of freedom.

46-50

10th

I

Maximum number of nodes on symmetry axis. Default is 50.

51-55

11th

I

Maximum number of connections of any blocks. Default is 10.

Not used. Enter 0.

218 DEFINE (Mesh2D Block Type) Define Block Type

DEFINE (Mesh2D Block Type)

Define Block Type

Description This option allows the block type and the nodal number of the boundary points to be specified. Note:

Marc always generates node connections in a counterclockwise direction. See Marc Volume A: Theory and User Information for correct specification of boundary node number order when a distributed load has to be applied to any surface of the block.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word DEFINE.

2nd data block One per block. 1-5

1st

I

Type of block: 1, 2, 3, or 4.

6-10

2nd

I

Number of intervals in the first direction (P1 - P2). Number of increments between the first and second boundary nodes.

11-15

3rd

I

Number of intervals in the second direction (P2 - P3). M=N for a type 3 triangular block. Number of increments between second and third boundary nodes.

16-20

4th

I

First boundary node number defining the block.

21-25

5th

I

Second boundary node number defining the block.

26-30

6th

I

Third boundary node number defining the block.

31-35

7th

I

Fourth boundary node number defining the block.

I

Continue until necessary boundary nodes have been defined. A maximum of 12 is possible and these must follow the order defined in Marc Volume A: Theory and User Information.

Etc.

Main Index

MANY TYPES 219 Define Multiple Elements

MANY TYPES

Define Multiple Elements

Description This option allows you to specify different element types per block. Default is that all elements are of the same type specified in the BLOCKS option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words MANY TYPES.

2nd data block 1-5

1st

I

Element type block 1.

6-10

2nd

I

Element type block 2. Etc. for all blocks.

Continuations (more than 16 blocks) are given in Format 16I5.

Main Index

220 START NUMBER Specify Starting Element

START NUMBER

Specify Starting Element

Description This option allows you to give a lowest element number and node number for this MESH2D sequence. This option can be used more than once; for example, if MESH2D is used more than one time in a single run. Default is that Marc starts generation with element 1 and node 1. Format Format Fixed

Free

Data Entry Enter

1st data block 1-12

1st

A

Enter the words START NUMBER.

2nd data block

Main Index

1-5

1st

I

Starting node number.

6-10

2nd

I

Starting element number.

BOUNDARY 221 Define Boundary Nodes

BOUNDARY

Define Boundary Nodes

Description This allows the coordinates of the boundary nodes to be read in. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word BOUNDARY.

2nd data block Boundary node coordinates, one per node; NNO series.

Main Index

1-5

1st

I

Boundary node number.

6-15

2nd

F

First (X or Z) coordinate.

16-25

3rd

F

Second (Y or R) coordinate.

222 SPECIFIED NODES Specify Node Coordinates

SPECIFIED NODES

Specify Node Coordinates

Description This option allows the coordinates of certain nodes of the generated mesh to be specified. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words SPECIFIED NODES.

I

Number of sets of nodal points coordinates to be specified, (maximum 100).

2nd data block 1-5

1st

3rd data block One per specified node.

Main Index

1-10

1st

F

First coordinate of a specified nodal point.

11-20

2nd

F

Second coordinate of a specified nodal point.

MAPPER 223 Invoke User Subroutine MAP2D

MAPPER

Invoke User Subroutine MAP2D

Description This option invokes the MAP2D user subroutine (see Marc Volume D: User Subroutines and Special Routines) for boundary node coordinate generation or modification. It is used when it is more convenient to program the boundary node coordinates rather than reading them in. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word MAPPER. This invokes the MAP2D user subroutine. If the coordinates input on the BOUNDARY parameter are to be modified, this option must follow the BOUNDARY parameter.

Main Index

224 CONSTRAINT Generate Boundary Condition Constraints

CONSTRAINT

Generate Boundary Condition Constraints

Description This feature allows boundary conditions to be generated for a particular degree of freedom for all the nodal points on one side of a block. At the present time, there is no method available for setting boundary conditions on those nodes generated via the SYMMETRY option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONSTRAINT.

I

Number of sides to be constrained.

2nd data block 1-5

1st

3rd data block

Main Index

1-5

1st

I

Number of the block to be constrained.

6-10

2nd

I

Number of the side to be constrained.

11-15

3rd

I

Degree of freedom to be constrained.

16-25

4th

F

Displacement value to be given to the constrained degree of freedom.

MERGE (Model Definition) 225 Specify Minimum Distance Between Nodes

MERGE (Model Definition)

Specify Minimum Distance Between Nodes

Description This allows a minimum distance between nodes to be specified. Any nodes separated by less than the minimum distance is automatically merged into a single node. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word MERGE.

F

Separation distance below which nodes are merged together.

2nd data block 1-10

Main Index

1st

226 MERGE SELECTIVE Specify Minimum Distance Between Nodes by Block

MERGE SELECTIVE

Specify Minimum Distance Between Nodes by Block

Description This option, used in conjunction with the CONNECT option, allows you to define which nodes are to be merged in mesh blocks that border each other. This is especially useful if gaps are to be defined between the blocks. As with the MERGE option, you specify a minimum distance and a list of block numbers in which nodes are to be merged. Nodes which are separated by less than the minimum distance specified are considered duplicates, and merged into a single node if they lie within the same or connected blocks. Nodes located within the specified minimum distance on unconnected blocks (those disconnected using the CONNECT option) are not merged. For more information about connecting blocks, see the description of the CONNECT option in this document. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words MERGE SELECTIVE.

I

Enter the number of sets of data to be used to enter merge distance and block numbers.

2nd data block 1-5

1st

Data blocks 3 and 4 are entered as pairs, one for each data set. 3rd data block 1-10

1st

F

Enter the minimum separation distance.

4th data block Enter a list of block numbers.

Main Index

CONNECT 227 Connect or Disconnect Mesh Blocks

CONNECT

Connect or Disconnect Mesh Blocks

Description This option is used to connect or disconnect two blocks during the generation of the final mesh. Default is that two blocks are connected if they join the same boundary points in the DEFINE option. It is especially useful to disconnect two blocks if gaps are to be defined in between the blocks. The MERGE SELECTIVE option must be used in combination with this option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONNECT.

2nd data block 1-5

1st

I

Number of block connections to specify.

6-10

2nd

I

Unit number for input of 3rd data block; defaults to data input.

3rd data block One per continuation.

Main Index

1-5

1st

I

First connected block.

6-10

2nd

I

Second connected block.

11-15

3rd

I

Set to 0 to connect the two blocks; set to 1 to disconnect the two blocks.

228 PRTCONNECT Print Out Block Connections

PRTCONNECT

Print Out Block Connections

Description This option gives a printout of the current BLOCKS connection information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word PRTCONNECT.

SYMMETRY 229 Define Axis of Symmetry

SYMMETRY

Define Axis of Symmetry

Description This allows symmetry axes to be defined so that further mesh blocks can be generated by reflection about the axes. Be sure that enough space is allocated in the BLOCKS option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word SYMMETRY.

I

Number of symmetric axes.

2nd data block 1-5

21st

3rd data block One per symmetry axis.

Main Index

1-10

1st

F

First coordinate of a point on the axis of symmetry.

11-20

2nd

F

Second coordinate of a point on the axis of symmetry.

21-30

3rd

F

First component of a vector along the axis of symmetry.

31-40

4th

F

Second component of a vector along the axis of symmetry.

230 GENERATE End of Mesh Generation Data

GENERATE

End of Mesh Generation Data

Description This signifies the end of the mesh generation data and instructs Marc to proceed with the mesh generation. When the mesh has been generated, Marc proceeds to the next option found in the model definition options. If you wish to stop without proceeding to plotting or analysis, a blank block should immediately follow the GENERATE option. This causes Marc to stop on an illegal data exit. Provisions should be made to save the mesh on permanent file by appropriate control blocks if only mesh generation is desired. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

Main Index

1st

A

Enter the word GENERATE.

Chapter 3: Model Definition Options 231 Mesh Definition

Chapt Mesh Definition er 3: This section describes the geometry input required to describe the object to be analyzed. The finite mesh can be generated using MESH2D, Marc Mentat, or some other preprocessor. The element Mode element topology and coordinates can be processed using a variety of options. This final set of connectivity and coordinates can be written to an auxiliary file through the WRITE option. Additional geometric quantities l can be input through the GEOMETRY or NODAL THICKNESS options; see Marc Volume B: Element Defini Library for the data required for particular element types. The ROTATION A option is used to give the axis for the calculation of centrifugal loads. The degrees of freedom associated with nodes can be transformed tion from their natural system (see Marc Volume B: Element Library for the definition for each particular Optio element) to a user-defined local system. Kinematic constraints can be imposed between degrees of freedom using either the TYING or SERVO LINK option. Finally, springs can be defined using the ns SPRINGS option. The NEW parameter can be used to specify a change in format.

Main Index

232 NEW (Model Definition) Use New Format

NEW (Model Definition)

Use New Format

Description This option can be used to switch from input with extended format to the default width or vice-versa. Input is interpreted to be in the format defined here until another NEW option is encountered. This option must not appear embedded inside any model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word NEW.

11-15

2nd

I

Enter 1 if the default width of the data fields is used for input. This overrides the EXTENDED parameter. Enter 2 if the double width of the data fields is used for input.

Main Index

DEFINE (Sets) 233 Define Sets

DEFINE (Sets)

Define Sets

Description This option allows you to define a setname and to associate members to the set. These sets can be used wherever a list of items is requested. Multiple numbers of sets can be used by repeating this model definition block. In defining the members of a set, any of the conventions in the Input of List Items in Chapter 1 Introduction can be used. A previously defined set can be used to describe a set. If the input version is 10 or greater, the set can be 32 characters in length. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word DEFINE.

The rest of this data block is free format beginning with the third field. 11-20

2nd

A

Enter the type of set: ELEMENT – set of elements ELSQ

– set of elements (unsorted)

NODE

– set of nodes

NDSQ

– set of nodes (unsorted)

INT

– set of integration points

LAYER

– set of beam or shell layers

DOF

– set of degrees of freedom (unsorted)

INCS

– set of increment numbers

POINT

– set of points

CURVE

– set of curves

SURFACE – set of surfaces

Main Index

BODY

– set of body numbers

EDGE

– set of element: edge pairs

FACE

– set of element: face pairs

EDGEMT

– set of element: edge pairs. Edge number given using Marc Mentat convention.

FACEMT

– set of element: face pairs. Face number given using Marc Mentat convention.

234 DEFINE (Sets) Define Sets

Format Fixed

Free

Data Entry Entry ORNSUR

– set of surface: orientation, where the orientation is given in Marc convention 1 – top surface 2 – bottom surface.

ORNCUR

– set of curve: orientation, where the orientation is given in Marc convention: 1– top surface 2 – bottom surface.

MNORSU

– set of surface: orientation, where the orientation is given in Marc Mentat convention: 0 – top surface 1 – bottom surface.

MNORCU – set of curve: orientation, where the orientation is given in Marc Mentat convention: 0 – top surface 1 – bottom surface. ELNODE 21-30

3rd

A

– set of element relative_node pairs. For example, relative_node is 1 or 2 for 2-node beam element.

Enter the word SET. (This is optional.) Enter the word OSET for an open set (see Note 4).

31-62

4th

A

Enter the name of the set.

2nd data block 1-80

Notes:

1st

Enter a list of items that are of the type defined to be members of the set whose name is given.

(1) A setname cannot be used in a list unless it has been previously defined. (2) For unsorted set types DOF, ELSQ, and NDSQ, the verbs EXCEPT and INTERSECT cannot be used in the list of items. (3) EDGE, EDGEMT, FACE, FACEMT, ORNSUR, MNORSU, ORNCUR, MNORCU can only be used with the table input format. (4) When an open set is requested, nodes or elements not defined elsewhere are not automatically created.

Main Index

DEFINE (Sets) 235 Define Sets

Example The example below defines a set to be called WALL consisting of nodes 1, 3, 5, 7, …19. DEFINE NODE SET WALL 1 TO 20 BY 2

The example below defines a set to be called LOADIT consisting of edge 2 of elements 1, 3, 5, 7, ... 19. DEFINE EDGE SET LOADIT 1:2 TO 20:2 BY 2

Main Index

236 CONNECTIVITY Specify Element Connectivity

CONNECTIVITY

Specify Element Connectivity

Description This series gives the element connectivity; for example, the nodal points for each element. Data can be input from data or an external file by exercising the appropriate option. For two-dimensional elements, the nodal points must be given in a counterclockwise sequence. Several blocks of connectivity data can be input. For example, one block can be read in from file while additional ones are read from data blocks, each block starting with the word CONNECTIVITY. In a coupled thermal-stress analysis, the element type (second field, 3rd data block) should be a stress type element if both a structural and thermal analysis is required. If a heat transfer element type is given, the element is considered rigid in the stress analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the word CONNECTIVITY.

In many cases, when the whole mesh is in a file, just CONNECTIVITY and a blank should be included here and the INPUT TAPE parameter must be used. 2nd data block 1-5

1st

I

Number of elements to be read in this option (optional); defaults to total number of elements in the mesh.

6-10

2nd

I

Enter the unit number for input of connectivity; defaults to unit number specified on the INPUT TAPE parameter.

11-15

3rd

I

Set to 1 to suppress printing of element connectivity list during this option.

3rd data block Element connectivity array. This data block is repeated once for each element given in data block 2.

Main Index

1-5

1st

I

Element number.

6-10

2nd

I

Element type or alias (see ALIAS parameter).

11-15

3rd

I

Nodal point.

CONNECTIVITY 237 Specify Element Connectivity

Format Fixed 16-20 21-25

Free 4th

Data Entry Entry I

Nodal point.

I

Repeat until all nodes of the element have been defined. The required ordering of the nodes is given in Marc Volume A: Theory and User Information. Continuation for elements with more than 14 nodes/element (for example, library element 21, 35, 57, etc.) is in format 16I5.

Main Index

238 CONN FILL Specify Element Connectivity Interpolator

CONN FILL

Specify Element Connectivity Interpolator

Description This option completes the filling of connectivity lists by generating midside nodes in between the corner nodes provided. At the same time, it generates coordinates for the new node created. The coordinates are formed by averaging the coordinates of the end nodes of the respective side on the connectivity list. It is used for converting linear displacement elements to quadratic displacement elements. The option works for 4-node quadrilaterals and 8-node bricks. You must remember to turn on the bandwidth optimization option after using this option and before an analysis. Note:

This does not calculate the coordinates correctly if going from element 4 to element 22 or 24.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words CONN FILL.

2nd data block

Main Index

1-5

1st

I

Enter the starting node number for the midside nodes.

6-10

2nd

I

Enter 1 to set the node count to the maximum node number used in this option.

11-15

3rd

I

Give the start of the element list for this option. Default is 1.

16-20

4th

I

Give the end of the element list for this option. Default is number of elements specified in the analysis.

CONN GENER 239 Copy Element Connectivity Data

CONN GENER

Copy Element Connectivity Data

Description This input performs the function of an incremental mesh generator by copying the pattern of the connectivity data for previously defined elements. If the new elements are to be connected to the master elements, a common node A needs to be given. The position of node A in the connectivity list of the new element and its position in the connectivity list of the master element needs to be given. Marc then numbers all the other nodes in the new element by making the algebraic difference between the numbers of all the nodes in the new element the same as that of the corresponding nodes in the element being copied. This option copies the connectivity from a series of elements defined by a starting and end element number and uses it to calculate the connectivity for a new series of elements. The new series of elements is defined by the input of a starting and end element number. When the list of the elements being copied from is ended, the recently generated elements will take its place as the elements to be copied from. This is repeated until the list defined for the new elements is exhausted. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words CONN GENER.

2nd data block

Main Index

1-5

1st

I

Number of the first element for which the connectivity is being generated.

6-10

2nd

I

Number of the last element for which the connectivity is being generated. All the elements between the first and last element will be generated.

11-15

3rd

I

Number of the first element used as a master.

16-20

4th

I

Number of the last element used as a master.

21-25

5th

I

Give the position of node A in the connectivity list of the generated element. Node A can belong to a master element. If there is no common node between the generated and the master elements, enter 1.

26-30

6th

I

Give the position of node A in the connectivity list of the master element. If there is no common node, enter 1.

240 CONN GENER Copy Element Connectivity Data

Format Fixed 31-35

Free 7th

Data Entry Entry I

Enter 1 for decrease of 1 element per series of master elements. Enter 2 for decrease of 2 elements per series of master elements. The two element decrease is restricted to use with three-node triangular elements.

36-40

Main Index

8th

I

This entry is only required if there is no common node between the generated and master elements. This defines an increment to each of the nodes in the master element which then gives the connectivity list of the generated element.

UFCONN 241 Invoke the UFCONN User Subroutine

UFCONN

Invoke the UFCONN User Subroutine

Description This option calls the UFCONN user subroutine to generate or modify element connectivity (see Marc Volume D: User Subroutines and Special Routines.) The option can be repeated as often as necessary. This option must follow the CONNECTIVITY option. Format Format Fixed

Free

Dat Entry Entry

1st data block 1-6

1st

A

Enter the word UFCONN.

2nd data block Enter a list of elements for which the UFCONN user subroutine is called.

Main Index

242 COORDINATES Enter Node Coordinates

COORDINATES

Enter Node Coordinates

Description This option defines the coordinates of each nodal point. The nodal data can be input in several blocks. The latest data input for a particular nodal point is used. Like the element connectivity data, this data can be input from an external file since this coordinate data can be automatically generated by a mesh generator. Local corrections can be made to the generated mesh by input of the modified nodal coordinates from data blocks. Usually for the general shell elements (4, 8, and 24), the FXORD option and the UFXORD user subroutine can help with input of coordinates. In Marc, the nodes need not be numbered sequentially. In most cases, when all the coordinates are input by file, just the coordinates and a blank are required here and the INPUT TAPE parameter must be used. If the COORD SYSTEM, CYLINDRICAL, or FXORD options are used, the coordinate positions entered here are with respect to coordinate system entered in these options. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the word COORDINATES.

2nd data block 1-5

1st

I

Enter the maximum number of coordinate directions to be read in per node; defaults to the number of coordinates per node. Repeated COORDINATES blocks need not have the same value in this field.

6-10

2nd

I

Enter the number of nodal points read-in in this option; (optional) default to the number of nodes in the mesh.

11-15

3rd

I

Enter the unit number for input of coordinates; defaults to the file number specified on the INPUT TAPE parameter.

16-20

4th

I

Set to 1 to suppress print-out of nodal coordinate list during this option input.

3rd data block One data line per nodal point.

Main Index

1-5

1st

I

Nodal point number.

6-15

2nd

F

Coordinate 1.

16-25

3rd

F

Coordinate 2.

COORDINATES 243 Enter Node Coordinates

Format Fixed

Free

Data Entry Entry

26-35

4th

F

Coordinate 3.

36-45

5th

F

Coordinate 4.

Etc.

Etc.

See library element description in Marc Volume B: Element Library for the definition of coordinates for a particular element. Input 6 coordinates per data line; continuation data lines in format 6E10.5.

Main Index

244 INCLUDE (Model Definition) Insert File into the Input File

INCLUDE (Model Definition)

Insert File into the Input File

Discription Inserts an external file into the input file. The include statement may appear in either the parameter, model definition, or history definition section. In Marc, an include file may reference another include file up to a level of 10 deep. The total length of the file name, including the directory path is limited to 240 characters. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word INCLUDE.

11-80

2nd

A

Physical filename. If the file name is specified without a path, the file should be in the same directory as the input file. If a path is given, the file should be in the path relative to the current working directory. Also, note that the file name is case sensitive and blanks should not be included in the name.

Main Index

FXORD 245 Coordinate Generation and Transformation Coordinates

FXORD

Coordinate Generation and Transformation Coordinates

SHELL COORDINATE GENERATION OPTION Description This option is used to generate coordinates for Elements 4, 8, or 24. (Refer to Marc Volume B: Element Library and Marc Volume A: Theory and User Information for further information on the use of this block). This can be used for mapping of certain types of standard shell geometries such as cylinders, spheres, etc. It can also be used to transform cylindrical coordinates into Cartesian coordinates. The CYLINDRICAL or COORD SYSTEM options are more powerful for cylindrical coordinates. Note that when a continuous surface has a line of discontinuity in φ1 or φ 2 (the surface coordinate) such

as a complete cylinder has at φ = 0° and 360°, two nodes must be placed at each nodal location on the line to allow the distinct coordinate input, and tying type 100 used to join degrees of freedom. In general, different surfaces coming together must also use the intersecting shell tyings. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word FXORD.

11-12

2nd

A

Enter the word NO if coordinates after FXORD are not to be printed out.

I

Number of sets of shell geometry specifications to be input.

2nd data block 1-5

1st

Data blocks 3, 4, 5, and 6 are provided once for each consecutive series of nodes with a different shell geometry specification. 3rd data block 1-5

1st

I

Identification number of surface type. See Table 3-1 and Marc Volume A: Theory and User Information.

6-10

2nd

I

First node of this series.

11-15

3rd

I

Last node of this series.

16-20

4th

I

Set to 1 if local (x,y,z) set in which surface is defined must be transformed to the global (x,y,z) set. If so, data blocks 4, 5 and 6 must be input to define the transformation. If not, data blocks 4, 5 and 6 are omitted.

4th data block Enter the global (x,y,z) coordinates of the origin of the local (x,y,z) system in which the shell surface is generated.

Main Index

246 FXORD Coordinate Generation and Transformation Coordinates

Format Fixed

Free

Data Entry Entry

1-10

1st

F

Global x-coordinate origin.

11-20

2nd

F

Global y-coordinate origin.

21-30

3rd

F

Global z-coordinate origin.

5th data block Enter the global (x,y,z) coordinates of a point on the positive x-axis of the local system. 1-10

1st

F

Global x-coordinate of the point.

11-20

2nd

F

Global y-coordinate of the point.

21-30

3rd

F

Global z-coordinate of the point.

6th data block Enter the global (x,y,z) coordinates of a point on, or near to, the positive y-axis of the local system. This point defines the local (x,y) plane in the global system. 1-10

1st

F

Global x-coordinate of the point.

11-20

2nd

F

Global y-coordinate of the point.

21-30

3rd

F

Global z-coordinate of the point.

Table 3-1 describes the

Table 3-1

ϕ1, ϕ2 directions for the FXORD option contained in Marc.

Input to FXORD Nodal Data Input (See Marc Volume A:

Input Code Type 0 1

User Information

Surface Description General Surface Surface x3=x3(x1, x2)

All units are length measure, unless specified otherwise All 11 Coords. for El. 8 All 14 Coords. for El. 4 2

∂x 3 ∂x 3 ∂ x 3 x 1, x 2, x 3, -------- , -------- , ----------------∂x 1 ∂x 2 ∂x 1 ∂x 2

Surface Coordinates used in program (θ1, θ2)

θ1, θ2,

NonCartesian Coordinate s YES

first two input x1, x2

YES

θ, φ

YES

(last coordinate only needed for element type 4) 2

Axisymmetric shell (about x3 axis)

∂R θ, φ, R, ------∂φ

:

dR l en gt h ------- in -------------------- uni t s dφ ra d ia ns

Main Index

(in radians)

FXORD 247 Coordinate Generation and Transformation Coordinates

Table 3-1

Input to FXORD Nodal Data Input (See Marc Volume A:

Input Code Type

User Information

Surface Description

All units are length measure, unless specified otherwise

NonCartesian Coordinate s

3

General Cylinder

dx 1 dx 2 s, x 3, x 1, x 2, -------- , -------ds ds

s, x3

NO

4

Circular Cylinder

q, x3, R: θ in degrees

NO

(about x3 axis)

R at 1st node only

R, θ, x3 (R, θ in length measure)

5

Flat Plate x3=0

x 1, x 2

x1, x2

NO

6

Curved Pipe

θ, φ, r, R: θ, φ in degrees r and R at 1st node only

r, θ, R, φ (both in length measure)

YES

(elbow)

Main Index

Surface Coordinates used in program (θ1, θ2)

7

Cylindrical

r, θ, x3

x1, x2, x3

NO

8

Spherical

r, θ, φ

x1, x2, x3

NO

248 NODE CIRCLE Generate Coordinates for Circular Arcs

NODE CIRCLE

Generate Coordinates for Circular Arcs

Description This option generates the coordinates of a series of nodes which lie on a circular arc. The coordinates of the first node on the arc must be previously given. The circle must lie in the x-y plane. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE CIRCLE.

2nd data block 1-5

1st

I

Node number of the first node on the arc.

6-10

2nd

I

Total number of nodes on arc.

11-15

3rd

I

First increment in series of node numbers to be generated.

16-20

4th

I

Second increment in series of node numbers to be generated. Entry of the second increment alternates the increment in node numbers and is used for 8 node quadrilaterals. It is only used if a nonzero number is entered in this field.

21-25

5th

I

Scaling of angle between each pair of nodes as a percentage. A default of 100 percent is used.

26-35

6th

F

Number of degrees between the first pair of nodes.

3rd data block

Main Index

1-10

1st

F

First coordinate of the center of the circle.

11-20

2nd

F

Second coordinate of the center of the circle.

NODE FILL 249 Coordinate Interpolation for Incremental Mesh Generation

NODE FILL

Coordinate Interpolation for Incremental Mesh Generation

Description This option performs the function of an incremental mesh generator for nodes. It achieves this by interpolation. In its simplest form, it takes the coordinates defined by two end nodes and divides the line between them into a specified number of equally spaced nodes. Additional data can be input to vary the distances between the generated nodes in a geometric ratio. This option is often used with the UFXORD user subroutine to obtain a warped curve in space. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE FILL.

2nd data block

Main Index

1-5

1st

I

Number of the first node in the series. The coordinate data for this node must have been previously defined.

6-10

2nd

I

Number of the last node in the series. The coordinate data for this node must have been previously defined.

11-15

3rd

I

Node number increments to be taken in the above list.

16-20

4th

I

Second increment in series of node numbers to be generated. Entry of the second increment alternates the increment in node numbers and is used for 8-node quadrilaterals. It is only used if a nonzero number is entered in this field.

21-25

5th

I

Scaling of the distances between successive nodes as a percentage. A default of 100 percent is used.

26-30

6th

I

Number of times that the series will be repeated. You should ensure that all starting and ending nodes in the series have been defined previously. This repeat feature defaults to 1 series.

31-35

7th

I

Print flag is set equal to 1, nodal coordinate printout is omitted. If set equal to 2, only the generated coordinates are printed. If set equal to 0 or left blank, all coordinates are printed.

36-40

8th

I

Increment in first and last nodes in the series if the series is repeated more than once. Defaults so that the next series will start from the node after the last node in the preceding series.

250 NODE GENER Generate Node Coordinates

NODE GENER

Generate Node Coordinates

Description This option performs the function of an incremental mesh generator for nodes. It is used when elements such as the quadratic 8-node elements require different spacing in successive nodal rows. It achieves this by using a list of nodes as the master pattern. It then creates a new set of nodes by giving the new set of nodes the same coordinate spacing as the list of nodes. Additional optional data allows the spacing to be changed as a percentage of the spacing between the nodes. When the list of nodes is used up, the newly generated nodes takes its place on the list and the process is repeated until the number of nodes to be generated has been completed. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE GENER.

2nd data block 1-5

1st

I

Number of the first node for which coordinates are being generated. This coordinate data for this node must have been previously defined).

6-10

2nd

I

Number of the last node in the series. (This coordinate data for this node must have been previously defined.)

11-15

3rd

I

Number of the first node used as a master.

16-20

4th

I

Number of the last node used as a master.

21-25

5th

I

Increment in the node numbers of the two node series above. A default value of 1 is used.

26-30

6th

I

Second increment in series of node numbers to be generated. Entry of the second increment alternates the increment in node numbers and is used for 8-node quadrilaterals. It is only used if a nonzero number is entered in this field.

31-35

7th

I

Scaling of distance between each pair of nodes as a percentage. A default of 100 percent is used.

36-40

8th

I

Enter 1 for decrease of 1 node per series of master nodes. Default is 0. Enter 2 for a decrease of 2 nodes per series.

41-45

9th

I

Print flag if set equal to 1, nodal coordinate printout is omitted. If set equal to 2, only the generated coordinates are printed. If set equal to 0 or left blank, all coordinates are printed.

Main Index

NODE MERGE 251 Merge Duplicate Nodes

NODE MERGE

Merge Duplicate Nodes

Description This option searches through all the nodes and merges all nodes which are closer to each other than a minimum-specified distance. The default minimum distance is 0.001 The merge provision only alters the node numbers defined by the COORDINATES and CONNECTIVITY options. Loading and boundary conditions must be applied to the new node numbers after nodal merge. The node merge command cannot be used with shells or beam elements. The WRITE option can be used to save the new mesh. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE MERGE.

2nd data block 1-5

1st

I

Set to 1 to set the node count to the minimum number found after the use of this option.

6-10

2nd

I

Set to starting node number or nodal merge. Default is 1.

Main Index

11-15

3rd

I

Set to last node number for nodal merge. Default to total number of nodes specified in SIZING parameter.

16-25

4th

F

Separation distance below which nodes will be merged together.

26-30

5th

I

Set to 1 to suppress printout of new connectivity.

252 UFXORD Invoke the UFXORD User Subroutine

UFXORD

Invoke the UFXORD User Subroutine

Description This block invokes the call to the UFXORD user subroutine to generate or modify nodal coordinates (see Marc Volume D: User Subroutines and Special Routines). The block can be repeated as often as necessary. This option must follow the COORDINATES option. If the nodes are specified in the CYLINDRICAL or COORD SYSTEM options, the coordinates defined in the user subroutine are with respect to the local coordinate system. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word UFXORD.

2nd data block Enter a list of nodes for which the UFXORD user subroutine is called.

Main Index

CYLINDRICAL 253 Define Cylindrical Coordinate System

CYLINDRICAL

Define Cylindrical Coordinate System

Description This option allows for the input of a cylindrical coordinate system such that both the nodal input and output of a group of nodal points are treated in this cylindrical coordinate system. For nodes listed in this option, nodal input (that is, COORDINATES, POINT LOAD, FIXED DISP, INITIAL DISP, INITIAL VEL, etc.) and nodal output (that is, incremental and total displacements, etc.) are to be given in the cylindrical coordinate system defined here. Note:

All coordinate systems defined with this option are based upon the original model and they are not updated during the analysis.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CYLINDRICAL.

2nd data block 1-5

1st

I

Number of sets of cylindrical coordinate data (required for this option).

6-10

2nd

I

Unit number for reading data. Defaults to input deck.

11-15

3rd

I

Enter nonzero integer to suppress printing of generated rectangular coordinates and nodal transformations after the END OPTION option.

Repeat data blocks 3, 4, 5, and 6 once for each data set. 3rd data block – coordinates of origin 1-10

1st

F

Enter x coordinate (with respect to global Cartesian coordinates) of point defining origin of cylindrical coordinate system.

11-20

2nd

F

Enter y coordinate of origin.

21-30

3rd

F

Enter z coordinate of origin.

4th data block – coordinates of point 1

Main Index

1-10

1st

F

Enter x coordinate (with respect to global Cartesian coordinates) of point such that vector from origin to this point defines the z axis of cylindrical coordinate system.

11-20

2nd

F

Enter y coordinate of z axis point.

21-30

3rd

F

Enter z coordinate of z axis point.

254 CYLINDRICAL Define Cylindrical Coordinate System

Format Fixed

Free

Data Entry Entry Note:

If the calculated direction cosines of the local Z-axis are zero, they are reset to (0., 0., 1.). This is the default for two-dimensional cylindrical coordinates.

5th data block – coordinates of point 2 1-10

1st

F

Enter x-coordinate (with respect to global Cartesian coordinates) of a point such that a vector from the origin to this point defines the axis from which θ is measured in planes perpendicular to the z-axis.

11-20

2nd

F

Enter y-coordinate of this point.

21-30

3rd

F

Enter z-coordinate of this point. Note:

If the calculated direction cosines of the local X-axis are zero, they are reset to (1., 0., 0.). ˆ Z

Point 1

Z

Origin Y

θ

ˆ X Point 2

X

6th data block Enter a list of nodes using this cylindrical coordinate system. Marc assumes that the coordinates of these nodes are given in cylindrical coordinates with respect to the cylindrical axes defined in data blocks 3, 4 and 5. Coordinates are entered as r, theta, z, where theta is in degrees. Marc also calculates nodal transformations for these nodes such that all nodal input and output is given with respect to the cylindrical coordinate system attached to these nodes.

Main Index

WRITE 255 Write Connectivity and Coordinates

WRITE

Write Connectivity and Coordinates

Description This option allows you to write the final connectivity and coordinates to an auxiliary file. The values written are those after all internal mesh generations (MESH2D, FXORD or incremental generators) and all external (UFXORD, UFCONN) transformations have been performed. The coordinates are output in the global system, not in the local coordinate system specified in either the CYLINDRICAL or COORD SYSTEM options. All node numbers are in the user system; that is, nonoptimized. Note:

The connectivity and coordinates data are written to the auxiliary file in the format (default or extended) based on the last related valid option (see the EXTENDED parameter as well as the NEW (model and history definition options).

Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-10

1st

A

Enter the word WRITE.

11-15

2nd

I

Enter the unit number to write to. Default is unit 1.

256 ADAPTIVE Define Error Criteria Used in Adaptive Analysis

ADAPTIVE

Define Error Criteria Used in Adaptive Analysis

Description This model definition set controls the error criteria for local adaptive meshing. The ADAPTIVE parameter must also be included. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word ADAPTIVE.

2nd data block 1-5

1st

I

Enter the number of criteria to use.

6-10

2nd

I

Enter the unit number to read data, defaults to input.

11-15

3rd

I

Enter the frequency to perform adaptive meshing, default is every increment.

16-20

4th

I

Enter the unit number to which the adaptive mesh data will be written.

21-25

5th

I

Enter 1 for ignoring attach information when an element edge or face which is attached to a curve or surface is subdivided. By default, the new nodes are projected to the curve or surface.

Data blocks 3 and 4 are repeated in pairs for each criteria selected. 3rd data block 1-5

1st

I

Enter the criteria type: 1: Mean Strain Energy Subdivide element if: element strain energy > f1 * total strain energy/NUMEL f2 to f6 is not used

Main Index

ADAPTIVE 257 Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry 2: Zienkiewicz-Zhu Error Criterion The error norm is defined as 2

π

2

ϒ

2

=

=

∫ ( σ∗ – σ ) dV ----------------------------------------------------------2 2 ∫ σ d V + ∫ ( σ∗ – σ ) d V 2 ∫ ( E∗ – E ) dV ----------------------------------------------------------2 2 ∫ E dV + ∫ ( E – E∗ ) dV

or

The stress error and strain energy errors are X =

∫ ( σ∗ – σ )

2

dV

and

Y =

∫ ( E∗ – E )

2

dV

The allowable element stress error is AES = f2 * X/NUMEL + f3 * X * f1/π/NUMEL The allowable element strain energy error is AEE = f4 * Y/NUMEL + f5 * X * f1/γ/NUMEL where NUMEL is the number of elements in the mesh. If f2, f3, f4, f5 are input as zero, f2 = 1.0. If stress error testing is to be performed, f1 ≠ 0 and f2 and/or f3 ≠ 0, f4 = 0, f5 = 0. The element will be subdivided when: π > f1 and Xel > AES. If strain energy error testing is to be performed, f1 ≠ 0 and f2 = 0, f3 = 0, f4 ≠ 0, and/or f5 ≠ 0. The element will be subdivided when: γ > f1 and Yel > AEE The default is f2 = 1.0 if f2, f3, f4, f5 are input as 0.0. It is advisable that f2 + f3 ≈ 1 or f4 + f5 ≈ 1.0. 3: Stress Discontinuity (not yet implemented) 4: Node within Box Subdivide element if at least one of the nodes:

Main Index

258 ADAPTIVE Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry f1 < x < f2 and f3 < y < f4 and f5 < z < f6 The coordinates of the box may be moved at the end of each increment using the UADAPBOX user subroutine or the box may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block. -4: Node location within box Subdivision criteria is the same as Type 4. If all nodes of element leave the box, the subdivided elements are merged together. The coordinates of the box may be moved at the end of each increment using the UADAPBOX user subroutine or the box may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block. 5: Node in Contact Subdivide element if at least one of the nodes is in contact or belongs to a segment which is contacted f1 to f6 are not used, enter 0 or blank 6: Aspect Ratio (not yet implemented) 7: Skewness Ratio (not yet implemented) 8: Thermal Gradient (used for heat transfer and coupled analysis) Subdivide element if: gradient > maximum gradient * f1 or gradient > f2 and temperature > f3 (if given) typical value of f1 = 0.75 (f1 must be < 1.0) f4 to f8 are not used, enter 0 or blank 9: Equivalent stress, strain Subdivide element if: von Mises stress > f1 * maximum von Mises stress or von Mises stress > f2 Equivalent strain > f3 * maximum equivalent strain

Main Index

ADAPTIVE 259 Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry or Equivalent strain > f4 Equivalent plastic strain > f5 maximum equivalent plastic strain or Equivalent plastic strain > f6 Equivalent creep strain > f7*maximum equivalent creep strain or Equivalent creep strain > f8. 10: User subroutine UADAP Subdivide element if: user/maximum user > f1 or user > f2 f3 to f6 are not used, enter 0 or blank user is defined in user subroutine UADAP 11: Previously Defined Mesh Use the refined mesh from a previous analysis as the starting point to this analysis. (see 4th data block). 12. Zienkiewicz-Zhu plastic strain error criterion: 2

p 2

∫ ( ε * – ε ) dV = ------------------------------------------------------------p2 p p 2 ∫ ε dV + ∫ ( ε * –ε ) d V p

α

The plastic strain error is: A =

∫ (ε

p*

p 2

– ε ) dV

The allowable element plastic strain error is AEPS = f2 * A/NUMEL + f3 * A * f1/α/NUMEL The element will be subdivided when: α > f1 and Ae > AEPS. NUMEL is the number of elements in the mesh.

Main Index

260 ADAPTIVE Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry 13. Zienkiewicz-Zhu creep strain error criterion: β

=

c 2

∫(ε * – ε ) dV ------------------------------------------------------------c2 c* c 2 ∫ ε dV + ∫ ( ε – ε ) dV c

2

The creep strain error is: B =

∫(ε

c*

c 2

– ε ) dV

The allowable element creep strain error is AECS = f2 * B/NUMEL + f3 * B * f1/β/NUMEL The element will be subdivided when: β > f1 and Bel > AECS. NUMEL is the number of elements in the mesh. 14: Pressure Gradient (used only for diffusion analysis) gradient > maximum gradient * f1 or gradient > f2 and pressure > f3 (if given) typical value of f1 = 0.75 (f1 must be < 1.0) 15: Electrical Potential Gradient (used only for electrostatic analysis) Subdivide element if: gradient > maximum gradient * f1 or gradient > f2 and potential > f3 (if given) typical value of f1 = 0.75 (f1 must be < 1.0) 16: Magnetic Potential Gradient (used only for magnetostatic analysis) Subdivide element if: gradient > maximum gradient * f1 or gradient > f2 and potential > f3 (if given) typical value of f1 = 0.75 (f1 must be < 1.0) 17. Elements in cutter path. This criterion can only be used for analysis of NC Machining problems.

Main Index

ADAPTIVE 261 Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry 18. Angle between shell elements. Subdivide element if the change in the angle between neighboring shell elements is larger than f1. 19: Node location within a Cylindrical Region Subdivide element if at least one of the nodes is in the region defined by a cylinder: f1 = radius f2 = x-coordinate of first point on axis f3 = y-coordinate of first point on axis f4 = z-coordinate of first point on axis f5 = x-coordinate of second point on axis f6 = y-coordinate of second point on axis f7 = z-coordinate of second point on axis The coordinates of the box may be moved at the end of each increment using the UADAPBOX user subroutine or the box may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block. -19: Node location within a Cylindrical Region Subdivision criteria is the same as Type 19. If all nodes of element leave the cylinder, the subdivided elements are merged together. The coordinates of the cylinder may be moved at the end of each increment using the UADAPBOX user subroutine or the cylinder may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block. 20: Node location within a Spherical Region Subdivide element if at least one of the nodes: f1 = radius f2 = x-coordinate of center f3 = y-coordinate of center f4 = z-coordinate of center

Main Index

262 ADAPTIVE Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry The coordinates of the box may be moved at the end of each increment using the UADAPBOX user subroutine or the box may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block. -20: Node location within Spherical Region Subdivision criteria is the same as Type 20. If all nodes of element leave the sphere, the subdivided elements are merged together. The coordinates of the sphere may be moved at the end of each increment using the UADAPBOX user subroutine or the sphere may be automatically created and moved based on the 3rd and 4th fields of the 3rd data block.

6-10

2nd

I

Enter the maximum number of levels to adapt an element.

11-15

3rd

I

Enter 3 for box associated with criteria 4 or -4 to automatically follow weld pool.

16-20

4th

I

Enter the weld flux ID specified in the WELD FLUX option.

21-25

5th

I

Not used.

26-30

6th

I

Not used.

31-63

7th

A

Enter the name of the element set that will use this criteria. Default is to apply the adaptive criteria to all elements.

Fields 3 and 4 are currently only used for the NODE IN BOX criterion in conjunction with a welding analysis. Weld pool dimensions should be specified in the WELD FLUX option. Box dimensions specified in the 4th data block below are not used. 4th data block (except for criteria type 11)

Main Index

1-10

1st

E

First parameter f1

11-20

2nd

E

Second parameter f2

21-30

3rd

E

Third parameter f3

31-40

4th

E

Fourth parameter f4

41-50

5th

E

Fifth parameter f5

ADAPTIVE 263 Define Error Criteria Used in Adaptive Analysis

Format Fixed

Free

Data Entry Entry

51-60

6th

E

Sixth parameter f6

61-70

7th

E

Seventh parameter f7

71-80

8th

E

Eighth parameter f8.

4th data block (criteria type 11) Include the data file written by the previous analysis (the unit number was specified on the second data block).

Main Index

264 ADAPT GLOBAL (Model Definition) Define Meshing Parameters Used in Global Remeshing

ADAPT GLOBAL (Model Define Meshing Parameters Used in Global Remeshing Definition) Description This model definition set provides control parameters used for the global remeshing. The REZONING parameter must also be included in the parameter section. The ADAPT GLOBAL model definition option can also be used to support boundary conditions assigned to the remeshing body for 2-D, 3-D solid (tetrahedral) and 3-D shell. When applying boundary conditions, the new table style input format is preferred. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the words ADAPT GLOBAL.

2nd data block 1-5

1st

I

Enter the number of bodies to be remeshed.

6-10

2nd

I

Enter the unit number to read data; defaults to input.

11-15

3rd

I

Not used.

The 3rd through 5th data blocks are repeated as a set for each body to be remeshed. 3rd data block 1-5

1st

I

Enter 2 for Advancing Front 2-D quad or mixed mesher. Enter 3 for Delaunay 2-D mesher. Enter 4 for 2-D Overlay mesher. Enter 5 for 3-D Overlay Hexahedral mesher. Enter 6 for Delaunay 3-D tetrahedral mesher. Enter 7 for Relax mesh generator. Enter 8 for Stretch mesh generator. Enter 9 for Shave mesh generator. Enter 10 for quadtree mesher. (FEMUTEC externally supplied) Enter 11 for MD Patran 3-D tetrahedral meshers. Enter 12 for triangular shell mesh generator. Enter 18 for reading new mesh from .mesh file. Note:

Main Index

jobid_b*.mesh file name is expected where * is the remeshing body number and jobid is the job name.

ADAPT GLOBAL (Model Definition) 265 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry Enter 19 for quadrilateral shell mesh generator.

6-10

2nd

I

Enter 1 to remesh body (default). Enter 2 if first relax mesh; if that fails, do full remeshing. Enter 3 if relax mesh only.

11-15

3rd

I

Enter the body to be remeshed (default = 1).

16-20

4th

I

Enter the element type; default is to previous element type. Note:

This element type must also be specified on the ELEMENTS parameter.

21-25

5th

I

Enter the number of criteria.

26-30

6h

I

Not used; enter 0.

31-35

7th

I

Echo mode for Overlay Hexahedral Meshing 0 Default; no message print out. 1 Some message print out. 100 Prints out more messages and saves all the meshing input files. For details about these files, see Appendix I: 3-D Remeshing Files.

Repeat the 4th block for each criteria (5th field, 3rd data block). 4th data block 1-5

1st

I

Enter 1 if increment frequency is used. Enter 2 if element distortion is used (2-D only). Enter 3 if angle based. Enter 4 if aspect ratio based. Enter 5 if strain change. Enter 6 if penetration based. Enter 7 if force remeshing at next opportunity. Enter 8 if recession distance based.

6-10

2nd

I

Enter the frequency in increments if criteria 1.

11-20

3rd

E

For criteria 3, enter maximum change in angle from the reference angle for quadrilaterals. Default is 40°. The reference angle is the angle of the current mesh without deformation. For 3-D analysis, enter minimum volume ratio for hexahedral element. Default is 0.1. For criteria 4, enter the maximum aspect ratio allowed. Default is 10.0. For criteria 5, enter maximum change of equivalent strain allowed before remeshing occurs.

Main Index

266 ADAPT GLOBAL (Model Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry Default is 0.4. For criteria 6, enter the penetration limit; default is 2*contact tolerance. For criteria 8, enter the maximum element side reduction fraction before remeshing occurs. If current length divided by the original length < tolerance, remeshing will occur.

21-30

4th

E

For criteria 3, enter maximum change in angle from the reference angle for triangles. Default is 40°. The reference angle is the angle of the current mesh without deformation. For 3-D analysis, enter minimum volume ratio for tetrahedral element. Default is 0.1. For criteria 8, enter the total amount of recession before remeshing occurs.

5th data block (Two-dimensional Advancing Front All Quadrilateral or Mixed Mesher) Mesher type = 2 1-5

1st

I

Enter 0 for all quadrilateral mesh. Enter 1 for mixed quadrilateral/triangular mesh. Enter 2 for all triangular mesh.

6-15

2nd

E

Enter the target element size.

16-25

3rd

E

Enter outline vertex angle of the two adjacent segments. (Default = 120°)

26-30

4th

I

Target number of elements after remeshing; default means no such control. If both the 2nd and 4th fields are default, the number of elements in the previous mesh are used.

31-35

5th

I

Curvature outline control. Enter number of divisions of line segments to fit a curvature circle. Default = 36. Enter -1 to obtain uniform outline points.

Main Index

36-45

6th

E

Outline smoothing ratio range 0 - 1.0; default = 0.8.

46-55

7th

E

Minimum target element size; default = 1/3*target element size.

56-65

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

66-75

9th

E

Not used; enter 0.

76-80

10th

I

Number of local refinement boxes.

ADAPT GLOBAL (Model Definition) 267 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

5th data block (Two-dimensional Delaunay Triangular Mesher) Mesher type = 3 1-5

1st

I

Not used; enter 0.

6-15

2nd

E

Enter the target element size.

16-25

3rd

E

Enter outline vertex angle of the two adjacent segments (default 120°).

26-30

4th

I

Target number of elements after remeshing; default means no such control.

31-35

5th

I

Curvature outline control. Enter number of divisions of line segments to fit a curvature circle. Default = 36. Enter -1 to obtain uniform outline points.

36-45

6th

E

Outline smoothing ratio range 0-1.0; default = 0.8.

46-55

7th

E

Minimum target element size; default = 1/3*target element size.

56-65

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

66-75

9th

E

Not used; enter 0.

76-80

10th

I

Number of local refinement boxes.

5th data block (Two-dimensional Overlay Quadrilateral Mesher) Mesher type = 4 1-10

1st

E

Enter the element target length.

11-15

2nd

I

Enter 1 if elements on the boundary in contact are to be refined one level if necessary. Enter 2 if elements on the boundary in contact are to be refined two levels if necessary.

Main Index

16-20

3rd

I

Enter 1 if elements in the interior can be merged together. Four elements at a time will be merged.

21-25

4th

I

Target number of elements after remeshing; default means no such control.

26-30

5th

I

Not used; enter 0.

31-40

6th

E

Not used; enter 0.

41-50

7th

E

Not used; enter 0.

51-60

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

268 ADAPT GLOBAL (Model Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

5th data block (Three-dimensional Delaunay Tetrahedral Mesher) Mesher type = 6 1-10

1st

E

Enter target atom size (A).

11-20

2nd

E

Enter edge parameter (value is between 0.0 and 1.0). A value of 1 means that all element edges between elements not in the same plane will be considered a hard edge.

21-30

3rd

E

Minimum edge length.

31-40

4th

E

Minimum edge angle.

41-50

5th

E

Gap distance.

51-55

6th

I

Not used; enter 0.

56-60

7th

I

Enter 1 for volume control.

5th data block (Relax Mesh Generator) Mesher type = 7 1-5

1st

I

Enter the number of relaxes to be performed.

6-10

2nd

I

Enter the global direction to relax in, default is all directions.

11-20

3rd

E

Enter the sweep distance, nodes closer than this distance will be swept together.

5th data block (Stretch Generator) Mesher type = 8 1-5

1st

I

Enter the first corner node number, if zero, then the second field gives the streamline region that is used to define the stretching orientation.

6-10

2nd

I

Enter the node increment in first direction, or the streamline region number.

11-15

3rd

I

Enter number of nodes in first direction. Enter the contact body which if nodes contact, they should not be adjusted, if zero all nodes will be adjusted.

16-20

4th

I

Enter the node increment in second direction.

21-25

5th

I

Enter the number of nodes in second direction.

26-30

6th

I

Enter the node increment in third direction (3-D only).

31-35

7th

I

Enter the number of nodes in third direction (3-D only).

5th data block (Shave Mesh Generator) Mesher type = 9 This 5th data block is not required. 5th data block (Three-dimensional MD Patran Tetrahedral Mesher) Mesher type = 11

Main Index

1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

ADAPT GLOBAL (Model Definition) 269 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Number of local refinement boxes; default = 0.

56-60

7th

I

Enter 1 for volume control; default = 1.

61-65

8th

I

Curvature refinement control. Enter number of division to fit a curvature cycle. Default = 0 (no such control).

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Three-dimensional Triangular Shell Mesher) Mesher type = 12 1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Number of local refinement boxes; default = 0.

56-60

7th

I

Not used; enter 0.

61-65

8th

I

Curvature refinement control. Enter number of division to fit a curvature cycle. Default = 0 (no such control).

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Three-dimensional Triangular Shell Mesher) Mesher type = 19

Main Index

1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Not used; enter 0.

56-60

7th

I

Not used; enter 0.

270 ADAPT GLOBAL (Model Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

61-65

8th

I

Not used; enter 0.

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Reading .mesh file) Mesher type = 18 1-10

1st

I

Enter mesh file type. Default = 3. Enter 1 for mesh file in .t18 format Enter 2 for mesh file in .feb format Enter 3 for mesh file in .dat format (Marc input format)

5th data block (Three-dimensional Overlay Hexahedral Mesher) Mesher type = 5 1-10

1st

E

Enter target atom size (Ax). For cylindrical grid, Ar.

11-20

2nd

E

Enter target atom size (Ay). For cylindrical grid, AË.

21-30

3rd

E

Enter target atom size (Az).

31-40

4th

E

Enter edge parameter (value is between 0.0 and 1.0). A value of 1 means that all element edges between elements not in the same plane will be considered a hard edge.

41-50

5th

E

Minimum edge length. If an edge length is less than this value, it will not be considered as a hard edge.

51-60

6th

E

Minimum edge angle. If the angle between element faces is less than this value, the common edge will not be considered as a hard edge.

61-70

7th

E

Gap distance.

71-75

8th

I

The template file name is specified on the 9th data block. Enter 1 if grid-based template Enter 2 if mesh-based template. Enter 3 if kernel-based template.

76-80

9th

I

Enter 1 for volume control.

6th data block (Two-dimensional Advancing Front or Delaunay Mesher [If refinement boxes are used]) Repeat for each box (6th field, 5th data block) 1-5

1st

I

Enter refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in box.

Main Index

ADAPT GLOBAL (Model Definition) 271 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Body ID 1. if not zero, corner 1 will be attached to this rigid body.

16-20

4th

I

Body ID 2. if not zero, corner 2 will be attached to this rigid body.

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

8th

F

Enter x coordinate of corner 2.

51-60

9th

F

Enter y coordinate of corner 2.

6th data block (Three-dimensional MD Patran Tetrahedral Mesher [If refinement boxes are used]) Repeat for each box (6th field, 5th data block) 1-5

1st

I

Enter refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in box.

11-15

3rd

I

Body ID 1. If not 0, corner 1 will be attached to this rigid body.

16-20

4th

I

Body ID 2. If not 0, corner 2 will be attached to this rigid body.

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

7th

F

Enter z coordinate of corner 1.

51-60

8th

F

Enter x coordinate of corner 2.

61-70

9th

F

Enter y coordinate of corner 2.

71-80

10th

F

Enter z coordinate of corner 2.

6th data block (Two-dimensional Quadtree Mesher or 3-D Hexahedral Mesher) 1-5

1st

I

Number of boxes used for element refinement; entered on 10th series.

6-10

2nd

I

Enter number of levels to coarsen (merge) the interior elements.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 0 for no wedge elements Enter 1 to allow wedge elements. Enter to split hexahedral elements.

31-35

7th

I

Enter 1 to perform shuffle after mesh is snapped to contact surface (default). Enter 2 to avoid shuffle.

Main Index

272 ADAPT GLOBAL (Model Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

36-40

8th

I

Enter 1 for Coons projection in meshing phase. This improves the accuracy, but increases the cost.

41-45

9th

I

Number of shakes. Default is 10.

46-50

10th

I

Number of tries. Default is 5.

51-55

11th

I

Type of enhancement.

56-60

12th

I

Edge detection: Enter 0 to detect new edges and use contact data. Enter 1 to use contact data only. Enter 2 to detect new edges. Enter 3 to not use edge information. Enter 4 to use previously detected edges, new edges, and contact information. Enter 5 to use contact data and previous edges. Enter 6 to use user edges previously detected and new edges. Enter 7 to use previous edge information only.

7th data block (Three-dimensional Overlay Hexahedral Mesher Only) 1-5

1st

I

Grid type: Enter 1 for Cartesian (default). Enter 2 for cylindrical. Enter 3 for user defined.

6-10

2nd

I

For cylindrical grid: Enter 1 for axis aligned with x-direction. Enter 2 for axis aligned with y-direction. Enter 3 for axis aligned with z-direction.

11-15

3rd

I

Maximum allowed refinement levels.

16-20

4th

I

First user-defined integer parameter.

21-25

5th

I

Second user-defined integer parameter.

26-30

6th

I

Third user-defined integer parameter.

8th data block (Three-dimensional Overlay Hexahedral Mesher Only [Version 11 only])

Main Index

1-10

1st

F

For cylindrical grid, enter the angle of the part.

11-20

2nd

F

Enter the geometric refinement tolerance.

21-30

3rd

F

Enter the surface curvature tolerance.

ADAPT GLOBAL (Model Definition) 273 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

31-40

4th

F

First user-defined real parameter.

41-50

5th

F

Second user-defined real parameter.

51-60

6th

F

Third user-defined real parameter.

9th data block (Three-dimensional Overlay Hexahedral Mesher Only and Template-based Mesh Requested) 1-32

1st

A

Enter the template name.

10th data block (Three-dimensional Overlay Hexahedral Mesher [if refinement boxes are used]) One can either specify that refinement is in a box based upon coordinate positions or between two bodies. Repeat for each box (1st field, 6th data block) 1-5

1st

I

Enter the refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in the box. 1 = minimum number of elements in x-direction between bodies. 2 = minimum number of elements in y-direction between bodies. 3 = minimum number of elements in z-direction between bodies. 4 = exact number of elements in x-direction between bodies. 5 = exact number of elements in y-direction between bodies. 6 = exact number of elements in z-direction between bodies.

Main Index

11-15

3rd

I

Body ID 1. If refinement is in the box, corner 1 is attached to this rigid body

16-20

4th

I

Body ID 2. If refinement is in the box, corner 2 is attached to this rigid body

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

7th

F

Enter z coordinate of corner 1.

51-60

8th

F

Enter x coordinate of corner 2.

61-70

9th

F

Enter y coordinate of corner 2.

71-80

10th

F

Enter z coordinate of corner 2.

274 POINTS Define Geometric Points

POINTS

Define Geometric Points

Description These geometrical entities are used with the ADAPTIVE, ADAPT GLOBAL, or for prescribing boundary conditions. Finite elements entities are associated with these geometric entities using the ATTACH NODE options. The use of POINTS with these options has the following consequences: 1. ADAPT GLOBAL, ATTACH NODE If a node is attached to a point entity, then this point is considered a hard point. Upon remeshing, a new node will always be located at this point. This facilitates the application of fixed displacements, point loads, etc. 2. ATTACH NODE and all nodal based boundary conditions If a nodal boundary condition such as a point load or fixed displacement is applied to the point, then all nodes attached to the point will have the boundary condition applied. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word POINTS.

2nd data block 1-5

1st

I

Enter the number of points to be defined.

6-10

2nd

I

Enter the unit number to read geometric information, defaults to input.

3rd data block (Repeat for each point)

Main Index

1-5

1st

I

Point identifier

6-15

2nd

E

X-coordinate of point.

16-25

3rd

E

Y-coordinate of point.

26-35

4th

E

Z-coordinate of point.

CURVES 275 Define Geometric Curves

CURVES

Define Geometric Curves

Description These geometrical entities are used with the ADAPTIVE, ADAPT GLOBAL, or for prescribing boundary conditions. Finite elements entities are associated with these geometric entities using the ATTACH NODE or ATTACH EDGE options. The use of CURVES with these options has the following consequences: 1. ADAPTIVE, ATTACH NODE, ATTACH EDGE, ELASTIC If the nodes of an element edge (2-D) are attached to a curve then if this element is subdivided, the newly created node will be placed on the curve. If ATTACH NODE or ATTACH EDGE are not used, the newly created nodes are placed midway between the original nodes of this edge (face). 2. ATTACH EDGE and all boundary condition options Distributed loads, foundations, and films may be applied to curves. All finite elements that have edges attached to these curves will be appropriately loaded. 3. ATTACH NODE and all nodal based boundary conditions If a nodal boundary condition such as a point load or fixed displacement is applied to the curve, then all nodes that are attached to the curve will have the boundary condition applied. 4. ADAPT GLOBAL If boundary conditions are applied to a curve, then, when a new mesh is created using ADAPT GLOBAL, the edges are reattached to the curves automatically and the boundary conditions are correctly applied. 5. CAVITY The CAVITY option may use curves defined here as symmetry surfaces. You can either directly enter the coordinates/dimensions of the curves or define geometric point entities and then reference these point entities using negative curve types. In the following pages, this is called relational input and is available for 2-D Polylines, Circular Arc, Circle, 2-D NURBS (internally generated). This is the preferred input style. Orientation A curve has an orientation associated with it. This has three consequences: 1. If a table has an independent value of arc length and elements are attached to this curve. The arc length is a monotonically increasing function which has a value of zero at the beginning of the curve.

Main Index

276 CURVES Define Geometric Curves

2. If an axisymmetric shell or 2-D beam is attached to the curve, and a distributed boundary condition is applied to the curve, then for mechanical loads: a. a positive load on the top surface is in the direction opposite to the normal, b. a positive load on the bottom surface is in the direction of the normal. for thermal loads: a. a positive load on the top surface is a flux added to the first degree of freedom, b. a positive load on the bottom surface is a flux added to the last degree of freedom. 3. A radiating cavity has an orientation based upon the normal to the surface. The normal to a curve is based upon the right-hand rule relative to the direction of the curve. When specifying the top and bottom surfaces of a curve, the following format is used in the ATTACH EDGE, DIST LOADS, FILMS, FOUNDATION, EMISSIVITY, and CAVITY options. Marc

Mentat

top

1

0

bottom

2

1

Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word CURVES.

2nd data block 1-5

1st

I

Enter the number of curves to be defined.

6-10

2nd

I

Enter the unit number to read geometric information; defaults to input.

3rd data block 1-5

1st

I

Curve identifier

6-10

2nd

I

Enter the curve type: 1: 3-D Polyline 2: 2-D Circular Arc 3: 2-D Circle 4: 2-D NURBS Curve (full description)

Main Index

CURVES 277 Define Geometric Curves

Format Fixed

Free

Data Entry Entry 5: 2-D NURBS Curve (internally generate) 6: 3-D Trimming Curve If the curve type is a negative number, it uses relational input format.

A. CURVE TYPE 1 FOR 3-D POLYLINE For nonrelational input, use data block series 4a and 5a. For relational input, use data block 4b. 4a data block 1-5

1st

I

Number of points on polyline.

5a data block (nonrelational input) Enter the coordinate points, one per line. 1-10

1st

E

X-coordinate.

11-20

2nd

E

Y-coordinate.

21-30

3rd

E

Z-coordinate.

5b data block (relational input) Enter a list of point identifiers making up the polyline. B. CURVE TYPE 2 FOR 2-D CIRCULAR ARC (in x-y plane) 4a data block (nonrelational input) 1-10

1st

E

X-coordinate of starting point.

11-20

2nd

E

Y-coordinate of starting point.

21-30

3rd

E

X-coordinate of ending point.

31-30

4th

E

Y-coordinate of ending point.

41-50

5th

E

X-coordinate of center.

51-60

6th

E

Y-coordinate of center.

61-70

7th

E

Radius.

4b data block (relational input) 1-5

1st

I

Enter point identifier of starting point.

6-10

2nd

I

Enter point identifier of ending point.

11-15

3rd

I

Enter point identifier of center.

C. CURVE TYPE 3 FOR 2-D CIRCLE (in x-y plane) 4a data block (nonrelational input)

Main Index

1-10

1st

E

X-coordinate of center.

11-20

2nd

E

Y-coordinate of center.

21-30

3rd

E

Radius.

278 CURVES Define Geometric Curves

Format Fixed

Free

Data Entry Entry

4b data block (relational input) 1-5

1st

I

Enter point identifier of center.

6-10

2nd

I

Enter point identifier of point whose first coordinate is the radius.

D. CURVE TYPE 4 FOR 2-D NURBS - FULL DESCRIPTION 4th data block 1-5

1st

I

Number of control points (NPU).

6-10

2nd

I

Order of NURBS (NOU).

5th data block Enter NPU homogeneous coordinates in E10 format (8 per line); use as many lines as necessary. The homogeneous coordinates are between 0 and 1. 6th data block Enter (NPU plus NOU) knot vectors in E10 format (8 per line); use as many lines as necessary. The components of the knot vector are between 0 and 1. 7a data block (nonrelational input) Enter the physical coordinates of control points - 1 control point per line (3 coordinates). There should be NPU lines. 1-10

1st

E

X-coordinate of control point.

11-20

2nd

E

Y-coordinate of control point.

21-30

3rd

E

Z-coordinate of control point.

7b data block (relational input) Enter NPU point identifiers in I5 format (16 per line); use as many lines as necessary. E. CURVE TYPE 5 FOR 2-D NURBS - INTERNALLY GENERATED For nonrelational input, use data block series 4a and 5a. For relational input, use data block 4b 4a data block 1-5

1st

I

Number of control points (NPU); minimum number is four.

5a data block Enter the physical coordinates of control points - 1 control point per line (3 coordinates). There should be NPU lines. 1-10

1st

E

X-coordinate of control point.

11-20

2nd

E

Y-coordinate of control point.

21-30

3rd

E

Z-coordinate of control point.

4b data block Enter a list of control point identifiers; minimum number is four.

Main Index

CURVES 279 Define Geometric Curves

Format Fixed

Free

Data Entry Entry

F. CURVE TYPE 6 FOR 3-D TRIMMNG CURVE 4th data block 1-5

1st

I

Number of control points (NPU).

6-10

2nd

I

Order of NURBS (NOU).

5th data block Enter NPU homogeneous coordinates in E10 format (8 per line); use as many lines as necessary. The homogeneous coordinates are between 0 and 1. 6th data block Enter (NPU plus NOU) knot vectors in E10 format (8 per line); use as many lines as necessary. The components of the knot vector are between 0 and 1. 7a data block (nonrelational input) Enter the physical parametric and coordinates of control points - 1 control point per line (5 coordinates). There should be NPU lines. 1-10

1st

E

X-coordinate of control point.

11-20

2nd

E

Y-coordinate of control point.

21-30

3rd

E

Z-coordinate of control point.

30-40

4th

E

Enter first parametric coordinate with respect to the surface that this curve trims.

41-50

5th

E

Enter second parametric coordinate.

7b data block (relational input) For point identifiers and parametric coordinates with respect to the surface that this curve trims. There should be NPU lines.

Main Index

1-5

1st

I

Enter point identifier.

6-15

2nd

E

Enter first parametric coordinate with respect to the surface that this curve trims.

280 SURFACES Define Geometrical Surfaces

SURFACES

Define Geometrical Surfaces

Description These geometrical entities are used with the ADAPTIVE, ADAPT GLOBAL, or for prescribing boundary conditions. Finite elements entities are associated with these geometric entities using the ATTACH NODE or ATTACH FACE options. The use of CURVES with these options has the following consequences: 1. ADAPTIVE, ATTACH NODE, ATTACH FACE, ELASTIC If the nodes of an element face (3-D) are attached to a surface then if this element is subdivided, the newly created node will be placed on the surface. If ATTACH NODE or ATTACH FACE are not used, the newly created nodes are placed midway between the original nodes of this face. 2. ATTACH FACE and all boundary condition options Distributed loads, foundations, and films may be applied to surfaces. All finite elements that have faces attached to these surfaces will be appropriately loaded. 3. ATTACH NODE and all nodal based boundary conditions If a nodal boundary condition such as a point load or fixed displacement is applied to the surface, then all nodes that are attached to the surface will have the boundary condition applied. 4. The CAVITY option may use surfaces defined here to define symmetry surfaces. You can either directly enter the coordinates/dimensions of the surfaces or define geometric point entities and then reference these point entities, use negative surface types. In the following pages, this is called relational input and is available for Plane, Sphere, Cylinder, 3-D NURBS (internally generated), and Polysurface. This is the preferred input style. Orientation A curve has an orientation associated with it. This has three consequences: 1. If a table has an independent value of arc length and elements are attached to this curve. The arc length is a monotonically increasing function which has a value of zero at the beginning of the curve. 2. If an axisymmetric shell or 2-D beam is attached to the curve, and a distributed boundary condition is applied to the curve, then for mechanical loads: a. a positive load on the top surface is in the direction opposite to the normal, b. a positive load on the bottom surface is in the direction of the normal. for thermal loads: a. a positive load on the top surface is a flux added to the first DOF, b. a positive load on the bottom surface is a flux added to the last DOF. 3. A radiating cavity has an orientation based upon the normal to the surface.

Main Index

SURFACES 281 Define Geometrical Surfaces

The normal to a curve is based upon the right hand rule relative to the direction of the curve. When specifying the top and bottom surfaces of a curve, the following format is used in the ATTACH FACE, DIST LOADS, FILMS, FOUNDATION, EMISSIVITY, and CAVITY options.

Marc

Mentat

top

1

0

bottom

2

1

Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word SURFACES.

2nd data block 1-5

1st

I

Enter the number of surfaces to be defined.

6-10

2nd

I

Enter the unit number to read geometric information; defaults to input.

3rd data block 1-5

1st

I

Surface identifier

6-10

2nd

I

Enter the surface type: 1: Plane 2: Sphere 3: Cylinder 4: NURBS Surface (full description) 5: NURBS Surface (internally generate) 6: 3-D Polysurface If the surface type is a negative number, it uses relational input format.

A. SURFACE TYPE 1 FOR PLANE 4a data block (nonrelational input) Enter coordinates at four points; one point per line.

Main Index

1-10

1st

E

X-coordinate.

11-20

2nd

E

Y-coordinate.

21-30

3rd

E

Z-coordinate.

282 SURFACES Define Geometrical Surfaces

Format Fixed

Free

Data Entry Entry

4b data block (relational input) 1-5

1st

I

Enter the first point identifier.

6-10

2nd

I

Enter the second point identifier.

11-15

3rd

I

Enter the third point identifier.

16-20

4th

I

Enter the fourth point identifier.

B. SURFACE TYPE 2 FOR SPHERE 4a data block (nonrelational input) 1-10

1st

E

X-coordinate of center.

11-20

2nd

E

Y-coordinate of center.

21-30

3rd

E

Z-coordinate of center.

31-40

4th

E

Radius.

4b data block (relational input) 1-5

1st

I

Enter the point identifier of the center.

6-10

2nd

I

Enter the point identifier of a point whose first coordinate is the radius.

C. SURFACE TYPE 3 FOR CYLINDER/CONE 4a data block (nonrelational input) 1-10

1st

E

X-coordinate of starting point on axis.

11-20

2nd

E

Y-coordinate of starting point on axis.

21-30

3rd

E

Z-coordinate of starting point on axis.

31-40

4th

E

Radius at starting point.

41-50

5th

E

X-coordinate of ending point on axis.

51-60

6th

E

Y-coordinate of ending point on axis.

61-70

7th

E

Z-coordinate of ending point on axis.

71-80

8th

E

Radius at ending point.

4b data block (relational input)

Main Index

1-5

1st

I

Enter the point identifier of the starting point on the axis.

6-10

2nd

I

Enter the point identifier of a point whose first coordinate is the radius at the start point.

11-15

3rd

I

Enter the point identifier of the endpoint on the axis.

16-20

4th

I

Enter the point identifier of a point whose first coordinate is the radius at the endpoint.

SURFACES 283 Define Geometrical Surfaces

Format Fixed

Free

Data Entry Entry

D. SURFACE TYPE 4 FOR 3-D NURBS – FULL DESCRIPTION 4th data block 1-5

1st

I

Number of control points in first direction (NPU).

6-10

2nd

I

Order of NURBS in first direction (NOU).

11-15

3rd

I

Number of control points in second direction (NPV).

16-20

4th

I

Order of NURBS in second direction (NOV).

21-25

5th

I

Enter the number of trimming curves (NTRIM).

5th data block Enter NPU times NPV homogeneous coordinates in E10 format (8 per line); use as many lines as necessary. The homogeneous coordinates are between 0 and 1. 6th data block Enter (NPU plus NOU) plus (NPV plus NOV) knot vectors in E10 format (8 per line); use as many lines as necessary. The components of the knot vector are between 0 and 1. 7a data block (nonrelational input) Enter the physical coordinates of NPU times NPV control points 1 control point per line (3 coordinates). There should be NPU times NPV lines. 1-10

1st

E

X-coordinate of control point.

11-20

2nd

E

Y-coordinate of control point.

21-30

3rd

E

Z-coordinate of control point.

7b data block (relational input) Enter NPU times NPV point identifiers of the control points in I5 format (16 per line); use as many lines as necessary. 8th data block Enter NTRIM curve identifiers in I5 format (16 per line); use as many lines as necessary. Note these curves should have previously defined using the CURVES model definition option with a curve type of six. E. SURFACE TYPE 5 FOR 3-D NURBS – INTERNALLY GENERATED 4th data block 1-5

1st

I

Number of control points in first direction (NPU). Minimum is 4.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Number of control points in second direction (NPV). Minimum is 4.

Main Index

284 SURFACES Define Geometrical Surfaces

Format Fixed

Free

Data Entry Entry

5a data block (nonrelational input) Enter the physical coordinates of NPU times NPV control points 1 control point per line (3 coordinates). There should be NPU times NPV lines. 1-10

1st

E

X-coordinate of control point.

11-20

2nd

E

Y-coordinate of control point.

21-30

3rd

E

Z-coordinate of control point.

5b data block (relational input) Enter NPV lists of control point identifiers. Each list must have NPU points. F. SURFACE TYPE 6 FOR 3-D POLYSURFACE For 3-D polysurface, use the 4a, 5a, and 6a data blocks for nonrelational input. For 3-D polysurface, use the 4b and 5b data blocks for relational input. 4a data block 1-5

1st

I

Number of Polygons.

6-10

2nd

I

Number of Polygon vertices.

5a data block The 5a data block is repeated for each polygon. 1-5

1st

I

Polygon ID.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

First vertex ID.

16-20

4th

I

Second vertex ID.

21-25

5th

I

Third vertex ID.

26-30

6th

I

Fourth vertex ID (if zero, then polygon is a triangle).

6a data block The 6a data block is repeated for each vertex point. 1-5

1st

I

Vertex ID.

6-15

2nd

E

Enter the X-coordinate of vertex.

16-25

3rd

E

Enter the Y-coordinate of vertex.

26-35

4th

E

Enter the Z-coordinate of vertex.

I

Number of polygons.

4b data block 1-5

Main Index

1st

SURFACES 285 Define Geometrical Surfaces

Format Fixed

Free

Data Entry Entry

5b data block The 5b data block is repeated for each polygon. 1-5

1st

I

Polygon ID.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter point identifier for first vertex of polygon.

16-20

4th

I

Enter point identifier for second vertex of polygon.

21-25

5th

I

Enter point identifier for third vertex of polygon.

26-30

6th

I

Enter point identifier for fourth vertex of polygon. If zero, this polygon is a triangle.

Main Index

286 STRING Define Curves Forming a String for Arc Length Calculation

STRING

Define Curves Forming a String for Arc Length Calculation

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows the user to associates a number of curves together, in a fixed order so that a continuous arc length may be created. This arc length could be used as an independent variable in the TABLE option. Note that the curves themselves do not need to match coordinates at their endpoints. The STRING option indicates that they are “topologically” continuous. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word STRING.

I

Enter the number of strings.

2nd data block 1-5

1st

Data blocks 3 and 4 are repeated for each string. 3rd data block 1-5

1st

I

Enter the string ID.

I

Enter a list of curves in the string. List must be in correct order.

4th data block 1-80

1st

List verbs EXCEPT and INTERSECT are illegal here. As an example; given three parts with six curves, the string option could be used.

Main Index

STRING 287 Define Curves Forming a String for Arc Length Calculation

String 2, 1, 1,3,5, 2, 2,4,6, For the outer surface (string number 1), the cap has a radius r = 1.0, so for points along curve 1, the arc length goes from 0. to 1.5708, along curve 3 from 1.5708 to 2.5708, and along curve 5 from 2.5708 to 3.0707.

Main Index

288 ATTACH NODE Define the Nodes Attached to Surfaces

ATTACH NODE

Define the Nodes Attached to Surfaces

Description This option allows you to attach nodes to a point, curve, or surface. This option is used for ADAPTIVE meshing and/or application of boundary conditions. When used in conjunction with adaptive mesh analysis, if two points on an edge of an element are attached to a curve or surface, any new points created by the adaptive procedure are placed on the curve. This improves the geometric modeling. Note:

In the case of Updated Lagrange or if no surface is defined, the new nodes are placed midway between the previous nodes.

When used with boundary conditions if a nodal load (POINT LOAD, POINT FLUX, etc.) is applied to a point/curve/surface, the nodes attached to this point/curve/surface will all receive this same load. If a kinematic boundary condition (FIXED DISP, FIXED TEMPERATURE, etc.) is applied to a point/curve/surface, the nodes attached to this point/curve/surface will be constrained to satisfy this condition. To utilize this option for the application of boundary conditions, the table driven boundary condition input must be used. See VERSION or TABLE parameter on how to activate this input option. Note that nodal boundary conditions are always applied in the transformed system, hence if some of the nodes attached to the curve have local systems, the user may need to exercise caution. A node can be attached to as many as three surfaces; any additional surfaces are ignored. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ATTACH NODE.

2nd data block 1-5

1st

I

Enter the number of data sets.

6-10

2nd

I

Enter the unit number to read data, defaults to input.

Repeat the third and possibly the fourth data block as often as necessary. You can enter a point ID, curve ID, or a surface ID on the 3rd data block. 3rd data block

Main Index

1-5

1st

I

Enter the node number if a zero is entered, the 4th data block will be used.

6-10

2nd

I

Enter a point ID.

ATTACH NODE 289 Define the Nodes Attached to Surfaces

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter a curve ID.

16-20

4th

I

Enter a surface ID.

4th data block Enter a list of nodes which are attached to this curve or surface.

Main Index

290 ATTACH EDGE Define the Element Edges Which are Attached to Curves

ATTACH EDGE

Define the Element Edges Which are Attached to Curves

Description This option allows you to attach an element edge to a curve. This option is used in conjunction with the CURVES option. To utilize this option, the table driven boundary condition input must be used. See VERSION or TABLE parameter on how to activate this input option. When used with boundary conditions if a nodal load (POINT LOAD, POINT FLUX, etc.) is applied to a curve, the nodes which define the edge that are attached to the curve will all receive this same load. If a kinematic boundary condition (FIXED DISP, FIXED TEMPERATURE, etc.) is applied to a curve, the nodes which define the edges that are attached to the curve will be constrained to satisfy this condition. When a distributed load (DIST LOADS, DIST FLUXES, etc.) is applied to a curve, the distributed load will be applied to the element edges attached the curve. Note:

Nodal boundary conditions are always applied in the transformed system, hence if some of the nodes which define edges that are attached to the curve have local systems, the user may need to exercise caution.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ATTACH EDGE.

2nd data block 1-5

1st

I

Enter the number of data sets.

6-10

2nd

I

Enter the unit number to read data, defaults to input.

11-15

3rd

I

Enter 0, if face given using Marc convention. Enter 1, if face given using Marc Mentat convention.

3rd data block 1-5

1st

I

Enter curve identifier.

I

Enter a list of element: edge pairs which are attached to this curve.

4th data block 1-80

Main Index

1st

ATTACH FACE 291 Define the Element Faces which are attached to Surfaces

ATTACH FACE

Define the Element Faces which are attached to Surfaces

Description This option allows you to attach an element face to a surface. This option is used in conjunction with the SURFACES option. To utilize this option, the table driven boundary condition input must be used. See VERSION or TABLE parameter on how to activate this input option. When used with boundary conditions if a nodal load (POINT LOAD, POINT FLUX, etc.) is applied to a surface, the nodes which define the faces that are attached to the surface will all receive this same load. If a kinematic boundary condition (FIXED DISP, FIXED TEMPERATURE, etc.) is applied to a surface, the nodes which define the faces that are attached to the surface will be constrained to satisfy this condition. When a distributed load (DIST LOADS, DIST FLUXES, etc.) is applied to a surface, the distributed load will be applied to the element faces attached the surface. Note that nodal boundary conditions are always applied in the transformed system, hence if some of the nodes which define faces that are attached to the surface have local systems, the user may need to exercise caution. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ATTACH FACE.

2nd data block 1-5

1st

I

Enter the number of data sets.

6-10

2nd

I

Enter the unit number to read data, defaults to input.

11-15

3rd

I

Enter 0, if face given using Marc convention. Enter 1, if face given using Marc Mentat convention.

3rd data block 1-5

1st

I

Enter surface identifier.

I

Enter a list of element: face pairs which are attached to this surface.

4th data block 1-80

Main Index

1st

292 GEOMETRY Specify Geometrical Data

GEOMETRY

Specify Geometrical Data

Description The element geometry is specified in distinct sets. The information required varies from one element type to another. As a rule, the thickness of shell elements is given in the first defined variable (EGEOM1). The geometry for a particular element can be defined repeatedly and only the last data is used. This feature is designed for local variations of geometric data. The GEOMETRY option is unnecessary if the element description does not require either EGEOM1, EGEOM2, or EGEOM3. (See Marc Volume B: Element Library). Notes:

The NODAL THICKNESS model definition option can also be used for the input of beam/shell thickness. For beam elements, the eighth data variable (EGEOM8) is used to indicate the use of offsets, pin codes, and coordinate system to define local x-axis. Activating this flag requires the input of additional data blocks (4 and/or 5a). For shell elements, the eighth data variable (EGEOM8) is used to indicate shell offsets. Activating this flag requires the input of the 5b data block.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word GEOMETRY.

2nd data block 1-5

1st

I

Number of distinct sets of element geometries to be input (optional).

6-10

2nd

I

Enter unit number for input of geometry defaults to input.

3rd data block Element geometries. The 3rd through 6th data blocks are entered as pairs, one for each distinct data set.

Main Index

1-10

1st

F

EGEOM1

11-20

2nd

F

EGEOM2

21-30

3rd

F

EGEOM3

31-40

4th

F

EGEOM4

41-50

5th

F

EGEOM5

51-60

6th

F

EGEOM6

61-70

7th

F

EGEOM7

GEOMETRY 293 Specify Geometrical Data

Format Fixed 71-80

Free 8th

Data Entry Entry F

EGEOM8 For beam and shells, EGEOM8 is the negative of the sum of three numbers = -(ioffset + iorien + ipin) ioffset

=

0 – no offsets. 1 – offsets with beams; include the 5a data block. 2 – offsets with shells; include the 5b data block.

iorien

=

0 – conventional definition of local beam orientation, beam axis given in 4th through 6th field in global system. 10 – the local beam orientation is given with respect to the coordinate system of the first beam node.

ipin

=

0 – no pin codes are used. 100 – pin codes are used; include the 4th data block.

Notes:

iorien and ipin are only valid for beam elements.

See library element descriptions in “Quick Reference” of Marc Volume B: Element Library for the meaning of EGEOM1, etc. for each element type. 4th data block Necessary only if ipin = 100 1-5

1st

I

Enter the pin code associated with the first node of the beam.

6-10

2nd

I

Enter the pin code associated with the second node of the beam. The degrees of freedom are defined in the element’s coordinate system and the pin flags are applied at the offset ends of the beam. The pin code is a packed integer of up to five unique integers 1 through 6 with no embedded blanks.

5a data block Necessary only if ioffset = 1

Main Index

1-10

1st

F

X component of offset vector at beam node 1

11-20

2nd

F

Y component of offset vector at beam node 1

21-30

3rd

F

Z component of offset vector at beam node 1

31-40

4th

F

X component of offset vector at beam node 2

41-50

5th

F

Y component of offset vector at beam node 2

51-60

6th

F

Z component of offset vector at beam node 2

294 GEOMETRY Specify Geometrical Data

Format Fixed 61-65

66-70

71-75

Free 7th

8th

9th

Data Entry Entry I

I

I

Interpolation flag for higher-order beams 0 –

no interpolation of offset vector for midside node (Offset vector at midside node set to 0.).

1 –

linear interpolation of offset vector for midside node

Coordinate system flag for offset vector at beam node 1 0 –

vector in global coordinate system.

1 –

vector in element coordinate system.

2 –

vector along associated shell normal at node.

3 –

vector in local coordinate system at node 1.

Coordinate system flag for offset vector at beam node 2 0 –

vector in global coordinate system

1 –

vector in element coordinate system.

2 –

vector along associated shell normal at node.

3 –

vector in local coordinate system at node 2.

5b data block Necessary only if ioffset = 2 1-10

1st

F

Offset magnitude at corner node 1

11-20

2nd

F

Offset magnitude at corner node 2

21-30

3rd

F

Offset magnitude at corner node 3

31-40

4th

F

Offset magnitude at corner node 4

41-45

5th

I

Interpolation flag for higher-order shells

46-50

6th

I

0 –

no interpolation of offset for mid-side nodes.

1

linear interpolation of offset for mid-side nodes

Constant Offset flag 0 –

offset magnitude is variable. Four data fields are used to specify offset magnitudes at corner nodes.

1 –

offset magnitude is constant. First data field is used to specify offset magnitudes at corner nodes.

6th data block Enter a list of elements to which the above geometry is applied.

Main Index

GEOMETRY 295 Specify Geometrical Data

Notes:

For elements 7, 10, 11, and 19, enter 1 in the EGEOM2 field to activate the constant dilatation option. This improves the behavior of the element for nearly incompressible analysis. See Marc Volume B: Element Library for further details. For elements 3, 7, and 11, enter 1 in the EGEOM3 field to activate the assumed strain formulation. This improves the element bending behavior. This is an alternative to the ASSUMED STRAIN parameter. For elements 109 and 110, the penalty factor used to add the constraint for the vector potential (Marc Volume A: Theory and User Information) to the set of equations for magnetostatic calculations can be set in the EGEOM2 field. For element 185, enter a value greater than 0 and less than 1 in the EGEOM5 field to scale down the transverse shear modulus for homogenous material (a common value is 5/6). Beam offset capability is possible for elements 5, 14, 25, 36, 45, 52, 65, 76, 77, 78, 79, 98. Enter -1 in the EGEOM8 field and the offset information via the 4a data block. See Marc Volume B: Element Library for further details. The components of the local x-axis for beam elements are entered in the EGEOM4-EGEOM6 fields. These components can be entered in the global Cartesian coordinate system (default) or in a local coordinate system. In the latter case, the local coordinate system used to define the beam x-axis is flagged through the EGEOM8 field and is taken to be the coordinate system defined at the first nodal point of the beam element using the TRANSFORMATION, CYLINDRICAL, or COORD SYSTEM options. Enter -10 or -11 in the EGEOM8 field to indicate that the fields EGEOM4-EGEOM6 are in the local coordinate system. If EGEOM8 is -11, it further indicates that the beam elements are offset and that the nodal offset vectors are provided via the 4a data block. Shell offset capability is possible for elements 1, 22, 50, 75, 85, 86, 87, 88, 89, 138, 139, 140. Enter -2 in the EGEOM8 field and the offset information via the 4b data block. See Marc Volume B: Element Library for further details.

Main Index

296 NODAL THICKNESS Define Nodal Thickness

NODAL THICKNESS

Define Nodal Thickness

Description This option allows you to specify beam or shell thicknesses on a nodal basis. Interpolation to the element integration points is automatically taken care of using the element displacement shape functions as discussed for each element in Marc Volume B: Element Library. Notes:

If you specify element thicknesses for an element using the GEOMETRY model definition option, that data is used instead of the NODAL THICKNESS data input here. Also note that for composite elements, if you give the actual layer thicknesses, the sum of these layer thicknesses overrides both GEOMETRY data and NODAL THICKNESS data. If you input percentages of total thickness in the COMPOSITE data, then GEOMETRY data (or, if no GEOMETRY, then NODAL THICKNESS data from this option) is used. Since the NODAL THICKNESS option allows input of only one thickness per node, thickness discontinuities must be input using GEOMETRY. See Marc Volume B: Element Library for elements which use nodal thicknesses.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODAL THICKNESS.

2nd data block 1-5

1st

I

Number of data sets used to input nodal thickness values. The UTHICK user subroutine can be used for modifying NODAL THICKNESS values.

6-10

2nd

I

Enter the unit number for input of nodal thicknesses. Defaults to input deck.

Data blocks 3 and 4 are repeated as pairs, one for each data set. 3rd data block 1-10

1st

F

Enter nodal thickness value

4th data block Enter a list of nodes associated with the nodal thickness given above.

Main Index

ACTUATOR 297 Define the Length of the Actuator Link

ACTUATOR

Define the Length of the Actuator Link

Description This option can be used in conjunction with the truss element type 9 to simulate an actuator. This is often used in mechanism analyses to allow the prescription of the relative distance between two points. This option should be used with the LARGE DISP parameter whenever large rotations of the actuator or large displacements are anticipated. The original length of the actuator is given in the fourth field of the GEOMETRY option. The actuator is treated as an elastic link. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ACTUATOR.

2nd data block 1-5

1st

I

Enter the number of actuators (optional).

6-10

2nd

I

Enter unit number for input of actuator data. Defaults to input.

3rd data block Repeat for each actuator to be modified.

Main Index

1-5

1st

I

Enter the element number

6-15

2nd

F

Enter the new length of the actuator.

16-20

3rd

I

Enter the table ID for the length of the actuator.

298 TRANSFORMATION Define Nodal Coordinates for Transformation

TRANSFORMATION

Define Nodal Coordinates for Transformation

Description This option defines nodal coordinates for calculation of a direction cosine matrix, which is then used for transforming the global degrees of freedom of a specified node to a new local coordinate system. This block can be used to set up local coordinate systems at a number of flagged nodes, for application of boundary conditions in a transformed system, or for printout purposes. Five points should be noted: 1. The displacements and loads or reactions are output in the transformed system at such nodes. 2. The transformation is done on all Cartesian displacements. Thus, for the shell elements, the derivative degrees of freedom become the derivative of the transformed displacements with respect to the original surface coordinate system. 3. Transformations are assumed to be orthogonal. 4. All kinematic conditions such as boundary conditions, initial displacements, initial velocity and ties at that node must be input in the transformed system. 5. All concentrated nodal loads must be applied in the transformed system. Format Format Fixed

Free

Data Entry Entry

1st data block 1-14

1st

A

Enter the word TRANSFORMATION.

2nd data block 1-5

1st

I

Number of distinct sets of transformations data to be entered (optional).

6-10

2nd

I

Enter unit number for input of transformation data, defaults to input.

11-15

3rd

I

Enter 1 to suppress printout of transformation data.

The 3rd and 4th data blocks are entered as pairs, one for each distinct data set. 3rd data block

Main Index

1-5

1st

I

6-15

2nd

F

16-25

3rd

F

26-35

4th

F

Node number. Enter 0 to read a list of nodes. See 4th data block. Global coordinates of a first point A such that the vector from this point to the node is direction 1 of the local coordinate system. (See Figure 3-1a.)

TRANSFORMATION 299 Define Nodal Coordinates for Transformation

Format Fixed

Free

Data Entry Entry

36-45

5th

F

46-55

6th

F

56-66

7th

F

Global coordinates of a second point, such that this point, the first point, and the node define the 1-2 plane of the local coordinate system. Direction 2 of the local coordinate system will be constructed perpendicular to direction 1 such that this second point has a positive 2 coordinate in the local 1-2 plane. See Figure 3-1b “Three-dimensional Analysis”). Direction 3 of the local coordinate system is given by a cross product of direction 1 with direction 2.

4th data block Include only if the first field in the 3rd data block is 0. Enter a list of nodes for which the above transformation is applied. Note that for elements in a plane (for example,; 1, 2, 3, 5, 6, 10, 11, 12, 15, 16, 17, 19, etc.) only the first two coordinates of the first point (cols. 6-15 and 16-25) need be supplied. See Figure 3-1.

Main Index

300 TRANSFORMATION Define Nodal Coordinates for Transformation

TRANSFORMATION 1,

Local 1

Local 2

N,xA,yA,xB,yB Point B

Node N

Y

Point A X (a) Two-dimensional Analysis Plane defined by Node N, Point A, and Point B

TRANSFORMATION 1, N,xA,yA,zA,xB,yB,zB

Point B Local 2 Local 1 Node N Y Local 3 (= Local 1 x Local 2) Point A

Z

X (b) Three-dimensional Analysis

Figure 3-1

Main Index

Transformation Option

COORD SYSTEM 301 Define Coordinate System for Nodal Coordinates and Degrees of Freedom

COORD SYSTEM

Define Coordinate System for Nodal Coordinates and Degrees of Freedom

Description This option allows you to specify that the coordinates of a node are with respect to a local coordinate system. This is consistent with the CP identification number on the MD Nastran GRID Bulk Data Entry. This option also allows you to specify the nodal coordinate system of the degrees of freedom. This is consistent with the CD identification number on the MD Nastran GRID Bulk Data Entry. Thie coordinate systems defined here are similar to the MD Nastran CORD1R, CORD1C, CORD1S, CORD2R, CORD2C, and CORD2S options. Note that the data entered here should not be changed upon restart. Similar to the use of the TRANSFORMATION option, the following points should be noted: 1. The displacements and loads or reactions are output in the transformed system at such nodes. 2. The transformation is done on all Cartesian displacements. Thus, for the shell elements, the derivative degrees of freedom become the derivative of the transformed displacements with respect to the original surface coordinate system. 3. All kinematic conditions such as fixed displacement, initial displacements, initial velocity and ties at that node must be input in the transformed system. 4. All concentrated nodal loads must be applied in the transformed system. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words COORD SYSTEM.

2nd data block 1-5

1st

I

Enter the number of coordinate systems (not required).

6-10

2nd

I

Enter unit number of read data; defaults to input file.

A

Enter coordinate system type:

3rd data block 1-6

1st

CORD1C CORD1R CORD1S CORD2C CORD2R CORD2S

Main Index

302 COORD SYSTEM Define Coordinate System for Nodal Coordinates and Degrees of Freedom

Format Fixed 11-15

Free 2nd

Data Entry Entry I

Enter 1 if coordinates defined are with respect to the coordinate system. Enter 0 if coordinate data is not transformed based on this coordinate system.

16-20

3rd

I

Enter 1 if degrees of freedom are to be transformed based upon this coordinate system. Enter 0 if degrees of freedom are not to be transformed.

21-25

4th

I

Enter 1 if transformation is to be updated based upon the deformation of nodes G1A, G2A, and G3A for coordinate systems CORD1C, CORD1R, and CORD1S. This option should only be used with table-driven boundary conditions.

Repeat 4a and 7th data block for each CORD1:coordinate system. 4a data block Used if coordinate system type is CORD1C, CORD1R, or CORD1S; see Remarks. 1-5

1st

I

Enter coordinate system identification number; must be unique. Same as MD Nastran CIDA.

6-10

2nd

I

Enter first node number ID; same as MD Nastran G1A.

11-15

3rd

I

Enter second node number ID; same as MD Nastran G2A.

16-20

4th

I

Enter third node number ID; same as MD Nastran G3A.

Repeat 4b, 5th, 6th, and 7th data block for each CORD2:coordinate system 4b data block Used if coordinate system type is CORD2C, CORD2R, or CORD2S; see Remarks. 1-5

1st

I

Enter coordinate system identification number; must be unique. Same as MD Nastran CID.

6-10

2nd

I

Enter the coordinate system that points given below are with respect to. Default is the global coordinate system. This is the same as MD Nastran RID.

5th data block Used if coordinate system type is CORD2C, CORD2R, or CORD2S.

Main Index

1-10

1st

E

First coordinate of point A.

11-20

2nd

E

Second coordinate of point A.

21-30

3rd

E

Third coordinate of point A.

31-40

4th

E

First coordinate of point B.

41-50

5th

E

Second coordinate of point B.

51-60

6th

E

Third coordinate of point B.

COORD SYSTEM 303 Define Coordinate System for Nodal Coordinates and Degrees of Freedom

Format Fixed

Data Entry Entry

Free

6th data block Used if coordinate system type is CORD2C, CORD2R, or CORD2S. 1-10

1st

E

First coordinate of point C.

11-20

2nd

E

Second coordinate of point C.

21-30

3rd

E

Third coordinate of point C.

7th data block Enter a list of node numbers to which this system is to be applied. Remarks CORD1C z

uz

G2

G3

uθ P

G1

Z

θ

ur R

x

Figure 3-2

y

CORDIC Definition

1. GiA must be defined in coordinate systems with definitions that do not involve the coordinate system being defined. The first point is the origin, the second lies on the z-axis, and the third lies in the plane of the azimuthal origin. The three grid points GiA must be noncolinear and not coincident. 2. The location of a grid point (P in Figure 3-2) in this coordinate system is given by (R, θ, Z) where θ is measured in degrees. 3. The displacement coordinate directions at P are dependent on the location of P as shown above by ( u r, u θ, u z ) . 4. It is recommended that points on the z-axis only have their z-displacement directions defined in this coordinate system.

Main Index

304 COORD SYSTEM Define Coordinate System for Nodal Coordinates and Degrees of Freedom

CORD1R z

uz G2

P G3

uy G1

Z

ux

y X

Y

x

Figure 3-3

CORD1R Definition

1. GiA must be defined in coordinate systems with definitions that do not involve the coordinate system being defined. The first point is the origin, the second lies on the z-axis, and the third lies in the x-z plane. The three grid points GiA must be noncolinear and not coincident. 2. The location of a grid point (P in Figure 3-3) in this coordinate system is given by (X, Y, Z). 3. The displacement coordinate directions at P are shown above by

( u x, u u, u z )

.

CORD1S z

G2

uφ θ

ur P

G3 G1

φ

R

uθ

x y

Figure 3-4

CORD1S Definition

1. GiA must be defined in coordinate systems with a definition that does not involve the coordinate system being defined. The first point is the origin, the second lies on the z-axis, and the third lies in the plane of the azimuthal origin. The three grid points GiA must be noncolinear and not coincident. 2. The location of a grid point (P in Figure 3-4) in this coordinate system is given by (R, θ, φ) where θ and φ are measured in degrees.

Main Index

COORD SYSTEM 305 Define Coordinate System for Nodal Coordinates and Degrees of Freedom

3. The displacement coordinate directions at P are dependent on the location of P as shown above by ( u r, u θ, u φ ) . 4. It is recommended that points on the z-axis only have their z-displacement directions defined in this coordinate system. CORD2C z

uz

B

uθ P C A

Z

ur θ R

x

Figure 3-5

y

CORD2C Definition

1. The three points [(A1, A2, A3), (B1, B2, B3), (C1, C2, C3)] must be unique and noncolinear. Noncolinearity is checked by the geometry processor. The first point defines the origin. The second point defines the direction of the z-axis. The third lies in the plane of the azimuthal origin. The reference coordinate system must be independently defined. 2. If RID is zero or blank, the basic coordinate system is used. 3. The location of a grid point (P in Figure 3-5) in this coordinate system is given by (R, θ, Z), where θ is measured in degrees. 4. The displacement coordinate directions at P are dependent on the location of P as shown above by ( u r, u θ, u z ) . 5. It is recommended that points on the z-axis only have their z-displacement directions defined in this coordinate system.

Main Index

306 COORD SYSTEM Define Coordinate System for Nodal Coordinates and Degrees of Freedom

CORD2R z uz

B

P

uy

C A

Z

ux

y X

x

Y

Figure 3-6

CORD2R Definition

1. The three points [(A1, A2, A3), (B1, B2, B3), (C1, C2, C3)] must be unique and noncolinear. Noncolinearity is checked by the geometry processor. The first point defines the origin. The second defines the direction of the z-axis. The third point defines a vector which, with the z-axis, defines the x-z plane. The reference coordinate system must be independently defined. 2. If RID is zero or blank, the basic coordinate system is used. 3. The location of a grid point (P in the Figure 3-6) in this coordinate system is given by (X, Y, Z). 4. The displacement coordinate directions at P are shown by

( u x, u y, u z )

.

CORD2S z B

uφ θ

A

φ

x

ur

P

C R

uθ y

Figure 3-7

CORD2S Definition

1. The three points [(A1, A2, A3), (B1, B2, B3), (C1, C2, C3)] must be unique and noncolinear. Noncolinearity is checked by the geometry processor. The first point defines the origin. The second point defines the direction of the z-axis. The third lies in the plane of the azimuthal origin. The reference coordinate system must be independently defined. 2. If RID is zero or blank, the basic coordinate system is used.

Main Index

COORD SYSTEM 307 Define Coordinate System for Nodal Coordinates and Degrees of Freedom

3. The location of a grid point (P in Figure 3-7) in this coordinate system is given by (R, θ, φ), where θ and φ are measured in degrees. 4. The displacement coordinate directions at P are shown above by

( u r, u θ, u φ )

.

5. It is recommended that points on the z-axis not have their displacement directions defined in this coordinate system.

Main Index

308 SHELL TRANSFORMATION Define Shell Transformation

SHELL TRANSFORMATION

Define Shell Transformation

Description This option allows you to transform the global degrees of freedom of (doubly curved) shells or beams to local degrees of freedom. It facilitates the input of boundary conditions, point loads and bending moments. A more detailed description of this capability is given in Marc Volume A: User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-20

1st

A

Enter the words SHELL TRANSFORMATION.

I

Number of data sets to be input (optional).

I

Unit number from which input is to be read (defaults to input).

2nd data block 1-5

1st

6-10

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Transformation type (see Marc Volume A: User Information). Transformation type 1 is used for beam elements 15, 16, and 17. Transformation types 2 to 4 are used for shell elements 4, 8 and 24.

6-15

2nd

F

First component of ˆt vector in surface θ1 - θ2 coordinate system. Only needed for transformation types 2 and 4.

16-25

3rd

F

Second component of ˆt vector in surface θ1 - θ2 coordinate system. Only needed for transformation types 2 and 4.

4th data block Enter a list of nodes to which the above displacements are applied.

Main Index

UTRANFORM 309 Invoke User Subroutine UTRANS

UTRANFORM

Invoke User Subroutine UTRANS

Description This option allows you to transfer the global degrees of freedom to local degrees of freedom. This is done through the UTRANS user subroutine (see Marc Volume D: User Subroutines and Special Routines). Note:

This option should not be used on boundary nodes which can come into contact with rigid surfaces in a contact analysis.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the word UTRANFORM.

2nd data block 1-5

1st

I

Number of data sets to be input.

6-10

2nd

I

Unit number from which input is to be read. Defaults to input.

The 3rd data block is entered once for each data set. 3rd data block Enter list of node numbers to which user transformations are applied.

Main Index

310 CYCLIC SYMMETRY Enter Data for a Cyclic Symmetric Structure

CYCLIC SYMMETRY

Enter Data for a Cyclic Symmetric Structure

Description This option is used to define data for a structure possessing cyclic symmetry, which means that the geometry and the loading vary periodically around a symmetry axis. This type of structure can be effectively analyzed by modeling only one section and applying the proper multipoint constraint equations to account for the cyclic symmetry. By defining the symmetry axis and the sector angle, the Marc program sets up the constraint equations automatically. Additionally, the rigid body rotation around the symmetry axis can be automatically suppressed. Note:

Cyclic Symmetry is: a. valid for only the continuum elements. However, the presence of beams and shells is allowed, but there is no connection of shells to shells, so the shell part can, for example, be a turbine blade and the volume part can be a turbine rotor. The blade is connected to the rotor and if there are 20 blades, 1/20 of the rotor is modeled and one complete blade. b. valid for nonlinear static analysis including remeshing as well as coupled analysis. c. invalid for pure heat transfer. d. valid for all analysis involving contact. This option can be combined with the CONTACT option. In this case, both sides of the cyclic symmetry sectors need to belong to the same contact body. Note:

If used with contact and the element is not in a contact body, it is not detected as being on a symmetry surface.

e. valid also for: eigenvalue analysis such as buckling or modal analysis, harmonic analysis, and transient dynamic analysis. However, there are restrictions in the case of modal analysis which are described in more detail in Marc Volume A: Theory and User Information, Chapter 9, Cyclic Symmetry. f. valid only if used in a non-contact analysis with a mixture of element types. If a combination of beam, shell, linear continuum and/or quadratic continuum elements is present and contact is not used in the model, exit 61 is issued. To overcome this problem, two different contact bodies must be defined: one consisting of only the linear continuum elements and one consisting of only the quadratic continuum elements. Shell and/or beam elements do not have to be a part of any contact body (see a. above). Only the elements belonging to the cyclically symmetric sector need to be in a contact body. In order to prevent unwanted contact items (CPU due to unneeded contact search, unwanted contacting nodes, etc.), turn off the normal Marc contact calculations by defining an empty contact table. In this case, both sides of every cyclic symmetry sector should belong to the same body, so that it is impossible to model one side with linear continuum elements and the other side of the sector with quadratic continuum elements.

Main Index

CYCLIC SYMMETRY 311 Enter Data for a Cyclic Symmetric Structure

g. When using CYCLIC SYMMETRY in 3-D, tetrahedral elements must be used if the body is to be remeshed. h. If used with the SPLINE option, the symmetry planes.

ε'

continuity is not applied between across the

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words CYCLIC SYMMETRY.

2nd data block 1-10

1st

E

First component of the direction cosine of symmetry axis.

11-20

2nd

E

Second component of the direction cosine of symmetry axis.

21-30

3rd

E

Third component of the direction cosine of symmetry axis.

3rd data block 1-10

1st

E

X-coordinate of point on symmetry axis.

11-20

2nd

E

Y-coordinate of point on symmetry axis.

21-30

3rd

E

Z-coordinate of point on symmetry axis.

4th data block 1-10

1st

E

Cyclic angle (in degrees).

11-20

2nd

E

Cyclic Symmetry Tolerance. Default is 0.5 times of the minimum element size.

I

Enter:

5th data block 1-5

1st

-1 To automatically suppress rigid body mode. 0 To have no suppression. >0 To suppress at node number given.

Main Index

312 CYCLIC SYMMETRY Enter Data for a Cyclic Symmetric Structure

Format Fixed 6-10

Free 2nd

Data Entry Entry I

Linearization flag; to be used if a cyclic symmetric structure consists of quadratic elements: 1 The outer boundary of the structure is described based on the corner nodes only. Multipoint constraints due to cyclic symmetry are not assigned to midside nodes. Instead, they are linearly tied to the corresponding corner nodes. -1 The outer boundary of the structure is described using a quadratic field. Due to cyclic symmetry, full quadratic multipoint constraints are set up; they are assigned both to corner and midside nodes. The default value is 1.

Main Index

TYING 313 Define Tying Constraints

TYING

Define Tying Constraints

Description This option is used to define homogeneous constraints. Constraints are defined by specifying a tied node and one or more associated retained nodes. Further details are provided in Marc Volume A: User Information. Special types of tying can be obtained using the UFORMSN user subroutine (see Marc Volume D: User Subroutines and Special Routines). A rigid link for either small deformation or large deformation can be implemented by using tying type 80 or using RBE2. To obtain tying constraint based on updated current coordinates, add 1000 to tying type code. For tying type associated with user derived tying (UFORMSN), subtract 1000 from tying type code. In a coupled thermal-mechanical analysis during the heat transfer subincrements, tying type 1 is used for all tying types except 31, 32, 33, 34, and 69. It is possible to have a tying constraint equation to be active for only selective passes in a multiphysics analysis. A tying constraint always consists of a tied node (removed from the system) and one or more retained nodes (which remain in the system). Each tying constraint is specified by a series of two data blocks (data blocks 3 and 3a). If a sequence of similar tying types must be specified, a list of nodes for tied nodes (3b) and corresponding retained nodes (3c - 3d) must be given. If the constraint equations utlize the same node numbers, either the AUTOMSET or the MPC-CHECK parameter should be invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word TYING.

2nd data block

Main Index

1-5

1st

I

Number of constraint equations to be read (optional).

6-10

2nd

I

Unit number for input of tying data. Defaults to input.

11-15

3rd

I

Enter 1 to suppress printout of tying data.

314 TYING Define Tying Constraints

Format Fixed

Free

Data Entry Entry

3rd data block Data blocks 3 and 3a or 3 and 3b, 3c, 3d, are given once for each constraint equation set. 1-5

1st

I

Enter the code for tying type. SeeTable and Marc Volume A: User Information for definition of default types and user-defined routines.

6-10

2nd

I

Enter 0 to indicate a list of nodes to be tied will be defined in data block 3b. Enter a node number to indicate an individual node to be tied.

11-15

3rd

I

Number of retained nodes for this tying type. If a standard Marc tying type is used this does not need to be entered.

16-20

4th

I

Enter a 0 if tying type is available for all passes in multiphysics analysis. Enter a packed number indicating which passes the tie should be active using: 1 – stress pass. 2 – heat pass. 4 – electrical pass in Joule analysis. 5 – diffusion pass. 6 – electrostatic pass For example, 24 means tie is active only in heat and electrical pass, but is not active in structural pass.

3a data block If the number of a node is entered in the second field of the 3rd data block (above), use data block 3a to list the retained nodes. 1-80

1st

I

Sequence of retained nodes for constraint in (16I5) format, etc.

3b data block If no tied node is entered in the second field of the 3rd data block (that is, 0 is entered), use data blocks 3b, 3c, and 3d to enter a list of nodes to be tied. Enter an unsorted list of nodes to be tied. 3c data block Enter an unsorted list of nodes which will be the first retained nodes associated with tied nodes given in data block 3b. 3d data block Same as 3c except second retained nodes, etc. Note:

Main Index

List verbs EXCEPT, INTERSECT and sorted node sets are illegal in these lists.

TYING 315 Define Tying Constraints

Table 3-2

Summary of Standard Tying Types

Tying Code

Number of Retained Nodes

Purpose

I < NDEG

1

Tie the Ith degree of freedom at the tied node to the Ith degree of freedom at the retained node

100

1

Tie all degrees of freedom at the tied node to the corresponding degrees of freedom at the retained node

23

1

Tie axisymmetric solid node to axisymmetric-shell (element type 1) node

15 Number of retained nodes is 1 less than the number of shell nodes in the z-r plane of the section

Remarks

Both tied and retained nodes must be transformed to local system. TRANSFORMATION option must be invoked. (See Marc Volume A: User Information, Table 9-17)

Special tying types for pipe bend element 17 to remove rigid body modes (see Volume B: Element Library)

16 Number of shell nodes Special tying types for pipe in the z-r plane of the bend element 17 to remove section rigid body modes (see Volume B: Element Library) 17

2

Special tying types for pipe bend element 17 to couple bend section into pipe line (see Volume B: Element Library)

18

2

Joining together the boundaries of intersecting shell, element type 4, 8, or 24. Fully moment carrying joint.

Tied node is also second retained node. Neither node can be transformed (see Marc Volume A: User Information, Table 9-15)

28

2

Joining intersecting shells, element type 4, 8, or 24. Pinned joint.

Tied node is also second retained node (see Marc Volume A: User Information, Table 9-15)

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

316 TYING Define Tying Constraints

Table 3-2

Summary of Standard Tying Types (continued)

Tying Code

Number of Retained Nodes

Purpose

Remarks

19

2

Use beam element 13 as a stiffener on shell elements 4 or 8. Tied node is beam node: First retained node is shell node, second is beam node again. Beam node should be on, or close to, the normal to the shell at the shell node.

20

3

Create an extra node in a shell Always use after tying type 21. type 8 element tied to the interpolation function of the shell. Use in conjunction with tying type 21 to tie a beam element 13 or a stiffener across a shell element.

21

2

Same as type 19, but tying beam to an interpolated shell node not as a vertex of an element – element type 8 only. Must be followed by type 20 to tie the interpolated shell node into the shell mesh.

Must be followed by a tying type 20.

24

2

Join intersecting shells or beams, element type 15-17.

Tied node is also second retained node. Neither node can be transformed. Tying is necessary only when there is a large angle between the two plates.

25

2

Join solid mesh to shell or beam (type 15 or 16).

Tied node is also second retained node.

26

2

Join solid mesh to axisymmetric shell (type 1 or 89).

Similar to 23, but no transformation needed. Tied node is also second to retained node.

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

TYING 317 Define Tying Constraints

Table 3-2

Summary of Standard Tying Types (continued)

Tying Code

Number of Retained Nodes

Purpose

Remarks

27

2

Join Fourier solid to Fourier shell (type 90).

Tied node is also second retained node.

31

2

Refine mesh of first order (linear displacement) elements in 2-D.

Tie interior nodes on refined side to corner nodes on coarse side.

32

2

Refine mesh of second order (quadratic displacement) elements in 2-D.

Tie interior nodes on refined side to the edge of an element on the coarse side.

33

4

Refine mesh of 8-node bricks Tie interior node on the refined side to the 4 corner nodes of an element face on the coarse side. The retained nodes must be entered in the same or opposite order as they occur in the element connectivity.

34

8

Refine mesh of 20-node bricks

Tie interior nodes on refined side to the 8 (4 corner, 4 midside) nodes of an element on the coarse side. The retained nodes must be entered in the same or opposite order as they occur in the element connectivity.

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

318 TYING Define Tying Constraints

Table 3-2

Summary of Standard Tying Types (continued)

Tying Code

Number of Retained Nodes 44 2 is 2-D or axisymmetric lower-order element edge

Purpose Rigidly tie a node with displacements and rotations to a surface patch. This is internally used for CWELD and CFAST option.

Remarks The number of retained nodes is required. This tying type fully supports large deformation/rotations. No transformations are required.

3 is 2-D or axisymmetric higher-order element edge 3 if 3-D lower-order triangular face 4 if 3-D lower-order quadrilateral face 6 if 3-D higher-order triangular face 8 if 3-D higher-order quadrilateral face 52

1

Pin joint for beam types 14, 25, or 52.

53

1

Fully moment carrying joint for beam types 14, 25, or 52.

13

2

Joining two elements type 13 Tied node is also the second under an arbitrary angle. retained node. Fully moment carrying joint.

>100

1

Generate several tyings of type < NDEG.

Tying code is the first degree of freedom multiplied by 100 added to the last degree of freedom; that is, 209 means tie 2nd to 9th d.o.f. at tied node to resp. 2nd and 9th degrees of freedom at retained node.

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

TYING 319 Define Tying Constraints

Table 3-2

Summary of Standard Tying Types (continued)

Tying Code

Number of Retained Nodes

Purpose

Remarks

69

2

Joint for creating gaps or overlaps between two parts of a model either by prescribing the total force on the nodes on either side of the gap or overlap or by prescribing the size of the gap or overlap.

The second retained node is the control node of the tying. The force on this node is equal to the total force on the tied nodes of all tyings that share this control node. The displacement of the node is equal to size of the gap or overlap between the parts. In non-mechanical passes, the tying reduces to tying type 100 between the tied and the first retained node.

80

2

Form a rigid link between tied node and retained node. This works for either small or large deformation. If a rigid region is to be modeled, use multiple ties of type 80, with the tied node of each link being a different node, and use the same common node as the retained node.

The second retained node is an extra node which contains the rigid body rotation. Therefore, it may not be connected to any elements in a model.

85

2

Tying of temperatures between shell and solid elements in heat transfer analysis (linear/quadratic/new composite temperature distribution in the thickness direction of shell elements).

Tied node is the shell node and two retained nodes are nodes of the solid element. Order of the retained nodes follows the shell node degrees of freedom. The assumption here is that the shell and brick have the same thickness.

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

320 TYING Define Tying Constraints

Table 3-2

Summary of Standard Tying Types (continued)

Tying Code

Number of Retained Nodes

Purpose

Remarks

86

3

Tying of temperatures between shell and solid element in heat transfer analysis (quadratic/new composite temperature distribution in the thickness direction of shell element).

Tied node is the shell node and three retained nodes are nodes of the solid element. Order of the retained nodes follows shell node degrees of freedom. Tied node should not have linear temperature distribution. The assumption here is that the shell and brick have the same thickness.

87

1

Tying of temperatures between two shell elements in a heat transfer analysis (linear/quadratic/new composite temperature distribution).

Tied and retained nodes are shell nodes. The tied node should have more or equal number of degree of freedom than the retained node. The assumption here is that the tied shell and retained shell have equal thickness.

Caution: TRANSFORMATION MUST NOT BE USED AT NODES INVOLVED IN TYING TYPES 13, 18, 19, 20, 21, 22, 24, 25, 49, 50, 51, 52, 53, OR 80.

Main Index

SERVO LINK 321 Input Homogeneous Linear Constraints

SERVO LINK

Input Homogeneous Linear Constraints

Description This option uses homogeneous linear constraint capability (TYING) to input simple constraints of the form: ut = a1 ur1 + a2 ur2 + . . . where ut is a degree of freedom to be constrained. ur1, ur2 etc., are the other retained degrees of freedom in this structure. a1, a2 etc., are constants provided in this option. If the constraint equations utlize the same node numbers, either the AUTOMSET or the MPC-CHECK parameter should be invoked. For more information, see Marc Volume A: Theory and User Information. Note that more complex constraints can be entered via the TYING model definition set and the UFORMSN user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SERVO LINK.

11-15

2nd

I

Number of servo links to be entered below; defaults to number given on the TIE parameter.

16-20

3rd

I

Enter unit number for input of servo links. Defaults to input.

21-25

4th

I

Enter 1 if the 4th data block is being used to define in which pass of a multiphysics analysis the servo link should be active.

Data blocks 2, 3, and 4 are entered as pairs, one for each servo link. 2nd data block

Main Index

1-5

1st

I

Number of retained nodes (must not exceed the value given in the TIE parameter, fourth field).

6-10

2nd

I

Tied degree of freedom, at tied node.

11-15

3rd

I

Tied node.

16-20

4th

I

First retained degree of freedom at first retained node.

21-25

5th

I

First retained node.

322 SERVO LINK Input Homogeneous Linear Constraints

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Second retained degree of freedom at second retained node.

31-35

7th

I

Second retained node. Etc. (Continuation data in 16I5 format).

3rd data block One set of this data block goes with each set from data block 2. 1-10

1st

F

Numerical constant a1 joining tied and first retained variables.

11-20

2nd

F

Numerical constant a2 joining tied and second retained variables Etc.

4th data block Needed only if 4th entry on the 1st data block is set to 1. 1-5

1st

I

Enter 0 if servo link is active for all passes in multiphysics analysis (default). Enter a packed number indicating which passes the servo link should be active using: 1 – stress pass. 2 – heat pass. 4 – electrical pass in Joule analysis. 5 – diffusion pass. 6 – electrostatic pass. For example, 24 means servo link is active only in heat and electrical pass, but is not active in structural pass.

Main Index

RBE2 323 Define MD Nastran RBE2 Element

RBE2

Define MD Nastran RBE2 Element

Description The RBE2 option defines a rigid kinematic link between a single retained node with dependent degrees of freedom specified at an arbitrary number of tied nodes. The distance between the tied nodes to the retained node must be greater than zero. To activate large rotation formulation, users can use the LARGE DISP parameter. If the updated Lagrange option is set, then the large rotation formulation is automatically used. If all degrees of freedom of the tied nodes are tied, then RBE2 simulates rigid body motion. This is similar with tying 80. But RBE2 is more general than tying 80. For example, when the rotations are not tied, then RBE2 simulates spherical link or it can be used to simulate slider connection. The degrees of freedom of the tied nodes are co-rotated with the rotation of the retained node. If the constraint equations utlize the same node numbers, either the AUTOMSET or the MPC-CHECK parameter should be invoked. For more information, see Marc Volume A: User and Theory Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word RBE2.

2nd data block 1-5

1st

I

Enter the number of distinct sets of RBE2 to be input.

6-10

2nd

I

Enter the unit number for input of RBE2; defaults to input.

3rd data block

Main Index

1-5

1st

I

Retained (reference) node. This node has 3 degrees of freedom in 2-D (two translations and one rotation about the global z-axis) and six degrees of freedom in 3-D (three translations and three rotations). Note that this may require the use of the RBE parameter.

6-10

2nd

I

Packed list of degrees of freedom of tied nodes to be constrained. If, for example, the first and the third degree of freedom must be constrained, enter 13. Put blank or zero if all translational and rotational degrees of freedom are constrained.

11-15

3rd

I

Number of tied nodes.

324 RBE2 Define MD Nastran RBE2 Element

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter a 0 if tying type is available for all passes in myltiphysics analysis. Enter a packed number indicating which passes the tie should be active using: 1 – stress pass. 2 – heat pass. 4 – electrical pass in Joule analysis. 5 – diffusion pass. 6 – electrostatic pass. For example, 24 means tie is active only in heat and electrical pass, but is not active in structural pass.

21-25

5th

I

REB2 ID; default equals 0.

4a data block Sequence of tied nodes in (1615) format.

Main Index

RBE3 325 Define MD Nastran RBE3 Element

RBE3

Define MD Nastran RBE3 Element

Description The RBE3 option defines the motion at a reference node as the weighted average of the motion at a set of other nodes. The distance between the reference node to the retained nodes must be greater than zero. This option is a powerful tool to distribute applied loads in a model. Forces and moments applied to reference nodes are distributed to a set of independent degrees of freedom based on the RBE3 geometry and local weighting factors. By defaults, the reference node is considered as a tied node. It is also possible to specify the subset of the retained nodes as tied nodes. In this case, the total number of degrees of freedom specified for every tied node must be the same as the degrees of freedom specified for the reference node. In this way, it possible to use the reference node as tied node for other tyings. If the choice of the tied nodes is not done properly, a singularity may occur during the internal manipulation of the tying matrix, user should modify their input file. To activate large rotation formulation, users can use the LARGE DISP parameter. If the updated Lagrange option is set, then large rotation formulation is automatically used. The degrees of freedom of the reference node are not co-rotated. The constrained degrees of freedom of all retained nodes on an RBE3 option must be adequate to define its rigid body motion, otherwise, A-matrix is singular and an error message is issued. It is recommended, that for most applications, only the translation components be used for the degrees of freedom of the retained nodes. An exception is the case where the retained nodes are colinear. A rotation component may then be added to one node to stabilize its associated rigid body mode. If the constraint equations utlize the same node numbers, either the AUTOMSET or the MPC-CHECK parameter should be invoked. For more information, see Marc Volume A: User and Theory Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word RBE3.

2nd data block

Main Index

1-5

1st

I

Enter the number of distinct sets of RBE3 to be input.

6-10

2nd

I

Enter the unit number for input of RBE3; defaults to input.

326 RBE3 Define MD Nastran RBE3 Element

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Reference node. This node has three degrees of freedom in 2-D (two translations and one rotation about the global z-axis) and six degrees of freedom in 3-D (three translations and three rotations). Note that this may require the use of the RBE parameter.

6-10

2nd

I

Packed list of degrees of freedom of tied node to be constrained. If (e.g. the first and the third degree of freedom must be constrained) enter 13. Put blank or zero if all translational and rotational degrees of freedom are constrained.

11-15

3rd

I

Number of different weighting factors.

16-20

4th

I

Number of user-defined MSETS, maximum is eight. This indicates that a subset of retained nodes entered on the 5th data block are also tied nodes given on the 6th data block.

21-25

5th

I

Enter a 0 if tying type is available for all passes in multiphysics analysis. Enter a packed number indicating which passes the tie should be active using: 1 – stress pass. 2 – heat pass. 4 – electrical pass in Joule analysis. 5 – diffusion pass. 6 – electrostatic pass For example, 24 means tie is active only in heat and electrical pass, but is not active in structural pass.

4th data block The 4th and 5th data blocks are repeated as pairs, one for each weighting factor. 1-10

1st

R

Weighting factor.

11-15

2nd

I

Packed list of degrees of freedom belonging to the weighting factor.

16-20

4th

I

Enter the number of tied nodes with this weighting factor. The nodes are entered in the 5th data block.

5th data block Sequence of retained nodes in (1615) format.

Main Index

RBE3 327 Define MD Nastran RBE3 Element

Format Fixed

Free

Data Entry Entry

6th data block Required only if 4th field of 3rd data block is nonzero. The listed tied nodes must be a subset of the retained nodes. The total number of tied degrees of freedom must be the same as the number of degrees of freedom specified for the reference node. 1-5

1st

I

The first tied node number.

6-10

2nd

I

Packed list of degrees of freedom belonging to the first tied node.

11-15

3rd

I

The second tied node number.

16-20

4th

I

Packed list of degrees of freedom belonging to the second tied node.

etc.

Main Index

328 RROD Rigid 2-node Constraint

RROD

Rigid 2-node Constraint

Description This option defines a 2-noded rigid constraint that has the similar characteristics as the MD Nastran RROD element. The constraint is applied using equation elimination like tying or servolinks. The link must have finite length and may undergo large rotations. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word RROD.

2nd data block 1-5

1st

I

Enter the number of rigid links (not required).

6-10

2nd

I

Enter the unit number (defaults to the standard input).

3rd data block 1-5

1st

I

Enter the ID of this link.

6-10

2nd

I

Enter the first node ID.

11-15

3rd

I

Enter the second node ID.

16-20

4th

I

Enter component number of one and only one dependent translational degree of freedon in the global coordinate system (MD Nastran CMA).

21-25

5th

I

Enter component number of one and only one dependent translational degree of freedon in the global coordinate system (MD Nastran CMB). Note:

Main Index

Either CMA or CMB must be nonzero, but not both.

PIN CODE 329 Define Pin Code for Beam Element

PIN CODE

Define Pin Code for Beam Element

Description The PIN CODE option is used to remove connections between the node and selected degrees-of-freedom of the beam. The degrees of freedom are defined in the element’s coordinate system and the pin codes are applied at the offset end of the beam. By default, a new internal node is generated for every pinned node, and constraints are setup between these two nodes. When FEATURE, 6901 is activated, Marc condenses out the pinned degrees of freedoms instead of creating a new node. To activate large rotation formulation, users can use the LARGE DISP, LARGE STRAIN, or UPDATE parameter. Note:

The degrees of freedom listed in the 3rd data block are with respect to an element coordinate system defined by the beam cross section axis.

For more information, see Marc Volume A: User and Theory Information. Format Format Fixe

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PIN CODE.

2nd data block 1-5

1st

I

Enter the number of distinct sets of PIN CODE to be input.

6-10

2nd

I

Enter the unit number for input of PIN CODE; defaults to input.

I

Packed list of degrees of freedom to be flagged. For example, when the first and the third degree of freedom are to remain free (unconstrained), enter 13.

3rd data block 1-5

1st

4th data block List of element:node pairs. For example, 100:1 means the first node of element ID 100. The node value must be 1 or 2. For 3-node beam elements, only the end nodes can be flagged with pin code.

Main Index

330 INSERT Define Host Bodies and List of Elements or Nodes to be Inserted

INSERT 3 Model Definiti on Option s

Define Host Bodies and List of Elements or Nodes to be Inserted

Description This option allows the definition of host bodies and lists of elements or nodes to be inserted in the host bodies. The degrees of freedom of the nodes in the inserted node list or element list are automatically tied using the corresponding degrees of freedom of the nodes in host body elements based on their isoparametric location in the elements. This option can be used to place reinforcing cords or rods, such as 2-D rebar membrane elements, into solid elements. This option can be used to apply point loads in some specific locations other than element nodes. It also can be used to link two different meshes. After local adaptive meshing or global meshing, the constraint equation is reformulated. In this way, one can apply a point load in a region and it will continue to be applied in the correct location after remeshing. If a node to be inserted is also a node of a host body element, no tying is applied to the node. Format Format Fixed

Free

Data Entry

1st data block 1-6

1st

A

Enter the word INSERT.

2nd data block 1-5

1st

I

Number of data sets to be read in (optional).

6-10

2nd

I

Unit numbers for input; defaults to standard input (unit 5).

Data blocks 3, 4, and 5 are given for each data set. 3rd data block 1-5

1st

I

INSERT data set ID.

6-10

2nd

I

Enter 1 if a list of elements to be inserted; default is 0 - a list of nodes to be inserted.

11-20

3rd

F

Exterior tolerance. A node is considered within a host element if the distance between the element and the node is smaller than the tolerance times average edge length of the element, unless the node is actually inside another host element. Default is 0.05.

21-25

4th

I

Enter a 0 if a list of elements defines the host body. Enter a 1 if a list of contact bodies defines the host body.

Main Index

INSERT 331 Define Host Bodies and List of Elements or Nodes to be Inserted

Format Fixed

Free

Data Entry

4th data block Enter a list of elements or contact bodies which define the host body. 5th data block If the second field of the 3rd data block is 1, enter a list of elements to be inserted. Otherwise, enter a list of nodes to be inserted.

Main Index

332 SPRINGS Input Linear or Nonlinear Spring (Dashpot)

SPRINGS

Input Linear or Nonlinear Spring (Dashpot)

Description This data set is used to input any linear or nonlinear springs. For dynamic analysis, a dashpot capability is offered as well. The spring can be used for mechanical, thermal, and electrical analysis. Note that for input files that have the VERSION,10 or later parameter, two data blocks are needed to define each linear or nonlinear spring. The force in a linear mechanical spring/dashpot is given by: F = K ( u 2 – u 1 ) + C ( u· 2 – u· 1 )

where K is the spring stiffness, C is the damping coefficient,

u2

is the displacement of the degree of

freedom at the second end of the spring (third and fourth fields), and

u1

is the displacement of the degree

of freedom at the first end of the spring (first and second fields). During heat transfer or electrical analysis (regular heat transfer analysis, Joule heating analysis, or the thermal part of a coupled thermo-mechanical analysis), the spring acts like a link. The dashpot is not active. During a coupled thermo-mechanical analysis, springs can act in only the stress part (only 5th field of the 2nd data block is nonzero), or can act in only the thermal part (only 8th field of the 2nd data block is nonzero), or in both stress and thermal parts (both 5th and 8th fields of the 2nd data block are nonzero). In the last case, care should be taken to ensure that the degrees of freedom specified are uniformly valid for both the stress and thermal parts of the coupled run. If the degrees of freedom are specified as zero for a mechanical run, the spring acts along the line joining the two nodes. This line direction is updated during an incremental stress analysis only if large displacement is flagged. If the thermal conduction or electrical conduction is specified for a true direction spring, the associated degrees of freedom for the spring are assumed as one. If the second node is specified as zero, the spring is assumed to be fixed to ground along the specified degree of freedom. The displacement of the ground along the specified degree of freedom is assumed to be zero. In the thermal part, the temperature of the ground is assumed to be zero. In the electrical part, the voltage of the ground is assumed to be zero. Note that for degree of freedom springs, the spring force is positive if the displacement of node 2 along the specified degree of freedom is greater than the displacement of node 1 along the specified degree of freedom. Note also that for degree of freedom springs, if user nodal transformations are used for one or both nodes, the spring force is calculated based on the local transformed degree of freedom. For springs connected to the ground, the displacement of node 2 along the appropriate degree of freedom is always zero. For true direction springs, the spring force is positive if the spring is in tension and negative if the spring is in compression and is independent of any nodal transformations.

Main Index

SPRINGS 333 Input Linear or Nonlinear Spring (Dashpot)

For a nonlinear spring/dashpot (mechanical, thermal or electrical analysis), the spring stiffness can be specified in one of three ways: a. Nonlinear Spring Force: This is defined using the TABLE parameter and TABLE model definition option. The spring force computed from the multi-variate table is scaled by the corresponding reference value provided in the 5th, 6th, 8th or 9th field of the 2nd data block. The gradient of the table is internally calculated and used for the spring stiffness. To facilitate the gradient calculation, the spring force needs to be specified as a function of: relative displacement for mechanical springs (type 38), relative velocity for dashpots (type 22), relative temperature for thermal links (type 12), relative voltage for electrical links (type 31). In addition, the spring force can be optionally varied as a function of: time (type 1), normalized time (type 2), increment number (type 3), or normalized increment number (type 4). In thermo-mechanical coupled analysis, the mechanical spring force and damping force can also be specified as a function of the average temperature of the spring (type 12). In Jouleheating analysis, the electrical conduction can also be specified as a function of the average temperature of the spring (type 12). If the value of any independent variable falls beyond its minimum or maximum value in the table, the last force value associated with that independent variable is used by default and can be linearly extrapolated by the user if desired. For more general nonlinearities, option (c) (USPRNG) can be used independently or in conjunction with option (a). b. Nonlinear Spring Stiffness: This is defined using the TABLE parameter and TABLE model definition option. The stiffness value computed from the multi-variate table is scaled by the corresponding reference value provided in the 5th, 6th, 8th or 9th field of the 2nd data block. The stiffness can be varied as a function of time (type 1), normalized time (type 2), increment number (type 3), or normalized increment number (type 4). The spring stiffness can also be varied as a function of relative displacement for mechanical springs (type 38), relative velocity for dashpots (type 22), relative temperature for thermal links (type 12), relative voltage for electrical links (type 31). In thermo-mechanical coupled analysis, the mechanical spring stiffness and dashpot damping can also be specified as a function of the average temperature of the spring (type 12). In Joule heating analysis, the electrical conduction can also be specified as a function of the average temperature of the spring (type 12). If the value of any independent variable falls beyond its minimum or maximum value in the table, the last stiffness value associated with that independent variable is used by default and can be linearly extrapolated by the user if desired. For more general nonlinearities, option (c) (USPRNG) can be used independently or in conjunction with option (b). c. The nonlinear spring stiffness can also be specified with the USPRNG user subroutine with the general relation: F = F ( u 2 – u 1, u· 2 – u· 1 )

See Marc Volume D: User Subroutines and Special Routines for details.

Main Index

334 SPRINGS Input Linear or Nonlinear Spring (Dashpot)

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word SPRINGS.

2nd data block Enter one data block per spring/dashpot. 1-5

1st

I

Node to which first end of spring/dashpot will be attached.

6-10

2nd

I

Degree of freedom at above node to which spring/dashpot will be attached. Enter 0 for a spring/dashpot acting in the direction from the first to the second node (this also requires a 0 on the 4th field).

11-15

3rd

I

Node to which other end of spring/dashpot will be attached. Enter 0 if the spring goes from the first end to the ground.

16-20

4th

I

Degree of freedom at above node to which spring will be attached. Enter 0 if the spring goes from the first end to the ground. Enter 0 for a spring/dashpot acting in the direction from the first to the second node (this also requires a 0 on the 2nd field).

21-30

5th

F

Reference stiffness of spring or scale factor to force versus displacement table.

31-40

6th

F

Reference damping coefficient of dashpot or scale factor to force versus relative velocity table (for dynamic analysis only).

41-50

7th

F

Initial force in spring.

51-60

8th

F

Reference thermal conduction of link or scale factor to flux versus relative temperature table.

61-70

9th

F

Reference electrical conduction of link or scale factor to electrical flux versus relative voltage table.

71-75

10th

I

Spring ID

76-80

11th

I

Numerical Stabilizer Flag

3rd data block Enter one data block per spring/dashpot

Main Index

1-5

1st

I

Table ID for nonlinear mechanical stiffness.

6-10

2nd

I

Table ID for nonlinear dashpot damping.

11-15

3rd

I

Table ID for nonlinear thermal conduction.

16-20

4th

I

Table ID for nonlinear electrical conduction.

SPRINGS 335 Input Linear or Nonlinear Spring (Dashpot)

21-25

5th

I

-1 mechanical stiffness is obtained from gradient values. Force versus relative displacement table is entered. 1 mechanical stiffness is obtained from direct values. Stiffness versus relative table is entered.

26-30

6th

I

-1 dashpot damping is obtained from gradient values. Force versus relative velocity table is entered. 1 dashpot damping is obtained from direct values. Damping coefficient versus relative velocity is entered.

31-35

7th

I

-1 thermal conduction is obtained from gradient values. Flux versus relative temperature table is entered. 1 thermal conduction is obtained from direct values. Thermal conduction versus temperature table is entered.

36-40

8th

I

-1 electrical conduction is obtained from gradient values. Electrical flux versus relative voltage table is entered. 1 electrical conduction is obtained from direct values. Electrical conductivity versus voltage table is entered.

Main Index

336 PBUSH Input Data for Cbush Elements

PBUSH

Input Data for Cbush Elements

Description This data set is used to input all relevant data for cbush elements (2-D - type 194 and 3-D - type 195). The definition of the cbush coordinate system, cbush nodal offsets and coefficients for stiffness, damping, mass, stress and strain recovery, thermal and electrical behavior can be provided through these data blocks. The connectivity for the cbush elements are specified through the CONNECTIVITY model definition option. Some details for each of the data specifications are provided herein. The reader is referred to Marc Volume A: Theory and User Information, Chapter 9 for more details. Cbush Coordinate System

Options are provided to define the local cbush coordinate system along the element, in the global coordinate system or in a user-defined coordinate system. For the element coordinate system, the x axis is defined along the element length and forms a perpendicular triad with the local y and z axes. For 3-D cbush elements, an extra node or an orientation vector is specified to define the local y-z plane. For large displacement analysis, this local coordinate system attached to the element is constantly updated. Alternately, the element coordinate system can be defined along global Cartesian coordinates or in a usercoordinate system defined through the COORD SYSTEM model definition option. In these options, the coordinate system remains fixed through the analysis and is not updated for large displacement analysis. Cbush Nodal Offsets

Options are provided for locating an offset point along the cbush element axis, in the global coordinate system, or in a user-defined coordinate system. In the first option, the offset point is located along the line joining the two end nodes of the cbush element. The distance of the offset point along this line from the first end node is user defined. Alternately, the offset point position can be defined in the global Cartesian coordinate system or in a user-coordinate system defined through the COORD SYSTEM model definition option. For all options, the offset vectors from each cbush end node are internally calculated, and for large displacement analysis, these offset vectors are updated based on the respective rotations at each end node. Cbush Properties

Mechanical stiffness and damping properties are defined in the local cbush coordinate system. Stiffness properties can be specified in coefficient form or through force-displacement curves. Damping properties are specified as nominal damping either in coefficient form or force-velocity curves, and structural damping in the form of coefficients. For 2-D cbush elements, up to three coefficients can be specified and for 3-D cbush elements, up to six coefficients can be specified.

Main Index

PBUSH 337 Input Data for Cbush Elements

The force in a linear mechanical cbush element is given by: { F } = [ K ] { u 2 – u 1 } + [ C ] { u· 2 – u· 1 }

where { F } is the force vector in the local coordinate system of the cbush element, [ K ] is a diagonal matrix of the cbush stiffness coefficients, [ C ] is a diagonal matrix of the cbush damping coefficients, { u 2 } is the vector of displacement degrees of freedom in the local cbush coordinate system at the second end of the cbush, and

{ u1 }

is the vector of displacement degrees of freedom in the local cbush coordinate

system at the first end of the cbush. [ C ] includes the contributions of nominal damping, structural damping, and stiffness proportional damping. If the second node is specified as zero, the cbush element is assumed to be fixed to ground with all the ground degrees of freedom taken as zero. Note that for cbush elements defined in the global coordinate or user-coordinate system, the cbush force for a particular dof is positive if the displacements of node 2 along the specified degrees of freedom is greater than the displacement of node 1 along the specified degrees of freedom. For cbush elements defined in the element coordinate system, the cbush force is positive if the cbush is in tension and negative if the cbush is in compression. Field Analysis

During heat transfer or electrical analysis (regular heat transfer analysis, Joule heating analysis, or the thermal part of a coupled thermo-mechanical analysis), the cbush element acts like a link. The dashpot is not active. For the ground cbush element in the thermal part, the temperature of the ground is assumed to be zero and in the electrical part, the voltage of the ground is assumed to be zero. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word PBUSH.

2nd data block 1-5

1st

I

Number of distinct sets of PBUSH entries.

6-10

2nd

I

Enter unit number for input of PBUSH data (default to standard input).

11-15

3rd

I

Enter 1 to suppress printout.

3rd data block 1-5

1st

I

Enter PBUSH ID.

6-10

2nd

I

Method to enter cbush spring behavior (default = 0). Enter 0 if no stiffness. Enter 1 if stiffness is entered in coefficient form. Enter 2 if stiffness is specified via force-displacement tables.

Main Index

338 PBUSH Input Data for Cbush Elements

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Method to enter cbush damping behavior (default=0). Enter 0 for no damping. Enter 1 if nominal damping is entered in coefficient form. Enter 2 if nominal damping is specified via force-velocity tables. Enter 3 if structural damping coefficients are entered. Enter 4 if both nominal damping and structural damping are specified in coefficient form. Enter 5 if nominal damping is specified via force-velocity tables and structural damping is entered in coefficient form.

16-20

4th

I

Enter node ID G0 (default 0).

21-25

5th

I

Enter Coordinate System ID CID. Enter -1 if element coordinate system is used. For 3-D, either G0 or Xi can be used to define the local y-z plane. Enter 0 if global coordinate system is to be used. Enter > 0 if user-defined coordinate system given via COORD SYSTEM option is to be used.

26-35

6th

F

Enter X1.

36-45

7th

F

Enter X2.

46-55

8th

F

Enter X3.

Note:

The local y-z plane for each 3-D cbush element are defined through either G0 or Xi. Xi are the components of an orientation vector measured from the first end-node GA in the displacement coordinate system at node GA. Node ID G0 is an alternate method to suppy this orientation vector. The G0 method supercedes the Xi method. The orientation vector is measured from end GA to G0. To use either of them, CID (field 5) should be set to -1. of G0 or Xi

CI D ≥ 0

supercedes any definition

4th data block 1-5

1st

I

Enter Offset Coordinate System ID (OCID) Enter -2 if no offsets are to be provided. Enter -1 if offset point is located on the line joining the two nodes. The value of offset is provided by the 2nd field. Enter 0 if offset point coordinates in fields 3 - 5 are given in the global coordinate system.

Main Index

PBUSH 339 Input Data for Cbush Elements

Format Fixed

Free

Data Entry Entry Enter > 0 if offset point coordinates in fields 3 - 5 are given in a userdefined coordinate system defined through the COORD SYSTEM option.

6 - 15

2nd

F

Enter the value of S for the location of the cbush spring-dashpot along the line joining the two end-nodes.

16-25

3rd

F

Enter S1

26-35

4th

F

Enter S2

36-45

5th

F

Enter S3

Notes:

The value of S defined in field 2 is used with OCID = -1 in field 1. measured from end GA. (1-S) is the distance from end GB.

0≤S≤1.

S is

Si in fields 3 - 5 are used with OC ID ≥ 0 in field 1. They refer to the components of the vector measured from the origin to the offset point. OCID = -2 is set when no offsets are to be provided. It is commonly used when only the local x stiffness is defined along the cbush element and effectively behaves like a true-direction spring. This is also the equivalent of the CBUSH1D element in MD Nastran. Enter 5th and 6th data blocks if field 2 of 3rd data block (method to enter stiffness) is 1. 5th data block 1-10

1st

F

Enter reference stiffness in the first direction.

11-20

2nd

F

Enter reference stiffness in the second direction.

21-30

3rd

F

Enter reference stiffness in the third direction.

31-40

4th

F

Enter reference stiffness in the fourth direction.

41-50

5th

F

Enter reference stiffness in the fifth direction.

51-60

6th

F

Enter reference stiffness in the sixth direction.

6th data block 1-5

1st

I

Enter table ID associated with stiffness in the first direction.

6-10

2nd

I

Enter table ID associated with stiffness in the second direction.

11-15

3rd

I

Enter table ID associated with stiffness in the third direction.

16-20

4th

I

Enter table ID associated with stiffness in the fourth direction.

21-25

5th

I

Enter table ID associated with stiffness in the fifth direction.

26-30

6th

I

Enter table ID associated with stiffness in the sixth direction.

Enter 7th and 8th data blocks if field 2 of the 3rd data block (method to enter stiffness) is 2.

Main Index

340 PBUSH Input Data for Cbush Elements

Format Fixed

Free

Data Entry Entry

7th data block 1-10

1st

F

Enter reference force in the first direction.

11-20

2nd

F

Enter reference force in the second direction.

21-30

3rd

F

Enter reference force in the third direction.

31-40

4th

F

Enter reference force in fourth direction.

41-50

5th

F

Enter reference force in fifth direction.

51-60

6th

F

Enter reference force in sixth direction.

8th data block 1-5

1st

I

Enter table ID associated with force vs. displacement in the first direction.

6-10

2nd

I

Enter table ID associated with force vs. displacement in the second direction.

11-15

3rd

I

Enter table ID associated with force vs. displacement in the third direction.

16-20

4th

I

Enter table ID associated with force vs. displacement in the fourth direction.

21-25

5th

I

Enter table ID associated with force vs. displacement in the fifth direction.

26-30

6th

I

Enter table ID associated with force vs. displacement in the sixth direction.

Notes:

Up to six coefficients and table IDs can be provided in data blocks 5 - 8. Note that for the tables referenced in data blocks 6 and 8, the stiffness or force can be a function of up to four independent variables. For data block 8, a mandatory independent variable type is displacement. Other independent variables in the tables referenced by data blocks 6 or 8 can be time, normalized time, increment number, normalized increment number, x, y, z original and current position coordinates, frequency (for harmonic analysis), temperature. For 3-D cbush elements, the first three directions refer to x, y and z translations while the 4 - 6 directions refer to x, y and z rotations. For 2-D cbush elements, the first two directions refer to x and y translations while the 3rd direction refers to z rotation.

Enter 9th and 10th data blocks if field 3 of 3rd data block (method to enter damping) is 1 or 4. 9th data block

Main Index

1-10

1st

F

Enter reference nominal damping coefficient in first direction.

11-20

2nd

F

Enter reference nominal damping coefficient in the second direction

21-30

3rd

F

Enter reference nominal damping coefficient in the third direction.

31-40

4th

F

Enter reference nominal damping coefficient in the fourth direction.

41-50

5th

F

Enter reference nominal damping coefficient in the fifth direction.

51-60

6th

F

Enter reference nominal damping coefficient in the sixth direction.

PBUSH 341 Input Data for Cbush Elements

Format Fixed

Free

Data Entry Entry

10th data block 1-5

1st

I

Enter table ID associated with nominal damping in the first direction.

6-10

2nd

I

Enter table ID associated with nominal damping in the second direction.

11-15

3rd

I

Enter table ID associated with nominal damping in the third direction.

16-20

4th

I

Enter table ID associated with nominal damping in the fourth direction.

21-25

5th

I

Enter table ID associated with nominal damping in the fifth direction.

26-30

6th

I

Enter table ID associated with nominal damping in the sixth direction.

Enter 11th and 12th data blocks if field 3 of 3rd data block (method to enter damping) is 2 or 5. 11th data block 1-10

1st

F

Enter reference force in the first direction.

11-20

2nd

F

Enter reference force in the second direction.

21-30

3rd

F

Enter reference force in the third direction.

31-40

4th

F

Enter reference force in the fourth direction.

41-50

5th

F

Enter reference force in the fifth direction.

51-60

6th

F

Enter reference force in the sixth direction.

12th data block 1-5

1st

I

Enter table ID associated with nominal damping force vs. velocity in the first direction.

6-10

2nd

I

Enter table ID associated with nominal damping force vs. velocity in the second direction.

11-15

3rd

I

Enter table ID associated with nominal damping force vs. velocity in the third direction.

16-20

4th

I

Enter table ID associated with nominal damping force vs. velocity in the fourth direction.

21-25

5th

I

Enter table ID associated with nominal damping force vs. velocity in the fifth direction.

26-30

6th

I

Enter table ID associated with nominal damping force vs. velocity in the sixth direction.

Enter 13th and 14th data blocks if field 3 of 3rd data block (method to enter damping) is 3, 4 or 5. 13th data block

Main Index

1-10

1st

F

Enter reference structural damping coefficient in the first direction.

11-20

2nd

F

Enter reference structural damping coefficient in the second direction.

21-30

3rd

F

Enter reference structural damping coefficient in the third direction.

342 PBUSH Input Data for Cbush Elements

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Enter reference structural damping coefficient in the fourth direction.

41-50

5th

F

Enter reference structural damping coefficient in the fifth direction.

51-60

6th

F

Enter reference structural damping coefficient in the sixth direction.

14th data block 1-5

1st

I

Enter table ID associated with structural damping in the first direction.

6-10

2nd

I

Enter table ID associated with structural damping in the second direction.

11-15

3rd

I

Enter table ID associated with structural damping in the third direction.

16-20

4th

I

Enter table ID associated with structural damping in the fourth direction.

21-25

5th

I

Enter table ID associated with structural damping in the fifth direction.

26-30

6th

I

Enter table ID associated with structural damping in the sixth direction.

Notes:

Up to six coefficients and tables can be provided in data blocks 9- 14. These coefficients and associated table IDs are used for transient dynamic analysis. Data blocks 9, 10, 13, and 14 can also be used for harmonic analysis with complex-valued damping. Note that for the tables referenced in data blocks 10, 12, and 14, the damping coefficient or force can be a function of upto four independent variables. For data block 12, a mandatory independent variable type is velocity. Other independent variables in the tables referenced by data blocks 10, 12, or 14 can be time, normalized time, increment number, normalized increment number, x, y, z position coordinates, frequency (for harmonic analysis), temperature. For 3-D cbush elements, the first three directions refer to x, y and z translations while the four - six directions refer to x, y and z rotations. For 2-D cbush elements, the first two directions refer to x and y translations while the third direction refers to z rotation.

15th data block 1-10

1st

F

Enter stress recovery coefficient for the translational components (default = 0).

11-20

2nd

F

Enter stress recovery components for the rotational components (default = 0).

21-30

3rd

F

Enter strain recovery coefficient for the translational components (default = 0).

31-40

4th

F

Enter strain recovery coefficients for the rotational components (default = 0).

41-50

5th

F

Enter lumped translational mass.

51-60

6th

F

Enter lumped rotational mass.

Note:

Fields 5 and 6 refer to the lumped mass values at each end-node. They are used for dynamic/harmonic analysis.

Enter 16th and 17th data blocks only for analyses where heat transfer plays a role (e.g., thermal analysis, thermo-mechanical coupled, Joule heating, etc.)

Main Index

PBUSH 343 Input Data for Cbush Elements

Format Fixed

Free

Data Entry Entry

16th data block 1-10

1st

F

Enter the thermal conduction coefficient.

11-20

2nd

F

Enter the electrical resistance coefficient.

17th data block 1-5

1st

I

Enter the table ID associated with the thermal conduction coefficient.

6-10

2nd

I

Enter the table ID associated with the electrical resistance coefficient.

18th data block Enter a list of elements associated with this PBUSH ID.

Main Index

344 CFAST Shell Patch Fastener Connection

CFAST

Shell Patch Fastener Connection

Description The CFAST option defines a flexible connection between two surface patches. The surfaces may be either shell elements or faces of continuum elements in 3-D applications and truss, beam, axisymmetric shell elements or edges of continuum elements in 2-D applications. The PFAST option is used in conjunction with the CFAST option to define the characteristics of the connection which behaves like a generalized spring. This option internally creates a bushing element (element type 194 or 195 for 2-D or 3-D analysis, respectively) and a set of tyings to connect the bushing nodes to the parts of the structure that are to be connected. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CFAST.

2nd data block 1-5

1st

I

Enter the number of sets of CFAST data to follow (optional).

6-10

2nd

I

Enter the unit number for input; defaults to input file.

11-15

3rd

I

Set to 1 to suppress printout.

3rd data block 1-5

1st

I

Enter the value of identifier of CFAST. Leave blank to allow internally created identifier.

6-15

2nd

A

Enter the method of connection as one of “PROP” or “ELEM”.

16-20

3rd

I

Enter the value of the property identifier of a PFAST entry.

21-25

4th

I

Enter the value of GS, the node number of the CFAST location. If GS is blank, enter the coordinates through fields 7, 8, and 9. GS is ignored if GA in field 5 and GB in field 6 are both nonzero.

26-30

5th

I

Enter the value of GA, the first node of the CFAST. If blank, GS is used for the projection on side A. If not blank and GB in field 6 is not blank, GA is used for the projection.

31-35

6th

I

Enter the value of GB, the second node of the CFAST. If blank, GS is used for the projection on side B. If not blank and GA in field 5 is not blank, GB is used for the projection.

36-45

Main Index

7th

E

Enter XS, the x-coordinate of the approximate CFAST location.

CFAST 345 Shell Patch Fastener Connection

Format Fixed

Free

Data Entry Entry

46-55

8th

E

Enter YS, the y-coordinate of the approximate CFAST location.

56-65

9th

E

Enter ZS, the z-coordinate of the approximate CFAST location.

66-75

10th

A

Enter the name of the CFAST. This name is only used for output purposes. If left blank, a default name is given as “cf” followed by the order number of the CFAST in the input sequence left-padded with zeros to obtain a ten-character string.

For the PROP method, enter the 4th and 5th data blocks as follows: 4th data block 1-5

1st

I

Not used.

6-10

2nd

I

Not used.

5th data block 1-32

1st

A

Enter the set name of SetA containing the items to search from for the first patch. The node GS or GA is projected onto an element from this set, and all the elements comprising the patch are automatically selected from the set. This set does not have to be disjoint with the set entered in the 2nd field of this data block, but the search procedure is facilitated if it is.

33-64

2nd

A

Enter the set name of SetB containing the items to search from for the second patch. The node GS or GB is projected onto an element from this set, and all the elements comprising the patch are automatically selected from the set. This set does not have to be disjoint with the set entered in the 1st field of this data block, but the search procedure is facilitated if it is.

For the ELEM method, enter the 4th and 5th data blocks as follows: 4th data block 1-5

1st

I

Enter the element number identifying the first patch. For a continuum element, a face number is required in the 3rd field of this data block to fully identify the patch. The node GS or GA is projected onto this element/face, and the elements comprising the patch are automatically selected. GS or GA must have a projection onto this element/face.

6-10

2nd

I

Enter the element number identifying the second patch. For a continuum element, a face number is required in the 4th field of this data block to fully identify the patch. The node GS or GB is projected onto this element/face, and the elements comprising the patch are automatically selected. GS or GB must have a projection onto this element/face.

Main Index

346 CFAST Shell Patch Fastener Connection

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter the face number to project to of the element entered in the 1st field of this data block (required for continuum elements; ignored for shell elements).

16-20

4th

I

Enter the face number to project to of the element entered in the 2nd field of this data block (required for continuum elements; ignored for shell elements).

A

Enter the set name of SetA containing the items to search from for the first patch. The node GS or GA is projected onto the master element specified in the 1st field of the 4th data block and all further elements comprising the patch are automatically selected from the set.

5th data block 1-32

1st

This entry is required for continuum elements, but is not required for shells. 33-64

2nd

A

Enter the set name of SetB containing the items to search from for the second patch. The node GS or GB is projected onto the master element specified in the 2nd field of the 4th data block and all further elements comprising the patch are automatically selected from the set. This entry is required for continuum elements, but is not required for shells.

Main Index

PFAST 347 CFAST Fastener Property

PFAST

CFAST Fastener Property

Description Defines the CFAST fastener property values. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PFAST.

2nd data block 1-5

1st

I

Enter the number of sets of PFAST data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

11-15

3rd

I

Set to 1 to suppress printout.

3rd data block 1-5

1st

I

Enter the PFAST property identification number.

6-15

2nd

E

Enter the diameter of the fastener.

16-20

3rd

I

Specify the element stiffness coordinate system. Enter -1 to use element connectivity to define x-axis. Value in 4th field is ignored. Enter 0 to use global x-axis as the element x-axis (default). Enter n to use the x-axis of the user’s defined coordinate system to define the element x-axis.

30-35

4th

I

Define if the coordinate system in the 3rd field is absolute or relative. Enter 0 for relative (default). The element y- and z-axis is determined internally. For more details, refer to Marc Volume A: Theory and User Information. Enter 1 for absolute. It is only valid when the value in the 3rd field is greater than -1. The selected coordinate system is used for the element.

36-45

5th

E

Enter the mass of the fastener.

4th data block

Main Index

1-10

1st

E

Enter the reference stiffness value in direction 1.

11-20

2nd

E

Enter the reference stiffness value in direction 2.

21-30

3rd

E

Enter the reference stiffness value in direction 3.

31-40

4th

E

Enter the reference rotational stiffness value in direction 1.

348 PFAST CFAST Fastener Property

Format Fixed

Free

Data Entry Entry

41-50

5th

E

Enter the reference rotational stiffness value in direction 2.

51-60

6th

E

Enter the reference rotational stiffness value in direction 3

5th data block 1-5

1st

I

Enter the table ID for the stiffness value in direction 1.

6-10

2nd

I

Enter the table ID for the stiffness value in direction 2.

11-15

3rd

I

Enter the table ID for the stiffness value in direction 3.

16-20

4th

I

Enter the table ID for the rotational stiffness value in direction 1.

21-25

5th

I

Enter the table ID for the rotational stiffness value in direction 2.

26-30

6th

I

Enter the table ID for the rotational stiffness value in direction 3.

6th data block 1-10

1st

E

Enter the reference damping value in direction 1.

11-20

2nd

E

Enter the reference damping value in direction 2.

21-30

3rd

E

Enter the reference damping value in direction 3.

31-40

4th

E

Enter the reference rotational damping value in direction 1.

41-50

5th

E

Enter the reference rotational damping value in direction 2.

51-60

6th

E

Enter the reference rotational damping value in direction 3.

7th data block

Main Index

1-5

1st

I

Enter the table ID for the damping value in direction 1

6-10

2nd

I

Enter the table ID for the damping value in direction 2

11-15

3rd

I

Enter the table ID for the damping value in direction 3

16-20

4th

I

Enter the table ID for the rotational damping value in direction 1.

21-25

5th

I

Enter the table ID for the rotational damping value in direction 2.

26-30

6th

I

Enter the table ID for the rotational damping value in direction 3.

CWELD 349 Weld or Fastener Element Connection

CWELD

Weld or Fastener Element Connection

Description This option allows the CWELD connector information to be specified. A and B refer to the two surfaces (shell elements or solid element faces), that are to be connected by the CWELD. Patch-to-patch connections can be shell-to-shell, shell-to-solid, and solid-to-solid. Point-to-patch connections can be point-to-shell or point-to-solid. For each CWELD connection, a complete set of data is entered. The first data block contains: • EWID, METHOD, PWID, MCID, BTYPE, TTYPE, α, WGHT, IPROJ, CWNAME

EWID is the connector beam element number and it may be left blank. In that case, Marc automatically generates the element, but its end nodes GA and GB can still be entered. If GA and/or GB are not specified, Marc automatically generates the missing nodes as well. If EWID is not blank, the element may be defined in the CONNECTIVITY option, but this is not required. If it is not defined in the CONNECTIVITY option, the nodes GA and/or GB are automatically generated if they were left blank. If the element is defined in the CONNECTVITY option, its definition must be made after the CWELD option in order to take effect. In that case, the element is redefined in terms of its type and its nodes. METHOD defines the connection method and is one of PARTPAT, ELPAT, ELEMID, GRIDID, or ALIGN. PWID is the identification number of a corresponding PWELD property entry. BTYPE is the beam element type used for the connector element. The orientation of the beam cross section is computed by using the GEOMETRY or PWELD input data. Alternatively the orientation of the beam cross section can be specified by MCID, the identification number of a coordinate system defined in the COORD SYSTEM option. The value α is the angle over which the beam cross section is rotated about the beam axis to obtain its final orientation. TTYPE specifies the connection type for the auxiliary nodes. WGHT is the exponent used in computing distance weight factors for RBE3 constraints. IPROJ is a flag to control the projection of auxiliary nodes to their respective patches. CWNAME is an optional CWELD name (character string) used only in the output file to reference the CWELD. Depending on the connection method, one or more data blocks follow. • For PARTPAT, they contain: GS, SetA, SetB, GA, GB, XS, YS, ZS • For ELPAT, they contain: GS, SHIDA, SHIDB, GA, GB, XY, YS, ZS, FaceA, FaceB, SetA,

SetB • For ELEMID, they contain: GS, SHIDA, SHIDB, GA, GB, XS, YS, ZS, FaceA, FaceB • For GRIDID, they contain: GS, SPTYP, GA, GB, XS, YS, ZS followed by GA1...GA8,

GB1...GB8 where SPTYP defines the surface patch type on both sides of the weld and can be QQ, TT, QT, TQ, Q, or T and GAi are the nodes of patch A and GBi are the nodes of patch B. • For ALIGN, they contain: GA, GB. No additional data is needed.

For all methods, the pairing surface patch information is required, which identifies the master patches and, in addition, for the indirect connection methods, the regions from where to select the secondary patches. It is possible to have point connections on either side when the master patch information for that

Main Index

350 CWELD Weld or Fastener Element Connection

side is omitted (i.e., the SetA or SetB for PARTPAT, the SHIDA or SHIDB for ELPAT and ELMID or the GA1..GA8 or GB1..GB8 for GRIDID is left blank). It is not possible to make point connections to automatically generated nodes. The node GS is the approximate CWELD location node or CWELD reference node. If GS is blank, the coordinates may be entered directly through XS, YS, and ZS and a GS-node is automatically created. If GA and GB are both entered explicitly, the GS input is ignored; otherwise, the GS input is used for the projection onto the surfaces on each side of the CWELD to determine the end locations of the beam. If GS is ignored, GA and GB are projected onto their respective surfaces. If GS and GA are not specified but GB is, then GB is used as GS. If GS and GB are not specified, but GA is, then GA is used as GS. If GS, GA, and GB are not specified, then the coordinates XS, YS, ZS are used. If GS is specified and maximally one of the GA or GB, then GS is used for the projections on both sides and GA or GB are ignored for this purpose. If one side of the connector makes a point connection and the connector node for that side has been left blank and the GS-node has been specified, the point connection is made to the GS-node and the GS-node is projected onto the opposite side to determine the location of the other connector node. If the node on the opposite side also makes a point connection, the node for that side must have been specified. SHIDA and SHIDB are element numbers defining master patches. For solid elements, face information must be entered as well to fully identify the patch. For shell elements, the face information is not required. Face identifiers for FaceA and FaceB follow the definitions specified in the FACE IDS option described in Marc Volume C: Program Input. Valid set types specifying the sets SetA and SetB with patches to search from when finding the projections are element and face sets for shell elements in 3-D models, face sets for continuum elements in 3-D models, element and edge sets for truss, beam and axysmmetric shell elements in 2-D models and edge sets for continuum elements in 2-D models. Below faces should be understood as edges when entering the data for a 2-D model. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CWELD.

2nd data block 1-5

1st

I

Enter the number of sets of CWELD data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

11-15

3rd

I

Set to 1 to suppress printing of the CWELD data during this option.

I

Enter the element number (EWID) of the connector element between the patches.

3rd data block 1-5

1st

Leave blank when the automatic element generation is used.

Main Index

6-15

2nd

A

Enter the method of connection as one of PARTPAT, ELPAT, ELEMID, GRIDID, ALIGN.

16-20

3rd

I

Enter the value of PWID, the property identifier of a PWELD entry.

CWELD 351 Weld or Fastener Element Connection

Format Fixed

Free

Data Entry Entry

30-35

4th

I

Enter the value of MCID, the identification number of a coordinate system defined in the COORD SYSTEM option to define the orientation of the beam cross section. Leave blank or enter 0 if the automatic procedure is to be used.

36-40

5th

I

Enter the value for BTYPE (the Marc beam element type to be used for the connection). Default is 98 in a 3-D and 5 in a 2-D analysis when EWID is blank or the element type used on the CONNECTIVITY input when EWID is not blank.

41-45

6th

I

Enter the value for TTYPE (the type of constraint used to connect the auxiliary nodes in the CWELD). Enter 0 (default) for RBE3 constraints. Enter 44 for Kirchhoff constraints. Enter 80 for combined RBE2 and RBE3 constraints.

46-55

7th

E

Enter the value for α, the angle over which to rotate the cross section about the beam axis to obtain its final orientation.

56-65

8th

E

Enter the value for WGHT, the RBE3 distance weighting exponent. Defaults to the value given on the SWLDPRM input.

66-70

9th

I

Enter the value for IPROJ. Enter 0 (default) if the auxiliary nodes should not be relocated.to their projections on the finite element model. Enter 1 to have the auxiliary nodes relocated to their projections on the finite element model.

71-80

10th

A

Enter the name of the CWELD. This name is only used for output purposes. If left blank, a default name will be given as “cw” followed by the order number of the CWELD in the input sequence left-padded with zeros to obtain a ten-character string.

For the PARTPAT method, enter the 4th and 5th data blocks as follows: 4th data block 1-5

1st

I

Enter the value of GS, the node number of the approximate CWELD location. If GS is blank, enter the coordinates through fields 6, 7, and 8. GS is ignored if GA in field 4 and GB in field 5 are both nonzero.

Main Index

6-10

2nd

I

Not used; enter zero.

11-15

3rd

I

Not used; enter zero.

352 CWELD Weld or Fastener Element Connection

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter the value of GA, the first node of the CWELD. If blank, GS is used for the projection on side A. If not blank and GB in field 5 is not blank, GA is used for the projection.

21-25

5th

I

Enter the value of GB, the second node of the CWELD. If blank, GS is used for the projection on side B. If not blank and GA in field 4 is not blank, GB is used for the projection.

26-35

6th

E

Enter XS, the x-coordinate of the approximate CWELD location.

36-45

7th

E

Enter YS, the y-coordinate of the approximate CWELD location.

46-55

8th

E

Enter ZS, the z-coordinate of the approximate CWELD location.

A

Enter the setname of SetA containing the patches to search from for side A of the connection. The GS or GA node is projected onto a patch from this set and all further patches involved in the connection are automatically selected from the set. This set does not have to be disjoint with the set entered in the 2nd field of this data block, but the search procedure is facilitated if it is.

5th data block 1-32

1st

If left blank, a point connection is assumed on this side. 33-64

2nd

A

Enter the setname of SetB containing the patches to search from for side B of the connection. The GS or GB node is projected onto a patch from this set and all further patches involved in the connection are automatically selected from the set. This set does not have to be disjoint with the set entered in the 1st field of this data block, but the search procedure is facilitated if it is. If left blank, a point connection is assumed on this side.

For the ELPAT method, enter the 4th and 5th data blocks as follows: 4th data block 1-5

1st

I

Enter the value of GS, the node number of the approximate CWELD location. If GS is blank, enter the coordinates through fields 6, 7, and 8. GS is ignored if GA in field 4 and GB in field 5 are both nonzero.

6-10

2nd

I

Enter the element number identifying the master patch on side A of the connection. For a continuum element, a face number is required in the 9th field of this data block to fully identify the patch. The GS or GA node will be projected onto this patch.

Main Index

CWELD 353 Weld or Fastener Element Connection

Format Fixed

Free

Data Entry Entry If blank or 0, a point connection is assumed on this side.

11-15

3rd

I

Enter the element number identifying the master patch on side B of the connection For a continuum element, a face number is required in the 10 field of this data block to fully identify the patch. The GS or GB node will be projected onto this patch. If blank or 0, a point connection is assumed on this side.

16-20

4th

I

Enter the value of GA, the first node of the CWELD. If blank, GS is used for the projection on side A. If not blank and GB on field 5 is not blank, GA is used for the projection.

21-25

5th

I

Enter the value of GB, the second node of the CWELD. If blank, GS is used for the projection on side B. If not blank and GA on field 4 is not blank, GB is used for the projection.

26-35

6th

E

Enter XS, the x-coordinate of the approximate CWELD location.

36-45

7th

E

Enter YS, the y-coordinate of the approximate CWELD location.

46-55

8th

E

Enter ZS, the z-coordinate of the approximate CWELD location.

56-60

9th

I

Enter the face number to project to of the element entered in the 2nd field of this data block (required for continuum elements; ignored for shell elements).

61-65

10th

I

Enter the face number to project to of the element entered in the 3rd field of this data block (required for continuum elements; ignored for shell elements).

A

Enter the setname of SetA containing the patches to search from for side A of the connection. The GS or GA node is projected onto the master patch specified in the 2nd field of the 4th data block and all further patches involved in the connection are automatically selected from the set.

5th data block 1-32

1st

If the master patch is a shell element, this field can be left blank and all shell elements in the model are considered. If the master patch is the face of a continuum element, a face set is required here.

Main Index

354 CWELD Weld or Fastener Element Connection

Format Fixed 33-64

Free 2nd

Data Entry Entry A

Enter the setname of SetB containing the patches to search from for side B of the connection. The GS or GB node is projected onto the master patch specified in the 3rd field of the 4th data block and all further patches involved in the connection are automatically selected from the set. If the master patch is a shell element, this field can be left blank and all shell elements in the model are considered. If the master patch is the face of a continuum element, a face set is required here.

For the ELEMID method, enter the 4th data block as follows: 4th data block 1-5

1st

I

Enter the value of GS, the node number of the approximate CWELD location. If GS is blank, enter the coordinates through fields 6, 7, and 8. GS is ignored if GA on field 4 and GB on field 5 are both nonzero.

6-10

2nd

I

Enter the element number identifying the master patch on side A of the connection. For a continuum element, a face number is required in the 9th field of this data block to fully identify the patch. The GS or GA node is projected onto this patch. If blank or 0, a point connection is assumed on this side.

11-15

3rd

I

Enter the element number identifying the master patch on side B of the connection. For a continuum element, a face number is required in the 10th field of this data block to fully identify the patch. The GS or GB node is projected onto this patch. If blank or 0, a point connection is assumed on this side.

16-20

4th

I

Enter the value of GA, the first node of the CWELD. If blank, GS is used for the projection on side A If not blank and GB on field 5 is not blank, GA is used for the projection.

21-25

5th

I

Enter the value of GB, the second node of the CWELD. If blank,GS is used for the projection on side B. If not blank and GA on field 4 is not blank, GB is used for the projection.

Main Index

26-35

6th

E

Enter XS, the x-coordinate of the approximate CWELD location.

36-45

7th

E

Enter YS, the y-coordinate of the approximate CWELD location.

46-55

8th

E

Enter ZS, the z-coordinate of the approximate CWELD location.

CWELD 355 Weld or Fastener Element Connection

Format Fixed

Free

Data Entry Entry

56-60

9th

I

Enter the face number to project to of the element entered in the 2nd field of this data block (required for continuum elements; ignored for shell elements).

61-65

10th

I

Enter the face number to project to of the element entered in the 3rd field of this data block (required for continuum elements; ignored for shell elements).

For the GRIDID method, enter the 4th, 5th and 6th data blocks as follows: 4th data block 1-5

1st

I

Enter the value of GS, the node number of the approximate cweld location. If GS is blank, enter the coordinates through fields 6, 7, and 8. GS is ignored if GA on field 4 and GB on field 5 are both nonzero.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Enter the value of GA, the first node of the CWELD. If blank, GS is used for the projection on side A. If not blank and GB on field 5 is not blank, GA is used for the projection.

21-25

5th

I

Enter the value of GB, the second node of the CWELD. If blank, GS is used for the projection on side B. If not blank and GA on field 4 is not blank, GB is used for the projection.

26-35

6th

E

Enter XS, the x-coordinate of the approximate CWELD location.

36-45

7th

E

Enter YS, the y-coordinate of the approximate CWELD location.

46-55

8th

E

Enter ZS, the z-coordinate of the approximate CWELD location.

56-65

9th

A

Enter the value of SPTYP defining the surface patch combination being connected as one of QQ, TT, QT, TQ, Q, or T. This field is optional and may be left blank.

5th data block If this data block is blank, a point connection is assumed on side A.

Main Index

1-5

1st

I

Enter the node number GA1.

6-10

2nd

I

Enter the node number GA2.

11-15

3rd

I

Repeat until all nodes of the patch on side A have been defined. A patch can have up to 8 nodes.

356 CWELD Weld or Fastener Element Connection

Format Fixed

Free

Data Entry Entry

6th data block If this data block is blank, a point connection is assumed on side B. 1-5

1st

I

Enter the node number GB1.

6-10

2nd

I

Enter the node number GB2.

11-15

3rd

I

Repeat until all nodes of the patch on side B have been defined. A patch can have up to 8 nodes.

For the ALIGN method, enter the 4th data block as follows: 4th data block

Main Index

1-5

1st

I

Not used; leave blank or enter 0.

6-10

2nd

I

Not used; leave blank or enter 0.

11-15

3rd

I

Not used; leave blank or enter 0.

16-20

4th

I

Enter the value of GA, the first node of the CWELD. May be blank if the element is entered through the CONNECTIVITY option.

21-25

5th

I

Enter the value of GB, the second node of the CWELD. May be blank if the element is entered through the CONNECTIVITY option.

PWELD 357 Connector Element Property

PWELD

Connector Element Property

Description The properties of the cweld connector element are entered through the PWELD option. The geometrical properties of the connector element between the two patches may also be entered here instead of entering them through the GEOMETRY option. The PWELD option contains the following information: PWID, D, MID, LDMIN, LDMAX, WTYPE EGEOM1, EGEOM2, ..., EGEOM8 The first line defines the general CWELD characteristics. If the second field on the first line (D) is nonzero, it represents the characteristic diameter (3-D analysis) or thickness (2-D anlaysis) of the CWELD that will be used to compute the positions of the auxiliary nodes. It also defines the cross-section properties if no further geometric data is supplied. PWID is the PWELD identifier referenced on the CWELD option. LDMIN and LDMAX are the minimum and maximum length to diameter ratios of the CWELD. WTYPE defines the connection type as either a general connection or a spotweld connection. MID is a material identification number. The second line defines the geometrical properties of the element in the same way they are defined in the GEOMETRY option for the particular element type. The data required for each element type can be found in Marc Volume B: Element Library. This second line is always required even when the characteristic dimension (diameter or thickness) D has been defined and no further data is needed. In that case, it should be left blank (or contain zeros only) and in 3-D models, the cross section will be circular with diameter D or in 2-D models, the cross section will be rectangular with thickness D and unit width. If the characteristic dimension D on the first line is zero and the first field on the second line is nonzero, a characteristic dimension will be estimated from the geometric properties. If the first field on the second line is zero, a nonzero value for D is required on the first line when using a method that generates auxiliary nodes and patches for its connections because it is currently not possible to estimate a characteristic diameter from BEAM SECT data. If the EGEOM4, EGEOM5, and EGEOM6 fields are all blank or zero, the local directions of the connector element are determined by one of the two procedures outlined in the Connector Orientation section of Marc Volume A: Theory and User information; otherwise, these values are used to define the local directions. In the latter case, it is possible to use a coordinate system defined at the first node of the element, but it is not possible to offset its nodes. If the geometrical properties are defined in both the PWELD and GEOMETRY options for the same connector elment, the properties defined in the PWELD option are used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word PWELD.

358 PWELD Connector Element Property

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter the number of sets of PWELD data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

3rd data block 1-5

1st

I

Enter the value for PWID, the PWELD identification number.

6-15

2nd

E

Enter the characteristic dimension D of the CWELD. If blank or zero, Marc will make an estimate if the cross-section data are not entered through the BEAM SECT parameter. In a 3-D analysis, D is the characteristic diameter. In a 2-D analysis, D is the characteristic thickness and the section will have a unit width.

16-20

3rd

I

Enter the value for MID; a material identification number to assign the material properties.

21-30

4th

E

Enter the value of LDMIN; the smallest ratio of length to diameter for stiffness calculation Default is DLDMIN, which defaults to 0.2 if not specified on the SWLDPRM option.

31-40

5th

E

Enter the value of LDMAX, the largest ratio of length to diameter for stiffness calculation. Default is DLDMAX, which defaults to 5.0 if not specified on the SWLDPRM option.

41-50

6th

A

Enter the value for WTYPE, the type of connection as SPOT for a spotweld connector or leave blank for a general connector.

4th data block

Main Index

1-10

1st

E

EGEOM1

11-20

2nd

E

EGEOM2

21-30

3rd

E

EGEOM3

31-40

4th

E

EGEOM4

41-50

5th

E

EGEOM5

51-60

6th

E

EGEOM6

61-70

7th

E

EGEOM7

71-80

8th

E

EGEOM8

SWLDPRM 359 Parameters for CWELD Connectors

SWLDPRM

Parameters for CWELD Connectors

Description A number of global parameters that control the behaviour of CWELD and CFAST connections and their output to the jobid.out file can be entered through this model definition option. These parameters and their descriptions are summarized in Table 3-3. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SWLDPRM.

A

Enter the name of the first parameter.

2nd data block 1-10

1st

11-…

2nd

…-…

3rd

…-…

4th

E or I Enter the value for the first parameter. A

Enter the name of the second parameter.

E or I Enter the value for the second parameter.

A maximum of four parameter,value pairs can be entered per line, but it may also be less. The parameter,value pairs can appear in any order. A parameter and its value cannot occur in different lines; they must appear on the same line. At least one pair is required per line. The second data block can be repeated as many times as desired. If a parameter is defined more than once, the last assigned value is the active value. Table 3-3 Name

Main Index

SWLDPRM Parameter Names and Descriptions

Type

Default

Description

CHKRUN

Integer > 0 (0 or 1)

0

This parameter is available in MD Nastran but has no meaning in Marc and is ignored.

GSMOVE

Integer > 0

0

Maximum number of times GS is moved in case a complete projection of all points has not been found.

NREDIA

0 < Integer < 4

0

Maximum number of times the characteristic diameter D is reduced in half in case a complete projection of all points has not been found.

360 SWLDPRM Parameters for CWELD Connectors

Table 3-3 Name PRTSW

SWLDPRM Parameter Names and Descriptions (continued)

Type 0 < Integer < 4

Default 0

Description Parameter to control the CWELD/CFAST diagnostic output to the Marc output file (jobid.out). 0 = no diagnostic output 1 = print errors only 2 = print errors and warnings only 3 = print projection diagnostics with no tying details 4 = print all diagnostics

GSPROJ

-90 < Real < 90

20.0

Maximum angle allowed between the normal vectors of master patch A and master patch B. The connection will not be generated if the angle between these two normal vectors is greater than the value of GSPROJ. If GSPROJ is negative, the program will always accept the connection and will only issue a warning if the angle is larger than |GSPROJ| (see Figure 9-62 in Marc Volume A: Theory and User Information).

GSCURV

-90 < Real < 90

20.0

Maximum angle allowed between the normal vectors of a patch to which an auxiliary node projects and its corresponding auxiliary and master patches. It provides a measure to monitor the curvature of a surface and to recognize patches that belong to, for example, stiffeners. A connection is not generated if the angle between the normal vectors is greater than 90-GSCURV meaning that the patches are almost normal to each other. In that case, the patch is rejected and the search proceeds to the next patch in the list. If the angle is between zero and GSCURV, no message is displayed. If the angle is between GSCURV and 90-GSCURV, a large angle warning is displayed. The following three tests are performed in the order given below when GSCURV is positive: If 0 < angle < GSCURV => OK If GSCURVE < angle < 90-GSCURV => trigger a warning. If angle > 90-GSCURV => reject. Note that the warning condition is never triggered when GSCURV > 45 as it is overruled by the reject condition. If GSCURV is negative, the projection is always accepted and a warning is issued when the angle is larger than |GSCURV| (see Figure 9-62 in Marc Volume A: Theory and User Information)

Main Index

SWLDPRM 361 Parameters for CWELD Connectors

Table 3-3

SWLDPRM Parameter Names and Descriptions (continued)

Name

Type

Default

Description

GSTOL

Real

0.0

Maximum allowable distance of the node GS to its projection on a patch. IF GSTOL is positive, the distance is relative to the characteristic CWELD/CFAST diameter D, (the tolerance is GSTOL*D). If GSTOL is negative, the distance is absolute (i.e., the tolerance is -GSTOL). If GS is used for the projection together with one of the methods PARTPAT/PROP or ELPAT/ELEM, an error is issued if the distance is too large. If GA and GB are used for the projection or if one of the ELEMID or GRIDID methods is used, the test only issues a warning if the distance is too large. If GSTOL is zero, any distance is accepted.

PROJTOL

0.0 < Real < 0.2 0.0

Tolerance to accept the projected point GA or GB if the computed coordinates of the projection point lie outside the patch boundary, but are located within PROJTOL*(dimension of the patch).

ACTVTOL

Integer > 0

Parameter controlling the behavior of PROJTOL for the different CWELD/CFAST connection methods. This parameter is entered as an integer and is converted to a four-character string. If its value is less than 1000, the string is prepended with zeros. The first character (from the left) controls the behavior when the PARTPAT/PROP method is used. The second controls the behavior when the ELPAT/ELEM method is used. The third controls the behavior when the ELEMID method is used and the fourth controls the behavior when the GRIDID method is used. For ALIGN, the PROJTOL tolerance has no significance. Each digit ( d i ) in the string can have the

Integer < 2211

1111

value 0 or 1 or 2, where the value 2 only has significance for the ELPAT/ELEM or PARTPAT/PROP methods. The values have the following meaning: 0 = PROJTOL is completely deactivated

Main Index

362 SWLDPRM Parameters for CWELD Connectors

Table 3-3 Name

SWLDPRM Parameter Names and Descriptions (continued)

Type

Default

Description 1 = PROJTOL is activated for ELEMID and GRIDID, PROJTOL is activated in initial projections for ELPAT/ELEM, PROJTOL is only activated over free edges of the patch in auxiliary projections for ELPAT/ELEM, and in initial and auxiliary projections for PARTPAT/PROP. Free edges have no neighbors within the set that defines the complete surface.

ACTVTOL (cont)

2 = PROJTOL is always activated CWSETS

Integer > 0

0

(0 or 1)

Parameter to control the automatic creation of four element sets with the elements involved in the CWELD/CFAST connections. 0 = the sets are not created 1 = four sets are created automatically: fastener_all_beams_inc000”, the set containing all connector beam elements. fastener_all_faces_sidea_inc0000, the set containing all elements with patches on side A of the connection. fastener_all_faces_sideb_inc0000, the set containing all elements with patches on side B of the connection. fastener_all_warnings_inc0000, the set containing all elements involved in CWELD/CFAST warning messages. Defining sets with any of these names must be avoided and are considered an error.

Main Index

MAXEXP

Integer > 0

2

Parameter to control the maximum number of expansions in the search for projections of the auxiliary nodes. First, the master patch is tried. If no projection is found on the master patch, a first expansion is made including all neighboring patches of the master patch. If no projection is found on any of the new patches, a second expansion is made including all neighbors of the patches tried so far. This process continues until the number of expansions exceeds MAXEXP. Two patches are neighbors if they share at least one node in their connectivities.

DLDMIN

Real > 0.0

0.2

Default value for LDMIN; the smallest ratio of length to characteristic diameter.

SWLDPRM 363 Parameters for CWELD Connectors

Table 3-3

SWLDPRM Parameter Names and Descriptions (continued)

Name

Type

Default

Description

DLDMAX

Real > 0.0

5.0

Default value for LDMAX; the largest ratio of length to characteristic diameter.

MAXITR

Integer > 0

25

The maximum number of iterations allowed in the iteration process for finding the projection on a patch.

EPSITR

Real > 0.0

1.0E-5

Tolerance to terminate the iteration process for finding the projection on a patch. If the parametric coordinate change in an iteration is less than EPSITR, the projection is accepted as converged.

DELMAX

Real > 0.0

0.1

Maximum allowable parametric coordinate change during the iteration process for finding the projection on a patch. At first DELMAX is not activated (i.e., the parametric coordinate change is not limited during the iteration process). The parameter is only activated when the full Newton Raphson iteration process for a projection did not converge. In that case, the iteration process is restarted with DELMAX activated.

CWSPOT

0 < Integer < 3

1

Parameter to choose the method for modifying the beam length. 1 = scale the stiffness of the beam 2 = reposition the end nodes of the beam 3 = reposition the auxiliary patch nodes and the end nodes of the beam.

RBE3WT

Real

0.0

Default RBE3 distance weighting exponent. The weight factor for each retained node in a RBE3 involved in a CWELD/CFAST connection is:

1 f i = ----ndi

where fi

is the weighting factor for retained node i.

di

is the distance from the tied node to retained node i

n

is the weighting exponent RBE3WT.

Negative values for RBE3WT are not recommended, since they result in heavier weighting for nodes further away. The default results in uniform weighting ( fi ) = 1 .

Main Index

364 SWLDPRM Parameters for CWELD Connectors

Table 3-3 Name BOXING

SWLDPRM Parameter Names and Descriptions (continued)

Type

Default

-1 < Integer < 1 0

Description Parameter to control the boxing algorithm used to speed up the search for master patches when connection method PARTPAT/PROP is used. -1 =The boxing algorithm is always deactivated 0 = The boxing algorithm may or may not be activated depending on the number of elements in the sets. 1 = The boxing algorithm is always activated

Main Index

SUPERELEM (Model Definition) 365 Perform Craig-Bampton Analysis for MD Adams MNF Interface

SUPERELEM (Model Perform Craig-Bampton Analysis for MD Adams MNF Interface Definition) Description This option triggers Marc to perform the Craig-Bampton method of Component Mode Synthesis and generate a Modal Neutral File (MNF) that can be uploaded into MD Adams models to represent flexible components. The option allows direct definition of the boundary or interface degrees of freedom. The option also allows automatic definition of interface degrees of freedom of the nodes that get in contact with selected rigid contact bodies. This is very useful for some nonlinear analyses such as tire footprint analysis in which the interface degrees of freedom are not known a priori. It also allows the specification of interface degrees of freedom of the control nodes of selected load-controlled rigid contact bodies. The two control nodes for load-controlled rigid bodies are consolidated into one node with six degrees of freedom before exporting to the MNF. Format Format Fixed

Free

Data Entry Entry

1st data block 1st

A

Enter the word SUPERELEM.

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter 1 to generate MNF.

1-10 2nd data block

The 3rd and 4th data blocks are entered as pairs. Data blocks 3a and 4a may be repeated if needed. A. List of Interface Degrees of Freedom. 3a data block 1-80

1st

I

Enter a list of degrees of freedom.

1st

I

Enter a list of interface nodes.

4a data block 1-80

B. List of Rigid Contact Bodies. All degrees of freedom of all nodes in contact with these bodies will be interface degrees of freedom. 3b data block 1-5

1st

I

Enter -1.

1st

I

Enter a list of rigid contact bodies.

4b data block 1-80

Main Index

366 SUPERELEM (Model Definition) Perform Craig-Bampton Analysis for MD Adams MNF Interface

Format Fixed

Free

Data Entry Entry

C. List of Load-controlled Rigid Contact Bodies. All degrees of freedom of the control nodes of these bodies will be interface degrees of freedom. 3c data block 1-5

1st

I

Enter -2.

1st

I

Enter a list of load-controlled rigid contact bodies.

4c data block 1-80

Main Index

SUPERELEM (DMIG Applications - Model Definition) 367 Create DMIG of Substructure

SUPERELEM (DMIG Applications - Model Definition)

Create DMIG of Substructure

Description This option allows the creation of a DMIG file containing the stiffness associated with the degrees of freedom specified here. This DMIG may be subsequently read into Marc or Nastran. The option allows direct definition of the degrees of freedom. The option also allows automatic definition of interface degrees of freedom of the nodes that get in contact with selected rigid contact bodies. This is very useful for some nonlinear analyses such as tire footprint analysis in which the interface degrees of freedom are not known a priori. It also allows the specification of interface degrees of freedom of the control nodes of selected load-controlled rigid contact bodies. The two control nodes for load-controlled rigid bodies are consolidated into one node with six degrees of freedom before exporting to the DMIG. This option can only occur once in the analysis. However, it may be used in either the model definition or the load increment section. The DMIG will be written to file jidname_dmigst_inc, where: jidname

is the job name

inc

is the increment number

Note:

If a node is subsequently going to be transformed, all degrees of freedom of all nodes must be specified here.

This option may only be used with direct solution techniques. Format Format Fixed

Free

Data Entry Entry

1st data block 1st

A

Enter the word SUPERELEM.

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

1-10 2nd data block

Main Index

368 SUPERELEM (DMIG Applications - Model Definition) Create DMIG of Substructure

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter 1 to create a DMIG file. Enter 3 to create a DMIGB file. DMIGB uses a different output format, which results in a smaller file (about one third of the size of a DMIG file). When a DMIGB file is included in a Marc analysis, the program uses a column-wise storage instead of a full in-core matrix storage. This memory reduction can be important for large DMIG files. The DMIGB format can be used only as input for a Marc analysis; it can not be used in a Nastran analysis.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 0 if all stiffness terms written to DMIG. Enter 1 if terms less than

x f ⋅ K1

Enter 2 if terms less than

xf

are filtered out.

are filtered out.

31-40

7th

F

Enter the value used for filtering

41-50

8th

A

Enter the name of the matrix; default is KAAX which is limited to eight characters.

xf ;

default = 1.e-8.

The 3rd and 4th data blocks are entered as pairs. Data blocks 3a and 4a may be repeated if needed. A.

List of Interface Degrees of Freedom.

3a data block 1-80

1st

I

Enter a list of degrees of freedom.

1st

I

Enter a list of interface nodes.

4a data block 1-80

B. List of Rigid Contact Bodies. All degrees of freedom of all nodes in contact with these bodies will be interface degrees of freedom. 3b data block

1-5

1st

I

Enter -1.

1st

I

Enter a list of rigid contact bodies.

4b data block 1-80

C. List of Load-controlled Rigid Contact Bodies. All degrees of freedom of the control nodes of these bodies will be interface degrees of freedom. 3c data block

Main Index

SUPERELEM (DMIG Applications - Model Definition) 369 Create DMIG of Substructure

Format Fixed 1-5

Free

Data Entry Entry

1st

I

Enter -2.

1st

I

Enter a list of load-controlled rigid contact bodies.

4c data block 1-80

Main Index

370 DMIG-OUT (Model Definition) Output Control of Matrices

DMIG-OUT (Model Definition)

Output Control of Matrices

Description This option allows you to control the output of matrices into DMIG format. These matrices may then be read in using the DMIG option and activated using either the B2GG, B2PP, K2GG, K2PP, M2GG, M2PP, and P2G options within Marc or within MD Nastran. To output the substructure matrix, use the SUPERELEM option. In the case of element matrix, they can either be written in the Marc global (MSC.Nastran Basic) or a local coordinate system. Both symmetric and nonsymmetric matrices are supported. Note that the scalar factor associated with the STIFSCALE option is not applied to the element matrices. This option may be repeated in each loadcase. The files created associated with element matrices have the names jidname_dmigXX_inc, where: Jidname

is the job ID name

XX

is the suffix associated with the matrix type

ST

stiffness matrix

DF

differential stiffness matrix

MS

mass matrix

DM

damping matrix

CO

conductivity matrix

SP

specific heat matrix

Inc

is the increment number

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word DMIG-OUT.

The 2nd and 3rd, 4th and 5th, 6th and 7th, 8th and 9th, 10th and 11th, 12th and 13th data blocks are entered as pairs as required. 2nd data block 1-10

1st

A

Enter the word STIFFNESS.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

Main Index

DMIG-OUT (Model Definition) 371 Output Control of Matrices

Format Fixed 16-20

Free 3rd

Data Entry Entry I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase. Enter -2 to switch off writing DMIG output.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Enter 0 to output global stiffness in untied state. Enter 1 to output global stiffness in tied state.

36-45

7th

E

Enter minimum value to be written to DMIG. Stiffness values below this value will be ignored.

3rd data block (only required if a list of elements or bodies to be given) 4th data block 1-10

1st

A

Enter the words DIFF MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

Main Index

372 DMIG-OUT (Model Definition) Output Control of Matrices

Format Fixed

Free

Data Entry Entry

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Stiffness values below this value will be ignored.

5th data block (only required if a list of elements or bodies to be given) 6th data block 1-10

1st

A

Enter the words MASS MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Mass values below this value will be ignored.

7th data block (only required if a list of elements or bodies to be given) 8th data block 1-10

1st

A

Enter the words DAMPING MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

Main Index

DMIG-OUT (Model Definition) 373 Output Control of Matrices

Format Fixed 21-25

Free 4th

Data Entry Entry I

Enter 1 to output in Marc global, Nastran basic (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Damping values below this value will be ignored.

9th data block (only required if a list of elements or bodies to be given) 10th data block 1-10

1st

A

Enter the word CONDUCTIVITY.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default).

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Enter 0 to output global conductivity in untied state. Enter 1 to output global conductivity in tied state.

36-45

7th

E

Enter minimum value to be written to DMIG. Conductivity values below this value will be ignored.

11th data block (only required if a list of elements or bodies to be given)

Main Index

374 DMIG-OUT (Model Definition) Output Control of Matrices

Format Fixed

Free

Data Entry Entry

12th data block 1-10

1st

A

Enter the word SPECIFIC.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default).

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Specific heat values below this value will be ignored.

13th data block (only required if a list of elements or bodies to be given)

Main Index

DMIG 375 Direct Matrix Input

DMIG

Direct Matrix Input

Description This option is compatable with MD Nastran and allows the direct input of matrices at nodal points. It permits matrices generated with either product to be entered into Marc. The matrix is defined by a single header entry and one or more column entries. A column entry is required for each column with nonzero element. The matrix may only be used for real symmetric or nonsymmetric stiffness matrices, real mass matrices, or for load matrices. The matrices are not activated unless a K2GG, K2PP, M2GG, M2PP, or P2G model or history definition option is used. It is advisable to have K2GG, M2GG, etc. placec before the DMIG in the input file. Note:

This option must be in fixed format using the MD.Nastran conversion of ten fields per line of width 8 or 16.

Header Entry Format 1

2

3

4

5

6

7

8

DMIG

NAME

"0"

IFO

TIN

TOUT

POLAR

G1

C1

9

10

NCOL

Column Entry Format DMIG

NAME

GJ

CJ

G2

C2

A2

B2

DMIG

STIF

0

1

3

DMIG

STIF

27

1

2

4

2.5+10

A1

B1

3.+5

3.+3

1.0

0.

- etc. -

Example

Main Index

4 2

0.

50

3

376 DMIG Direct Matrix Input

Field

Contents

NAME

Name of the matrix. See Remark 1.(One to eight alphanumeric characters, the first of which is alphabetic.) The name is case sensitive.

IFO

Form of matrix input. IFO = 6 must be specified for matrices selected by the K2GG, M2GG and B2GG options. (Integer) 1 = Square 9 or 2 = Rectangular 6 = Symmetric

TIN

Type of matrix being input: (Integer) 1 = Real, single precision (One field is used per element.) 2 = Real, double precision (One field is used per element.) 3 = Complex, single precision (Two fields are used per element.) (not available) 4 = Complex, double precision (Two fields are used per element.) (not available)

TOUT

Type of matrix created (not used; enter 0).

POLAR

Input format of Ai, Bi. (Integer=blank or 0 indicates real, imaginary format; Integer > 0 indicates amplitude, phase format.)

NCOL

Number of columns in a rectangular matrix. Used only for IFO = 9. See Remarks 5 and 6 (Integer > 0)

GJ

Node identification number for column index. (Integer > 0)

CJ

Degree of freedom number for node point GJ. (1 < Integer < 6;)

Gi

Node identification number for row index. (Integer > 0)

Ci

Degree of freedom number for Gi for a grid point. (1
Ai, Bi

Real and imaginary (or amplitude and phase) parts of a matrix element. If the matrix is real (TIN = 1 or 2), then Bi must be blank. (Real)

Remarks 1. Matrices may also be selected for all simulations by K2GG = NAME and M2GG = NAME. 2. The header entry containing IFO, TIN, and TOUT is required. Each nonnull column is started with a GJ, CJ pair. The entries for each row of that column follows. Only nonzero terms need be entered. The terms may be input in arbitrary order. A GJ, CJ pair may be entered more than once, but input of an element of the matrix more than once produces a fatal message. 3. Field 3 of the header entry must contain an integer 0. 4. For symmetric matrices (IFO = 6), a given off-diagonal element may be input either below or above the diagonal. While upper and lower triangle terms may be mixed, a fatal message is issued if an element is input both below and above the diagonal.

Main Index

DMIG 377 Direct Matrix Input

5. The recommended format for rectangular matrices requires the use of NCOL and IFO = 9. The number of columns in the matrix is NCOL. (The number of rows in all rectangular DMIG matrices is always the number of nodal points.) The GJ term is used for the column index. The CJ term is ignored. 6. If NCOL is not used for rectangular matrices, it is taken to be the maximum number of degrees of freedom per node. 7. The matrix names must be unique among all DMIGs. 8. TIN should be set consistent with the number of decimal digits required to read the input data adequately. For a single-precision specification on a short-word machine, the input is truncated after about eight decimal digits, even when more digits are present in a double-field format. If more digits are needed, a double precision specification should be used instead. However, note that a double precision specification requires a “D” type exponent even for terms that do not need an exponent. For example, unity may be input as 1.0 in single precision, but the longer form 1.0D0 is required for double precision. Note:

Main Index

In Marc, all matrices are stored as double precision.

378 K2GG, K2PP (Model Definition) Selects Direct Input Stiffness Matrix

K2GG, K2PP (Model Definition)

Selects Direct Input Stiffness Matrix

Description This option activates or deactivates a stiffness matrix defined by the DMIG option. This option should be in the input file before the matrix is read in by the DMIG option. Note:

If transformation or rigid body rotations of the stiffness matrix are to occur, all degrees of freedom of the nodes must appear on the DMIG file.

Form0at Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word K2GG or K2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

36-40

5th

I

Not used; enter 0.

41-45

6th

I

Enter 0 to suppress the transformation to the stiffness matrix although a transformation has been applied to the node (default - this implies that the stiffness matrix used is provided in the transformed system). Enter 1 to apply transformations to the stiffness matrix.

46-50

7th

I

Enter first node number used to rigidly rotate the stiffness matrix.

51-55

8th

I

Enter second node number used to rigidly rotate the stiffness matrix.

56-60

9th

I

Enter third node number used to rigidly rotate the stiffness matrix.

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the stiffness matrix before any constraints are applied. 3. A scale factor may be applied to the stiffness matrix specified here or to all stiffness matrices via the COEFFICIENT model definition option, CK2 entry. 4. If a transformation is to be applied to the stiffness matrix, the DMIG must contain all of the degrees of freedom associated with the node to which the transformation is applied. 5. Large roataion DMIG is based upon the node numbers given in the 7th, 8th, and 9th fields. If only the 7th field is used, then the rotation is based upon the rotation degrees of freedom of this node. If all these nodes are specified, then a triad is formed, and the rotation of this triad is used.

Main Index

M2GG, M2PP (Model Definition) 379 Selects Direction Input Mass Matrix

M2GG, M2PP (Model Definition)

Selects Direction Input Mass Matrix

Description This option activates or deactivates a mass matrix defined by the DMIG option in a dynamic analysis. Format Format Fixe

Free

Data Entry Entry

1-10

1st

A

Enter the word M2GG or M2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the mass matrix before any constraints are applied. 3. The matrix must be symmetric and field 4 on DMIG, name entry must contain a 6. 4. M2GG input must either be in consistent mass units or the COEFFICIENT model definition option, CM2 entry may be used.

Main Index

380 B2GG, B2PP (Model Definition) Selects Direction Input Damping Matrix

B2GG, B2PP (Model Definition)

Selects Direction Input Damping Matrix

Description This option activates or deactivates a damping matrix for dynamic or harmonic analysis defined by the DMIG option in a dynamic analysis. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word B2GG or B2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the damping matrix before any constraints are applied. 3. The matrix must be symmetric and field 4 on DMIG, name entry must contain the integer 6. 4. A scale factor may be applied to the damping matrix specified here or to all damping matrices via the COEFFICIENT model definition option, CB2 entry.

Main Index

P2G (Model Definition) 381 Selects Direction Input Load Vector

P2G (Model Definition)

Selects Direction Input Load Vector

Description This option activates or deactivates a load vector defined by the DMIG option. This load vector may be scaled by referencing a table which is a function of time. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word P2G.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate the load vector. Enter -1 to deactivate the load vector.

26-30

4th

E

Enter scale factor; default is 1.0.

31-35

5th

I

Enter a table ID.

Remarks 1. Terms are added to the load matrix before any constraints are applied. 2. The matrix must be rectangular in form ( i.e., field 4 on DMIG entry - IFO -must contain the integer 9). 3. A scale factor may be applied to the vector specified here or to all vectors via the COEFFICIENT model definition option entry.

Main Index

382 BACKTOSUBS (Model Definition) Recover Substructure Output

BACKTOSUBS (Model Definition)

Recover Substructure Output

Description This option allows you to perform a displacement and stress calculation for the substructure. It can be followed by output control options, such as PRINT ELEMENT, PRINT CHOICE, POST, etc. The file containing the displacements of the external nodes is given using the -sid option when the job is submitted. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word BACKTOSUBS.

MNF UNITS 383 MD Adams Modal Neutral File Units

MNF UNITS

MD Adams Modal Neutral File Units

Description This option defines the units used to define the model. If this option is not included, default is SI units (kilogram, meter, second, Newton). This option is only used for creating the MNF file. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word MNF UNITS.

I

Enter mass unit:

2nd data block 1-5

1st

1: kilogram 2: pound mass 3: slug 4: gram 5: ounce mass 6: kpound mass 7: megagram 8: dozen slug 6-10

2nd

I

Enter length unit: 1: kilometer 2: meter 3: centimeter 4: millimeter 5: mile 6: foot 7: inch

11-15

3rd

I

Enter time unit: 1: hour 2: minute 3: second 4: millisecond

Main Index

384 MNF UNITS MD Adams Modal Neutral File Units

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter force unit: 1: newton 2: pound force 3: kilogram force 4: ounce force 5: dyne 6: kNewton 7: kpound force

Main Index

STIFSCALE 385 Define Stiffness Scaling Factor

STIFSCALE

Define Stiffness Scaling Factor

Description This option allows the contributions of an element stiffness and mass matrix to be scaled before including them into the global stiffness matrix. The distributed loads associated with the element are also scaled. Note that this is a scalar multiple; no transformation occurs. Caution:

If you use this option, you must define the scale factor for all elements; the default is zero.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word STIFSCALE.

2nd data block 1-5

1st

I

Enter number of sets to be entered (optional).

6-10

2nd

I

Enter unit number from which the following data is read. Defaults to input.

F

Enter scaling factor.

3rd data block 1-10

1st

4th data block Enter a list of elements for which the above scaling is applied.

Main Index

386 COEFFICIENT Define Scaling Coefficients for Matrices

COEFFICIENT

Define Scaling Coefficients for Matrices

Description This option allows you to put in global coefficients that can be used to either define or scale matrices. It allows compatibility with MD Nastran PARAM of the same names that are used here. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word COEFFICIENT.

2nd data block 1-10

1st

E

Enter the value of ALPHA1 mass coefficient of Rayleigh Damping (default=0.0). If the DAMPING model definition option is included, the value entered here is ignored.

11-20

2nd

E

Enter the value of ALPHA2 stiffness coefficient of Rayleigh Damping (default=0.0). If the DAMPING model definition option is included, the value entered here is ignored.

21-30

3rd

E

Enter the value of CB1, factor applied to spring damping matrix. Default is 1.0

31-40

4th

E

Enter the value of CB2, factor applied to damping DMIG, default is 0.0 unless, B2GG references DMIG.

41-50

5th

E

Enter the value of CK1, factor applied to element stiffness matrix, and springs. Default is 1.0

51-60

6th

E

Enter the value of CK2, factor applied to Stiffness DMIG; default is 0.0 unless, K2GG references DMIG.

61-70

7th

E

Enter the value of CK3, factor applied to stiffness matrix from user element (USELEM user subroutine). Default =1.0

3rd data block

Main Index

1-5

1st

I

Enter table ID for ALPHA1.

6-10

2nd

I

Enter table ID for ALPHA2.

11-15

3rd

I

Enter table ID for CB1.

16-20

4th

I

Enter table ID for CB2.

21-25

5th

I

Enter table ID for CK1.

26-30

6th

I

Enter table ID for CK2.

31-35

7th

I

Enter table ID for CK3.

COEFFICIENT 387 Define Scaling Coefficients for Matrices

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

E

Enter the value of CM1 factor applied to element mass matrix, and mass points. Default is 1.0

11-20

2nd

E

Enter the value of CM2, factor applied to Mass DMIG; default is 0.0 unless M2GG references DMIG.

21-30

3rd

E

Enter the value of CM3, factor applied to use-defined element mass matrix. Default is 1.0

31-40

4th

E

Enter the value of CP1, factor applied to external loads, this is only allowed if the ELASTIC parameter is included. Caution should be exercised if the load is due to centrifugal effects, as this reflects a scaling of the mass, not the rotational speed.

41-50

5th

E

Enter the value of CP2, factor applied to load DMIG; default is 0.0 unless P2G references DMIG.

51-60

6th

E

Enter the value of CP3, factor applied to external load associated with user-defined elements. Default is 1.0

61-70

7th

E

Enter the value of G, uniform structural coefficient in the formulation of dynamic problems. Default is 0.0

5th data block 1-5

1st

I

Enter table ID for CM1.

6-10

2nd

I

Enter table ID for CM2.

11-15

3rd

I

Enter table ID for CM3.

16-20

4th

I

Enter table ID for CP1.

21-25

5th

I

Enter table ID for CP2.

26-30

6th

I

Enter table ID for CP3.

31-35

7th

I

Enter table ID for G.

6th data block 1-10

1st

E

Enter the value of W3, coefficient in damping matrix; default is 0.0, indicating do not include term.

11-20

2nd

E

Enter the value of W4, coefficient in damping matrix; default is 0.0, indicating do not include term.

7th data block

Main Index

1-5

1st

I

Enter table ID for W3.

6-10

2nd

I

Enter table ID for W4.

388 COEFFICIENT Define Scaling Coefficients for Matrices

Remarks 1. If the DAMPING model definition option is used to specify different damping coefficients based upon the element number, it is assumed to be active for all elements, and ALPHA1, ALPHA2, and CB1 coefficients are ignored. 2. If the STIFSCALE model definition option is used to specify scale factors based upon the element number, it is assumed to be active for all elements and the CK1, CK3, CM1, CM3, CP1, and CP3 coefficients are ignored.

Main Index

DEACTIVATE (Model Definition) 389 Deactivate Elements

DEACTIVATE (Model Definition)

Deactivate Elements

Description This option allows you to deactivate elements during the course of an analysis, which can be useful to model ablation or excavation. By default, after the elements are deactivated, they demonstrate zero stresses and strains on the post file. However, internally, they retain the stress state in effect at the time of deactivation and this state can be postprocessed or printed at any time. At a later stage in the analysis, the elements can again be activated with the ACTIVATE history definition option. As an alternative, you can use the UACTIVE user subroutine. The stress state is restored on the post file when the elements are reactivated. If this is not desirable, the stress/strain states can be permanently set to zero at deactivation by using the additional command line option ‘STRESS/STRAIN’. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word DEACTIVATE.

11-20

2nd

A

Enter the word STRESS to set the stresses to zero.

21-30

3rd

A

Enter the word STRAIN to set the strains to zero.

31-40

4th

A

Enter the word POST to update the post file geometry so deactivated elements are not shown.

41-50

5th

A

Enter the word NOPO to not update the post file geometry; the deactivated elements are shown.

2nd data block 1-80

Main Index

1st

I

Enter the list of elements to be deactivated at this time.

390 ERROR ESTIMATE Create Error Estimation

ERROR ESTIMATE

Create Error Estimation

Description You can request that Marc give information regarding the error associated with the finite element discretization. There are two measures; the first evaluates the stress discontinuity between elements. A large value implies that the stresses gradients are not accurately represented in the finite element mesh. In a classical linear elastic solution, this could be resolved by choosing quadratic elements over linear elements or refining the mesh. The second error measure examines geometric distortion in the model. It first examines the aspect ratios and warpage of the elements and in subsequent increments measures how much these ratios change. This measure can be used to indicate if the original mesh is good and whether, at a later time, rezoning is required. The evaluation of the stress error measure is moderately expensive. The evaluation of the geometric error measure is very inexpensive. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ERROR ESTIMATE.

2nd data block

Main Index

1-5

1st

I

Enter 1 if the stress measure is to be evaluated.

6-10

2nd

I

Enter 1 if the geometric measure is to be evaluated.

USDATA 391 Invoke USDATA User Subroutine for Initialization

USDATA

Invoke USDATA User Subroutine for Initialization

Description This option invokes the call to the USDATA user subroutine for the initialization of user variables. These variables (data) are stored in a common block USDACM that can be used in other user subroutines. This option also provides for the definition of the amount of memory for the data in the common block in REAL*4 words. If this memory is specified as nonzero, the data is automatically saved on the restart file for use in subsequent analysis. Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-6

1st

A

Enter the word USDATA.

11-15

2nd

I

Enter the number of REAL*4 words needed for the data stored in common block USDAM via the USDATA user subroutine.

392 USDATA Invoke USDATA User Subroutine for Initialization

Main Index

Chapter 3: Model Definition Options 393 Program Control

Chapt Program Control er 3: This section of the document describes various program control options. The information in this section relevant to all types of analyses (mechanical, heat, Joule, bearing, acoustic, electrostatic, Mode ismagnetostatic, and electromagnetic). In particular, the CASE COMBIN option allows you to combine separate load cases obtained from elastic analyses. The SOLVER option is used to control the solution l procedure of the linearized equations. The default is the direct solvers; as an alternative, the iterative Defini solver can be chosen. The OPTIMIZE option is very important to minimize the computational cost of the analysis, as the cost of analysis is proportional to the square of the size of the bandwidth. (Options POST, tion PRINT CHOICE, PRINT ELEMENT, PRINT SPRING, PRINT CONTACT, PRINT NODE, NODE SORT, Optio SUMMARY, ELEM SORT, and UDUMP all control the amount and method that you can obtain the resultant quantities.) The RESTART option is important for all nonlinear analysis or for postprocessing ns with Marc. As the solution to nonlinear problems is obtained using the incremental technique, the RESTART option is used to stop the analysis (checkpoint) and then continue it at some later time. The REAUTO option is used to overwrite previously defined control values upon restarting an analysis. The POST option is used to control the database that is used by Marc Mentat and MD Patran for

postprocessing.

Main Index

394 CASE COMBIN Combine Load Cases

CASE COMBIN

Combine Load Cases

Description This option allows you to combine different load cases for an elastic analysis. Each load case must be stored on a RESTART file and then combined with other cases as a scalar multiple (LAMBDA) of itself. All output element variables and nodal variables are combined. This option can be used only in conjunction with the ELASTIC parameter. A new restart file of the resulting combination is written as increment 0 if it is requested. The use of the CASE COMBIN option precludes the addition of any further load cases in the same run. Cases can only be combined from restart files. This option can be used to perform the superposition of the results of a Fourier analysis at certain locations around the circumference. The positions for which superposition is requested can be either equally spaced or specified by you. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words CASE COMBIN.

2nd data block 1-5

1st

I

Number of load cases to be read in and combined.

6-10

2nd

I

Number of stations for superposition of Fourier analysis. If input as a positive number the stations are equally spaced around the circumference starting at θ = 0. If preceded by a minus sign, the θ - values are read from data lines.

3rd data block Only used for Fourier result superposition and if the second integer on the 2nd data block is negative. 1-10

1st

F

Value of θ in degrees for first printout station.

11-20

2nd

F

Value of θ in degrees for second printout station. Continuation data is in Format 8E10.0.

Main Index

CASE COMBIN 395 Combine Load Cases

Format Fixed

Free

Data Entry Entry

4th data block The 4th data block is repeated for each load case.

Main Index

1-5

1st

I

Increment number on restart file to be read for this load case.

6-10

2nd

I

Input file number for restart file to be read. Default is Unit 9.

11-20

3rd

F

LAMBDA – Scalar multiplication factor to be used with this load case. Default is 1.0.

396 SOLVER (Model Definition) Specify Direct or Iterative Solver

SOLVER (Model Definition)

Specify Direct or Iterative Solver

Description This option defines the solver to be used in the analysis. You can specify either the direct or iterative solver. The choice of whether the in-core or out-of-core procedure is used is automatically determined by Marc, based upon the amount of workspace required and the amount of memory that can be allocated. You can also select whether a symmetric or nonsymmetric solver is used. Additionally, you can specify if the solution of a nonpositive definite system is to be obtained. For DDM, an out-of-core procedure is only available for solver type 8. As a convenience, it is necessary to specify the control parameters for the decoupled pre-conditioner only in the first domain file, eliminating unnecessary editing. When the iterative solver, type 2 or type 9, is chosen, additional parameters must be defined which are used to control the accuracy. Note:

It is not recommended to use the iterative solver type 2 for beam or shell models, because these problems are ill conditioned, resulting in a large number of iterations. For a wellconditioned system, the number of iterations should be less than the square root of the total number of degrees of freedom in the system. You control the maximum number of iterations allowed. If this is a positive number, Marc stops if this is exceeded. If this is a negative number, Marc prints a warning and continues to the next Newton-Raphson iteration or increment.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SOLVER.

I

Solver Type, enter:

2nd data block 1-5

1st

0 for Profile Direct Solver. 2 for Sparse Iterative. 4 for Sparse Direct Solver 6 for Hardware Provided Direct Sparse Solver 8 for Multifrontal Direct Sparse Solver. 9 for CASI Iterative solver. 10 for mixed direct/iterative solver.

Main Index

SOLVER (Model Definition) 397 Specify Direct or Iterative Solver

Format Fixed

Free

Data Entry Entry

6-10

2nd

I

Enter 1 for solving a nonsymmetric system. Only available for solver types 0 and 8. (Not supported for DDM.)

11-15

3rd

I

Enter 1 if the solution of nonpositive definite system is to be obtained.

16-20

4th

I

Enter 0 if standard pre-conditioner is to be used. Enter 3 if decoupled pre-conditioner is to be used. Default value is 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter, in millions, the number of four-byte words to be used by solver type 6, 8, or 10 before going out-of-core. Default is the same behavior as for other solvers. For solver type 6, this option is only available on SGI. For solver type 8 or 10, it is available on all platforms.

41-45

9th

Not used; enter 0.

46-50

10th

Not used; enter 0.

51-55

11th

Not used; enter 0.

56-60

12th

Not used; enter 0.

61-65

13th

Not used; enter 0.

66-70

14th

Enter 1 to activate AUTOSPC when singularity occurs. This is only applicable to the direct solvers. Enter -1 to deactivate AUTOSPC.

The 3rd and 4th data blocks are only required for solver type 2 (sparse iterative) or solver type 9 (CASI). They may also be used with the solver type 10. 3rd data block 1-5

1st

I

Enter maximum number of conjugate-gradient iterations. Default is 1000. For solver type 10, set to 0.

6-10

2nd

I

Enter 1 if the previous solution is to be used as the initial trial solution.

11-15

3rd

I

Solver type 2: Enter 3 for diagonal preconditioner. Enter 4 for scaled-diagonal preconditioner. Enter 5 for incomplete Cholesky preconditioner. Solver type 9: Enter 0 for CASI Primal Preconditioner.

Main Index

398 SOLVER (Model Definition) Specify Direct or Iterative Solver

Format Fixed

Free

Data Entry Entry Enter 1 for CASI Standard Preconditioner. Solver type 10: Enter 0; not used.

4th data block 1-10

1st

F

Enter tolerance on conjugate gradient convergence for stress analysis. The default for solver type 2 is 1.e-3. The default for solver type 9 is 1.e-8. The default for solver type 10 is 1.e-4.

Main Index

OPTIMIZE 399 Invoke Bandwidth Optimizers

OPTIMIZE

Invoke Bandwidth Optimizers

Description This option allows a choice of bandwidth optimizers to be invoked and is used to reduce computer costs in larger problems. Note that this option creates an internal node numbering different from your node numbering, but that all data input and output is in your node numbering system. In addition, you can output the obtained correspondence table for later use. This correspondence table can then be read in subsequent analyses. In a deformable contact analysis, the bandwidth is re-optimized when the contact conditions change. Note:

Gap elements can change the internal node numbers. This can result in a non-optimal node numbering system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word OPTIMIZE.

11-15

2nd

I

Enter: 2 Cuthill-McKee algorithm. 5 Read externally supplied correspondence table from unit specified in the fifth field. 9 Sloan Algorithm (default). 10 Minimum Degree Algorithm (only available for sparse direct solver - Solver Type 4). 11 Metis Nested Dissection Algorithm (only available for Multifrontal Direct Sparse Solver - Solver Type 8 or 10). Note:

Main Index

If sparse direct solver is used, the minimum degree Algorithm is used by default.

16-20

3rd

I

Enter 1 to have optimized mesh (elements then nodes) written to a file. (Not available for optimizer 11.)

21-25

4th

I

Unit number of optimized mesh file. Only used if the third field is set to 1. Default is 18 if left blank.

400 OPTIMIZE Invoke Bandwidth Optimizers

Format Fixed

Free

Data Entry Entry

26-30

5th

I

Unit number of correspondence table. If the second field is not equal to 5 the correspondence table is written to this unit. If the second field is 5 then the correspondence table is read from this unit. (Not available for optimizer 11.)

31-35

6th

I

Print flag for correspondence table. Set to 1 to suppress print out (default). Set to 2 to print table. 0

Special treatment of nodes with LM for R-P Flow and gap elements for all analysis types (default).

1

Special treatment for all nodes with LM, all analysis types.

2

No special treatment for nodes with LM.

Option 2 – Cuthill-McKee 2nd data block 1-5

1st

I

Number of different numbering schemes to be tried. Usually less than 20.

Option 5 – User-specified Correspondence Table 2nd data block 1st

I

Internal node numbers, continuation in 16I5 format on logical unit number given in the fifth field of data block 1.

Option 9 – Sloan Algorithm No continuation data. Option 10 – Minimum Degree Algorithms No continuation data. Option 11 – Metis Nested Dissection Algorithms No continuation data.

Main Index

POST (Model Definition) 401 Create File for Postprocessing

POST (Model Definition)

Create File for Postprocessing

Description This option creates a postprocessor file for time-history or variable versus variable plots using Marc Mentat or your own postprocessing. In the latter case, the file is accessed via the utility PLDUMP given in Marc Volume D: User Subroutines and Special Routines. You have two possibilities for the post file in association with restarted runs: a. If the POST option follows the RESTART option, Marc first copies the previous post file onto the new post file (up to the restart increment), thus providing a continuous post file from the beginning of the analysis. The old post file is closed after it has been read. It is important that the POST option of the restart job requests the same post variables to be written to the post file as requested in the previous data file. Otherwise, loss of data or I/O errors can occur. b. If the POST option precedes the RESTART option, the new post file contains only those increments analyzed in the current run. One or the other options should be chosen – if (B) is used, a continuous post file is not created, so that (A) cannot subsequently be used for this analysis unless you combine the files with your own program. Note:

In a modal or buckling analysis in addition to POST option, the RECOVER history definition option must be used for storing eigenvectors on post file.

Element data is written to the post file for each integration point of a continuum element or for the integration points on the layer requested; unless, either the CENTROID parameter is used or the average value is requested via the 14th field.

Main Index

Note:

The stresses/strains are generally engineering stresses/strains in an analysis involving only small deformations. In a geometrically nonlinear analysis, if the total Lagrangian formulation is used, the stresses and the strains are the second Piola-Kirchhoff stress and the Green-Lagrange strains, respectively. You can always request to output Cauchy stresses (post code 41-47 and 341) in the post file. If the updated Lagrangian formulation is used in the large deformation analysis, the stresses and the strains are generally Cauchy stresses and the logarithmic strains, respectively.

Note:

Marc 2008 will be the last version to support post revisions less that 7.

402 POST (Model Definition) Create File for Postprocessing

Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word POST.

I

Number of element variables to be written on the file (optional)

2nd data block 1-5

1st

For heat transfer, by default, the temperatures are written to a post file. Enter -1 to suppresses this. 6-10

2nd

I

Unit number on which to open the new binary post file (jid.t16). Defaults to unit 16 if left blank. See Table B-1 in Appendix B.

11-15

3rd

I

Unit number on which to open the previous binary post file (rid.t16) for a restarted run. Defaults to unit 17 if left blank. Note that all data from this file (up to the restart increment) is copied to the new file upon restart, so that the post file is continuous from the start of the analysis, provided the POST option follows the RESTART option.

16-20

4th

I

Set to 0 for binary post file. Set to 1 for formatted post file. Set to 2 for both binary and formatted post file.

21-25

5th

I

Set to 2 to generate a single post file in DDM runs. Defaults to multiple post files.

26-30

6th

I

Unit number on which to open the new formatted post file (jid.t19). Defaults to unit 19. See Table B-1 in Appendix B.

31-35

7th

I

Unit number on which to open the previous formatted post file for a restart run. Defaults to unit 20. See Table B-1 in Appendix B.

36-40

8th

I

Set to 1 to convert restart file to post file with no analysis. Increments to be converted are given in the third and eleventh field of RESTART model definition section.

41-45

9th

I

Number of increments between writing of post data. Defaults to write post file every increment.

46-50

10th

I

Number of user-defined post vectors. Vector is defined UPOSTV in user subroutine. This field is only used for 7- and 8-style post files.

51-55

11th

I

Enter 1 to generate Marc K2 style post file. Enter 3 to generate Marc K3 style post file. Enter 4 to generate Marc K4 style post file.

Main Index

POST (Model Definition) 403 Create File for Postprocessing

Format Fixed

Free

Data Entry Entry Enter 5 to generate Marc K5 style post file. Enter 6 to generate Marc K6 style post file. Enter 7 to generate Marc K7 style post file. Enter 8 to generate Marc 8 (not released) style post file. Enter 9 to generate MSC.Marc 2000 style post file. Enter 10 to generate MSC.Marc 2001 style post file. Enter 11 to generate MSC.Marc 2003 style post file. Enter 12 to generate MSC.Marc 2005 style post file (default). Enter 13 to generate MSC.Marc 2005r3 style post file.

56-60

12th

I

This field can be used for debugging purposes in a stress analysis: Enter 0 if no iterative data is needed. Enter 1 to get the iterative displacements. Enter 2 to get the iterative displacements and reaction/residual forces. Enter 3 to get the iterative displacements, reaction/residual forces and the touched bodies in a contact analysis. The iterative data is written as subincremental data. Note:

61-65

13th

I

The use of this option can generate a huge post file since the post data is written for every iteration.

Only for MSC.Marc 2000 and higher style post file. Enter the total number of nodal post codes (including user-defined nodal post codes). If a 0 is entered a default set of nodal data is written on the post file, depending on the analysis type. If a -1 is entered, no nodal data is written. Note:

66-70

14th

I

Displacements are not automatically written in the custom post file unless explicitly chosen. Besides the chosen quantities, if the deformation also needs to be visualized then the displacements also need to be chosen as nodal quantities.

Enter 1 if per element only the average element integration point data should be written on the post file. This might considerably reduce the size of the post file, but some significant information might be lost. The default is 0 where the element data is written on the post file for all available integration points.

71-75

Main Index

15th

I

Enter 1 if automatically generated extra nodes associated with element types 80-84 and 155-157 do not appear on the post file.

404 POST (Model Definition) Create File for Postprocessing

Format Fixed

Free

Data Entry Entry The default is 0, where all the available nodes are written on the post file.

76-80

16th

I

Enter 1 to exclude forces caused by glued contact from the contact normal and friction forces. The default is 0 where the contact normal and friction forces also contain the contributions due to glued contact.

Data blocks 3 and 4 are used for input of variables to be written on the post file. For 8- and lower style post files, only element data can be selected and the nodal data is written by default. For 9- and higher style post files, both element and nodal data can be selected. This data block is repeated for all selected element variables, and, for 9- and higher style post files, all selected nodal variables. 3rd data block (POST Version 13) Use for defining element post codes. 1-10

1st

A

Enter the word ELEMENT.

11-15

2nd

I

Enter an element post code. The code numbers are described in Table 3-4.

16-20

3rd

I

Enter the layer number for shell elements or continuum composite elements. For post codes 471 and 481, enter the global identification number of the rebar layer

21-68

4th

A

Enter a 48-character label associated with this post code for use in postprocessing.

3rd data block (POST Version 12 and earlier) 1-5

1st

I

Enter an element post code. The code numbers are described in Table 3-4.

6-10

2nd

I

Enter the layer number for shell elements or continuum composite elements. For post codes 471 and 481, enter the global identification number of the rebar layer

11-35

3rd

A

Enter a 24-character label associated with this post code for use in postprocessing.

4th data block Use for defining nodal post codes.

Main Index

1-10

1st

A

Enter the word NODAL.

11-15

2nd

I

Enter a nodal post code. The code numbers are described in Table 3-5.

16-63

3rd

A

Enter a 48-character label associated with this post code for use in postprocessing.

POST (Model Definition) 405 Create File for Postprocessing

Format Fixed

Free

Data Entry Entry

Data blocks 5, 6, and 7 are used for post file version 13 or higher to select elements and nodes to be written on the post file. They are all optional. If none of the block is present, all elements are written in the post file. 5a data block 1-10

1st

A

Enter the words SELECT ELEMENT

I

Enter a list of elements to be written to post file.

5b data block 1-80

1st

6a data block 1-10

1st

A

Enter the words SELECT BODY

11-15

2nd

I

Enter 1 if all elements of the selected contact body are placed on post file (default) Enter 2 if only the elements on the exterior surface are placed on the post file.

6b data block 1-80

I

Enter a list of contact bodies, for which the elements are to be written to post file.

For the 7th data block, these nodes are in addition to nodes based upon element selection; typically, it would be used for nodes not associated with elements. 7a data block 1-10

1st

A

Enter the words SELECT NODE

I

Enter a list of nodes to be written to post file.

7b data block 1-80

Main Index

406 POST (Model Definition) Create File for Postprocessing

Table 3-4

Element Post Codes

Codes

Main Index

Description

1-6

Components of strain. For rigid-perfectly plastic flow problems, components of strain rate

7

Equivalent plastic strain (integral of equivalent plastic strain rate). For rigid-perfectly plastic flow problems, equivalent plastic strain rate

8

Equivalent creep strain (integral of equivalent creep strain rate)

9

Total temperature

10

Increment of temperature

11-16

Components of stress

17

Equivalent von Mises stress

18

Mean normal stress (tensile positive) for Mohr-Coulomb

19

User-defined variable via the PLOTV user subroutine. See Marc Volume D: User Subroutines and Special Routines.

20

Thickness of element

21-26

Components of plastic strain

27

Equivalent plastic strain. ε

28

Plastic strain rate

29

Total value of second state variable

30

Forming Limit Parameter: FLP = calculated major engineering strain/maximum major engineering strain

31-36

Components of creep strain

37

Equivalent creep strain. ε

38

Total swelling strain (from the VSWELL user subroutine)

39

Total value of third state variable

41-46

Components of Cauchy stress

47

Equivalent Cauchy stress

48

Strain energy density

49

Thickness strain for plane stress: Mooney or Ogden material

51-56

Real components of harmonic stress

57

Equivalent real harmonic stress

58

Elastic strain energy density

59

Equivalent stress/yield stress

60

Equivalent stress/yield stress (at current temperatures)

c

p

2 --- Σ Δ ε ipj ΣΔ ε ijp 3

=

=

2 --- ΣΔ ε icj Σ Δε ijc 3

POST (Model Definition) 407 Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Main Index

Description

61-66

Imaginary components of harmonic stress

67

Equivalent imaginary harmonic stress

68

Plastic strain energy density

69

Current volume

71-76

Components of thermal strain

78

Original volume

79

Grain size

80

Damage indicator for Cockroft-Latham, Oyane, and Principal Stress criteria, and criteria using the UDAMAGE_INDICATOR user subroutine.

81-86

Components of cracking strain (only for stress analysis)

91-107

Failure indices associated with failure criteria

108-109

Interlaminar shear for thick composite shells (TSHEAR parameter must be present)

110

Interlaminar shear bond index for thick composite shells (only available if TSHEAR parameter is present and Allowable Shear Bond Stress, SB, has been prescribed on the COMPOSITE option) = max(Interlaminar shear components given by post codes 108 and 109)/SB

111-116

Components of stress in preferred coordinate system defined by the ORIENTATION option

121-126

Elastic strain

127

Equivalent elastic strain

128

Major engineering strain

129

Minor engineering strain

175

Equivalent viscoplastic strain rate (powder material)

176

Relative density (powder material)

177

Void volume fraction (damage model)

178

Lemaitre damage factor

179

Lemaitre relative damage

<0

User-defined variable via the PLOTV user subroutine. See Marc Volume D: User Subroutines and Special Routines.

241

Gasket Pressure

242

Gasket Closure

243

Plastic Gasket Closure

251

Global components of Interlaminar normal stress; layer n is between n and n+1

254

Global components of Interlaminar shear stress; layer n is between n and n+1

408 POST (Model Definition) Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Description

257

Interlaminar shear bond index for composite solids (only available if Allowable Shear Bond Stress, SB, has been prescribed on the COMPOSITE option) = magnitude of interlaminar shear vector calculated by post code 254/SB

261

Beam axis (required if beam moment plots are created with Marc Mentat). Orientation axis of CBUSH/CFAST elements 194 and 195.

264

Axial Force

265

Moment Mxx

266

Moment Myy

267

Shear Force Vxz

268

Shear Force Vyz

269

Torque

270

Bimoment

301

Total strains tensor

311

Stress tensor

321

Plastic strain tensor

331

Creep strain tensor

341

Cauchy stress tensor

351

Real harmonic stress tensor

361

Imaginary harmonic stress tensor

371

Thermal strain tensor

381

Cracking strain tensor

391

Stresses in preferred direction tensor

401

Elastic strain tensor

411

Stress in global coordinate system tensor

421

Elastic strain in global coordinate system tensor

431

Plastic strain in global coordinate system tensor

441

Creep strain in global coordinate system tensor

451

Velocity strains (for fluids)

461

Elastic strain in preferred direction tensor

471

Global components of the rebar stresses in the undeformed configuration (Second Piola-Kirchhoff). See Marc Volume B: Element Library for details.

481

Global components of the rebar stress in the deformed configuration (Cauchy). See Marc Volume B: Element Library for details.

Main Index

POST (Model Definition) 409 Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Description

487

Rebar angle.

501

Interlaminar normal stress; layer n is between n and n+1. See Marc Volume B: Element Library for details.

511

Interlaminar shear stress; layer n is between n and n+1. See Marc Volume B: Element Library for details.

531

Volume fraction of Martensite.

541

Phase transformation strain tensor.

547

Equivalent Phase Transformation strain PH = ε eq

548

Equivalent TWIN Strain T WIN = ε eq

549

IP 2 ⁄ 3Σ Δε ijTRI P Σ Δ ε iTR j

Equivalent Plastic Strain in the Multiphase Aggregate: PL = ε eq

Main Index

2 ⁄ 3ΣΔ ε ijTWI N Σ Δ ε ijTWI N

Equivalent TRIP Strain in the forward transformation T RIP = ε eq

551

2 ⁄ 3ΣΔ ε ijPH Σ Δ ε ijPH

PL 2 ⁄ 3 ΣΔ ε iPL j Σ Δ εi j

552

Equivalent Plastic Strain in the Austenite

553

Equivalent Plastic Strain in the Martensite

557

Yield Stress of Multiphase Aggregate

601-617

Strength ratios based upon FAIL DATA failure modes.

621

Generalized Strain (Harmonic only)

631

Imaginary Generalized Strain (Harmonic only)

641

Generalized Strain - curvatures tensor

661

Generalized Stress - Moments tensor

681

True Strain Tensor (for continuum elements)

691

Element Orientation Vector 1

694

Element Orientation Vector 2

697

Layer Orientation Angle

410 POST (Model Definition) Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Description

Post Codes for Heat Transfer Analysis 9 or 180

Total temperature

181-183

Components of temperature gradient T

184-186

Components of flux

271

Volumetric Mass density of pyrolysised solid (model C) or nonhomogeneous density

272

Volumetric Mass density of pyrolysis gas (model C)

273

Volumetric Mass density of liquid (model C)

274

χp

(Pyrolysis model B or C)

275

φw

(Pyrolysis model B or C)

276

χc

(Pyrolysis model B or C)

277

ρc

278

k

279

ρ g, w

280

mg

281

· ρ s, p

(Pyrolysis model C only)

282

· ρ s, l

(Pyrolysis model C only)

283

· ρ s, c

(Pyrolysis model C only)

ef f

eff

(Pyrolysis model B or C)

(Pyrolysis model B or C) Pyrolysis Volumetric Mass density of water vapor

(Pyrolysis model B or C)

Post Codes for Bearing Analysis 190

Pressure

191-193

Components of pressure gradient

194-196

Mass flux vector

Post Codes for Joule Heating Analysis 87

Voltage

88

Distributed current

89

Heat generated

197-199

Components of electric potential gradient

577-579

Components of current density

Post Codes for Acoustic Analysis

Main Index

190

Pressure

191-193

Components of pressure gradient

POST (Model Definition) 411 Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Description

Post Codes for Electrostatic Analysis 130

Electric potential (V)

561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

Post Codes for Magnetostatic Analysis 140

Magnetic potential (2-D analysis only) (Az)

571-573

Components of magnetic induction (B)

574-576

Components of magnetic field intensity (H)

Post Codes for Transient Electromagnetic Analysis 561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

567-569

Components of Lorentz force

571-573

Components of magnetic induction (B)

574-576

Components of magnetic field intensity (H)

577-579

Components of current density (J)

Post Codes for Harmonic Electromagnetic Analysis 131-133

Real components of electric field intensity (E)

134-136

Real components of electric displacement (D)

137-139

Real components of Lorentz force

141-143

Real components of magnetic induction (B)

144-146

Real components of magnetic field intensity (H)

147-149

Real components of current density (J)

151-153

Imaginary components of electric field intensity (E)

154-156

Imaginary components of electric displacement (D)

157-159

Imaginary components of Lorentz force

161-163

Imaginary components of magnetic induction (B)

164-166

Imaginary components of magnetic field intensity (H)

167-169

Imaginary components of current density (J)

Post Codes for Piezoelectric Analysis (Electrical Part)

Main Index

561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

412 POST (Model Definition) Create File for Postprocessing

Table 3-4

Element Post Codes (continued)

Codes

Description

Post Codes for Harmonic Piezoelectric Analysis (Electrical Part) 131-133

Real components of electric field intensity (E)

134-136

Real components of electric displacement (D)

151-153

Imaginary components of electric field intensity (E)

154-156

Imaginary components of electric displacement (D)

Post Codes for Soil Analysis 171

Porosity

172

Void ratio

173

Pore pressure

174

Preconsolidation pressure

Post Codes for Cure and Cure Shrinkage Analysis 285

Degree of cure

286

Total cure reaction heat

287

Degree of cure shrinkage

288

Volumetric cure shrinkage of resin

289-294

Cure shrinkage strain components in global coordinate system

295-300

Cure shrinkage strain components in preferred coordinate system

581-586

Cure shrinkage strain tensor in global coordinate system

591-596

Cure shrinkage strain tensor in preferred coordinate system

Notes:

For heat transfer, code 9 is used for all heat transfer elements. When using shells in heat transfer, it is important to enter a code for each layer in chronological order if post file is to be correctly read by the INITIAL STATE or CHANGE STATE options. Note that you do not need to select nodal values (that is, displacement, velocities and accelerations, and temperature for a heat transfer run) as these are automatically written to the post file. Eigenmodes (dynamic analysis) and eigenvectors (buckling analysis) are written to the post file only if indicated by the RECOVER or MODAL INCREMENT/BUCKLE INCREMENT option. Layered quantities for beams, shells, composite shells, composite solids, and rebar quantities.

Main Index

POST (Model Definition) 413 Create File for Postprocessing

For many post codes, a layer number is required, and is conventionally one to the last layer number in the element. Layer 1 is the top layer, layer 2 is the next layer, etc. for shells, composite shells, bricks, or rebar elements. In many shell applications, the number of layers in different elements is not the same. Two alternative mechanisms may be used to specify the layer number: I.The user can specify the following layer codes: 15000 - top layer 10000 - bottom layer 5000 - middle layer If the number of layers in a shell is an even number, it will use (nlayer +1)/2 where nlayer is the number of layers. II.If the user specifies the layer ID for the composite elements, then the user must specify the layer ID. This is useful in ply drop-off simulations. Note that post codes 91-107 refer to failure indices for different failure criteria and post codes 601-617 refer to associated strength ratios. More than 17 quantities are allowed in the analysis but only the first 17 quantities are available for postprocessing. For example. if three failure criteria (say, max. stress, Hoffman and Puck) are flagged, post codes 9197/601-607 would contain the six indices/ratios associated with maximum stress, post code 98 / 608 would contain the one index / ratio associated with Hoffman and post codes 99103 / 609-613 would contain the five indices / ratios associated with Puck criterion. Post codes 691 and 694 provide access to the first and second orientation vectors respectively. These vectors depict the alignment of the material coordinate system at the element level with respect to the global cartesian system. They are available for elements that are either composites, or using materials that are orthotropic/anisotropic / requiring the HOOKLW ANELAS user subroutines, or using the ORIENTATION option to identify the material coordinate system. Note that these element orientation vectors are averaged across all integration points of the element and presented as a single set of vectors at the element centroid. They are always calculated on the current element geometry and any layer IDs associated with post codes 691 and 694 are ignored. Note also that while the normal usage of these post vectors is in conjunction with the ORIENTATION option, if no special material orientation is provided, then they can also be used to obtain the element coordinate system for orthotropic materials, composites, etc. For composites, post code 697 provides access to the fiber angle in any layer. If used without any associated layer id, post code 697 provides access to all layer angles. Else, the user can obtain the angle for a specific layer L by using 697,L as the post code. Note that if there are no composite elements, post code 697 is ignored. The orientation vectors on the post file are available for visualization in Marc Mentat. Either element orientations or layer orientations can be plotted. Note that for layer orientation vectors to be available for a set of layers, the associated layer orientation angle should be available on the post file through post code 697.

Main Index

414 POST (Model Definition) Create File for Postprocessing

For post codes 411, 421, 431, and 441, global quantities for shell elements are reported for as many layers as requested and the same layer numbering system is used as for regular shell quantities. Layer 1 is the top surface; layer 2 is the next surface, etc. This convention is followed from MSC.Marc 2000 on. Caution has to be exercised in interpreting the results when strain and/or stress tensors are requested for beam and shell elements: 1. For most elements in this category (elastic beam elements 31, 52, 98 are exceptions), stress tensors (post codes 311, 351, 361) or their associated component values (post codes 11-16, 51-56, 61-66) and total strain tensor (post code 301) or its associated component values (post codes 1-6) can be requested with or without an associated layer number. When no layer number is requested, the generalized strains (stretches, shear strains) are reported for the strain post values and generalized stresses (axial force, shear forces) are reported for the stress post values. Generalized curvature strains and generalized moments can be requested through post codes 641 and 661 for shells and numerically integrated beams. Note that for shell elements, the generalized stresses are forces per unit length. Refer to Marc Volume B: Element Library for a definition of the generalized strain and stress output for each element type. When a layer number is used, the actual strain and stress components at the requested layer are reported. Layer number are ignored for post codes 641 and 661. 2. For conventional (non-numerically integrated) elastic beams (types 31, 52, 98), there are no layers - so only the generalized strains and stresses are reported for these elements. Refer to Marc Volume B: Element Library for a definition of the generalized strain and stress output for each element type. Equivalent quantities are not computed for these element types since they do not make physical sense. The thermal strain tensor (post code 371) or its associated components (post codes 71-76) are available. 3. For other stress tensors (post codes 341, 391, 411) and strain tensors (post codes 321, 331, 371, 381, 401, 421, 431, 441, 461), there are no generalized values and they can only be requested for a particular layer. If no layer number is provided by the user, by default, the tensors are reported for layer number 1. Numerically integrated solidsection beam elements (type 52 or 98) have layer numbers and from a postprocessing perspective behave as open or closed section beams or shells.

Main Index

POST (Model Definition) 415 Create File for Postprocessing

Table 3-5

Nodal Post Codes

Code 1 Displacement 2 Rotation 3 External Force 4 External Moment 5 Reaction Force 6 Reaction Moment 7 Fluid Velocity 8 Fluid Pressure 9 External Fluid Force 10 Reaction Fluid Force 11 Sound Pressure 12 External Sound Source 13 Reaction Sound Source 14 Temperature 15 External Heat Flux 16 Reaction Heat Flux 17 Electric Potential 18 External Electric Charge 19 Reaction Electric Charge 20 Magnetic Potential 21 External Electric Current 22 Reaction Electric Current 23 Pore Pressure 24 External Mass Flux 25 Reaction Mass Flux 26 Bearing Pressure 27 Bearing Force 28 Velocity 29 Rotational Velocity 30 Acceleration 31 Rotational Acceleration 32 Modal Mass

Main Index

Description

416 POST (Model Definition) Create File for Postprocessing

Table 3-5

Nodal Post Codes (continued)

Code

Description

33 Rotational Modal Mass 34 Contact Normal Stress 35 Contact Normal Force 36 Contact Friction Stress 37 Contact Friction Force 38 Contact Status 39 Contact Touched Body 40 Herrmann Variable 41

ρ sol id

42

M· g

43

· ρ s, p

(Pyrolysis Model B only)

44

· ρ s, l

(Pyrolysis Model B only)

(Pyrolysis Model B only)

(Pyrolysis Model B or C)

46 Tying Force 47 Coulomb Force 48 Tying Moment 49 Generalized Nodal Stress 50 Generalized Nodal Strain 51 Inertia Relief Load 52 Inertia Relief Moment 53 J-Integral 54 Stress Intensity, Mode I 55 Stress Intensity, Mode II 56 Stress Intensity, Mode III 57 Energy Release 58 Energy Release Rate I 59 Energy Release Rate II 60 Energy Release Rate III 61 — 62 Crack System Local X 63 Crack System Local Y 64 Crack System Local Z

Main Index

POST (Model Definition) 417 Create File for Postprocessing

Table 3-5

Nodal Post Codes (continued)

Code

Description

65 Near Contact Distance 66 Breaking Index (Normal) 67 Breaking Index (Tangential) 68 Breaking Index 69 Delamination Index (Normal) 70 Delamination Index Tangential) 71 Delamination Index 72 Recession 73 Glue Deactivation Status 74 VCCT Failure Index <0 User-defined nodal quantity via the UPSTNO user subroutine.

Note: The contact status (code 38) can have the following values: 0 if a node is neither in contact nor has tying constraints due to cyclic symmetry. 0.5 if a node is in near contact. 1 if a node is in true contact. 2 if a node has tying constraints due to cyclic symmetry.

Main Index

418 LOADCASE (Model Definition) Define Loadcase

LOADCASE (Model Definition)

Define Loadcase

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option is used to specify the boundary conditions and initial conditions that are active in this loadcase. This is used to activate or deactivate FIXED DISP, FIXED TEMPERATURE, etc., DIST LOADS, DIST FLUXES, etc., POINT LOAD, POINT FLUX, etc., FOUNDATION, FILMS, INITIAL DISP, INITIAL VEL, INITIAL TEMP, etc. Boundary conditions not explicitly activated are deactivated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word LOADCASE.

11-32

2nd

A

Enter the name of the loadcase (no blanks).

I

Enter the number of labels. This is required.

2nd data block 1-5

1st

3rd data block (Repeat as many times as specified on 2nd data block.) 1-32

1st

A

Enter the boundary condition or initial condition label.

33-40

2nd

I

Enter flag to control application of this boundary condition. This is applicable to FIXED DISP, DIST LOADS, POINT TEMP, and CHANGE STATE only. If a time dependent table (independent variable types 1,2,3,4) is applied to this boundary condition, this flag is ignored and the table is used to control the temporal variations. Enter 0 if load is applied instantaneously, or if boundary condition has been previously activated, it remains constant (default). Enter 1 if point load, distributed load or kinematic load is to be linearly changed from current magnitude to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state.

Main Index

LOADCASE (Model Definition) 419 Define Loadcase

Format Fixed

Free

Data Entry Entry Enter 2 if point load, distributed load or kinematic load is to be linearly changed from zero to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state. If the boundary condition is not included in a subsequent loadcase: point load, distributed load or kinematic load is linearly reduced in magnitude to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”. Enter 3 if point load, distributed load or kinematic load is to be linearly changed from zero to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state. If the boundary condition is not included in a subsequent loadcase: point load, distributed load is linearly reduced in magnitude to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”. Enter -1 or -2 load is removed “gradually”. point load, distributed load or kinematic load is linearly reduced in magnitude to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”. Enter -3 load is removed “gradually”,

Main Index

420 LOADCASE (Model Definition) Define Loadcase

Format Fixed

Free

Data Entry Entry point load, distributed load is linearly reduced in magnitude to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is linearly ramped to the initial temperatures, change state is linearly ramped to the “initial state”. Enter -4 Load is removed instantaneously, point load, distributed load is instantaneously reduced to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is instantaneously changed to the initial temperature, change state is instantaneously changed to the “initial state”. When POINT TEMP is used, the initial temperatures are prescribed in the INITIAL TEMP option. When CHANGE STATE is used, the “initial temperatures” are prescribed in the CHANGE STATE option.

Main Index

TRACK 421 Enter a List of Points to be Tracked

TRACK

Enter a List of Points to be Tracked

Description The analysis program creates a file containing information regarding the motion of a material particle which is at the coordinate position of the node in the undeformed state. This file is then used by the graphical user interface to visualize the motion of the point. It is also possible to track the material behavior (equivalent stress and equivalent plastic strain). This can be used for time history plots. This information is written to a file, jid.trk. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the work TRACK.

2nd data block 1-5

1st

I

Enter the number of nodal lists. Default is 1.

6-10

2nd

I

Unit number to read list of nodes. Defaults to input.

11-15

3rd

I

Enter 0 if no quantities are to be tracked. Enter 1 to track equivalent stress and equivalent plastic strain. Enter -1 if quantities specified in the 3rd data block are to be tracked.

16-20

4th

I

Enter the body number which contains these nodes. This is optional, but it does speed up the calculation.

3rd data block 1-10

1st

A

Enter the word QUANTITY.

11-15

2nd

I

Enter the element post code of the quantity to be tracked (see Table 3-4 in the POST option description).

16-40

3rd

I

Enter a 24 character label associated with this quantity for use in postprocessing.

4th data block Enter a list of nodes to be tracked.

Main Index

422 FLOW LINE Define a Flow Line Grid

FLOW LINE

Define a Flow Line Grid

Description This option allows you to define a grid (possibly independent of the original mesh) which is tracked during the analysis. This information is written to the post file. This facilitates viewing the motion of the material particles. Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the words FLOW LINE.

I

Enter 1 if original mesh is used as a grid.

2nd data block 1-5

1st

Enter 2 if Cartesian grid is used. Enter 3 if flow line file is used. See Appendix G Flow Line FIle Format: for the format of the .flw file. Enter 4 if circular grid is used for 2-D analysis only. The initial diameter will be 80% of the grid size specified in the 3rd data block. 6-10

2nd

I

Enter the body number to be flow lined. Default is body 1. Enter -1 to put flow lines on all bodies.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Number of segments used to draw flow line. Default =

5 for original mesh grid

= 100 for Cartesian grid =

50 for circular grid

3rd data block Required if a Cartesian or circular grid is used, Option 2 or 4. 1-5

1st

I

Enter 0 if Marc is to position grid. Enter 1 if grid is to pass through a point specified in the 8th, 9th, or 10th field.

6-10

Main Index

2nd

I

Enter the number of grid atoms in the x-direction.

FLOW LINE 423 Define a Flow Line Grid

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter the number of grid atoms in the y-direction.

16-20

4th

I

Enter the number of grid atoms in the z-direction.

21-30

5th

F

Enter the grid spacing in the x-direction.

31-40

6th

F

Enter the grid spacing in the y-direction.

41-50

7th

F

Enter the grid spacing in the z-direction.

51-60

8th

F

Enter the x-coordinate of the reference point.

61-70

9th

F

Enter the y-coordinate of the reference point.

71-80

10th

F

Enter the z-coordinate of the reference point.

3rd data block Required if flow line file is used, Option 3. 1-80

Main Index

1st

A

Enter the flow line file name.

424 IRM Intergraph Interface

IRM

Intergraph Interface

Description This option allows you to generate an IRM file which is compatible with Intergraph. Two types of quantities can be on this file: element and nodal quantities. The element quantities (stresses, strains, etc.) can either be component values or invariant values or both. They are each an average value within the element. The nodal quantities are values extrapolated from the integration points and a weighted average is calculated. Extreme care should be used interpreting the results with beam and/or shell elements. If the IRM option is used simultaneously with either or both of the SDRC and HYPERMESH options, internally the program treats the data in a cumulative manner. For example, if stresses are requested for the Intergraph file and creep strains are requested for the SDRC Universal file, both quantities are output into both files. The Intergraph results file is named jid.g. Note:

When the Intergraph results file is requested together with the Hypermesh results file, the invariant element quantities are automatically written into the Intergraph results file.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word IRM.

11-15

2nd

I

Enter the unit number to which to write file; default is 39.

16-20

3rd

I

Frequency to write out file.

If no element data is required, skip to the 4th data block. 2nd data block 1-10

1st

A

Enter the word ELEMENT.

Repeat 3rd data block as often as required. 3rd data block 1-5

Main Index

1st

I

Enter: 1

for stresses.

2

for total generalized strains.

3

for creep strains.

4

for thermal strains.

5

for plastic strains.

IRM 425 Intergraph Interface

Format Fixed

6-10

Free

2nd

Data Entry Entry

I

6

for strain energy.

7

for von Mises equivalent stress divided by the yield stress.

8

for failure indices.

Enter a layer number if shell elements. If the value in the first field is a 2, enter 0.

11-15

3rd

I

Enter 0 for component values. Enter 1 for invariants. Enter 2 for component and invariant values. Note:

When the Intergraph results file is requested together with the Hypermesh results file, the invariant element quantities are automatically written into the Intergraph results file.

If no nodal data is required, skip to the next model definition point. 4th data block 1-8

1st

A

Enter the word NODAL.

Repeat 5th data block as often as required 5th data block 1-5

1st

I

Enter: 1 for displacements. 2 for velocities. 4 for reaction forces. 5 for temperatures. 6 for generalized stresses. 7 for generalized strains. 8 for top/middle/bottom layer stresses. 9 for top/middle/bottom elastic strains. 10 for top/middle/bottom plastic strains. 11 for top/middle/bottom creep strains. 13 for eigenmodes. 14 for harmonic displacements and reactions. Note:

Main Index

If shell elements are not included in the model, specifying 8, 9, 10, or 11 results in only the top or actual component.

426 IRM Intergraph Interface

Internals of IRM files Element Data CAT = ELEM TYPE - A.B.C.D where A = S for stress E for total strain C for creep strain T for thermal strain P for plastic strain B = C for component I for invariant C = 1 for 1st component 2 for 2nd component 3 for 3rd component 4 for 4th component 5 for 5th component 6 for 6th component or C = 1 for lowest principal 2 for intermediate principal 3 for highest principal 4 for Von Mises Intensity 5 for mean normal (hydrostatic) 6 for Tresca D=

layer number

If strain energy is requested, then: TYPE A.D where

A = ETT for total strain energy density ETI for incremental strain energy density EET for total elastic strain energy density EEI for incremental elastic strain energy density EPT for total plastic strain energy density EPI for incremental plastic strain energy density D = layer number

Main Index

IRM 427 Intergraph Interface

If stress/yield stress is requested, then: TYPE A.D where

A = SYI for stress/original yield stress SYT for stress/yield stress at current temperature D = layer number

If failure indexes are requested, then: TYPE A.B.D where

A = FL B = 1 to 6 D = layer number

Nodal Data CAT = NODE TYPE = A.B.C. A= D

Main Index

for displacement

V

for velocity

A

for acceleration

R

for reactions

E

for eigenmode

M

for magnitude of harmonic displacement

P

for phase of harmonic displacement

N

for magnitude of harmonic reaction

Q

for phase of harmonic reaction

TEMP

for temperatures

GSC

for generalized stress components

GSI

for generalized stress invariants

GNC

for generalized strain components

GNI

for generalized strain invariants

TSC

for stress components, top layer

TSI

for stress invariants, top layer

MSC

for stress components, middle layer

MSI

for stress invariants, middle layer

BSC

for stress components, bottom layer

BSI

for stress invariants, bottom layer

428 IRM Intergraph Interface

TEC

for elastic strain components, top layer

TEI

for elastic strain invariants, top layer

MEC

for elastic strain components, middle layer

MEI

for elastic strain invariants, middle layer

BEC

for elastic strain components, bottom layer

BEI

for elastic strain invariants, bottom layer

TPC

for plastic strain components, top layer

TPI

for plastic strain invariants, top layer

MPC

for plastic strain components, mid layer

MPI

for plastic strain invariants, mid layer

BPC

for plastic strain components, bottom layer

BPI

for plastic strain invariants, bottom layer

TCC

for creep strain components, top layer

TCI

for creep strain invariants, top layer

MCC

for creep strain components, mid layer

MCI

for creep strain invariants, mid layer

BCC

for creep strain components, bottom layer

BCI

for creep strain invariants, bottom layer

B= X

for the X direction

Y

for the Y direction

Z

for the Z direction

THX

for rotation about X

THY

for rotation about Y

THZ

for rotation about Z

Skipped if A is not D, V, A or R C = 1 for 1st component 2 for 2nd component 3 for 3rd component 4 for 4th component 5 for 5th component 6 for 6th component

Main Index

IRM 429 Intergraph Interface

Skipped if A is D, V, A, or R I=

1 for minimum principle value 2 for intermediate principle value 3 for maximum principle value 4 for von Mises intensity 5 for dilatational value 6 for Tresca intensity

Main Index

430 SDRC SDRC I-DEAS™ Interface

SDRC

SDRC I-DEAS™ Interface

Description This option allows you to generate a Universal file which is compatible with the SDRC I-DEAS program. Two types of quantities can be on this file: element and nodal quantities. The element quantities (stresses, strains, etc.) written into the Universal file are only the component values. Once the Universal file is read into I-DEAS, the invariants are computed internally. They are each an average value within the element. The nodal quantities are values extrapolated from the integration points and a weighted average is calculated. Extreme care should be used interpreting the results with beam and/or shell elements. If the SDRC option is used simultaneously with either or both of the IRM and HYPERMESH options, internally the program treats the data in a cumulative manner. For example, if stresses are requested for the SDRC Universal file and creep strains are requested for the Hypermesh results file, both quantities are output into both files. The SDRC Universal file is named jid.unv. In addition, if the SDRC Universal file is required, the element results can be output as element or nodal variables. To output the element variables, use ELEMENT. To output the nodal variables, use ELEMENT NODE. Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word SDRC.

11-15

2nd

I

Enter the unit number to which to write file; default is 40.

16-20

3rd

I

Frequency to write out file.

If no element data is required, skip to the 4th data block. Enter either the 2a data block or 2b data block. 2a data block 1-10

1st

A

Enter the word ELEMENT.

A

Enter the word ELEMENT NODE.

2a data block 1-10

1st

Repeat 3rd data block as often as required.

Main Index

SDRC 431 SDRC I-DEAS™ Interface

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter: 1 for stresses. 2 for total strains. 3 for creep strains. 4 for thermal strains. 5 for plastic strains. 6 for strain energy. 7 for von Mises equivalent stress divided by the yield stress. 8 for failure indices.

6-10

2nd

I

Enter a layer number if shell elements.

If layer number equals zero, total generalized strain is output. If no nodal data is required, skip to the next model definition point. 4th data block 1-8

1st

A

Enter the word NODAL.

Repeat 5th data block as often as required 5th data block 1-5

1st

I

Enter: 1 for displacements. 2 for velocities. 3 for acceleration. 4 for reaction forces. 5 for temperatures. 6 for generalized stresses. 7 for generalized strains. 8 for top/middle/bottom layer stresses. 9 for top/middle/bottom elastic strains. 10 for top/middle/bottom plastic strains.

Main Index

432 SDRC SDRC I-DEAS™ Interface

Format Fixed

Free

Data Entry Entry 11 for top/middle/bottom creep strains. 13 for eigenmodes. 14 for harmonic displacements and reactions. Note:

Main Index

If shell elements are not included in the model, specifying 8, 9, 10, or 11 results in only the top or actual component.

HYPERMESH 433 HyperMesh Interface

HYPERMESH

HyperMesh Interface

Description This option allows you to generate a results file which is compatible with HyperMesh. Two types of quantities can be on this file: element and nodal quantities. The element quantities (stresses, strains, etc.) written into the results file are both the component values and the invariant values. They are each an average value within the element. The nodal quantities are values extrapolated from the integration points and a weighted average is calculated. Extreme care should be used interpreting the results with beam and/or shell elements. For writing of eigenmodes into the HYPERMESH results file, the Marc data file should contain either the MODAL INCREMENT or the BUCKLE INCREMENT model definition option, as appropriate, together with the DYNAMIC or BUCKLE parameter. Do not use related history definition options MODAL SHAPE, BUCKLE, or RECOVER. If the HYPERMESH option is used simultaneously with either or both of the IRM and SDRC options, internally the program treats the data in a cumulative manner. For example, if stresses are requested for the SDRC Universal file and creep strains are requested for the Hypermesh results file, both quantities are output into both files. The HyperMesh results file is named jid.hmr. Note:

When the Intergraph results file is requested together with the HyperMesh results file, the invariant element quantities are automatically written into the Intergraph results file.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word HYPERMESH.

11-15

2nd

I

Leave blank.

16-20

3rd

I

Frequency to write out file.

If no element data is required, skip to the 4th data block. 2nd data block 1-10

1st

A

Enter the word ELEMENT.

Repeat 3rd data block as often as required. 3rd data block 1-5

1st

I

Enter: 1 for stresses. 2 for total generalized strains. 3 for creep strains.

Main Index

434 HYPERMESH HyperMesh Interface

Format Fixed

Free

Data Entry Entry 4 for thermal strains. 5 for plastic strains. 6 for strain energy. 7 for von Mises equivalent stress divided by the yield stress. 8 for failure indices.

6-10

2nd

I

Enter a layer number if shell elements.

If the value in the first field is a 2, enter 0. If no nodal data is required, skip to the next model definition point. 4th data block 1-8

1st

A

Enter the word NODAL.

Repeat 5th data block as often as required. 5th data block 1-5

1st

I

Enter: 1 for displacements. 2 for velocities. 3 for acceleration. 4 for reaction forces. 5 for temperatures. 6 for generalized stresses. 7 for generalized strains. 8 for top/middle/bottom layer stresses. 9 for top/middle/bottom elastic strains. 10 for top/middle/bottom plastic strains. 11 for top/middle/bottom creep strains. 13 for eigenmodesa. Note:

a

Main Index

If shell elements are not included in the model, specifying 8, 9, 10, or 11 results in only the top or actual component

For writing of eigenmodes into the HYPERMESH results file, the Marc data file should contain either the MODAL INCREMENT or the BUCKLE INCREMENT model definition option, as appropriate, together with the DYNAMIC or BUCKLE parameter. Do not use related history definition options MODAL SHAPE, BUCKLE, or RECOVER.

PRINT CHOICE (Model Definition) 435 Specify Output

PRINT CHOICE (Model Definition)

Specify Output

Description This option allows you the control of the output from Marc. The data given here remains in control until a subsequent PRINT CHOICE set is inserted – such a set can be included with either the model definition or with history definition data set. See also PRINT ELEMENT and PRINT NODE. The default values print all elements and all nodes. Element quantities are printed at each integration point or at the centroid only, depending on whether the CENTROID parameter is used. For shells, only the extreme fibers are output, plus layers where the inelastic strains or state variables are nonzero. For beams, fibers with inelastic strains or nonzero state variables are printed. In addition, section forces are given for these elements. This option also allows debug output of certain items. The default is no debug printout. All of the above defaults are reset by the PRINT CHOICE option. The PRINT CHOICE option has no effect on the post processor file. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words PRINT CHOICE.

2nd data block 1-5

1st

I

Number of sets of first and last element numbers to be printed (maximum 10).

6-10

2nd

I

Number of sets of first and last node numbers to be printed (maximum 10).

11-15

3rd

I

Number of integration points to be printed in each element (not used if CENTROID is flagged).

16-20

4th

I

Number of layers to be printed. This is for beams and shells only and overrides the default described above.

21-25

5th

I

Increments between printout. Default is print every increment.

26-30

6th

I

Enter 1 for complex nodal quantities to be output as magnitude and phase, otherwise real and imaginary components are given.

31-35

7th

I

Debug print flag. Enter a nonzero value and use data block 7.

36-40

8th

I

Log file flag. Enter unit number to which log file is to be written.

3rd data block Include only if the first field of 2nd data block is not zero.

Main Index

436 PRINT CHOICE (Model Definition) Specify Output

Format Fixed

Free

Data Entry Entry

1-5

1st

I

First element in first set.

6-10

2nd

I

Last element in first set.

11-15

3rd

I

First element in second set.

16-20

4th

I

Last element in second set.

Etc.

5th

Etc. in I5 format.

4th data block Include only if the second field of 2nd data block is not zero. 1-5

1st

I

First node in first set.

6-10

2nd

I

Last node in first set.

11-15

3rd

I

First node in second set.

16-20

4th

I

Last node in second set.

Etc.

5th

Etc. in I5 format.

5th data block Include only if the third field of 2nd data block is not zero. I

Enter the list of integration points to be printed in (16I5) format (number of entries given in third field of data block 2). This is only used if CENTROID is not flagged. Be careful with analyses with several different element types.

6th data block Include only if the fourth field of 2nd data block is not zero. I

Enter the list of shell or beam fibers to be printed in (16I5) format. This overrides Marc default, so you should be careful to not unintentionally suppress plasticity or creep printout.

7th data block Include only if the seventh field of 2nd data block is not zero 1-5

Main Index

1st

16I5

Enter debug print flags. See the PRINT parameter.

PRINT ELEMENT (Model Definition) 437 Specify Elements to be Included in Output

PRINT ELEMENT (Model Definition) Specify Elements to be Included in Output Description This option allows you to choose which elements, and what quantities associated with an element are to be printed. If you do not specify NODE on the first data line, these values are at the integration points. This option can be used to print response quantities for the first 28 integration points of any element. This suffices for all elements, except continuum composite elements (types 149 - 154, 175 - 180) which can have as many as 2040 integration points. For print-outs at integration point numbers greater than 28 for continuum composite elements, use PRINT CHOICE. If you specify the word NODE, these values are the extrapolated nodal values. This extrapolation is currently not available for rebar elements, composite continuum elements, semi-infinite elements, or cavity elements. Note:

This option revokes any NO PRINT that precedes it. Therefore, NO PRINT followed by PRINT ELEMENT and not followed by PRINT NODE results in the selected element printout and full nodal printout. Use PRINT NODE with a blank node list to suppress node output.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PRINT ELEMENT.

11-20

2nd

A

Enter the word NODE (optional).

2nd data block 1-5

1st

I

Enter the number of sets to be given below (optional).

6-10

2nd

I

Increment between printout. Default is print every increment.

11-15

3rd

I

File unit to which output is to be written. Defaults to standard output, unit 6.

Data blocks 3, 4, and, if necessary, 5 and 6 are given once for each data set. 3rd data block 1-80

1st

A

Enter one or more of the following: STRAIN

output total strain.

STRESS

output total stress.

PLASTIC

output plastic strain.

CREEP

output creep, swelling and viscoelastic strain.

THERMAL output thermal strain

Main Index

438 PRINT ELEMENT (Model Definition) Specify Elements to be Included in Output

Format Fixed

Free

Data Entry Entry CREEP

output creep, swelling and viscoelastic strain.

THERMAL

output thermal strain

ENERGY

output of strain energy densities: • total strain energy • incremental total strain energy • total elastic strain energy • incremental elastic strain energy • plastic strain energy • incremental plastic strain energy

CRACK

output of cracking strain.

CAUCHY

output Cauchy stress.

STATE

output state variables.

PREFER

output stresses in preferred system.

ELECTRIC

output electric field and electric flux.

MAGNETIC output magnetic field and magnetic flux. CURRENT

output current.

ALL

output of all of the above.

4th data block Enter a list of elements to be printed. Note:

To suppress all element print-out, enter a blank list for the list of elements.

5th data block If the NODE option is not specified on the 1st data block, enter a list of integration points to be printed. If the NODE option is specified on the 1 data block, enter a list of node positions based upon the CONNECTIVITY option. These node positions range from one to the maximum number of nodes per element.

Main Index

PRINT ELEMENT (Model Definition) 439 Specify Elements to be Included in Output

Format Fixed

Free

Data Entry Entry

6th data block Enter a list of layers to be printed. This is only necessary if there are either thin walled beam, shell, rebar, solid composite elements in the mesh, (that is, element types 1, 4, 5, 8, 13, 14, 15, 16, 17, 22, 23, 24, 25, 45,46, 47, 48, 49, 50, 72, 75, 76, 77, 78, 79, 85, 86, 87, 88, 89, 90, 98, 138, 139, 140, 142, 143, 144, 145, 146, 147, 148, 149, 150, 151, 152, 153, 154, 165, 166, 167, 168, 169, 170, 175, 176, 177, 178, 179, 180). It is also necessary to include this data block if there are beam element types 52 or 98 and they are used with integrated solid cross sections.

Main Index

440 PRINT NODE (Model Definition) Specify Nodes to be Included in Output

PRINT NODE (Model Definition)

Specify Nodes to be Included in Output

Description This option allows you to choose which nodes and what nodal quantities are to be printed. Note:

This option revokes any NO PRINT that precedes it. Therefore, NO PRINT followed by PRINT NODE and not followed by PRINT ELEMENT results in the selected nodal output and full element output. Use PRINT ELEMENT with a blank element list to suppress element printout.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PRINT NODE.

2nd data block 1-5

1st

I

Enter the number of sets to be given below (optional).

6-10

2nd

I

Increment between printout. Default is print every increment.

11-15

3rd

I

File unit to which output is to be written, default to standard output, unit 6.

Data blocks 3 and 4 are entered as pairs, one for each data set. 3rd data block 1-80

1st

A

Enter one or more of the following: INCR

output incremental displacement or potentials

TOTA

output total displacement or potentials

VELO

output velocity

ACCE

output acceleration

LOAD

output total applied load

REAC

output reaction/residual force

TEMP

output temperature

FLUX

output flux Note:

MODE

Fluxes are only available if the parameter HEAT, 0, 0, 2 is used.

output eigenvector (modal or buckle)

STRESS output average generalized stresses at nodes

Main Index

PRINT NODE (Model Definition) 441 Specify Nodes to be Included in Output

Format Fixed

Free

Data Entry Entry VOLT

output voltage (Joule analysis)

PRES

output pressure (bearing analysis)

COOR

output coordinates (for rezoning)

INER

output inertia relief load (for interia relief analysis)

ALL

output all relevant quantities

4th data block Enter a list of nodes to be printed. Note:

Main Index

To suppress all nodal printout, enter a blank list for the list of nodes. The average nodal generalized stresses are obtained via an extrapolation and averaging procedure. If there is a geometric or material discontinuity at a node, this value is not correct unless either double nodes are used with kinematic tying, or you control which elements are to be averaged using the PRINT ELEMENT feature.

442 NO PRINT (Model Definition) Suppress Elements and Nodes in Output

NO PRINT (Model Definition)

Suppress Elements and Nodes in Output

Description This option suppresses element and nodal output. Note:

This option is revoked by using either the PRINT CHOICE, PRINT ELEMENT, or PRINT NODE options. Therefore, NO PRINT followed by a PRINT ELEMENT, for example, results in element and full nodal printout. Use PRINT NODE or PRINT ELEMENT with blank node or element lists to suppress all node or element output.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO PRINT.

PRINT SPRING (Model Definition) 443 Controls the Print Out of Springs

PRINT SPRING (Model Definition) Description This option controls the output for selected springs. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PRINT SPRING.

2nd data block Enter a list of springs to be printed

Main Index

Controls the Print Out of Springs

444 NO PRINT SPRING (Model Definition) Deactivates the Printing of All Springs

NO PRINT SPRING (Model Definition)

Deactivates the Printing of All Springs

Description This options supresses the output of spring results. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word NO PRINT SPRING.

PRINT CONTACT (Model Definition) 445 Prints the Contact Body Summary

PRINT CONTACT (Model Definition)

Prints the Contact Body Summary

Description This option ensures that the summary of contact information for each body is printed to the output file even if the NO PRINT option is activated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words PRINT CONTACT.

446 NO PRINT CONTACT (Model Definition) Suppresses the Contact Body Summary Printout

NO PRINT CONTACT (Model Definition)

Suppresses the Contact Body Summary Printout

Description This option deactivates the output of the summary of contact information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO PRINT CONTACT.

GRID FORCE (Model Definition) 447 Nodal Force Output at Element or Node Level

GRID FORCE (Model Definition) Nodal Force Output at Element or Node Level Description This option allows the user to output the contributions to the nodal force at either an element level or a nodal level. This is useful when constructing a free body diagram of part of the structure. The Marc for grid force balance is with respect to the global coordinate system. In Marc, the following contributions are considered: On an element level, the grid force balance is based upon the Internal forces Distributed Loads Foundation Forces Reaction Force On a nodal basis, it is much more complete and includes Internal Forces

Distributed + Point Forces

Foundation Forces

Spring Forces

Contact Normal Forces

Contact Friction Forces

Tying/MPC Forces

Inertia Forces

Damping Forces

DMIG Forces

Reaction Force Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word GRID FORCE.

2nd data block 1-5

1st

I

Frequency (increments) between writing out the grid forces.

6-10

2nd

I

Enter 1 if force output is based upon elements.

11-15

3rd

I

Enter 1 if force output is based upon nodes.

16-20

4th

I

Enter 0 if grid force output is to be written to standard output (default). Enter 1 if grid force output is to be written to file jid.grd.

21-25

Main Index

5th

I

Enter the number of times that grid force should be output in a load case; if 1 is entered, the output will occur at the last increment of the load case.

448 GRID FORCE (Model Definition) Nodal Force Output at Element or Node Level

Format Fixed

Free

Data Entry Entry

3rd and 4th data block are optional (may be repeated multiple number of times) 3rd data block 1-10

1st

A

Enter the words SELECT ELEMENT.

4th data block 1-80

Enter a list of elements for which grid force output will be done

5th and 6th data block are optional (may be repeated multiple number of times) 5th data block 1-10

1st

A

Enter the words SELECT BODY.

6th data block 1-80

Enter a list of contact bodies; grid force on an element level will be given for elements in these bodies.

7th and 8th data block are optional (may be repeated multiple number of times) 7th data block 1-10

1st

A

Enter the words SELECT NODE.

8th data block 1-80

Main Index

Enter a list of nodes for which forces will be output on a nodal basis.

PRINT VMASS (Model Definition) 449 Print Element Volumes, Masses, Costs, and Strain Energies

PRINT VMASS (Model Print Element Volumes, Masses, Costs, and Strain Energies Definition) Description This option allows you to obtain printed output of element volumes, masses, costs and strain energies. Options are provided for you to print the total quantities for each group of elements and the quantities for each element in the group or the total quantities for each group of elements only. In order to have correct mass computations, mass density for each element must be entered through one of the material options. In order to have the correct cost, the cost per unit mass or the cost per unit volume must be defined through the ISOTROPIC/ORTHOTROPIC option. The total strain energy and the plastic strain energy, if applicable, are printed. Note that volumes and masses for some special elements (for example, gap element, semi-infinite element, etc.) is not be computed. These quantities can be written on either standard output file unit 6, or your specified unit. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words PRINT VMASS.

2nd data block 1-5

1st

I

Enter the number of sets to be given below.

6-10

2nd

I

Enter 1 for option to print only total volumes, masses, costs, and strain energy for groups of elements. Default is 0.

11-15

3rd

I

File unit to which output is to be written; default to standard output, unit 6.

Either data block 3a or 3b may be used 3a data block Enter a list of elements to be printed. 3b data block Enter the negative of deformable body number (only one body number per data block).

Main Index

450 REAUTO Interrupt/Modify Load Sequence from Previous Analysis

REAUTO

Interrupt/Modify Load Sequence from Previous Analysis

Description Used for changing conditions on restart of a problem in an autoloading sequence, dynamics, creep, or heat transfer. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word REAUTO. This entry allows a reset of various parameters during restart. It can be used to override previously set values in the middle of automatic load incrementation. These values are originally set in the AUTO CREEP, AUTO INCREMENT, AUTO LOAD, AUTO STEP, DYNAMIC CHANGE, or TRANSIENT. Only the nonzero values set here are used. For AUTO LOAD, only the 3rd, 4th, and 5th fields are used; set other fields to 0.

2nd data block 1-10

1st

F

Time step size. The value should only be set in dynamic problems.

11-20

2nd

F

End value of time for this set of boundary conditions.

21-25

3rd

I

Total number of time steps in this set of boundary conditions or, for AUTO LOAD, number of equal load increments. To immediately complete previous set of load history data, set to 1.

26-30

4th

I

Not used, enter 0.

31-35

5th

I

Reassembly interval for mass and stiffness matrices; for linear problems, set equal to the value given in the third field.

36-40

6th

I

Desired number of recycles for the AUTO INCREMENT option.

41-50

7th

F

Maximum step size in AUTO INCREMENT option.

51-60

8th

F

Current percentage of total load to be applied (AUTO TIME or AUTO INCREMENT).

61-65

9th

I

Enter 1 to force remeshing immediately after restart. The meshing parameters based upon the ADAPT GLOBAL option, before the END OPTION, are used. Enter 2 to force remeshing immediately after restart and user will provide mesh file in jid_b*.mesh file in the format of a .t18 file. Enter 3 to force remeshing immediately after restart and user will provide mesh file in jid_b*.mesh file in the format of a .feb file.

Main Index

REAUTO 451 Interrupt/Modify Load Sequence from Previous Analysis

Format Fixed

Free

Data Entry Entry Enter 4 to force remeshing immediately after restart and user will provide the mesh file in jid_b*.mesh in the format of a standard Marc data file.

66-70

Notes:

10th

I

Enter 1 to force recalculation of radiation viewfactors immediately after restart.

“*” is the remeshing body number. When using REAUTO to read mesh files, you need to prepare mesh files for all defined remeshing bodies. Use ADAPT GLOBAL to read mesh files immediately after the restart. With this option, you can select the remeshing body.

Main Index

452 RESTART Set Flags for Restart

RESTART

Set Flags for Restart

Description This option sets up the flags for the restart files; both for the input of a previous restart file and for output of a restart file from the current analysis. When the ELASTIC parameter is included, always restart at increment 0. The following points should be noted concerning the RESTART option. • A restart write frequency must be specified when a restart file is to be output. The analysis can

then be restarted from any increment at which restart has been written. • The restart file contains only those increments written during the current part of the analysis. The

restart file is not continuous because of the large volume of data that can be involved. If it were written on the same file, the input/output time would be increased and also you might overflow the file storage in large problems. • At restart, the data governing the increments (or increment set) next to be analyzed must follow the END OPTION as incremental input data. Any file input, such as a file of temperature

increments describing a thermal history, must be skipped forward by you to the appropriate point; that is, to the beginning of the increment of the new part of the analysis. • During any option set for a series of increments (AUTO CREEP, DYNAMIC CHANGE, AUTO INCREMENT, AUTO LOAD, AUTO STEP, AUTO THERM CREEP, TRANSIENT), restart can be

effected and control parameters changed. Marc then continues to the end of the part of the analysis specified by the option. You have the option to terminate such a part of the analysis prematurely through the use of restart with the REAUTO option. • The RESTART INCREMENT history definition option can be used to modify parameters defined

in this option, or terminate the writing of a restart file. • The RESTART LAST option can be used to save only the last converged increment or to

periodically write restart data to individual files. • The old restart file is closed after it has been read.

The input data describing the problem is not saved, and therefore must be read in with each restart. This option specifies restart parameters; for example, input/output files, restart increment, and intervals at which restarts are to be written. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

Main Index

1st

A

Enter the word RESTART.

RESTART 453 Set Flags for Restart

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Set to 1 to write out restart data on a file. Set to 2 to read restart data from a file (that is, to restart a problem). Set to 3 to restart a problem and continue writing restart data for subsequent restart.

6-10

2nd

I

Number of increments between writing of restart data. For example, to write every three increments, set the second field to 3. This data is only used if the first field is set to 1 or 3. Defaults to 1 if left blank.

11-15

3rd

I

Enter the increment at which the restarted problem run begins. Only used if the first field of this data block is set to 2 or 3. The number here should be the number given in the message: RESTART DATA AT INCREMENT i on TAPE j

which appears on the output of the previous run of the problem at the point where the restart is desired. Note:

The problem can only be restarted at such points. The frequency of such points is determined by the data in columns 6 through 10 of this data block in the previous run of the problem. A restarted run should, in principle, have the same parameters as the original run. Only those parameters can be changed which do not affect the storage allocation within Marc.

Main Index

16-20

4th

I

Logical unit number for output of restart data; default logical unit number is 8 if nothing is given here and the RESTART option is specified in the parameters. Note that this file must be specified in the main program.

21-25

5th

I

Logical unit number for input of restart data from previous run; default is 9 if nothing is given here. Specify file in main program.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Not used; enter 0.

41-45

9th

I

Not used; enter 0.

46-50

10th

I

Set to 1 to print out increment specified in the third field through increment specified in the eleventh field. The job does not do any analysis. This is to, for example, allow you to recover increments suppressed by PRINT CHOICE.

454 RESTART Set Flags for Restart

Format

Main Index

Data Entry Entry

Fixed

Free

51-55

11th

I

Set to last increment on restart file to be read. This is used in conjunction with the tenth field above or the eighth field of the POST option.

56-60

12th

I

Enter the subincrement at which the restart problem begins. Defaults to zero. This can be used to postprocess either eigenvectors or harmonics.

61-65-

13th

I

Enter the last subincrement to be read. This is used in conjunction with the tenth field above or the eighth field of the POST option.

RESTART LAST 455 Use Condensed Restart File

RESTART LAST

Use Condensed Restart File

Description This option sets up the flags for a condensed restart file where only the last converged increment or some specific increment is saved. It can also be used to write a restart file on separate files at a specified frequency. Notes: Upon writing, the last converged increment is written to the restart file. Upon reading, this increment is subsequently read in and the analysis continues. The restart file is closed after it has been read. The REAUTO option can be used to terminate any multi-increment history definition block. The restart file name to store data at the last increment or at the end of analysis is jid.t08 by default. This file is overwritten when it is used. The file name to store data at specific increment or increment intervals or at the end of each loadcase is jid.i_n.to8, n being the increment number. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the word RESTART LAST.

I

Set to 1 to write out last increment of restart data on a file.

2nd data block 1-5

1st

Enter -1 to write out the last increment at the end of each loadcase and at the end of the analysis. Set to 2 to read restart data from a file (that is, to restart a problem). Set to 3 to restart a problem and write out the last increment of restart data for subsequent restart. Enter -3 to restart a problem and write out the last increment at the end of each loadcase and at the end of the analysis. 6-10

Main Index

2nd

I

Logical unit number for output of restart data; default unit number is 8 if nothing is given here.

456 RESTART LAST Use Condensed Restart File

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

16-20

4th

I

Logical unit number for input of restart data from previous run; default is 9 if nothing is given here. Enter frequency to write restart to individual files. The files will be named jid_i_nn.t08 (where nn is the current increment).

If the number here is less than zero, its positive number is the specific increment to write out the restart file. This option works when the first field is set to -1 or -3.

Main Index

UDUMP 457 Specify Nodes and Element for Postprocessing

UDUMP

Specify Nodes and Element for Postprocessing

Description This option allows you to specify which nodes and elements can be referenced for postprocessing through user subroutines. Nodal quantities are accessed through subroutine IMPD, element quantities are accessed through the ELEVAR user subroutine (see Marc Volume D: User Subroutines and Special Routines). During harmonic subincrements, the ELEVEC user subroutine is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word UDUMP.

2nd data block

Main Index

1-5

1st

I

First element, defaults to 1.

6-10

2nd

I

Last element, defaults to last element in mesh.

11-15

3rd

I

First node, defaults to 1.

16-20

4th

I

Last node, defaults to last node in mesh.

458 SUMMARY (Model Definition) Create Summary Report

SUMMARY (Model Definition)

Create Summary Report

Description This option produces a summary of the results of the increment and outputs them in a report format. This option is in effect until a NO SUMMARY option is encountered. The summary consists of the maximum and minimum of temperatures, stresses, strains, plastic strains, creep strains, displacements, velocities, accelerations and reaction forces. The option also produces a detailed accounting of both the memory usage and timing information. Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-10

1st

A

Enter the word SUMMARY.

11-15

2nd

I

Enter the unit number to be used for output, default is standard output, unit 6.

16-20

3rd

I

Enter the increment frequency of summary, default is every increment.

NO SUMMARY (Model Definition) 459 Do Not Create Summary

NO SUMMARY (Model Definition)

Do Not Create Summary

Description This option turns off the summary feature. The default is off unless the SUMMARY option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO SUMMARY.

460 ELEMENT SORT (Model Definition) Sort Element Results

ELEMENT SORT (Model Definition)

Sort Element Results

Description This option allows various element quantities to be sorted and the output given in report format. This option is in effect until a NO ELEM SORT option is encountered. This option allows you to sort either in ascending or descending order. In addition, you can use either the real numeric value or the absolute value. A range can be given over which to sort. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ELEM SORT.

2nd data block 1-5

1st

I

Enter number of sorts to be performed (optional). One data block, as given below, defines each sort.

6-10

2nd

I

Enter unit number to read sort data.

11-15

3rd

I

Enter the unit number to be used for output, default is standard output, unit 6.

16-20

4th

I

Enter the increment frequency, default is every increment.

3rd data block The 3rd data block is repeated once for each sort. 1-5

1st

I

Enter code indicating type of quantity to be sorted (see Table 3-6).

6-10

2nd

I

Enter 0 for sort in descending order. Enter 1 for sort in ascending order. Default is 0; sort in descending order.

11-15

3rd

I

Enter 1 for sort by real numerical value. Enter 0 for sort by absolute value. Default is 0; sort by absolute value.

Main Index

16-20

4th

I

Enter number of items to be included in sorted list.

21-25

5th

I

Enter lowest element number of range to be sorted. Defaults to 1.

26-30

6th

I

Enter highest element number of range to be sorted. Defaults to last element in mesh.

ELEMENT SORT (Model Definition) 461 Sort Element Results

Table 3-6

Element Sort Codes

Code

Description

Description

1 first stress

28 fourth plastic strain

2 second stress

29 fifth plastic strain

3 third stress

30 sixth plastic strain

4 fourth stress

31 equivalent plastic strain

5 fifth stress

32 mean plastic strain

6 sixth stress

33 Tresca plastic strain

7 equivalent stress

34 first principal plastic strain

8 mean stress

35 second principal plastic strain

9 Tresca stress

36 third principal plastic strain

10 first principal stress

37 first creep strain

11 second principal stress

38 second creep strain

12 third principal stress

39 third creep strain

13 first strain

40 fourth creep strain

14 second strain

41 fifth creep strain

15 third strain

42 sixth creep strain

16 fourth strain

43 equivalent creep strain

17 fifth strain

44 mean creep strain

18 sixth strain

45 Tresca creep strain

19 equivalent strain

46 first principal creep strain

20 mean strain

47 second principal creep strain

21 Tresca strain

48 third principal creep strain

22 first principal strain

49 temperature

23 second principal strain

61 voltage

24 third principal strain

73 first gradient

25 first plastic strain

74 second gradient

26 second plastic strain

75 third gradient

27 third plastic strain

Main Index

Code

462 NO ELEM SORT (Model Definition) Do Not Create Report Sorted by Element

NO ELEM SORT (Model Definition)

Do Not Create Report Sorted by Element

Description This option turns off the ELEM SORT feature. The default is off unless the ELEM SORT option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO ELEM SORT.

NODE SORT (Model Definition) 463 Sort Nodal Results

NODE SORT (Model Definition)

Sort Nodal Results

Description This option allows various nodal quantities to be sorted and the output given in report format. This option is in effect until a NO NODE SORT is encountered. NODE SORT allows you to sort either in ascending or descending order. In addition, you can use either the real numeric value or the absolute value. A range can be given over which to sort. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE SORT.

2nd data block 1-5

1st

I

Enter number of sorts to be performed (optional). One data block as given below defines each sort.

6-10

2nd

I

Enter unit number to read sort data.

11-15

3rd

I

Enter the unit number to be used for output, default is standard output, unit 6.

16-20

4th

I

Enter the increment frequency, default is every increment.

3rd data block The 3rd data block is entered once for each sort.

Main Index

1-5

1st

I

Enter code indicating type of quantity to be sorted (see Table 3-7).

6-10

2nd

I

Enter 0 for sort in descending order. Enter 1 for sort in ascending order. Default is 0, sort in descending value.

11-15

3rd

I

Enter 1 for sort by real numerical value. Enter 0 for sort by absolute value. Default is 0, sort by absolute value.

16-20

4th

I

Enter number of items to be included in sorted list.

21-25

5th

I

Enter lowest node number of range to be sorted. Defaults to 1.

26-30

6th

I

Enter highest node number of range to be sorted. Defaults to last node in mesh.

464 NODE SORT (Model Definition) Sort Nodal Results

Table 3-7 Code

Node Sort Codes Meaning

1-12 sort code I

Main Index

Result Results in the Ith component of the incremental displacement to be sorted.

13-34 sort code I +12

Results in the Ith component of the total displacement to be sorted.

25-36 sort code I + 24

Results in the Ith component of the velocity to be sorted.

37-48 sort code I + 36

Results in the Ith component of the acceleration to be sorted.

48-60 sort code I + 48

Results in the nodal temperature to be sorted.

61-72 sort code I + 60

Results in the Ith component of the reaction force to be sorted.

71-84 sort code I + 72

Results in the Ith component of the contact force to be sorted.

101 101

Sort on magnitude of incremental displacement.

102 102

Sort on magnitude of total displacement.

103 103

Sort on magnitude of velocity.

104 104

Sort on magnitude of acceleration.

105 105

Sort on magnitude of temperature.

106 106

Sort on magnitude of reaction force.

107 107

Sort on magnitude of contact force.

NO NODE SORT (Model Definition) 465 Cancel Report Sorted by Nodes

NO NODE SORT (Model Definition)

Cancel Report Sorted by Nodes

Description This option negates the NODE SORT option. The default is off unless the NODE SORT option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO NODE SORT.

466 DESIGN OBJECTIVE Define Objective Function to be Optimized

DESIGN OBJECTIVE

Define Objective Function to be Optimized

Description This option defines the objective function for the optimization process. It is not needed for a pure sensitivity analysis run. If it is specified for a pure sensitivity analysis run, the gradient of the objective function is also computed. Currently, the only option is to “minimize” the objective function. Format Format Fixed

Free

Data Entry Entry

1st data block 1-16

1st

A

Enter the words DESIGN OBJECTIVE.

A

Enter one of the following:

2nd data block N/A

1st

MATERIAL VOLUME MATERIAL MASS MATERIAL COST USER DEFINED Note:

For MATERIAL MASS, the mass density, and for MATERIAL COST, the material unit cost should be defined with the material data (for example, see ISOTROPIC) For USER DEFINED, you need to modify the user subroutine uobjfn.f. This routine is self-explanatory together with an example.

Main Index

DESIGN VARIABLES 467 Define Variable Design Parameters

DESIGN VARIABLES

Define Variable Design Parameters

Description This option defines the design variables. If a sensitivity analysis is required, the derivative of the response with respect to each design variable and the element contributions to the response are reported. If an optimization analysis is performed, then the design variables are modified to optimize the objective function. The option can be used more than once. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words DESIGN VARIABLES.

Data blocks 2 through 5 are repeated for each design variable. 2nd data block N/A

1st

I

Enter design variable set ID (optional). In general, this is not the same as design variable numbers assigned by Marc and defined in the output.

N/A

2nd

A

Enter, as appropriate, one of the words GEOMETRY, MATERIAL, or COMPOSITE.

N/A

3rd

A

For GEOMETRY, enter one of the following: CTHIC

– constant thickness over element

AREA

– cross-sectional area

IXX

– moment of inertia Ixx

IYY

– moment of inertia Iyy

BMHEI

– beam height

BMWID – beam width RADIU

– radius

WLLTH

– wall thickness

For MATERIAL, enter one of the following: YNGMD – Young’s modulus (isotropy)

Main Index

YNG11

– Young’s modulus E11

YNG22

– Young’s modulus E22

YNG33

– Young’s modulus E33

468 DESIGN VARIABLES Define Variable Design Parameters

Format Fixed

Free

Data Entry Entry POISR

– Poisson’s ratio (isotropy)

PSR12

– Poisson’s ratio ν12

PSR23

– Poisson’s ratio ν23

PSR31

– Poisson’s ratio ν31

SHR12

– Shear modulus G12

SHR23

– Shear modulus G23

SHR31

– Shear modulue G31

MASSD

– Mass density

For COMPOSITE, enter one of the following:

N/A

4th

LYRTH

– layer thickness (the “layer thickness option needs to be selected in the 3rd field of the 3rd data block under the COMPOSITE model definition option.)

PLYAN

– ply angle

I

Enter related composite group number if applicable.

3rd data block N/A

1st

E

Enter lower bound for value of variable.

N/A

2nd

E

Enter upper bound for value of variable.

A

Enter one of the following:

4th data block N/A

1st

LINKED or UNLINKED. N/A

2nd

A

Enter one of the following: ELEMENTS, MATERIALS, or LAYERS, depending on the second field in the 2nd data block.

5th data block N/A

Enter a list of elements if the second field of the 4th data block is ELEMENTS. Enter a list of material IDs if second field of the 4th data block is MATERIALS. Enter a list of layer numbers if second field of the 4th data block is LAYERS.

Main Index

DESIGN DISPLACEMENT CONSTRAINTS 469 Define Limits on Displacement Response

DESIGN DISPLACEMENT CONSTRAINTS

Define Limits on Displacement Response

Description This option is used to specify displacement constraints for a design sensitivity/design optimization process. The option can be used more than once. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words DESIGN DISPLACEMENT.

Data blocks 2 through 7 are repeated for each displacement constraint group. 2nd data block N/A

1st

A

Enter one of the words (preceded by the word ABSOLUTE where needed; for example, ABSOLUTE TRANSL1):

Main Index

TRANSL1 –

translation parallel to first axis

TRANSL2 –

translation parallel to second axis

TRANSL3 –

translation parallel to third axis

ROTATN1 –

rotation about first axis

ROTATN2 –

rotation about second axis

ROTATN3 –

rotation about third axis

RESTRAN –

resultant translation

RESROTA –

resultant rotation

DIRTRAN –

translation along a vector

DIRROTA –

rotation about a vector

DIRLTRA

–

relative translation along a vector

DIRLROT

–

relative rotation about a vector

RLTRAN1 –

relative translation 1 (first axis)

RLTRAN2 –

relative translation 2 (second axis)

RLTRAN3 –

relative translation 3 (third axis)

RLROTA1 –

relative rotation 1 (first axis)

RLROTA2 –

relative rotation 2 (second axis)

RLROTA3 –

relative rotation 3 (third axis)

470 DESIGN DISPLACEMENT CONSTRAINTS Define Limits on Displacement Response

Format Fixed N/A

Free 2nd

Data Entry Entry A

Enter either: < (for less than or equal to) or > (for greater than or equal to)

N/A

3rd

E

Enter the bound with the correct sign

The 3rd data block is only used if the 1st field of the 2nd data block is DIRTRAN, DIRROTA, DIRLTRA, DIRLROT; otherwise, it is skipped. 3rd data block N/A

1st

E

Enter first component of vector.

N/A

2nd

E

Enter second component of vector.

N/A

3rd

E

Enter third component of vector. Note:

Marc extracts the direction cosines.

4th data block N/A

1st

A

Enter the words LOAD CASES.

I

Enter a list of load cases for which this constraint is prescribed.

A

Enter the word NODES.

5th data block N/A 6th data block N/A

1st

7th data block N/A

If first field of 2nd data block does not begin with RL, enter the list of constrained nodes. If first field of 2nd data block begins with RL, enter the first and second node numbers which are constrained relative to one another.

Main Index

DESIGN STRESS CONSTRAINTS 471 Define Limits on Stress Response

DESIGN STRESS CONSTRAINTS

Define Limits on Stress Response

Description This option is used to specify stress constraints for a design sensitivity/design optimization process. The option can be used more than once. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words DESIGN STRESS.

Data blocks 2 through 7 are repeated for each stress constraint group. 2nd data block N/A

1st

I

Enter one of the words (preceded by the word ABSOLUTE where needed; for example, ABSOLUTE STRESS1): STRESS1 STRESS2 The stress components as defined for each element separately in Marc Volume B: Element Library (see below for “generalized stresses”).

STRESS3 STRESS4 STRESS5 STRESS6

Main Index

VOMSTRS –

von Mises equivalent stress

OSHSTRS –

octahedral shear stress

MAPSTRS –

maximum absolute principal stress

PRSTRS1

–

algebraically highest (first) principal stress

PRSTRS2

–

second principal stress

PRSTRS3

–

third principal stress

TRESTRS

–

Tresca equivalent stress

STRESSV

–

normal stress along a vector

SHSTRSP

–

maximum shear stress on a plane

472 DESIGN STRESS CONSTRAINTS Define Limits on Stress Response

Format Fixed

Free

Data Entry Entry GENSTS1 GENSTS9

N/A

2nd

A

generalized stresses 1 through 9 obtained by integration through thickness of layered elements as defined in Marc Volume B: Element Library.

Enter either: < (for less than or equal to) or > (for greater than or equal to)

N/A

3rd

E

Enter the bound with the correct sign.

The 3rd data block is only used if the 1st field of the 2nd data block is STRESSV or SHSTRSP; otherwise, it is skipped. 3rd data block N/A

1st

E

Enter first component of vector.

N/A

2nd

E

Enter second component of vector.

N/A

3rd

E

Enter third component of vector. Note:

Marc extracts the direction cosines.

4th data block N/A

1str

A

Enter the words LOAD CASES.

5th data block N/A

Enter a list of load cases for which this constraint is prescribed.

6th data block N/A

1st

A

Enter the word ELEMENTS.

7th data block N/A

Main Index

Enter the list of constrained elements.

DESIGN STRAIN CONSTRAINTS 473 Define Limits on Strain Response

DESIGN STRAIN CONSTRAINTS

Define Limits on Strain Response

Description This option is used to specify strain constraints for a design sensitivity/design optimization analysis. The option can be used more than once. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words DESIGN STRAIN.

Data blocks 2 through 6 are repeated for each constraint group. 2nd data block N/A

1st

I

Enter one of the words (preceded by the word ABSOLUTE if needed; for example, ABSOLUTE STRAIN1): STRAIN1 STRAIN2 STRAIN3 STRAIN4

The strain components as defined for each element separately in Marc Volume B: Element Library.

STRAIN5 STRAIN6 VOMSTRN – von Mises equivalent strain MAPSTRN – maximum absolute principal strain

N/A

2nd

A

PRSTRN1

– algebraically highest (first) principal strain

PRSTRN2

– second principal strain

PRSTRN3

– third principal strain

TRESTRN

– Tresca equivalent strain

Enter: < (for less than or equal to) or > (for greater than or equal to)

N/A

3rd

E

Enter the bound with the correct sign.

A

Enter the words LOAD CASES.

3rd data block N/A

Main Index

1st

474 DESIGN STRAIN CONSTRAINTS Define Limits on Strain Response

Format Fixed

Free

Data Entry Entry

4th data block N/A

Enter a list of load cases for which this constraint is prescribed.

5th data block N/A

1st

A

Enter the word ELEMENTS.

6th data block N/A

Main Index

Enter the list of constrained elements.

DESIGN FREQUENCY CONSTRAINTS 475 Define Limits on Eigenfrequency Response

DESIGN FREQUENCY CONSTRAINTS

Define Limits on Eigenfrequency Response

Description This option is used to specify free vibration frequency constraints for a design sensitivity or design optimization case. The option can be used more than once. Format Format Fixed

Free

Data Entry Entry

1st data block 1-16

1st

A

Enter the words DESIGN FREQUENCY.

Data blocks 2 though 4 are repeated for each constraint group. 2nd data block N/A

N/A

1st

2nd

A

A

Enter one of the following words: FRQCYCL –

frequency in cycles per unit time

FRQRADS –

frequency in radians per unit time

FGPCYCL –

difference or gap in frequency between any two modes to be prescribed; in cycles per unit time

FGPRADS –

difference or gap in frequency between any two modes to be prescribed; in radians per unit time

Enter either: < (for less than or equal to) or > (for greater than or equal to)

N/A

3rd

E

Enter the bound. This is always positive.

A

Enter the word FREQUENCIES.

3rd data block N/A

1st

4th data block N/A

1st

If the constraint is on the frequencies of modes, enter a list of constrained mode numbers. If the constraint is on the difference between the frequencies of two modes, enter the numbers of the two modes.

Main Index

476 DESIGN FREQUENCY CONSTRAINTS Define Limits on Eigenfrequency Response

Main Index

Chapter 3: Model Definition Options 477 Mechanical Analysis

Chapt Mechanical Analysis er 3: This section is the first of four sections describing the input format for mechanical analysis. This section analysis controls and boundary conditions. The three subsequent sections concentrate on Mode describes material properties, rate effects, and dynamic analysis. l The CONTROL option is required in all nonlinear analysis. It governs the number of increments and the Defini accuracy associated with the analysis. This section also discusses the procedures for J-integral calculation in fracture mechanics. tion The boundary conditions available for performing mechanical analysis are: Optio • Kinematic constraints of either zero or specified displacements. ns • Surface, volumetric or nodal loads. • Thermal loads. • Foundation support. • Surface contact.

These boundary conditions can be specified using a variety of techniques. The boundary conditions when given here in the model definition sections represent the total quantities to be applied in the zeroth increment. Mechanical loads are scaled if the SCALE parameter is included so that the model is at impending yield. Note that thermal loads are not scaled. In addition, as the zeroth increment is treated as linear elastic, the applied boundary conditions should not produce either material or geometry nonlinearities.

Main Index

478 CONTROL (Mechanical - Model Definition) Control Option for Stress Analysis

CONTROL (Mechanical - Model Definition) Control Option for Stress Analysis Description This option allows you to input parameters governing the convergence and the accuracy for nonlinear analysis. For heat transfer analysis, see the CONTROL (Heat Transfer) history definition option in Chapter 4, History Definition Options. For coupled thermal-stress analysis, data block 6 must be used. For coupled electrostatic-stress analysis, data block 7 must be used. For nonlinear static analysis, the controls are described in Marc Volume A: Theory and User Information. They do not appear on the restart file, and so must be re-entered on a restart run. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of load steps/increments in this run. Default is 9999. This is a cumulative number and is usually used to stop the run when restart is being used. If an ELASTIC parameter is included, this field is ignored and all load cases are analyzed.

6-10

2nd

I

Maximum number of recycles/increments during an increment for plasticity, or other tangent modulus nonlinearities. Default is 3. This should usually be increased to 10 for rigid-plastic flow option. If a negative number is entered, Marc does a maximum of the absolute value entered. If convergence has not been obtained, a warning is given and Marc proceeds to the next increment. This is not recommended.

11-15

3rd

I

Minimum number of recycles during an increment for plasticity or other tangent modulus nonlinearities. Default is 0. Note:

This data field forces this number of recycles to take place at all subsequent increments.

Caution: This value is overwritten by the PROPORTIONAL INCREMENT option. 16-20

4th

I

Flag for convergence testing. 0 or left blank Convergence is achieved when residuals satisfy the criterion.

Main Index

CONTROL (Mechanical - Model Definition) 479 Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry 1 Convergence is achieved when displacements satisfy the criterion. 2 Convergence is achieved when strain energy satisfies the criteria. 4 Convergence is achieved when either residual or displacement satisfies the criterion. 5 Convergence is achieved when both residual and displacement satisfies the criterion. Notes:

Testing on relative displacements or strain energy always requires at least one iteration. If nonlinear analysis is done with the CENTROID parameter, the residuals are not calculated and testing is always done on displacements. Nonlinear analysis with the CENTROID parameter is not recommended. If the fields are set as 0, 1, or 2, only the 3rd data block is needed. If the fields are set as 4 or 5, the 3a data block is also needed. In this case, the 3rd data block is set for residual testing and 3a data block is set for displacements check only.

21-25

26-30

5th

6th

I

I

Flag to specify relative or absolute error testing. If equal to 0

Testing is done on relative error.

If equal to 1

Testing is done on absolute value.

If equal to 2

Testing is done on relative error testing unless reactions or incremental displacements are below minimum value, in which case absolute tolerances testing is used.

Iterative procedure flag. 1 Full Newton-Raphson (default). 2 Modified Newton-Raphson (no reassembly during iteration). 3 Newton-Raphson with strain correction modification (see Marc Volume A: Theory and User Information). 8 Secant method.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced. Note:

Main Index

With use of gap and Herrmann elements, the matrix always is nonpositive definite and this entry has no significance.

480 CONTROL (Mechanical - Model Definition) Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry

36-40

8th

I

No longer used; enter 0.

41-45

9th

I

To print convergence control messages to log file, enter 1.

46-50

10th

I

Control on initial stress stiffness. 0 Normal-full contribution. 1 For Mooney material, reduce contribution of hydrostatic pressure on initial stress stiffness according to: σ i ni ti al = σ – f r ⋅ p ⋅ I

where σ i ni ti al is the stress tensor used in the initial stress stiffness matrix, σ is the current stress tensor, f r is entered through the PARAMETERS option, pressure and I I is a unit tensor.

p

is the hydrostatic

2 No initial stress stiffness. 3 Use stress at beginning of increment, not last iteration. 4 Results in the inclusion of only the positive stresses in the initial stress stiffness during the equilibrium iteration. Besides faster convergence, this leads to a stable analysis of very thin shell structures. 51-55

11th

I

Control parameter: 0 Do not allow switching of convergence testing between residuals and displacements. 1 Allow switching of convergence testing between residual and displacements if reaction forces or displacements become extremely small. For more details, see Marc Volume A: Theory and User Information. Note:

Set this parameter to 0 if any kind of absolute value testing is being used.

56-60

12th

I

Assembly flag. If set to 1, the stiffness matrix is assembled each iteration. Note that this switches off the modified Newton-Raphson procedure if chosen in the sixth field of this data block.

61-65

13th

I

For some material models, such as damage, cracking, and Chaboche, there is an inner iteration loop to insure accuracy. The maximum number of iterations allowed can be set here. Default is 50.

3rd data block Include if residual testing is required and the fourth field of the 2nd data block is 0, 4, or 5.

Main Index

CONTROL (Mechanical - Model Definition) 481 Control Option for Stress Analysis

Format Fixed 1-10

Free 1st

Data Entry Entry F

If relative residual checking: Maximum allowable value of maximum residual force divided by maximum reaction force. Default is 0.10.

11-20

2nd

F

If relative residual checking: Maximum allowable value of maximum residual moment divided by maximum reaction moment. Default is 0.0, in which case, no checking on residual moment occurs.

21-30

3rd

F

If relative residual checking: Minimum reaction force, if reaction force is less than this value, checking is bypassed or absolute testing is performed.

31-40

4th

F

If relative residual checking: Minimum moment: if moment is less than this value, checking is bypassed or absolute testing is performed.

41-50

5th

F

If absolute residual testing: Maximum value of residual force. Default is 0.0 in which case, no checking on residual force takes place.

51-60

6th

F

If absolute residual testing: Maximum value of residual moment. Default is 0.0 in which case, no checking on residual moments takes place. If absolute displacement testing, maximum value of rotation increment. Default is 0.0; in which case, no checking or rotations take place.

61-70

7th

F

Rigid Link Rotation Tolerance: Maximum allowable value of the change in rotation increment at the retained nodes of RBE2, rigid link (tying type 80) or beam-shell offset nodes. Default is 0.001 radians.

Notes:

If the 4th field of the 2nd data block is 4 or 5, the rigid link rotation tolerance entered in the 4th data block circumvents the corresponding value in the 3rd data block. The rigid link rotation tolerance if left at 0, is reset to 0.001 radians by the Marc solver to ensure backward compatibility for RBE2.Theare two ways to by-pass the link rotation check: the rigid link rotation tolerance can be set to a negative number, or the rigid link rotation tolerance can be left as 0.0 with an additional FEATURE,5701 added to the parameter section of the input.

Main Index

482 CONTROL (Mechanical - Model Definition) Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry

4th data block Include if displacement testing is required and the fourth field of the 2nd data block is 1, 4, or 5. 1-10

1

F

Maximum allowable value of the change in displacement increment divided by the displacement increment. Default is 0.10.

11-20

2nd

F

Maximum allowable value of the change in rotational increment divided by the rotational increment. Default is 0.0, in which case, no checking on change in rotational increment occurs.

21-30

3rd

F

Minimum displacement, if displacement increment is less than this value, checking is bypassed or absolute testing is performed.

31-40

4th

F

Minimum rotation: if rotation increment is less than this value, checking is bypassed.

41-50

5th

F

Maximum value of displacement increment. Default is 0.0; in which case, no checking on displacements takes place.

51-60

6th

F

Maximum value of rotation increment. Default is 0.0; in which case, no checking on rotations takes place.

61-70

7th

F

Rigid Link Rotation Tolerance: Maximum allowable value of the change in rotation increment at the retained nodes of RBE2, rigid link (tying type 80) or beam-shell offset nodes. Default is 0.001 radians.

Notes:

If the 4th field of the 2nd data block is 4 or 5, the rigid link rotation tolerance entered in the 4th data block circumvents the corresponding value in the 3rd data block. The rigid link rotation tolerance if left at 0, is reset to 0.001 radians by the Marc solver to ensure backward compatibility for RBE2.Theare two ways to by-pass the link rotation check: the rigid link rotation tolerance can be set to a negative number, or the rigid link rotation tolerance can be left as 0.0 with an additional FEATURE,5701 added to the parameter section of the input.

5th data block Include if energy testing is required and the fourth field of the 2nd data block is 2. 1-10

1st

F

Maximum allowable value of the change is energy increment. Default is 0.1.

Main Index

CONTROL (Mechanical - Model Definition) 483 Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry

6th data block Only necessary for coupled thermal-mechanical analysis. 1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are reevaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable. Note:

Only the temperature estimate error (3rd field) is checked for the TRANSIENT NON AUTO fixed stepping procedure. All three fields are checked for the transient adaptive stepping procedure. None of the three fields are checked for the auto step adaptive stepping procedure.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Maximum change of xsi,p allowed in pyrolysis calculation. Used to control automatic time step scheme.

51-60

6th

F

Maximum change of xsi,v allowed in pyrolysis calculation. Used to control automatic time step scheme.

61-70

7th

F

Maximum change of xsi,c allowed in pyrolysis calculation. Used to control automatic time step scheme.

71-80

8th

F

Maximum change in surface displacement per time step due to recession. This is used to control the time step for the TRANSIENT option.

7th data block Only necessary for coupled electrostatic structural analysis.

Main Index

1-10

1st

F

Maximum allowed relative error in residual charge.

11-20

2nd

F

Maximum allowed absolute error in residual charge.

484 PARAMETERS (Model Definition) Definition of Parameters used in Numerical Analysis

PARAMETERS (Model Definition)

Definition of Parameters used in Numerical Analysis

Description There are many parameters that are used in the finite element calculations. These parameters can be customized for your particular application. Some of these constants can be entered in other input blocks as well. The last nonzero value is used for the calculation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PARAMETERS.

E

Enter the scale factor which, when multiplied with the incremental strain, is used to predict the incremental strain in the next increment.

2nd data block 1-10

1st

Default is 1.0. 11-20

2nd

E

Enter the multiplier used to calculate the penalty factor to impose boundary conditions. The penalty factor is this multiplier times the maximum diagonal value of the operator matrix. Default multiplier is 1 x 109. If the APPBC parameter is used, this option is not used.

21-30

3rd

E

Enter the penalty factor used to satisfy incompressibility in rigid plastic analysis for plane strain, axisymmetric, or solid analysis when displacement elements are used. Default is 100.

31-40

4th

E

Enter the penalty factor used to satisfy incompressibility in fluid analysis when displacement elements are used. Default is 1 x 106.

41-50

5th

E

Beta parameter used in transient dynamic analysis using Newmark-beta procedure. Default is 0.25.

51-60

6th

E

Gamma parameter used in transient dynamic analysis using Newmarkbeta procedure. Default is 0.50.

61-70

Main Index

7th

E

Gamma1 parameter used in transient dynamic analysis using Single Step Houbolt procedure.

PARAMETERS (Model Definition) 485 Definition of Parameters used in Numerical Analysis

Format Fixed

Free

Data Entry Entry Default is 1.5.

71-80

8th

E

Gamma parameter used in transient dynamic analysis using Single Step Houbolt procedure. Default is -0.5.

3rd data block 1-10

1st

E

Enter the angle at which a node separates from a convex corner or becomes stuck in a concave corner for two-dimensional contact. Default is 8.625°.

11-20

2nd

E

Enter the angle at which a node separates from a convex corner or becomes stuck in a concave corner for three-dimensional contact. Default is 20.0°.

21-30

3rd

E

Enter the initial strain rate for rigid plastic analysis. Default is 1 x 10-4.

31-40

4th

E

Enter the cutoff strain rate for rigid plastic analysis. Default is 1 x 10-12.

41-50

5th

E

Enter the fraction of the hydrostatic pressure that is subtracted from the stress tensor in the initial stress calculation. See the tenth field of the CONTROL option. Default is 1.0

51-60

6th

E

Enter the factor used to calculate the drilling mode for shell elements type 22, 75, 138, 139, and 140.

Default is 0.0001. 61-70

7th

E

Enter the scale factor to the initial incremental displacements estimate for the increment after a rezoning increment. The default value is 1.0, which usually improves friction convergence, but may result in an inside-out element.

4th data block (Optional) 1-10

1st

E

Universal gas constant (R). Default is 8.314 J mol-1K-1.

11-20

2nd

E

Offset temperature between user units and absolute temperature. Default is 273.15°; that is, user input in Centigrade. If user temperature is in Kelvin (K) or Rankine (R), enter a negative value. The offset temperature is then set to zero.

21-30

3rd

E

Thermal Properties Evaluation Weight. Default is 0.5

Main Index

486 PARAMETERS (Model Definition) Definition of Parameters used in Numerical Analysis

Format Fixed 31-40

Free 4th

Data Entry Entry E

Surface projection factor for single step Houbolt. Default is 0.0.

41-50

5th

E

Stefan Boltzmann Constant. Default is 5.67051 x 10-8 W/m2K4.

51-60

6th

E

Planks second constant. Default is 14387.69 μM°K.

61-70

7th

E

Speed of light in a vacuum. Default is 2.9979 x 1014 μM/s

71-80

8th

E

Maximum change in the incremental displacement in a Newton-Raphson iteration. Default is 1 x 1030.

5th data block (Optional) 1-10

1st

E

Initial friction stiffness (only for friction models 6 and 7). This stiffness will be used during the first cycle of an increment to define the friction stiffness matrix in cases where a touching node has a zero normal force and the amount of sliding does not exceed the elastic sticking limit. If set to zero, Marc will estimate the initial friction stiffness based on the initial average stiffness of the contact body to which the touching node belongs.

Main Index

11-20

2nd

E

Specifies the minimum value that indicates a singularity if a direct solver is used. If a zero is given, that this value is set internally by Marc and depends on the solver being used.

21-30

3rd

E

Specify the maximum change in temperature per iteration in radiation simulations. This is useful to stabilize the solution. The default is 100.

31-40

4th

E

Enter parameter alphaf for the generalized alpha dynamic operator. Note that the value of alphaf defined here may be overruled by defining the spectral radius on the 6th field.

PARAMETERS (Model Definition) 487 Definition of Parameters used in Numerical Analysis

Format Fixed

Free

Data Entry Entry

41-50

5th

E

Enter parameter alpham for the generalized alpha dynamic operator. Note that the value of alpham defined here may be overruled by defining the spectral radius on the 6th field.

51-60

6th

E

Define the spectral radius S for the generalized alpha dynamic operator. The following conventions apply: • 0 ≤ S ≤ 1 : the 4th and 5th field are ignored and alphaf and alpham

are calculated based upon the spectral radius according to alphaf = - S /(1+ S ) and alpham = (1-2 S )/(1+ S ) • S = – 1 : the 4th and 5th field are ignored and neither alphaf nor alpham will be changed • S = – 2 : the 4th and 5th field are ignored and the values of alphaf and alpham will be optimized for a dynamic contact analysis • S = – 3 : the 4th and 5th field are ignored and the values of alphaf and alpham will be optimized for an analysis without dynamic

contact • S = – 4 : use the values of alphaf and alpham as entered on the 4th

and 5th field 61-70

Main Index

7th

E

RBE3 conditioning number. If the conditioning number is greater than this value, the RBE3 is probably singular and a warning message is printed. If the value is negative, the analysis is stopped. Default is 1 x 106.

488 FIXED DISP (with TABLE Input - Mechanical) Define Fixed Displacement

FIXED DISP (with TABLE Input - Mechanical)

Define Fixed Displacement

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This data block defines potential fixed displacements, including the magnitude, degrees of freedom and applied locations, and associates it with a boundary condition name. This boundary condition is activated or deactivated using the LOADCASE model or history definition option. The boundary conditions are specified either by giving the kinematic displacement, a list of degrees of freedom, and either a list of nodal numbers or a list of surfaces. The prescribed displacements are with respect to the degrees of freedom associated with the element, unless they have been transformed to a local coordinate system using either the TRANSFORMATION, COORD SYSTEM, SHELL TRANSFORMATION, or UTRANFORM options. The FORCDT or FORCDF user subroutines or the TABLE model definition option can be used to enter nonuniform time or frequency dependent boundary conditions. Note:

In static analysis, the boundary conditions specified must always be sufficient to remove all rigid body modes. It is advised that boundary conditions not be placed on nodes which might come into contact. Using a symmetry rigid body is preferred. Fourier loading using the table driven input format is not supported in this release. Use the non-table driven input instead.

Further detail is given in Marc Volume A: Theory and User Information. See Marc Volume B: Element Library, for a definition of the degrees of freedom for each element type. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED DISP.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

Unit number to read data default is the standard input file.

Data blocks 3 through 10 are repeated for each set.

Main Index

FIXED DISP (with TABLE Input - Mechanical) 489 Define Fixed Displacement

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutines are required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

4th

I

Enter the Fourier series number associated with prescribed displacement, enter 0 if no Fourier series.

21-25

5th

I

Enter a 0 if total displacements are to be given (default). Enter a 1 if incremental displacements relative to the position at the beginning of this loadcase are to be given.

26-30

6th

I

Not used.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE model definition option.

If a real displacement is to be defined, data blocks 4 and 5 are used. If a complex harmonic displacement is to be defined, data blocks 4 and 5 define the real component or the magnitude, and data blocks 6 and 7 define the imaginary component or the phase. 4th data block - Magnitudes 1-10

1st

E

Prescribed displacement for first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed displacement for second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed displacement for third degree of freedom listed in data block 8. A maximum of eight kinematic constraints can be specified.

5th data block - Table IDs 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

The 6th and 7th data blocks are only required if a complex harmonic boundary condition.

Main Index

490 FIXED DISP (with TABLE Input - Mechanical) Define Fixed Displacement

Format Fixed

Free

Data Entry Entry

6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of displacement or the phase of the first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed imaginary component of displacement or the phase of the second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed imaginary component of displacement or the phase of the third degree of freedom listed in data block 8.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for imaginary component or phase for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for imaginary component or phase for the third degree of freedom listed.

8th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 9th and 10th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention

Main Index

FIXED DISP (with TABLE Input - Mechanical) 491 Define Fixed Displacement

Format Fixed

Free

Data Entry Entry

10th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

Main Index

492 FIXED DISP (Mechanical) Define Fixed Displacement

FIXED DISP (Mechanical)

Define Fixed Displacement

The information provided here is based upon not using the table driven input style. Description This data defines the fixed displacement that each specified degree of freedom must take during the first and subsequent increments, unless it is further modified using the DISP CHANGE option. The boundary conditions are specified either by giving the kinematic displacement and a list of degrees of freedom and a list of nodal numbers or by the input of boundary conditions generated during mesh generation (MESH2D). The prescribed displacements are with respect to the degrees of freedom associated with the element, unless they have been transformed to a local coordinate system using either the TRANSFORMATION, COORD SYSTEM, SHELL TRANSFORMATION, or UTRANFORM options. Note:

In static analysis, the boundary conditions specified must always be sufficient to remove all rigid body modes. Fourier loading using the table driven input format is not supported in this release. Use the non-table driven input instead.

Further detail is given in Marc Volume A: Theory and User Information. See Marc Volume B: Element Library, for a definition of the degrees of freedom for each element type. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED DISP.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data is required in this option.

11-15

3rd

I

Unit number used for MESH2D option. Note:

The boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition data must be arranged accordingly.

For each set of boundary conditions use the 3rd, 4th, and 5th data blocks.

Main Index

FIXED DISP (Mechanical) 493 Define Fixed Displacement

Format Fixed

Free

Data Entry Entry

3a data block Use only if not Fourier Analysis. 1-10

1st

E

Prescribed displacement for first degree of freedom listed in data block 4.

11-20

2nd

E

Prescribed displacement for second degree of freedom listed in data block 4.

21-30

3rd

F

Prescribed displacement for third degree of freedom listed in data block 4. A maximum of eight kinematic constraints can be specified. The third data block is read as 8E10.3.

3b data block Use for Fourier analysis only. 1-5

1st

I

Enter the series number associated with this boundary condition.

6-15

2nd

F

Prescribed displacement for first degree of freedom listed in data block 4.

16-25

3rd

F

Prescribed displacement for second degree of freedom listed in data block 4.

26-35

4th

F

Prescribed displacement for third degree of freedom listed in data block 4.

36-45

5th

F

Prescribed displacement for fourth degree of freedom listed in data block 4.

46-55

6th

F

Prescribed displacement for fifth degree of freedom listed in data block 4.

4th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes to which the above boundary conditions are applied.

Main Index

494 DIST LOADS (with TABLE Input - Model Definition) Define Distributed Loads

DIST LOADS (with TABLE Input - Model Definition) Define Distributed Loads The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This data block defines potential distributed loads applied to the model, including the magnitude, type of load and location, and associates this with a boundary condition name. This boundary condition will be activated or deactivated using the LOADCASE model or history definition option. The FORCEM user subroutine can be used for nonuniform, time-dependent distributed loads, or the TABLE model definition option may be used. The distributed loads entered here are total loads. If no time-dependent tables are referenced and the ramping options in the LOADCASE model or history definition option are not used, the distributed load will be instantaneously applied in the loadcase. When used with global adaptive meshing, if the load is applied to a curve or a surface where element edges or faces are attached, the load is correctly applied after remeshing. Note:

If distributed load is applied on the bottom of a shell, the sign of the load is reversed, that is, a positive load is now in the direction of the normal to the surface. Fourier loading using the table driven input format is not supported in this release. Use the non-table driven input instead.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST LOADS.

2nd data block 1-5

1st

I

Enter the number of sets of distributed loads to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed load data, defaults to input.

The 3rd through 9th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

Main Index

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

DIST LOADS (with TABLE Input - Model Definition) 495 Define Distributed Loads

Format Fixed 6-10

Free 2nd

Data Entry Entry I

Enter 0 if no user subroutine required. Enter 1 if the FORCEM user subroutine required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

4th

I

Enter the Fourier series number associated with the load, enter 0 if no Fourier series.

21-25

5th

I

Enter the cavity number if necessary.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE model definition option.

If a real distributed load is to be defined, data blocks 4 and 5 are used. If a complex harmonic distributed load is to be defined, data blocks 4 and 5 define the real component or the magnitude, and data blocks 6 and 7 define the imaginary component or the phase. 4th data block 1-10

1st

F

Enter the magnitude of this type of distributed load. For load type 21 or 102 to 113, enter the magnitude of load in first coordinate direction.

11-20

2nd

F

For load type 21 or 102 to 113, enter the load in second coordinate direction.

21-30

3rd

F

For load type 21 or 102 to 113, enter the load in third coordinate direction.

5th data block 1-5

1st

I

Enter the table ID associated with the load. For load type 21 or 102 to 113, enter the table ID associated with the load in the first direction.

6-10

2nd

I

For load type 21 or 102 to 113, enter the table ID associated with the load in the second direction.

11-15

3rd

I

For load type 21 or 102 to 113, enter the table ID associated with the load in the third direction.

The 6th and 7th data blocks are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle

Main Index

1-10

1st

E

Prescribed imaginary component of load or phase angle.

11-20

2nd

E

For load type 21 or 102 to 113, enter the imaginary component of load in second coordinate direction.

496 DIST LOADS (with TABLE Input - Model Definition) Define Distributed Loads

Format Fixed 21-30

Free 3rd

Data Entry Entry E

For load type 21 or 102 to 113, enter the imaginary component of load in third coordinate direction.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase.

6-10

2nd

I

For load type 21 or 102 to 113, enter the table ID for imaginary component or phase in second direction.

11-15

3rd

I

For load type 21 or 102 to 113, enter the table ID for imaginary component or phase in third direction.

8th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal pressure 2: Shear stress in 1st tangent direction 3: Shear stress in 2nd tangent direction 4: Volumetric in x-direction 5: Volumetric in y-direction 6: Volumetric in z-direction 7: force/length in beams x-direction 8: force/length in beams y-direction 9: force/length in beams z-direction 11: Wave loading 13: Force/length on edge of shell on midplane; perpendicular to edge 14: Force/length on edge of shell on midplane; tangent to the edge; positive is from node 1 to node 1+1 15: Force/length on edge of shell; perpendicular to shell, for example, -v3 direction 21: General traction 100 + jaxis: Centrifugal based upon entering ω2,ω in radians/time 101: Inelastic heat generation

Main Index

DIST LOADS (with TABLE Input - Model Definition) 497 Define Distributed Loads

Format Fixed

Free

Data Entry Entry 102: Gravity 103 + jaxis: Coriolis based upon entering ω2,ω in radians/time 104 + jaxis: Centrifugal based upon entering ω (cycles/time) 105 + jaxis: Coriolis based upon entering ω (cycles/time) 106: Uniform body load (force per unit volume) 107: Nonuniform body load (force per unit volume) 110: Uniform beam load (force per unit length) 111: Nonuniform beam load (force per unit length) 112: Uniform load per unit area 113: Nonuniform load per unit area Note:

11-15

3rd

I

For problems with more than one rotation axes, jaxis equals the rotation ID times a thousand.

Enter the face ID.

9th data block The 9th and 10th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Mentat convention 19: Curve ID: orientation ID - Mentat convention

Main Index

498 DIST LOADS (with TABLE Input - Model Definition) Define Distributed Loads

Format Fixed

Free

Data Entry Entry

10th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

DIST LOADS (Model Definition) 499 Define Distributed Loads

DIST LOADS (Model Definition)

Define Distributed Loads

The information provided here is based upon not using the table driven input style. Description This block of data allows pressure (surface and volumetric) loads to be specified. These values are incremental values per increment if a fixed time-step procedure is used or the total change over the loadcase if an adaptive time-step procedure is used or the total value of the load if the ELASTIC parameter is used. User subroutine FORCEM can be used for nonuniform, time-dependent distributed loads. Note:

If FOLLOW FOR is included in the input file with DIST LOADS, the input about type of load, magnitude etc. (data blocks 3 and 4) needs to be consistent in the model and history definition options.

If FEATURE,203 is used, then the pressure on an edge (2-D) or face (3-D) is applied, unless all nodes of that edge or face are in contact with another body. If separation occurs, the distributed load is reapplied to the surface. For most distributed load types, one enters a load per unit length (on beams or shell edges) or a load per unit area. There are a few exceptions listed below: Load Type 100

Centrifugal

Enter ω2 (ω in radians/time)

102

Gravity

Enter three values (Force/mass)

103

Centrifugal and Coriolis

Enter ω2 (ω in radians/time)

104

Centrifugal

Enter ω (ω in cycles/time)

105

Centrifugal and Coriolis

Enter ω (ω in cycles/time)

106

Uniform Volumetric load

Enter three values force/volume

107

Nonuniform Volumetric load

Enter three values force/volume

110

Uniform load per unit length

Enter three values force/length

111

Nonuniform load per unit length

Enter three values force/length

112

Uniform load per unit area

Enter three values force/area

113

Nonuniform load per unit area

Enter three values force/area

General traction

Enter three values force/area

-10 to -21

Main Index

500 DIST LOADS (Model Definition) Define Distributed Loads

Table 3-8

CID Load Types (Not Table Driven Input)

IBODY

Specify Traction on Edge or Face

User Subroutine

-10

1

No

-11

1

Yes

-12

2

No

-13

3

Yes

-14

3

No

-15

3

Yes

-16

4

No

-17

4

Yes

-18

5

No

-19

5

Yes

-20

6

No

-21

6

Yes

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST LOADS.

2nd data block 1-5

1st

I

Enter the number of sets of distributed loads to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed load data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3a data block Use if conventional Marc input, not Fourier, not applied to a cavity, and not Nastran PLOAD4 style. 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library. For problems with more than one rotation axes, add the rotation axis ID times a thousand.

6-15

2nd

F

Enter the magnitude of this type of distributed load. For load types -10 to -21 or 102 to 113, enter the magnitude of load in first coordinate direction.

Main Index

DIST LOADS (Model Definition) 501 Define Distributed Loads

Format Fixed

Free

Data Entry Entry

16-25

3rd

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in second coordinate direction

26-35

4th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in third coordinate direction

36-40

5th

I

Distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.)

3b data block Use if distributed load is applied to cavity and not Fourier. The CAVITY parameter and CAVITY model definition option is also required. 1-5

1st

I

Enter the value of ibody_cavity. i bo dy _c a vi t y = ic a vi t y * 10000 + i c av it y _t y pe * 1000 + ib od y

where ibody_cavity is the cavity-modified value for the distributed load type. icavity is the cavity ID. icavity_type is the cavity load type: 0: cavity is closed. 1: cavity is loaded with an applied pressure. 2: cavity is loaded with an applied mass. 9: cavity load is defined by the UCAV user subroutine. ibody is the original value for the distributed load type (see library element description in Marc Volume B: Element Library.) 6-15

2nd

F

If icavity_type = 1, enter incremental pressure. If icavity_type = 2, enter incremental mass.

Main Index

16-25

3rd

F

Not used; enter 0.

26-35

4th

F

Not used; enter 0.

36-40

5th

I

Distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.)

41-45

6th

I

Enter -1 if the cavity load is not active.

502 DIST LOADS (Model Definition) Define Distributed Loads

Format Fixed

Free

Data Entry Entry

3c data block Use if Fourier Analysis. 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library. For problems with more than one rotation axes, add the rotation axis ID times a thousand.

6-15

2nd

I

Enter the series number associated with this load.

16-25

3rd

F

Enter the magnitude of this type of distributed load. For load types -10 to -21 or 102 to 113, enter the magnitude of load in first coordinate direction.

26-35

4th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in second coordinate direction.

36-40

5th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in third coordinate direction.

3d data block Use if Nastran PLOAD4 style input.

Main Index

1-5

1st

I

Parameter identifying the type of load plus 200. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter P1, the magnitude of load at node 1 of face or edge.

16-25

3rd

F

Enter P2, the magnitude of load at node 2 of face or edge.

26-35

4th

F

Enter P3, the magnitude of load at node 3 of face or edge.

36-45

5th

F

Enter P4, the magnitude of load at node 4 of face or edge. Not required if a triangular face.

46-55

6th

F

Enter first component of direction of load.

56-65

7th

F

Enter second component of direction of load.

DIST LOADS (Model Definition) 503 Define Distributed Loads

Format Fixed

Free

Data Entry Entry

66-75

8th

F

Enter third component of direction of load.

76-80

9th

I

If positive, distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.) If the direction of the load is given with respect to a COORD SYSTEM option, then enter the negative of the coordinate system ID.

Notes:

If the direction of the load is not defined, then the conventional Marc direction is used. If the direction of the load is defined, then it is fixed and not updated even if the FOLLOW FOR parameter is activated.

4th data block Enter a list of elements associated with the above distributed loads.

Main Index

504 FACE IDS Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

FACE IDS

Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

1-D 2-Node Elements y

FACE ID

NODES

1

1–2

FACE ID

NODES

1

1–2–3

2 1

x

1-D 3-Node Elements 3 2 1

2-D 4-Node Quadrilateral Elements 4

1

3

2

Load shown on FACE ID 1

Main Index

FACE ID

NODES

1

1–2

2

2–3

3

3–4

4

4–1

FACE IDS 505 Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

2-D 8-Node Quadrilateral Elements 4

7

3

8

FACE ID

NODES

1

1–5–2

2

2–6–3

3

3–7–4

4

4–8–1

6

1

5

2

2-D 3-Node Triangle 3

1

FACE ID

NODES

1

1–2

2

2–3

3

3–1

FACE ID

NODES

1

1–4–2

2

2–5–3

3

3–6–1

2

2-D 6-Node Triangle 3

6

1

5

4

2

3-D 3-Node Shell z

3

1 y x

Main Index

2

FACE ID

NODES

1

1–2–3

(top)

2

1–3–2

(bottom)

506 FACE IDS Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

3-D 4-Node Shell/Membrane 4

P

3

FACE ID

NODES

1

1–2–3–4

(top)

2

1–4–3–2

(bottom)

1

2

3-D 6-Node Shell 3

P

6

FACE ID

NODES

1

1–2–3–4–5–6

(top)

2

1–3–2–6–5–4

(bottom)

5

1

4

2

3-D 8-Node Shell 4

7

3

8

6

1

5

FACE ID

NODES

1

1–2–3–4–5–6–7–8

(top)

2

1–4–3–2–8–7–6–5

(bottom)

2

3-D 4-Node Tetrahedral 4 3

1 2

Main Index

FACE ID

NODES

1

1–2–4

2

2–3–4

3

3–1–4

4

1–2–3

FACE IDS 507 Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

3-D 6-Node Pentahedral 6 4

5

3

FACE ID

NODES

1

1–2–5–4

2

2–3–6–5

3

3 –1 – 4 – 6

4

1–3–2

5

4–5–6

1 2

3-D 15-Node Pentahedral 3 15 6

8

9

NODES

1 2 3 4 5

1 – 2 – 5 – 4 – 7 – 14 – 10 – 13 2 – 3 – 6 – 5 – 8 – 15 – 11 – 14 3 – 1 – 4 – 6 – 9 – 13 – 12 – 15 3–2–1–8–7–9 4 – 5– 6 – 10 – 11 – 12

11

12

7

1

2

14

13 4

FACE ID

5

10

3-D 8-Node Brick 8

7

5 6 4

1

3

2

Main Index

FACE ID

NODES

1

1–2–6–5

2

2–3–7–6

3

3–4–8–7

4

4–1–5–8

5

1–2–3–4

6

6–5–8–7

508 FACE IDS Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations

3-D 10-Node Tetrahedral 4

10

FACE ID

NODES

1

1 – 2 – 4 – 5 – 09 – 08

2

2 – 3 – 4 – 6 – 10 – 09

3

3 – 1 – 4 – 7 – 08 – 10

4

1 – 2 – 3 – 5 – 06 – 07

3

8

9 7 6

1 5 2

3-D 20-Node Brick 8 16

15 7

5 20

13

14

6

19

17

4 12

11 18

1

3 9

10 2

Main Index

FACE ID

NODES

1

1 – 2 – 6 – 5 – 09 – 18 – 13 – 17

2

2 – 3 – 7 – 6 – 10 – 19 – 14 – 18

3

3 – 4 – 8 – 7 – 11 – 20 – 15 – 19

4

4 – 1 – 5 – 8 – 12 – 17 – 16 – 20

5

1 – 2 – 3 – 4 – 09 – 10 – 11 – 12

6

6 – 5 – 8 – 7 – 13 – 16 – 15 – 14

POINT LOAD (with TABLE Input - Model Definition) 509 Define Nodal Point Loads

POINT LOAD (with TABLE Input - Model Definition)Define Nodal Point Loads The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This data block defines potential point loads, including the magnitude and location of application and associates this with a boundary condition name. This boundary condition will be activated or deactivated using the LOADCASE model or history definition option. Point loads can be specified as fixed direction loads or follower loads. The prescribed forces are with respect to the degrees of freedom associated with the element, unless they have been transformed to a local coordinate system using either the TRANSFORMATION, COORD SYSTEM, SHELL TRANSFORMATION, or UTRANFORM options. The point loads entered here are total loads. If no time-dependent tables are referenced and the ramping options in the LOADCASE model or history definition option are not used, the point load will be instantaneously applied in the loadcase. The FORCDT or FORCDF user subroutines or the TABLE model definition option can be used to enter nonuniform time or frequency dependent boundary conditions. Notes:

Fourier loading using the table driven input format is not supported in this release. Use the non-table driven input instead. The fourth field of the FOLLOW FOR parameter should be set to 1 when follower force point loads are used in the model. The follower load is only supported through the mesh based automated option wherein the nodal loads are specified in vector form and the initial load orientation with respect to the mesh is maintained as the structure deforms. The follower force option is not available for fourier loads or harmonic loads. Also, the follower force capability is not supported for point loads specified through the FORCDT user subroutine.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT LOAD.

2nd data block 1-5

1st

I

Enter number of sets of point loads to be entered (optional).

6-10

2nd

I

Enter unit number for input of point load data, defaults to input.

The 3rd through 8th data blocks are entered as pairs, one for each data set.

Main Index

510 POINT LOAD (with TABLE Input - Model Definition) Define Nodal Point Loads

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 8th and 9th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDT user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

4th

I

Enter the Fourier series number associated with the nodal load; enter 0 if no Fourier series.

21-25

5th

I

Enter 0 for fixed direction load. Enter -1 for automated follower force

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

If a real point load is to be defined, data blocks 3 and 4 are used. If a complex harmonic point load is to be defined, data blocks 4 and 5 define the real component or the magnitude; and data blocks 6 and 7 define the imaginary component or the phase. 4th data block Real magnitude. 1-10

1st

F

Nodal load associated with first degree of freedom.

11-20

2nd

F

Nodal load associated with second degree of freedom.

21-30

3rd

F

Nodal load associated with third degree of freedom.

31-40

4th

F

Nodal load associated with fourth degree of freedom.

41-50

5th

F

Nodal load associated with fifth degree of freedom.

51-60

6th

F

Nodal load associated with sixth degree of freedom.

5th data block - Table ID for Real Magnitude

Main Index

1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

16-20

4th

I

Table ID associated with the fourth degree of freedom.

21-25

5th

I

Table ID associated with the fifth degree of freedom.

POINT LOAD (with TABLE Input - Model Definition) 511 Define Nodal Point Loads

Format Fixed 26-30

Free 6th

Data Entry Entry I

Table ID associated with the sixth degree of freedom.

The 6th and 7th data blocks are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Imaginary component/phase associated with first degree of freedom.

11-20

2nd

E

Imaginary component/phase associated with second degree of freedom.

21-30

3rd

E

Imaginary component/phase associated with third degree of freedom.

31-40

4th

E

Imaginary component/phase associated with fourth degree of freedom.

41-50

5th

E

Imaginary component/phase associated with fifth degree of freedom.

51-60

6th

E

Imaginary component/phase associated with sixth degree of freedom.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase for first degree of freedom.

6-10

2nd

I

Enter the table ID for imaginary component or phase for second degree of freedom.

11-15

3rd

I

Enter the table ID for imaginary component or phase for third degree of freedom.

16-20

4th

I

Enter the table ID for imaginary component or phase for fourth degree of freedom.

21-25

5th

I

Enter the table ID for imaginary component or phase for fifth degree of freedom.

26-30

6th

I

Enter the table ID for imaginary component or phase for sixth degree of freedom.

The 8th and 9th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 8th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs

Main Index

512 POINT LOAD (with TABLE Input - Model Definition) Define Nodal Point Loads

Format Fixed

Free

Data Entry Entry 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention

9th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 8th data block.

Main Index

POINT LOAD (Model Definition) 513 Define Nodal Point Loads

POINT LOAD (Model Definition)

Define Nodal Point Loads

The information provided here is based upon not using the table driven input style. Description This block of data allows nodal point loads to be specified. The nodal loads can be specified as fixed direction loads or follower loads. For the fixed direction loads, the nodal forces are always specified in vector form. For the follower loads, two options are possible: Option 1 is the MD Nastran style Follower Force wherein the magnitudes of the nodal force and moment are specified and the direction is independently specified using 2 or 4 nodes. Option 2 is the Mesh Based Automated Follower Force wherein the nodal loads are specified in vector form and the initial load orientation with respect to the mesh is maintained as the structure deforms. For more details, refer to Marc Volume A: Theory and User Information. These values are incremental values unless the ELASTIC parameter is used or the 3rd field of the FOLLOW FOR parameter is set to 1, in which case they are total loads. When specified in the form of a load vector, the prescribed forces are with respect to the degrees of freedom associated with the element, unless they have been transformed to a local coordinate system using either the TRANSFORMATION, COORD SYSTEM, SHELL TRANSFORMATION, or UTRANFORM options. Notes:

Enter an upper bound to the number of nodes with point loads on the DIST LOADS parameter. The fourth field of the FOLLOW FOR parameter should be set to 1 when follower force loads are used in the model. When this global parameter for follower force point loads is turned on, the 5th data block is mandatory. The follower force option is not valid for fourier loads or harmonic loads. Also, the follower force capability is not supported for point loads specified through user subroutine FORCDT.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT LOAD.

2nd data block

Main Index

1-5

1st

I

Enter number of sets of point loads to be entered (optional).

6-10

2nd

I

Enter unit number for input of point load data, defaults to input.

11-15

3rd

I

Enter 1 to signal existence of more than one point loadcase on the same node. The loads are summed in this case.

514 POINT LOAD (Model Definition) Define Nodal Point Loads

Format Fixed

Free

Data Entry Entry

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3a data block Use if not Fourier Analysis. 1-10

1st

F

Nodal load associated with first degree of freedom. Nodal force magnitude for MD Nastran style follower force.

11-20

2nd

F

Nodal load associated with second degree of freedom. Nodal moment magnitude for MD Nastran style follower force.

21-30

3rd

F

Nodal load associated with third degree of freedom.

31-40

4th

F

Nodal load associated with fourth degree of freedom.

41-50

5th

F

Nodal load associated with fifth degree of freedom.

51-60

6th

F

Nodal load associated with sixth degree of freedom.

61-70

7th

F

Nodal load associated with seventh degree of freedom.

71-80

8th

F

Nodal load associated with eighth degree of freedom.

Continuation data is necessary, must be in 6E10.3 format. Continuation data is needed if more than eight degrees of freedom per node in analysis. Notes:

The nodal load vector is valid for fixed direction force or for automated follower force. Only the first two fields are used for the MD Nastran style follower force.

3b data block Use only if Fourier Analysis. 1-5

1st

I

Enter the series number associated with this load.

6-15

2nd

F

Nodal load associated with first degree of freedom.

16-25

3rd

F

Nodal load associated with second degree of freedom.

26-35

4th

F

Nodal load associated with third degree of freedom.

36-45

5th

F

Nodal load associated with fourth degree of freedom.

46-55

6th

F

Nodal load associated with fifth degree of freedom.

4th data block Enter a list of nodes having the point load given above. 5th data block Used only when 4th field of FOLLOW FOR parameter is 1. For the Nastran style follower force, enter as many lines as there are nodes in the 4th data block. 1-5

1st

I

0 = Fixed direction force -1 = Automated follower force

Main Index

POINT LOAD (Model Definition) 515 Define Nodal Point Loads

Format Fixed

Free

Data Entry Entry First node for Nastran style follower force

Main Index

6-10

2nd

I

Second node for Nastran style follower force

11-15

3rd

I

Third node for Nastran style follower force

16-20

4th

I

Fourth node for Nastran style follower force

516 HOLD NODES Neglect Incremental Displacement

HOLD NODES

Neglect Incremental Displacement

Description This model definition option indicates that the incremental displacement of the indicated nodes is to be neglected. This allows you to apply a load or displacement on the structure to generate a stress in the body without the displacements changing. In this way, an initial stress field may be generated. This option cannot be used with the multiplicative (FeFp) plasticity formulation (PLASTICITY, 5). At the end of the increment, this option is automatically deactivated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words HOLD NODES.

2nd data block 1-5

1st

I

Enter the number of sets of data.

6-10

2nd

I

Enter the unit number to read the data from.

I

Enter a list of degrees of freedom.

I

Enter a list of nodes for which the displacements will not be updated in this increment.

3rd data block 1-80

1st

4th data block 1-80

Main Index

1st

INERTIA RELIEF (Model Definition) 517 Define Inertia Relief

INERTIA RELIEF (Model Definition)

Define Inertia Relief

Description This option defines the parameters necessary for conducting an inertia relief analysis. The parameters are used to evaluate the Rigid Body Modes of the system. Once the modes are evaluated, the program evaluates the inertia relief load vector which balances the external load vector acting on the system. For more details of these procedures, you are referred to Inertia Relief in Chapter 5 in the Marc Volume A: Theory and User Information manual. When inertia relief is no longer active in a current loadcase, an option can be provided to remove or retain inertia relief loads from previous loadcases. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INERTIA RELIEF.

I

Flag for Rigid Body Mode evaluation method:

2nd data block 1-5

1st

0 - Inertia Relief is not active in current loadcase 3 - Support Method 6-10

2nd

I

Flag to retain/remove previous Inertia Relief Loading: 1 - retain load -1 - remove load immediately (default) -2 - remove load gradually

11-15 Note:

3rd

I

Number of Lines containing Support degree of freedom information (default 1)

Field 2 of data block 2 is only used if inertia relief is not active in the current loadcase (i.e., Field 1 of data block 2 is 0). Also, data block 3 is not necessary in this case.

Data block 3 is repeated as many times as specified in the 2nd data block, 3rd field. 3rd data block Use only if 1st field of 2nd data block is 3 (Support Method)

Main Index

1-5

1st

I

Node ID 1.

6-10

2nd

I

Degree of Freedom ID 1.

11-15

3rd

I

Node ID 2.

16-20

4th

I

Degree of Freedom ID 2.

518 INERTIA RELIEF (Model Definition) Define Inertia Relief

Format Fixed

Data Entry Entry

21-25

5th

I

Node ID 3.

26-30

6th

I

Degree of Freedom ID 3.

31-35

7th

I

Node ID 4.

36-40

8th

I

Degree of Freedom ID 4.

41-5

1st

I

Node ID 5.

46-10

2nd

I

Degree of Freedom ID 5.

51-55

3rd

I

Node ID 6.

56-60

4th

I

Degree of Freedom ID 6.

61-65

5th

I

Node ID 7.

66-70

6th

I

Degree of Freedom ID 7.

71-75

15th

I

Node ID 8.

76-80

16th

I

Degree of Freedom ID 8.

Note:

Main Index

Free

The degrees of freedom in fields 2, 4, etc. of data block 3 refer to the nodal degrees of freedom that define the rigid body motion (r-constraint set). The associated nodes are defined in fields 1,3, etc. The degrees of freedom that form part of the r-constraint set at any particular node can be specified in combined form (e.g., 123, 135, etc.). If all degrees of freedom at node N are to be part of this set, simply specify a negative number in the associated degrees of freedom field.

ROTATION A 519 Define Rotational Axis

ROTATION A

Define Rotational Axis

Description This option defines the rotation axis for centrifugal and/or Coriolis loading or for the STEADY STATE rolling option. This option is also used for steady state rolling analyses. The rotational speed is entered though the DIST LOADS option. Using an IBODY=100 or 104 results in centrifugal loading, using an IBODY=103 or 105 results in both centrifugal and Coriolis loading. If multiple rotation axis are supported for centrifugal and Coriolis loads, this all data blocks should be repeated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ROTATION A.

2nd data block 1-10

1st

F

11-20

2nd

F

21-30

3rd

F

31-35

4th

I

Direction cosines of the axis of rotation. Enter rotation axis ID; default is 1.

3rd data block

Main Index

1-10

1st

F

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

Global (x,y,z) coordinates of a point on the axis of rotation.

Velocity of the point on the axis of rotation, used for Coriolis loading only.

520 CORNERING AXIS Define Cornering Axis in Steady State Rolling Analysis

CORNERING AXIS

Define Cornering Axis in Steady State Rolling Analysis

Description This option defines the cornering axis for steady state rolling analysis. The cornering velocity is defined via the SS-ROLLING history definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CORNERING.

2nd data block 1-10

1st

F

First direction cosine of the cornering axis.

11-20

2nd

F

Second direction cosine of the cornering axis.

21-30

3rd

F

Third direction cosine of the cornering axis.

3rd data block

Main Index

1-10

1st

F

x coordinate of a point on the cornering axis.

11-20

2nd

F

y coordinate of a point on the cornering axis.

21-30

3rd

F

z coordinate of a point on the cornering axis.

FLUID DRAG 521 Define Fluid Drag

FLUID DRAG

Define Fluid Drag

Description This option defines parameters required for the evaluation of drag loads and buoyancy loads on beam type structures immersed in a fluid. The drag forces are defined by Morison’s equation. In static analyses, the fluid velocity is constant and defined here. In dynamic analyses, an additional contribution is added due to wave effects. Note:

In two dimensional analyses, the y-axis is considered vertically up, current is required only in x and y directions and the first direction cosine is either a one or minus one. In three dimensional analyses, the z-axis is considered vertically up. Those elements which require fluid drag must be indicated on the DIST LOADS option using a load type of 11. If an element is above the fluid surface, no drag or buoyancy is included.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FLUID DRAG.

2nd data block 1-10

1st

E

Enter the elevation of the sea bed.

11-20

2nd

E

Enter the surface elevation of the fluid outside the pipe.

21-30

3rd

E

Enter the surface elevation of the fluid inside the pipe.

31-40

4th

E

Enter the gravity constant.

41-50

5th

E

Enter mass density of fluid outside pipe.

51-60

6th

E

Enter mass density of fluid inside pipe.

61-70

7th

E

Enter the drag coefficient.

71-80

8th

E

Enter the inertia coefficient.

3rd data block

Main Index

1-10

1st

E

Current in x-direction.

11-20

2nd

E

Current in y-direction.

21-30

3rd

E

Current in z-direction.

31-40

4th

E

Gradient of x-current with elevation.

41-50

5th

E

Gradient of y-current with elevation.

522 FLUID DRAG Define Fluid Drag

Format Fixed 51-60

Free 6th

Data Entry Entry E

Gradient of x-current with elevation.

4th data block

Main Index

1-10

1st

E

Wave height.

11-20

2nd

E

Wave period.

21-30

3rd

E

Wave phase.

31-40

4th

E

First direction cosine in horizontal plane of wave front.

41-50

5th

E

Second direction cosine in horizontal plane of wave front.

CAVITY 523 Define Constants and Reference Values for Structures with Internal Cavities

CAVITY

Define Constants and Reference Values for Structures with Internal Cavities

Description This option allows you to enter the ambient pressure and ideal gas law exponent for structural analyses involving internal cavities. It also allows you to enter the reference gas pressure, temperature, and density for each cavity. When using the CAVITY option, the CAVITY parameter must also be included. (See Marc Volume A: Theory and User Information.) Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CAVITY.

2nd data block 1-10

1st

E

Ambient pressure. Default is 0.0.

11-20

2nd

E

Ideal gas law exponent. Default is 1.0.

Data block 3 is repeated for each cavity 3rd data block 1-5

1st

I

Cavity ID.

6-15

2nd

E

Gas reference pressure.

16-25

3rd

E

Gas reference temperature.

26-35

4th

E

Gas reference density.

36-40

5th

I

Cavity sign convention; used for shell and membrane elements: Set to 1 (default) if the signs of the cavity pressure and a positive element pressure are the same. Set to -1 if the signs of the cavity pressure and a positive element pressure are opposite. Note:

Main Index

The elements defining the cavity must be aligned.

524 PRE STATE Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

PRE STATE

Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

Description In a general multi-stage analysis, previous analysis results are often required as the initial state for the new analysis. The PRE STATE option includes the capability of the existing AXITO3D option to allow the transfer of data in a result file to the new analysis. This capability includes data transfer from a 2-D axisymmetric analysis to a 3-D analysis, from a 2-D plane strain analysis to a 3-D analysis, or simply data transfer to the same type of analysis. If, in the previous analysis, there are multiple deformable contact bodies, the PRE STATE option allows the user to specify which contact bodies in the previous analysis need the data transfer, by providing a list of contact body names. The PRE STATE option replaces the existing AXITO3D option. In order to have a correct data transfer, the following should be observed: 1. Correct data in the previous result file: For large strain metal plasticity, this would include at least stress (post code 311) and equivalent plastic strain (post code 7). For plasticity procedure using multiplicative elastic-plastic decomposition, total strain tensor (post code 301) and plastic strain tensor (post code 321) are required. For updated Lagrange rubber elasticity, strain (post code 301) and stress (post code 311) are needed. For an analysis involving temperature, thermal strain (post code 371) and temperature (post code 9) are required. Creep strain (post code 331) and equivalent creep strain (post code 37), velocity and acceleration are needed for a creep and dynamic analysis, respectively. Nodal displacement can be transferred as well as nodal velocity and acceleration but it should be consistent with the previous model. If the current model is created based on the original mesh in the previous model, nodal displacement should be included in the transfer. If the current model is created based on the final mesh, such as in the case of global remeshing, the nodal displacement should not be included in the transfer. By default, if total Lagrange procedure is used in the current model, nodal displacement is transferred. Therefore, in this case, it is important to create the model based on the initial mesh in the previous model. Nodal temperature is transferred by default in the thermal-mechanical coupled analysis. If the temperature at the integration points is required in the current model but not stored in the previous result file, nodal temperature is used instead. 2. Compatible analysis types In the current release, only 2-D plane strain to 3-D model and 2-D axisymmetric to 3-D model are supported in the 2-D to 3-D transfer. 2-D to 2-D and 3-D to 3-D transfer are based on the same mesh model. Not all the element types are supported in the analysis with the PRE STATE option as stated below. 3. Compatible element types It is important to select the correct element types compatible with the previous model for a 2-D to 3-D transfer. For the same element type transfer, not all the element types are supported. For axisymmetric to 3-D transfer, supported element types are:

Main Index

PRE STATE 525 Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

10 -> 7

20 -> 7

82 -> 84

83 -> 84

28 -> 21

67 -> 21

33 -> 35

66 -> 35

55 -> 57

59 -> 61

48 -> 23

142 -> 23

144 -> 146

145 -> 146

For 2-D plane strain to 3-D solid elements, supported elements types are: 11 -> 7

80 -> 84

19 -> 7

81 -> 84

27 -> 21

32 -> 35

29 -> 21

34 -> 35

For 2-D to 2-D and 3-D to 3-D transfer, the following element types are tested and supported: 7, 157, 10, 11, 19, 20 4. Compatible PRE STATE models and mesh numbering During the PRE STATE history data transfer, a list of contact bodies is transferred from a result file. If this is not a 2-D to 3-D conversion, the elemental data and nodal data are copied to the current model providing the elements and nodes within the bodies are matched. Element and nodal numbering sequence within the bodies should be continuous and in the same order although the numbers may not be the same. For 2-D to 3-D transfer, the mesh expansion is based on the method that Marc Mentat uses – that is, each base element in 2-D is expanded with number of repetitions in z-direction or around x axis in the axisymmetric to 3-D case. The element numbering follows each element expansion. If the new mesh in 3-D is not generated in such manner, the data transfer will be incorrect. For axisymmetric to 3-D, if MD Patran is used to generate the 3-D mesh, this can be specified in the input. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PRE STATE

I

Analysis Type in the previous model

2nd data block 1-5

Main Index

1st

526 PRE STATE Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

Format Fixed

Free

Data Entry Entry = 1 plane stress (not supported) = 2 plane strain = 3 axisymmetric = 4 3-D

6-10

2nd

I

Analysis Type in the current model = 1 plane stress (not supported) = 2 plane strain = 3 axisymmetric = 4 3-D

11-15

3rd

I

Enter the number of repetitions in 3-D expansion direction. Used only for axisymmetric to 3-D or plane strain to 3-D transfer. Default = 0.

16-20

4th

I

Increment to read from post file. -1 The last increment on the post file. -2 Input the time to read the post file at 3rd data block.

21-25

5th

I

Unit number from which the post file is read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

26-30

6th

I

Enter 0 for binary post file. Enter 1 for formatted post file.

31-35

7th

I

Enter 1 to move stress tensor (post code 311).

36-40

8th

I

Enter 1 to move equivalent plastic strain (post code 7).

41-45

9th

I

Enter 1 to move temperatures (post code 9 or 180).

46-50

10th

I

Enter 1 to move strain tensor (post code 301).

51-55

11th

I

Enter 1 to move plastic strain tensor (post code 321).

56-60

12th

I

Enter 1 to move thermal strain tensor (post code 371).

61-65

13th

I

Enter 1 to move creep strain tensor (post code 331).

66-70

14th

I

Enter 1 to move equivalent creep strain (post code 37).

71-75

15th

I

Enter 1 to move displacements, (as well as velocity and acceleration in a dynamic analysis). If total Lagrangian formulation is used in the analysis, the number is set to 1 by Marc. Displacements are always moved. In this case, the mesh of the data transfer body in the new model must be generated based on the undeformed model. Enter 0 if the new mesh is generated based on the deformed mesh in the previous model and the updated Lagrange is used in the analysis.

Main Index

PRE STATE 527 Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

Format Fixed

Free

Data Entry Entry = 1 plane stress (not supported) = 2 plane strain = 3 axisymmetric = 4 3-D

6-10

2nd

I

Analysis Type in the current model = 1 plane stress (not supported) = 2 plane strain = 3 axisymmetric = 4 3-D

11-15

3rd

I

Enter the number of repetitions in 3-D expansion direction. Used only for axisymmetric to 3-D or plane strain to 3-D transfer. Default = 0.

16-20

4th

I

Increment to read from post file. -1 The last increment on the post file. -2 Input the time to read the post file at 3rd data block.

21-25

5th

I

Unit number from which the post file is read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

26-30

6th

I

Enter 0 for binary post file. Enter 1 for formatted post file.

31-35

7th

I

Enter 1 to move stress tensor (post code 311).

36-40

8th

I

Enter 1 to move equivalent plastic strain (post code 7).

41-45

9th

I

Enter 1 to move temperatures (post code 9 or 180).

46-50

10th

I

Enter 1 to move strain tensor (post code 301).

51-55

11th

I

Enter 1 to move plastic strain tensor (post code 321).

56-60

12th

I

Enter 1 to move thermal strain tensor (post code 371).

61-65

13th

I

Enter 1 to move creep strain tensor (post code 331).

66-70

14th

I

Enter 1 to move equivalent creep strain (post code 37).

71-75

15th

I

Enter 1 to move displacements, (as well as velocity and acceleration in a dynamic analysis). If total Lagrangian formulation is used in the analysis, the number is set to 1 by Marc. Displacements are always moved. In this case, the mesh of the data transfer body in the new model must be generated based on the undeformed model. Enter 0 if the new mesh is generated based on the deformed mesh in the previous model and the updated Lagrange is used in the analysis.

Main Index

528 PRE STATE Transfer History Data from Previous Analysis to the Current Analysis as the Initial State

Format Fixed

Free

Data Entry Entry Enter 1 to move displacements If the new mesh is generated based on the initial configuration in the previous model.

76-80

16th

I

Enter 0 if the standard Marc Mentat numbering is used (default). Enter 1 if the position based mapping is required.

The 3rd data block is needed only if the 4th field of the 2nd data block is -2. 3rd data block 1-10

1st

F

Enter the time to read the post file.

4th data block 1-5

1st

I

Enter the number of contact bodies in data transfer. Default = 0, in this case all the elements in the previous model are transferred.

6-10

2nd

I

Enter 1 for rigid body rotation (not supported).

The 5th data block is required only when the first field of 4th data block is not zero. Repeat 5th data block for all contact names defined in the first field of the 4th data block. 5th data block 1-24

Main Index

1st

A

Enter contact body name in the previous model for data transfer.

AXITO3D (Model Definition) 529 Transfer Data from Axisymmetric Analysis to 3-D Analysis

AXITO3D (Model Definition)

Transfer Data from Axisymmetric Analysis to 3-D Analysis

Description In certain cases, it is possible to begin a numerical simulation using a 2-D axisymmetric model, even though the final problem is fully 3-D. Splitting the simulation in an axisymmetric and a 3-D part might be advantageous because of considerable computational savings, provided that there is an efficient data transfer from the axisymmetric to the 3-D model. The AXITO3D option is used in the input file of the 3D problem to import results of an axisymmetric analysis into a 3-D analysis. Since the results from the axisymmetric analysis are imported from the post file, care must be taken to write the appropriate data on the post file during the axisymmetric analysis. For example, for large strain metal plasticity, this would include at least stress (post code 311) and equivalent plastic strain (post code 7). For updated Lagrange rubber elasticity, strain (post code 301) and stress (post code 311) are needed. For an analysis involving temperature, thermal strain (post code 371) and temperature (post code 9) are required. Creep strain (post code 331) and equivalent creep strain (post code 37), velocity and acceleration are needed for a creep and dynamic analysis, respectively. The AXITO3D option can be used for most quadrilateral axisymmetric continuum elements. The following table shows the correlation between element types.

Main Index

Axisymmetric

3-D Solid

10

7

20

7

82

84

83

84

28

21

67

21

33

35

66

35

55

57

59

61

48

23

142

23

144

146

145

146

166

147

167

147

169

148

170

148

530 AXITO3D (Model Definition) Transfer Data from Axisymmetric Analysis to 3-D Analysis

The external applied load and displacement boundary conditions are transferred from the axisymmetric analysis to 3-D analysis using the table curve shift feature in Marc Mentat. This option cannot be used for beams, composites, and triangular elements.

There are three steps required to perform these types of analysis using Marc Mentat. 1. Perform axisymmetric analysis: a. Create axisymmetric model using Marc Mentat. b. Save the created model; for example, into stage_axi.mud. c. Run axisymmetric model and keep post file (stage_axi_job1.t16 or stage_axi_job1.t19). 2. Create 3-D model using Marc Mentat. a. Open axisymmetric model stage_axi.mud. b. Expand axisymmetric mesh to 3-D model via: MESH GENERATION→EXPAND→AXSYMMETRIC MODEL TO 3D and move the rigid

surfaces, if any, to the deformed configuration. c. Define data transfer parameters via: INITIAL CONDITIONS→MECHANICAL→AXSYMMETRIC-3D

d. Add additional model data such as contact surfaces if necessary. e. Save the created model with a different name to avoid overwriting the existing stage_axi.mud; for example, into stage_3d.mud. 3. Run 3-D model. Note:

(1) In the axisymmetric model, the node and element numbering have to start at 1 and have to be consecutive. (2) If a 3-D analysis is run outside of Marc Mentat, use the -pid command line option to read in a post file of axisymmetric analysis. For example, to submit a 3-D analysis, use the command: marc -j stage_3d_job1 -pid stage_axi_job1

(3) If remeshing/rezoning steps are performed in the axisymmetric analysis, the original mesh in the model is replaced by a new mesh. The 3-D analysis starts based on the deformed configuration. To replace step 2-a above, do the following: i. Open post file stage_axi.t16 (or stage_axi.t19) ii. Position to the desired increment. iii. Rezone. iv. Save the model to stage_3d.mud.

Main Index

AXITO3D (Model Definition) 531 Transfer Data from Axisymmetric Analysis to 3-D Analysis

v. Close post file. vi. Open stage_3d.mud. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word AXITO3D.

2nd data block 1-5

1st

I

Not used.

6-10

2nd

I

Not used.

11-15

3rd

I

Enter the number of repetitions in θ direction.

16-20

4th

I

Increment to read off post file. -1

The last increment on the post file of an axisymmetric job (default).

-2

Input the time to read the post file at 3rd data block.

21-25

5th

I

Unit number from which the post file is read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

26-30

6th

I

Enter 0 for binary post file. Enter 1 for formatted post file.

31-35

7th

I

Enter 1 to move stress tensor (post code S).

36-40

8th

I

Enter 1 to move equivalent plastic strain (post code 7).

41-45

9th

I

Enter 1 to move temperatures (post code 9 or 180).

46-50

10th

I

Enter 1 to move strain tensor (post code 301).

51-55

11th

I

Enter 1 to move plastic strain tensor (post code 321).

56-60

12th

I

Enter 1 to move thermal strain tensor (post code 371).

61-65

13th

I

Enter 1 to move creep strain tensor (post code 331).

66-70

14th

I

Enter 1 to move equivalent creep strain (post code 37).

71-75

15th

I

Enter 1 to move displacements, (as well as velocity and acceleration in a dynamic analysis). If total Lagrangian formulation is used in the analysis, the number is set to 1 by Marc. Displacements are always moved. In this case, the 3-D mesh must be generated based on the undeformed axisymmetric mesh.

Main Index

532 AXITO3D (Model Definition) Transfer Data from Axisymmetric Analysis to 3-D Analysis

Format Fixed

Free

Data Entry Entry If updated Lagrange is used in the analysis, enter 0 if the 3-D mesh is generated based on the deformed axisymmetric mesh. If the 3-D mesh is generated based on the original axisymmetric mesh, enter 1 to move displacements.

76-80

16th

I

Enter 1 if the 3-D mesh is not generated by Marc Mentat.

The 3rd data block is needed only if the 4th field of the 2nd data block is -2. 3rd data block 1-10

Main Index

1st

F

Enter the time to read the post file.

GLOBALLOCAL 533 Structural Zooming Analysis

GLOBALLOCAL

Structural Zooming Analysis

Description This option defines control parameters and a list of local nodes connecting to the global model in a structural zooming analysis. In order to achieve a better evaluation of the local gradients in the solution, a re-analysis of the model with some local variations may be needed. These variations may be due to changes in model geometry or in the finite element mesh. However, in cases that these local changes have negligible influence on the solution a certain distance away from the changes, it is computationally more efficient to model only the local changes and the vicinity affected. This can be accomplished by applying the existing loads and/or boundary conditions in the local model along with properly defined kinematic conditions to the local boundaries connecting to the global model. A typical Marc structural zooming analysis contains two steps: 1. Global run to obtain global results and a post file containing these results. 2. Local run to define kinematic boundary conditions in the local model and to obtain refined results in the local model. This procedure can be repeated as many times as desired. Any local analysis can be the global analysis of a subsequent refinement analysis. The GLOBALLOCAL option is used in the input of the local run to define the list of nodes connecting to the global model. Marc calculates the deformation (temperature) history of these nodes based on their locations in the global model and on the solution of the global analysis. The obtained deformation (temperature) history is then applied to the nodes as prescribed kinematic boundary conditions. The detailed steps include: a. Reading in the GLOBALLOCAL option to get the list of connecting nodes. b. Reading in the global model (element types, node coordinates, element connectivity, thickness if shell elements) and solution of the model from the previously generated post file of the global run. c. Finding the locations of local connecting nodes in the global model (the element each node is associated with and its isoparametric location within the element). d. Calculating the deformation (temperature) of each connecting node for every increment available in the global post file based on its location in the global elements associated using the interpolation techniques, and store the deformation (temperature) history in the format of time-dependant tables. e. Applying the deformation (temperature) history of the connecting nodes to the local model as prescribed kinematic boundary conditions. All the above steps are performed automatically inside Marc once the GLOBALLOCAL option is used in the input file of the local run.

Main Index

534 GLOBALLOCAL Structural Zooming Analysis

Factors to Consider in Global Analysis In the global analysis, it is a good idea to write the entire global model into the post file. The post file should contain, at least, nodal displacements for mechanical analyses or nodal temperatures for heat transfer analysis, or both for thermal-mechanical coupled analyses. If there are shell elements in the model, the shell thickness at each integration point (i.e., post code 20) should also be written into the post file. In order to form an accurate deformation (temperature) history of the connecting nodes in the local run, it is recommended that the results of all increments be put onto the post file. Smaller increment size (therefore, more increments) in the post file leads to a more accurate deformation (temperature) history of connecting nodes. The time scale in the global analysis must be the same as that of local analysis. It is recommended that the time range used in the local run [ 0, t l o ca l ] be equal to or less than the time range in the global run [ 0, t gl obal ] ; i.e., t local ≤ t globa l . If t local > t g lo bal , the extrapolation option defined in the 4th field of the 2nd data block of the GLOBALLOCAL option can be used. Element Types Supported The global to local modeling can be used in the following four cases: Global Model

Local Model

2-D Solid

2-D Solid

3-D Solid

3-D Solid

3-D Shell/Membrane

3-D Shell/Membrane

3-D Shell/Membrane

3-D Solid

Limitations The local run must be based on a single, continuous global post file. Therefore, if restart had been employed during the global analysis, a complete post file for the global analysis must be properly generated. This is also true if the global analysis is performed with DDM. Adaptive remeshing can be used in global but not in local runs. The element types not supported includes all rebar element types, all 1-D element types (truss, beam axisymmetric shell), all special element types (gap, semi-infinite …) and nonconventional shell types (type 4, 8, 24, 49, 68, and 72). In the current release, the feature does not support magnetostatic, fluid-solid or harmonic analysis.

Main Index

GLOBALLOCAL 535 Structural Zooming Analysis

Note:

If the local analysis is run outside of Marc Mentat, use the -pid command line option to read in the post file of global analysis. For example, to submit a local analysis, use the command line: marc -j local_model -pid global_model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the word GLOBALLOCAL.

I

Enter the number of geometry types

2nd data block 1-5

1st

(see the 3rd and the 4th data block). Default is 1. 5-10

2nd

I

= 0 if read in a binary global post file = 1 if read in a formatted global post file.

11-15

3rd

F

Exterior tolerance; used to find the associated global element for a connecting node. Default is 0.05. A connecting node is considered within a global element if the distance between the node and the element is smaller than the tolerance times the corresponding element edge length, unless the node is actually inside another global element.

16-20

4th

I

= 0 exit if the local run time range exceeds the global post file time range. = 1 use end value if the local run time range exceeds the global post file time range. = 2 use extrapolation if the local run time range exceeds the global post file time range.

26-35

5th

F

Timeshift. Global results will be taken at Local time + Timeshift. Default ID 0.d0. Timeshift cannot be negative.

The 3rd and 4th data blocks are repeated in pairs for as many geometry types as specified in the 1st field of the 2nd data block.

Main Index

536 GLOBALLOCAL Structural Zooming Analysis

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter the geometry types 2: Nodes 4: Surface IDs 5: Curve IDs 6: Point IDs Default is 2.

4th data block Enter the list of geometry entities, which must all be of the type prescribed in the 3rd data block.

Main Index

INIT STRESS (with TABLE Input) 537 Define Initial Stress

INIT STRESS (with TABLE Input)

Define Initial Stress

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define initial stresses and associate them with an initial condition name. These initial conditions will be activated using the LOADCASE model definition option. It is your responsibility to input a self-equilibrating set of stresses. These stresses should not produce any material nonlinearity. As an alternative, the UINSTR user subroutine can be used. To obtain the initial stress from the calculated value of a previous analysis, use the PRE STATE option. Notes:

It is not recommended to use the CENTROID parameter with initial stresses because the residual load cannot be accurately calculated. For shells and beams, these are the real physical stress, not the generalized stresses. The stresses entered should be in the element coordinate system and not the preferred material coordinate system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INIT STRESS.

2nd data block 1-5

1st

I

Number of sets of initial stress data to be entered (optional)

6-10

2nd

I

Unit number for input of initial stress data. Defaults to input file.

The 3rd through 7th data blocks are repeated once for each data set. The components of stress are given in the order described for each element type in Marc Volume B: Element Library. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine is required. Enter 1 if the UINSTR user subroutine is used.

11-15

Main Index

3rd

I

Not used; enter 0.

538 INIT STRESS (with TABLE Input) Define Initial Stress

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Enter the first component of stress.

11-20

2nd

F

Enter the second component of stress.

21-30

3rd

F

Enter the third component of stress.

31-40

4th

F

Enter the fourth component of stress.

41-50

5th

F

Enter the fifth component of stress.

51-60

6th

F

Enter the sixth component of stress.

61-70

7th

F

Enter the seventh component of stress.

5th data block 1-5

1st

F

Table ID associated with the first component of stress.

6-10

2nd

F

Table ID associated with the second component of stress.

11-15

3rd

F

Table ID associated with the third component of stress.

16-20

4th

F

Table ID associated with the fourth component of stress.

21-25

5th

F

Table ID associated with the fifth component of stress.

26-30

6th

F

Table ID associated with the sixth component of stress.

31-35

7th

F

Table ID associated with the seventh component of stress.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 - Element IDs 3 - Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

INIT STRESS 539 Define Initial Stress

INIT STRESS

Define Initial Stress

The information provided here is based upon not using the table driven input style. Description Option A allows the user to enter initial stresses into the model. It is the user’s responsibility to input a self-equilibrating set of stresses. These stresses should not produce any material nonlinearity. As an alternative, the UINSTR user subroutine can be used. For analysis that involves the machining capability of Marc, there exists another option (Option B) to input the initial stress. Option B allows users to have the initial stress data stored in a data file. The data file is in ASCII text format. Notes:

It is not recommended to use the CENTROID parameter with initial stresses because the residual load cannot be accurately calculated. For shells and beams, these are the real physical stress, not the generalized stresses. The stresses entered should be in the element coordinate system and not the preferred material coordinate system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INIT STRESS.

2nd data block 1-5

1st

I

Number of sets of initial stress data to be entered (optional)

6-10

2nd

I

Unit number for input of initial stress data. Defaults to input file.

10-15

3rd

I

Enter 1 if there exists initial stress data stored in an ASCII data file. (Default is set to 0.) Note:

This option only works in combination with the MACHINING parameter. In the current version of Marc, the only element types supported are: 7, 117, and 134.

The 3rd, 4th, 5th, and 6th (and, if necessary, 7th) data blocks are repeated once for each data set. The components of stress are given in the order described for each element type in Marc Volume B: Element Library.

Main Index

540 INIT STRESS Define Initial Stress

Format Fixed

Free

Data Entry Entry

Option A Option A is only necessary if the third field of the 2nd data block is set to 0. In this case, the 3rd, 4th, 5th, and 6th data blocks are repeated once for each data set. 3rd data block 1-10

1st

F

Enter the first component of stress.

11-20

2nd

F

Enter the second component of stress.

21-30

3rd

F

Enter the third component of stress.

31-40

4th

F

Enter the fourth component of stress.

41-50

5th

F

Enter the fifth component of stress.

51-60

6th

F

Enter the sixth component of stress.

61-70

7th

F

Enter the seventh component of stress.

I

Enter a list of elements for which initial stress prescribed above is applied.

4th data block 1-80

1st

5th data block Only necessary if CENTROID parameter is not used. 1-80

1st

I

Enter a list of integration points for which the initial stresses are applied.

6th data block Only necessary for shell or beam analysis. 1-80

1st

I

Enter a list of layers for which the initial stress is prescribed.

Option B Option B is necessary only if the third field of the 2nd data block is set to 1. In this case, the 3rd, 4th, 5th, 6th, and 7th data blocks are repeated once for each data set. 3rd data block 1-5

1st

I

Enter 0 if the residual stress data is not defined by a text data file. Enter 1 to 3 if the stress data is given in a separate text data file.

6-80

2nd

A

1

if stresses are defined in one direction only (1-D space).

2

if stresses are defined in 2-D space.

3

if stresses are defined in 3-D space.

Enter the name of text file that contains the initial stress data if the first field is set to 1, 2, or 3.

4th data block (If the first field of the 3rd data block is set to 0.)

Main Index

1-10

1st

F

Enter the first component of stress.

11-20

2nd

F

Enter the second component of stress.

INIT STRESS 541 Define Initial Stress

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Enter the third component of stress.

31-40

4th

F

Enter the fourth component of stress.

41-50

5th

F

Enter the fifth component of stress.

51-60

6th

F

Enter the sixth component of stress.

61-70

7th

F

Enter the seventh component of stress.

4th data block (If the first field of the 3rd data block is set to 1, 2, or 3.) 1-10

1st

F

Enter the first component of base vector, V1.

11-20

2nd

F

Enter the second component of base vector, V1.

21-30

3rd

F

Enter the third component of base vector, V1.

31-40

4th

F

Enter the first component of base vector, V2.

41-50

5th

F

Enter the second component of base vector, V2.

51-60

6th

F

Enter the third component of base vector, V2. Note:

In case of 1-D or 2-D, the primary axes are V1 and V2; if 3-D, the primary axes are V1, V2, and V3. Here, V3 is defined by the cross product of V1 and V2.

5th data block 1-80

1st

I

Enter a list of elements for which initial stress prescribed above is applied.

6th data block Only necessary if CENTROID parameter is not used. 1-80

1st

I

Enter a list of integration points for which the initial stresses are applied.

7th data block Only necessary for shell or beam analysis. 1-80

1st

I

Enter a list of layers for which the initial stress is prescribed.

ASCII Text Data Format This ASCII text data format is used in a separate text file as defined by input Option B when the first field of the 3rd data block is set as nonzero. 1st data block 1st

Main Index

I

Enter the total number of points (optional).

542 INIT STRESS Define Initial Stress

Format Fixed

Free

Data Entry Entry

2nd data block 1st

F

First coordinate of starting point of the coordinate system defined in the ASCII text file.

2nd

F

Second coordinate of starting point of the coordinate system defined in the ASCII text file.

3rd

F

Third coordinate of starting point of the coordinate system defined in the ASCII text file.

3rd and 4th data blocks are repeated for each point till the end of the file. 3rd data block 1st

F

Enter the first coordinate component of the point.

2nd

F

Enter the second coordinate component of the point.

3rd

F

Enter the third coordinate component of the point.

1st

F

Enter the first component of stress.

2nd

F

Enter the second component of stress.

3rd

F

Enter the third component of stress.

4th

F

Enter the fourth component of stress.

5th

F

Enter the fifth component of stress.

6th

F

Enter the sixth component of stress.

4th data block

Main Index

INITIAL PLASTIC STRAIN (with TABLE Input) 543 Define Initial Strain

INITIAL PLASTIC STRAIN (with TABLE Input)

Define Initial Strain

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define potential initial plastic strains, and associate them with an initial condition name. The initial condition is activated using the LOADCASE model definition option. Occasionally, in metal forming analysis, it is required to define the previous amount of equivalent plastic strain. This history dependent variable represents the amount of plastic deformation that the model was subjected to, and is used in the work (strain) hardening model. Initial Plastic Strain may be used in three different ways with the new table input format. Method 1 is when data is directly input. While not explicitly stated, the data can always be a function of a table, where the independent variables are, e.g., positioned to allow a nonhomogeneous field. Method 2 is based upon reading the plastic strain from a post file created in a previous stress analysis. Method 3 is using INITPL user subroutine to define initial plastic strain variables. 1. Read the range of elements, integration points and layers and a corresponding value. 2. Read the initial values from a step of the post output file from a previous analysis with Marc. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 3. Read the initial values through the INITPL user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INIT PLASTIC STRAIN. Number of sets of initial plastic

2nd data block 1-5

1st

I

6-10

2nd

I

stain data to be entered (optional) Unit number for input of initial plastic stain data. Defaults to input file.

3rd data block

Main Index

1-5

1st

I

Not used: enter 0.

6-10

2nd

I

Enter the method:

544 INITIAL PLASTIC STRAIN (with TABLE Input) Define Initial Strain

Format Fixed

Free

Data Entry Entry 3 - use binary post file 5 - use ASCII post file 6 - use data lines (default) 7 - use the INITPL user subroutine.

11-15

3rd

I

If method 3 or 5, enter the step number to read. If method 6, enter the number of geometric types used to define this boundary condition.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

A

Enter unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

4th data block (Used only if method = 6 or 7) 1-10

1st

F

Enter the first magnitude of the initial equivalent plastic strain.

5th data block (Used only if method = 6 or 7) 1-5

1st

F

Table ID associated with the initial equivalent plastic strain.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd field of the 2nd data block (only used if method = 6 or 7). 6th data block 1-5

1st

I

Enter the geometry type: 1 - Element IDs 3 - Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be al the type prescribed in the 6th data block.

INITIAL PLASTIC STRAIN 545 Define Initial Plastic Strain

INITIAL PLASTIC STRAIN

Define Initial Plastic Strain

The information provided here is based upon not using the table driven input style. Description This option allows you to define potential initial plastic strains. and associate them with an initial condition name. The initial condition is activated using the LOADCASE model definition option. Occasionally, in metal forming analysis, it is required to define the previous amount of equivalent plastic strain. This history dependent variable represents the amount of plastic deformation that the model was subjected to, and is used in the work (strain) hardening model. Four ways of specifying the initial equivalent plastic strain values are shown below: • Read the range of elements, integration points and layers and a corresponding value. • Read the initial values through user subroutine INITPL. • Read the initial values from a step of the post output file from a previous analysis with Marc.

With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. • Read a list of elements, integration points and layers and a corresponding value.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PLASTIC STRAIN.

2nd data block 1-5

1st

I

Not used, enter 0.

6-10

2nd

I

Enter 1 to initialize the equivalent plastic strain via the 3rd and 4th data blocks below. In this case, the third field must also be defined. Enter 2 to initialize the equivalent plastic strain via the INITPL user subroutine. This subroutine is now called in a loop over all elements in the mesh. Enter 3 to read the initial values of the equivalent plastic strain from the post file written by a previous analysis. In this case, the fourth and fifth field must also be defined. Enter 4 to initialize the equivalent plastic strain via the 5th, 6th, 7th, and 8th data blocks shown below. See also the third field on this block.

Main Index

546 INITIAL PLASTIC STRAIN Define Initial Plastic Strain

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. Then this entry gives the number of pairs of data blocks in series 3 and 4 or in series 5, 6, 7 8 used to input the equivalent plastic strain. Defaults to 1.

16-20

4th

I

Only used if the second field is set to 3. Then this entry defines the unit number from which the post file information from the previous run is to be read.

21-25

5th

I

Only used if the second field is set to 3. In that case, this entry defines the step number of the previous analysis.

26-30

6th

31-35

7th

I

Set to 1 if option 3 is used, and a formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2. Set to 1 to suppress printout of equivalent plastic strains values that are initialized in INITPL.

Not used, enter 0.

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of sets is equal to the number given in the third field above. 3rd data block 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with this value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value.

21-25

5th

I

First layer of cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value can only be bigger than 1 for beam or shell elements.

F

Initial value of the equivalent plastic strain for the above range of points.

4th data block 1-10

1st

Data blocks 5, 6, 7, and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

Initial value of the equivalent plastic strain at zeroth increment.

6th data block Enter a list of elements to which the above value is applied. 7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above value is applied.

Main Index

INITIAL PLASTIC STRAIN 547 Define Initial Plastic Strain

Format Fixed

Free

Data Entry Entry

8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above value is applied.

Main Index

548 INITIAL STATE (with TABLE Input) Initialize State Variables

INITIAL STATE (with TABLE Input)

Initialize State Variables

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define potential initial state variables and associate them with an initial condition name. The initial condition is activated using the LOADCASE model definition option. The number of state variables per integration point is defined in the STATE VARS parameter. The default is one, with temperature always being the first state variable at an integration point. If more than one state variable per integration point has been assigned, this option can be used repeatedly to initialize all the state variables. The default value of state variables not initialized is zero. Initial State may be used in three different ways with the new table input format. Method 1 is when data is directly input and not read from a post file. While not explicitly stated, the data can always be a function of a table, where the independent variables are position to allow a nonhomogeneous field. They may also be a function of time, but will be evaluated at time equals zero. Method 2 is based upon reading the state variable from a post file created in a previously generated heat transfer analysis. 1. The initial value is the value entered here including the evaluation of the table. 2. The initial state variable is obtained by reading in a single increment from the post file. Only a single increment is read in. 3. The INITSV user subroutine is used to define the initial state variables. Notes:

The Fourier series number is not applicable to the methods where the initial conditions are read from the post file. The Fourier series number is not supported in Version 2005. Initial temperature values read in by this option are assumed to define the stress-free temperature field. Temperature changes which cause thermal strains are read in through the CHANGE STATE options. In a coupled analysis, the temperatures are not independent state variables and the INITIAL TEMP option must be used.

Main Index

INITIAL STATE (with TABLE Input) 549 Initialize State Variables

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL STATE.

2nd data block 1-5

1st

I

Enter the number of sets of data (not required).

6-10

2nd

I

Enter the unit number to read data.

I

Enter the state variable identifier

3rd data block 1-5

1st

(1 for temperature). Enter -1 if multiple state variables are read from a post file. In this case, the 8th data block is also required. 6-10

2nd

I

Enter the method: 3 - use binary post file 5 - use ASCII post file 6 - use data lines (default) 7 - use the INITSV user subroutine.

11-15

3rd

I

If method 3 or 5, enter the step number to read. If method 6, enter the number of geometric types used to define this boundary condition.

16-20

4th

I

Enter the Fourier Series Number

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used, enter 0.

31-35

7th

A

Enter boundary condition label.

4th data block (Used only if method = 6 or 7) 1-10

1st

E

Enter the magnitude of the initial state variable.

5th data block (User only if method = 6 or 7) 1-10

1st

I

Enter the table ID associated with the initial state variable.

The 6th and 7th data blocks are repeated for as many geometric types as specified in the in the third field of the 2nd data block (only used if method = 6 or 7).

Main Index

550 INITIAL STATE (with TABLE Input) Initialize State Variables

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1 - Element IDs 3 - Volume/Region/Body ID

7th data block 1-80

Enter a list of geometric entities to which the above initial condition are applied. All the geometric entities must be of the type prescribed in the 6th data block.

The 8th data block is required only if multiple state variables are read from a post file if the first field of the 3rd data block is -1. 8th data block 1-80

Main Index

I

Enter a list of state variables.

INITIAL STATE 551 Initialize State Variables

INITIAL STATE

Initialize State Variables

The information provided here is based upon not using the table driven input style. Description This option provides various ways of initializing the state variables throughout the model. The number of state variables per integration point is defined in the STATE VARS parameter. The default is one, with temperature always being the first state variable at an integration point. If more than one state variable per integration point has been assigned, this option can be used repeatedly to initialize all the state variables. The default value of state variables not initialized is zero. Four ways of providing the state variable initial values are shown below: •

Read the range of elements, integration points and layers and a corresponding state variable value.

• Read the initial values through the INITSV user subroutine. • Read the initial values from a step of the binary or formatted post output file from a previous

heat transfer analysis with Marc. This technique is most common for thermal stress analysis to initialize temperature (the first state variable at any point). With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. • Read a list of elements, integration points and layers and a corresponding state variable value.

Note:

Initial temperature values read in by this option are assumed to define the stress-free temperature field. Temperature changes which cause thermal strains are read in through the CHANGE STATE or AUTO THERM options. In a coupled analysis, the temperatures are not independent state variables and the INITIAL TEMP option must be used.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

Main Index

1st

A

Enter the words INITIAL STATE.

552 INITIAL STATE Initialize State Variables

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter the state variable IDentifier for the state variable being set (1,2,etc.). 1=temperature. If more than one state variable is being used, the STATE VARS parameter must be included. Enter -1 if multiple state variables are read from a post file. In this case, the 9th data block is also required.

6-10

2nd

I

Enter 1 to initialize the state variable via the 3rd and 4th data block below. See also the third field on this data block. Enter 2 to initialize the state variable via the INITSV user subroutine. This subroutine is now called in a loop over all elements in the mesh. Enter 3 to read the file values of the state variable from the post file written by a previous heat transfer analysis. In this case, the fourth and fifth fields must also be defined. Enter 4 to initialize the state variable via the 5th, 6th, 7th, and 8th data blocks as given below. Also, see the third field on this data block.

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. Then this entry gives the number of pairs of data blocks in series 3 and 4 or in series 5, 6, 7, and 8 used to input the state variable.

16-20

4th

I

Only used if the second field is set to 3. Then this entry defines the unit number from which the post file information from the previous heat transfer run is to be read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

21-25

5th

I

Only used if the second field is set to 3. In that case, this entry defines the increment number on the heat transfer run post file to be used as the definition of the initial state variable values.

26-30

6th

31-35

7th

I

Set to 1 if option 3 is used, and a formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2. Set to 1 to suppress printout of state variable values that are initialized in the INITSV user subroutine.

41-45

9th

I

Enter the post code number to be read into this state variable, default is 9 (temperature).

Not used, enter 0.

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of sets is equal to the number given in the third field above. 3rd data block

Main Index

1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with the value.

INITIAL STATE 553 Initialize State Variables

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value.

21-25

5th

I

First layer of cross section point with this value.

26-30

6th

I

Last layer or cross section point with this value can only be bigger than 1 for beam or shell elements.

F

Initial value of this state variable for the above range of points.

4th data block 1-10

1st

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

New total value of this state variable for the points given below at the start of the zeroth increment.

6th data block Enter a list of elements to which the above state variable is applied. 7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above state variable is applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above state variable is applied.

Main Index

554 CHANGE STATE (with TABLE Input - Model Definition) Redefine State Variables

CHANGE STATE (with TABLE Input - Model Definition)

Redefine State Variables

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to potentially define the state variables. and associate them with a boundary condition name. The boundary condition is activated using the LOADCASE model or history definition option. State variables are initialized in the INITIAL STATE model definition set. The number of state variables per point is defined in the STATE VARS parameter. The default is one, with temperature always being the first state variable at a point. If more than one state variable per point has been assigned, this option can be used repeatedly to change the values of all state variables. The default value is no change if this option is not used. CHANGE STATE may be used in several different ways with the new table input format. Methods 1 to 4 discuss behavior when data is directly input and not read from a post file. While not explicitly stated, the data can always be a function of a table, where the independent variables are position to allow a nonhomogeneous field. They may be a function of time as described below.

Methods 5-7 are based upon reading the state variable from a post file created in a previously generated heat transfer analysis. 1. Change the state variable in a loadcase with a single increment typically in conjunction with AUTO LOAD and a single increment. The state variable takes the value entered here including all table effects. 2. Change the state variable over multiple increments of fixed time step, typically used with AUTO LOAD, DYNAMIC CHANGE, or TRANSIENT NON AUTO; in the later case, the state variable is not the first one (temperature). In this case, the state variable will either: a. Immediately take the value given here, if there is no table of time, and the ramp parameter is not activated on the LOADCASE model or history definition option. b. Linearly ramp the state variable from the value given at the beginning of the loadcase to the value at the end of the loadcase, if the ramp parameter is set on the LOADCASE model or history definition option. Note the values may include tables that are functions of time. They will be evaluated twice, at the beginning and end of loadcase. c. A general variation based upon a state variable that is a function of time. 3. Change the state variable over multiple increments using a variable time step procedure typically used with AUTO STEP or TRANSIENT; in the later case, the state variable is not the first one (temperature). In this case, the state variable will either: a. Immediately take the value given here, if there is no table of time and the ramp parameter is not activated on the LOADCASE model or history definition option.

Main Index

CHANGE STATE (with TABLE Input - Model Definition) 555 Redefine State Variables

b. Linearly ramp the state variable from the value given at the beginning of the loadcase to the value at the end of the loadcase, if the ramp parameter is set on the LOADCASE model or history definition option. Note the values may include tables that are functions of time. They will be evaluated twice: at the beginning and at the end of loadcase. c. A general variation based upon a state variable that is a function of time. 4. Change the state variable over multiple increments using a variable time step procedure where increment is based upon change in temperature, typically used with AUTO THERM. The state variable entered here may include a table reference, but the table should not be a function of time. This procedure should not be used with the ramp procedure. The difference in the temperature is determined, and if this is greater than the amount specified the loadcase will be divided into multiple increments. 5. Change the state variable by reading in a single increment from the post file. This is typically done using AUTO LOAD, and a single step. The 5th field of the 2nd line is one. If the time increment is not provided, the program will use the time associated with the heat transfer analysis. 6. Change the state variable in a multiple number of steps, each of which is associated to an increment in the heat transfer analysis. This is typically done using AUTO LOAD, and the number of increments equals the number of increments to be read, which is the same as the 5th field of the 2nd line. 7. Change the state variable by reading in a series of increments from a previously generated heat transfer job, and either dividing or consolidating the thermal increments based upon a maximum allowed change in the state variable. Used in conjunction with the AUTO THERM option. 8. Change the state variable by reading in a single increment from the post file, but apply the change in state variable over multiple increments based upon a user-defined criteria specified in the AUTO STEP option. The 5th field of the 2nd data block should be a -1. 9. Change the state variable by reading in a series of increments from the post file, and either dividing or consolidating the thermal increments based upon a user-defined criteria specified in the AUTO STEP option. In this case, the 5th field of the 2nd data block is not used and enough increments are read to satisfy the time period defined on the AUTO STEP option. 10. The NEWSV user subroutine is used to define the new state variables. The Fourier series number is not applicable to the methods where the initial conditions are read from the post file. The Fourier series number is not supported in version 2005. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

Main Index

1st

A

Enter the words CHANGE STATE.

556 CHANGE STATE (with TABLE Input - Model Definition) Redefine State Variables

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter the number of sets of data (not required).

6-10

2nd

I

Enter the unit number to read data.

I

Enter the state variable identifier (1 for temperature).

3rd data block 1-5

1st

Enter -1 if multiple state variables are read from a post file. In this case, the 8th data block is also required. 6-10

2nd

I

Enter the method: 3 - use binary post file 5 - user ASCII post file 6 - use data blocks (default) 7 - use user subroutine.

11-15

3rd

I

If method 3 or 5, enter the first step number to read. If method 6 or 7, enter the number of geometric types used to define this boundary condition.

16-20

4th

I

Enter the Fourier Series Number.

21-25

5th

I

For CHANGE STATE and method 3 or 5, enter the number of increments to be read in from post file in conjunction with AUTO THERM.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter boundary condition label.

4th data block (User only if method = 6 or 7) 1-10

1st

E

Enter the magnitude of the new state variable.

11-20

2nd

E

Enter the magnitude of the state variable at the beginning of the loadcase. This is required only if the ramp procedure is used.

5th data block 1-5

1st

I

Enter the table ID associated with the new state variable.

6-10

2nd

I

Enter the table ID associated with the state variable at the beginning of the loadcase. This is required only if the ramp procedure is used.

The 6th and 7th data blocks are repeated for as many geometric types as specified in the third field of the 3rd data block (used only if method = 6 or 7).

Main Index

CHANGE STATE (with TABLE Input - Model Definition) 557 Redefine State Variables

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1 - Element IDs 3 - Volume/Region/Body ID.

7th data block 1-80

Enter a list of geometric entities to which the above new state variables are applied. All the geometric entities must be of the type prescribed in the 6th data block.

The 8th data block is required only if multiple state variables are read from a post file if the first field of the 3rd data block is -1. 8th data block 1-80

Main Index

I

Enter a list of state variables.

558 CHANGE STATE (Model Definition) Redefine State Variables

CHANGE STATE (Model Definition)

Redefine State Variables

The information provided here is based upon not using the table driven input style. Description This option provides various ways of changing the state variables throughout the model. State variables are initialized in the INITIAL STATE model definition set. The number of state variables per point is defined in the STATE VARS parameter. The default is one, with temperature always being the first state variable at a point. If more than one state variable per point has been assigned, this option can be used repeatedly to change the values of all state variables. The default value is no change if this option is not used. In this option, the values of the state variable at the end of the current increment are read in. When the temperature is being defined, the following points should be noted: • For “history following analysis”, the thermal strains are based on temperature change during

this step. • For elastic re-analysis (ELASTIC parameter) the thermal strains are always based on temperature

change between the initial, stress free temperature field and the values read in here. • The AUTO LOAD option is available for specifying a time-varying history of state variables. The

value of the total state variable at the end of each increment is specified. • The AUTO THERM option is available for automatic control of a nonlinear (elastic-plastic)

temperature loaded stress problem, to be used in conjunction with this option. • The THERMAL LOADS option can be used as an alternative to input the change of temperature.

Either incremental or total temperatures can be specified using this option. • The AUTO THERM CREEP option is available for automatic control of a thermally loaded

elastic-plastic-creep problem, to be used in conjunction with this option. • The AUTO STEP option is available for automatic control of a nonlinear thermally loaded

problem, to be used in conjunction with this option. Time steps based on default recycling criteria and/or user-defined physical criteria are used to determine appropriate state variable increments. Four ways of changing any state variable through CHANGE STATE are possible: • Read a range of elements, integration points and layers and a corresponding state variable value

for the end of the current step. • Read the state variable values for the end of the current step through the NEWSV

user subroutine.

Main Index

CHANGE STATE (Model Definition) 559 Redefine State Variables

• Read the state variable values for the end of the current step from a named step of the post file

output from a previous heat transfer analysis with Marc. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by the user. Providing state variables through the thermal post file is currently supported for AUTO LOAD, AUTO THERM, AUTO THERM CREEP and AUTO STEP. It is not supported other adaptive stepping procedures. • For AUTO LOAD, a one-to-one correspondence between the thermal increments on the post

file and the mechanical increments is assumed between the user-defined starting and ending post increments. • For AUTO THERM or AUTO THERM CREEP, based on the user-defined allowable

temperature change, the thermal increments on the post file can be subdivided into many mechanical increments. • For AUTO STEP, thermal values on the post file are used to determine interpolated values of

state variables for the mechanical run. The interpolation is based on how the current mechanical loadcase time compares with the times read in from the thermal post file. Use of a state variable criterion to control the temperature increment is optional. The starting increment to be read in from the thermal post file (5th field of the 2nd data block) is userdefined. The number of sets of input to be read in (6th field of the 2nd data block) is not supported for AUTO STEP. Instead, the thermal information is read till the mechanical loadcase time or the thermal post file is completed. The post file is rewound and read from the beginning at the start of each loadcase or at any time a cutback is used by the AUTO STEP algorithm to reduce the current time step. • Read a list of elements, integration points, and layers and a corresponding state variable value.

It should be noted that the end of the current step is interpreted as the end of the current increment for fixed stepping procedures (AUTO LOAD, DYNAMIC CHANGE, CREEP INCREMENT) and as the end of the loadcase for adaptive stepping procedures (AUTO STEP, AUTO THERM, AUTO INCREMENT, AUTO CREEP). Note:

Using this option, total state variable values are input. From Marc 2001 onwards, the incremental change in the state variables is reset to 0 before each new increment if the AUTO LOAD option is used.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

Main Index

1st

A

Enter the words CHANGE STATE.

560 CHANGE STATE (Model Definition) Redefine State Variables

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter the state variable identifier for the state variable being changed (1,2,3,etc.) 1 = temperature. If more than one state variable is being used, the STATE VARS parameter must be included. Enter -1 if multiple state variables are read from a post file. In this case, the 9th data block is also required.

6-10

2nd

I

Enter 1 to change the state variable via the 3rd and 4th data blocks below. In this case, the third field must also be defined, and the sixth field if the AUTO THERM option is in use. Enter 2 to change the state variable via the NEWSV user subroutine. This subroutine is now called in a loop on all the elements in the mesh. Enter 3 to read the new values of the state variable from a post file written by a previous heat transfer analysis. In this case, the fourth and fifth field must be defined, and the sixth field if the AUTO THERM option is in use. Enter 4 to change the state variable via data blocks 5, 6, 7, and 8 below.

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. In that case, this entry gives the number of data blocks set in data blocks 3 and 4 used to input the new value of the state variable (optional).

16-20

4th

I

Only nonzero if the second field is set to 3. Then. this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Only nonzero if the second field is set to 3. In that case, this entry defines the step number on the heat transfer run post file to be read as the definition of the new value of the state variable at the end of the current step. This is currently only supported for AUTO LOAD, AUTO THERM, and AUTO STEP.

26-30

6th

I

Only used if the AUTO LOAD or AUTO THERM options are in use. Give the number of sets of input to be read to define the temperature history. Not used for AUTO STEP.

31-35

7th

I

Enter 1 if formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2. Set to 1 to suppress printout of state variable values that are defined in NEWSV.

41-45

Main Index

9th

I

Enter the post code number to be read into this state variable; default is 9 (temperature).

CHANGE STATE (Model Definition) 561 Redefine State Variables

Format Fixed

Free

Data Entry Entry

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of sets is equal to the number given in the third field above. 3rd data block 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with this value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value (11-15 and 16-20 can only be bigger than 1 if ALL POINTS parameter is used).

21-25

5th

I

First layer or cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value (21-25 and 26-30 can only be bigger than 1 for beam or shell elements).

F

New value of this state variable for the above range of points at the end of the current step.

4th data block 1-10

1st

Data blocks 5, 6, 7, and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

New total value of this state variable for the points given below at the start of the zeroth increment.

6th data block Enter a list of elements to which the above state variable is applied. 7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above state variable is applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above state variable is applied. The 9th data block is required only if multiple state variables are read from a post file if the first field of the 2nd data block is -1. 9th data block 1-80

Main Index

I

Enter a list of state variables.

562 THERMAL LOADS (Model Definition) Input Temperature Data

THERMAL LOADS (Model Definition)

Input Temperature Data

The information provided here is based upon not using the table driven input style. This option is not available with the table driven input. Description This option allows input of temperature and other state variables (see STATE VARS parameter). You can specify either a uniform or nonuniform change in temperature (or other state variables). If a nonuniform change is desired, the change of every state variable at every layer of every integration point of every element must be specified. In this case, Marc calls user subroutine CREDE for every element in the mesh. CREDE already exists in the standard version of Marc with coding to read data in loops over integration

points, layers and state variables, as illustrated below: NSTRES NEQST NSTATS READ VARIABLE DATA

NSTRES = Maximum number of integration points per elements NEQST = Maximum number of layers per element NSTATS = Maximum number of state variables

The data to be read should be put in the 4th data block of this option. For particular elements with less than the maximum number of integration points or layers, dummy values should be input when the integration point or layer number exceed the appropriate range. See the description of CREDE in Marc Volume D: User Subroutines and Special Routines for other necessary information. If temperature (state variable) data is on a file, this file can be read from CREDE. However, if temperature data is on a post file from a Marc heat transfer analysis that uses the same mesh, the CHANGE STATE option provides a much simpler method for reading temperature data. If the Fourier decomposition method is being used to analyze an arbitrarily loaded axisymmetric structure, the THERMAL LOADS option must be invoked separately for each Fourier series term that has temperatures (state variables) associated with it. If there is no variation of these variables in the circumferential direction, only the 0th term of the series should be specified.

Main Index

THERMAL LOADS (Model Definition) 563 Input Temperature Data

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words THERMAL LOADS.

I

Enter 1 if uniform incremental temperature (state variable) is applied to all elements.

2nd data block 1-5

1st

Enter 2 if nonuniform incremental temperature (state variable) is read via the CREDE user subroutine. Enter 3 if nonuniform total temperature (state variable) is read via the CREDE user subroutine. 6-10

2nd

I

If a Fourier analysis; the Fourier term with which this loading is associated.

E

If the first field of data block 2 is 1, enter the uniform increments in temperature and any additional state variables are applied to all elements.

E

Include only if the first field of data block 2 is 2 or 3, and using the default CREDE user subroutine. Temperature and state variable data to be read in by CREDE. All data blocks should contain 8 values, do not start a new data block for each element.

3rd data block 1-80

1st

4th data block 1-80

Main Index

1st

564 INITIAL TEMP (with TABLE Input - Thermal Stress) Define Initial Temperatures

INITIAL TEMP (with TABLE Input - Thermal Stress)

Define Initial Temperatures

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define initial temperatures at nodal points for thermal stress problems. This option allows you to define the magnitude and the location and associate them with an initial condition name. The initial condition is activated by the LOADCASE model definition option. For heat transfer analyses, see INITIAL TEMP for heat transfer. Note:

For shell analyses, a uniform temperature is used through the thickness direction.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL TEMP.

2nd data block 1-5

1st

I

Enter the number of sets of prescribed temperatures (optional).

6-10

2nd

I

Enter file number for input of prescribed temperatures data, defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine is required. Enter 1 if the USINC user subroutine is used.

Main Index

11-15

3rd

I

Flag to indicate that initial conditions are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then. this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Enter step number to be read.

INITIAL TEMP (with TABLE Input - Thermal Stress) 565 Define Initial Temperatures

Format Fixed

Free

Data Entry Entry If -1 is entered, the last step of the post file is used.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

If data is read from post file, the 4th through 7th blocks may be skipped. 4th data block 1-10

1st

F

Enter the magnitude of the initial temperature.

I

Enter the table ID associated with the geometric variation in initial temperature.

5th data block 1-5

1st

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 2 - Node IDs 3 - Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

566 INITIAL TEMP (Thermal Stress) Define Initial Temperatures

INITIAL TEMP (Thermal Stress)

Define Initial Temperatures

The information provided here is based upon not using the table driven input style. Description This option provides initial temperatures at nodal points for thermal stress problems. For heat transfer analyses, see INITIAL TEMP for heat transfer. Note:

For shell analyses, a uniform temperature is used through the thickness direction.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL TEMP.

I

Enter the number of sets of prescribed temperatures (optional).

2nd data block 1-5

1st

Enter -1 if the USINC user subroutine is used. In this case, data blocks 3 and 4 are not used. 6-10

2nd

I

Enter file number for input of prescribed temperatures data, defaults to input.

11-15

3rd

I

Flag to indicate that initial conditions are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then. this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Enter step number to be read. If -1 is entered, the last step of the post file is used.

Main Index

26-30

6th

I

Enter 1 if a formatted post file is used.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter 1 if the whole model has a default temperature given in the next field and only nodes not having this default temperature are given in the 3rd and 4th data blocks.

41-50

9th

E

Default temperature for all nodes in the model.

INITIAL TEMP (Thermal Stress) 567 Define Initial Temperatures

Format Fixed

Free

Data Entry Entry

Data blocks 3 and 4 are given in NSET pairs, only if the flag in the third field is not equal to 1. 3rd data block 1-10

1st

E

Initial temperature.

4th data block Enter list of nodes for which the above initial temperature is applied.

Main Index

568 POINT TEMP (with TABLE Input - Model Definition) Define Point Temperatures

POINT TEMP (with TABLE Input - Model Definition)

Define Point Temperatures

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define temperatures at nodal points for an uncoupled thermal stress problem and associate them with a boundary condition name. The boundary condition will be activated or deactivated using the LOADCASE model or history definition option. Note:

For shell analyses, a uniform temperature is used through the thickness direction.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT TEMP.

2nd data block 1-5

1st

I

Enter the number of sets of prescribed temperatures (optional).

6-10

2nd

I

Enter file number for input of prescribed temperatures data; defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine is required. Enter 1 if the USINC user subroutine is used.

Main Index

11-15

3rd

I

Flag to indicate that temperatures are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then, this entry defines the unit number from which the post file information is read.

21-25

5th

I

Enter step number to be read.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

POINT TEMP (with TABLE Input - Model Definition) 569 Define Point Temperatures

Format Fixed

Free

Data Entry Entry

If data is read from post file, the 4th through 7th blocks may be skipped. 4th data block 1-10

1st

F

Enter the magnitude of the temperature.

I

Enter the table ID associated with the temperature.

5th data block 1-5

1st

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 2 - Node IDs 3 - Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. the geometric entities must all be of the type prescribed in the 6th data block.

570 POINT TEMP (Model Definition) Define Point Temperatures

POINT TEMP (Model Definition)

Define Point Temperatures

The information provided here is based upon not using the table driven input style. Description This option defines temperatures at the end of the increment at nodal points for an uncoupled thermal stress problem. Note:

For shell analyses, a uniform temperature is used through the thickness direction.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT TEMP.

I

Enter the number of sets of prescribed temperatures (optional).

2nd data block 1-5

1st

Enter -1 if the USINC user subroutine is used. In this case, the 3rd and 4th data blocks are not used. 6-10

2nd

I

Enter file number for input of prescribed temperatures data; defaults to input.

11-15

3rd

I

Flag to indicate that temperatures are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then, this entry defines the unit number from which the post file information is read.

21-25

5th

I

Enter step number to be read.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter 1 if the whole model has a default temperature given in the next field and only nodes not having this default temperature are given in the 3rd and 4th data blocks.

41-50

9th

E

Default temperature for all nodes in the model.

Data blocks 3 and 4 are given in NSET pairs, only if the flag in the third field is not equal to 1.

Main Index

POINT TEMP (Model Definition) 571 Define Point Temperatures

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

E

Temperatures at the end of the increment.

4th data block Enter list of nodes for which the above initial temperature is applied.

Main Index

572 FORCDT Input Displacement or Load Histories

FORCDT

Input Displacement or Load Histories

Description This option specifies the nodes for which the FORCDT user subroutine is called when not using the table driven input (see Marc Volume D: User Subroutines and Special Routines). The FORCDT user subroutine can be used to prescribe the kinematic displacements and point loads. To prescribe displacements/temperatures, they must also be defined in FIXED DISP, FIXED TEMPERATURE, etc. When using the table driven input format, the use of the FORCDT user subroutine is activated on the FIXED DISP, etc. or POINT LOAD model definition options. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

A

Enter the word FORCDT.

11-15

I

Enter the number of lists to be given below. Default is 1.

2nd data block The 2nd data block is entered once for each data set. 1-80

Main Index

1st

I

List of nodes for which the FORCDT user subroutine is used.

FOUNDATION (with TABLE Input - Model Definition) 573 Input Elastic Foundation Data

FOUNDATION (with TABLE Input - Model Definition)

Input Elastic Foundation Data

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines a foundation, including the magnitude and application location and associates it with a boundary condition name (see Marc Volume A: Theory and User Information). The foundation will be activated or deactivated using the LOADCASE model definition option. A foundation damping may be applied for dynamic or harmonic analyses. Nonlinear foundations are available via user subroutine UFOUND (see Marc Volume D: User Subroutines and Special Routines) or via use of the TABLE option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word FOUNDATION.

2nd data block 1-5

1st

I

Number of sets of data blocks to be used to input the lists of element and foundation stiffnesses (optional).

6-10

2nd

I

Enter unit number for input of foundation data, defaults to input.

The 3rd through 7th data blocks are entered as pairs, once for each list. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the USPRNG user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

574 FOUNDATION (with TABLE Input - Model Definition) Input Elastic Foundation Data

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

E

Foundation stiffness per unit surface area (or per unit length for beam elements).

11-20

2nd

E

Foundation damping per unit surface area or per unit length for beam elements.

5th data block 1-5

1st

I

Enter the table ID to be associated with the foundation stiffness.

6-10

2nd

I

Enter the table ID to be associated with the foundation damping.

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal stiffness 2: Shear stiffness in 1st tangent direction 3: Shear stiffness in 2nd tangent direction 4: Volumetric in x-direction 5: Volumetric in y-direction 6: Volumetric in z-direction 7: Stiffness/length in x-direction for beams 8: Stiffness/length in y-direction for beams 9: Stiffness/length in z-direction for beams

11-15

3rd

I

Enter the face ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs

Main Index

FOUNDATION (with TABLE Input - Model Definition) 575 Input Elastic Foundation Data

Format Fixed

Free

Data Entry Entry 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Mentat convention 19: Curve ID: orientation ID - Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

576 FOUNDATION (Model Definition) Input Elastic Foundation Data

FOUNDATION (Model Definition)

Input Elastic Foundation Data

The information provided here is based upon not using the table driven input style. Description This option allows the specification of elements and associated foundation stiffness to be used with the elastic foundation option (see Marc Volume A: Theory and User Information). Nonlinear foundations are available via the USPRNG user subroutine (see Marc Volume D: User Subroutines and Special Routines). Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word FOUNDATION.

2nd data block 1-5

1st

I

Number of sets of data blocks to be used to input the lists of element and foundation stiffnesses (optional).

6-10

2nd

I

Enter unit number for input of foundation data. Defaults to input.

3rd data block The 3rd and 4th data blocks are entered as pairs, once for each list. 1-5

1st

I

Parameter identifying the type of elastic foundation; this is the same parameter as used in the DIST LOADS option. See Marc Volume B: Element Library for a description of the possible distributed load types for each element type in Marc.

6-15

2nd

E

Spring stiffness per unit surface area (or per unit length for beam elements).

4th data block 1-80

Main Index

1st

Enter a list of elements to which the above foundation is applied.

FOURIER 577 Describe Fourier Coefficients

FOURIER

Describe Fourier Coefficients

Description This option is used to describe all the Fourier coefficients for each series used. The FOURIER parameter must be included. If the Fourier coefficients of a series are known, they can be input directly. The function F(θ) to be expanded into a Fourier series can be described by an arbitrary number of pairs of data [θ, F(θ)]. The starting location (θ = 0) as well as the ending location (θ = 360) must be included. They can have different values F(θ). The function F(θ) can also be described via a UFOUR user subroutine for an arbitrary number of stations around the circumference. Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the word FOURIER.

2nd data block 1-5

1st

I

Number of Fourier series for which coefficients are input via data blocks.

6-10

2nd

I

Number of Fourier series for which the coefficients are calculated from user input [θ, F(θ)]. The description of F(θ) is given via data blocks. The number of coefficients to be calculated depends on the number of Fourier harmonics specified on the parameter data block.

11-15

3rd

I

Number of Fourier series for which the function F(θ) is determined by a user subroutine. The details on the UFOUR user subroutine are found in Marc Volume D: User Subroutines and Special Routines.

3rd data block Only included if the first parameter of the 2nd data block is nonzero. This series is repeated for each Fourier expansion for which coefficients are input via data blocks. 1-5

1st

I

Number of coefficients to be read for this series.

6-15

2nd

E

Fourier coefficients a0, a 1, b1, . . . an, bn,. Continuation data is in format 8E10.0.

The following group is included only if the second parameter of the 2nd data block is nonzero. This group is repeated for each F(θ) function. 4th data block 1-5

Main Index

1st

I

Number of [θ, F(θ)] pairs to be read in for this function.

578 FOURIER Describe Fourier Coefficients

Format Fixed

Free

Data Entry Entry

5th data block Four pairs of [θ, F(θ)] per data block. Continuation data is in format 8E10.0

Main Index

1-10

1st

F

Value in degrees of first station.

11-20

2nd

F

F(θ) – value for first station.

21-30

3rd

F

Value in degrees of second station.

31-40

4th

F

F(θ) – value for second station (etc.)

J-INTEGRAL 579 Define Path for J-Integral Estimation

J-INTEGRAL

Define Path for J-Integral Estimation

Description This option gives an estimation of the J-Integral for a crack configuration, based on differential stiffness technique. The technique is based upon moving nodes around the crack tip by a small distance and estimating the energy change. This model definition set is used to input the list of nodes to be moved, and the direction and size of those motions. Usually, the motion is 10 times smaller than the crack element size. Marc prints out the change in strain energy, which must then be divided by the change in crack surface area to obtain the J-Integral. Note:

For each evaluation the first list must contain the crack tip. The CENTROID parameter should not be used in conjunction with this option. With second order elements, we suggest the use of 1/4 point elements at the crack tip.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word J-INTEGRAL.

2nd data block 1-5

1st

I

Number of lists in this path.

6-10

2nd

I

Logical unit number for reading this data. Defaults to input.

Data blocks 3 and 4 are entered as paris, one for each list. 3rd data block 1-10

1st

F

Motion of these nodes in the 1st coordinate direction.

11-20

2nd

F

Motion in the second coordinate direction, etc. in (8E10) format. (Provide enough data to define the motion in each coordinate direction). Note:

The motion of the midsize nodes should be proportional to their position along the sides of the elements.

4th data block Enter a list of nodes to be moved.

Main Index

580 LORENZI Define Path for Modified J-Integral

LORENZI

Define Path for Modified J-Integral

Description This option gives an estimation of the J-Integral for a crack configuration using the domain integration method (a similar method is the deLorenzi method). The domain integration method has the advantage that it can also be used for problems with thermal behavior and for dynamic analysis. This procedure is only available for continuum elements. Only the nodes defining the crack front (crack tip in two dimensions) need to be defined. Marc automatically finds integrations paths according to the format below. The complete J-Integral is evaluated and printed. For the case of linear elastic material with no external loads on the crack faces, the program automatically separates mode I, mode II, and mode III (3D only) stress intensity factors from the J-Integral. Note:

The CENTROID parameter should not be used in conjunction with this option. With second order elements, we suggest the use of 1/4 point elements at the crack tip.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word LORENZI.

2nd data block 1-5

1st

I

Not used.

6-10

2nd

I

Enter the unit number to read the data.

11-15

3rd

I

Enter 1 for new input format.

3rd data block 1-5

1st

I

Enter the number of cracks (optional).

6-10

2nd

I

0 = no mode separation 1 = mode separation is activated. Default.

Data blocks 4 through 7 are repeated for each crack. 4th data block 1-5

2nd

I

Enter input style of rigid regions. 1 = direct input of nodes and/or elements. 2 = automatic search based on topology (default) 3 = automatic search based on geometry.

6-25

Main Index

1st

A

Crack name.

LORENZI 581 Define Path for Modified J-Integral

Format Fixed

Free

Data Entry Entry

5th data block Enter a node path defining the crack front (for 2-D, the node at the crack tip). Direct Input 5a data block 1-5

1st

I

Number of rigid regions for this crack.

6-10

2nd

I

Enter 1 if crack is at a symmetry plane.

Data block 6a is repeated for each rigid region. 6a data block Enter a list of nodes for the rigid region. 7a data block 1-10

1st

E

First component of shift vector.

11-20

2nd

E

Second component of shift vector.

21-30

3rd

E

Third component of shift vector (only for 3-D).

Topology Search 5b data block 1-5

1st

I

Number of rigid regions for each crack tip node

6-10

2nd

I

Shift vector (2-D); normal to crack face (3-D) 0 = entered values 1 = automatic determination (default)

11-20

3rd

E

Enter the tolerance for multiple nodes at the crack tip (default = 0.0).

6b data block (included only if second parameter of data block 5b is equal to 0) 1-10

1st

E

First component of shift vector (2-D); first component of the normal to crack face (3-D).

11-20

2nd

E

Second component of shift vector (2-D); second component of the normal to crack face (3-D).

21-30

3rd

E

Third component of the normal to crack face (3-D only).

Geometry Search 5c data block 1-5

1st

I

Number of rigid regions for each crack tip node.

6-10

2nd

I

Shift vector (2-D); normal to crack face (3-D) 0 = entered values 1 = automatic determination (default)

Main Index

582 LORENZI Define Path for Modified J-Integral

Format Fixed 11-20

Free 3rd

Data Entry Entry E

Enter the tolerance for multiple nodes at the crack tip (default = 0.0).

6c data block (included only if second parameter of data block 5b is equal to 0) 1-10

1st

E

First component of shift vector (2-D); first component of the normal to crack face (3-D).

11-20

2nd

E

Second component of shift vector (2-D); second component of the normal to crack face (3-D).

21-30

3rd

E

Third component of the normal to crack face(3-D only)

Data block 7c is repeated for each rigid region. 7c data block

Main Index

1-10

1st

E

Enter radius of rigid region to be found.

11-20

2nd

E

Enter relative length of cylinder for path search (3-D only).

VCCT 583 Virtual Crack Closure Technique

VCCT

Virtual Crack Closure Technique

Description This option defines that the virtual crack closure technique is to be used for evaluating energy release rates. The user defines the node (in 2-D or for shells) or nodes (in 3-D) that define each crack.The supported elements are lower- and higher-order 2-D solids and 3-D shells, lower- and higher-order 3-D hexahedral solids, and lower order 3-D tetrahedral solids. For 3-D solids, it is important that a regular mesh around the crack front is used. See Volume A for details. Multiple cracks can be defined and results are obtained for each crack separately. Each crack consists of a crack tip node in 2-D for shells and a list of nodes along the crack front for 3-D solids. Shell elements can be used for defining a 2-D style line crack and also be connected to the face of another shell or 3-D solid to form a 3-D style surface crack. These different cases are automatically identified. For crack propagation, there are two modes of growth: fatigue and direct. For fatigue style, the user specifies a load sequence time period. During the load sequence, the largest energy release rate and the corresponding estimated crack growth direction is recorded. At the end of the load sequence, the crack is grown using the specified method. For direct growth, the crack grows as soon as the crack growth criterion is fulfilled. Note that Gc and the respective mode specific limits can be made a function of the accumulated crack growth length to model a crack growth resistance behavior. Crack opening or propagation may be modeled using three techniques. In the first method, the body in which the crack is located is remeshed based upon the criteria defined in the ADAPT GLOBAL option and the crack is extended by the user specified length. This is currently available for planar and axisymmetric models only. In the second method, the uncracked area is represented by elements with double nodes and ties, RBE2 or RROD or by elements that are glued together via CONTACT TABLE with TABLES. In the third method, the crack grows along element edges or faces. New nodes are automatically inserted and the element connectivity at one side of the crack is changed in order to expand the crack. See Marc Volume A: Theory and User Information, Chapter 5: Structural Procedure Library, Fracture Mechanics for details. The settings for a crack can be modified in the history section and after restart. Also, a crack can be activated or deactivated for these cases. The check for an existing crack is done by matching the name of the crack, as given in the 4th data block. The settings will change only when a new VCCT option is encountered.

Main Index

584 VCCT Virtual Crack Closure Technique

Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the word VCCT.

I

Enter the number of cracks.

2nd data block 1-5

1st

The 3rd through 8th data blocks are repeated for each crack. If crack propagation is specified, also read data blocks 6 through 8. 3rd data block 1-5

1st

I

Flag for activating or deactivating an existing crack. 0 – leave as is 1 – activate 2 – deactivate

6-10

2nd

I

Specification of crack propagation 0 – no crack propagation 1 – fatigue style crack propagation 2 – direct crack propagation

4th data block 1-20

1st

A

Enter the name of the crack. Must be unique for each crack.

5th data block Enter an unsorted list of nodes defining the crack front. For 2-D and shells, this will be a single node. If crack propagation is specified (2nd field of 3rd data block equal to 1 or 2), enter data blocks 6 through 8. 6th data block 1-5

1st

I

Specification of crack growth 1 – remeshing 2 – release user tyings or glued contact 3 – break up mesh at edges or faces

Main Index

VCCT 585 Virtual Crack Closure Technique

Format Fixed 6-10

Free 2nd

Data Entry Entry I

Specification of method used for the crack growth direction 1 – maximum hoop stress criterion (default) 2 – along pure mode with largest Gi–Gic where i is mode I, II or III 3 – always along mode I 4 – along given vector; for this case read data block 9

11-15

3rd

I

Specification of crack growth increment for fatigue. 1 – fixed increment or via user subroutine 2 – Paris law

16-20

4th

I

Crack growth criterion 1 – Total G > Gc (default) 2 – GI > GIc or GII > GIIc or GIII > GIIIc 3 – Power law mixed mode criterion

G I ⎞ n 1 ⎛ G II ⎞ n 2 ⎛ G III ⎞ n 3 ⎛ ------+ ---------+ ----------->1 ⎝ G Ic⎠ ⎝ G II c⎠ ⎝ G I IIc⎠

4 – Reeder mixed mode criterion G I + G II + G I II ------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------->1 n + G G G III ⎛ G II + G I II ⎞ n 1 II III ⎞ 1 ⎛ G Ic + ( G IIc – G Ic ) -------------------------------------+ ( G III c – G II c ) ------------------------ ⎜ --------------------------------------⎟ ⎝ G I + G II + G II I⎠ G II + G II I ⎝ G + G + G ⎠ I II III

If fatigue crack propagation is specified (2nd field of 3rd data block equal to 1) 7a data block 1-10

1st

E

Crack growth increment. If the option of releasing tyings or glued contact is used, the length of the released element edge is used. Ignored for growth defined by Paris law

11-20

2nd

E

Time period for fatigue load sequence.

21-30

3rd

E

Paris law energy release rate threshold Gth.

31-40

4th

E

Paris law parameter C.

41-50

5th

E

Paris law parameter m.

51-60

6th

E

Minimum growth increment.

If direct crack propagation is specified (2nd field of 3rd data block equal to 2) 7b data block

Main Index

1-10

1st

E

Crack growth increment. If the option of releasing tyings or glued contact or breaking up element edges is used, the length of the released element edge is used.

11-20

2nd

E

Crack growth resistance Gc for total G.

586 VCCT Virtual Crack Closure Technique

Format Fixed 21-30

Free 3rd

Data Entry Entry E

Crack growth resistance for mode I, GIc. Defaults to Gc

31-40

4th

E

Crack growth resistance for mode II, GIc. Defaults to Gc

41-50

5th

E

Crack growth resistance for mode III, GIIIc. Defaults to Gc

51-60

6th

E

Exponent n1 for mixed mode methods, default 2.0

51-60

7th

E

Exponent n2 for mixed mode method 1, default 2.0

51-60

8th

E

Exponent n3 for mixed mode method 1, default 2.0

8th data block 1-5

1st

I

Table ID for scaling of the first value given in the 7th data block. For old style input (not table driven), these are ignored.

11-20

2nd

I

Table ID for scaling of the second value.

21-30

3rd

I

Table ID for scaling of the third value.

31-40

4th

I

Table ID for scaling of the forth value.

41-50

5th

I

Table ID for scaling of the fifth value.

51-60

6th

I

Table ID for scaling of the sixth value (fatigue only).

If crack growth direction vector is specified (crack growth direction option equal to 4) 9th data block

Main Index

1-10

1st

E

x component of crack growth direction vector

11-20

2nd

E

y component of crack growth direction vector

21-30

3rd

E

z component of crack growth direction vector

DELAMINATION 587

DELAMINATION Description This option defines a delamination, or in other words a mesh split. A stress criterion is used for determining if the mesh should split. The split can either be done in the interface between two materials or within a material. The criterion used is ⎛σ -----n-⎞ ⎝ Sn⎠

m

σt n + ⎛ -----⎞ > 1 ⎝ S t⎠

Here σ n is the normal stress, σ t is the tangential stress, S n is the allowable normal stress given below, the allowable tangential stress given below and m and n are the exponents given below.

St

For the option of splitting between materials, the normal direction is perpendicular to the material interface. The stress tensor of the nodal extrapolated stresses is transformed into this system. For the option of splitting within a material the system is given by the respective element edges in 2D and faces in 3D. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

I

Enter the word DELAMIN.

2nd data block 1-5

1st

I

Enter the number of sets (required).

6-10

2nd

I

Enter the unit number. Defaults to input file.

Data block 3 through 5 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the first material ID

6-10

2nd

I

Enter the second material ID; note that if this is the same as first material, then delamination within material.

11-15

3rd

I

Enter the delamination type: 0 – calculate delamination index and split mesh if necessary (default) 1 – only calculate a delamination index for post processing

16-20

Main Index

4th

I

Enter the material ID of a cohesive material. If specified, cohesive elements using this material will be inserted when the mesh breaks up.

588 DELAMINATION

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Allowable normal stress

11-20

2nd

F

Allowable tangential stress

21-30

3rd

F

m – exponent for normal stress (default 2.0)

31-40

4th

F

n – exponent for tangential stress (default 2.0)

It table input is used 5th data block 1-5

1st

I

Table ID for allowable normal stress

6-10

2nd

I

Table ID for allowable tangential stress

11-15

3rd

I

Table ID for m

16-20

4th

I

Table ID for n

The delamination criteria is based upon

Main Index

n

m

( σ n ⁄ σ n a ) + ( σ t ⁄ σ ta ) > 1

ISLAND REMOVAL 589 Deactivate Islands of Connected Elements

ISLAND REMOVAL

Deactivate Islands of Connected Elements

Description This option subdivides the mesh into islands of connected regions. If the number of elements in an island is less than or equal to a specified number, then all elements of this island are deactivated. This check is performed after element deactivation has taken place where the deactivation can be due to model input (DEACTIVATE option), the UACTIVE user subroutine, or through material damage or failure. Two elements are considered connected if they share a node for line elements, an edge for 2-D elements, or a face for 3-D solid elements. This option us useful for cases where we would get unconnected elements or regions of elements after the neighboring elements have been deactivated. There is no check performed to see if the island to be deactivated has enough boundary conditions. Only the number of elements in the island is used for determining if the elements should be deactivated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ISLAND REM

I

Enter the number of elements to use as a limit for element deactivation. If the number of elements in an island is less than or equal to this number, then all elements of this island are deactivated.

2nd data block 1-10

Main Index

1st

590

Main Index

Chapter 3: Model Definition Options 591 Contact

Chapt Contact er 3: This section describes surface geometry definition, motion definition, and friction description in two- and contact applications. The basic philosophy behind these applications is the existence Mode three-dimensional of one or more bodies that may or may not come into contact with one another, or even contact with themselves during an analysis. As far as the contact is concerned, it is the surface associated with the l body that plays a role. Defini Some bodies can be deformable, others can be rigid. However, deformable surfaces must always be tion declared in the input file before any rigid surface. Optio Deformable and Rigid Surfaces ns Marc Volume C: Program Input

A deformable surface is simply defined by the set of elements that constitute the body to which it is associated. When a node of another body or the same body (in self contact) comes into contact with a deformable surface, information regarding the contacted surface is obtained. This is based upon the coordinates of the nodes on the face of the element or the coordinates and an averaged normal if the SPLINE option is used. This can improve the accuracy of the solution. A rigid surface does not deform. There are two modes to describe the geometric profile of a rigid surface. In the first, labeled the PieceWise Linear approach (PWL), the profile is defined by sets of geometrical data which can be comprised of straight lines, circles and splines, ruled surfaces, surfaces of revolution and patches, etc. These sets have to be given in a proper sequence around the rigid body they define, even if it is not necessary that the full enclosure be defined. In the second method, labeled Analytical, the geometric profile is defined by prescribing 2-D NURBS curves, 3-D NURBS surfaces, or exact quadratic descriptions. Using this method, the surface is divided into line segments or patches; this is used for visualization (K6 style post file) or by the searching algorithm. The contact condition is based on the true surface geometry. This method is more accurate for curved surfaces, and might reduce the number of iterations, especially if friction is present. In coupled thermal-stress contact, it is possible to have a surface defined strictly by thermal elements with a rigid body motion applied to it.

Motion of Surfaces Deformable surfaces can move either because of contact with other surfaces, or because of directly applied displacement boundary conditions or loads. To each surface, we associate a point (center of rotation) that can be anywhere in space. A translative velocity and a rotational velocity around that point define the instantaneous motion of the surface. These velocities are integrated forward in time to define the motion of the surfaces. It is also possible to directly prescribe the location of the rigid body. As an alternative, you can prescribe a force or torque to the rigid body. The force is applied with the POINT LOAD option. The CONTACT model definition option can be used for the input of constant rigid body motions which do not change with time during the analysis. However, changes in rigid body motion (time dependent

Main Index

592 Marc Volume C: Program Input Contact

motion) can be simulated either by the load history option MOTION CHANGE or by the MOTION user subroutine activated through the UMOTION model definition option.

Cautions It is recommended that whenever several deformable bodies are present, the OPTIMIZE option be exercised. In static analysis, it is also necessary to artificially connect (for instance, by very low stiffness springs) deformable bodies that during an analysis might be completely separated from other deformable bodies and have no kinematic boundary conditions applied to them. This is to avoid rigid body motion. When the debug printout parameter PRINT is used in a contact analysis, IDEV = 5 or 8, it produces information on when any node on the boundary comes into contact or separates from any surface. It also produces information on whether a contact node is fixed to a surface or is free to slide along it. In addition to the information printed with IDEV = 5, when IDEV = 8 is entered, the incremental displacement and the reaction forces for those nodes in contact with rigid surfaces are printed in a local coordinate system. The CONTACT option creates ties between nodes which come into contact with another deformable body. If a node can come into contact with another deformable body or with a load controlled rigid body, one should avoid using these nodes as tied nodes in TYING, SERVO LINK, RBE2, or RBE3. There are three implied loops in this block of data: the outermost loop is over the number of surfaces; the next loop is over the number of sets of geometrical data for each surface; and the innermost loop is over the number of points comprised in each set. In case of deformable surfaces, the two inner loops reduce to the list of elements.

Control Variables and Option Flags The variable RVCNST (3rd data block, 1st field) depends on the selected friction model: 1. For the relative velocity based arctangent model it allows the system to self-adaptively search for sticking zones. RVCNST should be a relative sliding velocity very small compared to the typical sliding velocities in the model, but not so small that it would be overcome by changes between iterations. It is suggested you use values between 10-1 and 10-2 times a typical relative surface velocity. Marc default is 1.0. 2. For the stick-slip model, RVCNST indicates the slip to stick transition region, indicating a relative displacement magnitude in the direction of the friction force which is still accepted by the program. Its value should be small compared to a typical element length. The default value in Marc is 1.0e-6. 3. For the bilinear model, RVCNST is the relative displacement below which elastic stick is simulated. The default value is automatically determined by Marc, based on the dimensions of the elements in the deformable contact bodies. The variable ERROR (3rd data block, 2nd field) determines the tolerance for contact. A too small tolerance might provoke too many increment splits or iterations. A too coarse tolerance produces unrealistic behavior. If left blank, the code calculates ERROR as the smallest nonzero element dimension

Main Index

Chapter 3: Model Definition Options 593 Contact

divided by 20 or the shell thickness divided by 4. If there are splines in surface definitions, a value should be entered. (See SPLINE definition.) The user can control the type of friction in a contact analysis (2nd data block, 4th field). Either a friction (shear friction or Coulomb friction) or a frictionless condition can be assumed in the analysis. The friction behavior can be based on a continuous velocity based model, a true-stick-slip model or a bilinear displacement based model with an elastic sticking region. The computation of Coulomb friction in a contact problem can be based on either nodal stresses or nodal forces (2nd data block, 5th field). When shell or beam elements are in the body, it uses the nodal force based friction model. This is also true for the stick-slip friction model and the bilinear model.

Contact/Penetration In a contact analysis, the constraints imposed are to insure that penetration does not occur. Historically, the user can specify one of three different procedures to be used (2nd data block, 7th field). The first procedure, called Increment Splitting, is not recommended anymore. The two remaining are called Iterative Penetration Checking Procedure and Time Step Reduction Procedure. The Iterative Penetration Checking Procedure is recommended for most contact analyses. It may effectively add contact constraints during the Newton-Raphson iterations by scaling the iterative displacement vector of an iteration and bringing new nodes into contact at the start of the next iteration. In this sense, one is iterating on both global equilibrium and contact simultaneously. This procedure is always used when beam-beam contact is invoked. It is automatically used for quasi-static problems using AUTO STEP. The Time Step Reduction Procedure is recommended for dynamic contact analyses using an adaptive time stepping procedure. When this procedure is active, the time step of an increment may be reduced to make sure that nodes do not penetrate during the current increment, but instead are brought into contact at the beginning of the next increment. It is automatically used for dynamic problems using AUTO STEP.

Separation A node separates from a body depending on whether the force or the stress exceeds a threshold value (3rd data block, 5th field). It is possible to indicate whether the testing is based upon the force or the stress, how the stress is calculated, and how the threshold is calculated (2nd data block, 12th field). This choice has a significant influence on the accuracy and convergence of problems when: a. the contact forces are low, b. on rolling problems (where nodes periodically contact and separate), and c. in connector problems. It is recommended that a stress-based criterion is used, because it eliminates the numerical influence of element sizes, and that either physically meaningful tolerances are specified or a relative tolerance is entered. When quadratic contact is used, the separation criterion is always based upon a stress, which is

Main Index

594 Marc Volume C: Program Input Contact

obtained by extrapolating, averaging, and transforming the stresses at the integration points. The default separation threshold is: • the maximum residual force if separation is based upon nodal forces (the separation flag on the CONTACT option is 0); • the maximum stress at reaction nodes times the convergence tolerance (given on the CONTROL

option) if separation is based on absolute stresses, where a stress is calculated as a nodal force divided by a nodal area (the separation flag on the CONTACT option is 1); • 10% of the maximum compressive stress for all the contacting nodes if separation is based on any of the other methods (the separation flag on the CONTACT option is 2, 3 or 4).

For beam-to-beam contact, contact stresses cannot be calculated and separation can only be based on nodal forces. Hence, if within one model both beam-to-beam contact and contact between continuum elements occur and separation should be based on stresses, then it is recommended to enter the separation threshold for beam-to-beam contact using a CONTACT TABLE. Otherwise, the default separation stress would be used as a force to decide if beam-to-beam contact constraints should be released. During each load increment, separations can occur. You can control the maximum number of nodal separations allowed in each increment to reduce computational costs (2nd data block, 6th field). During the analysis, a node may come into contact and separate within the same increment. This may be due to either the nonlinear motions or due to small contact forces/stresses that are developed. This often leads to oscillations in the contact status which leads to multiple iterations and higher computational costs. This behavior may be controlled using the flag on the 2nd data block, 9th field. This chattering behavior is automatically suppressed for explicit dynamics.

Optional Heat Transfer Data In a coupled thermal-stress-contact analysis, a film coefficient is needed for calculating heat transfer from any other surface that contacts the current surface (deformable-to-rigid, or deformable-to-deformable). If the surface is modeled as a rigid surface, the rigid surface temperature is also needed for the analysis. In addition, both a film coefficient and an ambient temperature must be given for the simulation of heat transfer between the surface and surrounding environment. If the near thermal contact option is invoked using CONTACT TABLE, it is also possible to have transmission of heat when bodies are close to one another. The thermal fluxes have components of convection and radiation. This requires input of the distance that is considered to be close and additional thermal parameters. Unlike the error tolerance, it is not possible for the program to determine a default value.

Optional Electrical Data (Joule Heating Analysis) In Joule heating or coupled thermal-structural-electrical problems, current may be transmitted between contact bodies. This current is assumed to be continuous (that is, no electrical arcing). This requires additional data analogous to the heat transfer data.

Main Index

Chapter 3: Model Definition Options 595 Contact

Time Step Control The automatic contact procedure is controlled by the time step. This is used to determine the motion of rigid surfaces and to control the splitting of increments if penetration occurs. Even in a quasi-static analysis, a time step must be defined by you. Several procedures can be used to enter this data. • The AUTO LOAD and TIME STEP history definition options can be used to define several time

steps, each of the same magnitude. • The DYNAMIC CHANGE or TRANSIENT NON AUTO history definition options can be used to

define a time period which is divided into equal time steps. • With the AUTO STEP or AUTO INCREMENT history definition option, you define a total time

period which is divided into variable size time steps.

Dynamic Contact - Impact The automatic contact procedure can also be used in dynamic analyses to model impact problems. This can be used with the implicit Newmark-beta or single step Houbolt operator or the explicit central difference operator. The DYNAMIC parameter is used to control the choice. When the Newmark-beta or single step Houbolt operator is used, either the DYNAMIC CHANGE or AUTO STEP option can be used to control the time step. When the central difference procedure is used, the DYNAMIC CHANGE option should be used, and the time step must be less than the stability limit. The stability limit is automatically calculated by Marc.

Two-dimensional Rigid Surfaces In a two-dimensional problem, the rigid surfaces can be represented by any of or a combination of the following geometric entities: (1) straight line segments (ITYPE = 1), (2) circular arcs (ITYPE = 2), and (3) spline (ITYPE = 3). The variable ITYPE defines the type of the geometric entities to be used for a rigid surface. Note that the normal vector of the geometric entities (line segments, circular arc, and the spline) always points into the rigid-body. The normal vector direction is determined from the direction of the geometric entity, following a right-handed rule. Care must be taken in entering the coordinates (x, y) data, in a correct direction, for rigid-surfaces. Line Segments When option ITYPE = 1 is chosen, the number NPOINT and the coordinates (x, y) of (NPOINT) points must be entered for the definition of the rigid surface. Marc automatically creates a rigid surface consisting of (NPOINT -1) linear segments for the contact problem. A two-dimensional rigid surface consisted of line segments is shown in Figure 3-1. This entity supports analytic description/procedure.

Main Index

596 Marc Volume C: Program Input Contact

η Start point 1

2

Rigid body

3 4

y

End point

5 6

x

Figure 3-1

7

8

Two-dimensional Rigid Surface (Line Segment, ITYPE = 1)

Circular Arc When ITYPE = 2 is chosen, one circular segment is created by Marc. There are five different methods available to define a circular arc in two dimensions. Each method requires four data blocks with the following type of data: Starting Point of Arc

(SP)

Ending Point of Arc

(EP)

Center of Circle

(C)

Radius of Circle

(R)

Tangent Angles

(TA)

Swept Angle

(SA)

Number of Subdivisions (NS) Clearly, not all of this information is required for each method. Table 3-9 describes which data is required. The default number of subdivisions is 10. If the analytical approach is used, the number of subdivisions does not influence the accuracy, but is only used for visualization purposes. Table 3-1

Data Required for Circular Arc Input Method

Data Block

0

1

2

3

4

1

SP

SP

SP

SP

SP

2

EP

EP

EP

EP

blank

3

C

C

C

TA1, TA2

C

4

R, NS

R, NS

R, NS

R, NS

SA, NS

Notes:

Main Index

For methods 1 and 3, a positive radius means the center of the circle is on the surface side. A negative radius means the center of the circle is on the outside.

Chapter 3: Model Definition Options 597 Contact

For method 2, the first coordinate of the center is taken into account, determining whether the center is above (>0) or below (<0) the segment defined by the end points. For planar problems, SP, EP and C are X, Y data. For axisymmetric problems, SP, EP and C are Z, R data. For methods 0, 1 and 2, if R is zero, it is calculated as distance from the center to the starting point. This entity supports analytical description/procedure. A two-dimensional rigid surface represented by a circular arc is shown in Figure 3-2 and Figure 3-3.

η Start point 1

End point Center + Radius

Note: Figure 3-2

Main Index

For additional circular arc definitions, see Figure 3-3

Two-dimensional Rigid Surface (Circular Arc, ITYPE = 2, METHOD = 0)

598 Marc Volume C: Program Input Contact

EP

EP

SP

SP

R

R

+

+

C

C

Method 0 Positive R

Method 1 Negative R

EP

TA2

SP

SA

R

SP

TA1

+

X

C

Method 3 Positive R Figure 3-3

Main Index

+

C

Method 4 Positive R

Two-dimensional Rigid Surface (Circular Arc)

Chapter 3: Model Definition Options 599 Contact

Spline When ITYPE = 3 is chosen, Marc creates a spline by passing from the second point through to the second to last point entered. The first and the last points entered are used to define the tangents at the beginning and end of the spline. If a nonanalytical approach is used, then the spline is internally split into linear segments in such a way that the maximum difference between any of them and the spline is less than the contact tolerance ERROR. This operation is done before the automatic tolerance calculation; therefore, a value for ERROR must be entered whenever a spline is used. Figure 3-4 shows a twodimensional rigid surface defined by a spline. 6

End point

Note: the normal vector η is pointed into the rigid body.

5 4

3

2

1

Rigid body

Start point

η Figure 3-4

Two-dimensional Rigid Surface (Spline, ITYPE = 3)

This entity supports analytical description/procedure if only one spline is used in a particular rigid body.

Three-dimensional Rigid Surfaces In a three-dimensional problem, the rigid surfaces are represented by any of or a combination of the following three-dimensional surface entities: Surface Entity Type

Type Identification (ITYPE)

Ruled surface

4

Surface of revolution

5

Bezier surface

6

4-node patch

7

Poly-surface

8

NURB

9

Cylinder

10

Sphere

11

The variable ITYPE defines the type of surface entity to be used for a rigid surface. Since most of the three-dimensional surfaces can be easily and adequately represented by a finite element mesh of 4-node plate (patch) elements, the option ITYPE = 7 is a very convenient way of representing threedimensional rigid surfaces. Both the connectivities and the coordinates of the 4-node patches can be generated using Marc Mentat, or entered through the DIGEOM user subroutine.

Main Index

600 Marc Volume C: Program Input Contact

The three-dimensional surface entities mentioned above, except 4-node patches, can in turn be generated from three-dimensional geometric entities. Available three-dimensional geometric entities are: Geometric Entity Type

Type Identification (JTYPE)

Straight line segment

1

3-D circular arc

2

Spline

3

Bezier Curve

4

Poly line

5

The variable JTYPE defines the type of geometric entities to be used for the generation of three-dimensional rigid surfaces. For the (PWL) approach, note that all geometrical data in 3-D space is reduced to 4-node patches. The four nodes will probably not be on the same plane. The error in the approximation is determined by the number of subdivisions of the defined surfaces. Note that the normal to a patch is defined by the righthand rule, based on the sequence in which the four points are entered. Ruled Surface (ITYPE = 4) When ITYPE = 4 is chosen, a ruled surface is created by Marc based on the input of two surface generators, defined by straight line segment (JTYPE = 1), 3-D circular arc (JTYPE = 2), spline (JTYPE = 3) or Bezier curve (JTYPE = 4). If the surface generator is not a 3-D circular arc, the number NPOINT1 (NPOINT2) and the coordinates (x, y, z) of these NPOINT1 (NPOINT2) points must be entered for the definition of the surface generators. In case the surface generator is a 3-D circular arc, a method (METH) must be selected for the definition of the circular arc. A 3-D circular arc is defined by four points. In addition, the number of subdivisions, NDIV1, along the first (surface generator) and the NDIV2 along the second (from the first surface generator to second surface generator) direction must also be entered. For a (PWL) approach, Marc creates (NDIV1) x (NDIV2) 4-node patches automatically to represent the prescribed ruled surface. For analytical approach, (NDIV1 + 1) x (NDIV2 + 1) points are created and a NURB surface is general which passes exactly through these points. The accuracy in general is controlled by the number of points. Figure 3-5 shows a typical ruled surface.

Main Index

Chapter 3: Model Definition Options 601 Contact

Start point

End point

η

2 2nd Geometric entity

Start point 1 End point

1st Geometric entity 1: first direction 2: second direction η: normal direction into the rigid body

z y x NDIV2 = 3 NDIV1 = 4 NDIV1 = number of divisions in the first direction NDIV2 = number of divisions in the second direction

Figure 3-5

Three-dimensional Rigid Surface (Ruled Surface, ITYPE = 4)

Surface of Revolution (ITYPE = 5) When ITYPE = 5 is chosen, a surface of revolution is created by Marc based on the input of one surface generator, defined by straight line segment (JTYPE = 1), 3-D circular arc (JTYPE = 2), spline (JTYPE = 3) or Bezier curve (JTYPE = 4). If the surface generator is not a 3-D circular arc, the number NPOINT and the coordinates (x, y, z) of these NPOINT points must be entered for the definition of the surface generator. In case the surface generator is a 3-D circular arc, a method (METH) must be selected for the definition of the circular arc. A 3-D circular arc is defined by four points. In addition, the number of subdivisions NDIV1 along the surface generator and NDIV2 along the second (circumferential) direction must also be entered.

Main Index

602 Marc Volume C: Program Input Contact

Marc then creates (NDIV1 x NDIV2) four-node patches automatically, to represent the prescribed surface of revolution. The axis of revolution is defined by the coordinates (x, y, z) of two points in space, and an angle of rotation from the initial position is also needed for the definition of the surface of revolution. A positive rotation is about the axis formed from point 1 to point 2. Figure 3-6 shows a typical surface of revolution. Axis of revolution defined by the coordinates of points 1 and 2 Start point Surface generation (initial position) 1 2

Point 1 Angle of rotation

η

End point

Point 2 z

1: First direction 2: Second direction

x

Figure 3-6

y

η: Normal direction into the rigid body (see Figure 3-8)

Three-dimensional Rigid Surface (Surface of Revolution, ITYPE = 5)

Bezier Surface (ITYPE = 6) When ITYPE = 6 is chosen, a Bezier surface is defined by the coordinates (x, y, z) of NPOINT1 x NPOINT2 control points. NPOINT1 points are entered along the first direction and then repeated NPOINT2 times to fill through the second direction of the surface. NPOINT1 and NPOINT2 have to be at least equal to 4. Number of subdivisions (NDIV1, NDIV2) entered has to be equal or greater than NPOINT1 and NPOINT2 for Bezier surface. (NPOINT1-1) x (NPOINT2-1) 4-node patches are created by Marc for the definition of a Bezier surface. Figure 3-7 shows a typical Bezier surface. It can be treated as an analytical surface, an exact conversion to NURBS is performed.

Main Index

Chapter 3: Model Definition Options 603 Contact

r13

r23

r22 r03

r33 r32

r12

r21 r11 r31

NPOINT2 = 4 NDIV2 = 4

r02 2

r20 r01

r10

η z

r30 1

y

r00

x

NPOINT1 = 4 NDIV1 = 4

1: First direction 2: Second direction h: Normal direction into the rigid body (see Figure 3-8)

Figure 3-7

Three-dimensional Rigid Surface (Bezier Surface, ITYPE = 6)

Four-node patches (ITYPE = 7) When ITYPE = 7 is chosen, you enter directly all the 4-node patches that comprise this surface. They are entered following the same format Marc would use to read the connectivities and coordinates of a mesh of 3-D 4-node elements (element type 18 or 75). In this way, a finite element preprocessor can be used to create surfaces. Alternatively, this data can be entered via the user subroutine DIGEOM, further permitting you to read by yourself from any data you have access to. Figure 3-8 shows a typical 4-node patch surface. It cannot be used as an analytical surface. Both the value of ERROR and BIAS can also be specified on the CONTACT TABLE option for a specific combination of bodies. A BIAS of zero will be used for glued contact and contact with a symmetry body even if a nonzero value is specified on the third data block, unless it is specified via the CONTACT TABLE option.

Main Index

604 Marc Volume C: Program Input Contact

z

Number of patches = 12 Number of nodes = 20 Nodal coordinates can be entered using user subroutine DIGEOM

12

y x

13

7 8

1 12

2

η

Rigid body

13 2

7

8 η

12

13 1

7

Rigid body

8 1: First direction 2: Second direction

η: Normal vector (right-hand rule) into the rigid body Figure 3-8

Three-dimensional Rigid Surface (4-Node Patch, ITYPE = 7)

Poly-surface (ITYPE = 8) When ITYPE = 8 is chosen, a poly-surface is defined by the coordinates (x, y, z) of NPOINT1 x NPOINT2 control points. NPOINT1 points are entered along the first direction and then repeated NPOINT2 times to fill through the second direction of the surface. NPOINT1 and NPOINT2 have to be at least equal to 4 for a poly-surface and there is no need to divide it. A typical poly-surface is shown in Figure 3-9. In a three-dimensional contact problem, as in a two-dimensional situation, the surface generators can be represented in a variety of ways. It can be treated as an analytical surface. Approximate conversion to NURBS.

Main Index

Chapter 3: Model Definition Options 605 Contact

53 54

52

43

51

55

44

42

45 34

33

41

35

32

NPOINT2 = 5

24

23 31

25

22

2 21 z

12 y

14

13

h

11

15

1 NPOINT1 = 5

x 1: First direction 2: Second direction

η: Normal direction into the rigid body Figure 3-9

Three-dimensional Rigid Surface (Poly Surface, ITYPE = 8)

Nonuniform Rational Bspline Surface, NURBS (ITYPE = 9) When ITYPE = 9 is chosen, a NURBS is defined by the coordinates (x, y, z) of NPOINT1 x NPOINT2 control points, NPOINT1 x NPOINT2 homogeneous coordinates and (NPOINT1+NORDER1) + (NPOINT2+NORDER2) normalized knot vectors. If only the control points are entered, the interpolation scheme is used such that the surface passes through all of control points. The homogeneous coordinates and knot vectors are calculated by Marc. NPOINTS and NPOINT2 have to be at least equal to 3 for the interpolation scheme. A typical NURBS is shown in Figure 3-10.

Main Index

606 Marc Volume C: Program Input Contact

+10 +8

+6

+9 +7

+5 +4

+2

+3

Z Y

X

+1

Figure 3-10

Nonuniform Rational Bspline Surface, NURBS (ITYPE = 9)

Cylinder (Cone) Surface (ITYPE = 10) When ITYPE = 10 is chosen, a cylinder is defined by the coordinates (x, y, z) of the center, C1, with radius, R1, in top face and the coordinate (x, y, z) of center, C2, with radius, R2, in bottom face. The normal vector of cylinder is inwards. If a negative value of R1 is entered, the normal vector is outwards. A typical cylinder is shown in Figure 3-11.

Main Index

Chapter 3: Model Definition Options 607 Contact

R1

C1

R2 C2

X

Y Z

Figure 3-11

Cylinder (Cone) Surface (ITYPE = 10)

Sphere Surface (ITYPE = 11) When ITYPE = 11 is chosen, a sphere is defined by the coordinates (x, y, z) of the center, C1, with radius, R1. The normal vector of sphere is inwards. If a negative value of R1 is entered, the normal vector is outwards. A typical sphere is shown in Figure 3-12.

Main Index

608 Marc Volume C: Program Input Contact

R1

C1

Z

X

Figure 3-12

Y

Sphere Surface (ITYPE = 11)

3-D Circular Arc When JTYPE = 2 is chosen, a circular arc is created by Marc. There are three different methods (Table 3-10) available to define a circular arc in three dimensions. Each method requires four data blocks, with the following type of data:

Main Index

Starting point of arc

(SP)

Ending point of arc

(EP)

Enter of circle

(C)

Radius of circle

(R)

Swept angle

(SA)

Swept angle flag

(SAF)

Middle point

(MP)

Arbitrary point (lying in plane of circle)

(AP)

Chapter 3: Model Definition Options 609 Contact

Table 3-2

Defining Circular Arcs Method

Data Block

0

1

2

1

SP

SP

SP

2

EP

MP

AP

3

C

EP

C

4

R

SAF

SA

Notes:

For Method 1, a positive radius means the center of the circle is on the surface side. A negative radius means the center of the circle is on the outside. For Method 2, a SAF that is positive means an angle less than 180, a negative value an angle greater than 180. For Method 3, the starting point, arbitrary point and center define the plane in which the circular arc lies. SP, EP, C, MP and AP are X, Y, Z data. For an arc with 180 degrees, either Method 1 or Method 2 is recommended.

A three-dimensional rigid surface represented by a circular arc is shown in Figure 3-13. EP EP MP SA

SP

R

SP

SP

+

+

C

C

Method 0

Method 1

AP

Method 2 Figure 3-13

Three-dimensional Rigid Surface (Circular Arc)

Spline When JTYPE = 3 is chosen, the spline passes by all NPOINT declared, and has zero curvature at the ends (enter at least 4 points). Bezier curve When JTYPE = 4 is chosen, a Bezier curve is defined by NPOINT control points (enter at least 4 points).

Main Index

610 Marc Volume C: Program Input Contact

Poly-line When JTYPE = 5 is chosen, a poly-line defined by NPOINT control points.

Selective Contact Surfaces In both the two- and three-dimensional contact problems, contact is always detected between nodes on the surface of a deformable body and the geometrical profile of another surface. There are two modes of the order in which a node checks contact with other bodies - so called single-sided contact and doublesided contact. The default version is the double-sided contact procedure. In the single-sided contact procedure, by default, the nodes on a lower numbered body can come into contact with equally or higher numbered surfaces. For instance, the boundary nodes of body number 1 are checked against the surface profiles of bodies 1, 2, 3, .... The boundary nodes of body number 2, however, are only checked against surface profiles of bodies 2, 3, ... It is possible, therefore, that due to surface discretization, a node of body 2 slightly penetrates the surface of body 1. The order of contact checking can be defined via the CONTACT TABLE option. The double-sided contact option checks possible contact between any two surfaces (surface i is checked for contact with surface j, and surface j is also checked for contact with surface i, where i, j = 1, 2, 3, ..., total number of surfaces in the problem). When defining contact bodies for a deformable-to-deformable analysis, it is important to define them in the proper order. As a general rule, a body with a finer mesh should be defined before a body with a coarser mesh. For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change. In addition, an option (CONTACT TABLE model definition and load incrementation options) is provided to you for the selection of contact surfaces. Through this option, you can choose, for instance, the surface no. 1 to be in contact with surfaces 3, 5, 6, 7, but not with surfaces 2 and 4. This option can repeatedly be used during an analysis by specifying it in the history definition option. You can further restrict the potential contact by using the CONTACT NODE or the EXCLUDE option.

User Subroutines A number of user subroutines are available to you for two- and three-dimensional contact problems. These are listed in Table 3-11.

Main Index

Chapter 3: Model Definition Options 611 Contact

Table 3-3 User Subroutine

Option Required

MOTION (2-D) MOTION (3-D)

CONTACT (2-D), CONTACT (3-D), UMOTION

To define surface motion.

UFRIC

CONTACT (2-D), CONTACT (3-D), UFRICTION

To define friction data.

UFRICBBC

CONTACT (2-D) CONTACT (3-D) CONTACT TABLE

To define the separation force for beam-to-beam contact.

UHTCOE

CONTACT (2-D), CONTACT (3-D), UHTCOEF

To define film coefficient and sink temperature.

UHTCON

CONTACT (2-D), CONTACT (3-D), UHTCON

To define film coefficient between contact surfaces.

UVTCOE

JOULE CONTACT (2-D) CONTACT (3-D) UHTCOEF

To define environment electrical film coefficient.

UVTCON

JOULE CONTACT (2-D) CONTACT (3-D) UHTCON

To define contact electrical film coefficient.

UMDCOE

DIFFUSION CONTACT UHTCOEF

Definition of variable mass diffusion coefficients and sink pressure on free surfaces.

UMDCON

DIFFUSION CONTACT UHTCON

Definition of variable mass diffusion coefficients of surfaces that are in contact with other surfaces.

UMDNRC

DIFFUSION UHTCON CONTACT CONTACT TABLE

Definition of mass diffusion coefficients between surfaces almost in contact.

DIGEOM

CONTACT (2-D), CONTACT (3-D)

To define coordinates of 4-node patches.

SEPFOR

CONTACT (2-D), CONTACT (3-D)

To define the separation force.

Note:

Main Index

User Subroutines for Contact Problems Contents

Marc Volume D: User Subroutines and Special Routines manual provides more detailed information on these subroutines.

612 Marc Volume C: Program Input Contact

Table 3-3 User Subroutine

User Subroutines for Contact Problems (continued) Option Required

Contents

SEPFORBBC

CONTACT (2-D), CONTACT (3-D) CONTACT TABLE

To define the separation force for beam-to-beam contact.

SEPSTR

CONTACT (2-D), CONTACT (3-D)

To define the separation stress.

UNORST

CONTACT (2-D), CONTACT (3-D)

To define normal stress at each node in contact.

Note:

Marc Volume D: User Subroutines and Special Routines manual provides more detailed information on these subroutines.

Contact with Adaptive Meshing or Rezoning In a contact (or any other) problem, the original mesh can be badly deteriorated during the analysis due to excessive deformation. Rezoning of the deteriorated mesh generally allows the continuation of the analysis to completion. This can be performed automatically using the ADAPT GLOBAL model definition option or manually using the REZONING parameter, and the rezoning options CONNECTIVITY CHANGE and COORDINATE CHANGE. When using the ADAPT GLOBAL option, this will be performed as often as necessary. Note that in a contact problem, only the deformable surface definition can be changed. After rezoning occurs, rigid surfaces must be kept the same and cannot be changed. The upper bound to the number of nodes that lie on the periphery of any deformable body must be sufficiently high to account for an increase in the number of nodes.

Spring-Back Analysis In metal forming analysis, the spring-back condition is of great interest to engineers for the study of the state of residual stresses in the workpiece. However, it is a difficult numerical problem and generally requires a large number of load increments for a final solution. The RELEASE load incrementation option allows the release (separation) of all the nodes in contact with a particular surface at the beginning of the increment. A spring-back condition can be obtained in one load increment. Marc iterates the solution within the increment automatically for an equilibrium solution.

Contact Tolerance A node comes into contact with another body when it enters the contact tolerance zone. This area is dependent upon the value of ERROR and BIAS entered on the third data block. When BIAS is zero, the tolerance is equidistant from the actual surface as shown in Figure 3-14 (a); otherwise, the situation shown in Figure 3-14 (b) is used. If a node would have moved past line B, then increment splitting would occur if the fixed time step procedure is used and the increment splitting procedure is used.

Main Index

Chapter 3: Model Definition Options 613 Contact

ERROR

ERROR*(1-BIAS)

ERROR

ERROR*(1+BIAS)

B (a) Equidistant Default

Figure 3-14

(b) Biased

Contact Tolerances

Corner Conditions When a node slides along a surface composed of multiple segments, three conditions can occur based on the angle that the segments make. This is true for both two-dimensional and three-dimensional problems. The Figure 3-15 shows the two-dimensional case for simplicity. If the angle between the two segments is between 180 - β < α < 180° + β, the node smoothly slides between the segments. If the angle is such that 0 < α < 180 - β, the node sticks in the sharp concave corner. If the angle is such that α > 180 + β, the node separates. The value of β is 8.625° for two-dimensional problems and 20° for three-dimensional problems. These values can be reset using the PARAMETERS option.

α

Smooth

Sharp Concave

Sharp Convex

Figure 3-15

Corner Conditions

Friction There are several friction models available in Marc. The friction types, entered on the second line of the CONTACT option, are as follows:

Main Index

614 Marc Volume C: Program Input Contact

0

No friction

1

Shear friction: velocity based smoothing function

2

Coulomb friction: velocity based smoothing function

3

Shear friction for rolling: velocity based smoothing function

4

Coulomb friction for rolling: velocity based smoothing function

5

Stick-slip model: step function

6

Coulomb friction: displacement based bilinear function

7

Shear friction: displacement based bilinear function

More details on these models are presented in Marc Volume A: Theory and User Information. For model types (1-4), you need to define both the friction constant and the value of RVCNST(C). This value is used to smooth out the discontinuous behavior of friction. The value of RVCNST can be interpreted as the value of the relative velocity when sliding occurs. A very small value results in a difficulty to converge; while a very large value results in hardly any effect of friction. This is depicted in Figure 3-16. -

Ft 1

C = 0.01 C = 0.1 C=1

C = 10 C = 100

10 vr

-10

-1

Figure 3-16

Stick-slip Approximation (Fn = 1)

Using the stick-slip friction model, type 5, three parameters (α, β, and e) are available to control the numerical behavior. Here α represents a tolerance on the frictional force before sliding occurs. The node changes from stick to slip when F t > αμ F n

Main Index

Chapter 3: Model Definition Options 615 Contact

So the difference between the static and the dynamic coefficient of friction is expressed by α. Parameter β can be seen as the amount of relative displacement in the direction of the friction force to enforce the friction condition to change from slip to stick. The tolerance on the convergence of the solution is given by e. It is required that Ft 1 – e ≤ --------p- ≤ 1 + e Ft

where F t p is the tangential force at the previous iteration. This is shown in Figure 3-17. The stick-slip model automatically used the nodal based friction procedure.

2β

μFn

αμFn

Ft

2εβ Δut

α = 1.05 (default; can be user-defined) β = 1 x 10-6 (default; can be user-defined) ε = 1 x 10-6 (fixed; so that εβ ≈ 0) e = 5 x 10-2 (default; can be user-defined)

Figure 3-17

Stick-slip Friction Parameters

Finally, the friction models 6 and 7 (see Figure 3-18 for the Coulomb model) offer two parameters to control the numerical behavior: δ and e. The parameter δ can be seen as the slip threshold: as long as the relative tangential displacement in a contact node is smaller than δ, there exists an “elastic” or stick condition. Its default value is determined automatically by the program. Parameter e is used to control the accuracy of the friction solution. A friction solution is considered to be converged if: p

F t – Ft -------------------------------≤e p Ft

where F pt is the total friction force of the previous iteration and force vector.

Main Index

(i)

indicates a component of the friction

616 Marc Volume C: Program Input Contact

Ft μF n

δ

Figure 3-18

Δu t

Bilinear Friction Model

The shear friction model 7 works similar to type 6, but introduces a limit on the friction force if plasticity is observed and is better suited to simulate; e.g., bulk forming processes. Both types 6 and 7 are always based on nodal forces.

Main Index

CONTACT with TABLES (2-D) 617 Define Two-dimensional Contact Surface

CONTACT with TABLES (2-D)

Define Two-dimensional Contact Surface

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows for the input of 2-D contact surface definition (rigid or deformable) in contact problems. It also allows you to input friction type, relative sliding velocity for sticking conditions, contact tolerance, location of center of rotation, initial angular position of surface, velocity of center of rotation, angular velocity, as well as friction coefficient. For coupled analysis, additional input is required to define the thermal, electrical, and diffusion behavior if applicable. In acoustic-solid analysis, it also allows for the input of reactive boundary conditions. Near thermal contact is only available with input version 10 or greater. Notes:

Always define deformable surfaces before rigid surfaces. Always define acoustic bodies before structural bodies.

If the UMOTION option and MOTION user subroutine are used, velocity data can be skipped. If the UFRICTION option and UFRIC user subroutine are used, friction data can be skipped, but the friction type must be identified. If, in a coupled thermal-stress-contact problem, the UHTCOEF option and UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and UHTCON user subroutine are used in a coupled thermal-stress-contact problem, film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart:

Main Index

Friction type

4th field

2nd data line

Maximum number of separations

6th field

2nd data line

Suppression of splitting

7th field

2nd data line

Relative sliding velocity

1st field

3rd data line

Contact distance

2nd field

3rd data line

Thermal close distance

3rd field

3rd data line

Separation force

5th field

3rd data line

Bias factor

6th field

3rd data line

618 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Note:

The CONTACT TABLE option offers the possibility to specify data per pair of contact bodies. Data which can be entered through the CONTACT TABLE option is designated with a red asterisk (*).

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Friction type 0: No Friction (default) 1: Shear Friction 2: Coulomb Friction 3: Shear Friction for Rolling 4: Coulomb Friction for Rolling 5: Stick-slip Coulomb Friction 6: Bilinear Coulomb Friction 7: Bilinear Shear Friction

21-25

5th

I

Enter 0 (default) for the calculation of Coulomb friction based on nodal stress. This can only be activated for friction types 1 to 4. Friction types 5 to 7 always use nodal force. Enter 1 for the calculation of Coulomb friction based on nodal force instead of nodal stress.

26-30

6th

I

Maximum number of separations allowed in each increment. Default is 9999.

31-35

7th

I

Enter 0 (default) to use the increment splitting procedure for the fixed time step procedures (AUTO LOAD, DYNAMIC CHANGE, TRANSIENT NON AUTO). Enter 1 for the suppression of the splitting of an increment in fixed time step procedure. Enter 2 for adaptive time step procedure. Default is 0.

Main Index

CONTACT with TABLES (2-D) 619 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry Enter 3 (preferred) to use contact procedure which does not require increment splitting (iterative penetration checking procedure).

36-40

8th

I

Enter 0 (default) to reset NCYCLE=0 which does not result in the initialization of the Newton-Raphson procedure. Enter 3 to not reset NCYCLE=0 when separation occurs; this speeds up the solution but might result in instabilities.

41-45

9th

I

Control separations within an increment. When 0 (default) is entered, if the force on a node is greater than the separation force, the node separates and an iteration occurs. When 1 is entered, if a node, which was in contact at the end of the previous increment, has a force greater than the separation force, the node does not separate in this increment, but separates at the beginning of the next increment. When 2 is entered, if a new node comes into contact during this increment, it is not allowed to separate during this increment (prevents chattering). When 3 is entered, both (1) and (2) above are in effect.

46-50

10th

I

Parameter governing normal direction/thickness contribution of shell (ISH). Enter 0 – Check Node Contact with top and bottom surface; including shell thickness Enter 1 – Nodes only come into contact with bottom layer Enter 2 – Nodes only come into contact with bottom layer and ignore shell thickness Enter -1 – Nodes only come into contact with top layer Enter -2 – Nodes only come into contact with top layer and ignore shell thickness

51-55

11th

I

Enter 0 (default) for full printout of the rigid surface geometry. Enter 1 to reduce printout of surface definition.

56-60

12th

I

Separation flag. This flag is related to the separation threshold entered on the 5th field of the 3rd data block and may have the following values: 0: Separation is based on nodal forces. If the contact normal force on a node in contact exceeds the threshold, the node separates. 1: Separation is based on absolute nodal stresses where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold, the node separates.

Main Index

620 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry 2: Separation is based on absolute nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 3: Separation is based on relative nodal stresses, where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. 4: Separation is based on relative nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. The default value is 0. Notice that for true quadratic contact, only stressbased separation (2 or 4) can be used.

61-65

13th

I

Not used; enter 0.

66-70

14th

I

Linearization flag, to be used if a contact body consists of quadratic elements: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

71-75

15th

I

Not used; enter 0.

76-80

16th

I

Enter 1 to get the tying information due to initial contact written into the jid.t01 file. This file can be included in a second analysis, so that (glued) contact conditions can be obtained without actually defining contact bodies in the second analysis. Enter 3 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx where xxx is the increment number the Marc format is used. Enter 4 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx. The MD Nastran MPC format is used.

Main Index

CONTACT with TABLES (2-D) 621 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

F

For friction types 1, 2, 3, or 4 enter the relative sliding velocity between bodies below which sticking is simulated (RVCNST). Default = 1.0. For friction type 5, enter the slip-to-stick transition region (β); Default is 1.e-6. For friction types 6 and 7, enter the slip threshold (δ). Default = 0.0, which means that the actual value is automatically determined.

11-20*

2nd

F

Distance below which a node is considered touching a body (ERROR). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50*

5th

F

Separation threshold. The physical meaning of this threshold (a force, a stress or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block.

51-60*

6th

F

Contact tolerance BIAS factor. (0-1) Not used for glued contact and contact with a symmetry body.

61-70

7th

F

For stick-slip model, enter the friction coefficient multiplier (α). Defaults to 1.05.

71-80

8th

F

For stick-slip model, enter the friction force tolerance (e). Defaults to 0.05.

Data blocks 4 through 22 are repeated once for each body to be defined. Numbering of Contact Bodies: When defining contact bodies for a deformable-to-deformable analysis, it is important to define them in the proper order. As a general rule, a body with a finer mesh should be defined before a body with a coarser mesh. For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change. Note:

The CONTACT TABLE option allow the contact body numbering to be either automatic or user-defined.

4th data block

Main Index

1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

622 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Format Fixed 11-15

Free 3rd

Data Entry Entry I

For deformable bodies, enter 0 if double-sided deformable-deformable contact with default search order based upon body IDs. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined. For deformable bodies, enter 2 if double-sided deformable-deformable contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option. This is recommended for simulations with global adaptive remeshing.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

For rigid bodies, enter 0 (default) if the piecewise linear representation is used. For rigid bodies, enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The user-defined coordinates of this node are ignored and replaced with the coordinates of the center of rotation given in the 5th data block. Note:

31-35

7th

I

In Mentat, the coordinates of this node are used to define the center of rotation.

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. This node number should not be the same as the node number given in the 6th field. The position of this node is at the center of rotation given in the 5th data block. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x- and y-displacement as degree of freedom 1 and 2 Node 2 has z-rotation as degree of freedom 1 The first node of a load-controlled body use the TRANSFORMATION or COORD SYSTEM option to allow for movement in user-defined directions.

Main Index

CONTACT with TABLES (2-D) 623 Define Two-dimensional Contact Surface

Format Fixed 36-40

Free 8th

Data Entry Entry I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body; 4: heat-rigid body; 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of ratio.

31-40

4th

F

Initial Angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

7th data block (Only required if a mechanical-displacement analysis) 1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Growth factor of rigid surface in first coordinate direction.

51-60

6th

F

Growth factor of rigid surface in second coordinate direction.

61-70

7th

F

Growth factor of rigid surface in third coordinate direction.

71-80*

8th

F

Friction Coefficient.

8th data block

Main Index

624 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

1-5

1st

I

Enter the table ID for the first component of velocity, or target position of center of rotation.

6-10

2nd

I

Enter the table ID for the second component of velocity, or target position of center of rotation.

11-15

3rd

I

Enter the table ID for the third component of velocity, or target position of center of rotation.

16-20

4th

I

Enter the table ID for the angular velocity.

21-25

5th

I

Enter the table ID for growth factor in first coordinate direction.

26-30

6th

I

Enter the table ID for growth factor in second coordinate direction.

31-35

7th

I

Enter the table ID for growth factor in third coordinate direction.

36-40

8th

I

Enter the table ID for the friction coefficient.

9th data block 1-10

1st

F

Heat Transfer coefficient (film) to environment (HCVE).

11-20

2nd

F

Environment sink temperature (TSINK).

21-30*

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY). (Required for rigid body only.)

41-50*

5th

F

Enter the convection coefficient for near field behavior (HCV).

51-60*

6th

F

Enter the natural convection coefficient for near field behavior (HNC).

61-70*

7th

F

Enter the exponent associated with natural convection (BNC).

71-80*

8th

F

Enter the surface emissivity ( ε ) for radiation to the environment or near thermal radiation.

10th data block The 10th data block is only necessary if heat transfer is included.

Main Index

1-5

1st

I

Enter the table ID for the heat transfer coefficient to environment (HCVE).

6-10

2nd

I

Enter the table ID for the environment sink temperature (TSINK).

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

21-25

5th

I

Enter the table ID for the convection coefficient for near field behavior (HCV).

26-30

6th

I

Enter the table ID for natural convection coefficient for near field behavior (HNC).

CONTACT with TABLES (2-D) 625 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Enter the table ID for the exponent associated with natural convection. (BNC).

36-40

8th

I

Enter the table ID for surface emissivity ( ε ) for radiation to the environment or near thermal radiation.

11th data block (Only if heat transfer is included) 1-10*

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

12th data block (Only if heat transfer is included) 1-5

1st

I

Enter the table ID associated with (HBL).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distance (s) is less than ERROR, bodies are in contact

q = H CT ( T B – T A ) .

2. If separation distance (s) is greater than ERROR, but less than DQ NEAR , and zero. DQ NEAR must be defined via the CONTACT TABLE option. q = H CV ( T B – T A ) + H NC ( T B – T A )

BNC

4

DQ NEAR

is not

4

+ σε ( T B – T A )

⎧ ⎫ S S + ⎨ H CT ⎛⎝ 1 – --------------------------⎞⎠ + H BL -------------------------- ⎬ ( T B – T A ) DQN EAR DQN EAR ⎭ ⎩

The last term is only included if HBL is not zero. The Stefan Boltzmann constant ( σ ) is entered via the PARAMETERS model definition option. Radiation is based upon the absolute temperatures using the offset temperature entered via the PARAMETERS model definition option. 3.

If separation distance S is greater than DQN EA R or E R ROR if DQN EA R defined, then convection and radiation to the environment occurs. 4

is not

4

q = H CVE ( T SI NK – T A ) + σε ( T SI NK – T A )

13th data block (Only if Joule Heating is included) 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30*

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage (Required for rigid body only).

41-50*

5th

F

Electrical transfer coefficient for near field behavior.

51-60*

6th

F

Enter the separation distance dependent electrical transfer coefficient.

14th data block (Only if Joule Heating is included) 1-5

Main Index

1st

I

Enter the table ID for the electrical transfer coefficient to environment.

626 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

6-10

2nd

I

Enter the table ID for the sink voltage.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

21-25

5th

I

Enter the table ID for the electrical transfer coefficient for near field behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent electrical transfer coefficient.

15th data block (Only used if coupled mass diffusion) 1-10

1st

E

Enter the mass flow rate coefficient to environment.

11-20

2nd

E

Enter the environment sink pressure (PSINK).

21-30*

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure (required for rigid body only).

41-50*

5th

E

Enter the mass flow rate coefficient for near field behavior.

51-60*

6th

E

Enter separation distance dependent mass flow rate coefficient.

16th data block (Only used if coupled mass diffusion) 1-5

1st

I

Enter the table ID for the mass flow rate coefficient to environment.

6-10

2nd

I

Enter the table ID for the environment sink pressure (PSINK).

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

21-25

5th

I

Enter the table ID for the mass rate coefficient for near field behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent mass flow rate coefficient.

17th data block The 17th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

1 ----c1

reactive boundary coefficient.

18th data block The 18th data block is only necessary for harmonic acoustic analysis. 1-5

Main Index

1st

I

Enter the table ID associated with

1 ----k1

reactive boundary coefficient.

CONTACT with TABLES (2-D) 627 Define Two-dimensional Contact Surface

Format Fixed 6-10

Free 2nd

Data Entry Entry I

Enter the table ID associated with

1 ----c1

reactive boundary coefficient.

The 19th through 22nd data blocks are repeated for as many geometrical data as required (NETTY). A. For 2-D Deformable Bodies 19a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 2-D Rigid Body (Line-Segment) 19b data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 20th data block is repeated once for each point entered. 20b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Circular Arc) 19c data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 20c data block is repeated four times. 20c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (Spline) 19d data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 20d data block is repeated for each point to be entered. 20d data block

Main Index

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

628 CONTACT with TABLES (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

E. For 2-D Rigid Body (NURBS) The 19e data block is repeated NPTU times for control points. 19e data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

20e data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 21e data block is repeated NPTU times for homogeneous coordinate. 21e data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 22e data block is repeated NPTU+ NORU times for knot vectors. 22e data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

CONTACT (2-D) 629 Define Two-dimensional Contact Surface

CONTACT (2-D)

Define Two-dimensional Contact Surface

The information provided here is based upon not using the table driven input style. Description This option allows for the input of 2-D contact surface definition (rigid or deformable) in contact problems. It also allows you to input friction type, relative sliding velocity for sticking conditions, contact tolerance, location of center of rotation, initial angular position of surface, velocity of center of rotation, angular velocity, as well as friction coefficient. In acoustic-solid analysis, it also allows for the input of reactive boundary conditions. Notes:

Always define deformable surfaces before rigid surfaces. Always define acoustic bodies before structural bodies.

If the UMOTION option and the MOTION user subroutine are used, velocity data can be skipped. If the UFRICTION option and the UFRIC user subroutine are used, friction data can be skipped, but the friction type must be identified. If, in a coupled thermal-stress-contact problem, the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used in a coupled thermal-stress-contact problem, film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart: Friction type

4th field

2nd data line

Maximum number of separations

6th field

2nd data line

Suppression of splitting

7th field

2nd data line

Relative sliding velocity

1st field

3rd data line

Contact distance

2nd field

3rd data line

Separation force

5th field

3rd data line

Bias factor

6th field

3rd data line

Note:

Main Index

The CONTACT TABLE option offers the possibility to specify data per pair of contact bodies. Data which can be entered through the CONTACT TABLE option is designated with a red asterisk (*).

630 CONTACT (2-D) Define Two-dimensional Contact Surface

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Friction type 0: No Friction (default) 1: Shear Friction 2: Coulomb Friction 3: Shear Friction for Rolling 4: Coulomb Friction for Rolling 5: Stick-slip Coulomb Friction 6: Bilinear Coulomb Friction 7: Bilinear Shear Friction

21-25

5th

I

Enter 0 (default) for the calculation of Coulomb friction based on nodal stress. This can only be activated for friction types 1 to 4. Friction types 5 to 7 always used nodal force. Enter 1 for the calculation of Coulomb friction based on nodal force instead of nodal stress.

26-30

6th

I

Maximum number of separations allowed in each increment. Default is 9999.

31-35

7th

I

Enter 0 (default) to use the increment splitting procedure for the fixed time step procedures (AUTO LOAD, DYNAMIC CHANGE, TRANSIENT NON AUTO). Enter 1 for the suppression of the splitting of an increment in fixed time step procedure. Enter 2 for adaptive time step procedure. Enter 3 (preferred) to use contact procedure which does not require increment splitting (iterative penetration checking procedure).

36-40

8th

I

Enter 0 (default) to reset NCYCLE = 0 which does not result in the initialization of the Newton-Raphson procedure. Enter 3 to not reset NCYCLE=0 when separation occurs; this speeds up the solution but might result in instabilities.

Main Index

CONTACT (2-D) 631 Define Two-dimensional Contact Surface

Format Fixed 41-45

Free 9th

Data Entry Entry I

Control separations within an increment. When 0 (default) is entered, if the force on a node is greater than the separation force, the node separates and an iteration occurs. When 1 is entered, if a node, which was in contact at the end of the previous increment, has a force greater than the separation force, the node does not separate in this increment, but separates at the beginning of the next increment. When 2 is entered, if a new node comes into contact during this increment, it is not allowed to separate during this increment (prevents chattering). When 3 is entered, both (1) and (2) above are in effect.

46-50

51-55

10th

11th

I

I

Parameter governing normal direction/thickness contribution of shell (ISH). Enter 0 –

Check Node Contact with top and bottom surface; including shell thickness

Enter 1 –

Nodes only come into contact with bottom layer

Enter 2 –

Nodes only come into contact with bottom layer and ignore shell thickness

Enter -1 –

Nodes only come into contact with top layer

Enter -2 –

Nodes only come into contact with top layer and ignore shell thickness

Enter 0 (default) for full print out of the rigid surface geometry. Enter 1 to reduce printout of surface definition.

56-60

12th

I

Separation flag. This flag is related to the separation threshold entered on the 5th field of the 3rd data block and may have the following values: 0: Separation is based on nodal forces. If the contact normal force on a node in contact exceeds the threshold, the node separates. 1: Separation is based on absolute nodal stresses where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 2: Separation is based on absolute nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold, the node separates.

Main Index

632 CONTACT (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry 3: Separation is based on relative nodal stresses, where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. 4: Separation is based on relative nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. The default value is 0. Notice that for true quadratic contact, only stressbased separation (2 or 4) can be used.

61-65

13th

I

Not used; enter 0.

66-70

14th

I

Linearization flag, to be used if a contact body consists of quadratic elements: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

71-75

15th

I

Not used; enter 0.

76-80

16th

I

Enter 1 to get the tying information due to initial contact written into the jid.t01 file. This file can be included in a second analysis, so that (glued) contact conditions can be obtained without actually defining contact bodies in the second analysis. Enter 3 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx where xxx is the increment number the Marc format is used. Enter 4 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx. The MD Nastran MPC format is used.

3rd data block 1-10

1st

F

For friction types 1, 2, 3, or 4 enter the relative sliding velocity between bodies below which sticking is simulated (RVCNST). Default = 1.0.

Main Index

CONTACT (2-D) 633 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry For friction type 5, enter the slip-to-stick transition region (β); Default is 10-6. For friction types 6 and 7, enter the slip threshold (δ). Default = 0.0, which means that the actual value is automatically determined.

11-20*

2nd

F

Distance below which a node is considered touching a body (ERROR). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50*

5th

F

Separation threshold. The physical meaning of this threshold (a force, a stress or a percentage of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block.

51-60*

6th

F

Contact tolerance BIAS factor. (0-1) Not used for glued contact and contact with a symmetry body.

61-70

7th

F

For stick-slip model, enter the friction coefficient multiplier (α). Defaults to 1.05

71-80

8th

F

For stick-slip and bilinear models, enter the friction force tolerance (e). Defaults to 0.05.

The 4th through the 15th data blocks are repeated once for each body to be defined. Numbering of Contact Bodies: When defining contact bodies for a deformable-to-deformable analysis, it is important to define them in the proper order. As a general rule, a body with a finer mesh should be defined before a body with a coarser mesh. For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change. Note:

The CONTACT TABLE option allow the contact body numbering to be either automatic or user-defined.

4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

For deformable bodies, enter 0 if double-sided deformable-deformable contact with default search order based upon body IDs. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used.

Main Index

634 CONTACT (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry Note that, in this case, results are dependent upon the order in which contact bodies are defined. For deformable bodies, enter 2 if double-sided deformable-deformable contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option. This is recommended for simulations with global adaptive remeshing.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

For rigid bodies, enter 0 (default) if the piecewise linear representation is used. For rigid bodies, enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The user-defined coordinates of this node are ignored and replaced with the coordinates of the center of rotation given in the 5th data block. Note:

31-35

7th

I

In Mentat, the coordinates of this node are used to define the center of rotation.

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. This node number should not be the same as the node number given in the 6th field. The position of this node is at the center of rotation given in the 5th data block. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x- and y-displacement as degree of freedom 1 and 2 Node 2 has z-rotation as degree of freedom 1 The TRANSFORMATION or COORD SYSTEM option may be used to transform the degrees of freedom on the first node to allow for movement in user-defined directions.

36-40

8th

I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body;

Main Index

CONTACT (2-D) 635 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry 4: heat-rigid body; 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis; Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

7th data block

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80*

8th

F

Friction coefficient.

636 CONTACT (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

8th data block The 8th data block is only necessary if heat transfer is included. 1-10

1st

F

Heat transfer coefficient (film) to environment ( H CVE ).

11-20

2nd

F

Environment sink temperature ( T S INK ).

21-30*

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

41-50*

5th

F

Enter the convection coefficient for near field behavior ( H CV ).

51-60*

6th

F

Enter the natural convection coefficient for near field behavior ( H NC ).

61-70*

7th

F

Enter the exponent associated with natural convection ( B NC ).

71-80*

8th

F

Enter the surface emissivity for either near field behavior or radiation to environment ( ε ).

9th data block The 9th data block is only necessary if heat transfer is included. 1-10*

1st

F

Enter the separation distance dependent heat transfer file coefficient ( H BL ).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distances ( S ) is less than

ERROR ,

bodies are in contact

2. If separation distance ( S ) is greater than ERROR , but less than defined in the CONTACT TABLE option. q = H CV ( T B – T A ) + H NC ( T B – T A )

B NC

q = H CT ( T B – T A ) .

DQ NEAR ,

and

DQ NEAR

is

+ σε ( T B4 – T A4 )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ T B – T A ⎝ D QNE A R⎠ DQ NEAR ⎭ ⎩

The last term is included only when

H BL

is not zero.

The Stefan Boltzmann constant ( σ ) is entered via the PARAMETERS model definition option. Radiation is based upon the absolute temperatures using the offset temperature entered via the PARAMETERS model definition option.

3. If separation distance

S

is greater than

DQ NEAR

or

convection and radiation to the environment occurs.

Main Index

ERROR

if

DQ NEAR

is not defined, then 4

4

q = H CVE ( T SI NK – T A ) + σε ( T SINK – T A )

CONTACT (2-D) 637 Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

10th data block The 10th data block is only necessary for Joule heating. 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30*

3rd

F

Contact electrical transfer coefficient.

31-40

4th

F

Body voltage (required for rigid body only).

41-50*

5th

F

Electrical transfer coefficient for near field behavior.

51-60*

6th

F

Enter the separation distance dependent electrical transfer coefficient.

11th data block The 11th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1---k1

reactive boundary coefficient.

11-20

2nd

F

1 ----c1

reactive boundary coefficient.

A. For 2-D Deformable Bodies The 12th through the 15th data blocks are repeated for each set of body entities (NSURGN). 12a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 2-D Rigid Body (Line-Segment) 12b data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 13b data block is repeated once for each point entered. 13b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Circular Arc) 12c data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 13c data block is repeated four times.

Main Index

638 CONTACT (2-D) Define Two-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

13c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (Spline) 12d data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 13d data block is repeated for each point to be entered. 13d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

E. For 2-D Rigid Body (NURBS) 12e data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 13e data block is repeated NPTU times for control points. 13e data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 14e data block is repeated NPTU times for homogeneous coordinate. 14e data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 15e data block is repeated NPTU+ NORU times for knot vectors. 15e data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

CONTACT with TABLES (3-D) 639 Define Three-dimensional Contact Surface

CONTACT with TABLES (3-D)

Define Three-dimensional Contact Surface

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows for the input of 3-D contact surface definition (rigid or deformable) in contact problems. It also allows you to input friction type, relative sliding velocity for sticking conditions, contact tolerance, location of center of rotation, initial angular position of surface, velocity of center of rotation, angular velocity, as well as friction coefficient. For coupled analysis, additional input is required to define the thermal, electrical, and diffusion behavior if applicable. In acoustic-solid analysis, it also allows for the input of reactive boundary conditions. Near thermal contact is only available with input version 10 or greater. Notes:

Always define deformable surfaces before rigid surfaces. Always define acoustic bodies before structural bodies.

If the UMOTION option and the MOTION user subroutine are used, velocity data can be skipped. If the UFRICTION option and the UFRIC user subroutine are used, friction data can be skipped, but the friction type must be identified. If, in a coupled thermal-stress-contact problem, the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used in a coupled thermal-stress-contact problem, film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart:

Main Index

Friction type

4th field

2nd data line

Maximum number of separations

6th field

2nd data line

Suppression of splitting

7th field

2nd data line

Relative sliding velocity

1st field

3rd data line

Contact distance

2nd field

3rd data line

Thermal close distance

3rd field

3rd data line

Separation force

5th field

3rd data line

Bias factor

6th field

3rd data line

640 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Note:

The CONTACT TABLE option offers the possibility to specify data per pair of contact bodies. Data which can be entered through the CONTACT TABLE option is designated with a red asterisk (*).

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Friction type 0: No Friction 1: Shear Friction 2: Coulomb Friction 3: Shear Friction for Rolling 4: Coulomb Friction for Rolling 5: Stick-slip Coulomb Friction 6: Bilinear Coulomb Friction 7: Bilinear Shear Friction

21-25

5th

I

Enter 0 (default) for the calculation of Coulomb friction based on nodal stress. This can only be activated for friction types 1 to 4. Friction types 5 to 7 always use nodal force. Enter 1 for the calculation of Coulomb friction based on nodal force instead of nodal stress.

26-30

Main Index

6th

I

Maximum number of separations allowed in each increment. Default is 9999.

CONTACT with TABLES (3-D) 641 Define Three-dimensional Contact Surface

Format Fixed 31-35

Free 7th

Data Entry Entry I

Enter 0 (default) to use the increment splitting procedure for the fixed time step procedures (AUTO LOAD, DYNAMIC CHANGE, TRANSIENT NON AUTO). Enter 1 for the suppression of the splitting of an increment in fixed time step procedure. Enter 2 for adaptive time step procedure. Default is 0. Enter 3 (preferred) to use contact procedure which does not require increment splitting (iterative penetration checking procedure).

36-40

8th

I

Enter 0 (default) to reset NCYCLE=0 which does not result in the initialization of the Newton-Raphson procedure. Enter 3 to not reset NCYCLE=0 when separation occurs; this speeds up the solution but might result in instabilities.

41-45

9th

I

Control separations within an increment. When 0 (default) is entered, if the force on a node is greater than the separation force, the node separates and an iteration occurs. When 1 is entered, if a node, which was in contact at the end of the previous increment, has a force greater than the separation force, the node does not separate in this increment, but separates at the beginning of the next increment. When 2 is entered, if a new node comes into contact during this increment, it is not allowed to separate during this increment (prevents chattering). When 3 is entered, both (1) and (2) above are in effect.

46-50

51-55

10th

11th

I

I

Parameter governing normal direction/thickness contribution of shell (ISH). Enter 0 –

Check Node Contact with top and bottom surface; including shell thickness

Enter 1 –

Nodes only come into contact with bottom layer

Enter 2 –

Nodes only come into contact with bottom layer and ignore shell thickness

Enter -1 –

Nodes only come into contact with top layer

Enter -2 –

Nodes only come into contact with top layer and ignore shell thickness

Enter 0 (default) for full print out of the rigid surface geometry. Enter 1 to reduce printout of surface definition.

Main Index

642 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

56-60

12th

Data Entry Entry I

Separation flag. This flag is related to the separation threshold entered on the 5th field of the 3rd data block and may have the following values: 0: Separation is based on nodal forces. If the contact normal force on a node in contact exceeds the threshold, the node separates. 1: Separation is based on absolute nodal stresses where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 2: Separation is based on absolute nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 3: Separation is based on relative nodal stresses, where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. 4: Separation is based on relative nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. The default value is 0. Notice that for true quadratic contact, only stressbased separation (2 or 4) can be used.

61-65

13th

I

Enter 1 to activate beam-to-beam contact. Enter 1+100*FREQ to activate beam-to-beam contact and write Mentat mfd-files with the given frequency that contain line segments connecting the beam-to-beam contact locations of touching beam elements.

66-70

14th

I

Linearization flag, to be used if a contact body consists of quadratic elements: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact.

Main Index

CONTACT with TABLES (3-D) 643 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry The default value is 1.

71-75

15th

I

Not used; enter 0.

76-80

16th

I

Enter 1 to get the tying information due to initial contact written into the jid.t01 file. This file can be included in a second analysis, so that (glued) contact conditions can be obtained without actually defining contact bodies in the second analysis. Enter 3 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx where xxx is the increment number the Marc format is used. Enter 4 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx. The MD Nastran MPC format is used.

3rd data block 1-10

1st

F

For friction types 1, 2, 3, or 4 enter the relative sliding velocity between bodies below which sticking is simulated (RVCNST). Default = 1.0. For friction type 5, enter the slip-to-stick transition region (β); Default is 1.e-6. For friction types 6 and 7, enter the slip threshold (δ). Default = 0.0, which means that the actual value is automatically determined.

11-20*

2nd

F

Distance below which a node is considered touching a body (ERROR). Leave blank if you want Marc to calculate it.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50*

5th

F

Separation threshold. The physical meaning of this threshold (a force, a stress or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block. Notice that the CONTACT TABLE option offers the possibility to define a separation threshold per pair of contact bodies.

51-60*

6th

F

Contact tolerance BIAS factor. (0-1) Not used for glued contact and contact with a symmetry body.

61-70

7th

F

For stick-slip model, enter the friction coefficient multiplier (α). Defaults to 1.05

71-80

8th

F

For stick-slip model, enter the friction force tolerance (e). Defaults to 0.05.

Data blocks 4 through 26 are repeated once for each body to be defined.

Main Index

644 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

Numbering of Contact Bodies: When defining contact bodies for a deformable-to-deformable analysis, it is important to define them in the proper order. As a general rule, a body with a finer mesh should be defined before a body with a coarser mesh. For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change. Note:

The CONTACT TABLE option allow the contact body numbering to be either automatic or user-defined.

4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

For deformable bodies, enter 0 (default) if double-sided deformabledeformable contact with default search order based upon body IDs. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined. For deformable bodies, enter 2 if double-sided deformable-deformable contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option. This is recommended for simulations with global adaptive remeshing.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

For rigid bodies, enter 0 (default) if the piecewise linear representation is used. For rigid bodies, enter 1 if analytic form is to be used. This is required if trimmed NURBS are entered.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The user-defined coordinates of this node are ignored and replaced with the coordinates of the center of rotation given in the 5th data block. Note:

Main Index

In Mentat, the coordinates of this node are used to define the center of rotation.

CONTACT with TABLES (3-D) 645 Define Three-dimensional Contact Surface

Format Fixed 31-35

Free 7th

Data Entry Entry I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. This node number should not be the same as the node number given in the 6th field. The position of this node is at the center of rotation given in the 5th data block. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/ other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

36-40

8th

I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body; 4: heat-rigid body; 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of ratio.

31-40

4th

F

Initial Angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0

6th data block

Main Index

1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

646 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

7th data block 1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Growth factor of rigid surface in first coordinate direction.

51-60

6th

F

Growth factor of rigid surface in second coordinate direction.

61-70

7th

F

Growth factor of rigid surface in third coordinate direction.

71-80*

8th

F

Friction Coefficient.

8th data block 1-5

1st

I

Enter the table ID for the first component of velocity, or target position of center of rotation.

6-10

2nd

I

Enter the table ID for the second component of velocity, or target position of center of rotation.

11-15

3rd

I

Enter the table ID for the third component of velocity, or target position of center of rotation.

16-20

4th

I

Enter the table ID for the angular velocity.

21-25

5th

I

Enter the table ID for growth factor in first coordinate direction.

26-30

6th

I

Enter the table ID for growth factor in second coordinate direction.

31-35

7th

I

Enter the table ID for growth factor in third coordinate direction.

36-40

8th

I

Enter the table ID for the friction coefficient.

The 9th data block is only necessary if heat transfer is included. 9th data block

Main Index

1-10

1st

F

Heat Transfer coefficient (film) to environment (HCVE).

11-20

2nd

F

Environment sink temperature (TSINK).

21-30*

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY). (Required for rigid body only.)

41-50

5th

F

Enter the convection coefficient for near field behavior (HCV).

CONTACT with TABLES (3-D) 647 Define Three-dimensional Contact Surface

Format

Data Entry Entry

Fixed

Free

51-60*

6th

F

Enter the natural convection coefficient for near field behavior (HNC).

61-70*

7th

F

Enter the exponent associated with natural convection (BNC).

71-80*

8th

F

Enter the surface emissivity ( ε ) for radiation to the environment or near thermal radiation.

The 10th data block is only necessary if heat transfer is included. 10th data block 1-5

1st

I

Enter the table ID for the heat transfer coefficient to environment (HCVE).

6-10

2nd

I

Enter the table ID for the environment sink temperature (TSINK).

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

21-25

5th

I

Enter the table ID for the convection coefficient for near field behavior (HCV).

26-30

6th

I

Enter the table ID for natural convection coefficient for near field behavior (HNC).

31-35

7th

I

Enter the table ID for the exponent associated with natural convection. (BNC).

36-40

8th

I

Enter the table ID for surface emissivity ( ε ) for radiation to the environment or near thermal radiation.

11th data block (Only if heat transfer is included) 1-10*

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

12th data block (Only if heat transfer is included) 1-5

1st

I

Enter the table ID associated with (HBL).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distance (s) is less than ERROR, bodies are in contact

q = H CT ( T B – T A )

2. If separation distance (s) is greater than ERROR, but less than DQ NE A R , and zero. DQ NEAR must be defined via the CONTACT TABLE option. q = H CV ( T B – T A ) + H NC ( T B – T A )

BNC

4

4

+ σε ( T B – T A )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ ( T B – T A ) ⎝ DQN EAR⎠ DQN EAR ⎭ ⎩

Main Index

DQ NE A R

.

is not

648 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

The last term is only included if HBL is not zero. The Stefan Boltzmann constant ( σ ) is entered via the PARAMETERS model definition option. Radiation is based upon the absolute temperatures using the offset temperature entered via the PARAMETERS model definition option.

3. If separation distance

S

is greater than DQ NEAR or

E R ROR

convection and radiation to the environment occurs.

if

DQ NEAR

is not defined, then 4

4

q = H CVE ( T SI NK – T A ) + σε ( T SI NK – T A )

13th data block (Only if Joule Heating is included) 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30*

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage (Required for rigid body only).

41-50*

5th

F

Electrical transfer coefficient for near field behavior.

51-60*

6th

F

Enter the separation distance dependent electrical transfer coefficient.

14th data block (Only if Joule Heating is included) 1-5

1st

I

Enter the table ID for the electrical transfer coefficient to environment.

6-10

2nd

I

Enter the table ID for the sink voltage.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

21-25

5th

I

Enter the table ID for the electrical transfer coefficient for near field behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent electrical transfer coefficient.

15th data block (Only used if coupled mass diffusion)

Main Index

1-10

1st

E

Enter the mass flow rate coefficient to environment.

11-20

2nd

E

Enter the environment sink pressure (PSINK).

21-30*

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure (required for rigid body only).

41-50*

5th

E

Enter the mass flow rate coefficient for near field behavior.

51-60*

6th

E

Enter separation distance dependent mass flow rate coefficient.

CONTACT with TABLES (3-D) 649 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

16th data block (Only used if coupled mass diffusion) 1-5

1st

I

Enter the table ID for the mass flow rate coefficient to environment.

6-10

2nd

I

Enter the table ID for the environment sink pressure (PSINK).

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

21-25

5th

I

Enter the table ID for the mass rate coefficient for near behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent mass flow rate coefficient.

17th data block The 17th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

1---c1

reactive boundary coefficient.

18th data block The 18th data block is only necessary for harmonic acoustic analysis. 1-5

1st

I

Enter the table ID associated with

1---k1

reactive boundary coefficient.

6-10

2nd

I

Enter the table ID associated with

1---c1

reactive boundary coefficient.

The 19th through 26th data blocks are repeated for each set of body entities (NSURGN). A. For 3-D Deformable Body 19a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 3-D Rigid Body (Ruled Surface) 19b data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

Main Index

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

650 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed 21-25

Free 5th

Data Entry Entry I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 20b data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 20b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

C. For 3-D Rigid Body (Surface of Revolution) 19c data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 Method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 20c data block is repeated NPOINT times for surface of revolution. 20c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

21c data block

Main Index

1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

CONTACT with TABLES (3-D) 651 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

D. For 3-D Rigid Surface (Bezier Surface) 19d data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 20d data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 20d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

E. For 3-D Rigid Surface (4-Node Patch) 19e data block 1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

16-20

4th

I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 20e data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1) 20e data block

Main Index

1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

652 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 21e data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 21e data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

F. For 3-D Rigid Surface (Poly-Surface) 19f data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 20f data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 20f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

G. For 3-D Rigid Surface (NURBS) 19g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 20g data block is repeated (NPTU ∗ NPTV) for control points. 20g data block

Main Index

CONTACT with TABLES (3-D) 653 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 21g data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 21g data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 22g data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 22g data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 23g, 24g, 25g, and 26g. 23g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 24g data block is repeated NPTU times for control points. 24g data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 25g data block is repeated NPTU times for homogeneous coordinate. 25g data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 26g data block is repeated NPTU+ NORU times for knot vectors. 26g data block 1-10

1st

F

Component of knot vector between 0 and 1.

H. For 3-D Rigid Surface (Cylinder) 19h data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

20h data block

Main Index

1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

654 CONTACT with TABLES (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

I. For 3-D Rigid Surface (Sphere) 19i data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

20i data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

CONTACT (3-D) 655 Define Three-dimensional Contact Surface

CONTACT (3-D)

Define Three-dimensional Contact Surface

The information provided here is based upon not using the table driven input style. Description This option allows for the input of 3-D contact surface definition (rigid or deformable) in contact problems. It also allows you to input friction type, relative sliding velocity for sticking condition, contact tolerance, location of center of rotation, initial angular position of surface, velocity of center of rotation, angular velocity, as well as friction coefficient. In acoustic-solid analysis it also allows for the input of reactive boundary conditions. Notes:

Always define deformable surfaces before rigid surfaces. Always define acoustic bodies before structural bodies.

If the UMOTION option and the MOTION user subroutine are used, velocity data can be skipped. If the UFRICTION option and the UFRIC or UFRICBBC user subroutine are used, friction data can be skipped, but the friction type must be identified. If, in a coupled thermal-stress-contact problem, the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used in a coupled thermal-stress-contact problem, film coefficient data between surfaces in contact can be skipped. If the 4-node patch option for the definition of rigid surface and the DIGEOM user subroutine are used, the coordinates of the patches can be skipped. The following data can be changed upon restart:

Main Index

Friction type

4th field

2nd data line

Maximum number of separations

6th field

2nd data line

Suppression of splitting

7th field

2nd data line

Relative sliding velocity

1st field

3rd data line

Contact distance

2nd field

3rd data line

Separation force

5th field

3rd data line

Bias factor

6th field

3rd data line

Frequency for writing beam-to-beam contact location mfd-files

13th field

2nd data line

656 CONTACT (3-D) Define Three-dimensional Contact Surface

Note:

The CONTACT TABLE option offers the possibility to specify data per pair of contact bodies. Data which can be entered through the CONTACT TABLE option is designated with a red asterisk (*).

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Friction type: 0: No Friction (default) 1: Shear Friction 2: Coulomb Friction 3: Shear Friction for Rolling 4: Coulomb Friction for Rolling 5: Stick-slip Coulomb Friction 6: Bilinear Coulomb Friction 7: Bilinear Shear Friction

21-25

5th

I

Enter 0 (default) for the calculation of Coulomb friction based on nodal stress. This can only be activated for friction types 1 to 4. Friction types 5 to 7 always use nodal force. Enter 1 for the calculation of Coulomb friction based on nodal force instead of nodal stress.

26-30

6th

I

Maximum of separations allowed in each increment. Default is 9999.

31-35

7th

I

Enter 0 (default) to use the increment splitting procedure for the fixed time step procedures (AUTO LOAD, DYNAMIC CHANGE, TRANSIENT NON AUTO). Enter 1 for the suppression of the splitting of an increment in fixed time procedure. Enter 2 for adaptive time stepping procedure.

Main Index

CONTACT (3-D) 657 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry Enter 3 (preferred) to use contact procedure which does not require increment splitting (iterative penetration checking procedure).

36-40

8th

I

Enter 0 (default) to reset NCYCLE=0 which does not result in the initialization of the Newton-Raphson procedure. Enter 3 to not reset NCYCLE = 0; this speeds up the solution but might result in instabilities (not relevant for iterative penetration check).

41-45

9th

I

Control separations within an increment. When 0 (default) is entered, if the force on a node is greater than the separation force, the node separates and an iteration occurs. When 1 is entered, if a node which was in contact at the end of the previous increment has a force greater than the separation force, the node does not separate in this increment, but separates at the beginning of the next increment. When 2 is entered, if a new node comes into contact during this increment, it is not allowed to separate during this increment (prevents chattering). When 3 is entered, both (1) and (2) above is in effect.

46-50

10th

I

Parameter governing normal direction/thickness contribution of shell (ISH). Enter 0 – Check Node Contact with top and bottom surface; including shell thickness Enter 1 – Nodes only come into contact with bottom layer Enter 2 – Nodes only come into contact with bottom layer and ignore shell thickness Enter -1 – Nodes only come into contact with top layer Enter -2 – Nodes only come into contact with top layer and ignore shell thickness

51-55

11th

I

Enter 0 (default) for full printout of the rigid surface geometry. Enter 1 to reduce printout of surface definition.

56-60

12th

I

Separation flag. This flag is related to the separation threshold entered on the 5th field of the 3rd data block and may have the following values: 0: Separation is based on nodal forces. If the contact normal force on a node in contact exceeds the threshold, the node separates. 1: Separation is based on absolute nodal stresses where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold, the node separates.

Main Index

658 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry 2: Separation is based on absolute nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 3: Separation is based on relative nodal stresses, where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. 4: Separation is based on relative nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. The default value is 0. Notice that for true quadratic contact, only stress-based separation (2 or 4) can be used.

61-65

13th

I

Enter 1 to activate beam-to-beam contact. Enter 1+100*FREQ to activate beam-to-beam contact and write Mentat mfd-files with the given frequency that contain line segments connecting the beam-to-beam contact locations of touching beam elements.

66-70

14th

I

Linearization flag, to be used if a contact body consists of quadratic elements: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

71-75

15th

I

Not used; enter 0.

76-80

16th

I

Enter 1 to get the tying information due to initial contact written into the jid.t01 file. This file can be included in a second analysis, so that (glued) contact conditions can be obtained without actually defining contact bodies in the second analysis. Enter 3 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx where xxx is the increment number the Marc format is used.

Main Index

CONTACT (3-D) 659 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry Enter 4 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx. The MD Nastran MPC format is used.

3rd data block 1-10

1st

F

For friction types 1, 2, 3, or 4 enter the relative sliding velocity between bodies below which sticking is simulated (RVCNST). Default is 1.0. For friction type 5, enter the slip-to-stick transition region (β); Default is 10-6. For friction types 6 and 7, enter the slip threshold (δ). Default = 0.0, which means that the actual value is automatically determined.

11-20*

2nd

F

Distance below which a node is considered touching a body (ERROR). Leave it blank if you want Marc to calculate it.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50*

5th

F

Separation threshold. The physical meaning of this threshold (a force, a stress or a percentage of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block.

51-60*

6th

F

Contact tolerance BIAS factor. (0-1) Not used for glued contact and contact with a symmetry body.

61-70

7th

F

For stick-slip model, enter the friction coefficient multiplier (α). Defaults to 1.05

71-80

8th

F

For stick-slip model and bilinear models, enter the friction force tolerance (e). Defaults to 0.05.

The 4th through the 15th data blocks are repeated once for each body to be defined. Numbering of Contact Bodies: When defining contact bodies for a deformable-to-deformable analysis, it is important to define them in the proper order. As a general rule, a body with a finer mesh should be defined before a body with a coarser mesh. For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change. Note:

The CONTACT TABLE option allow the contact body numbering to be either automatic or user-defined.

4th data block

Main Index

1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of body entities, NSURGN, to be input for this rigid body. Enter 0 if deformable body.

660 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed 11-15

Free 3rd

Data Entry Entry I

For deformable bodies, enter 0 if double-sided deformable-deformable contact with default search order based upon body IDs. For rigid bodies, enter 1 if body is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that in this case, results are dependent upon the order in which contact bodies are defined. For deformable bodies, enter 2 if double-sided deformable-deformable contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option. This is recommended for simulations with global adaptive meshing.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

For rigid bodies, enter 0 (default) if the piecewise linear representation is used. For rigid bodies, enter 1 if analytic form is to be used. This is required if trimmed NURBS are entered.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The user-defined coordinates of this node are ignored and replaced with the coordinates of the center of rotation given in the 5th data block. Note:

31-35

7th

I

In Mentat, the coordinates of this node are used to define the center of rotation.

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. This node number should not be the same as the node number given in the 6th field. The position of this node is at the center of rotation given in the 5th data block. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz

Main Index

CONTACT (3-D) 661 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

36-40

8th

I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body; 4: heat-rigid body; 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis; Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

7th data block

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

662 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80*

8th

F

Friction coefficient.

8th data block The 8th data block is only necessary if heat transfer is included. 1-10

1st

F

Heat transfer coefficient (film) to environment ( H CVE ).

11-20

2nd

F

Environment sink temperature ( T S INK ).

21-30*

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

41-50*

5th

F

Enter the convection coefficient for near field behavior ( H CV ).

51-60*

6th

F

Enter the natural convection coefficient for near field behavior ( H NC ).

61-70*

7th

F

Enter the exponent associated with natural convection ( B NC ).

71-80*

8th

F

Enter the surface emissivity for either near field behavior or radiation to environment ( ε ).

9th data block The 9th data block is only necessary if heat transfer is included. 1-10*

1st

F

Enter the separation distance dependent heat transfer file coefficient ( H BL ).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distances ( S ) is less than

ERROR ,

bodies are in contact

2. If separation distance ( S ) is greater than E R R OR , but less than defined in the CONTACT TABLE option. q = H CV ( T B – T A ) + H NC ( T B – T A )

B NC

q = H CT ( T B – T A ) .

DQ NE A R ,

and

DQ NE A R

is

+ σε ( T B4 – T A4 )

⎧ ⎫ S S + ⎨ H CT ⎛⎝ 1 – --------------------------⎞⎠ + H BL -------------------------- ⎬ T B – T A D QNE A R DQ NEAR ⎩ ⎭

The last term is included only when

H BL

is not zero.

The Stefan Boltzmann constant ( σ ) is entered via the PARAMETERS model definition option.

Main Index

CONTACT (3-D) 663 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

Radiation is based upon the absolute temperatures using the offset temperature entered via the PARAMETERS model definition option. 3. If separation distance S is greater than DQ NEAR or ERROR if convection and radiation to the environment occurs. 4

DQ NEAR

is not defined, then

4

q = H CVE ( T SINK – T A ) + σε ( T SINK – T A )

10th data block The 10th data block is only necessary for Joule heating. 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30*

3rd

F

Contact electrical transfer coefficient.

31-40

4th

F

Body voltage (required for rigid body only).

41-50*

5th

F

Electrical transfer coefficient for near field behavior.

51-60*

6th

F

Enter the separation distance dependent electrical transfer coefficient.

11th data block The 11th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1---k1

reactive boundary coefficient.

11-20

2nd

F

1---c1

reactive boundary coefficient.

A. For 3-D Deformable Body The 12th through the 19th data blocks are repeated for each set of body entities (NSURGN). 12a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 3-D Rigid Body (Ruled Surface) 12b data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

Main Index

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

664 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed 21-25

Free 5th

Data Entry Entry I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 13b data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 13b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

C. For 3-D Rigid Body (Surface of Revolution) 12c data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 Method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 13c data block is repeated NPOINT times for surface of revolution. 13c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

14c data block

Main Index

1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

CONTACT (3-D) 665 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

D. For 3-D Rigid Surface (Bezier Surface) 12d data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 13d data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 13d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

E. For 3-D Rigid Surface (4-Node Patch) 12e data block 1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

16-20

4th

I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 13e data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1) 13e data block

Main Index

1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

666 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 14e data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 14e data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

F. For 3-D Rigid Surface (Poly-Surface) 12f data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 13f data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 13f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

G. For 3-D Rigid Surface (NURBS) 12g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 13g data block is repeated (NPTU ∗ NPTV) for control points. 13g data block

Main Index

CONTACT (3-D) 667 Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 14g data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 14g data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 15g data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 15g data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 16g, 17g, 18g, and 19g. 16g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 17g data block is repeated NPTU times for control points. 17g data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 18g data block is repeated NPTU times for homogeneous coordinate. 18g data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 19g data block is repeated NPTU + NORU times for knot vectors. 19g data block 1-10

1st

F

Component of knot vector between 0 and 1.

H. For 3-D Rigid Surface (Cylinder) 12h data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

13h data block

Main Index

1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

668 CONTACT (3-D) Define Three-dimensional Contact Surface

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

I. For 3-D Rigid Surface (Sphere) 12i data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

13i data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

CONTACT TABLE with TABLES (Model Definition) 669 Define Contact Table

CONTACT TABLE with TABLES (Model Definition)

Define Contact Table

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option overrides information provided on the CONTACT option to allow the user to give more detailed information concerning the interaction of the bodies. In particular, this option allows you to specify which bodies contact which other bodies, and what is their behavior after contact occurs. If this option is not included, the default for contact analysis is that every body detects the possibility of contact with all other bodies, and itself if it is a flexible body. When the CONTACT TABLE option is entered, the default of detection for every body is overridden. Instead, you specify the relationship of detection between bodies for contact. The touching body does not contact itself unless you request it. This is useful for deactivating or activating bodies to either reduce computational costs, or because the physical process (such as manufacturing) involves multiple stages with different body interactions. Whenever the touched body is a flexible one, by default, the capability of double-sided contact is applied between the contacting bodies. This can be switched off by selecting single-sided contact on the CONTACT option or by setting the searching order in the CONTACT TABLE option. A positive value of the interference closure implies that there is an overlap between the bodies; a negative value implies that a gap exists. In addition, you can invoke the glue option, delayed slide off a deformable body, and stress-free initial contact. In the glue option, when a node contacts a rigid body, the relative tangential displacement is zero. When a node contacts a deformable body, all the translational degrees of freedom are tied. By default, if a node slides off the boundary of a deformable body at a sharp corner by a distance more than the contact tolerance, contact between the node and the contacted body is lost. By invoking the delayed sliding off option, the tangential contact tolerance is increased by a user-defined value. In any static contact analysis, a node contacting a body is projected onto the contacted segment of this body. Due to inaccuracies in the finite element model, this might introduce undesired stress changes, since an overlap or a gap between the node and the contacted segment will be closed. The option for stress-free initial contact forces a change of the coordinates of a node contacting a deformable body, thus avoiding the stress changes. In combination with the glue option, a similar effect can be obtained; however, the overlap or gap remains. The following control variables of contact between bodies can be modified throughout the table: contact tolerance, separation threshold, friction coefficient, interference closure and contact heat transfer and electrical coefficients. For an acoustic-solid analysis, you can also modify the reactive boundary coefficients.

Main Index

670 CONTACT TABLE with TABLES (Model Definition) Define Contact Table

The near thermal contact option can only be invoked using the CONTACT TABLE option. In this case, one must specify the distance at which near thermal contact occurs and the additional parameters to control the thermal (and electrical) flux. The previous value of those control variables is not overridden unless nonzero values are entered here. Notes:

This option should be placed after the CONTACT option. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT TABLE after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONTACT TABLE.

2nd data block 1-5

1st

I

Enter the number of sets of bodies to be input.

6-10

2nd

I

Enter the version number for reading the CONTACT TABLE block. Enter 2 if the 5th, 8th, 9th, 16th, 17th, 18th, and 19th data blocks are to be read to control contact, ungluing, and multiphysics. Default is 0.

The 3rd through the 22nd data blocks are entered once for each set of bodies to be input. 3rd data block 1-5

1st

I

Enter the touching body number.

6-15

2nd

F

Enter the contact tolerance ( E R R OR ).

16-25

3rd

F

Enter the distance below which near thermal or electrical contact behavior occurs ( DQ NE A R ). A 0 entered here indicates that near contact behavior is not included.

26-35

4th

F

Not used; enter 0.

36-45

5th

F

Not used; enter 0.

46-55

6th

F

Not used; enter 0.

56-65

7th

F

Enter 0 (default) if there is no additional constraint on the tangential displacement when contact occurs. No constraints are placed on rotational degrees of freedom. Enter 1 to insure that there is no relative tangential displacement when the node comes into contact. A possible relative normal displacement might originate from an initial gap or overlap between the node and the contacted body, as the node will be projected onto the contacted body.

Main Index

CONTACT TABLE with TABLES (Model Definition) 671 Define Contact Table

Format Fixed

Free

Data Entry Entry Enter 2 to insure that there is no relative tangential and normal displacement when the node comes into contact. An existing initial gap or overlap between the node and the contacted body is not removed, as the node is not projected onto the contacted body. Enter 3 to insure full moment carrying glue when shells contact. The node will be projected onto the contacted body. Enter 4 to insure full moment carrying glue when shells contact. The node will not be projected onto the contact body.

66-70

8th

I

Enter 0 (default) if search order is based upon first checking bodies with lower body number versus bodies with higher body number. Enter 1 to indicate that the searching order for deformable contact bodies is from the touching body to the touched bodies on the 5th data block. This might change the default order for deformable bodies, which is from bodies with a lower number to bodies with a higher number. Enter 2 to let the program decide which searching order is optimal for deformable bodies. This order is set up such that searching is done starting with the body having the smallest element edge. This option forces singlesided contact between the touching and touched bodies: searching is done only from one body to another and not the other way around.

71-75

9th

I

Enter 0 (default) if during initial contact, a projection onto the contact surface induces a stress. Enter 1 to modify the coordinates of a node in contact with a deformable body so that stress-free initial contact can be obtained. Enter 2 to extend the tangential error tolerance at sharp corners of deformable bodies to delay sliding off a contacted segment. Enter 3 to have both 1 and 2 active.

76-80

10th

I

Only relevant if the glue option is invoked and the separation force has not been set. Enter 0 (default) if a node should not separate. Enter 1 to invoke the separation behavior procedure, as specified on the 12th field of the 2nd data block of the CONTACT option. Enter 2 to invoke the breaking glue capability. A node will be released if the break criterion is fulfilled. Then the node will do regular contact with separation instead of being glued. The stress limits for this capability are specified in the 8th data block below.

Main Index

672 CONTACT TABLE with TABLES (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter the table ID for the contact tolerance.

11-15

3rd

I

Enter the table ID for the near contact distance.

5th data block Only required if version number is equal to 2. 1-5

1st

I

Enter the boundary description flag for the touching body (entered on the 3rd data block).

6-10

2nd

I

Enter the boundary description flag for the touched body (entered on the 18th data block).

The boundary description flag is given by A+10*B+1000*C, where parameter A is related to continuum elements in a body, parameter B is related to shell elements in a body and parameter C is related to beam elements and/or shell edges in a body. The possible values of these parameters and their meaning are: A = 1:

the outside edges (2-D) or faces (3-D) of continuum elements are included in the boundary description (default).

B = 1:

both top and bottom faces, including thickness offset, are included in the boundary description.

B = 2:

only bottom faces, including thickness offset, are included in the boundary description.

B = 3:

only bottom faces, ignoring thickness offset, are included in the boundary description.

B = 4:

only top faces, including thickness offset, are included in the boundary description.

B = 5:

only top faces, ignoring thickness offset, are included in the boundary description.

B = 6:

both top and bottom faces, ignoring thickness offset, are included in the boundary description. The default value of B depends on the parameter governing the normal direction/thickness contribution of shell elements as entered on the CONTACT option. Note:

Main Index

The choice B = 6 for both bodies in a contact combination is only meaningful for glued contact. If in such cases separation is allowed, separated nodes will not come into contact anymore, unless a new CONTACT TABLE is defined to reset the value of B.

C = 0:

neither beam elements nor shell edges are included in the boundary description.

C = 1:

beam elements are included in the boundary description (allowing for beam-tobeam contact).

CONTACT TABLE with TABLES (Model Definition) 673 Define Contact Table

Format Fixed

Free

Data Entry Entry

C = 10:

shell edges are included in the boundary description.

C = 11:

both beam elements and shell edges are included in the boundary description. If beam-to-beam contact is not activated on the CONTACT option, the default value of C is 0, otherwise the default value is 1.

6th data block Only required if a mechanical-displacement solution is obtained. 1-10

1st

F

Enter the contact separation threshold. The physical meaning of this threshold (a force, a stress, or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block of the CONTACT option.

11-20

2nd

F

Enter the friction coefficient.

21-30

3rd

F

Enter the interference closure amount, normal to the contact surface.

31-40

4th

F

Enter the friction stress limit

σ limit .

This entry is only used for friction type 6 (Coulomb friction using the bilinear model). If the shear stress due to friction reaches this limit value, then the applied friction force will be reduced so that the maximum friction stress is given by min ( μ σ n ,σ limit ) , with μ the friction coefficient and σ n the contact normal stress. Default for this entry is 1.e20.

Main Index

41-50

5th

F

Enter the contact tolerance BIAS factor (0-1). This value will overrule the BIAS factor entered on the 6th field of the 3rd data block of the CONTACT option if nonzero.

51-60

6th

F

Enter the delayed slide off distance (this entry is only used if delayed slide off has been activated by the 9th entry of the 3rd data block). When using the delayed slide off option, a node sliding on a segment will slide off this segment only if it passes the node (2-D) or edge (3-D) at a sharp corner over a distance larger than the delayed slide off distance. By default, the delayed slide off distance is related to the dimensions of the contacted segment by a 20 percent increase of its isoparametric domain.

61-70

7th

F

Enter the hard-soft ratio (this entry is only used if double-sided contact with automatic constraint optimization is used, as defined on the 4th data block of the CONTACT option). The hard-soft ratio can be used by the program if there is a significant difference in the (average) stiffness of the contact bodies (expressed by the trace of the initial stress-strain law). If the ratio of the stiffnesses is larger than the hard-soft ratio, the nodes of the softest body are the preferred slave nodes. By default, the hard-soft ratio is 2.

674 CONTACT TABLE with TABLES (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

7th data block Only required if a mechanical-displacement solution is obtained. 1-5

1st

I

Enter the table ID for the contact separation threshold.

6-10

2nd

I

Enter the table ID for the friction coefficient.

11-15

3rd

I

Enter the table ID for the interface closure amount.

16-20

4th

I

Enter the table ID for the friction stress limit.

8th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-10

1st

F

Normal stress to break glued contact (SN).

11-20

2nd

F

Tangential stress to break glued contact (ST).

21-30

3rd

F

Enter exponent for breaking normal stress term (m). Default = 2.

31-40

4th

F

Enter exponent for breaking tangential stress term (n). Default = 2. The glue breaks when

m

n

( σ N ⁄ SN ) + ( σ T ⁄ ST ) > 1

9th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-5

1st

I

Enter the table ID associated with normal stress to break glued contact.

6-10

2nd

I

Enter the table ID associated with tangential stress to break glued contact.

11-15

3rd

I

Enter the table ID associated with exponent of normal stress term.

16-20

4th

I

Enter the table ID associated with exponent of tangential stress term.

10th data block Only required if heat transfer is included.

Main Index

1-10

1st

F

Enter the contact heat transfer coefficient. (HCT)

11-20

2nd

F

Enter the convection heat transfer coefficient for near behavior. (HCV)

21-30

3rd

F

Enter the natural convection heat transfer coefficient for near behavior. (HNC)

31-40

4th

F

Enter the exponent associated with the natural convection for near behavior. (BNC)

41-50

5th

F

Enter the surface emissivity. (ε)

51-60

6th

F

Enter the separation distance dependent thermal convection coefficient. (HBL)

CONTACT TABLE with TABLES (Model Definition) 675 Define Contact Table

Format Fixed

Free

Data Entry Entry

11th data block Only required if heat transfer is included. 1-5

1st

I

Enter the table ID for the contact heat transfer coefficient.

6-10

2nd

I

Enter the table ID for the heat transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID for the natural convection heat transfer coefficient for near behavior.

16-20

4th

I

Enter the table ID for the exponent associated with the natural convection for near behavior.

21-25

5th

I

Enter the table ID for the surface emissivity.

26-30

6th

I

Enter the table ID for the separation dependent thermal convection coefficient.

12th data block Only required for Joule heating. 1-10

1st

F

Enter the contact electrical coefficient (coupled Joule analysis only).

11-20

2nd

F

Enter the electrical transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent electrical transfer coefficient.

13th data block Only required for Joule heating. 1-5

1st

I

Enter the table ID associated with the contact electrical coefficient.

6-10

2nd

I

Enter the table ID associated with the electrical transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID associated with the separation distance dependent electrical transfer coefficient.

14th data block Only required for coupled mass diffusion analysis.

Main Index

1-10

1st

F

Enter the contact mass transfer coefficient).

11-20

2nd

F

Enter the mass transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent mass diffusion coefficient.

676 CONTACT TABLE with TABLES (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

15th data block Only required for coupled mass diffusion analysis. 1-5

1st

I

Enter the table ID associated with the contact mass transfer coefficient.

6-10

2nd

I

Enter the table ID associated with the mass transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID associated with the separation distance dependent mass diffusion coefficient.

16th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-10

1st

F

Not used; enter 0.

17th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-5

1st

I

Not used; enter 0.

18th data block Only required if magnetostatic analysis is included. 1-10

1st

F

Not used; enter 0.

19th data block Only required if magnetostatic analysis is included. 1-5

1st

I

Not used; enter 0.

20th data block Only required for harmonic acoustic analysis.

Main Index

1-10

1st

F

Enter the

1---k1

reactive boundary coefficient.

11-20

2nd

F

Enter the

1---c1

reactive boundary coefficient.

CONTACT TABLE with TABLES (Model Definition) 677 Define Contact Table

Format Fixed

Free

Data Entry Entry

21st data block Only required for harmonic acoustic analysis. 1-5

1st

I

Enter the table ID for the

1 ----k1

reactive boundary coefficient.

6-10

2nd

I

Enter the table ID for the

1 ----c1

reactive boundary coefficient.

22nd data block Enter a list of touched bodies for which the touching body detects contact with the parameters above.

Main Index

678 CONTACT TABLE (Model Definition) Define Contact Table

CONTACT TABLE (Model Definition)

Define Contact Table

The information provided here is based upon not using the table driven input style. Description This option overrides information provided on the CONTACT option to allow the user to give more detailed information concerning the interaction of the bodies. In particular, this option allows you to specify which bodies contact which other bodies, and what is their behavior after contact occurs. If this option is not included, the default for contact analysis is that every body detects the possibility of contact with all other bodies, and itself if it is a flexible body. When the CONTACT TABLE option is entered, the default of detection for every body is overridden. Instead, you specify the relationship of detection between bodies for contact. The touching body does not contact itself unless you request it. This is useful for deactivating or activating bodies to either reduce computational costs, or because the physical process (such as manufacturing) involves multiple stages with different body interactions. Whenever the touched body is a flexible one, by default, the capability of double-sided contact is applied between the contacting bodies. This can be switched off by selecting single-sided contact on the CONTACT option or by setting the searching order in the CONTACT TABLE option. A positive value of the interference closure implies that there is an overlap between the bodies; a negative value implies that a gap exists. In addition, you can invoke the glue option, delayed slide off a deformable body, and stress-free initial contact. In the glue option, when a node contacts a rigid body, the relative tangential displacement is zero. When a node contacts a deformable body, all the translational degrees of freedom are tied. By default, if a node slides off the boundary of a deformable body at a sharp corner by a distance more than the contact tolerance, contact between the node and the contacted body is lost. By invoking the delayed sliding off option, the tangential contact tolerance is increased by a user-defined value. In any static contact analysis, a node contacting a body is projected onto the contacted segment of this body. Due to inaccuracies in the finite element model, this might introduce undesired stress changes, since an overlap or a gap between the node and the contacted segment will be closed. The option for stress-free initial contact forces a change of the coordinates of a node contacting a deformable body, thus avoiding the stress changes. In combination with the glue option, a similar effect can be obtained; however, the overlap or gap remains. The following control variables of contact between bodies can be modified throughout the table: contact tolerance, separation threshold, friction coefficient, interference closure and contact heat transfer and electrical coefficients. For an acoustic-solid analysis, you can also modify the reactive boundary coefficients.

Main Index

CONTACT TABLE (Model Definition) 679 Define Contact Table

The near thermal contact option can only be invoked using the CONTACT TABLE option. In this case, one must specify the distance at which near thermal contact occurs and the additional parameters to control the thermal (and electrical) flux. The previous value of those control variables is not overridden unless nonzero values are entered here. Notes:

This option should be placed after the CONTACT option. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT TABLE after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONTACT TABLE.

2nd data block 1-5

1st

I

Enter the number of sets of bodies to be input.

6-10

2nd

I

Enter the version number for reading the CONTACT TABLE block. Enter 2 if the 4th, 6th, 10th, and 11th data blocks are to be read to control contact, ungluing, and multiphysics. Default is 0.

The 3rd through the 13th data blocks are entered once for each set of bodies to be input. 3rd data block 1-5

1st

I

Enter the touching body number.

6-15

2nd

F

Enter the contact tolerance ( E R R OR ).

16-25

3rd

F

Enter the distance below which near thermal or electrical contact behavior occurs ( DQ NE A R ). A zero entered here indicates that near contact behavior is not included.

26-35

4th

F

Not used; enter 0.

36-45

5th

F

Not used; enter 0.

46-55

6th

F

Not used; enter 0.

56-65

7th

F

Enter 0 (default) if there is no additional constraint on the tangential displacement when contact occurs. No constraints are placed on rotational degrees of freedom. Enter 1 to insure that there is no relative tangential displacement when the node comes into contact. A possible relative normal displacement might originate from an initial gap or overlap between the node and the contacted body, as the node will be projected onto the contacted body.

Main Index

680 CONTACT TABLE (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry Enter 2 to insure that there is no relative tangential and normal displacement when the node comes into contact. An existing initial gap or overlap between the node and the contacted body is not removed, as the node is not projected onto the contacted body. Enter 3 to insure full moment carrying glue when shells contact. The node will be projected onto the contacted body. Enter 4 to insure full moment carrying glue when shells contact. The node will not be projected onto the contact body.

66-70

8th

I

Enter 0 (default) if search order is based upon first checking bodies with lower body number versus bodies with higher body number. Enter 1 to indicate that the searching order for deformable contact bodies is from the touching body to the touched bodies on the 8th data block. This might change the default order for deformable bodies, which is from bodies with a lower number to bodies with a higher number. Enter 2 to let the program decide which searching order is optimal for deformable bodies. This order is set up such that searching is done starting with the body having the smallest element edge. This option forces singlesided contact between the touching and touched bodies: searching is done only from one body to another and not the other way around.

71-75

9th

I

Enter 0 (default) if, during initial contact, a projection onto the contact surface induces a stress. Enter 1 to modify the coordinates of a node in contact with a deformable body so that stress-free initial contact can be obtained. Enter 2 to extend the tangential error tolerance at sharp corners of deformable bodies to delay sliding off a contacted segment. Enter 3 to have both 1 and 2 active.

76-80

10th

I

Only relevant if the glue option is invoked and the separation force has not been set. Enter 0 if a node should not separate (default). Enter 1 to invoke the separation behavior procedure, as specified on the 12th field of the 2nd data block of the CONTACT option. Enter 2 to invoke the breaking glue capability. A node will be released if the break criterion is fulfilled. Then the node will do regular contact with separation instead of being glued. The stress limits for this capability are specified in the 6th data block below.

Main Index

CONTACT TABLE (Model Definition) 681 Define Contact Table

Format Fixed

Free

Data Entry Entry

4th data block Only required if version number is equal to 2. 1-5

1st

I

Enter the boundary description flag for the touching body (entered on the 3rd data block).

6-10

2nd

I

Enter the boundary description flag for the touched body (entered on the 11th data block).

The boundary description flag is given by A+10*B+1000*C, where parameter A is related to continuum elements in a body, parameter B is related to shell elements in a body and parameter C is related to beam elements and/or shell edges in a body. The possible values of these parameters and their meaning are: A=1:

the outside edges (2-D) or faces (3-D) of continuum elements are included in the boundary description (default).

B=1:

both top and bottom faces, including thickness offset, are included in the boundary description.

B=2:

only bottom faces, including thickness offset, are included in the boundary description.

B=3:

only bottom faces, ignoring thickness offset, are included in the boundary description.

B=4:

only top faces, including thickness offset, are included in the boundary description.

B=5:

only top faces, ignoring thickness offset, are included in the boundary description.

B=6:

both top and bottom faces, ignoring thickness offset, are included in the boundary description. The default value of B depends on the parameter governing the normal direction/thickness contribution of shell elements as entered on the CONTACT option. Note:

The choice B=6 for both bodies in a contact combination is only meaningful for glued contact. If in such cases separation is allowed, separated nodes will not come into contact anymore, unless a new CONTACT TABLE is defined to reset the value of B.

C=0:

neither beam elements nor shell edges are included in the boundary description.

C=1:

beam elements are included in the boundary description (allowing for beam-tobeam contact).

C=10:

shell edges are included in the boundary description.

C=11:

both beam elements and shell edges are included in the boundary description. If beam-to-beam contact is not activated on the CONTACT option, the default value of C is 0, otherwise the default value is 1.

Main Index

682 CONTACT TABLE (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

5th data block Only required if a mechanical-displacement solution is obtained. 1-10

1st

F

Enter the contact separation threshold. The physical meaning of this threshold (a force, a stress, or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block of the CONTACT option.

11-20

2nd

F

Enter the friction coefficient.

21-30

3rd

F

Enter the interference closure amount; normal to the contact surface.

31-40

4th

F

Enter the friction stress limit

σ limit .

This entry is only used for friction type 6 (Coulomb friction using the bilinear model). If the shear stress due to friction reaches this limit value, then the applied friction force will be reduced so that the maximum friction stress is given by min ( μ σn ,σ limit ) , with μ the friction coefficient and σ n the contact normal stress. Default for this entry is 1.e20.

Main Index

41-50

5th

F

Enter the contact tolerance BIAS factor (0-1). This value will overrule the BIAS factor entered on the 6th field of the 3rd data block of the CONTACT option if nonzero.

51-60

6th

F

Enter the delayed slide off distance (this entry is only used if delayed slide off has been activated by the 9th entry of the 3rd data block). When using the delayed slide off option, a node sliding on a segment will slide off this segment only if it passes the node (2-D) or edge (3-D) at a sharp corner over a distance larger than the delayed slide off distance. By default, the delayed slide off distance is related to the dimensions of the contacted segment by a 20 percent increase of its isoparametric domain.

61-70

7th

F

Enter the hard-soft ratio (this entry is only used if double-sided contact with automatic constraint optimization is used, as defined on the 4th data block of the CONTACT option). The hard-soft ratio can be used by the program if there is a significant difference in the (average) stiffness of the contact bodies (expressed by the trace of the initial stress-strain law). If the ratio of the stiffnesses is larger than the hard-soft ratio, the nodes of the softest body are the preferred slave nodes. By default, the hard-soft ratio is 2.

CONTACT TABLE (Model Definition) 683 Define Contact Table

Format Fixed

Free

Data Entry Entry

6th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-10

1st

F

Normal stress to break glued contact (SN).

11-20

2nd

F

Tangential stress to break glued contact (ST).

21-30

3rd

F

Enter exponent for breaking normal stress term (m). Default = 2.

31-40

4th

F

Enter exponent for breaking tangential stress term (n). Default = 2. The glue breaks when

m

n

( σ N ⁄ SN ) + ( σ T ⁄ ST ) > 1

7th data block Only required if heat transfer is included. 1-10

1st

F

Enter the contact heat transfer coefficient ( H T ).

11-20

2nd

F

Enter the convection heat transfer coefficient for near behavior ( H CV ).

21-30

3rd

F

Enter the natural convection heat transfer coefficient for near behavior ( H NC ).

31-40

4th

F

Enter the exponent associated with the natural convection for near behavior ( B NC ).

41-50

5th

F

Enter the surface emissivity ( ε ).

51-60

6th

F

Enter the separation distance dependent thermal convection coefficient ( H BL ).

8th data block Only required for Joule heating. 1-10

1st

F

Enter the contact electrical coefficient (coupled Joule analysis only).

11-20

2nd

F

Enter the electrical transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent electrical coefficient.

9th data block Only required for coupled mass diffusion analysis. 1-10

1st

F

Enter the contact mass transfer coefficient.

11-20

2nd

F

Enter the mass transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent mass diffusion coefficient.

10th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-10

Main Index

1st

F

Not used; enter 0.

684 CONTACT TABLE (Model Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

11th data block Only required if magnetostatic analysis is included. 1-10

1st

F

Not used; enter 0.

12th data block Only required for harmonic acoustic analysis. 1-10

1st

F

Enter the

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

Enter the

1 ----c1

reactive boundary coefficient.

13th data block Enter a list of touched bodies for which the touching body detects contact with the parameters above.

Main Index

SPLINE (Model Definition) 685 Analytical Surface used to Represent a Deformable Body

SPLINE (Model Definition)

Analytical Surface used to Represent a Deformable Body

Description In order to improve the accuracy for a deformable-deformable contact analysis, the outer surface of a contacted body can be described based on a spline (2-D) or Coons surface (3-D) description. The analytical surface is then used to calculate the normal to the deformable body and the closest point projection of a contacting node. In 2-D, for a contacted segment, a spline is created based on: tangent at first and second point of segment position of first and second point of segment In 3-D, for a contacted segment, a Coons surface is created based on: tangent vectors at corner points of segment position of corner points of segment zero twist vectors Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word SPLINE.

2nd data block 1-5

1st

I

Enter the number of deformable bodies for which the spline description must be applied.

6-10

2nd

I

Enter the increment frequency of writing the spline representation in Marc Mentat model files, called jid_spline_inc.mfd, where inc is the increment number. These files can be used to visualize the spline description and can be merged to the post file during post processing. Default is zero, so that no additional files are generated.

The 3rd and 4th data blocks are repeated for each deformable body with a spline description. 3rd data block

Main Index

1-5

1st

I

Body number.

6-10

2nd

I

For 3-D analyses only: enter 1 to enforce C0-continuity at edges where the normal vector to the outer contour of the structure shows a discontinuity (also see the 4th data block below).

686 SPLINE (Model Definition) Analytical Surface used to Represent a Deformable Body

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter 1 to automatically determine nodes (2-D) or edges (3-D) where the normal vector to the outer contour of the structure shows a discontinuity.

16-25

4th

F

Used only if the 3rd entry of this data block is set to 1: enter the threshold angle to decide if there is a normal vector discontinuity between two adjacent segments of the contact body defined in the first entry of this data block. The threshold angle should be between 0 and 90 degrees; the default value is 60 degrees.

4th data block Enter a list of nodes defining nodes (2-D) or edges (3-D) where the normal vector to the outer contour of the structure shows a discontinuity. Notes:

In 3-D, when there is a normal vector discontinuity at an element edge, the corner nodes defining the edge must be entered one after another. If the automatic detection is activated using the 3rd data block above, the nodes/edges with a normal vector discontinuity found by the program will be added to the list defined here.

As an example for the 2-D contact body below, (which is the second body in the model and the only body for which the SPLINE option is active), based on user-defined normal vector discontinuities the SPLINE option would be: spline 1 2 1

14

27

40

Finite Element Model

Main Index

Spline Representation

SPLINE (Model Definition) 687 Analytical Surface used to Represent a Deformable Body

Alternatively, using the automatic detection the input would be: spline 1 2 0

1

60.000

As an example for the 3-D contact body below (which is the second body in the model and the only body for which the SPLINE option is active), based on user-defined normal vector discontinuities the SPLINE option would be: spline 1 2 26 27 29 97 107 103 113 38 40 39

93 99 32 37 121

95 29 34 117 119

31 30 105 115 36

Finite Element Model

26 99 109 37 41

103 101 35 35 113

93 30 33 115 123

27 32 111 111 41

28 101 107 39 40

Main Index

1

60.000

97 33 36 119 121

28 31 109 117

Coons Representation

Alternatively, using the automatic detection the input would be: spline 1 2 0

95 105 34 38 123

c c c c

688 SPLINE (Model Definition) Analytical Surface used to Represent a Deformable Body

The effect of enforcing C0-continuity can be seen in the figures below.

C0-discontinuous

Main Index

C0-continuous

UMOTION 689 Invoke User Subroutine to Prescribe Surface Motion

UMOTION

Invoke User Subroutine to Prescribe Surface Motion

Description This option calls the MOTION user subroutine to define surface motions. See Marc Volume D: User Subroutines and Special Routines. This option also calls the UGROWRIGID user subroutine to define a scale factor to be applied to the size of the rigid bodies during the analysis as a function of time. Note:

This option should be placed after the CONTACT option.

Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-7

1st

A

Enter the word UMOTION.

11-15

2nd

I

Enter a 2 if the UGROWRIGID user subroutine is to be called to grow rigid bodies.

690 UFRICTION Invoke User Subroutine to Define Surface Friction Behavior

UFRICTION

Invoke User Subroutine to Define Surface Friction Behavior

Description This option calls the UFRIC user subroutine to define friction coefficients. If beam-to-beam contact is activated, the option also calls the UFRICBBC user subroutine to define friction coefficients for beam-to-beam contact (see Marc Volume D: User Subroutines and Special Routines). Note:

Use this option only in conjunction with the CONTACT option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

Main Index

1st

A

Enter the word UFRICTION.

UHTCOEF 691 Invoke User Subroutine to Define Surface/Environment Thermal Behavior

UHTCOEF

Invoke User Subroutine to Define Surface/Environment Thermal Behavior

Description This option activates the calls to user subroutines in contact analyses to influence the behavior between the surface and the environment. For heat transfer, the UHTCOE user subroutine may be used to define heat transfer coefficients (film coefficients) and sink temperatures of a free surface subjected to convective or radiative heat transfer. The UVTCOE user subroutine is used to define the analogous quantities for electrical contact in a coupled Joule heating analysis. In a diffusion analysis, the UMDCOE user subroutine is used to define the mass transfer coefficient and the environment pressure. (see Marc Volume D: User Subroutines and Special Routines). Note:

Use only in conjunction with the CONTACT option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

Main Index

A

Enter the word UHTCOEF.

692 UHTCON Invoke User Subroutine to Define Surface to Surface Behavior

UHTCON

Invoke User Subroutine to Define Surface to Surface Behavior

Description This option activates the calls to user subroutines in contact analyses to influence the behavior between surfaces. For heat transfer, the UHTCON user subroutine to define heat transfer coefficients (film coefficients) between surfaces in contact. In Joule heating analysis, the UVTCON user subroutine is used to define the analogous quantities for electrical contact.In a diffusion analysis, the UMDCON user subroutine is used to define the analogous mass transfer coefficient (see Marc Volume D: User Subroutines and Special Routines). Note:

Use only in conjunction with the CONTACT option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

Main Index

1st

A

Enter the word UHTCON.

CONTACT NODE (Model Definition) 693 Define Nodes for Surface Contact

CONTACT NODE (Model Definition)

Define Nodes for Surface Contact

Description This option is used to define which nodes in a body might potentially contact other surfaces. This option can be used to reduce the computational cost if a body has many exterior nodes and it is known for which nodes contact might occur. If this option is not used, all exterior surface nodes are checked for contact. Notes:

If this option is used and a node number is not explicitly listed, that node might penetrate other bodies. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT NODE option after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words CONTACT NODE.

I

Enter the number of bodies for which exterior nodes are defined

I

Body number.

I

Enter a list of nodes that are potential contact nodes.

2nd data block 1-5

1st

3rd data block 1-5

1st

4th data block 1-80

Main Index

1st

694 DEACT GLUE (Model Definition) Define Deact Glue for Nodes in Glued Contact

DEACT GLUE (Model Definition) Define Deact Glue for Nodes in Glued Contact Description This option is used to define nodes of a glued interface that should have regular contact instead of glued contact. The option has no effect if defined for a contact body which is not in glued contact. If two bodies are glued together, this option can be used to specify certain nodes that should not be glued, for example to define an initial crack. Unless single sided contact is used, it is best to identify nodes of both sides of the contact interface to make sure that the selected part is not glued. The deact glue only influences the contacting node. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DEACT GLUE.

I

Enter the number of bodies for which deact glue nodes are defined.

I

Body number.

I

Enter a list of nodes that should have regular contact.

2nd data block 1-5

1st

3rd data block 1-5

1st

4th data block 1-80

Main Index

1st

EXCLUDE (Model Definition) 695 Ignore Contact with Certain Regions

EXCLUDE (Model Definition)

Ignore Contact with Certain Regions

Description For certain contact problems, you might wish to influence the decision regarding the deformable segment a node contacts. By means of the EXCLUDE option, you can specify a list of nodes defining segments to be excluded from the contacted bodies. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word EXCLUDE.

I

Enter the number of deformable bodies for which the EXCLUDE option must be applied.

2nd data block 1-5

1st

The 3rd and 4th data blocks are repeated for each deformable body with the EXCLUDE option. 3rd data block 1-5

1st

I

Body number.

4th data block Enter a list of nodes defining segments to be excluded from contacted bodies. Notes:

In 2-D, each segment must be defined by two nodes. In 3-D, each segment must be defined by four nodes. If, in a 3-D, a segment corresponds to a tetrahedral or a collapsed hexahedral element, then the last two nodes of the set of four should be identical.

Main Index

696

Main Index

Chapter 3: Model Definition Options 697 Material Properties

Chapt Material Properties er 3: This section describes the material properties that can be associated with the model. These consist of both specification of the constitutive model used to describe the material behavior and the actual material Mode the data necessary to represent the material. l The ISOTROPIC model definition option can be used for the input of simple engineering material Defini properties, including the fluid density in fluid-solid interaction problems. Additional model definition options such as ORTHOTROPIC, ANISOTROPIC, MOONEY, OGDEN, ARRUDBOYCE, GENT, FOAM, tion and HYPOELASTIC, NLELAST, GASKET, SHAPE MEMORY, POWDER and SOIL are available for more Optio complex material representations. When not using the table driven input, the STRAIN RATE option allows the definition of a strain-rate dependent yield stress; the WORK HARD option allows the user to ns specify work hardening slopes for elastic-plastic behavior. Variations of material properties with temperatures such as Young’s modulus, Poisson’s ratio, etc. can be entered through TEMPERATURE EFFECTS, ORTHO TEMP, and TIME-TEMP options. When using the table driven input format, all these behaviors can be defined with the TABLE input. Cracking data and failure criteria data can be entered using CRACK DATA and FAIL DATA, respectively. Finally, the GAP DATA option can be used for the input of gap width, frictional coefficient, etc. for the gap-friction element (element type 12 and 97). Marc Volume C: Program Input

In addition, the COMPOSITE model definition option allows you to input layer information for a laminated composite material and the ORIENTATION option allows for the definition of the preferred material directions. A material consisting of multiple components may be defined using the MIXTURE option. A brief description of the material models which Marc has the capability of representing is given below. For additional details, refer to Marc Volume A: User Information.

A. Elastic Behavior 1. Isotropic Elastic Compressible Material – This is a material represented by Hooke’s Law. This material has a linear relation between stress and strain and its behavior is not path dependent. The stress strain relations can be expressed as σ i j = λ δij ε kk + 2Gε i j where λ, the Lame constant, and G, the shear modulus, can be expressed as:

λ= νE/((1+ν)(1-2ν)) and G = E/2(1+ν) E and ν are the familiar Young’s modulus and Poisson’s ratio, respectively, and can be specified using the ISOTROPIC model definition option. 2. Orthotropic Elastic Compressible Material – For an isotropic material, every plane is a plane of symmetry and every direction is an axis of symmetry. An orthotropic material, however, has only three mutually orthogonal planes of symmetry. With respect to a coordinate system parallel to these planes, the constitutive law for this material is given by the following more general form of Hooke’s Law:

Main Index

698 Marc Volume C: Program Input Material Properties

⎧ ⎪ ⎪ ⎪ ⎪ ⎨ ⎪ ⎪ ⎪ ⎪ ⎩

ε 11 ⎫ ⎪ ε 22 ⎪ ⎪ ε 33 ⎪ ⎬ = γ 12 ⎪ ⎪ γ 23 ⎪ ⎪ γ 31 ⎭

ν 21 ν 31 1 -------- – ------- – -------E 11 E 22 E 33

0

0

0

ν 12 1 ν 32 – -------- -------- – -------E 11 E 22 E 33

0

0

0

ν 13 ν 23 1 - – -------- -------– ------E 11 E 22 E 33

0

0

0

0

0

0

1 --------G 12

0

0

0

0

0

0

1-------G 23

0

0

0

0

0

0

1 --------G 31

⎧ ⎪ ⎪ ⎪ ⎪ ⎨ ⎪ ⎪ ⎪ ⎪ ⎩

σ 11 ⎫ ⎪ σ 22 ⎪ ⎪ σ 33 ⎪ ⎬ τ 12 ⎪ ⎪ τ 23 ⎪ ⎪ τ 31 ⎭

Due to symmetry of this compliance matrix, E11 ν21 = E22 ν12, E22 ν32 = E33 ν23, and E33 ν13 = E11 ν31. Using these relations, a general orthotropic material has nine independent constants: E11, E22, E33, ν12, ν23, ν31, G12, G23, G31. These nine constants can be specified using the ORTHOTROPIC option. Note that the inequalities E22 > ν232 E33, E11 > ν122 E22, and E33 > ν312

E11 must be satisfied in order for the orthotropic material to be stable. This is checked by Marc. 3. Anisotropic Elastic Compressible Material – This is a material represented by the generalized Hookes’ Law. This material has a linear relation between stress and strain and its behavior is not path dependent. The stress-strain relation can be expressed as:

σij = Cijkl ekl. All of the values of C can be specified using either the ANELAS or HOOKLW user subroutine. As an alternative, the user can supply the compliance matrix in the HOOKLW user subroutine. The ANISOTROPIC model definition option is used to direct Marc to call these user subroutines when necessary. 4. Isotropic Incompressible Material Mooney-Rivlin form – The nonlinear elastic material can be represented by a certain class of strain energy functions. The form of this function is: W = C10 (I1 -3) + C01 (I2 -3) + C11 (I1 -3)(I2 -3) + C20 (I1 -3)2 + C30 (I1 -3)3 where I1, I2 are the first and second invariants of the elastic strain. This strain energy function can represent the Neo-Hookean materials (C01, C11, C20, and C30 are zero) or Mooney-Rivlin materials (C11, C20, and C30 are zero). The material has a nonlinear relation between stress and strain; hence, an incremental procedure must be performed. Alternative energy functions can be specified via the UENERG user subroutine. The stress-strain relations can be expressed as

∂W σ i j = --------- . ∂ε i j

The constants are supplied by you through the MOONEY option. Note that this material model can be used to represent large-strain elastic materials.

Main Index

Chapter 3: Model Definition Options 699 Material Properties

5. Isotropic Elastic Incompressible Material-Ogden Formulation - Another representation of nonlinear elastic material is by the Ogden strain energy function. This model can be used to represent large-strain behavior in elastic materials. For plane stress, displacement elements are always used. The strain energy function is

∑

W =

n = 1

Note:

μ –α ⁄ 3 α α α -----n- J n ( λ 1 n + λ 2 n + λ 3 n – 3 ) + 4.5K ( J 1 / 3 – 1 ) 2 αn

There are two modes for performing rubber (Mooney, Ogden, Arruda Boyce, Gent) analysis for plane strain, generalized plane strain, axisymmetric, or solid analysis. This mode is set on the ELASTICITY or LARGE STRAIN parameters. If the total Lagrange formulation is invoked, the elements, in this case, must be of the Herrmann formulation. If the updated Lagrange formulation is invoked, the elements can have a conventional displacement formulation.

6. Isotropic Incompressible Arruda-Boyce Model - An invariant based model simulating micromechanical behavior of rubber elasticity. 2 3 4 5 1 1 11 19 519 W = nk θ --- ( I 1 – 3 ) + ---------- ⎛ I – 9⎞ + ------------------2- ⎛ I – 27⎞ + ------------------3- ⎛ I – 81⎞ + ------------------------4- ⎛ I – 243⎞ ⎠ ⎝ ⎠ ⎝ ⎠ ⎝ ⎠ 2 20 N ⎝ 1 1050N 1 7000N 1 673750N 1

7. Isotropic Incompressible Gent Model - An invariant based model simulating micro-mechanical behavior of rubber elasticity. ⎛ I1 – 3 ⎞ E W = – --- ( I m – 3 ) log ⎜ 1 – ---------------⎟ 6 I m – 3⎠ ⎝

8. Isotropic Elastic Foam Material - This nonlinear elastic material has the characteristic that it can have both large strain deviatoric and volumetric behavior. The material model is used in conjunction with the displacement elements. The strain energy function is W =

∑ n =1

μ α α α -----n- ( λ 1 n + λ 2 n + λ 3 n – 3 ) + αn

∑ n=1

β μ -----n ⎛ 1 – J n⎞ ⎠ βn ⎝

Conventional displacement based elements are always used with the foam material model. 9. Generalized Isotropic Hyperelastic Materials - Generalized strain energy functions which include the above mentioned Mooney-Rivlin, Ogden, Arruda-Boyce, Gent models and foam model as special cases can be defined using the UELASTOMER user subroutine. The MOONEY model definition option directs Marc to call UELASTOMER for strain-invariant-based energy functions with volumetric-deviatoric split. The OGDEN model definition option directs Marc to call UELASTOMER for principal-stretch-based energy functions with volumetric-deviatoric split. The FOAM model definition option activates UELASTOMER for generalized compressible foam models of both the invariant-based and the principal-stretch-based.

Main Index

700 Marc Volume C: Program Input Material Properties

10. General Anisotropic Nonlinear Elastic Material – This can be represented by the hypoelastic material model. The material has a nonlinear relation between stress and strain; hence, an incremental procedure must be performed. The stress-strain relation can be expressed as · · σ i j = C ij kl ε + g ij where Cijkl and gij are functions of elastic strain and temperature. The HYPOELASTIC model definition option should be used to direct Marc to call the HYPELA2 user subroutine when necessary or to define the hypoelastic material data. 11. Predefined Nonlinear Elastic Materials – The NLELAST option may be used to specify that the model has nonlinear material behavior of a type that has been implemented in Marc. These models may be summarized as follows: a. Nonlinear equivalent stress-equivalent strain representation b. Young’s modulus function of strain invariants c. Principal strain-based model d. Linear elastic with tension/compression limits e. Bi-modulus linear elastic with tension/compression limits f. Orthotropic nonlinear The table driven input method must be used with this option. For further details, see Marc Volume A: Theory and User Information, Chapter 3: Data Entry, Table Driven Input.

B. Elastic-Plastic Behavior Elastic-plastic material can be described using a variety of models. The differentiation between these models is due to: a. the inclusion or exclusion of elastic effects; b. the yield function; c. the flow rule, and d. the hardening rule. 1. Rigid Plastic Material – This is the only material model which excludes the elastic strains. The capability is based on the iteration for the velocity field in an incompressible, non-Newtonian ·

fluid. The nonlinear stress-strain relation can be expressed as S i j = G ( ε ) ε ij . Note that as the material is incompressible, a traction boundary condition must be specified; otherwise the stress field is only known to an arbitrary hydrostatic pressure. Only the yield stress need be entered. 2. Elastic-Perfectly-Plastic Material – This is a material which behaves elastically until it reaches the yield stress. The material has no ability to support additional load (in a uniaxial sense) upon yield. The material has a nonlinear relation between the stress rate and strain rate and is path dependent. You need only specify the elastic constants and the yield stress. Marc uses the von Mises yield function and the associated flow law.

Main Index

Chapter 3: Model Definition Options 701 Material Properties

3. Elastic-Plastic Isotropic-Hardening Material – This is a model which behaves elastically until it reaches the yield stress. After yielding the material strains or work hardens according to the isotropic model. The yield surface uniformly expands in all directions with increasing equivalent plastic strain. The additional information necessary to define the rate of growth of the yield surface is prescribed through the WORK HARD or TABLE option. Four new hardening models have been added for modeling the hardening behavior. Power Law Model –

·n m σy = A ( εo + ε ) + B ε

Rate Power Law Model – Kumar model –

m ·n σy = A ε ε + B

σ = B 0∗ sinh

Johnson-Cook model –

–1

· 1⁄n Q ⁄ ( nRT ) ⎛ --ε-⎞ e ⎝ A⎠

n · T – T room m ρ ε ⎞⎞ ⎛ σ y = ⎛ A + B ε ⎞ ⎛ 1 + C ln ⎛ ---1 – ⎛ ---------------------------------⎞ ⎞ · ⎝ T melt – T room⎠ ⎠ ⎝ ε ⎠⎠ ⎝ ⎝ ⎠⎝ 0

4. Elastic-Plastic Kinematic-Hardening Material – This is a material whose yield surface behavior is governed by the kinematic hardening model. In this model, the yield surface translates in stress space depending upon the change in plastic strain. The rate of translation is prescribed through the WORK HARD or TABLE option. This option is set through the ISOTROPIC, ORTHOTROPIC or ANISOTROPIC model definition option. 5. Elastic-Plastic Combined-Hardening Material – This is a material whose yield surface behavior is governed by a combination of both the isotropic and kinematic hardening models. That is, the yield surface both expands in size and shifts in space. This behavior is given through the WORK HARD or TABLE option. This option is set through the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition option. 6. Elastic-Plastic-ORNL Hardening – This is a model whose yield surface is governed by the ORNL constitutive theory. This model also allows plastic creep interaction. This option is set through the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition option. 7. The Chaboche model is a combined isotropic/kinematic hardening model. 8. Anisotropic Yield Surface – It is also possible to use the anisotropic yield function of Hill or Barlat. For 3-D models, these yield surfaces are noncircular when observed in deviatoric stress space. These anisotropic yield functions may be used in conjunction with isotropic, orthotropic, or anisotropic elasticity. In addition, the yield function can be dependent upon the strain rate; this can be specified by using the STRAIN RATE or TABLE option. 9. Elastic-Plastic Material with Mohr-Coulomb Yield Surface – is a model which allows the representation of materials in which the yield surface is dependent on the hydrostatic stress. It is appropriate for modeling soils. The yield function dependence on the shear stress is given using the WORK HARD or TABLE option; the dependence on the hydrostatic stress is given in the ISOTROPIC option. This option is set through the ISOTROPIC model definition option. 10. The yield surface can also be modified based upon the Gurson model for void damage. In this model, a modified von Mises criteria, with hydrostatic stress and void dependency, is used. The DAMAGE option is used to activate this model.

Main Index

702 Marc Volume C: Program Input Material Properties

11. A special viscoplastic model for powder materials can be entered through the POWDER option. In this model, the material properties are also dependent on the relative density of the material. These materials are always assumed to be isotropic. 12. A general viscoplastic option is available for materials that are modeled using unified creepplasticity rules. In this procedure, the elastic properties are defined in either the ISOTROPIC or ORTHOTROPIC option and the inelastic properties are provided through the UVSCPL user subroutine. 13. Superplastic material behavior can be modeled using Power Law and Rate Power Law defined in ISOTROPIC model definition option.

C. Temperature Dependent Material Properties All of the parameters (except density) necessary to represent the material properties can be given as a function of temperature. These effects are specified using the TEMPERATURE EFFECTS, ORTHO TEMP or TABLE option.

D. Relative Density Dependent Material Properties In powder materials, the materials can be given as a function of the relative density where a relative density of 1.0 implies a fully compacted material. This data is entered through the DENSITY EFFECTS option.

E. Low Tension Material In addition to using the ISOTROPIC model definition option for the input of Young’s modulus, Poisson’s ratio, yield stress, etc., the CRACK DATA model definition option must be used for the specification of critical cracking stress, tension-softening modulus, crushing strain and shear retention factor. These data can be alternatively specified by the UCRACK and TENSOF user subroutines. Detailed discussion on low tension material can be found in Marc Volume A: User Information.

F. Soil Materials When performing a coupled fluid-soil analysis, the soil material can be modeled either as a linear elastic material, a nonlinear elastic material or using the modified CAM-CLAY model.

G. Material Dependent Failure Criteria Ten failure criteria are available in Marc. They are maximum stress, maximum strain, Tsai-Wu, Hoffman, Hill, Puck, and three variations of the Hashin failure criteria. Detailed discussion on failure criteria can be found in Marc Volume A: User Information. During each analysis, up to three fail criteria can be selected; failure indices are calculated and printed for every integration point. The model definition option FAIL DATA (or user subroutine UFAIL) is used for the input of failure criteria data.

Main Index

Chapter 3: Model Definition Options 703 Material Properties

H. Characterization of Gap Elements The GAP DATA model definition option allows for the input of gap closure distance, gap elastic stiffness, contact coefficient of friction and momentum ratio. Detailed discussion on gap elements (elements 12 and 97) can be found in Marc Volume B: Element Library.

I. Laminated Composite A laminated composite is a “material” made of several thin layers of separate materials with different material behavior, layer thicknesses, and orientations from one layer to the next. To model laminated composite plates, shells, or beams with Marc, use the COMPOSITE option. In this option, three quantities are specified on a layer-by-layer basis: material identification number, layer thickness, and ply angle. The entire set of data (a “composite group”) is then associated with a list of elements. For each individual layer, all of the above mentioned constitutive laws can be used with the exception of the low tension material. The layer thickness can be constant or variable (in the case of variable total thickness elements), and the ply angle can change from one layer to the next. The orientation of the 0 ply angle within each element is defined in the ORIENTATION option. These elements are used in conjunction with shell elements, composite continuum elements, or the solid shell element. For more information on the specific assumptions employed by the COMPOSITE option, see Marc Volume A: User Information.

J. Material Preferred Direction Every element type in Marc has a default orientation (that is, a default coordinate system) within which element stress-strain calculations take place. This system is also assumed to be the coordinate system of material symmetry. This is especially important for nonisotropic materials (orthotropic, anisotropic, or composite materials). With the ORIENTATION option, you specify the orientation of the material axes of symmetry (or the 0 ply angle line, if composite) in one of five different ways: 1) as a specific angle offset from an element edge, 2) as a specific angle offset from the line created by two intersecting planes, 3) as a particular coordinate system specified by user-supplied unit vectors, 4) by referencing a coordinate system defined by the COORD SYSTEM option, or 5) as specified by the ORIENT user subroutine. For more information on these options, see Marc Volume A: Theory and User Information.

K. Material Property (Element) Coordinate Systems in Marc When defining material properties in Marc, you should be aware of the three coordinate systems used by Marc. They are: Global Coordinate System The material data supplied in the ISOTROPIC and ORTHOTROPIC options are always considered to be defined with respect to the material principal axes of symmetry. For continuum problems (that is, those using 2-D or 3-D solid elements), this coordinate system is aligned (by default) with the global xyz coordinate system. (For truss, beam and shell problems, see Marc (or Local) Coordinate System.) This is not normally a problem for isotropic materials since every

Main Index

704 Marc Volume C: Program Input Material Properties

direction is then a principal direction. For orthotropic materials, however, the material principal coordinates are seldom aligned with the global coordinates. For this reason, a second coordinate system is needed. User-defined (or “preferred”) Coordinate System If the material principal axes of symmetry are not aligned with the global coordinate system, a second coordinate system is used. This is the user-defined “preferred” coordinate system. This coordinate system is usually taken to be coincident with the material principal coordinates. The orientation of the preferred coordinate system and, hence, of the material principal axes, is defined by the ORIENTATION option on an element-by-element basis. In this way, you can completely define through the input file, the material data and orientation of a general orthotropic material. Marc (or Local) Coordinate System For truss, beam, and shell problems, the material principal axes of symmetry are aligned (by default) with special local element dependent coordinate systems. For example, for shell element 72, these local coordinates are the respect to these

v˜ 1 v˜ 2 v˜ 3

v˜ 1 v˜ 2 v˜ 3

surface coordinates so that material property data are assumed to begin with

coordinates. For isotropic materials, this is not normally a problem. For

orthotropic materials, the material principal axes cannot be aligned with the v˜ 1 v˜ 2 v˜ 3 axes. As in continuum problems, the ORIENTATION option is used to define a second set of preferred coordinates. This allows you to arbitrarily orient orthotropic materials in shells with local coordinates. Composite Shells In composite shells, the orientation of the materials in each shell layer can vary from layer to layer. In this case, the ORIENTATION option is used to locate the 00 ply angle direction in the shell surface. (If the ORIENTATION option is omitted, the 00 ply angle direction coincides with the v˜ 1 axis. See previous

section.) For each layer, additional ply angle offsets from this 00 ply angle direction are given in the COMPOSITE option. This allows you to arbitrarily orient an arbitrary composite layup in shells with local coordinates. Numerical Procedure for LARGE STRAIN The Tables 3-12 and 3-13 use these keywords:

Main Index

A

–

Additive strain rate decomposition

M

–

Multiplicative strain rate decomposition

TL

–

Total Lagrange

UL

–

Updated Lagrange

SS

–

Small Strain

LS

–

Large Strain (logarithmic)

GL

–

Green-Lagrange

Chapter 3: Model Definition Options 705 Material Properties

Table 3-12

Influence of LARGE STRAIN, 1 on Numerical Procedure

Material Option ISOTROPIC

Suboption 1 ELASTIC VON MISES

ORTHOTROPIC

ANISOTROPIC

Plane strain, Axisymmetric, Solid Herrmann Based

UL - LS - A

UL - LS - A

TL -GL

Truss, Beam, Plane stress, Membrane, Shell

ISOTROPIC

UL - LS - A

UL - LS - A

UL-LS-M

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

CHABOCHE

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

LIN MOHRC

UL - LS - A

UL - LS - A

N/A

PBL MOHRC

UL - LS - A

UL - LS - A

N/A

BUY MOHRC

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

GEN-PLAST

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

RIGID

SS (membranes)

SS-UL

SS-UL

IMPL-CREEP

UL - LS - A

UL - LS - A

N/A

ELASTIC VON MISES

Notes:

Suboption 2

Plane strain, Axisymmetric , Solid Displacement Based

UL - LS - A

UL - LS - A

TL -GL

ISOTROPIC

UL - LS - A

UL - LS - A

N/A

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

ELASTIC

UL - LS - A

UL - LS - A

TL -GL

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

706 Marc Volume C: Program Input Material Properties

Table 3-12

Influence of LARGE STRAIN, 1 on Numerical Procedure (continued)

Material Option

Suboption 1 VON MISES

Suboption 2

Truss, Beam, Plane stress, Membrane, Shell

Plane strain, Axisymmetric , Solid Displacement Based

Plane strain, Axisymmetric, Solid Herrmann Based

ISOTROPIC

UL - LS - A

UL - LS - A

N/A

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

Nastran

UL-LS

UL-LS

UL-LS

Invariant

UL-LS

UL-LS

UL-LS

Principal strain

UL-LS

UL-LS

N/A

Linear elastic w /limit

UL-LS

UL-LS

UL-LS

Bi-modulus w/limit

UL-LS

UL-LS

UL-LS

orthotropic nonlin.

UL-LS

UL-LS

N/A

HYPOELASTIC

UL-LS

UL-LS

UL-LS

MOONEY

TL -GL

UL - LS

UL - LS

ARRUDA-BOYCE

TL -GL

UL - LS

UL - LS

GENT

TL -GL

UL - LS

UL - LS

OGDEN

TL -GL

UL - LS

UL - LS

FOAM

TL -GL

UL - LS

N/A

NLELAST

Notes:

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

Chapter 3: Model Definition Options 707 Material Properties

Table 3-12

Influence of LARGE STRAIN, 1 on Numerical Procedure (continued)

Material Option

Suboption 1

Suboption 2

Truss, Beam, Plane stress, Membrane, Shell

Plane strain, Axisymmetric , Solid Displacement Based

Plane strain, Axisymmetric, Solid Herrmann Based

GASKET

N/A

UL - LS

N/A

SHAPE MEMORY THERMO-MECH

UL - LS -A

UL - LS -A

N/A

N/A

UL - LS -M

N/A

COMPOSITE

UL - LS - no finite

UL -LS

N/A

POWDER

N/A

UL -LS-A

N/A

SOIL

N/A

UL - LS - A

N/A

COHESIVE

N/A

UL-LS

N/A

GASKET

N/A

UL-LS

N/A

AURICCHIO

Notes:

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

708 Marc Volume C: Program Input Material Properties

Table 3-13

Influence LARGE STRAIN, 2 on Numerical Procedure

Material Option ISOTROPIC

Plane strain, Axisymmetric , Solid Displacement Based

Plane strain, Axisymmetric, Solid Herrmann Based

UL - LS - M

UL - LS - M

TL - GL

ISOTROPIC

UL - LS - M

UL - LS - M

UL-LS-M

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

CHABOCHE

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

LIN MOHRC

UL - LS - A

UL - LS - A

N/A

PBL MOHRC

UL - LS - A

UL - LS - A

N/A

BUY MOHRC

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

GEN-PLAST

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

RIGID

SS (membranes)

SS-UL

SS-UL

IMPL-CREEP

UL - LS - A

UL - LS - A

N/A

ELASTIC

UL - LS

UL - LS

TL - GL

ISOTROPIC

UL - LS - A

UL - LS - A

N/A

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

Suboption 1 ELASTIC VON MISES

ORTHOTROIC

VON MISES

Notes:

Suboption 2

Truss, Beam, Plane stress, Membrane, Shell

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

Chapter 3: Model Definition Options 709 Material Properties

Table 3-13

Influence LARGE STRAIN, 2 on Numerical Procedure (continued) Plane strain, Axisymmetric , Solid Displacement Based

Plane strain, Axisymmetric, Solid Herrmann Based

UL - LS - A

UL - LS - A

TL - GL

ISOTROPIC

UL - LS - A

UL - LS - A

N/A

KINEMATIC

UL - LS - A

UL - LS - A

N/A

COMBINED

UL - LS - A

UL - LS - A

N/A

HILL

UL - LS - A

UL - LS - A

N/A

BARLAT

UL - LS - A

UL - LS - A

N/A

ORNL

UL - LS - A

UL - LS - A

N/A

VISCO-PLAS

UL - LS - A

UL - LS - A

N/A

Nastran

UL-LS

UL-LS

UL - LS

Invariant

UL-LS

UL-LS

UL - LS

Principal strain

UL-LS

UL-LS

N/A

Linear elastic w /limit

UL-LS

UL-LS

UL - LS

Bi-modulus w/limit

UL-LS

UL-LS

UL - LS

orthotropic nonlin.

UL-LS

UL-LS

N/A

HYPOELASTIC

UL-LS

UL-LS

UL-LS

MOONEY

TL -GL

UL-LS

UL-LS

ARRUDA-BOYCE

TL -GL

UL-LS

UL-LS

GENT

TL -GL

UL-LS

UL-LS

OGDEN

TL -GL

UL-LS

UL-LS

Material Option ANISOTROPIC

Suboption 1 ELASTIC VON MISES

NLELAST

Notes:

Suboption 2

Truss, Beam, Plane stress, Membrane, Shell

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

710 Marc Volume C: Program Input Material Properties

Table 3-13

Influence LARGE STRAIN, 2 on Numerical Procedure (continued)

Material Option

Suboption 1

Suboption 2

Truss, Beam, Plane stress, Membrane, Shell

Plane strain, Axisymmetric , Solid Displacement Based

Plane strain, Axisymmetric, Solid Herrmann Based

FOAM

TL -GL

UL-LS

N/A

GASKET

N/A

UL - LS

N/A

SHAPE MEMORY THERMO-MECH

UL - LS -A

UL - LS -A

N/A

N/A

UL - LS -M

N/A

COMPOSITE

UL - LS - no finite

UL-LS

N/A

POWDER

N/A

UL -LS-A

N/A

SOIL

N/A

UL - LS - A

N/A

COHESIVE

N/A

UL-LS

N/A

GASKET

N/A

UL-LS

N/A

AURICCHIO

Notes:

If cracking requested on ISOTROPIC option, then it always uses UL-LS-A, and Herrmann elements are not supported. If Gurson damage model requested on DAMAGE then it always uses UL-LS-A, and Herrmann elements are not supported

Main Index

ISOTROPIC (with TABLE Input - Stress) 711 Define Mechanical Data for Isotropic Materials

ISOTROPIC (with TABLE Input - Define Mechanical Data for Isotropic Materials Stress) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define material properties, a yield criterion, and a strain hardening law for an isotropic material. You can also associate these material properties with a list of element numbers. Defaults for this option are von Mises yield criterion, isotropic strain hardening law (with a slope of 0.0), and an equivalent yield stress of 1020. Therefore, the default is an elastic nonyielding isotropic material. See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 15 are repeated as a set, once for each set of isotropic material defined. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.),for cross-referencing CREEP, CRACK DATA, FAIL DATA, etc. and user subroutines.

6-15

Main Index

2nd

A

Enter one of the following yield criteria: ELASTIC

– Purely elastic material

VON MISES

– von Mises (Default)

HILL

– Hill’s (1948) Yield.

BARLAT

– Barlat’s (1991) Yield.

LIN MOHRC

– Linear Mohr-Coulomb

PBL MOHRC

– Parabolic Mohr-Coulomb

BUY MOHRC

– Buyukozturk Concrete Model

NORM ORNL

– Normal ORNL

712 ISOTROPIC (with TABLE Input - Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

16-25

Free

3rd

Data Entry Entry

A

CRMO ORNL

– 2-1/4 Cr-Mo ORNL

REVP ORNL

– Reversed Plasticity ORNL

ARST ORNL

– Full alpha reset ORNL.

GEN-PLAST

– Generalized Plasticity Model

VISCO PLAS

– Viscoplastic model through the UVSCPL user subroutine

RIGID

– Rigid-plastic material, no elasticity, von Mises yield

IMPL CREEP

– Implicit creep model, both plasticity and creep, von Mises criterion.

Enter one of the following hardening rules: ISOTROPIC

– Isotropic hardening (Default)

KINEMATIC

– Kinematic hardening

COMBINED

– Combined (isotropic kinematic) hardening.

CHABOCHE

– Nonlinear (in)viscid isotropic-kinematic hardening.

POWER LAW

–

RATE POWER LAW – JOHNSON-COOK

–

KUMAR

–

For superplastic forming analyses (SPF), only POWER LAW is available as hardening rule. 26-30

4th

I

Not used; enter 0.

31-35

5th

I

Enter 1 to turn on concrete cracking.

36-40

6th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file. Enter -8 if data read in US from database.

Main Index

ISOTROPIC (with TABLE Input - Stress) 713 Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

41-45

7th

I

Number of viscoplastic parameters to be read through data block 5b or the number of phases in this material.

46-57

8th

A

Enter the material name to cross-reference with material database.

4th data block The data entered in the following blocks are the reference values that are used with tables or are constants. 1-10

1st

F

Young’s modulus (Not required for RIGID).

11-20

2nd

F

Poisson’s ratio (Not required for RIGID).

21-30

3rd

F

Mass density (stress analysis).

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Equivalent (von Mises) tensile yield stress. (For Mohr-Coulomb behavior, this is at zero hydrostatic stress. For implicit viscoplasticity, back stress.)

51-60

6th

F

For ORNL yield criteria, equivalent 10th cycle tensile yield stress. (For Mohr-Coulomb yield criteria, α-β parameter.) For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used. For Mohr-Coulomb yield criteria, α-β parameter. For implicit creep, equivalent (von Mises) tensile yield stress.

61-70

7th

F

Enter the cost per unit volume.

71-80

8th

F

Enter the cost per unit mass.

5th data block 1-5

1st

I

Table ID for Young’s modulus.

6-10

2nd

I

Table ID for Poisson’s ratio.

11-15

3rd

I

Table ID for mass density.

16-20

4th

I

Table ID for coefficient of thermal expansion.

21-25

5th

I

Table ID for equivalent tensile yield stress.

26-30

6th

I

Table ID for ORNL 10th cycle yield stress or Mohr Coulomb α-β parameter.

6a data block Necessary only for Hill and Barlat’s yield criteria.

Main Index

1-10

1st

F

YRDIR1 (for Hill) or M (for Barlat)

11-20

2nd

F

YRDIR2 (for Hill) or C1 (for Barlat)

714 ISOTROPIC (with TABLE Input - Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

YRDIR3 (for Hill) or C2 (for Barlat)

31-40

4th

F

YRSHR1 (for Hill) or C3 (for Barlat)

41-50

5th

F

YRSHR2 (for Hill) or C6 (for Barlat)

51-60

6th

F

YRSHR3 (for Hill)

6aa data block Necessary only for Hill and Barlat’s yield criteria. Note:

In this release, table IDs are input but not used.

1-5

1st

I

Table ID for YRDIR1 (for Hill) or M (for Barlat)

6-10

2nd

I

Table ID for YRDIR2 (for Hill) or C1 (for Barlat)

11-15

3rd

I

Table ID for YRDIR3 (for Hill) or C2 (for Barlat)

16-20

4th

I

Table ID for YRSHR1 (for Hill) or C3 (for Barlat)

21-25

5th

I

Table ID for YRSHR2 (for Hill) or C6 (for Barlat)

26-30

6th

I

Table ID for YRSHR3 (for Hill)

6b data block The following blocks are only used for CHABOCHE hardening rule. 1-10

1st

F

R0 for isotropic hardening.

11-20

2nd

F

R∞ for isotropic hardening (Q0 in case of using plastic-strain-range memorization, see 6c data block)

21-30

3rd

F

b coefficient for isotropic hardening.

31-40

4th

F

C coefficient for kinematic hardening.

41-50

5th

F

γ coefficient for kinematic hardening.

51-60

6th

F

K value for viscosity model.

61-70

7th

F

n coefficient for viscosity model.

6bb data block The following blocks are only used for CHABOCHE hardening rule.

Main Index

1-5

1st

I

Table ID for R0 for isotropic hardening.

6-10

2nd

I

Table ID for R∞ for isotropic hardening (Q0 in case of using plastic-strainrange memorization).

11-15

3rd

I

Table ID for b coefficient for isotropic hardening.

16-20

4th

I

Table ID for C coefficient for kinematic hardening.

21-25

5th

I

Table ID for γ coefficient for kinematic hardening.

ISOTROPIC (with TABLE Input - Stress) 715 Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Table ID for K value for viscosity model.

31-35

7th

I

Table ID for n coefficient for viscosity model.

6c data block Necessary only for CHABOCHE hardening rule with plastic-strain-range memorization. Notice that if no memorization is required, then provide a blank line. 1-10

1st

F

Qm coefficient for isotropic hardening.

11-20

2nd

F

μ coefficient for isotropic hardening.

21-30

3rd

F

η coefficient to introduce progressive memory.

6cc data block Necessary only for CHABOCHE hardening rule with plastic-strain-range memorization. Notice that if no memorization is required, then provide a blank line. 1-5

1st

I

Table ID for Qm coefficient for isotropic hardening.

6-10

2nd

I

Table ID for μ coefficient for isotropic hardening.

11-15

3rd

I

Table ID for η coefficient to introduce progressive memory.

7th data block Necessary only in a coupled thermal-stress analysis 1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistance (Joule Analysis).

41-50

5th

F

Emissivity.

51-60

6th

F

Enter the enthalpy of formation.

61-70

7th

F

Enter the reference temperature of enthalpy of formation.

8th data block Necessary only in a coupled thermal-stress analysis.

Main Index

1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density.

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

26-30

6th

I

Table ID for enthalpy of formation.

716 ISOTROPIC (with TABLE Input - Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

9th data block Necessary only in a coupled electrostatic-stress analysis. 1-10

1st

F

Permittivity constant.

10th data block Necessary only in a coupled electrostatic-stress analysis. 1-5

1st

I

Table ID for permittivity constant.

11th data block The following blocks are only used if viscoplastic material and the seventh field of data block 3 is entered. Enter 8 fields per data line. 1-10

1st

Enter the first viscoplastic parameter

11-20

2nd

Enter the second viscoplastic parameter.

12a data block The following two blocks (12a and 12b) are read in for Power Law or Rate Power Law model. Power Law Model –

·n m σy = A ( εo + ε ) + B ε

Rate Power Law Model –

m·n σ y = Aε ε + B, σ 0

If the value is less than the minimum yield stress, the minimum yield stress is used. 1-10

1st

F

Enter coefficient A.

11-20

2nd

F

Enter exponent m.

21-30

3rd

F

Enter coefficient B.

31-40

4th

F

Enter exponent n.

41-50

5th

F

Enter

σ0

for the Rate Power Law Model or

If 0 is entered,

E ε 0 = ⎛ ---⎞ ⎝ A⎠

1 ------------m–1

and

σ0 = 0

12b data block

Main Index

1-5

1st

I

Enter the table ID for the coefficient A.

6-10

2nd

I

Enter the table ID for the exponent m.

11-15

3rd

I

Enter the table ID for the coefficient B.

16-20

4th

I

Enter the table ID for the exponent n.

21-25

5th

I

Enter the table ID for the

σ0 .

ε0

for the Power Law Model.

ISOTROPIC (with TABLE Input - Stress) 717 Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

The following blocks (13a and 13b) are read in for Kumar model only. σ = B 0 sinh

–1

· 1⁄n Q ⁄ ( nRT ) ⎛ ε----p-⎞ e ⎝ A⎠

A is a constant or n is a constant or

B3

ln A = B 1 + B 2 ⁄ ε p B3

n = B4 + B 5 ⁄ εp

The activation energy (Q) is specified in the MATERIAL DATA option. The universal gas constant (R) is specified in the PARAMETERS option. 13a data block 1-10

1st

F

Enter coefficient B0.

11-20

2nd

F

Enter coefficient A; if A = 0, then B1, B2, and B3 is used.

21-30

3rd

F

Enter B1.

31-40

4th

F

Enter B2.

41-50

5th

F

Enter B3.

51-55

6th

I

Enter the table ID for the coefficient B0.

56-60

7th

I

Enter the table ID for the coefficient A.

13b data block 1-10

1st

E

Enter coefficient n; if n = 0, then B4, B5, and B6 is used.

11-20

2nd

E

Enter B4.

21-30

3rd

E

Enter B5.

31-40

4th

E

Enter B6.

41-45

5th

I

Enter the table ID for the exponent n.

14th data block The following block is read in for the Johnson-Cook model. · T – T room ⎞ m⎞ ⎛ ε p⎞ ⎞ ⎛ n ⎛ ⎛ -------------------------------σ y = ( A + B ε p ) ⎜ 1 + C ln ⎜ ---· -⎟ ⎟ 1 – ⎝ T ⎠ ⎠ ⎝ε ⎠⎠ ⎝ ⎝ m elt – T room 0

where

T

is the current temperature,

T melt

is the material melt temperature, and

temperature. ε p is the effective plastic strain, strain rate.

Main Index

A, B, C, n,

and

m

are constants.

· εp

T room

is the effective plastic strain rate and

is the ambient · ε0

is the reference

718 ISOTROPIC (with TABLE Input - Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

1-10

1st

F

Enter A.

11-20

2nd

E

Enter B.

21-30

3rd

F

Enter n.

31-40

4th

F

Enter C.

41-50

5th

F

Enter m (default is 1.0)

51-60

6th

F

Enter

T melt .

61-70

7th

F

Enter

T room .

71-80

8th

F

Enter

· ε0

(default is

1.0s – 1 ).

15th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

ISOTROPIC (Stress) 719 Define Mechanical Data for Isotropic Materials

ISOTROPIC (Stress)

Define Mechanical Data for Isotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define material properties, a yield criterion, and a strain hardening law for an isotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the TEMPERATURE EFFECTS model definition. Defaults for this option are von Mises yield criterion, isotropic strain hardening law (with a slope of 0.0 if the WORK HARD model definition is omitted), and an equivalent yield stress of 1020. Therefore, the default is an elastic nonyielding isotropic material. See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 12 are repeated as a set, once for each set of isotropic material defined. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.),for cross-referencing TEMPERATURE EFFECTS and WORK HARD data.

6-15

Main Index

2nd

A

Enter one of the following yield criteria: ELASTIC

– Purely elastic material

VON MISES

– von Mises (Default).

HILL

– Hill’s (1948) Yield.

BARLAT

– Barlat’s (1991) Yield.

LIN MOHRC

– Linear Mohr-Coulomb.

PBL MOHRC

– Parabolic Mohr-Coulomb.

720 ISOTROPIC (Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

16-25

Free

3rd

Data Entry Entry

A

BUY MOHRC

– Buyukozturk Concrete Model.

NORM ORNL

– Normal ORNL.

CRMO ORNL

– 2-1/4 Cr-Mo ORNL.

REVP ORNL

– Reversed Plasticity ORNL.

ARST ORNL

– Full alpha reset ORNL.

GEN-PLAST

– Generalized Plasticity Model.

VISCO PLAS

– Viscoplastic model through the UVSCPL user subroutine.

RIGID

– Rigid-plastic material, no elasticity, von Mises yield.

IMPL CREEP

– Implicit creep model, both plasticity and creep, von Mises criterion.

Enter one of the following hardening rules: ISOTROPIC

– Isotropic hardening (Default).

KINEMATIC

– Kinematic hardening.

COMBINED

– Combined hardening (isotropic/kinematic).

CHABOCHE

– Nonlinear (in)viscid isotropic-kinematic hardening.

POWER LAW

–

RATE POWER LAW – JOHNSON-COOK

–

KUMAR

–

For superplastic forming analyses (SPF), only POWER LAW and RATE POWER LAW are available as hardening rules. 26-30

4th

I

Not used; enter 0.

31-35

5th

I

Enter 1 to turn on concrete cracking.

36-40

6th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file.

Main Index

ISOTROPIC (Stress) 721 Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry Enter -8 if data read in US from database.

41-45

7th

I

Number of viscoplastic parameters to be read through the 8th data block.

46-55

8th

A

Enter the material name to cross-reference with material data base for temperature dependent properties, strain rate, and work hardening effects.

4th data block The data entered in the following blocks should be the values at the lowest temperature expected during an analysis, not necessarily at the stress-free temperature. 1-10

1st

F

Young’s modulus (Not required for RIGID).

11-20

2nd

F

Poisson’s ratio (Not required for RIGID).

21-30

3rd

F

Mass density (stress analysis).

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Equivalent (von Mises) tensile yield stress. For Mohr-Coulomb behavior, this is at zero hydrostatic stress. For implicit creep, back stress.

51-60

6th

F

For ORNL yield criteria, equivalent 10th cycle tensile yield stress. For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used. For Mohr-Coulomb yield criteria, α-β parameter. For implicit creep, equivalent (von Mises) tensile yield stress.

61-70

7th

F

Enter the cost per unit volume.

71-80

8th

F

Enter the cost per unit mass.

5a data block Necessary only for Hill and Barlat’s yield criteria. 1-10

1st

F

YRDIR1 (for Hill) or M (for Barlat)

11-20

2nd

F

YRDIR2 (for Hill) or C1 (for Barlat)

21-30

3rd

F

YRDIR3 (for Hill) or C2 (for Barlat)

31-40

4th

F

YRSHR1 (for Hill) or C3 (for Barlat)

41-50

5th

F

YRSHR2 (for Hill) or C6 (for Barlat)

51-60

6th

F

YRSHR3 (for Hill)

5b data block The following blocks are only used for CHABOCHE hardening rule.

Main Index

722 ISOTROPIC (Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

1-10

1st

F

R0 for isotropic hardening.

11-20

2nd

F

R∞ for isotropic hardening (Q0 in case of using plastic-strain-range memorization, see 5c data block)

21-30

3rd

F

b coefficient for isotropic hardening.

31-40

4th

F

C coefficient for kinematic hardening.

41-50

5th

F

γ coefficient for kinematic hardening.

51-60

6th

F

K value for viscosity model.

61-70

7th

F

n coefficient for viscosity model.

5c data block Necessary only for CHABOCHE hardening rule with plastic-strain-range memorization. Notice that if no memorization is required, then provide a blank line. 1-10

1st

F

Qm coefficient for isotropic hardening.

11-20

2nd

F

μ coefficient for isotropic hardening.

21-30

3rd

F

η coefficient to introduce progressive memory.

6th data block Necessary only in a coupled thermal-stress analysis. 1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Resistivity (if Joule analysis)

41-50

5th

F

Emissivity.

7th data block Necessary only in a coupled electrostatic-stress analysis. 1-10

1st

F

Permittivity constant.

8th data block The following blocks are only used if viscoplastic material and the seventh field of data block 3 is greater than zero. Enter 8 fields per data line. 1-10

1st

Enter the first viscoplastic parameter

11-20

2nd

Enter the second viscoplastic parameter.

9th data block The following block is read in for Power Law or Rate Power Law model. Power Law Model –

Main Index

·n m σy = A ( εo + ε ) + B ε

ISOTROPIC (Stress) 723 Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

Rate Power Law Model –

m ·n σ y = A ε ε + B, σ 0

If the value is less than the minimum yield stress, the minimum yield stress is used. 1-10

1st

F

Enter coefficient A.

11-20

2nd

F

Enter exponent m.

21-30

3rd

F

Enter coefficient B.

31-40

4th

F

Enter exponent n.

41-50

5th

F

Enter

σ0

for the Rate Power Law Model or

If 0 is entered,

E ε 0 = ⎛ ---⎞ ⎝ A⎠

1 ------------m–1

and

ε0

for the Power Law Model.

σ0 = 0

The following blocks (10a and 10b) are read in for Kumar model only. σ = B 0 sinh

–1

· 1⁄n Q ⁄ ( nRT ) ⎛ ε----p-⎞ e ⎝ A⎠ B

A is a constant or

ln A = B 1 + B 2 ⁄ ε p B

n is a constant or

n = B4 + B 5 ⁄ εp

3

3

The activation energy (Q) is specified in the MATERIAL DATA option. The universal gas constant (R) is specified in the PARAMETERS option. 10a data block 1-10

1st

F

Enter coefficient B0.

11-20

2nd

F

Enter coefficient A; if A = 0, then B1, B2, and B3 is used.

21-30

3rd

F

Enter B1.

31-40

4th

F

Enter B2.

41-50

5th

F

Enter B3.

10b data block

Main Index

1-10

1st

E

Enter coefficient n; if n = 0, then B4, B5, and B6 is used.

11-20

2nd

E

Enter B4.

21-30

3rd

E

Enter B5.

31-40

4th

E

Enter B6.

724 ISOTROPIC (Stress) Define Mechanical Data for Isotropic Materials

Format Fixed

Free

Data Entry Entry

11th data block The following block is read in for the Johnson-Cook model. · T – T room ⎞ m⎞ ⎛ ε p⎞ ⎞ ⎛ n ⎛ ⎛ -------------------------------σ y = ( A + B ε p ) ⎜ 1 + C ln ⎜ ---· -⎟ ⎟ ⎝ 1 – ⎝ T ⎠ ⎠ ⎝ ε ⎠⎠ ⎝ m elt – T room 0

where

T

is the current temperature,

temperature. strain rate.

εp

T melt

is the material melt temperature, and

is the effective plastic strain,

A, B, C, n,

and

m

· εp

T room

is the effective plastic strain rate and

is the ambient · ε0

is the reference

are constants.

1-10

1st

F

Enter A.

11-20

2nd

E

Enter B.

21-30

3rd

F

Enter n.

31-40

4th

F

Enter C.

41-50

5th

F

Enter m (default is 1.0)

51-60

6th

F

Enter

T melt .

61-70

7th

F

Enter

T room .

71-80

8th

F

Enter

· ε0

(default is

1.0s – 1 ).

12th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

ORTHOTROPIC (with TABLE Input - Mechanical) 725 Define Mechanical Data for Orthotropic Materials

ORTHOTROPIC (with TABLE Input - Mechanical)

Define Mechanical Data for Orthotropic Materials

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define material properties, a yield criterion, and a strain hardening law for an orthotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the TABLE model definition option. Defaults for this option are von Mises yield criterion, isotropic strain hardening law (with a slope of 0, if the WORK HARD model definition is omitted), and an equivalent yield stress of 1020. Therefore, the default is an elastic nonyielding orthotropic material. See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 17 are entered as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.); for cross-referencing CREEP, FAIL DATA, etc., and user subroutines.

6-15

2nd

A

Enter one of the following yield criteria: ELASTIC

– Purely elastic material

VON MISES

– von Mises (Default)

HILL

– Hill’s (1948) Yield.

BARLAT

– Barlat’s (1991) Yield.

NORM ORNL – Normal ORNL CRMO ORNL – 2-1/4 Cr-Mo ORNL

Main Index

726 ORTHOTROPIC (with TABLE Input - Mechanical) Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry REVP ORNL

– Reversed Plasticity ORNL

ARST ORNL

– Full alpha reset ORNL

VISCO PLAS – Viscoplastic model through the UVSCPL user subroutine. 16-25

3rd

A

Enter one of the following hardening rules: ISOTROPIC

– Isotropic hardening (Default)

KINEMATIC

– Kinematic hardening

COMBINED

– Combined (isotropic/kinematic) hardening

26-30

4th

I

IANELS flag, enter 1 to call the ANELAS, HOOKLW ANPLAS, ANEXP, ANKOND, and ORIENT user subroutines.

31-35

5th

I

Not used, enter 0.

36-40

6th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file. Enter -8 if data read in US from database.

41-45

7th

I

Number of viscoplastic parameters to be read through data block 7b or the number of phases in this material.

46-57

8th

A

Enter the material name to cross-reference with material database.

Notes: Since all material properties in an orthotropic material are independent, it is your responsibility to enter all the data required to match the dimension of the stress-strain law of the elements listed for this material (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. The data entered in the following data lines are the reference values that are used with tables or are constants. These values are with respect to the user coordinate (1, 2, 3) system. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior. 4th data block

Main Index

1-10

1st

F

E11 – Young’s modulus.

11-20

2nd

F

E22 – Young’s modulus.

ORTHOTROPIC (with TABLE Input - Mechanical) 727 Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

E33 – Young’s modulus.

31-40

4th

F

ν12 – Poisson’s ratio.

41-50

5th

F

ν23 – Poisson’s ratio.

51-60

6th

F

ν31 – Poisson’s ratio.

61-70

7th

F

ρ

– Mass density (stress analysis).

5th data block 1-5

1st

I

Table ID for E11.

6-10

2nd

I

Table ID for E22.

11-15

3rd

I

Table ID for E33.

16-20

4th

I

Table ID for ν12.

21-25

5th

I

Table ID for ν23.

26-30

6th

I

Table ID for ν31.

31-35

7th

I

Table ID for mass density.

6th data block 1-10

1st

F

G12 – Shear modulus.

11-20

2nd

F

G23 – Shear modulus.

21-30

3rd

F

G31 – Shear modulus.

31-40

4th

F

α11 – Coefficients of thermal expansion.

41-50

5th

F

α22 – Coefficients of thermal expansion.

51-60

6th

F

α33 – Coefficients of thermal expansion.

61-70

7th

F

Enter the cost per unit volume.

71-80

8th

F

Enter the cost per unit mass.

7th data block

Main Index

1-5

1st

I

Table ID for G12.

6-10

2nd

I

Table ID for G23.

11-15

3rd

I

Table ID for G31.

16-20

4th

I

Table ID for α11.

21-25

5th

I

Table ID for α22.

26-30

6th

I

Table ID for α33.

728 ORTHOTROPIC (with TABLE Input - Mechanical) Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

8th data block 1-10

1st

F

Equivalent (von Mises) tensile yield stress. Default: 1020. (For implicit viscoplasticity, back stress.)

11-20

2nd

F

For ORNL, 10th cycle equivalent yield stress. For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used.

21-30

3rd

F

YRDIR1 (for Hill) or M (for Barlat).

30-40

4th

F

YRDIR2 (for Hill) or C1 (for Barlat).

41-50

5th

F

YRDIR3 (for Hill) or C2 (for Barlat).

51-60

6th

F

YRSHR1(for Hill) or C3 (for Barlat).

61-70

7th

F

YRSHR2 (for Hill) or C6 (for Barlat).

71-80

8th

F

YRSHR3 (for Hill)

9th data block 1-5

1st

I

Table ID for tensile yield stress.

6-10

2nd

I

Table ID for ORNL 10th cycle yield stress.

11-15

3rd

I

Table ID for YRDIR1 (for Hill) or M (for Barlat).

16-20

4th

I

Table ID for YRDIR2 (for Hill) or C1 (for Barlat).

21-25

5th

I

Table ID for YRDIR3 (for Hill) or C2 (for Barlat).

26-30

6th

I

Table ID for YRSHR1 (for Hill) or C3 (for Barlat).

31-35

7th

I

Table ID for YRSHR2 (for Hill) or C6 (for Barlat).

36-40

8th

I

Table ID for YRSHR3 (for Hill).

10th data block Necessary only in a coupled thermal-stress analysis.

Main Index

1-10

1st

F

K11 – Thermal conductivities.

11-20

2nd

F

K22 – Thermal conductivities.

21-30

3rd

F

K33 – Thermal conductivities.

31-40

4th

F

ρ

41-50

5th

F

Specific heat

– Mass density (heat transfer analysis).

ORTHOTROPIC (with TABLE Input - Mechanical) 729 Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

51-60

6th

F

R11 – If Joule heating analysis, resistivity.

61-70

7th

F

R22 – If Joule heating analysis, resistivity.

71-80

8th

F

R33 – If Joule heating analysis, resistivity.

11th data block Necessary only in a coupled thermal-stress analysis and the input format is 2 or greater. 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for mass density.

21-25

5th

I

Table ID for specific heat.

26-30

6th

I

Table ID for R11.

31-35

7th

I

Table ID for R22.

36-40

8th

I

Table ID for R33.

12th data block Necessary only if coupled thermal-stress. 1-10

1st

F

Emissivity

11-20

2nd

F

Enter the enthalpy of formation.

21-30

3rd

F

Enter the reference temperature of enthalpy of formation.

13th data block Necessary only in a coupled thermal-stress analysis. 1-5

1st

I

Table ID for emissivity.

6-10

2nd

I

Table ID for enthalpy of formation.

11-15

2nd

I

Table ID for reference temperature of enthalpy of formation.

14th data block Necessary only in a coupled electrostatic-stress analysis

Main Index

1-10

1st

F

ε11 – Electrical permittivity.

11-20

2nd

F

ε22 – Electrical permittivity.

21-30

3rd

F

ε33 – Electrical permittivity.

730 ORTHOTROPIC (with TABLE Input - Mechanical) Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

15th data block Necessary only in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for ε11 – Electrical permittivity.

6-10

2nd

I

Table ID for ε22 – Electrical permittivity.

11-15

3rd

I

Table ID for ε33 – Electrical permittivity.

16th data block The following data blocks are only required if viscoplastic material and the seventh field, data block 3, is entered. Enter 8 fields per block. 1-10

1st

F

Enter first viscoplastic parameter.

11-20

2nd

F

Enter second viscoplastic parameter.

17th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

ORTHOTROPIC (Mechanical) 731 Define Mechanical Data for Orthotropic Materials

ORTHOTROPIC (Mechanical)

Define Mechanical Data for Orthotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define material properties, a yield criterion, and a strain hardening law for an orthotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the ORTHO TEMP model definition. Defaults for this option are von Mises yield criterion, isotropic strain hardening law (with a slope of 0. if the WORK HARD model definition is omitted), and an equivalent yield stress of 1020. Therefore, the default is an elastic nonyielding orthotropic material. See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3-8 are entered as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.); for cross-referencing ORTHO TEMP, WORK HARD data and user subroutines.

6-15

2nd

A

Enter one of the following yield criteria: ELASTIC

– Purely elastic material

VON MISES

– von Mises (Default).

HILL

– Hill’s (1948) Yield.

BARLAT

– Barlat’s (1991) Yield.

NORM ORNL

– Normal ORNL.

CRMO ORNL – 2-1/4 Cr-Mo ORNL.

Main Index

732 ORTHOTROPIC (Mechanical) Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry REVP ORNL – Reversed Plasticity ORNL. ARST ORNL – Full alpha reset ORNL. VISCO PLAS – Viscoplastic model through the UVSCPL user subroutine.

16-25

3rd

A

Enter one of the following hardening rules: ISOTROPIC

– Isotropic hardening (Default).

KINEMATIC

– Kinematic hardening.

COMBINED

– Combined hardening; (isotropic/kinematic).

26-30

4th

I

IANELS flag, enter 1 to call the ANELAS, HOOKLW, ANPLAS, ANEXP, ANKOND, and ORIENT user subroutines.

31-35

5th

I

Not used, enter 0.

36-40

6th

I

Not used, enter 0.

41-45

7th

I

Number of viscoplastic parameters to be read through data block 7b.

46-55

8th

A

Enter the material name to cross-reference with material data base for temperature dependent properties, strain rate, and work hardening effects.

Notes: Since all material properties in an orthotropic material are independent, it is your responsibility to enter all the data required to match the dimension of the stress-strain law of the elements listed for this material (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. The data entered in the following data lines should be the values at the lowest temperature expected during an analysis, not necessarily at the stress-free temperature. These values are with respect to the user coordinate (1, 2, 3) system. 4th data block 1-10

1st

F

E11 – Young’s modulus.

11-20

2nd

F

E22 – Young’s modulus.

21-30

3rd

F

E33 – Young’s modulus.

31-40

4th

F

ν12 – Poisson’s ratio.

41-50

5th

F

ν23 – Poisson’s ratio.

51-60

6th

F

ν31 – Poisson’s ratio.

61-70

7th

F

ρ

– Mass density (stress analysis).

5th data block

Main Index

1-10

1st

F

G12 – Shear modulus.

11-20

2nd

F

G23 – Shear modulus.

ORTHOTROPIC (Mechanical) 733 Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

G31 – Shear modulus.

31-40

4th

F

α11 – Coefficients of thermal expansion.

41-50

5th

F

α22 – Coefficients of thermal expansion.

51-60

6th

F

α33 – Coefficients of thermal expansion.

61-70

7th

F

Enter the cost per unit volume.

71-80

8th

F

Enter the cost per unit mass.

6th data block 1-10

1st

F

Equivalent (von Mises) tensile yield stress. Default: 1020. (For implicit viscoplasticity, back stress.)

11-20

2nd

F

For ORNL, 10th cycle equivalent yield stress. For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used.

21-30

3rd

F

YRDIR1 (for Hill) or M (for Barlat)

30-40

4th

F

YRDIR2 (for Hill) or C1 (for Barlat)

41-50

5th

F

YRDIR3 (for Hill) or C2 (for Barlat)

51-60

6th

F

YRSHR1(for Hill) or C3 (for Barlat)

61-70

7th

F

YRSHR2 (for Hill) or C6 (for Barlat)

71-80

8th

F

YRSHR3 (for Hill)

7th data block Necessary only in a coupled thermal-stress analysis

Main Index

1-10

1st

F

K11 – Thermal conductivities.

11-20

2nd

F

K22 – Thermal conductivities.

21-30

3rd

F

K33 – Thermal conductivities.

31-40

4th

F

ρ

41-50

5th

F

Specific heat

51-60

6th

F

R11 – Resistivities (if Joule analysis).

61-70

7th

F

R22 – Resistivities (if Joule analysis).

71-80

8th

F

R33 – Resistivities (if Joule analysis).

– Mass density (heat transfer analysis).

734 ORTHOTROPIC (Mechanical) Define Mechanical Data for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

7b data block Necessary only if coupled and radiation analysis. 1-10

1st

F

Emissivity

7c data block Necessary only in a coupled electrostatic-stress analysis 1-10

1st

F

ε11 – Electric permittivity.

11-20

2nd

F

ε22 – Electric permittivity.

21-30

3rd

F

ε33 – Electric permittivity.

7d data block The following data block is only required if viscoplastic material and the seventh field, data block 3, is entered. Enter 8 fields per block. 1-10

1st

F

Enter first viscoplastic parameter.

11-20

2nd

F

Enter second viscoplastic parameter.

Note:

Data block 7d is provided for possible future expansion. Implicit viscoplasticity (through the UVSCPL user subroutine) or implicit creep is not currently supported for

orthotropic materials. 8th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.).

Main Index

ANISOTROPIC (with TABLE Input - Mechanical) 735 Stress or Coupled-Thermal Stress Analysis

ANISOTROPIC (with TABLE Input Mechanical)

Stress or Coupled-Thermal Stress Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description A general temperature dependent orthotropic material model is available through the Marc input file by the use of the ORTHOTROPIC and TABLE options. If a more general model is needed, you can supply such a model through the ANELAS, HOOKLW, ANEXP, ANKOND, ANPLAS, or ORIENT user subroutines. Two ways to request a call to these subroutines are shown below: • Use the flag (3rd data block, fourth field) on the ORTHOTROPIC option to modify the material

data entered there. • Use the ANISOTROPIC model definition option to call these subroutines.

See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ANISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of anisotropic material data sets to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3, 4, 5, 6, and 7 are repeated as a set NSET times. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing CREEP, FAIL DATA, etc., and user subroutines.

6-15

2nd

A

Enter one of the following yield criteria: ELASTIC

–

Purely elastic material

VON MISES

–

von Mises (default)

HILL

–

Hill’s (1948) Yield.

BARLAT

–

Barlat’s (1991) Yield.

NORM ORNL –

Main Index

Normal ORNL

736 ANISOTROPIC (with TABLE Input - Mechanical) Stress or Coupled-Thermal Stress Analysis

Format Fixed

16-25

26-30

Free

3rd

4th

Data Entry Entry

A

I

CRMO ORNL –

2-1.3 Cr-Mo ORNL

REVP ORNL

–

Reversed Plasticity ORNL

ARST ORNL

–

Full alpha reset ORNL

Enter one of the following hardening rules: ISOTROPIC

–

Isotropic hardening (default)

KINEMATIC

–

Kinematic hardening

COMBINED

–

Combined hardening (isotropic/kinematic)

Enter 1 if the ANELAS, ANEXP, ANPLAS, and HOOKLW user subroutines are to be called. Enter 2 if the anisotropic stress strain law, etc., is to be entered in data blocks (6th data block).

31-35

5th

I

Not used; enter 0.

36-40

6th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file. Enter -8 if data read in US from database.

41-45

7th

I

Not used; enter 0.

46-57

8th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

Mass density (stress analysis).

11-20

2nd

F

Equivalent (von Mises) yield stress.

21-30

3rd

F

If ORNL yielding, 10th cycle yield stress. For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used.

Main Index

31-40

4th

F

Mass density (heat transfer analysis).

41-50

5th

F

Specific Heat.

51-60

6th

F

Electrical resistance.

ANISOTROPIC (with TABLE Input - Mechanical) 737 Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

61-70

7th

F

Cost of material per unit volume (optional).

71-80

8th

F

Cost of material per unit mass (optional).

5th data block 1-5

1st

I

Table ID for mass density.

6-10

2nd

I

Table ID for equivalent yield stress.

11-15

3rd

I

Table ID for ORNL 10th cycle yield.

16-20

4th

I

Table ID for mass density (heat transfer).

21-25

5th

I

Table ID for specific heat.

26-30

6th

I

Table ID for electrical resistance.

Data blocks 6a to 6ee are only required if the fourth field of the 3rd data block is 2. 6a data block 1-10

1st

F

C11

11-20

2nd

F

C12

21-30

3rd

F

C13

31-40

4th

F

C14

41-50

5th

F

C15

51-60

6th

F

C16

61-70

7th

F

C22

71-80

8th

F

C23

6aa data block 1-5

1st

I

Table ID for C11

6-10

2nd

I

Table ID for C12

11-15

3rd

I

Table ID for C13

16-20

4th

I

Table ID for C14

21-25

5th

I

Table ID for C15

26-30

6th

I

Table ID for C16

31-35

7th

I

Table ID for C22

36-40

8th

I

Table ID for C23

F

C24

6b data block 1-10

Main Index

1st

738 ANISOTROPIC (with TABLE Input - Mechanical) Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

11-20

2nd

F

C25

21-30

3rd

F

C26

31-40

4th

F

C33

41-50

5th

F

C34

51-60

6th

F

C35

61-70

7th

F

C36

71-80

8th

F

C44

6bb data block 1-5

1st

I

Table ID for C24

6-10

2nd

I

Table ID for C25

11-15

3rd

I

Table ID for C26

16-20

4th

I

Table ID for C33

21-25

5th

I

Table ID for C34

26-30

6th

I

Table ID for C35

31-35

7th

I

Table ID for C36

36-40

8th

I

Table ID for C44

6c data block 1-10

1st

F

C45

11-20

2nd

F

C46

21-30

3rd

F

C55

31-40

4th

F

C56

41-50

5th

F

C66

6cc data block

Main Index

1-5

1st

I

Table ID for C45

6-10

2nd

I

Table ID for C46

11-15

3rd

I

Table ID for C55

16-20

4th

I

Table ID for C56

21-25

5th

I

Table ID for C66

ANISOTROPIC (with TABLE Input - Mechanical) 739 Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

Use only as many terms as are required for the element type chosen. All three (A, B, and C) blocks must be used. For plane stress, only C11, C12, C13, C22, C24, C33 must be entered. 6d data block 1-10

1st

F

α11

11-20

2nd

F

α12

21-30

3rd

F

α13

31-40

4th

F

α22

41-50

5th

F

α23

51-60

6th

F

α33

6dd data block 1-5

1st

I

Table ID for α11

6-10

2nd

I

Table ID for α12

11-15

3rd

I

Table ID for α13

16-20

4th

I

Table ID for α22

21-25

5th

I

Table ID for α23

26-30

6th

I

Table ID for α33

6e data block 1-10

1st

F

YRDIR1 (for Hill) or M (for Barlat)

11-20

2nd

F

YRDIR2 (for Hill) or C1 (for Barlat)

21-30

3rd

F

YRDIR3 (for Hill) or C2 (for Barlat)

31-40

4th

F

YRSHR1 (for Hill) or C3 (for Barlat)

41-50

5th

F

YRSHR2 (for Hill) or C6 (for Barlat)

51-60

6th

F

YRSHR3 (for Hill)

6ee data block

Main Index

1-10

1st

I

Table ID for YRDIR1 (for Hill) or M (for Barlat)

11-20

2nd

I

Table ID for YRDIR2 (for Hill) or C1 (for Barlat)

21-30

3rd

I

Table ID for YRDIR3 (for Hill) or C2 (for Barlat)

31-40

4th

I

Table ID for YRSHR1 (for Hill) or C3 (for Barlat)

41-50

5th

I

Table ID for YRSHR2 (for Hill) or C6 (for Barlat)

51-60

6th

I

Table ID for YRSHR3 (for Hill)

740 ANISOTROPIC (with TABLE Input - Mechanical) Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

Data blocks 6f and 6ff are only required if the fourth field is a 2 in a coupled analysis. 6f data block 1-10

1st

F

K11

11-20

2nd

F

K12

21-30

3rd

F

K13

31-40

4th

F

K22

41-50

5th

F

K23

51-60

6th

F

K33

6ff data block 1-5

1st

I

Table ID for K11

6-10

2nd

I

Table ID for K12

11-15

3rd

I

Table ID for K13

16-20

4th

I

Table ID for K22

21-25

5th

I

Table ID for K23

26-30

6th

I

Table ID for K33

Data blocks 6g and 6gg are only required if the fourth field of the 3rd data block is a 2 and a Joule heating analysis is being performed. 6g data block 1-10

1st

F

R11 – Resistivity if Joule heating.

11-20

2nd

F

R12 – Resistivity if Joule heating.

21-30

3rd

F

R13 – Resistivity if Joule heating.

31-40

4th

F

R22 – Resistivity if Joule heating.

41-50

5th

F

R23 – Resistivity if Joule heating.

51-60

6th

F

R33 – Resistivity if Joule heating.

6gg data block

Main Index

1-5

1st

I

R11 – Table IDs if Joule heating.

6-10

2nd

I

R12 – Table IDs if Joule heating.

11-15

3rd

I

R13 – able IDs if Joule heating.

16-20

4th

I

R22 – Table IDs if Joule heating.

ANISOTROPIC (with TABLE Input - Mechanical) 741 Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

21-25

5th

I

R23 – Table IDs if Joule heating.

26-30

6th

I

R33 – Table IDs if Joule heating.

7th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

742 ANISOTROPIC (Mechanical) Stress or Coupled-Thermal Stress Analysis

ANISOTROPIC (Mechanical)

Stress or Coupled-Thermal Stress Analysis

The information provided here is based upon not using the table driven input style. Description A general temperature dependent orthotropic material model is available through the Marc input file by the use of the ORTHOTROPIC and ORTHO TEMP options. If a more general model is needed, you can supply such a model through the ANELAS, HOOKLW, ANEXP, ANKOND, ANPLAS, or ORIENT user subroutines. Two ways to request a call to these subroutines are shown below: • Use the flag (3rd data block, fourth field) on the ORTHOTROPIC option to modify the material

data entered there. • Use the ANISOTROPIC model definition option to call these subroutines.

See Tables 3-12 and 3-13 to determine procedure used when the LARGE STRAIN parameter is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ANISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of anisotropic material data sets to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3, 4, and 5 are repeated as a set NSET times. 3rd data block

Main Index

1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing ORTHO TEMP, WORK HARD data and user subroutines.

6-15

2nd

A

Enter one of the following yield criteria: VON MISES

–

von Mises (default)

HILL

–

Hill’s (1948) Yield.

BARLAT

–

Barlat’s (1991) Yield.

NORM ORNL –

Normal ORNL

CRMO ORNL –

2-1.3 Cr-Mo ORNL

ANISOTROPIC (Mechanical) 743 Stress or Coupled-Thermal Stress Analysis

Format Fixed

16-25

26-30

Free

3rd

4th

Data Entry Entry

A

I

REVP ORNL

–

Reversed Plasticity ORNL

ARST ORNL

–

Full alpha reset ORNL

Enter one of the following hardening rules: ISOTROPIC

–

Isotropic hardening (default)

KINEMATIC

–

Kinematic hardening

COMBINED

–

Combined hardening (isotropic/kinematic)

Enter 1 if the ANELAS, ANEXP, ANPLAS, and HOOKLW user subroutines are to be called. Enter 2 if the anisotropic stress strain law, etc., is to be entered in data blocks (4a, 4b, 4c, 4d, 4e, 4f).

4th data block 1-10

1st

F

Mass density (stress analysis)

11-20

2nd

F

Equivalent (von Mises) yield stress

21-30

3rd

F

If ORNL yielding, 10th cycle yield stress. For von Mises, Hill, and Barlat criteria with combined hardening, enter the kinematic hardening fraction (F: 0 to 1) F = 0: Pure isotropic hardening, F = 1: pure kinematic hardening, 0 < F < 1: combined hardening. This is only available if the PLASTICITY,4 parameter is used.

31-40

4th

F

Mass density (heat transfer analysis)

41-50

5th

F

Specific Heat

51-60

6th

F

Leave blank.

61-70

7th

F

Cost of material per unit volume (optional).

71-80

8th

F

Cost of material per unit mass (optional).

Data blocks 4a, 4b, and 4c used to define anisotropic elastic stress strain relation. Data block 4a only required if the fourth field is a 2. 4a data block

Main Index

1-10

1st

F

C11

11-20

2nd

F

C12

21-30

3rd

F

C13

31-40

4th

F

C14

41-50

5th

F

C15

744 ANISOTROPIC (Mechanical) Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

51-60

6th

F

C16

61-70

7th

F

C22

71-80

8th

F

C23

Data block 4b only required if the fourth field is a 2. 4b data block 1-10

1st

F

C24

11-20

2nd

F

C25

21-30

3rd

F

C26

31-40

4th

F

C33

41-50

5th

F

C34

51-60

6th

F

C35

61-70

7th

F

C36

71-80

8th

F

C44

Data block 4c only required if the fourth field is a 2 4c data block 1-10

1st

F

C45

11-20

2nd

F

C46

21-30

3rd

F

C55

31-40

4th

F

C56

41-50

5th

F

C66

Use only as many terms as are required for the element type chosen. All three blocks must be used. For plane stress, only C11, C12, C13, C22, C24, C33 must be entered. Data block 4d is only required if the fourth field is a 2. It defines the anisotropic thermal expansion coefficients. 4d data block

Main Index

1-10

1st

F

α11

11-20

2nd

F

α12

21-30

3rd

F

α13

ANISOTROPIC (Mechanical) 745 Stress or Coupled-Thermal Stress Analysis

Format Fixed

Free

Data Entry Entry

31-40

4th

F

α22

41-50

5th

F

α23

51-60

6th

F

α33

Data block 4e is only required if the fourth field is a 2. It defines the anisotropic plasticity. 4e data block 1-10

1st

F

YRDIR1 (for Hill) or M (for Barlat)

11-20

2nd

F

YRDIR2 (for Hill) or C1 (for Barlat)

21-30

3rd

F

YRDIR3 (for Hill) or C2 (for Barlat)

31-40

4th

F

YRSHR1 (for Hill) or C3 (for Barlat)

41-50

5th

F

YRSHR2 (for Hill) or C6 (for Barlat)

51-60

6th

F

YRSHR3 (for Hill)

Data block 4f required only if the fourth field is a 2 and heat transfer is included. 4f data block 1-10

1st

F

K11

11-20

2nd

F

K12

21-30

3rd

F

K13

31-40

4th

F

K22

41-50

5th

F

K23

51-60

6th

F

K33

Data block 4g required only if the fourth field is a 2 and Joule heating is included. 4g data block 1-10

1st

F

R11

11-20

2nd

F

R12

21-30

3rd

F

R13

31-40

4th

F

R22

41-50

5th

F

R23

51-60

6th

F

R33

5th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

746 HYPOELASTIC (with TABLE Input) Define Data for Hypoelastic Materials

HYPOELASTIC (with TABLE Input)

Define Data for Hypoelastic Materials

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to input data associated with Marc’s hypoelastic material model. You must define the material stress/strain law through the HYPELA2 user subroutine (or, for element type 52 or 98 without using numerically integrated solid cross section, the UBEAM user subroutine). Note:

In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word HYPOELASTIC.

2nd data block 1-5

1st

I

Enter the number of hypoelastic material data sets to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3, 4, 5, and 6 are repeated as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing CREEP, etc., and user subroutines.

6-10

2nd

I

Enter 1 to call the ANEXP and ORIENT user subroutines.

11-15

3rd

I

Flag to use the HYPELA2 user subroutine. Enter 1 to pass in deformation gradient (F) and rotation (R). Enter 2 to pass in deformation gradient (F) and stretch ratios (λ). Enter 3 to pass in F, R, and λ. Enter 13 to pass in F, R, and λ. Kinematic quantities are calculated at the mid increment if the LARGE STRAIN parameter is used which results in logarithmic strains. Enter 23 to pass in F, R, and λ. Kinematic quantities are calculated at the end of the increment if the LARGE STRAIN parameter is used.

Main Index

HYPOELASTIC (with TABLE Input) 747 Define Data for Hypoelastic Materials

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database for temperature dependent properties, strain rate, and workhardening effects.

4th data block 1-10

1st

F

ρ – mass density (stress analysis).

11-20

2nd

F

α – coefficient of thermal expansion.

21-30

3rd

F

K – thermal conductivity.

31-40

4th

F

Specific heat.

41-50

5th

F

Resistivity.

51-60

6th

F

ρ – mass density (heat transfer analysis).

61-70

7th

F

Emissivity.

5th data block 1-5

1st

I

Table ID for mass density.

6-10

2nd

I

Table ID for coefficient of thermal expansion.

11-15

3rd

I

Table ID for thermal conductivity.

16-20

4th

I

Table ID for specific heat.

21-25

5th

I

Table ID for electrical resistivity.

26-30

6th

I

Table ID for mass density (heat transfer).

31-35

7th

I

Table ID for emissivity.

6th data block Enter a list of elements using this material model. (Do not enter composite elements using this material in a layer.)

Main Index

748 HYPOELASTIC Define Data for Hypoelastic Materials

HYPOELASTIC

Define Data for Hypoelastic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to input data associated with Marc’s hypoelastic material model. You must define the material stress/strain law through the HYPELA2 user subroutine (or, for element type 52 or 98 without using numerically integrated solid cross section, the UBEAM user subroutine). Note:

In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word HYPOELASTIC.

2nd data block 1-5

1st

I

Enter the number of hypoelastic material data sets to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data block 3, 4, 5 are repeated as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing TEMPERATURE EFFECTS data and user subroutines.

6-10

2nd

I

Enter 1 to call the ANEXP and ORIENT user subroutines.

11-15

3rd

I

Flag to use the HYPELA2 user subroutine. Enter 1 to pass in deformation gradient (F) and rotation (R). Enter 2 to pass in deformation gradient (F) and stretch ratios (λ). Enter 3 to pass in F, R, and λ. Enter 13 to pass in F, R, and λ. Kinematic quantities are calculated at the mid increment if the LARGE STRAIN parameter is used which results in logarithmic strains. Enter 23 to pass in F, R, and λ. Kinematic quantities are calculated at the end of the increment if the LARGE STRAIN parameter is used.

Main Index

HYPOELASTIC 749 Define Data for Hypoelastic Materials

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

ρ – mass density (stress analysis).

11-20

2nd

F

α – coefficient of thermal expansion.

21-30

3rd

F

K – thermal conductivity.

31-40

4th

F

Specific heat.

41-50

5th

F

Resistivity (if Joule analysis).

51-60

6th

F

ρ – mass density (heat transfer analysis).

61-70

7th

F

Emissivity.

5th data block Enter a list of elements using this material model. (Do not enter composite elements using this material in a layer.)

Main Index

750 MOONEY (with TABLE Input) Define Data for Mooney-Rivlin Materials

MOONEY (with TABLE Input)

Define Data for Mooney-Rivlin Materials

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to enter all the material data for a Mooney-Rivlin rubber material. The UMOONY user subroutine can be used to enter temperature dependent coefficients. The UENERG user subroutine can be used to enter a general strain energy function. If rate effects are also present, the VISCELMOON model definition option can also be required. A list of elements can also be associated with this material. The strain energy function is: W = C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 ) + C 11 ( I 1 – 3 ) ⋅ ( I 2 – 3 ) + C 20 ( I 1 – 3 ) 2 + C 30 ( I 1 – 3 ) 3 + U

where

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i= 1

Notes:

For a Neo-Hookean material model, only C10 is needed. For a Mooney/Rivlin material model, only C10 and C01 are needed. For the full 3rd-order invariant model of Jamus, Green and Simpson, use all C10, C01, C11, C20, C30. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case must be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements with Total Lagrange are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. These material identifications cannot be referenced by any composite group. The values C10, C01, C11, C20, and C30 can be redefined using the UMOONY user subroutine.

Main Index

MOONEY (with TABLE Input) 751 Define Data for Mooney-Rivlin Materials

Although a general strain energy function can be defined by using the UENERG user subroutine, it is still required to define the elements associated with the material identifier here. The UELASTOMER user subroutine may be used to define a general material based upon the strain invariants. It is always called when the updated Lagrange procedure is used. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word MOONEY.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 12 are repeated as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Data input mode - Enter 0.

16-20

4th

I

Not used; enter 0.

21-32

5th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

C10 – Mooney-Rivlin constant.

11-20

2nd

F

C01 – Mooney-Rivlin constant.

21-30

3rd

F

ρ

– mass density (stress analysis).

31-40

4th

F

α

– coefficient of thermal expansion.

41-50

5th

F

C11 – higher order constants

51-60

6th

F

C20 – higher order constants.

61-70

7th

F

C30 – higher order constants.

71-80

8th

F

K

5th data block

Main Index

– bulk modulus.

752 MOONEY (with TABLE Input) Define Data for Mooney-Rivlin Materials

Format Fixed

Free

Data Entry Entry

Only necessary for input format 2 or greater. 1-5

1st

I

Table ID for C10.

6-10

2nd

I

Table ID for C01.

11-15

3rd

I

Table ID for mass density.

16-20

4th

I

Table ID for α.

21-25

5th

I

Table ID for C11.

26-30

6th

I

Table ID for C20.

31-35

7th

I

Table ID for C30.

36-40

8th

I

Table ID for K.

6th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

7th data block 1-5

1st

I

Table ID for

D1 .

6-10

2nd

I

Table ID for

D2 .

11-15

3rd

I

Table ID for

D3 .

16-20

4th

I

Table ID for

D4 .

21-25

5th

I

Table ID for

D5 .

8th data block Only necessary in a coupled thermal-stress analysis.

Main Index

1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistance.

41-50

5th

F

Emissivity.

MOONEY (with TABLE Input) 753 Define Data for Mooney-Rivlin Materials

Format Fixed

Free

Data Entry Entry

9th data block Necessary only in a coupled thermal-stress analysis. 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

10th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

11th data block Only necessary in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for permittivity constant.

12th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

754 MOONEY Define Data for Mooney-Rivlin Materials

MOONEY

Define Data for Mooney-Rivlin Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to enter all the material data for a Mooney-Rivlin rubber material. The UMOONY user subroutine can be used to enter temperature dependent coefficients. The UENERG or UELASTOMER user subroutine can be used to enter a general strain energy function. If rate effects are present, the VISCELMOON model definition option can be used. A list of elements can also be associated with this material. The strain energy function is: W = C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 ) + C 11 ( I 1 – 3 ) ⋅ ( I 2 – 3 ) + C 20 ( I 1 – 3 ) 2 + C 30 ( I 1 – 3 ) 3 + U

where

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i= 1

Notes:

For a Neo-Hookean material model, only C10 is needed. For a Mooney/Rivlin material model, only C10 and C01 are needed. For the full third-order invariant model of James-Green-Simpson, use all C10, C01, C11, C20, C30. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior The values C10, C01, C11, C20, and C30 can be redefined using the UMOONY user subroutine.

Main Index

MOONEY 755 Define Data for Mooney-Rivlin Materials

Although a general strain energy function can be defined by using the UENERG user subroutine, it is still required to define the elements associated with the material identifier here. The UELASTOMER user subroutine may be used to define a general material based upon the strain invariants. It is always called when the updated Lagrange procedure is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word MOONEY.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 8 are repeated as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number.

4th data block 1-10

1st

F

C10 – Mooney-Rivlin constant.

11-20

2nd

F

C01 – Mooney-Rivlin constant.

21-30

3rd

F

ρ

– mass density (stress analysis).

31-40

4th

F

α

– coefficient of thermal expansion.

41-50

5th

F

C11 – higher order constant.

51-60

6th

F

C20 – higher order constant.

61-70

7th

F

C30 – higher order constant.

71-80

8th

F

K

– bulk modulus.

5th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0.

Main Index

1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

756 MOONEY Define Data for Mooney-Rivlin Materials

Format Fixed

Free

Data Entry Entry

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

6th data block Only necessary in a coupled thermal-stress analysis 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Resistivity (if Joule analysis).

41-50

5th

F

Emissivity.

7th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

8th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

ARRUDBOYCE (with TABLE Input) 757 Define Data for Arruda-Boyce Model

ARRUDBOYCE (with TABLE Input)

Define Data for Arruda-Boyce Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to enter all the material data for the Arruda-Boyce rubber material model. The UARRBO user subroutine can be used to enter temperature dependent coefficients. If rate effects are also present, the VISCELMOON model definition option may also be required. A list of elements can also be associated with this material. The strain energy function is: 2 3 4 5 1 1 11 19 519 W = n kθ --- ( I 1 – 3 ) + ---------- ⎛⎝ I – 9⎞⎠ + ------------------2- ⎛ I – 27⎞ + ------------------3- ⎛ I – 81⎞ + ------------------------4- ⎛ I – 243⎞ + U ⎝ ⎠ ⎝ ⎠ ⎝ ⎠ 2 20N 1 1050 N 1 7000 N 1 673750N 1

where

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i =1

Notes:

This model is very sensitive to material instabilities. Positive, physical coefficients are essential. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior

Main Index

758 ARRUDBOYCE (with TABLE Input) Define Data for Arruda-Boyce Model

These material identifications cannot be referenced by any composite group. The values nkθ and N can be redefined using the UARRBO user subroutine. For nkθ = 2C1 and N → ∞, one term Mooney-Rivlin (or Neo-Hookean) material model can be recovered. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ARRUDBOYCE.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 12 are repeated as a set; once for each data set. 3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Data Input Mode; enter 0

16-20

4th

I

Not used; enter 0.

21-32

5th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

nkθ –

linear term where n is the chain density, k is the Boltzmann constant, and θ is the temperature.

11-20

2nd

F

N

–

number of links between chemical crosslinks.

21-30

3rd

F

ρ

–

mass density (stress analysis).

31-40

4th

F

α

–

coefficient of thermal expansion.

41-50

5th

F

K

–

bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

5th data block

Main Index

1-5

1st

I

Table ID for rubber modulus (nkθ).

6-10

2nd

I

Table ID for N.

11-15

3rd

I

Table ID for mass density.

ARRUDBOYCE (with TABLE Input) 759 Define Data for Arruda-Boyce Model

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Table ID for coefficient of thermal expansion.

21-25

5th

I

Table ID for bulk modulus.

6th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

7th data block 1-5

1st

I

Table ID for

D1 .

6-10

2nd

I

Table ID for

D2 .

11-15

3rd

I

Table ID for

D3 .

16-20

4th

I

Table ID for

D4 .

21-25

5th

I

Table ID for

D5 .

8th data block Necessary only in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistivity.

41-50

5th

F

Emissivity.

9th data block Necessary only in a coupled thermal-stress analysis.

Main Index

1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

760 ARRUDBOYCE (with TABLE Input) Define Data for Arruda-Boyce Model

Format Fixed

Free

Data Entry Entry

10th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

11th data block Only necessary in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for permittivity constant.

12th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

ARRUDBOYCE 761 Define Data for Arruda-Boyce Model

ARRUDBOYCE

Define Data for Arruda-Boyce Model

The information provided here is based upon not using the table driven input style. Description This option allows you to enter all the material data for the Arruda-Boyce rubber material model. The UARRBO user subroutine can be used to enter temperature dependent coefficients. If rate effects are also present, the VISCELMOON model definition option may also be required. A list of elements can also be associated with this material. The strain energy function is: 2 3 4 5 1 1 11 19 519 W = n kθ --- ( I 1 – 3 ) + ---------- ⎛⎝ I – 9⎞⎠ + ------------------2- ⎛ I – 27⎞ + ------------------3- ⎛ I – 81⎞ + ------------------------4- ⎛ I – 243⎞ + U ⎝ ⎠ ⎝ ⎠ ⎝ ⎠ 2 20N 1 1050 N 1 7000 N 1 673750N 1

where

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i =1

Notes:

This model is very sensitive to material instabilities. Positive, physical coefficients are essential. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior These material identifications cannot be referenced by any composite group.

Main Index

762 ARRUDBOYCE Define Data for Arruda-Boyce Model

The values nkθ and N can be redefined using the UARRBO user subroutine. For nkθ = 2C1 and N → ∞, one term Mooney-Rivlin (or Neo-Hookean) material model can be recovered. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ARRUDBOYCE.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 8 are repeated as a set; once for each data set. 3rd data block 1-5

1st

I

Material identification number.

4th data block 1-10

1st

F

nkθ –

linear term where n is the chain density, k is the Boltzmann constant, and θ is the temperature.

11-20

2nd

F

N

–

number of statistical links of length in the chain between chemical crosslinks.

21-30

3rd

F

ρ

–

mass density (stress analysis).

31-40

4th

F

α

–

coefficient of thermal expansion.

41-50

5th

F

K

–

bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

5th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0.

Main Index

1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

ARRUDBOYCE 763 Define Data for Arruda-Boyce Model

Format Fixed

Free

Data Entry Entry

6th data block Only necessary in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis). Note:

In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior.

31-40

4th

F

Resistivity (if Joule analysis).

41-50

5th

F

Emissivity.

7th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

8th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

764 GENT (with TABLE Input) Define Data for the Gent Model

GENT (with TABLE Input)

Define Data for the Gent Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to enter all the material data for the Gent rubber material model. The UGENT user subroutine can be used to enter temperature dependent coefficients. If rate effects are also present, the VISCELMOON model definition option can also be required. A list of elements can also be associated with this material. The strain energy function is: I 1* –E W = ------ I m log ⎛ 1 – -----⎞ + U ⎝ 6 I m⎠

where

where

I 1* = I 1 – 3

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i= 1

Notes:

Negative coefficients are nonphysical. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults of isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior These material identifications cannot be referenced by any composite group. The values E and Im can be redefined using the UGENT user subroutine.

Main Index

GENT (with TABLE Input) 765 Define Data for the Gent Model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GENT.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 12 are repeated as a set; once for each data set. 3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Data Input mode; enter 0

16-20

4th

I

Not used; enter 0.

21-32

5th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

ρ

– mass density (stress analysis).

11-20

2nd

F

α

– coefficient of thermal expansion.

21-30

3rd

F

E

– small strain tensile modulus.

31-40

4th

F

Im – maximum value of first invariant (defines maximum stretch in the chains). I m > 3

41-50

5th

F

K

– bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

5th data block

Main Index

1-5

1st

I

Table ID for mass density.

6-10

2nd

I

Table ID for coefficient of thermal expansion.

11-15

3rd

I

Table ID for small strain tensile modulus.

16-20

4th

I

Table ID for maximum value of first invariant.

21-25

5th

I

Table ID for bulk modulus.

766 GENT (with TABLE Input) Define Data for the Gent Model

Format Fixed

Free

Data Entry Entry

6th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

7th data block 1-5

1st

I

Table ID for

D1 .

6-10

2nd

I

Table ID for

D2 .

11-15

3rd

I

Table ID for

D3 .

16-20

4th

I

Table ID for

D4 .

21-25

5th

I

Table ID for

D5 .

8th data block Only necessary in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistivity.

41-50

5th

F

Emissivity.

9th data block Necessary only in a coupled thermal-stress analysis. 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

10th data block Only necessary in a coupled electrostatic-stress analysis 1-10

Main Index

1st

F

Permittivity constant.

GENT (with TABLE Input) 767 Define Data for the Gent Model

Format Fixed

Free

Data Entry Entry

11th data block Only necessary in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for permittivity constant.

12th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

768 GENT Define Data for the Gent Model

GENT

Define Data for the Gent Model

The information provided here is based upon not using the table driven input style. Description This option allows you to enter all the material data for the Gent rubber material model. The UGENT user subroutine can be used to enter temperature dependent coefficients. If rate effects are also present, the VISCELMOON model definition option can also be required. A list of elements can also be associated with this material. The strain energy function is: I 1* –E W = ------ I m log ⎛ 1 – -----⎞ + U ⎝ 6 I m⎠

where

where

I 1* = I 1 – 3

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i= 1

Notes:

Negative coefficients are nonphysical. The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the Total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the Updated Lagrange formulation is used, either Herrmann or displacement elements may be used. (Near-incompressibility is imposed by using the mixed approach and condensing out the pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults of isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior These material identifications cannot be referenced by any composite group. The values E and Im can be redefined using the UGENT user subroutine.

Main Index

GENT 769 Define Data for the Gent Model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GENT.

2nd data block 1-5

1st

I

Enter the number of data sets to follow.

6-10

2nd

I

Unit number for data input. Defaults to input file.

Data blocks 3 through 8 are repeated as a set; once for each data set. 3rd data block 1-5

1st

I

Material identification number.

4th data block 1-10

1st

F

ρ

– mass density (stress analysis).

11-20

2nd

F

α

– coefficient of thermal expansion.

21-30

3rd

F

E

– small strain tensile modulus.

31-40

4th

F

Im – maximum value of first invariant (defines maximum stretch in the chains). I m > 3 .

41-50

5th

F

K

– bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

5th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

6th data block Only necessary in a coupled thermal-stress analysis.

Main Index

1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

770 GENT Define Data for the Gent Model

Format Fixed 21-30

Free 3rd

Data Entry Entry F

Mass density (heat transfer analysis). Note:

In a coupled thermal-stress analysis, the thermal material model defaults of isotropic heat transfer behavior.

31-40

4th

F

Resistivity (if Joule analysis).

41-50

5th

F

Emissivity.

7th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

8th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

OGDEN (with TABLE Input) 771 Define Data for Ogden or Principal Stretch Based Material Model

OGDEN (with TABLE Input)

Define Data for Ogden or Principal Stretch Based Material Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define the data associated with the Ogden model for incompressible and nearly incompressible rubber material. The strain energy function for this model has the form: N

∑

W =

n =1

where

μ α α α –α ⁄ 3 -----n- [ J n ( λ 1 n + λ 2 n + λ 3 n ) – 3 ] + U αn

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i =1

This option can also be used to activate the general principal stretch based models through the UELASTOMER and UOGDEN user subroutines. Notes:

The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the updated Lagrange formulation is invoked, the elements must be conventional displacement formulation. (Near-incompressibility is imposed using mixed approach and condensing out pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior

Main Index

772 OGDEN (with TABLE Input) Define Data for Ogden or Principal Stretch Based Material Model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word OGDEN.

2nd data block 1-5

1st

I

Enter the number of sets of Ogden material data to follow (optional).

6-10

2nd

I

Enter the logical unit number for input. Defaults to input file.

Data blocks 3 through 13 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the material identification.

6-10

2nd

I

Enter the number of terms (N) that defines the strain energy function.

11-15

3rd

I

Enter 1 for Ogden model (default). Enter 3 for generalized principal stretch based model using the UELASTOMER user subroutine.

16-20

4th

I

Data input mode; enter 0.

21-32

5th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

K - bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

11-20

2nd

F

Enter the mass density.

21-30

3rd

F

Enter the coefficient of thermal expansion.

31-40

4th

F

Reference value of modulus μ.

41-50

5th

F

Reference value of exponent α.

If the table IDs of the 4th and 5th fields of the 5th data block are zero, then the reference values ( μ , β ) are not used and the 12th data block is used instead. 5th data block

Main Index

1-5

1st

I

Table ID for bulk modulus.

6-10

2nd

I

Table ID for mass density.

11-15

3rd

I

Table ID for coefficient of thermal expansion.

16-20

4th

I

Table ID for modulus.

21-25

5th

I

Table ID for exponent.

α,

OGDEN (with TABLE Input) 773 Define Data for Ogden or Principal Stretch Based Material Model

Format Fixed

Free

Data Entry Entry

6th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

7th data block 1-5

1st

I

Table ID for

D1 .

6-10

2nd

I

Table ID for

D2 .

11-15

3rd

I

Table ID for

D3 .

16-20

4th

I

Table ID for

D4 .

21-25

5th

I

Table ID for

D5 .

8th data block Only necessary in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistivity.

41-50

5th

F

Emissivity.

9th data block Necessary only in a coupled thermal-stress analysis. 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

10th data block Only necessary in a coupled electrostatic-stress analysis 1-10

Main Index

1st

F

Permittivity constant.

774 OGDEN (with TABLE Input) Define Data for Ogden or Principal Stretch Based Material Model

Format Fixed

Free

Data Entry Entry

11th data block Only necessary in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for permittivity constant.

Data block 12 is repeated once for each term specified in the 3rd data block. Not used if generalized stretch based model. Not used if table based input is used and the table IDs given on the 5th data block are nonzero. 12th data block 1-10

1st

F

Enter the modulus.

11-20

2nd

F

Enter the power.

13th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

OGDEN 775 Define Data for Ogden or Principal Stretch Based Material Model

OGDEN

Define Data for Ogden or Principal Stretch Based Material Model

The information provided here is based upon not using the table driven input style. Description This option allows you to define the data associated with the Ogden model for incompressible and nearly incompressible rubber material. The strain energy function for this model has the form: N

∑

W =

n =1

where

μ –α ⁄ 3 α α α -----n- [ J n ( λ 1 n + λ 2 n + λ 3 n ) – 3 ] + U αn

9 U = --- K ( J – 1 ) 2 2

A series form of the volumetric strain energy U to capture the nonlinear pressure-volumetric strain relationship is also implemented and can be used by using a FEATURE,3402 parameter in the input. The volumetric strain energy is expressed as: J

U =

∑ Di ( J – 1 ) 2 i =1

This option can also be used to activate the general principal stretch based models through the UELASTOMER user subroutine. Notes:

The procedure used is defined on the LARGE DISP or LARGE STRAIN parameters. If the total Lagrange formulation is invoked, the elements in this case can be of the Herrmann formulation except for plane stress. If the updated Lagrange formulation is invoked, the elements must be conventional displacement formulation. (Near-incompressibility is imposed using mixed approach and condensing out pressure degrees of freedom.) For plane stress, displacement elements are always used. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior The UELASTOMER user subroutine is only available in the updated Lagrange mode.

Main Index

776 OGDEN Define Data for Ogden or Principal Stretch Based Material Model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word OGDEN.

2nd data block 1-5

1st

I

Enter the number of sets of Ogden material data to follow (optional).

6-10

2nd

I

Enter the logical unit number for input. Defaults to input file.

Data blocks 3 through 8 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the material identification.

6-10

2nd

I

Enter the number of terms (N) which define the strain energy function.

11-15

3rd

I

Enter 1 for Ogden model (default). Enter 3 for generalized principal stretch based model using the UELASTOMER user subroutine.

4th data block 1-10

1st

F

K - bulk modulus; default is such that the material is incompressible (enter -1 if a series form of volumetric free energy is flagged in a FEATURE,3402 parameter).

11-20

2nd

F

Enter the mass density.

21-30

3rd

F

Enter the coefficient of thermal expansion.

5th data block Only necessary for analysis with FEATURE,3402 parameter and user-specified bulk modulus of -1.0. 1-10

1st

F

D1

coefficient of the volumetric strain energy function.

11-20

2nd

F

D2

coefficient of the volumetric strain energy function.

21-30

3rd

F

D3

coefficient of the volumetric strain energy function.

31-40

4th

F

D4

coefficient of the volumetric strain energy function.

41-50

5th

F

D5

coefficient of the volumetric strain energy function.

6th data block Only necessary in a coupled thermal-stress analysis.

Main Index

1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

OGDEN 777 Define Data for Ogden or Principal Stretch Based Material Model

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Resistivity (if Joule analysis).

41-50

5th

F

Emissivity.

7th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

Data block 8 is repeated once for each term specified in the 3rd data block. Not used if generalized stretch based model. 8th data block 1-10

1st

F

Enter the modulus.

11-20

2nd

F

Enter the power.

9th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

778 NLELAST Simplified Nonlinear Elastic Models Input

NLELAST

Simplified Nonlinear Elastic Models Input

Description This option allows for the input of simplified nonlinear elastic models, which do not have a well defined strain energy function. It allows an easy way to represent behavior that is observed in tests. See Marc Volume A: Theory and User Information for further details. Notes:

When used in conjunction with the LARGE DISP parameter, the table used to enter the stress-strain data should be the second Piola Kirchhoff stress versus the Green Lagrange strain. When used in conjunction with LARGE DISP, UPDATE, and FINITE, or PLASTICITY,3, or LARGE STRAIN, the stress-strain data should be the true (Cauchy) stress versus logarithmic strain. It is not recommended to represent materials when large strains are present. The MD Nastran compatible model with Herrmann elements shows slow convergence; conventional displacement elements should be used. The principal strain-loaded model (3) and the orthotropic model (6) cannot be used with Herrmann elements.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word NLELAST.

2nd data block 1-5

1st

I

Number of distinct sets of NLELAST entries (optional).

6-10

2nd

I

Enter unit number for input of NLELAST data (default to standard input).

Repeat 3rd through 18th data block for each NLELAST material defined. 3rd data block 1-5

1st

I

Enter the material ID.

6-10

2nd

I

Material model: Enter 1 for Nastran compatible model. Enter 2 for invariant based model. Enter 3 for principal strain based model. Enter 4 for linear elasticity with tension compression limits.

Main Index

NLELAST 779 Simplified Nonlinear Elastic Models Input

Format Fixed

Free

Data Entry Entry Enter 5 for bi-modulus linear elasticity with tension compression limits. Enter 6 for orthotropic nonlinear elasticity based upon strains in local direction.

11-15

3rd

I

Enter 1 if Bilateral model; i.e., both tension and compression data will be used (default). Enter 2 if only tension data will be used (Nastran pre-Version 64).

16-20

4th

I

Enter 1 to indicate constant Poisson’s ratio (default) (Nastran model). Enter 2 to indicate constant bulk modulus (Nastran model).

21-25

5th

I

Enter 0 – material has no limits on tension/compression behavior (default). Enter 1 to activate no/limited tension model. Enter 2 to activate no/limited compression model. Enter 3 to activate no/limited tension and/or compression model.

26-37

6th

A

Enter the material name to cross reference with material database.

4th data block – For models 1,2,3,4 or 5 1-10

1st

E

Model model 1or 3; enter the reference value to the stress-strain curve; default=1.0. For model 2, enter the reference Young’s modulus. For model 4 or 5, enter the reference value of Young’s modulus for tensile behavior.

11-20

2nd

E

Enter the Poisson’s ratio.

21-30

3rd

E

Enter the mass density.

31-40

4th

E

Enter the coefficient of thermal expansion.

41-50

5th

E

Enter the Shear modulus for material model 3.

51-60

6th

E

Tensile stress limit if 5th field of 3rd data block is 1 or 3.

61-70

7th

E

Compressive stress limit if 5th field of 3rd data block is 2 or 3.

5th data block For models 1, 2, 3, 4, or 5

Main Index

1-5

1st

I

Enter the table ID used to describe stress-strain law.

6-10

2nd

I

Enter the table ID for Poisson’s ratio.

11-15

3rd

I

Enter the table ID for mass density.

16-20

4th

I

Enter the table ID for coefficient of thermal expansion.

780 NLELAST Simplified Nonlinear Elastic Models Input

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Enter the table ID for the shear modulus for material model 3.

26-30

6th

I

Enter the table ID for tensile stress limit.

31-35

7th

I

Enter the table ID for compressive stress limit.

6th data block - for model 5 only 1-10

1st

E

For model 5; enter the reference value of Young’s modulus for compressive behavior.

11-20

2nd

E

Enter the Poisson’s ratio for compressive behavior.

7th data block - for model 5 only 1-5

1st

I

Enter the table ID for Young’s modulus for compressive behavior.

6-10

2nd

I

Enter the table ID for Poisson’s ratio for compressive behavior.

8th data block – for model 6 only 1-10

1st

E

E 11

– Reference value for Young’s modulus.

11-20

2nd

E

E 22

– Reference value for Young’s modulus.

21-30

3rd

E

E 33

– Reference value for Young’s modulus.

31-40

4th

E

ν 12

– Reference value for Poisson’s ratio.

41-50

5th

E

ν 23

– Reference value for Poisson’s ratio

51-60

6th

E

ν 31

– Reference value for Poisson’s ratio

61-70

7th

E

ρ

– Mass density (stress analysis)

9th data block – for model 6 only 1-5

1st

I

Table ID for

E 11 .

6-10

2nd

I

Table ID for

E 22 .

11-15

3rd

I

Table ID for

E 33 .

16-20

4th

I

Table ID for

ν 12 .

21-25

5th

I

Table ID for

ν 23 .

26-30

6th

I

Table ID for

ν 31 .

31-35

7th

I

Table ID for ρ .

10th data block – for model 6 only

Main Index

1-10

1st

E

G 12

– Reference value for shear modulus.

11-20

2nd

E

G 23

– Reference value for shear modulus.

NLELAST 781 Simplified Nonlinear Elastic Models Input

Format Fixed

Free

Data Entry Entry

21-30

3rd

E

G 31

– Reference value for shear modulus.

31-40

4th

E

α 11

– Coefficient of thermal expansion.

41-50

5th

E

α 22

– Coefficient of thermal expansion.

51-60

6th

E

α 33

– Coefficient of thermal expansion.

11th data block – for model 6 only 1-5

1st

I

Table ID for

G 12 .

6-10

2nd

I

Table ID for

G 23 .

11-15

3rd

I

Table ID for

G 31 .

16-20

4th

I

Table ID for

α 11 .

21-25

5th

I

Table ID for

α 22 .

26-30

6th

I

Table ID for

α 33 .

12th data block (only required in a coupled thermal-stress analysis) models 1-5 1-10

1st

E

Enter the thermal conductivity.

11-20

2nd

E

Enter the specific heat.

21-30

3rd

E

Enter the mass density (heat transfer analysis).

31-40

4th

E

Enter the electrical resistance (Joule Analysis).

41-50

5th

E

Enter the emissivity.

13th data block (only required in a coupled thermal-stress analysis), models 1-5 1-5

1st

I

Enter the table ID used for thermal conductivity.

6-10

2nd

I

Enter the table ID for specific heat.

11-15

3rd

I

Enter the table ID for mass density.

16-20

4th

I

Enter the table ID for electrical resistance.

21-25

5th

I

Enter the table ID for emissivity.

14th data block (only required for coupled thermal-stress analysis) model 6

Main Index

1-10

1st

F

K11 – Thermal conductivities.

11-20

2nd

F

K22 – Thermal conductivities.

21-30

3rd

F

K33 – Thermal conductivities.

31-40

4th

F

ρ

41-50

5th

F

Specific heat

– Mass density (heat transfer analysis).

782 NLELAST Simplified Nonlinear Elastic Models Input

Format Fixed

Free

Data Entry Entry

51-60

6th

F

R11 – If Joule heating analysis, resistivity.

61-70

7th

F

R22 – If Joule heating analysis, resistivity.

71-80

8th

F

R33 – If Joule heating analysis, resistivity.

15th data block (only required for coupled thermal-stress analysis) model 6 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for mass density.

21-25

5th

I

Table ID for specific heat.

26-30

6th

I

Table ID for R11.

31-35

7th

I

Table ID for R22.

36-40

8th

I

Table ID for R33.

16th data block (only required for coupled thermal-stress analysis) model 6 1-10

1st

F

Emissivity

11-20

2nd

F

Enter the enthalpy of formation.

21-30

3rd

F

Enter the reference temperature of enthalpy of formation.

17th data block (only required for coupled thermal-stress analysis) model 6 1-5

1st

I

Table ID for emissivity.

6-10

2nd

I

Table ID for enthalpy of formation.

11-15

2nd

I

Table ID for reference temperature of enthalpy of formation.

18th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

FOAM (with TABLE Input) 783 Define Data for Foam Material Model

FOAM (with TABLE Input)

Define Data for Foam Material Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define the data associated with the foam model for highly compressible rubber material. The foam model can be used for plane strain, axisymmetric, and solid elements using the conventional displacement elements. The strain energy function for this model has the form. N

W =

∑ n =1

Notes:

μ α α α -----n- ( λ 1 n + λ 2 n + λ 3 n – 3 ) + αn

N

∑ n=1

μ β -----n ( 1 – J n ) βn

In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. The foam model is only available for continuum elements (plane strain, axisymmetric, or solids) for Total Lagrange or Updated Lagrange. The procedure used for the Foam formulation is defined on the LARGE DISP or LARGE STRAIN parameters.

The use of the UELASTOMER user subroutine is only available in updated Lagrange mode. Viscoelasticity may be included in the updated Lagrange mode using the VISCELFOAM model definition option. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior If the bulk modulus is entered, then βi = 0 for all values of i. If the bulk modulus is zero and all βi are 0, then the material is treated as an Ogden material.

Main Index

784 FOAM (with TABLE Input) Define Data for Foam Material Model

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word FOAM.

2nd data block 1-5

1st

I

Enter the number of sets of Foam material data to follow (optional).

6-10

2nd

I

Enter the logical unit number for input. Defaults to input file.

Data blocks 3 through 11 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the material identification.

6-10

2nd

I

Enter the number of terms (N) that defines the strain energy function.

11-15

3rd

I

Data input mode; enter 0.

16-20

4th

I

Flag for user-defined foam models: = 0 no user-defined foam model (default). = 1 energy function based on strain invariants. = 2 energy function based on principal stretches. = 3 energy function based on strain invariants and with the form of deviatoric split. = 4 energy function based on principal stretches and with the form of deviatoric split

21-32

5th

A

Enter the material name to cross-reference with material database for temperature dependent properties, strain rate, and workhardening effects.

4th data block 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Enter the mass density.

21-30

3rd

F

Enter the coefficient of thermal expansion.

31-40

4th

F

Enter reference value of modulus μ.

41-50

5th

F

Enter reference value of exponent α.

51-60

6th

F

Enter reference value of exponent β.

If the table IDs of the 4th, 5th, and 6th fields of the 5th data block are zero, then the reference values ( μ , α , β ) are not used and the 8th data block is used instead.

Main Index

FOAM (with TABLE Input) 785 Define Data for Foam Material Model

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for mass density.

11-15

3rd

I

Table ID for coefficient of thermal expansion.

16-20

4th

I

Table ID for modulus μ.

21-25

5th

I

Table ID for exponent α.

26-30

6th

I

Table ID for exponent β.

6th data block Only necessary in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Electrical resistance.

41-50

5th

F

Emissivity.

7th data block Necessary only in a coupled thermal-stress analysis. 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

8th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

9th data block Only necessary in a coupled electrostatic-stress analysis 1-5

1st

I

Table ID for permittivity constant.

Data block 10 is repeated once for each term specified in the 3rd data block. Not used if the table based input is used and the table IDs given on the 5th data block are nonzero.

Main Index

786 FOAM (with TABLE Input) Define Data for Foam Material Model

Format Fixed

Free

Data Entry Entry

10th data block 1-10

1st

F

Enter the modulus ( μ n ).

11-15

2nd

F

Enter the power for deviatoric behavior ( α n ).

21-30

3rd

F

Enter the power for volumetric behavior ( β n ).

11th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

FOAM 787 Define Data for Foam Material Model

FOAM

Define Data for Foam Material Model

The information provided here is based upon not using the table driven input style. Description This option allows you to define the data associated with the foam model for highly compressible rubber material. The foam model can be used for plane strain, axisymmetric, and solid elements using the conventional displacement elements. The strain energy function for this model has the form. N

W =

∑ n =1

Notes:

μ α α α -----n- ( λ 1 n + λ 2 n + λ 3 n – 3 ) + αn

N

∑ n=1

μ β -----n ( 1 – J n ) βn

In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. The foam model is only available for continuum elements (plane strain, axisymmetric, or solids) for Total Lagrange or Updated Lagrange. The procedure used for the Foam formulation is defined on the LARGE DISP or LARGE STRAIN parameters.

The use of the UELASTOMER user subroutine is only available in updated Lagrange mode. Viscoelasticity may be included in the updated Lagrange mode using the VISCELFOAM model definition option. In a coupled thermal-stress analysis, the thermal material model defaults to isotropic heat transfer behavior. In a coupled electrostatic-stress analysis, the electrostatic material model defaults to isotropic electrostatic behavior Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word FOAM.

2nd data block

Main Index

1-5

1st

I

Enter the number of sets of Foam material data to follow (optional).

6-10

2nd

I

Enter the logical unit number for input. Defaults to input file.

788 FOAM Define Data for Foam Material Model

Format Fixed

Free

Data Entry Entry

Data blocks 3 through 8 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the material identification.

6-10

2nd

I

Enter the number of terms (N) which define the strain energy function.

11-15

3rd

i

Not used; enter 0.

16-20

4th

I

Flag for user-defined foam models: = 0 no user-defined foam model (default). = 1 energy function based on strain invariants. = 2 energy function based on principal stretches. = 3 energy function based on strain invariants and with the form of deviatoric split. = 4 energy function based on principal stretches and with the form of deviatoric split

4th data block 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Enter the mass density.

21-30

3rd

F

Enter the coefficient of thermal expansion.

31-40

4th

F

Enter reference value of modulus μ.

41-50

5th

F

Enter reference value of exponent α.

51-60

6th

F

Enter reference value of exponent β.

5th data block Only necessary in a coupled thermal-stress analysis. 1-10

1st

F

Conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Resistivity (if Joule analysis).

41-50

5th

F

Emissivity.

6th data block Only necessary in a coupled electrostatic-stress analysis 1-10

1st

F

Permittivity constant.

Data block 7 is repeated once for each term specified in the 3rd data block.

Main Index

FOAM 789 Define Data for Foam Material Model

Format Fixed

Free

Data Entry Entry

7th data block 1-10

1st

F

Enter the modulus (μn).

11-15

2nd

F

Enter the power for deviatoric behavior (αn).

21-30

3rd

F

Enter the power for volumetric behavior (βn).

8th data block Enter a list of element numbers associated with this particular elastomeric material.

Main Index

790 GASKET Define Material Data for Gasket Materials

GASKET

Define Material Data for Gasket Materials

Description This option allows you to specify the material properties for a gasket material, such as the loading and unloading paths, the yield pressure, the transverse shear modulus and the membrane behavior of the gasket (see Gasket in Marc Volume A: Theory and User Information). The loading and unloading paths should be defined using the TABLE option and must be given as a relation between the pressure on the gasket and the gasket closure (variable type 37). The reference value of these tables is always 1. The loading and unloading curves may also be a function of the temperature type (variable 12), and the coordinates (variable types 5, 6, and 7). The yield pressure, tensile modulus, and transverse modulus can be functions of the temperature and coordinates. The initial gap can only be a function of the coordinates. The membrane behavior should be specified using the ISOTROPIC option. Note:

This option can be used only with the lower-order solid composite element types 149, 151, and 152.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word GASKET.

2nd data block 1-5

1st

I

Enter the number of sets of gasket material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 7 are repeated as a set; once for each set of gasket material to be input. 3rd data block

Main Index

1-5

1st

I

Enter the gasket material identification number.

6-10

2nd

I

Enter the material identification number of the isotropic material to be used for the membrane behavior of the gasket. In a coupled analysis, the thermal properties are also associated with this material ID.

GASKET 791 Define Material Data for Gasket Materials

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Enter gasket behavior type in the thickness direction. Currently only type 0 (elastic-plastic) is supported.

6-10

2nd

I

Enter the table identification number of the loading path of the gasket.

11-15

3rd

I

Enter the number of unloading paths to be read through data block 4a. If a 0 is entered here, the gasket behavior will be fully elastic. Up to 10 unloading paths may be specified.

4a data block Necessary only if the number of unloading paths entered in the 3rd field of the 4th data block is nonzero. 1-5

1st

I

Enter the table identification number of the first unloading path of the gasket.

6-10

2nd

I

Enter the table identification number of the second unloading path of the gasket if present.

11-15

3rd

I

Enter the table identification number of the third unloading path of the gasket if present.

16-20

4th

I

Enter the table identification number of the fourth unloading path of the gasket if present.

21-25

5th

I

Enter the table identification number of the fifth unloading path of the gasket if present.

26-30

6th

I

Enter the table identification number of the sixth unloading path of the gasket if present.

31-35

7th

I

Enter the table identification number of the seventh unloading path of the gasket if present.

36-40

8th

I

Enter the table identification number of the eighth unloading path of the gasket if present.

41-45

9th

I

Enter the table identification number of the ninth unloading path of the gasket if present.

46-50

10th

I

Enter the table identification number of the tenth unloading path of the gasket if present.

5th data block

Main Index

1-10

1st

F

Enter the yield pressure.

11-20

2nd

F

Enter the tensile modulus (pressure per unit length).

21-30

3rd

F

Enter the transverse shear modulus (force per unit area).

31-40

4th

F

Enter the initial gap.

792 GASKET Define Material Data for Gasket Materials

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the table identification number associated with the yield pressure.

6-10

2nd

I

Enter the table identification number associated with the tensile modulus.

11-15

3rd

I

Enter the table identification number associated with the transverse shear modulus.

16-20

4th

I

Enter the table identification number associated with the initial gap.

7th data block Enter a list of elements associated with this material. The elements have to be of lower-order solid composite type (element types 149, 151, or 152).

Main Index

TABLE 793 Define Table

TABLE

Define Table

Description This option defines the data associated with a function or parametric input. These tables are referenced when defining material properties, boundary conditions, contact, and springs. A quantity may be a function of up to four independent variables. The function may be defined either in a piecewise linear manner using a set of points or by a mathematical equation. The value used in the analysis is the value of the evaluated table obtained by linear interpolation multiplied by the reference value given in the input. If the reference value is entered as 0.0, it is taken as 1.0 and, hence, the table value is used. The scaling by the reference value is useful when applying boundary conditions. If the independent variable is out of range of the table, the user can specify whether the function should be evaluated at the endpoint of the table or by extrapolation. When an equation is defined, the value used in the analysis is the evaluation of the equation multiplied by the reference value. If the reference value is entered as 0.0, it is taken as 1.0 and, hence, the equation is not scaled. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word TABLE.

11-42

2nd

A

Enter the table name.

2nd data block 1-5

1st

I

Table ID.

6-10

2nd

I

Number of independent variables.

11-15

3rd

I

Unit number to read data.

16-20

4th

I

Set to 1 to suppress printout.

21-25

5th

I

Enter method to read function: 0 – one row at a time 1 – one data point at a time 2 – read X 1 , function pairs (only available if number of independent variables is one). 3 – a formula is used.

Main Index

794 TABLE Define Table

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter the first independent variable type.

6-10

2nd

I

Enter the number of

11-15

3rd

I

Enter 1 to not allow extrapolation of

X1

data points (nw1).

Enter 2 to allow extrapolation of

X1

(default).

X1 .

16-20

4th

I

Enter the second independent variable type.

21-25

5th

I

Enter the number of

26-30

6th

I

Enter 1 to not allow extrapolation of

X2

data points (nw2).

Enter 2 to allow extrapolation of

X2

(default).

X2 .

31-35

7th

I

Enter the third independent variable type.

36-40

8th

I

Enter the number of

41-45

9th

I

Enter 1 to not allow extrapolation of

X3

data points (nw3).

Enter 2 to allow extrapolation of

X3

(default).

X3 .

46-50

10th

I

Enter the fourth independent variable type.

51-55

11th

I

Enter the number of

56-60

12th

I

Enter 1 to not allow extrapolation of

X4

data points (nw4).

Enter 2 to allow extrapolation of

X4

(default).

X4 .

Independent Variable Type 1 time 2 normalized time

28 contact force 29 contact body

3 increment number

30 σn (normal stress) 31 voltage 32 current 33 ⎛ current radius ⎞ 2 ------------------------------------ (see THROAT) ⎝ ⎠

4 normalized increment 5 x coordinate 6 y coordinate

F M

55 normalized arc distance 56 distance to other contact surface (near contact only) 57 term of series 58 hydrostatic stress 59 hydrostatic strain 60 B g, p = m· g, p ⁄ αm .

radius of throat

34

χp

(pyrolysis damage).

61

8

35

φw

(water vapor fraction).

62 2nd state variable

36

χc

(coking damage).

63 3rd state variable

s = x2 + y2 + z2 9 θ angle 10 mode number

Main Index

B g, w = m· g, w ⁄ αm .

7 z coordinate

37 gasket closure distance

64 4th state variable

TABLE 795 Define Table

11 12 13 14 15

frequency temperature function fourier

16

· ε (equivalent strain rate) B g = m· ⁄ αm (normalized

17

ε

p

(equivalent plastic strain)

mass flow rate). 18 arc length 19 relative density (not available for shells) 20 σ (equivalent stress) 21 magnetic induction 22 velocity 23 particle diameter 24 x0 coordinate 25 y0 coordinate 26 z0 coordinate 27

s0 =

2

2

2

x0 + y0 + z0

38 39 40 41 42

displacement magnitude stress rate experimental data porosity void ratio

65 66 67 68 69

43

·c ε

70 1st strain invariant

(equivalent creep strain rate) 44 minor principal total strain

5th state variable loadcase number degree of cure magnetic field intensity equivalent mechanical strain

71 2nd strain invariant

45 distance from neutral axis 72 (-t/2, +t/2) 46 normalized distance from neutral 73 axis (-1, +1) 47 local x-coordinate of layer point 74 for open or closed section beam 48 local y-coordinate of layer point 75 for open or closed section beam 49 1st isoparametric coordinate -1 to (not available in this release) -100 50 2nd isoparametric coordinate (not available in this release) 51 wavelength (used in spectral radiation) 52 creep strain ε er 53 pressure or primary quantity in diffusion 54 equivalent strain rate for nonNewtonian viscosity

3rd strain invariant any strain component damage accumulated crack growth parametric variable 1 to 100

Independent variable types (5, 6, 7) will have the following characteristics. 1. When used to evaluate material behavior, they will be original integration point coordinates unless the updated Lagrange procedure is used. 2. When used to evaluate DIST LOADS, they will be the original integration point coordinates unless the FOLLOW FOR parameter is used. 3. When used to evaluate boundary conditions FIXED DISP, etc. or POINT LOAD, etc., they will be the original nodal coordinates unless the FOLLOW FOR parameter is used. Independent variable types (24, 25, 26) have the same characteristics as (4, 5, 6) except the original nodal coordinate will be used for FIXED DISP or POINT LOAD, regardless of whether the FOLLOW FOR parameter is invoked. Note:

Main Index

If remeshing occurs, then “original” means the coordinates after the remeshing is done.

796 TABLE Define Table

If the method to read the function is 0, use the 4th, 5th, 6th, 7th, and 8a data blocks. If the method to read the function is 1, use the 4th, 5th, 6th, 7th, and 8b data blocks. If the method to read the function is 2, use the 9th data block. If the method to read the function is 3, use the 10th data block. A mathematical formula may be either 80 characters or 160 characters long if EXTENDED input format is used. The formula is defined in terms of independent variables V1, V2, V3, and/or V4, where the meaning of those variables is based on the variable type defined in the 3rd data block. The evaluation is based upon usual mathematical standards moving from left to right with the conventional rules of the use of parentheses. The following mathematical symbols/operations are available. +

addition

-

subtraction

*

multiplication

/

division

^

exponential

!

factor

%

mod

In addition to V1, V2, V3, and V4, the following constants may be used in the equation: pi

p

e

exponent

tz

offset temperature entered via PARAMETERS option

q

Activation energy entered via MATERIAL DATA option

r

Universal gas constant entered via PARAMETERS option

sb

Stefan Boltzman constant entered via PARAMETERS option

The following mathematical functions may be used in an equation:

Main Index

cos

cosine (x)

x in radians

sin

sine (x)

x in radians

tan

tangent (x)

x in radians

dcos

cosine (x)

x in degrees

dsin

sine (x)

x in degrees

dtan

tangent (x)

x in degrees

TABLE 797 Define Table

acos

inverse cosine (x)

f in radians

asin

inverse sine (x)

f in radians

atan

inverse tangent (x)

f in radians

atan2

inverse tangent (x,y)

f in radians

dacos

inverse cosine (x)

f in degrees

dasin

inverse sine (x)

f in degrees

datan

inverse tangent (x)

f in degrees

datan2

inverse tangent (x,y)

f in degrees

log

log based 10

ln

natural log

exp

exponent

cosh

hyperbolic cosine

sinh

hyperbolic sine

tanh

hyperbolic tangent

acosh

inverse hyperbolic cosine

asinh

inverse hyperbolic sine

atanh

inverse hyperbolic tangent

sqrt

square root

rad

convert degrees to radians

deg

convert radians to degrees

abs

obtain absolute value

int

truncates the value to whole

frac

take the fractional value

max

takes the maximal value

min

takes the minimal value

mod

return the remainder of x, based on y mod(x,y) = x - y * int (x/y)

Example 1

If a load on a cantilever has a linear dependence on x and a sinusoidal variation with time between 0 and 1 second, you would enter A * V 1 * sin ( 2. * pi * V 2 )

where the first variable is type 5 (x-coordinate) and the second variable is type 1 (time).

Main Index

798 TABLE Define Table

Example 2

If the creep strain rate is described by the Dorn-Weertman relation n –Q ⁄ R T · εc = A σ e ,

the formula would be A * V 1 ^n * exp ( – q ⁄ ( R * V 2 ) )

where V1, the first variable, is type 20 (equivalent stress) and V2, the second variable, is type 12 (temperature).

Format Fixed

Free

Data Entry Entry

The 4th data block is used to give the values of the first independent variable. Enter nw1 values, 8 values per line. Repeat as necessary, the data points must be in ascending order. If the independent variable is a parametric variable, this data block is not required. The value of the parametric variable is 1 to nw1 and is given on the output. 4th data block 1-10

1st

E

Enter first data point for first independent variable.

11-20

2nd

E

Enter second data point for first independent variable.

21-30

3rd

E

Enter third data point for first independent variable.

etc. The 5th data block is used to give the values of the second independent variable. If there is only one independent variable, skip to data line 8. Enter nw2 values, 8 values per line. Repeat as necessary, the data points must be in ascending order. If the independent variable is a parametric variable, this data block is not required. The value of the parametric variable is 1 to nw2, and is given on the output. 5th data block 1-10

1st

E

Enter first data point for second independent variable.

11-20

2nd

E

Enter second data point for second independent variable.

21-30

3rd

E

Enter third data point for second independent variable.

etc. The 6th data block is used to give the values of the third independent variable. If there is only one independent variable, skip to data line 8. Enter nw3 values, 8 values per line. Repeat as necessary, the data points must be in ascending order. If the independent variable is a parametric variable, this data block is not required. The value of the parametric variable is 1 to nw3 and is given on the output. 6th data block

Main Index

1-10

1st

E

Enter first data point for third independent variable.

11-20

2nd

E

Enter second data point for third independent variable.

TABLE 799 Define Table

Format Fixed

Free

21-30

Data Entry Entry

3rd

E

Enter third data point for third independent variable.

etc. The 7th data block is used to give the values of the fourth independent variable. If there is only one independent variable, skip to data line 8. Enter nw4 values, 8 values per line. Repeat as necessary, the data points must be in ascending order. If the independent variable is a parametric variable, this data block is not required. The value of the parametric variable is 1 to nw4 and is given on the output. 7th data block 1-10

1st

E

Enter first data point for fourth independent variable.

11-20

2nd

E

Enter second data point for fourth independent variable.

21-30

3rd

E

Enter third data point for fourth independent variable.

etc. 8th data block If the reading method is zero (5th field of line 2), the function is read by giving nw1 data points (nw4*nw3*nw2) times. The program reads the data using the following method. do k4=1, nw4 do k3=1, nw3 do k2=1, nw2 read nw1 values f(X1, K2, K3, K4) enddo enddo enddo The nw1 data are read in 8 per line using the following 7a block format 8a data block 1-10

1st

E

Enter first value of function.

11-20

2nd

E

Enter second value of function.

21-30

3rd

E

Enter third value of function.

etc.

Main Index

800 TABLE Define Table

Format Fixed

Free

Data Entry Entry

If the reading method is one (5th field of line 2), the function is read one value at a time; hence, nw1*nw2*nw3*nw4 lines. do k4=1, nw4 do k3=1, nw3 do k2=1, nw2 do k1=1, nw1 read one values f(K1, K2, K3, K4) enddo enddo enddo enddo The value is read using the 8b block format. 8b data block 1-10

1st

E

Enter value of function.

9th data block Only used if read method = 2; enter nw1 line each with the value of independent variable and function. If the independent variable is a parameter, enter the value of the function in the first field. 1-10

1st

E

Enter value of independent variable

11-20

2nd

E

Enter value of function.

Only used if read method = 3, enter a line with the formula. 10th data block 1-80

Main Index

1st

A

Enter formula.

STRAIN RATE (Material Properties) 801 Define Strain Rate Dependent Yield Stress

STRAIN RATE (Material Properties) Define Strain Rate Dependent Yield Stress The information provided here is based upon not using the table driven input style. If table driven input is provided, the strain rate dependence should be defined in the table unless the Cowper-Symonds model is used. For the Cowper-Symonds model, this option should be used. Description This option allows the definition of a strain rate dependent yield stress, for use in dynamic and flow (for example, extrusion) problems. This can also be used in static analysis by entering a fictitious time using the TIME STEP option. The zero strain rate yield stress is given on the ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC options. This option must be repeated for each different material for which strain rate data is necessary. The yield stress variation with strain rate is given using one of three options: a. The breakpoints and slopes for a piecewise linear approximation to the yield stress strain rate curve are given. The strain rate breakpoints should be in ascending order, or b. The yield stress and stain rate data points lying on the yield stress, strain rate curve are input directly. The data is entered in ascending order of strain rate. This method is flagged by entering the word DATA on the first data block. c. The Cowper and Symonds model is used. The yield stress is scaled with a factor

· 1⁄P ε . 1 + ⎛ ----⎞ ⎝ C⎠

Note that if multiple material models are used, they must all be expressed as piecewise linear, or as Cowper and Symonds model. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words STRAIN RATE.

13-80

2nd

A

Enter the word DATA to indicate that option B is being used. Enter the word COWPER to indicate that the Cowper and Symonds model is used.

2nd data block 1-5

1st

I

For option A, enter the number of slopes of yield versus strain rate curve. For option B, enter the number of data points. Not used for Cowper and Symonds model; enter 0.

6-10

Main Index

2nd

I

Material type identification (1,2,3...) for cross-reference to ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC options.

802 STRAIN RATE (Material Properties) Define Strain Rate Dependent Yield Stress

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Unit number for input of the set of this block. Defaults to blocks.

3a data block Data block 3a is used in conjunction with option A. The number of blocks in this series is equal to that given in the first field of data block 2. 1-10

1st

F

Enter the slope of the yield versus strain rate curve.

11-20

2nd

F

Enter the strain rate value above which the above slope becomes operational. Note, the first strain rate breakpoint must be zero.

3b data block Data block 3b is used in conjunction with option B. 1-10

1st

F

Enter the value of the yield strength.

11-20

2nd

F

Enter the associated strain rate. Note that the first strain rate must be zero.

3c data block Data block 3c is used in conjunction with option C.

Main Index

1-10

1st

F

Enter the value of C.

11-20

2nd

F

Enter the value of P.

FORMING LIMIT 803 Forming Limit Properties

FORMING LIMIT

Forming Limit Properties

Description This option defines the variation of forming limit properties with minor principal engineering. The curve describing the relationship between minor principal engineering strain and forming limit is also called Forming Limit Diagram (FLD). According to the forming limit values, Forming Limit Parameters (FLP) are calculated based on the in-plane principal engineering strains and the FLD data input through this FORMING LIMIT option. The FLP results can be postprocessed by specifying post code number 30. There are three formats to describe the FLD curves: 1. Fitted function definition 2. Predicted function definition 3. TABLE definition Note:

FLP is only available for shell/membrane elements.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FORMING LI.

I

Input option parameter.

2nd data block 1-5

1st

0. To input the FLD data as a fitted function (see Marc Volume A: Theory and User Information). 1. To input the FLD data by theory prediction. 2. To input the data by the TABLE option. 6-10

2nd

I

Number of FLD data points. Defaults to 9.

11-15

3rd

I

Material ID number.

16-20

4th

I

Input unit number. Defaults to standard input.

Option A 3a data block

Main Index

1-10

1st

F

C0 – First parameter of the FLD curve.

11-20

2nd

F

C1 – Second parameter of the FLD curve.

21-30

3rd

F

C2 – Third parameter of the FLD curve.

31-40

4th

F

C3 – Fourth parameter of the FLD curve.

804 FORMING LIMIT Forming Limit Properties

Format Fixed

Free

41-50

5th

Data Entry Entry F

C4 – Fifth parameter of the FLD curve.

4a data block 1-10

1st

F

D1 – Sixth parameter of the FLD curve.

11-20

2nd

F

D2 – Seventh parameter of the FLD curve.

21-30

3rd

F

D3 – Eighth parameter of the FLD curve.

31-40

4th

F

D4 – Ninth parameter of the FLD curve.

Note:

C0, C1, C2, C3, C4, D1, D2, D3, D4 are the parameters defining the function of FLD curve; refer to Marc Volume A: Theory and User Information for details.

Option B This data block is necessary when the first field of the 2nd data block equals to 1. 3b data block 1-10

1st

F

Strain-hardening exponent.

11-20

2nd

F

Thickness coefficient.

Note:

Strain-hardening exponent is the n value as defined in the power law form of strain-hardening equation σ = k ε pn . The thickness coefficient is defined by the unit used in the model. For example, if the shell thickness is defined by “Inch”, the thickness coefficient is 3.59. If the shell thickness is defined by “mm”, the thickness coefficient is 0.141. Users should choose the proper value according to the unit used in defining the shell thickness.

Option C This data block is necessary when the first field of the 2nd data block equals to 2. 3c data block

Main Index

1-5

1st

I

Enter the Table ID for the FLD data sets.

6-15

2nd

F

Reference value of forming limit diagram.

WORK HARD 805 Define Workhardening Data

WORK HARD

Define Workhardening Data

The information provided here is based upon not using the table driven input style. When using table driven input, the table associated with the yield stress should incorporate the effects of work(strain) hardening, temperature, and rate effects. Description This option allows you to specify the material stress-strain relation for elastic-plastic behavior. Further details on this option are given in Marc Volume A: Theory and User Information. The workhardening data can be entered in one of three forms. a. The breakpoints and slopes for a piecewise linear approximation to the stress-strain curves are given. The piecewise linear curve is entered in ascending order of equivalent plastic strain. b. The stress and plastic strain data points lying on the stress-strain curve are input directly. The data is entered in ascending order of plastic strains. This method is flagged by entering the word DATA on the WORK HARD option. These data points are used to calculate slope breakpoint data. c. By the WKSLP user subroutine. This routine is called for every integration point where elastic-plastic behavior occurs. See Marc Volume D: User Subroutines and Special Routines for details. Note that if this option is used, it must be used for ALL material types. This option must be repeated for each different material for which workhardening data is necessary. Note:

When performing a small deformation analysis without the LARGE DISP or LARGE STRAIN parameters, the work hard data should be given in terms of engineering stress and engineering strain. If a large displacement analysis is performed where the LARGE DISP parameter is included but without either the LARGE STRAIN or UPDATE parameter, you should use the second Piola-Kirchhoff stress and the Green Lagrange strain. If either the LARGE STRAIN parameter is included, you should enter the work hard information in terms of true stress and true strain.

Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-9

1st

A

Enter the words WORK HARD.

11-80

2nd

A

Enter the word DATA to indicate that option B is being used.

806 WORK HARD Define Workhardening Data

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

For option A, enter number of slopes of the workhardening curve. For option B, enter the number of data points. For option C, enter -1. For implicit creep, this field is for data associated with the back stress.

6-10

2nd

I

This is the same in the first field except it is for the data associated with the 10th cycle yield used in the ORNL constitutive theory. For implicit creep, this field is for data associated with the yield stress.

11-15

3rd

I

Material type identification (1,2,3 etc.) for cross-referencing with the ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC options.

16-20

4th

I

Enter unit number for input of workhardening data. Defaults to input file.

Data blocks 3a and 4a are used in conjunction with Option A. 3a data block The number of blocks entered is equal to the number of slopes entered above. Included only if the first field of 2nd data block > 0. 1-15

1st

F

Enter the slope of the workhardening curve.

16-30

2nd

F

Enter the breakpoint when the slope becomes operative. The breakpoint and slope data should be described in ascending order of the equivalent plastic strain, the first slope starting at zero plastic strain. Note:

The workhardening slope should be for a uniaxial tension specimen, and is the change in stress per unit of plastic strain, not per unit of total strain. See Marc Volume A: Theory and User Information. For implicit creep, the slope-breakpoint data in data block 3a is for the back stress versus creep strain.

4a data block Included only if the first field of 2nd data line > 0. Then, number of blocks is equal to that number. 1-15

1st

F

Slope of 10th cycle workhardening curve (stress change per plastic strain change).

16-30

2nd

F

Breakpoint when above slope becomes operative. First breakpoint should be at zero plastic strain. Note:

For implicit creep, the slope-breakpoint data in data block 4a is for the yield stress versus plastic strain.

Data blocks 3b and 4b are used in conjunction with Option B.

Main Index

WORK HARD 807 Define Workhardening Data

Format Fixed

Free

Data Entry Entry

3b data block The number of blocks entered is equal to the number of data points entered above. 1-15

1st

F

Enter the equivalent stress.

16-30

2nd

F

Enter the equivalent plastic strain. The data should be described in ascending order of equivalent plastic strain; the first data set starting at zero plastic strain. Note:

For implicit creep, the stress-strain data in data block 3b is for the back stress versus equivalent creep strain.

4b data block Included only if the first field of 2nd data line > 0. Then, number of data lines is equal to that number. 1-15

1st

Enter the equivalent stress associated with the 10th cycle work-hardening curve.

16-30

2nd

Enter the equivalent plastic strain. Note:

Main Index

For implicit creep, the stress-strain data in data block 4b is for the yield stress versus equivalent plastic strain.

808 TEMPERATURE EFFECTS (Stress) Define Effects of Temperature

TEMPERATURE EFFECTS (Stress)

Define Effects of Temperature

The information provided here is based upon not using the table driven input style. If table driven input is used, material data should include references to tables that provide temperature dependent behavior. Description This option defines the variation of material properties (Young’s modulus, yield stress, Poisson’s ratio, and coefficient of thermal expansion) with temperature. The values read in through either the ISOTROPIC or POWDER option are those at the lowest temperature specified. Properties are not defined below the lowest temperature. The temperature dependency can be entered using one of the following two options: a. The variation of a particular property with temperature is specified as a piecewise linear curve. Breakpoints must be given in ascending order of temperature. b. The particular property value and temperature lying on the relevant curve are input directly. Data points must be given in increasing order of temperature. This option is flagged by entering the word DATA on the first data line. Note:

For Mooney materials, the temperature dependence for C10 and C01 can be defined by replacing C10 for “Young’s modulus” and C01 for “Poisson’s ratio”. The other constants can be specified by utilizing the UMOONY user subroutine. For the Arruda-Boyce model, the temperature dependence of nkT and N can be defined using the “Young’s modulus” and “Poisson’s ratio” field, respectively. For the Gent model, the temperature dependence of E (tension modulus) and Im (maximum invariant) can be defined in these fields, respectively.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words TEMPERATURE EFFECTS.

21-80

2nd

A

Enter the word DATA to indicate that option B is used.

For option A, use data blocks 2a, 3a, 4a, 5a, 6a, 7a and 8a. For option B, use data blocks 2b, 3b, 4b, 5b, 6b, 7b and 8b, below.

Main Index

TEMPERATURE EFFECTS (Stress) 809 Define Effects of Temperature

Format Fixed

Free

Data Entry Entry

Option A 2a data block 1-5

1st

I

Number of slopes of yield stress versus temperature curve. For implicit creep, number of slopes of back stress versus temperature curve.

6-10

2nd

I

Number of slopes of Young’s modulus versus temperature curve.

11-15

3rd

I

Number of slopes of Poisson’s ratio versus temperature curve

16-20

4th

I

Number of slopes for instantaneous coefficient of thermal expansion versus temperature.

21-25

5th

I

Number of slopes of 10th cycle yield stress versus temperature curve of ORNL constitutive theory option, or for powder materials, number of slopes of viscosity versus temperature. For implicit creep, number of slopes of yield stress versus temperature curve.

26-30

6th

I

31-35

7th

I

Number of slopes of the workhardening versus temperature curve. Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data lines.

3a data block The number entered in the first field of data line 2 defines the number of data lines in data block 3. 1-15

1st

F

Enter the slope of yield stress versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative. Note:

For implicit creep, the slope-breakpoint data in data block 3a is for the back stress versus temperature.

4a data block The number entered in the second field of data line 2 defines the number of data lines required in data block 4. 1-15

1st

F

Enter the slope of Young’s modulus versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

5a data block The number in the third field of data line 2 defines the number of data lines required in data block 5.

Main Index

1-15

1st

F

Enter the slope of Poisson’s ratio versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

810 TEMPERATURE EFFECTS (Stress) Define Effects of Temperature

Format Fixed

Free

Data Entry Entry

6a data block The number in the fourth field of data line 2 defines the number of data lines required in data block 6. 1-15

1st

F

Enter the slope of instantaneous coefficient of thermal expansion.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative. These are instantaneous values.

7a data block Slopes/breakpoints for 10th cycle yield or viscosity versus temperature curve. The number in the fifth field of data block 2 defines the number of data lines required in data block 7. 1-15

1st

F

Slope of 10th cycle yield or viscosity versus temperature curve.

16-30

2nd

F

Temperature at which this slope becomes operative. Note:

For implicit creep, the slope-breakpoint data in data block 7a is for the yield stress versus temperature.

8a data block Slopes and breakpoints of the curve describing the ratio of the workhardening curve at temperature to the workhardening curve at the first breakpoint of this set; that is, H ( ε p, T o ) • R ( T ) is the workhardening slope at T given in terms of

H ( ε p, T o )

εp

the workhardening slope at plastic strain

breakpoint of this set, To, and R(T), the ratio parameter. In these data lines

dR ------dT

and the first

the slope of the ratio

curve, is input. The ratio R(T) is not dependent on ε p , only on T. The number in the sixth field of data block 2 defines the number of lines required in data block 8. 1-15

1st

F

Slope of ratio of workhardening slope versus temperature curve.

16-30

2nd

F

Temperature at which this slope becomes operative.

I

Number of data points on the yield stress versus temperature curve.

Option B 2b data block 1-5

1st

For implicit creep, number of data points of back stress versus temperature curve.

Main Index

6-10

2nd

I

Number of data points on the Young’s modulus versus temperature curve.

11-15

3rd

I

Number of data points on the Poisson’s ratio versus temperature curve.

16-20

4th

I

Number of data points on the instantaneous coefficient of thermal expansion versus temperature.

TEMPERATURE EFFECTS (Stress) 811 Define Effects of Temperature

Format Fixed 21-25

Free 5th

Data Entry Entry I

Number of data points on the 10th cycle yield stress versus temperature curve of ORNL constitutive theory option, or number of data points on the viscosity versus temperature curve for powder materials. For implicit creep, number of data points of yield stress versus temperature curve.

26-30

6th

I

31-35

7th

I

Number of data points on the workhardening versus temperature curve. Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data lines.

3b data block The number entered in the first field of data line 2 defines the number of data lines in data block 3. 1-15

1st

F

Enter the value of the yield stress.

16-30

2nd

F

Enter the associated temperature. Note:

For implicit creep, the value in data block 3b is for the back stress versus temperature.

4b data block The number entered in the second field of data line 2 defines the number of data lines required in data block 4. 1-15

1st

F

Enter the value of the Young’s modulus.

16-30

2nd

F

Enter the associated temperature.

5b data block The number in the third field of data line 2 defines the number of data lines required in data block 5. 1-15

1st

F

Enter the value of the Poissons’s ratio.

16-30

2nd

F

Enter the associated temperature.

6b data block The number in the fourth field of data line 2 defines the number of data lines required in data block 6. 1-15

1st

F

Enter the value of the instantaneous coefficient of thermal expansion.

16-30

2nd

F

Enter the associated temperature.

7b data block The number in the fifth field of data line 2 defines the number of data lines required in data block 7. 1-15

1st

F

Enter the value of the 10th cycle yield or viscosity.

16-30

2nd

F

Enter the associated temperature. Note:

Main Index

For implicit creep, the value in data block 7b is for the yield stress versus temperature.

812 TEMPERATURE EFFECTS (Stress) Define Effects of Temperature

Format Fixed

Free

Data Entry Entry

8b data block Data points on the curve describing the ratio of the workhardening curve at a given temperature to the workhardening curve at the first temperature of this set; that is, H ( ε p, T o ) • R ( T ) is the workhardening slope at plastic strain,

εp

, and the first temperature of this set, T, and R(T), the ratio parameter.

The same temperature effects are applied for all values of

εp

; that is, the ratio R(T) is not dependent

on ε p , only on T. The number in the sixth field of data block 2 defines the number of data lines required in data block 8. 1-15

1st

F

Enter the value of the ratio of the workhardening slope vs. the temperature curve, R(T).

16-30

2nd

F

Enter the associated temperature. Note:

Main Index

In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment. Also, a first order correction is made for the effect of temperature change on the total elastic stresses because of changes in material properties. Even in the elastic case, you should not expect a simple calculation with property values corresponding to the temperature at the end of the increment. More details are given on the discussion of temperature-dependent plasticity in Marc Volume A: Theory and User Information.

TEMPERATURE EFFECTS (Coupled Thermal-Stress) 813 Temperature Effects in Coupled Thermal-Stress Analysis

TEMPERATURE EFFECTS (Coupled Thermal- Temperature Effects in Coupled Thermal-Stress Analysis Stress) The information provided here is based upon not using the table driven input style. If table driven input is used, material data should include references to tables that provide temperature dependent behavior. Description This option defines the variation of material properties (Young’s modulus, yield stress, Poisson’s ratio, and coefficient of thermal expansion) with temperature. The values read in through either the ISOTROPIC or POWDER options are those at the lowest temperature specified. Properties are not defined below the lowest temperature. The temperature dependency can be entered using one of the following two options: a. The variation of a particular property with temperature is specified as a piecewise linear curve. Breakpoints must be given in ascending order of temperature. b. The particular property value and temperature lying on the relevant curve are input directly. Data points must be given in increasing order of temperature. This option is flagged by entering the word DATA on the first data line. Notes:

For Mooney materials, the temperature dependence for C10 and C01 can be defined by replacing C10 for “Young’s modulus” and C01 for “Poisson’s ratio”. The other constants can be specified by utilizing the UMOONY user subroutine. For the Arruda-Boyce model, the temperature dependence of nkT and N can be defined using the “Young’s modulus” and “Poisson’s ratio” field, respectively. For the Gent model, the temperature dependence of E (tension modulus) and Im (maximum invariant) can be defined in these fields, respectively. In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment. Also, a first order correction is made for the effect of temperature change on the total elastic stresses because of changes in material properties. Even in the elastic case, you should not expect a simple calculation with property values corresponding to the temperature at the end of the increment. More details are given on the discussion of temperature-dependent plasticity in Marc Volume A: Theory and User Information.

Main Index

814 TEMPERATURE EFFECTS (Coupled Thermal-Stress) Temperature Effects in Coupled Thermal-Stress Analysis

Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words TEMPERATURE EFFECTS.

21-80

2nd

A

Enter the word DATA to indicate that option B is used.

For option A, use data blocks 2a and 13a. For option B, use data blocks 2b through 13b, below. Option A 2a data block 1-5

1st

I

Number of slopes of yield stress versus temperature curve.

6-10

2nd

I

Number of slopes of Young’s modulus versus temperature curve.

11-15

3rd

I

Number of slopes of Poisson’s ratio versus temperature curve.

16-20

4th

I

Number of slopes for instantaneous coefficient of thermal expansion versus temperature.

21-25

5th

I

Number of slopes of 10th cycle yield stress versus temperature curve of ORNL constitutive theory option, or for powder materials, number of slopes of viscosity versus temperature.

26-30

6th

I

Number of slopes of the workhardening versus temperature curve.

31-35

7th

I

Number of slopes of conductivity versus temperature curve

36-40

8th

I

Number of slopes of specific heat versus temperature curve.

41-45

9th

I

Number of latent heats to be entered.

46-50

10th

I

Number of slopes of resistivity versus temperature curve.

51-55

11th

I

Number of slopes of emissivity versus temperature curve.

56-60

12th

I

Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

61-55

13th

I

Logical unit number for input of this set of data. Defaults to blocks.

3a data block The number entered in the first field of data line 2 defines the number of data lines in data block 3.

Main Index

1-15

1st

F

Enter the slope of yield stress versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

TEMPERATURE EFFECTS (Coupled Thermal-Stress) 815 Temperature Effects in Coupled Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

4a data block The number entered in the second field of data line 2 defines the number of data lines required in data block 4. 1-15

1st

F

Enter the slope of Young’s modulus versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

5a data block The number in the third field of data line 2 defines the number of data lines required in data block 5. 1-15

1st

F

Enter the slope of Poisson’s ratio versus the temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

6a data block The number in the fourth field of data line 2 defines the number of data lines required in data block 6. 1-15

1st

F

Enter the slope of instantaneous coefficient of thermal expansion.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative. These are instantaneous values.

7a data block Slopes/breakpoints for 10th cycle yield or viscosity versus temperature curve. The number in the fifth field of data line 2 defines the number of data lines required in data block 7. 1-15

1st

F

Enter the slope of 10th cycle yield stress or viscosity versus temperature curve.

16-30

2nd

F

Enter the temperature at which this slope becomes operative.

8a data block Slopes and breakpoints of the curve describing the ratio of the workhardening curve at temperature to the workhardening curve at the first breakpoint of this set; that is, H ( ε p, T o ) • R ( T ) is the workhardening slope at T given in terms of

H ( ε p, T o )

the workhardening slope at plastic strain

breakpoint of this set, To, and R(T), the ratio parameter. In these data lines

dR-----dT

εp

and the first

the slope of the ratio

curve, is input. The ratio R(T) is not dependent on ε p , only on T. The number in the sixth field of data line 2 defines the number of data lines required in data block 8.

Main Index

1-15

1st

F

Enter the slope of ratio of workhardening slope versus temperature curve.

16-30

2nd

F

Enter the temperature at which this slope becomes operative.

816 TEMPERATURE EFFECTS (Coupled Thermal-Stress) Temperature Effects in Coupled Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

9a data block Conductivity variation. Number of data lines as given on data line 2, seventh field. 1-15

1st

F

Enter the slope of conductivity versus temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

10a data block Specific heat variation. Number of data lines as given on data line 2, eighth field. 1-15

1st

F

Enter the slope of specific heat versus temperature curve.

16-30

2nd

F

Temperature above which this slope becomes operative.

11a data block Latent heat. Number of data lines given on data line 2, ninth field. 1-15

1st

F

Enter the latent heat.

16-30

2nd

F

Enter the solidus temperature (lower phase change limit).

31-45

3rd

F

Enter the liquidus temperature (upper phase change limit).

12a data block Resistivity variation. Number of data lines as given on data line 2, eleventh field. 1-15

1st

F

Enter the slope of resistivity versus temperature curve.

16-30

2nd

F

Enter the temperature at which this slope becomes operative.

13a data block Emissivity variation. Number of data lines as given on data line 2, tenth field. 1-15

1st

F

Enter the slope of emissivity versus temperature curve.

16-30

2nd

F

Enter the temperature at which this slope becomes operative.

Option B 2b data block

Main Index

1-5

1st

I

Number of data points on the yield stress versus temperature curve.

6-10

2nd

I

Number of data points on the Young’s modulus versus temperature curve.

11-15

3rd

I

Number of data points on the Poisson’s ratio versus temperature curve.

16-20

4th

I

Number of data points on the instantaneous coefficient of thermal expansion versus temperature.

21-25

5th

I

Number of data points on the 10th cycle yield stress versus temperature curve of ORNL constitutive theory option, or number of data points on the viscosity versus temperature curve for powder materials.

26-30

6th

I

Number of data points on the workhardening versus temperature curve.

31-35

7th

I

Number of data points on the conductivity versus temperature curve.

TEMPERATURE EFFECTS (Coupled Thermal-Stress) 817 Temperature Effects in Coupled Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

36-40

8th

I

Number of data points on the specific heat versus temperature curve.

41-45

9th

I

Number of latent heats to be entered.

46-50

10th

I

Number of data points on the resistivity versus temperature curve.

51-55

11th

I

Number of data points on the emissivity versus temperature curve.

56-60

12th

I

Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

61-65

13th

I

Logical unit number for input of this set of data. Defaults to data lines.

3b data block The number entered in the first field of data line 2 defines the number of data lines in data block 3. 1-15

1st

F

Enter the value of the yield stress.

16-30

2nd

F

Enter the associated temperature.

4b data block The number entered in the second field of data line 2 defines the number of data lines required in data block 4. 1-15

1st

F

Enter the value of the Young’s modulus.

16-30

2nd

F

Enter the associated temperature.

5b data block The number in the third field of data line 2 defines the number of data lines required in data block 5. 1-15

1st

F

Enter the value of the Poissons’s ratio.

16-30

2nd

F

Enter the associated temperature.

6b data block The number in the fourth field of data line 2 defines the number of data lines required in data block 6. 1-15

1st

F

Enter the value of the instantaneous coefficient of thermal expansion.

16-30

2nd

F

Enter the associated temperature.

7b data block The number in the fifth field of data line 2 defines the number of data lines required in data block 7.

Main Index

1-15

1st

F

Enter the value of the 10th cycle yield or viscosity.

16-30

2nd

F

Enter the associated temperature.

818 TEMPERATURE EFFECTS (Coupled Thermal-Stress) Temperature Effects in Coupled Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

8b data block Data points on the curve describing the ratio of the workhardening curve at a given temperature to the workhardening curve at the first temperature of this set; that is, H ( ε p, T o ) • R ( T ) is the workhardening slope at plastic strain,

εp

1-15

1st

F

Enter the value of the ratio of the workhardening slope vs. the temperature curve, R(T).

16-30

2nd

F

Enter the associated temperature.

, and the first temperature of this set, T, and R(T), the ratio parameter.

Note:

The same temperature effects are applied for all values of ε p , that is, the ratio R(T) is not dependent on ε p , only on T. The number in the sixth field of data line 2 defines the number of data lines required in data block 8.

9b data block Conductivity variation. Number of data lines as given on data line 2, seventh field. 1-15

1st

F

Enter the value of the conductivity.

16-30

2nd

F

Enter the associated temperature.

10b data block Specific heat variation. Number of data lines as given on data line 2, eighth field. 1-15

1st

F

Enter the value of the specific heat.

16-30

2nd

F

Enter the associated temperature.

11b data block Latent heat. Number of data lines as given on data line 2, ninth field. 1-15

1st

F

Enter the value of the latent heat.

16-30

2nd

F

Enter the solidus temperature (lower phase change limit).

31-45

3rd

F

Enter the liquidus temperature (upper phase change limit).

12b data block Emissivity variation. Number of data lines as given on data line 2, tenth field.

Main Index

1-15

1st

F

Enter the value of the emissivity.

16-30

2nd

F

Enter the associated temperature.

TEMPERATURE EFFECTS (Coupled Thermal-Stress) 819 Temperature Effects in Coupled Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

13b data block Resistivity variation. Number of data lines as given on data line 2, eleventh field. 1-15

1st

F

Enter the slope of resistivity heat.

16-30

2nd

F

Enter the associated temperature. Note:

Main Index

In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment. Also, a first order correction is made for the effect of temperature change on the total elastic stresses because of changes in material properties. Even in the elastic case, you should not expect a simple calculation with property values corresponding to the temperature at the end of the increment. More details are given on the discussion of temperature-dependent plasticity in Marc Volume A: User Information.

820 ORTHO TEMP (Structural) Define Temperature Effects for Orthotropic Materials

ORTHO TEMP (Structural)

Define Temperature Effects for Orthotropic Materials

The information provided here is based upon not using the table driven input style. If table driven input is used, material data should include references to tables that provide temperature dependent behavior. Description This option defines the variation of all orthotropic material properties with temperature. Note that the values read in through the ORTHOTROPIC model definition option are those at the lowest temperature defined. Properties at temperatures below this temperature are defined to be equal to properties at this temperature. The variation of a particular property is defined as a piecewise linear curve. Two options are available to define this curve. a. Slope/breakpoint data in ascending order of temperature can be given. b. Property value/temperature data in ascending order of temperature can be given. This option is flagged by entering the word DATA after the string ORTHO TEMP on data block 1. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ORTHO TEMP.

12-15

2nd

A

Enter the word DATA to indicate that Option B defined above is to be used. (There must be a space or comma between ORTHO TEMP and DATA.)

For Option A, use the 2a-22a data blocks. For Option B, use the 2b-22b data blocks. Option A 2a data block 1-5

1st

I

Number of slopes of yield vs. temperature curve.

6-10

2nd

I

Number of slopes of E11 vs temperature curve.

11-15

3rd

I

Number of slopes of E22 vs temperature curve. Enter -1 to have (E22 vs. temp.) ≡ (E11 vs. temp.).

16-20

4th

I

Number of slopes of E33 vs. temperature curve. Enter -1 to have (E33 vs. temp.) ≡ (E11 vs. temp.).

21-25

Main Index

5th

I

Number of slopes of ν12 vs. temperature curve.

ORTHO TEMP (Structural) 821 Define Temperature Effects for Orthotropic Materials

Format Fixed 26-30

Free 6th

Data Entry Entry I

Number of slopes of ν23 vs. temperature curve. Enter -1 to have (ν23 vs. temp.) ≡ (ν12 vs. temp.).

31-35

7th

I

Number of slopes of ν31 vs. temperature curve. Enter -1 to have (ν31 vs. temp.) ≡ (ν12 vs. temp.)

36-40

8th

I

Number of slopes of G12 vs. temperature curve.

41-45

9th

I

Number of slopes of G23 vs. temperature curve. Enter -1 to have (G23 vs. temp.) ≡ (G12 vs. temp.).

46-50

10th

I

Number of slopes of G31 vs. temperature curve. Enter -1 to have (G31 vs. temp.) ≡ (G12 vs. temp.).

51-55

11th

I

Number of slopes of α11 vs. temperature curve.

56-60

12th

I

Number of slopes of α22 vs. temperature curve. Enter -1 to have (α22 vs. temp.) ≡ (α11 vs. temp.).

61-65

13th

I

Number of slopes of α33 vs. temperature curve. Enter -1 to have (α33 vs. temp.) ≡ (α11 vs. temp.).

66-70

14th

I

Number of slopes of the workhardening vs. temperature curve.

71-75

15th

I

Enter the material identification for this data set.

76-80

16th

I

Enter the unit number for input of this data. Defaults to input file.

3a data block Include this data block only in a coupled thermal-stress analysis. 1-5

1st

I

Number of slopes of K11 vs. temperature curve.

6-10

2nd

I

Number of slopes of K22 vs. temperature curve. Enter -1 to have (K22 vs. temp.) ≡ (K11 vs. temp.).

11-15

3rd

I

Number of slopes of K33 vs. temperature curve. Enter -1 to have (K33 vs. temp.) ≡ (K11 vs. temp.).

Main Index

16-20

4th

I

Number of slopes of specific heat vs. temperature curve.

21-25

5th

I

Number of latent heats.

26-30

6th

I

Number of slopes of resistivity 11 versus temperature.

31-35

7th

I

Number of slopes of resistivity 22 versus temperature.

36-40

8th

I

Number of slopes of resistivity 33 versus temperature.

41-45

9th

I

Number of slopes of emissivity versus temperature.

822 ORTHO TEMP (Structural) Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

4a data block The number of data lines in this block is the number in data block 2a, first field. 1-15

1st

F

Enter the slope of yield vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

5a data block The number of data lines in this block is the number in data block 2a, second field. 1-15

1st

F

Enter the slope of E11 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

6a data block The number of data lines in this block is n, the number in data block 2a, third field, or 0 if n = -1. 1-15

1st

F

Enter the slope of E22 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

7a data block The number of data lines in this block is n, the number in data block 2a, fourth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of E33 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

8a data block The number of data lines in this block is the number in data block 2a, fifth field. 1-15

1st

F

Enter the slope of ν12 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

9a data block The number of data lines in this block is n, the number in data block 2a, sixth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of ν23 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

10a data block The number of data lines in this block is n, the number in data block 2a, seventh field, or 0 if n = -1. 1-15

1st

F

Enter the slope of ν31 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

11a data block The number of data lines in this block is the number in data block 2a, eighth field. 1-15

Main Index

1st

F

Enter the slope of G12 vs. temperature curve.

ORTHO TEMP (Structural) 823 Define Temperature Effects for Orthotropic Materials

Format Fixed 16-30

Free 2nd

Data Entry Entry F

Temperature at which above slope becomes operative.

12a data block The number of data lines in this block is n, the number in data block 2a, ninth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of G23 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

13a data block The number of data lines in this block is n, the number in data block 2a, tenth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of G31 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

14a data block The number of data lines in this block is the number in data block 2a, eleventh field. 1-15

1st

F

Enter the slope of α11 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

15a data block The number of data lines in this block is n, the number in data block 2a, twelfth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of α22 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

16a data block The number of data lines in this block is n, the number in data block 2a, thirteenth field, or 0 if n=-1. 1-15

1st

F

Enter the slope of α33 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

17a data block The number of data lines in this block is the number in data block 2a, fourteenth field. 1-15

1st

F

Enter the slope of the ratio of work hardening slope vs. temperature.

16-30

2nd

F

Temperature at which above slope becomes operative. Note:

To define the dependence of 10th cycle yield on temperature, use the YIEL user subroutine.

The following data blocks are used only in a coupled thermal-stress analysis.

Main Index

824 ORTHO TEMP (Structural) Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

18a data block The number of data lines in this block is the number in the first field of the 3a data block. 1-15

1st

F

Enter the slope of K11 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

19a data block The number of data lines in this block is n, the number in the second field of the 3a data block, or 0 if n = -1. 1-15

1st

F

Enter the slope of K22 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

20a data block The number of data lines in this block is n, the number in the third field of the 3a data block, or 0 if n = -1. 1-15

1st

F

Enter the slope of K33 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

21a data block The number of data lines in this block is the number in the fourth field of the 3a data block. 1-15

1st

F

Enter the slope of specific heat vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

22a data block The number of data lines in this block is the number in the fifth field of the 3a data block. 1-15

1st

F

Enter latent heat value.

16-30

2nd

F

Solidus temperature (lower phase change limit).

31-45

3rd

F

Liquidus temperature (upper phase change limit).

23a data block The number of data lines in this block is the number in the sixth field of the 3a data block. 1-15

1st

F

Enter the slope of

16-30

2nd

F

Temperature at which above slope becomes operative.

R 11

versus temperature curve.

24a data block The number of data lines in this block is n, the number in the seventh field of the 3a data block or 0 if n = -1.

Main Index

1-15

1st

F

Enter the slope of

16-30

2nd

F

Temperature at which above slope becomes operative.

R 22

versus temperature curve.

ORTHO TEMP (Structural) 825 Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

25a data block The number of data lines in this block is n, the number in the seventh field of the 3a data block or 0 if n = -1. 1-15

1st

F

Enter the slope of

16-30

2nd

F

Temperature at which above slope becomes operative.

R 33

versus temperature curve.

26a data block The number of data lines in this block is the number in the ninth field of the 3a data block. 1-15

1st

F

Enter the value of emissivity.

16-30

2nd

F

Enter the associated temperature.

Option B 2b data block 1-5

1st

I

Number of data points of yield.

6-10

2nd

I

Number of data points of E11 vs. temperature curve.

11-15

3rd

I

Number of data points of E22 vs. temperature curve. Enter -1 to have (E22 vs. temp.) ≡ (E11 vs. temp.).

16-20

4th

I

Number of data points of E33. Enter -1 to have (E33 vs. temp.) ≡ (E11 vs. temp.).

21-25

5th

I

Number of data points of ν12.

26-30

6th

I

Number of data points of ν23. Enter -1 to have (ν23 vs. temp.) ≡ (ν12 vs. temp.).

31-35

7th

I

Number of data points of ν31. Enter -1 to have (ν31 vs. temp.) ≡ (ν12 vs. temp.).

36-40

8th

I

Number of data points of G12.

41-45

9th

I

Number of data points of G23. Enter -1 to have (G23 vs. temp.) ≡ (G12 vs. temp.).

46-50

10th

I

Number of data points of G31. Enter -1 to have (G23 vs. temp.) ≡ (G12 vs. temp.).

51-55

1th1

I

Number of data points of α11.

56-60

12th

I

Number of data points of α22. Enter -1 to have (α22 vs. temp.) ≡ (α11 vs. temp.).

Main Index

826 ORTHO TEMP (Structural) Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

61-65

13th

Data Entry Entry I

Number of data points of α33. Enter -1 to have (α33 vs. temp.) ≡ (α11 vs. temp.).

66-70

14th

I

Number of data points of the workhardening vs. temperature curve.

71-75

15th

I

Enter the material identification for this data set.

76-80

16th

I

Enter the unit number for input of this data. Defaults to input file.

3b data block Include this data block only in a coupled thermal-stress analysis. 1-5

1st

I

Number of data points of K11

6-10

2nd

I

Number of data points of K22. Enter -1 to have (K22 vs. temp.) ≡ (K11 vs. temperature).

11-15

3rd

I

Number of data points of K33. Enter -1 to have (K33 vs. temp.) ≡ (K11 vs. temperature).

16-20

4th

I

Number of data points of specific heat

21-25

5th

I

Number of latent heats.

4b data block The number of data lines in this block is the number in data block 2b, first field. 1-15

1st

F

Enter the value of yield stress.

16-30

2nd

F

Enter the associated temperature.

5b data block The number of data lines in this block is the number in data block 2b, second field. 1-15

1st

F

Enter the value of E11.

16-30

2nd

F

Enter the associated temperature.

6b data block The number of data lines in this block is n, the number in data block 2b, third field, or 0 if n = -1. 1-15

1st

F

Enter the value of E22.

16-30

2nd

F

Enter the associated temperature.

7b data block The number of data lines in this block is n, the number in data block 2b, fourth field, or 0 if n = -1.

Main Index

1-15

1st

F

Enter the value of E33.

16-30

2nd

F

Enter the associated temperature.

ORTHO TEMP (Structural) 827 Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

8b data block The number of data lines in this block is the number in data block 2b, fifth field. 1-15

1st

F

Enter the value of ν12.

16-30

2nd

F

Enter the associated temperature.

9b data block The number of data lines in this block is n, the number in data block 2b, sixth field, or 0 if n = -1. 1-15

1st

F

Enter the value of ν23.

16-30

2nd

F

Enter the associated temperature.

10b data block The number of data lines in this block is n, the number in data block 2b, seventh field, or 0 if n = -1. 1-15

1st

F

Enter the value of ν31.

16-30

2nd

F

Enter the associated temperature.

11b data block The number of data lines in this block is the number in data block 2b, eighth field. 1-15

1st

F

Enter the value of G12.

16-30

2nd

F

Enter the associated temperature.

12b data block The number of data lines in this block is n, the number in data block 2b, ninth field, or 0 if n = -1. 1-15

1st

F

Enter the value of G23.

16-30

2nd

F

Enter the associated temperature.

13b data block The number of data lines in this block is n, the number in data block 2b, tenth field, or 0 if n = -1. 1-15

1st

F

Enter the value of G31.

16-30

2nd

F

Enter the associated temperature.

14b data block The number of data lines in this block is the number in data block 2b, eleventh field.

Main Index

1-15

1st

F

Enter the value of α11.

16-30

2nd

F

Enter the associated temperature.

828 ORTHO TEMP (Structural) Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

15b data block The number of data lines in this block is n, the number in data block 2b, twelfth field, or 0 if n = -1. 1-15

1st

F

Enter the value of α22.

16-30

2nd

F

Enter the associated temperature.

16b data block The number of data lines in this block is n, the number in data block 2b, thirteenth field, or 0 if n = -1. 1-15

1st

F

Enter the value of α33.

16-30

2nd

F

Enter the associated temperature.

17b data block The number of data lines in this block is the number in data block 2b, fourteenth field. 1-15

1st

F

Enter the value of work hardening slope.

16-30

2nd

F

Enter the associated temperature. Note:

To define the dependence of 10th cycle yield on temperature, use the YIEL user subroutine.

The following five data blocks are used only in a coupled thermal-stress analysis. 18b data block The number of data lines in this block is the number in data block 3b, first field. 1-15

1st

F

Enter the value of K11.

16-30

2nd

F

Enter the associated temperature.

19b data block The number of data lines in this block is n, the number in data block 3b, second field, or 0 if n = -1. 1-15

1st

F

Enter the value of K22.

16-30

2nd

F

Enter the associated temperature.

20b data block The number of data lines in this block is n, the number in data block 3b, third field, or 0 if n = -1. 1-15

1st

F

Enter the value of K33.

16-30

2nd

F

Enter the associated temperature.

21b data block The number of data lines in this block is the number in data block 3b, fourth field.

Main Index

1-15

1st

F

Enter the value of specific heat.

16-30

2nd

F

Enter the associated temperature.

ORTHO TEMP (Structural) 829 Define Temperature Effects for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

22b data block The number of data lines in this block is the number in data block 3b, fifth field. 1-15

1st

F

Enter latent heat value.

16-30

2nd

F

Solidus temperature (lower phase change limit).

31-45

3rd

F

Liquidus temperature (upper phase change limit).

23b data block The number of data lines in this block is the number in the sixth field of the 3b data block. 1-15

1st

F

Enter the slope of

16-30

2nd

F

Enter the associated temperature.

R 11

versus temperature curve.

24b data block The number of data lines in this block is n, the number in the seventh field of the 3b data block or 0 if n = -1. 1-15

1st

F

Enter the slope of

16-30

2nd

F

Enter the associated temperature.

R 22

versus temperature curve.

25b data block The number of data lines in this block is n, the number in the seventh field of the 3b data block or 0 if n = -1. 1-15

1st

F

Enter the slope of

16-30

2nd

F

Enter the associated temperature.

R 33

versus temperature curve.

26b data block The number of data lines in this block is the number in the ninth field of the 3b data block

Main Index

1-15

1st

F

Enter the value of emissivity.

16-30

2nd

F

Enter the associated temperature.

830 TIME-TEMP Define Effects of Time/Temperature Transformation

TIME-TEMP

Define Effects of Time/Temperature Transformation

Description This option provides you with the option of defining either mechanical or thermal (heat transfer) properties as a function of both temperature and the rate at which the temperature changes. It can also be used to describe the effects of phase transformations on these properties. You are reminded to include the T-T-T parameter when invoking this option. If the material properties are strictly dependent on temperature and not time as well, the TEMPERATURE EFFECTS option should be used instead. In performing a thermal-stress analysis, the mechanical properties, which can be defined as a function of time-temperature-transformation (T-T-T), are the Young’s modulus, Poisson’s ratio, yield stress, work or strain hardening rate, and thermal coefficient of expansion. The effects of volumetric change due to phase transformation can be included through the definition of the thermal coefficient of expansion. In performing a transient heat transfer analysis, the thermal properties, which can be defined as a function of T-T-T, are the thermal conductivity and the specific heat per unit reference mass. Here, the effects of heat or phase transformation can be included through the definition of the specific heat. You are expected to have the test data for each property of each material group in a tabular form. For a given cooling rate, the value of a property must be known at discrete points over a range of temperature. There can be several sets of this data corresponding to measurements at several different cooling rates. The cooling tests must be of a specific type known as “Newton Cooling”; for example, the temperature change in the material is controlled such that T(t) = A exp(-at) + B Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words TIME-TEMP.

I

Enter the total number of different material groups with time-temperaturetransformation dependent properties.

2nd data block 1-5

1st

3rd data block This data block is used to specify the minimum and maximum temperatures bracketing the range over which the property values given below are meant to apply. 1-10

1st

F

Enter the value of the minimum temperature.

11-20

2nd

F

Enter the value of the maximum temperature.

Data blocks 4 through 8 are repeated for each material group.

Main Index

TIME-TEMP 831 Define Effects of Time/Temperature Transformation

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Enter the material group number whose properties are defined in the following data block.

6-10

2nd

I

Enter the element number corresponding to the first element in a consecutive list of elements for this material group.

11-15

3rd

I

Enter the element number corresponding to the last elements in a consecutive list of elements for this material group.

5th data block a) Stress Analysis 1-5

1st

I

Enter the number of cooling rates used to define the Young’s modulus for this material group. If this number is preceded by a minus sign, all properties for this material group are assigned the same number of cooling rates. In this case, the remaining fields on this block need not be specified.

6-10

2nd

I

Enter the number of cooling rates used to define the Poisson’s ratio for this material group.

11-15

3rd

I

Enter the number of cooling rates used to define the yield point for this material group.

16-20

4th

I

Enter the number of cooling rates used to define the work hardening rate for this material group.

21-25

5th

I

Enter the number of cooling rates used to define the coefficient of thermal expansion for this material group.

b) Heat Transfer (Thermal) Analysis

Main Index

1-5

1st

I

Enter the number of cooling rates used to define the thermal conductivity for this material group.

6-10

2nd

I

Enter the number of cooling rates used to define the specific heat per unit reference mass for this material group.

832 TIME-TEMP Define Effects of Time/Temperature Transformation

Format Fixed

Free

Data Entry Entry

6th data block The coefficients associated with the definition of each cooling rate are specified in this data block. The cooling rates are described by the formula T(t) = Aij exp(-aij t) + Bij where i refers to a particular cooling rate and j refers to a particular property This data block is comprised of sets of blocks. There can be as many as five sets for a thermal-stress analysis and a maximum of two sets for a heat transfer analysis corresponding to the maximum number of properties which can be a function of time-temperature-transformation in each case. The number of blocks in each set corresponds to the five (stress analysis) or two (heat transfer analysis) entries given in the fifth data block. The order of the block sets is the same as for the entries on data block 5. On each block, specify the coefficients for a particular rate. The order within each set must be from the fastest to the slowest rate. 1-10

1st

F

Enter the value of the coefficient “A” in the above equation.

11-20

2nd

F

Enter the value of the coefficient “a” in the above equation.

21-30

3rd

F

Enter the value of the constant “B” in the above equation.

31-50

4th

I

If the number of cooling rates associated with each property is the same and magnitude (that is, coefficients) of these rates is also the same, enter a positive integer in this field on the first block (only) in this series. It is then necessary to specify the coefficients of each cooling rate for only a single property of the material group being used.

I

Specify the number of temperature points at which a property value is specified for each cooling rate associated with a given property. If more than sixteen cooling rates are being used, use additional blocks. The order is from the fastest to the slowest cooling rate. Beginning on a new block repeat this block set for each property. The order in which properties are considered corresponds to the order specified in data block 5. (16I5)

7th data block 1-80

1st

If the number of temperature points is the same for all cooling rates of all properties, enter this value in the first field preceded by a minus sign.

Main Index

TIME-TEMP 833 Define Effects of Time/Temperature Transformation

Format Fixed

Free

Data Entry Entry

8th data block The actual property values are defined in this data block. This series should be considered as a data block. There are as many sub-blocks in it as there are properties with time-temperature-transformation dependent effects for this material group. The order in which the property subblocks should be specified is given in data blocks 5(a) or 5(b). Each property sub-block can be considered as consisting of a series of block sets. The number of block sets per sub-block corresponds to the number of cooling rates for the particular property in question. These block sets are specified in the order of fastest to slowest cooling rate. Each block set of a sub-block, corresponding to a given cooling rate for a given property, contains as many blocks as there are temperature levels where a discrete value of the property is defined. The property values must be defined in the order of increasing temperature levels.

Main Index

1-10

1st

F

Enter the value of the material property for a particular cooling rate and temperature level.

11-20

2nd

F

Enter the temperature level corresponding to the property value defined above.

834 SHAPE MEMORY (with TABLE Input) Define the Properties of Shape Memory Model

SHAPE MEMORY (with TABLE Input)

Define the Properties of Shape Memory Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define material properties used in conjunction with shape memory material model. Two models are provided, a thermo-mechanical and a simplified mechanical (Auricchio) model. Details of these models are provided in Marc Volume A: Theory and User Information, Chapter 7. Notes:

The simplified mechanical model only supports ndi = 3 cases (3-D, plane-strain, and axisymmetric elements). It does not support ndi = 1 and ndi = 2 (1-D and plane-stress elements). In the current release, the table IDs are not used.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SHAPE MEMORY.

2nd data block 1-5

1st

I

Enter the number of sets Shape Memory material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 10 (thermo-mechanical model) or data blocks 3 to 6 (mechanical model) are repeated as a set; once for each set of shape memory material defined. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing TEMPERATURE EFFECTS and WORK HARD data.

6-10

2nd

I

Shape memory alloy model type: 0 or 1 Thermo-mechanical shape memory model. 2 Mechanical shape memory (Auricchio) model.

Main Index

11-15

3rd

I

Not used.

16-20

4th

I

Not used.

21-32

5th

A

Enter the material name.

SHAPE MEMORY (with TABLE Input) 835 Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

Data blocks 4a, 5a, 6a, 7a, 8a, 9a, and 10a are associated with the thermo-mechanical model. 4a data block Austenite Properties 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Coefficient of thermal expansion.

31-40

4th

F

Equivalent (von Mises) tensile yield stress.

41-50

5th

F

Mass density.

4aa data block Austenite Properties 1-5

1st

I

Table ID for Young’s modulus.

6-10

2nd

I

Table ID for Poisson’s ratio.

11-15

3rd

I

Table ID for coefficient of thermal expansion.

16-20

4th

I

Table ID for equivalent (von Mises) tensile yield stress.

5a data block Martensite Properties 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Coefficient of thermal expansion.

31-40

4th

F

Equivalent (von Mises) tensile yield stress.

5aa data block Martensite Properties 1-5

1st

I

Table ID for Young’s modulus.

6-10

2nd

I

Table ID for Poisson’s ratio.

11-15

3rd

I

Table ID for coefficient of thermal expansion.

16-20

4th

I

Table ID for equivalent (von Mises) tensile yield stress.

6a data block Kinetics of Phase Transformation

Main Index

σ eq M s = M s0 + -------Cm

σ eq M f = M f0 + -------Cm

σ eq A s = A s0 + -------Ca

σ eq A f = A f0 + -------Ca

836 SHAPE MEMORY (with TABLE Input) Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

1-10

1st

F

Martensite start temperature in the stress-free condition ( M s0 ).

11-20

2nd

F

Martensite finish temperature in the stress-free condition ( M f0 ).

21-30

3rd

F

Slope of the stress-dependence of martensite start finish and start temperatures ( C m ).

31-40

4th

F

Austenite start temperature in the stress-free condition ( A s0 ).

41-50

5th

F

Austenite finish temperature in the stress-free condition ( A f0 ).

51-60

6th

F

Slope of the stress-dependence of austenite start finish and start temperatures ( C a ).

6aa data block Kinetics of Phase Transformation 1-5

1st

I

Table ID for martensite start temperature in the stress-free condition ( M s0 ).

6-10

2nd

I

Table ID for martensite finish temperature in the stress-free condition ( M f0 ).

11-15

3rd

I

Table ID for slope of the stress-dependence of martensite start finish and start temperatures ( C m ).

16-20

4th

I

Table ID for austenite start temperature in the stress-free condition ( A s0 ).

21-25

5th

I

Table ID for austenite finish temperature in the stress-free condition ( A f0 ).

26-30

6th

I

Table ID for slope of the stress-dependence of austenite start finish and start temperatures ( C a ).

7a data block Transformation Strains 1-10

1st

F

T ). Equivalent deviatoric transformation strain ( ε eq

11-20

2nd

F

Volumetric part of the transformation strain ( ε vT ).

21-30

3rd

F

Twinning stress ( σ efg f ). Twinning becomes operational when the equivalent stress reaches the twinning stress.

Main Index

SHAPE MEMORY (with TABLE Input) 837 Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

7aa data block Transformation Strains 1-5

1st

I

T ). Table ID for equivalent deviatoric transformation strain ( ε eq

6-10

2nd

I

Table ID for volumetric part of the transformation strain ( ε vT ).

11-15

3rd

I

Table ID for twinning stress ( σ efg f ). Twinning becomes operational when the equivalent stress reaches the twinning stress.

8a data block Coefficient of function

g

σ eq σ eq g ⎛ --------⎞ = 1 – exp g a ⎛ --------⎞ ⎝ g0 ⎠ ⎝ g0 ⎠

gb

σ eq + g c ⎛ --------⎞ ⎝ g0 ⎠

gd

σ eq + g e ⎛ --------⎞ ⎝ g0 ⎠

1-10

1st

F

Coefficient

11-20

2nd

F

Exponent

21-30

3rd

F

Coefficient

31-40

4th

F

Exponent

41-50

5th

F

Coefficient

51-60

6th

F

Exponent

gf

ga .

gb . gc .

gd . ge .

gf .

8aa data block Coefficient of function

Main Index

g

1-5

1st

I

Table ID for coefficient

6-10

2nd

I

Table ID for exponent

11-15

3rd

I

Table ID for coefficient

16-20

4th

I

Table ID for exponent

11-25

5th

I

Table ID for coefficient

26-30

6th

I

Table ID for exponent

ga .

gb . gc .

gd . ge .

gf .

838 SHAPE MEMORY (with TABLE Input) Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

9a data block Coefficient of function

g

(continued)

1-10

1st

F

Stress level ( g 0 ) used to nondimensionalizing the stress in the function.

11-20

2nd

F

Maximum value of function g , ( g ma x ), if a cut off value is needed.

21-30

3rd

F

Stress at which the maximum value of g = off value is needed (normalized with g 0 ).

31-40

4th

F

Initial martensite volume fraction (0 - 1). Default value = 0.0

g max

g is reached ( σ max ) if a cut

9aa data block Coefficient of function

g

(continued)

1-5

1st

I

Table ID for stress level ( g 0 ) used to nondimensionalizing the stress in the function.

6-10

2nd

I

Table ID for maximum value of function g , ( g max ), if a cut off value is needed.

11-15

3rd

I

Table ID for stress at which the maximum value of g ( σ max ) if a cut off value is needed (normalized with

16-20

4th

I

is reached

g 0 ).

Table ID for initial martensite volume fraction (0 - 1). Default value = 0.0

Data blocks 4b and 5b are associated with Auricchio’s model. 4b data block 1-10

1st

F

Young’s modulus (Austenite phase)

11-20

2nd

F

Poisson’s ratio (Austenite phase)

21-30

3rd

F

σ sAS

31-40

4th

F

σ fAS

41-50

5th

F

σ sS A

51-60

6th

F

σ fS A

61-70

7th

F

Mass density

4bb data block

Main Index

g = g max

1-5

1st

I

Table ID for Young’s modulus (Austenite phase)

6-10

2nd

I

Table ID for Poisson’s ratio (Austenite phase)

11-15

3rd

I

Table ID for

σ sAS

16-20

4th

I

Table ID for

σ fAS

SHAPE MEMORY (with TABLE Input) 839 Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Table ID for

σ sSA

26-30

6th

I

Table ID for

σ fSA

5b data block 1-10

1st

F

εL

11-20

2nd

F

α

21-30

3rd

F

Reference temperature used to measure stresses ( T o ).

31-40

4th

F

Slope of the stress-dependence for martensite ( C m ).

41-50

5th

F

Slope of the stress-dependence for austenite ( C a ).

51-60

6th

F

Young’s modulus of Martensite phase; if 0, defaults to Austenite phase.

61-70

7th

F

Poisson’s ratio of Martensite phase; if 0, defaults to Austenite phase.

5bb data block

Main Index

1-5

1st

I

Table ID for

εL

6-10

2nd

I

Table ID for

α

11-15

3rd

I

Table ID for reference temperature used to measure stresses ( T o ).

16-20

4th

I

Table ID for slope of the stress-dependence for martensite ( C m ).

11-25

5th

I

Table ID for slope of the stress-dependence for austenite ( C a ).

26-30

6th

I

Table ID for Young’s modulus of Martensite phase.

31-35

7th

I

Table ID for Poisson’s ratio of Matensite phase.

840 SHAPE MEMORY Define the Properties of Shape Memory Model

SHAPE MEMORY

Define the Properties of Shape Memory Model

The information provided here is based upon not using the table driven input style. Description This option allows you to define material properties used in conjunction with shape memory material model. Two models are provided, a thermo-mechanical and a simplified mechanical (Auricchio) model. Details of these models are provided in Marc Volume A: Theory and User Information, Chapter 7. Note:

The simplified mechanical model only supports ndi = 3 cases (3-D, plane-strain, and axisymmetric elements). It does not support ndi = 1 and ndi = 2 (1-D and plane-stress elements).

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SHAPE MEMORY.

2nd data block 1-5

1st

I

Enter the number of sets Shape Memory material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 10 (thermo-mechanical model) or data blocks 3 to 6 (mechanical model) are repeated as a set; once for each set of shape memory material defined. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing TEMPERATURE EFFECTS and WORK HARD data.

6-10

2nd

I

Shape memory alloy model type: 0 or 1 Thermo-mechanical shape memory model. 2 Mechanical shape memory (Auricchio) model.

11-15

3rd

I

Not used

16-20

4th

I

Not used

21-32

5th

A

Enter the material name.

Data blocks 4a through 10a are associated with the thermo-mechanical model.

Main Index

SHAPE MEMORY 841 Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

4a data block Austenite Properties 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Coefficient of thermal expansion.

31-40

4th

F

Equivalent (von Mises) tensile yield stress.

41-50

5th

F

Mass density

5a data block Martensite Properties 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Coefficient of thermal expansion.

31-40

4th

F

Equivalent (von Mises) tensile yield stress.

6a data block Kinetics of Phase Transformation σ eq M s = M s0 + -------Cm σ eq A s = A s0 + -------Ca

σ eq M f = M f0 + -------Cm σ eq A f = A f0 + -------Ca

1-10

1st

F

Martensite start temperature in the stress-free condition ( M s0 ).

11-20

2nd

F

Martensite finish temperature in the stress-free condition ( M f0 ).

21-30

3rd

F

Slope of the stress-dependence of martensite start finish and start temperatures ( C m ).

31-40

4th

F

Austenite start temperature in the stress-free condition ( A s0 ).

41-50

5th

F

Austenite finish temperature in the stress-free condition ( A f0 ).

51-60

6th

F

Slope of the stress-dependence of austenite start finish and start temperatures ( C a ).

7a data block Transformation Strains

Main Index

1-10

1st

F

T ). Equivalent deviatoric transformation strain ( ε eq

11-20

2nd

F

Volumetric part of the transformation strain ( ε vT ).

842 SHAPE MEMORY Define the Properties of Shape Memory Model

Format Fixed 21-30

Free 3rd

Data Entry Entry F

Twinning stress ( σ efg f ). Twinning becomes operational when the equivalent stress reaches the twinning stress.

8a data block Coefficient of function

g

σ eq σ eq g b σ eq g d σ eq g f g ⎛ --------⎞ = 1 – exp g a ⎛ --------⎞ + g c ⎛ --------⎞ + g e ⎛ --------⎞ ⎝ g0 ⎠ ⎝ g0 ⎠ ⎝ g0 ⎠ ⎝ g0 ⎠

1-10

1st

F

Coefficient

11-20

2nd

F

Exponent

21-30

3rd

F

Coefficient

31-40

4th

F

Exponent

41-50

5th

F

Coefficient

51-60

6th

F

Exponent

ga .

gb . gc .

gd . ge .

gf .

9a data block Coefficient of function

g

(continued)

1-10

1st

F

Stress level ( g 0 ) used to nondimensionalizing the stress in the function.

11-20

2nd

F

Maximum value of function g , ( g ma x ), if a cut off value is needed.

21-30

3rd

F

Stress at which the maximum value of g = off value is needed (normalized with g 0 ).

31-40

4th

F

Initial martensite volume fraction (0 - 1). Default value = 0.0

g max

g is reached ( σ max ) if a cut

10a data block Enter a list of elements associated with this material. Data blocks 4b through 6b are associated with Auricchio’s model. 4b data block

Main Index

1-10

1st

F

Young’s modulus of Austenite phase

11-20

2nd

F

Poisson’s ratio of Austenite phase

21-30

3rd

F

σ sAS

31-40

4th

F

σ fAS

41-50

5th

F

σ sS A

SHAPE MEMORY 843 Define the Properties of Shape Memory Model

Format Fixed

Free

Data Entry Entry

51-60

6th

F

σ fSA

61-70

7th

F

Mass Density

5b data block 1-10

1st

F

εL

maximum strain obtained by detwinning. Default = 0.07.

11-20

2nd

F

α

coefficient of thermal expansion.

21-30

3rd

F

Reference temperature used to measure stresses ( T o ).

31-40

4th

F

Slope of the stress-dependence for martensite ( C m ).

41-50

5th

F

Slope of the stress-dependence for austenite ( C a ).

51-60

6th

F

Young’s modulus of Martensite phase; if 0, defaults to Austenite phase.

61-70

7th

F

Poisson’s ratio of Martensite phase; if 0, defaults to Austenite phase.

6b data block Enter a list of elements associated with this material.

Main Index

844 CRACK DATA (with TABLE Input) Define Material Properties for Concrete Cracking

CRACK DATA (with TABLE Input)

Define Material Properties for Concrete Cracking

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option inputs the uniaxial cracking data for a low tension (concrete) material. The standard material properties, like Young’s modulus, Poisson’s ratio etc., are given in the ISOTROPIC option. Cross reference is given by the material identification number. Cracking data can alternatively be specified by the UCRACK, TENSOF, and USHRET user subroutines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CRACK DATA.

2nd data block 1-5

1st

I

Enter the number of distinct sets of cracking material properties to be input (optional).

6-10

2nd

I

Enter the unit number for input of cracking data. Default to input.

The 3rd and 4th data blocks are repeated once for each distinct data set. 3rd data block

Main Index

1-5

1st

I

Material type identification (1, 2, 3, ...) for cross-referencing the ISOTROPIC option.

6-15

2nd

F

Critical cracking stress.

16-25

3rd

F

Modulus for tension softening material. (If no value is entered, stress goes to zero upon cracking.)

26-35

4th

F

Strain at which crushing of the material occurs. If this value is not given, it is automatically set to some large value.

36-45

5th

F

Shear retention factor.

CRACK DATA (with TABLE Input) 845 Define Material Properties for Concrete Cracking

Format Fixed

Free

Data Entry Entry

4th data block

Main Index

1-5

1st

I

Not used; enter zero.

6-10

2nd

I

Table ID associated with critical cracking stress.

11-15

3rd

I

Table ID associated with tension softening modulus.

16-20

4th

I

Table ID associated with crushing strain.

21-25

5th

I

Table ID associated with shear retention factor.

846 CRACK DATA Define Material Properties for Concrete Cracking

CRACK DATA

Define Material Properties for Concrete Cracking

The information provided here is based upon not using the table driven input style. Description This option inputs the uniaxial cracking data for a low tension (concrete) material. The standard material properties, like Young’s modulus, Poisson’s ratio etc., are given in the ISOTROPIC option. Cross reference is given by the material identification number. Cracking data can alternatively be specified by the UCRACK, TENSOF, and USHRET user subroutines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CRACK DATA.

2nd data block 1-5

1st

I

Enter the number of distinct sets of element properties to be input (optional).

6-10

2nd

I

Enter the unit number for input of cracking data. Default to input.

The 3rd data block is repeated once for each distinct data set. 3rd data block

Main Index

1-5

1st

I

Material type identification (1, 2, 3, ...) for cross-referencing the ISOTROPIC option.

6-15

2nd

F

Critical cracking stress.

16-25

3rd

F

Modulus for tension softening material. (If no value is entered, stress goes to zero upon cracking.)

26-35

4th

F

Strain at which crushing of the material occurs. If this value is not given, it is automatically set to some large value.

36-45

5th

F

Shear retention factor.

FAIL DATA (with TABLE Input) 847 Define Failure Criteria Data

FAIL DATA (with TABLE Input)

Define Failure Criteria Data

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option is used to define material dependent failure criteria data. Up to three failure criteria per material can be specified. Failure indices are calculated and printed for every integration point at which material dependent failure data exists. This option can also be used to invoke the progressive failure of a material. The supported failure criteria types are: MX STRESS MX STRAIN TSAI-WU HOFFMAN HILL HASHIN HASHIN-TAPE HASHIN-FABRIC PUCK UFAIL Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FAIL DATA.

2nd data block 1-5

1st

I

Enter the number of materials with Marc calculated failure criteria. If blank, Marc reads until no more failure criteria data are left.

6-10

2nd

I

Enter the unit number for reading. Defaults to input.

Data blocks 3 through 7 are repeated as a set, once for each material with Marc calculated failure criteria, as described above.

Main Index

848 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Number of sets of failure criteria data for this material. No more than three sets are allowed.

11-15

3rd

I

Flag to invoke the progressive failure option. Enter 0 for no progressive failure analysis. Enter 1 for the standard Marc method. Enter 2 for gradual selective stiffness degradation. Enter 3 for immediate selective stiffness degradation.

Data blocks 4 through 7 are entered for each set of failure criteria data. Data blocks 6 and 7 are not required unless progressive failure option 2 or 3 is used. For MX Stress: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

Enter the words MX STRESS. X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress in z-direction.

4b data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum tensile stress in x-direction.

11-15

3rd

I

Table ID for maximum compressive stress in x-direction.

16-20

4th

I

Table ID for maximum tensile stress in y-direction.

21-25

5th

I

Table ID for maximum compressive stress in y-direction.

26-30

6th

I

Table ID for maximum tensile stress in z-direction.

31-35

7th

I

Table ID for maximum compressive stress in z-direction.

FAIL DATA (with TABLE Input) 849 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

Sxy – Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz – Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx – Maximum absolute value of shear stress in zx-plane. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

5b data block 1-5

1st

I

Table ID for maximum shear stress in xy-plane.

6-10

2nd

I

Table ID for maximum shear stress in yz-plane.

11-15

3rd

I

Table ID for maximum shear stress in zx-plane.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

1st

I

Set to 1 is failure in positive x-direction is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if failure in negative x-direction is critical.

11-15

3rd

I

Set to 1 if failure in positive y-direction is critical.

16-20

4th

I

Set to 1 if failure in negative y-direction is critical.

21-25

5th

I

Set to 1 if failure in positive z-direction is critical.

26-30

6th

I

Set to 1 if failure in negative z-direction is critical.

31-35

7th

I

Set to 1 if failure in xy-plane is critical.

36-40

8th

I

Set to 1 if failure in yz-plane is critical.

41-45

9th

I

Set to 1 if failure in zx-plane is critical.

Enter the words MX STRAIN.

For MX Strain: 4th data block

Main Index

1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

εx – Maximum tensile strain in x-direction. εxc – Maximum absolute value of compressive strain in x-direction. εy – Maximum tensile strain in y-direction.

850 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

41-50

5th

F

51-60

6th

F

61-70

7th

F

εyc – Maximum absolute value of compressive strain in y-direction. εz – Maximum tensile strain in z-direction. εzc – Maximum absolute value of compressive strain in z-direction.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum tensile strain in x-direction.

11-15

3rd

I

Table ID for maximum compressive strain in x-direction.

16-20

4th

I

Table ID for maximum tensile strain in y-direction.

21-25

5th

I

Table ID for maximum compressive strain in y-direction.

26-30

6th

I

Table ID for maximum tensile strain in z-direction.

31-35

7th

I

Table ID for maximum compressive strain in z-direction.

5th data block 1-10

1st

F

γxy – Maximum absolute value of shear strain in xy-plane.

11-20

2nd

F

γyz – Maximum absolute value of shear strain in yz-plane.

21-30

3rd

F

γzx – Maximum absolute value of shear strain in zx-plane.

5b data block 1-5

1st

I

Table ID for maximum shear strain in xy-plane.

6-10

2nd

I

Table ID for maximum shear strain in yz-plane.

11-15

3rd

I

Table ID for maximum shear strain in zx-plane.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness faction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block

Main Index

1-5

1st

I

Set to 1 is failure in positive x-direction is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if failure in negative x-direction is critical.

11-15

3rd

I

Set to 1 if failure in positive y-direction is critical.

16-20

4th

I

Set to 1 if failure in negative y-direction is critical.

21-25

5th

I

Set to 1 if failure in positive z-direction is critical.

26-30

6th

I

Set to 1 if failure in negative z-direction is critical.

31-35

7th

I

Set to 1 if failure in xy-plane is critical.

FAIL DATA (with TABLE Input) 851 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

36-40

8th

I

Set to 1 if failure in yz-plane is critical.

41-45

9th

I

Set to 1 if failure in zx-plane is critical.

For Hoffman or Hill: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

Enter either HOFFMAN or HILL. X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress z-direction. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined for Hoffman. For Hill, Xc, Yc, and Zc are assumed to be equal to X, Y, and Z respectively and are not used.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum tensile stress in x-direction.

11-15

3rd

I

Table ID for maximum compressive stress in x-direction.

16-20

4th

I

Table ID for maximum tensile stress in y-direction.

21-25

5th

I

Table ID for maximum compressive stress in y-direction.

26-30

6th

I

Table ID for maximum tensile stress in z-direction.

31-35

7th

I

Table ID for maximum compressive stress in z-direction.

5th data block 1-10

1st

F

Sxy

– Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz

– Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx

– Maximum absolute value of shear stress in zx-plane.

31-40

4th

F

Failure index. Default is 1.0.

5b data block

Main Index

1-5

1st

I

Table ID for maximum shear stress in xy-plane.

6-10

2nd

I

Table ID for maximum shear stress in yz-plane.

11-15

3rd

I

Table ID for maximum shear stress in zx-plane.

852 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

1st

I

Set to 1 if failure in positive x-direction is critical (leads to element deactivation).

Enter the word TSAI-WU.

For Tsai-Wu: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

4th

F

61-70

5th

F

X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress in z-direction. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum tensile stress in x-direction.

11-15

3rd

I

Table ID for maximum compressive stress in x-direction.

16-20

4th

I

Table ID for maximum tensile stress in y-direction.

21-25

5th

I

Table ID for maximum compressive stress in y-direction.

26-30

6th

I

Table ID for maximum tensile stress in z-direction.

31-35

7th

I

Table ID for maximum compressive stress in z-direction.

5th data block

Main Index

1-10

1st

F

Sxy – Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz – Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx – Maximum absolute value of shear stress in zx-plane.

31-40

4th

F

41-50

5th

F

Failure index. Default is 1.0. Fxy – Interactive strength tensor constant for the xy-plane.

FAIL DATA (with TABLE Input) 853 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

61-60

6th

F

Fyz – Interactive strength tensor constant for the yz-plane.

61-70

7th

F

Fzx – Interactive strength tensor constant for the zx-plane. Note:

Fxy should be such that

1 1 - -------2 < --------F xy ⋅ X X c YY c

, etc.

5b data block 1-5

1st

I

Table ID for maximum shear stress in xy-plane.

6-10

2nd

I

Table ID for maximum shear stress in yz-plane.

11-15

3rd

I

Table ID for maximum shear stress in zx-plane.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Table ID for Fxy.

26-30

6th

I

Table ID for Fyz.

31-35

7th

I

Table ID for Fzx.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

1st

I

Set to 1 if failure in positive x-direction is critical (leads to element deactivation).

Enter the word HASHIN.

For HASHIN: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

X – Maximum fiber tensile stress. Xc – Maximum fiber compressive stress. Y – Maximum matrix tensile stress. Yc Note:

Maximum matrix compressive stress. Xc and Yc default to the values of X and Y, respectively, if left undefined.

4b data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum fiber tensile stress.

11-15

3rd

F

Table ID for maximum fiber compressive stress.

854 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Table ID for maximum matrix tensile stress.

21-25

5th

I

Table ID for maximum matrix compressive stress.

5th data block 1-10

1st

F

Sxy -

Maximum in-plane shear stress.

11-20

2nd

F

Syz -

Maximum transverse shear stress.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

5b data block 1-5

1st

I

Table ID for maximum in-plane shear stress.

6-10

2nd

I

Table ID for maximum transverse shear stress.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block

Main Index

1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

31-40

4th

F

a4 – Factor for E3 reduction due to fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

41-50

5th

F

a5 – Factor for G12 reduction from fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

FAIL DATA (with TABLE Input) 855 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

Enter the word HASHIN-TAPE.

For HASHIN-TAPE 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

Xc – Maximum tape fiber compressive stress.

31-40

4th

F

Y – Maximum tape cross fiber tensile stress.

41-50

5th

F

X – Maximum tape fiber tensile stress.

Yc – Maximum tape cross fiber compressive stress. Note:

Xc and Yc default to the values of X and Y, respectively, if left undefined.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum tape fiber tensile stress.

11-15

3rd

F

Table ID for maximum tape fiber compressive stress.

16-20

4th

I

Table ID for maximum tape cross fiber tensile stress.

21-25

5th

I

Table ID for maximum tape cross fiber compressive stress.

5th data block 1-10

1st

F

Sxy – Maximum in-plane shear stress.

11-20

2nd

F

Syz – Maximum y-z transverse shear stress.

21-30

3rd

F

Sxz – Maximum x-z transverse shear stress.

31-40

4th

F

Not used; enter 0.

5b data block 1-5

1st

I

Table ID for maximum in-plane shear stress.

6-10

2nd

I

Table ID for maximum y-z transverse shear stress.

11-15

3rd

I

Table ID for maximum x-z transverse shear stress.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3.

Main Index

856 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

31-40

4th

F

a4 – Factor for E3 reduction due to fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

6-10

2nd

I

41-50

5th

F

Set to 1 if fiber compression failure is critical. a5 – Factor for G12 reduction from fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

For HASHIN-FABRIC 4th data block

Main Index

1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

Enter the word HASHIN-FABRIC. X – Maximum first fiber tensile stress. Xc – Maximum first fiber compressive stress. Y – Maximum second fiber tensile stress.

FAIL DATA (with TABLE Input) 857 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

41-50

5th

F

51-60

6th

F

61-70

7th

F

Yc – Maximum second fiber compressive stress. Z – Maximum thickness tensile stress. Zc – Maximum thickness compressive stress. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum first fiber tensile stress.

11-15

3rd

F

Table ID for maximum first fiber compressive stress.

16-20

4th

I

Table ID for maximum second fiber tensile stress.

21-25

5th

I

Table ID for maximum second fiber compressive stress.

26-30

6th

I

Table ID for maximum thickness tensile stress

31-35

7th

I

Table ID for maximum thickness compressive stress

5th data block 1-10

1st

F

Sxy – Maximum in-plane shear stress.

11-20

2nd

F

Syz – Maximum y-z transverse shear stress.

21-30

3rd

F

Sxz – Maximum x-z transverse shear stress.

31-40

4th

F

Not used; enter 0.

5b data block 1-5

1st

I

Table ID for maximum in-plane shear stress.

6-10

2nd

I

Table ID for maximum y-z transverse shear stress.

11-15

3rd

I

Table ID for maximum x-z transverse shear stress.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block

Main Index

1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

S11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

858 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

For PUCK: 4th data block Enter the work PUCK.

1-10

1sT

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

Yc – Maximum matrix compressive stress.

51-60

6th

F

S12 – Maximum in-plane shear stress.

X – Maximum fiber tensile stress. Xc – Maximum fiber compressive stress. Y – Maximum matrix tensile stress.

Note:

Xc and Yc default to the values of X and Y, respectively, if left undefined.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum fiber tensile stress.

11-15

3rd

I

Table ID for maximum fiber compressive stress.

16-20

4th

I

Table ID for maximum matrix tensile stress.

21-25

5th

I

Table ID for maximum matrix compressive stress.

26-30

6th

I

Table ID for maximum in-plane shear stress.

5th data block 1-10

1st

F

p12C – slope of fracture envelope, in-plane compression.

11-20

2nd

F

p12T – slope of fracture envelope, in-plane tension. Defaults to p12C.

21-30

3rd

F

p23C – slope of fracture envelope, transverse compression.

31-40

4th

F

p23T – slope of fracture envelope, transverse tension. Not needed for plane stress. Defaults to p23C. Note:

For plane stress, either p12C or p23C is given (and optionally p12T). For this case the fracture angle is calculated analytically.

5b data block 1-5

1st

I

Not used; enter zero.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3.

Main Index

FAIL DATA (with TABLE Input) 859 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

31-40

4th

F

a4 – Factor for E3 reduction due to fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

41-50

5th

F

a5 – Factor for G12 reduction from fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression mode B failure is critical.

21-25

5th

E

Set to 1 if matrix compression mode C failure is critical.

For UFAIL: For UFAIL type failure criterion, enter only the word UFAIL in the 4th data block and leave all other fields blank. 4th data block 1-10

1st

A

Enter the word UFAIL.

There is not 5th data blocks for this option. Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3.

Main Index

860 FAIL DATA (with TABLE Input) Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

Main Index

1st

I

Set to 1 if failure is critical (leads to element deactivation).

FAIL DATA 861 Define Failure Criteria Data

FAIL DATA

Define Failure Criteria Data

The information provided here is based upon not using the table driven input style. Description This option is used to define material dependent failure criteria data. Up to three failure criteria per material can be specified. Failure indices are calculated and printed for every integration point at which material dependent failure data exists. This option can also be used to invoke the progressive failure of a material. The supported failure criteria types are: MX STRESS MX STRAIN TSAI-WU HOFFMAN HILL HASHIN HASHIN-TAPE HASHIN-FABRIC PUCK UFAIL Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FAIL DATA.

2nd data block 1-5

1st

I

Enter the number of materials with Marc calculated failure criteria. If blank, Marc reads until no more failure criteria data are left.

6-10

2nd

I

Enter the unit number for reading. Defaults to input.

Data blocks 3 through 7 are repeated as a set, once for each material with Marc calculated failure criteria, as described above.

Main Index

862 FAIL DATA Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Number of sets of failure criteria data for this material. No more than three sets are allowed.

11-15

3rd

I

Flag to invoke the progressive failure option. Enter 0 for no progressive failure analysis. Enter 1 for the standard Marc method. Enter 2 for gradual selective stiffness degradation. Enter 3 for immediate selective stiffness degradation.

Data blocks 4 and 7 are entered as pairs, once for each set of failure criteria data. The 6th and 7th data blocks are not required unless progressive failure option 2 or 3 is used. For MX Stress: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

Enter the words MX STRESS. X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress in z-direction.

5th data block 1-10

1st

F

Sxy – Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz – Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx – Maximum absolute value of shear stress in zx-plane. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

Main Index

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

FAIL DATA 863 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

7th data block 1-5

1st

I

Set to 1 is failure in positive x-direction is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if failure in negative x-direction is critical.

11-15

3rd

I

Set to 1 if failure in positive y-direction is critical.

16-20

4th

I

Set to 1 if failure in negative y-direction is critical.

21-25

5th

I

Set to 1 if failure in positive z-direction is critical.

26-30

6th

I

Set to 1 if failure in negative z-direction is critical.

31-35

7th

I

Set to 1 if failure in xy-plane is critical.

36-40

8th

I

Set to 1 if failure in yz-plane is critical.

41-45

9th

I

Set to 1 if failure in zx-plane is critical.

Enter the words MX STRAIN.

For MX Strain: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

εzc – Maximum absolute value of compressive strain in z-direction

εx – Maximum tensile strain in x-direction. εxc – Maximum absolute value of compressive strain in x-direction. εy – Maximum tensile strain in y-direction. εyc – Maximum absolute value of compressive strain in y-direction. εz – Maximum tensile strain in z-direction.

5th data block 1-10

1st

F

γxy – Maximum absolute value of shear strain in xy-plane.

11-20

2nd

F

γyz – Maximum absolute value of shear strain in yz-plane.

21-30

3rd

F

γzx – Maximum absolute value of shear strain in zx-plane.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block

Main Index

1-5

1st

I

Set to 1 is failure in positive x-direction is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if failure in negative x-direction is critical.

864 FAIL DATA Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Set to 1 if failure in positive y-direction is critical.

16-20

4th

I

Set to 1 if failure in negative y-direction is critical.

21-25

5th

I

Set to 1 if failure in positive z-direction is critical.

26-30

6th

I

Set to 1 if failure in negative z-direction is critical.

31-35

7th

I

Set to 1 if failure in xy-plane is critical.

36-40

8th

I

Set to 1 if failure in yz-plane is critical.

41-45

9th

I

Set to 1 if failure in zx-plane is critical.

For Hoffman or Hill: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

Enter either HOFFMAN or HILL. X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress in z-direction. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined for Hoffman. For Hill, Xc, Yc and Zc are assumed to be equal to X, Y, and Z respectively and are not used.

5th data block 1-10

1st

F

Sxy

– Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz

– Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx

– Maximum absolute value of shear stress in zx-plane.

31-40

4th

F

Failure index. Default is 1.0.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

Main Index

1st

I

Set to 1 if failure in positive x-direction is critical (leads to element deactivation).

FAIL DATA 865 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

For Tsai-Wu: 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

4th

F

61-70

5th

F

Enter the word TSAI-WU. X – Maximum tensile stress in x-direction. Xc – Maximum absolute value of compressive stress in x-direction. Y – Maximum tensile stress in y-direction. Yc – Maximum absolute value of compressive stress in y-direction. Z – Maximum tensile stress in z-direction. Zc – Maximum absolute value of compressive stress in z-direction. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

5th data block 1-10

1st

F

Sxy – Maximum absolute value of shear stress in xy-plane.

11-20

2nd

F

Syz – Maximum absolute value of shear stress in yz-plane.

21-30

3rd

F

Szx – Maximum absolute value of shear stress in zx-plane.

31-40

4th

F

41-50

5th

F

Fxy – Interactive strength tensor constant for the xy-plane.

61-60

6th

F

Fyz – Interactive strength tensor constant for the yz-plane.

61-70

7th

F

Fzx – Interactive strength tensor constant for the zx-plane.

Failure index. Default is 1.0.

Note:

Fxy should be such that

1 12 < --------- ⋅ -------F xy X X c YY c

, etc.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

1st

I

Set to 1 if failure in positive x-direction is critical (leads to element deactivation).

Enter the word HASHIN.

For HASHIN: 4th data block

Main Index

1-10

1st

A

11-20

2nd

F

X – Maximum fiber tensile stress.

866 FAIL DATA Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

31-40

4th

F

41-50

5th

F

Xc – Maximum fiber compressive stress. Y – Maximum matrix tensile stress. Yc – Maximum matrix compressive stress. Note:

Xc and Yc default to the values of X and Y, respectively, if left undefined.

5th data block 1-10

1st

F

Sxy – Maximum in-plane shear stress.

11-20

2nd

F

Syz – Maximum transverse shear stress.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block

Main Index

1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

31-40

4th

F

a4 – Factor for E3 reduction due to fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

41-50

5th

F

a5 – Factor for G12 reduction from fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

FAIL DATA 867 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

Enter the word HASHIN-TAPE.

For HASHIN-TAPE 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

Y – Maximum tape cross fiber tensile stress.

41-50

5th

F

Yc – Maximum cross fiber compressive stress.

X – Maximum fiber tensile stress. Xc – Maximum fiber compressive stress.

Note:

Xc and Yc default to the values of X and Y, respectively, if left undefined.

5th data block 1-10

1st

F

Sxy – Maximum in-plane shear stress.

11-20

2nd

F

Syz – Maximum y-z transverse shear stress.

21-30

3rd

F

Sxz – Maximum x-z transverse shear stress.

31-40

4th

F

Not used; enter 0.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block

Main Index

1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

868 FAIL DATA Define Failure Criteria Data

Format Fixed 31-40

Free 4th

Data Entry Entry F

a4 – Factor for E3 reduction due to fiber failure. Takes values

between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure. 41-50

5th

F

a5 – Factor for G12 reduction from fiber failure. Takes values

between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure. 7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

For HASHIN-FABRIC 4th data block 1-10

1st

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

51-60

6th

F

61-70

7th

F

Enter the word HASHIN-FABRIC. X – Maximum first fiber tensile stress. Xc – Maximum first fiber compressive stress. Y – Maximum second fiber tensile stress. Yc – Maximum second fiber compressive stress. Z – Maximum thickness tensile stress. Zc – Maximum thickness compressive stress. Note:

Xc, Yc, and Zc default to the values of X, Y, and Z, respectively, if left undefined.

5th data block 1-10

1st

F

Sxy – Maximum in-plane shear stress.

11-20

2nd

F

Syz – Maximum y-z transverse shear stress.

21-30

3rd

F

Sxz – Maximum x-z transverse shear stress.

31-40

4th

F

Not used; enter 0.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3.

Main Index

FAIL DATA 869 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

16-20

4th

E

Set to 1 if matrix compression failure is critical.

Enter the work PUCK.

For PUCK: 4th data block 1-10

1sT

A

11-20

2nd

F

21-30

3rd

F

31-40

4th

F

41-50

5th

F

Yc – Maximum matrix compressive stress.

51-60

6th

F

S12 – Maximum in-plane shear stress.

X – Maximum fiber tensile stress. Xc – Maximum fiber compressive stress. Y – Maximum matrix tensile stress.

Note:

Xc and Yc default to the values of X and Y, respectively, if left undefined.

4b data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for maximum fiber tensile stress.

11-15

3rd

I

Table ID for maximum fiber compressive stress.

16-20

4th

I

Table ID for maximum matrix tensile stress.

21-25

5th

I

Table ID for maximum matrix compressive stress.

26-30

6th

I

Table ID for maximum in-plane shear stress.

5th data block

Main Index

1-10

1st

F

p12C – slope of fracture envelope, in-plane compression.

11-20

2nd

F

p12T – slope of fracture envelope, in-plane tension. Defaults to p12C.

870 FAIL DATA Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

p23C – slope of fracture envelope, transverse compression.

31-40

4th

F

p23T – slope of fracture envelope, transverse tension. Not needed for plane stress. Defaults to p23C. Note:

For plane stress, either p12C or p23C is given (and optionally p12T). For this case the fracture angle is calculated analytically.

5b data block 1-5

1st

I

Not used; enter zero.

Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

11-20

2nd

F

a2 – Factor for E2 reduction due to matrix compression failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E2 is reduced in the same way as for matrix tension. A value of 1.0 leads to no E2 reduction due to matrix compression failure.

21-30

3rd

F

a3 – Factor for G12 reduction relative to E2 reduction. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 is reduced in the same way as E2. A value of 1.0 leads to no G12 reduction.

31-40

4th

F

a4 – Factor for E3 reduction due to fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where E3 is reduced in the same way E1. A value of 1.0 leads to an E3 reduction due to E2 only. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

41-50

5th

F

a5 – Factor for G12 reduction from fiber failure. Takes values between 0.0 and 1.0. Defaults to 0.0 where G12 reduces only due to matrix failure. A value of 1.0 leads to a G12 reduction due to only fiber failure. Values between 0.0 and 1.0 lead to a mixture of degradation from matrix and fiber failure.

7th data block

Main Index

1-5

1st

I

Set to 1 if fiber tension failure is critical (leads to element deactivation).

6-10

2nd

I

Set to 1 if fiber compression failure is critical.

11-15

3rd

E

Set to 1 if matrix tension failure is critical.

FAIL DATA 871 Define Failure Criteria Data

Format Fixed

Free

Data Entry Entry

16-20

4th

E

Set to 1 if matrix compression mode B failure is critical.

21-25

5th

E

Set to 1 if matrix compression mode C failure is critical.

For UFAIL: For UFAIL type failure criteria, enter only the word UFAIL in the 4th data block and leave all other fields blank. 4th data block 1-10

1st

A

Enter the word UFAIL.

There is no 5th data block for this option. Data blocks 6 and 7 are entered only if the progressive failure option is 2 or 3. 6th data block 1-10

1st

F

a1 – Residual stiffness fraction. For failure option 3, it is the fraction of initial stiffness upon failure. For failure option 2, the stiffness is not reduced more than this fraction. Defaults to 0.01.

7th data block 1-5

Main Index

1st

I

Set to 1 if failure is critical (leads to element deactivation).

872 MATERIAL DATA Define Additional Material Data Constants

MATERIAL DATA

Define Additional Material Data Constants

Description This option allows you to enter additional material constants that may be required by constitutive laws, damage models, grain size models, etc. Those fields explicitly mentioned are used by Marc models; the other fields may be arbitrarily used and then passed to user subroutines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words MATERIAL DATA.

2nd data block 1-5

1st

I

Enter the number of sets.

6-10

2nd

I

Enter the maximum number of material data values per material ID. Defaults to 1.

Repeat 3rd and 4th data blocks in sets. 3rd data block 1-5

1st

I

Enter material ID.

4th data block If more than 8 constants, repeat 4th data block as necessary. 1-10

1st

E

Enter the Activation Energy.

11-20

2nd

E

Enter next constant.

etc. Note:

Main Index

The 2nd to 8th fields can be used by a smart user who wants to push material.

GRAIN SIZE 873 Define Grain Size Growth Model

GRAIN SIZE

Define Grain Size Growth Model

Description This option allows you to define a model to predict the grain size based upon the process history. The grain size can be placed on the post file for viewing. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GRAIN SIZE.

2nd data block 1-5

1st

I

Enter the number of sets of data.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Repeat 3rd and 4th data blocks for each data set. 3rd data block 1-4

1st

I

Enter the material ID.

6-10

2nd

I

Enter the grain growth model. Enter 1 for Yada model Enter -1 for the UGRAIN user subroutine.

4th data block For Yada model: The grain size (g) is defined by: if

ε < ε growth g = g 0

if

· – C 2 – C 3∗ Q ⁄ R T ε ≥ ε growth g = C 1 × ε *e

where ε growth = C 4∗ e

C5 ⁄ T

The activation energy (Q) is specified in the MATERIAL DATA option and the universal gas constant (R) is specified in the PARAMETERS option.

Main Index

1-10

1st

F

Enter the initial grain size g0.

11-20

2nd

F

Enter the initial grain size C1.

874 GRAIN SIZE Define Grain Size Growth Model

Format Fixed

Main Index

Free

Data Entry Entry

21-30

3rd

F

Enter the initial grain size C2.

31-40

4th

F

Enter the initial grain size C3.

41-50

5th

F

Enter the initial grain size C4.

51-60

6th

F

Enter the initial grain size C5.

DAMAGE 875 Define Properties for Damaging Materials

DAMAGE

Define Properties for Damaging Materials

Description This option allows you to define a set of data for a specific material which includes a damage model. The specific model and associated data can also be specified with this option. Gurson Model

For elasto-plastic materials, the damage model is based on a Gurson model for the yield surface definition for materials with voids: q 2 σ kk σ 2 * * 2 F = ⎛ -----⎞ + 2 q 1 f cosh ⎛ --------------⎞ – [ 1 + ( q 1 f ) ] = 0 ⎝ σ y⎠ ⎝ 2σ y ⎠

Void nucleation and void growth are based on a model by Tvergaard and Needleman. Here, f * is introduced to model the rapid decrease in load carrying capacity if void coalescence occurs: f f

*

*

= f

if

f ≤ fc

fu – fc = f c + --------------- ( f – f c ) fF – fc

if

f > fc

the nucleation can be either stress or strain controlled. The strain controlled nucleation is given by: p

fN 1 ⎛ εm – ε n⎞ · -⎟ f nucleation = -------------- exp – --- ⎜ ------------------2⎝ S ⎠ S 2π

2

·p εm

Additional data for the initial void volume fraction can be defined with the UVOID user subroutine. Other nucleation models are allowed via the UVOIDN user subroutine. Rubber Models

For elastomeric materials, the model is based on the undamaged strain energy function W ° multiplied by a Kachanov damage factor, K . The damage capability is available for Ogden strain energy model using the total Lagrange formulation as well as the Mooney-Rivlin, Ogden, and general principal stretch based model using the updated Lagrange formulation. W = K ⋅ W°

Both continuous damage (Miehe’s formulation) as well as the discontinuous damage (Mullin’s effect) can be modeled within an additive: K = d

∞

N

+

∑ n =1

a dn

α exp ⎛ – ------⎞ + ⎝ η n⎠

or a multiplicative format:

Main Index

N

∑ m= 1

β β d m exp ⎛ – ------⎞ ⎝ λ m⎠

( N = 1, 2 )

876 DAMAGE Define Properties for Damaging Materials

K = d

∞

N

+

∑ n =1

if

( N = 1, 2 )

∞

has not been specified, it will be automatically calculated by Marc such that at zero values of the Kachanov factor K = 1 .

d

β,

α + δn β d n exp ⎛ – --------------------⎞ ⎝ ηn ⎠

α

and

Lemaitre Model

The Lemaitre damage model is a phenomenological approach to ductile damage in ferrous materials that are subject to large plastic deformations as they occur in the manufacturing processes. The model is based on the thermodynamic dissipation potential of the material where ductile damage is considered as a specific energy that is released when macroscopic fracture occurs. The Lemaitre model may only be used with continuum elements. Without going further into detail the mathematical derivation can be found in: Lemaitre, J.: A Course on Damage Mechanics, 2nd Ed., Springer Verlag, Berlin, 1996. In the following paragraphs, some basic formulas are given that serve for the calculation and the interpretation of the damage values. The material parameters can be derived by uniaxial tensile tests for the assumed forming conditions (strain rate, temperature). Some standard values are given in this context, more information can be found in the mentioned literature. The Lemaitre damage model calculates three damage values which have different meanings. Macroscopic damage is characterized by plastic deformation that leads to pore growth, pore coalescence and final rupture of the material matrix. The damage growth begins approximately after an equivalent plastic strain threshold, ε d . This is the first material parameter to be defined in an experiment. For mild steels, it is assumed to be between 0.1 and 0.2. The so-called absolute damage D represents the ductile damage growth in the material. The incremental damage law is given as follows: 2

f(η) ⋅ σ d D = -----------------------------------------2- dε p , 2E ⋅ S ⋅ ( 1 – D )

0≤D≤1

where the triaxiality function as follows: 2 f ( η ) = --- ( 1 + v ) + 3 ( 1 – 2v )η 2 3

σ

is the von Mises stress,

E

f(η)

contains information about the state of stresses and is defined

σm η = ------σ

the Young’s modulus,

v

the Poisson’s ratio,

σm

the mean normal stress,

D

the current integrated value of the absolute damage at that material point and d ε p the effective plastic strain increment. For most steels, one can assume a maximum value of D from 0.15 to 0.4 at fracture. Copper might even reach D = 0.9 . The more ductile the material, the higher D becomes. S is called the damage resistance factor, a material parameter to be determined from tensile tests. S is from 1 to 8 according to the ductility of the material (1 low, 8 high). This parameter influences mostly the growth of D and can also be determined by data correlation (for example, simulate the material test then derive the correct material parameter).

Main Index

DAMAGE 877 Define Properties for Damaging Materials

The critical damage D c is used to compare the ductile damage D with the “state” of the material; such as, whether the actual conditions (stresses, strains, state of stresses, already reached damage, etc.) might be critical for macroscopic failure: 2

σU 2 D c = D 1c -------------------------(1 – D) 2 (σ f(η))

1 ≥ Dc ≥ 0

D 1c is the critical damage in the uniaxial loadcase, the third material parameter to be determined by tensile tests. Most steels show a D 1 c from 0.15 to 0.4. σ v is the ultimate stress during the tensile test (before necking begins). The lower D c , the more likely a material damage is. Note that D c behaves

contrary to

D : Dc = 1

for the “safe” material and low for possible damaged regions.

In fact the comparison between D and D c is necessary to identify critical forming zones: as long as D is (much) lower than D c , the forming operation is safe. When D reaches D c , the damage probability tends to be 100%. The comparison is done by the relative damage value D rel (reflected in the postprocessing): D D rel = -----Dc

0 ≤ D rel ≤ 1

When D rel approaches 1 in a specific region, fracture is highly possible whereas small values indicate a “safe” region. Simplified Model

For elastic, elastic-plastic, or rigid-plastic materials, there is the option for you to define a simplified damage model. You define the damage factor (df) in the UDAMAG user subroutine. If model 9 is used, then: p ·p σ y = σ y ( ε , ε , T )* ( 1.0 – d f )

If model 10 is used, then: p ·p σ y = σ y ( ε , ε , T )* ( 1.0 – d f )

and

E = E ( T )* ( 1.0 – df )

The normal data for a specific material are defined with the ISOTROPIC, ORTHOTROPIC, and WORK HARD options. Cross-reference to this material is made with the material number. For orthotropic materials, the Young’s moduli and the shear moduli are all scaled equally. These simplified models may not be used with the FeFp elastic-plastic formulation, soil models, or in conjunction with viscoelasticity.

Main Index

878 DAMAGE Define Properties for Damaging Materials

Cockroft-Latham Damage Indicator

Cockroft-Latham damage indicator does not affect the yield stress. It is a postprocessing value to indicate a possible damage area. It can also be used to initiate crack by removing elements in the area. σ max ·

- ε dt ≥ C ∫ ----------σ

where

σ ma x

is the maximum principal stress,

plastic strain rate.

C

σ

is the effective von Mises stress and

ε·

is the effective

C

is material

is material constant threshold for damage.

The Cockroft-Latham model may only be used with continuum elements. Principal-tension Damage Indicator

This damage indicator does not affect the yield stress. σ max

- dt ≥ C ∫ ----------σ

where σ ma x is the maximum principal stress and constant threshold for damage.

σ

is the effective von Mises stress.

This model may only be used with continuum elements. Oyane Damage Indicator σm

- + B⎞ ε dt ≥ C ∫ ⎛⎝ -----⎠ σ ·

Similar to Cockroft-Latham, Oyane damage indicates a possible damage area where average stress, B and C are both material constants.

σm

is the mean or

The Oyane model may only be used with continuum elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DAMAGE.

2nd data block

Main Index

1-5

1st

I

Enter the number of distinct sets of material properties to be input (optional).

6-10

2nd

I

Enter the logical unit number for reading damage data. Defaults to input.

11-15

3rd

I

Enter 1 if critically damaged elements should be removed from the post file (valid only for Gurson Model).

DAMAGE 879 Define Properties for Damaging Materials

Format Fixed

Free

Data Entry Entry

The 3rd and 4th data blocks are entered as pairs, once for each distinct data set. 3rd data block 1-5

1st

I

Material type identification (1, 2, 3, etc.) for cross-referencing to ISOTROPIC or OGDEN options.

6-10

2nd

I

Damage Model: 0 – Gurson Model, with no nucleation. 1 – Gurson Model, with plastic-strain controlled nucleation. 2 – Gurson Model, with stress controlled nucleation. 3 – Gurson Model, with nucleation controlled by the UVOIDN user subroutine. 4 – Elastomeric damage model; additive decomposition of the Kachanov factor. 5 – Elastomeric damage model; multiplicative decomposition of the Kachanov factor. 6 – Elastomeric damage model controlled by the UELDAM user subroutine. 7 or 8 – Lemaitre damage model. 9 – Simplified damage model. 10 – Simplified model, damage applied to yield stress and Young’s modulus. 11 – Cockroft-Latham damage indicator. 12 – Principal-tension damage indicator. 13 – Oyane damage indicator.

11-20

3rd

F

Scalar factor at infinity ( d ∞ ); used only for rubber damage with additive or multiplicative decomposition of the Kachanov factor.

21-25

4th

I

Number of auxiliary damage variables to be stored per integration point for damage models 9 and 10.

4a data block Use only if the method of void nucleation (shown above) is 0, 1, 2, or 3.

Main Index

1-10

1st

F

First yield surface multiplier q1 (recommended is q1 = 1.5).

11-20

2nd

F

Second yield surface multiplier q2 (recommended is q2 = 1).

21-30

3rd

F

Initial void volume fraction.

880 DAMAGE Define Properties for Damaging Materials

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Critical void volume fraction. This value represents the value at which coalescence of voids start (fc).

41-50

5th

F

Failure void volume fraction (fF). This is the value of the void volume fraction at which the stiffness of the material has reduced to zero.

51-60

6th

F

If strain controlled, enter the mean strain for nucleation. If stress controlled, enter the mean stress for nucleation. Not needed if UVOIDN user subroutine is used.

61-70

7th

F

Standard deviation in nucleation relation (S). Not needed if UVOIDN user subroutine is used.

71-80

8th

F

Volume fraction of void nucleating particles fN. Not needed if UVOIDN user subroutine is used. Note:

The presence of these blocks in the model definition option automatically overwrites the yield criterion specified for a specific material on the ISOTROPIC option. Currently, the model can only be used for isotropic hardening materials.

4b data block Use only for elastomeric damage model, additive decomposition, two term Prony series. β

1-10

1st

F

First scalar factor, continuous damage ( d1 ).

11-20

2nd

F

First relaxation parameter, continuous damage (λ1).

21-30

3rd

F

Second scalar factor, continuous damage ( d2 ).

31-40

4th

F

Second relaxation parameter, continuous damage (λ2).

41-50

5th

F

First scalar factor, discontinuous damage ( d1 ).

51-60

6th

F

First relaxation parameter, discontinuous damage (η1).

61-70

7th

F

Second scalar factor, discontinuous damage ( d2 ).

71-80

8th

F

Second relaxation parameter, discontinuous damage (η2).

β

α

α

4c data block Use only for elastomeric damage model, multiplicative decomposition, two term Prony Series.

Main Index

1-10

1st

F

First scalar factor (d1).

11-20

2nd

F

First proportioning term (δ1).

21-30

3rd

F

First relaxation rate constant (η1).

DAMAGE 881 Define Properties for Damaging Materials

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Second scalar factor (d2).

41-50

5th

F

Second proportioning term (δ2).

51-60

6th

F

Second relaxation rate constant (η2).

4d data block Used only for Lemaitre models, type 7 and 8. 1-10

1st

F

Critical uniaxial damage

( D 1c ) .

11-20

2nd

F

Corrected ultimate stress

( σv ) .

21-30

3rd

F

Damage resistance factor

(S) .

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Plastic strain threshold before damage

( εd ) .

4e data block Used only for damage models type 11, 12, and 13. 1-10

1st

F

Damage threshold. Default 0.

11-20

2nd

F

Material constant (B) of Oyane damage model.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Damage crack threshold (element removal). Default 0 (no such control).

Note:

Main Index

For damage models 11, 12, and 13, the UDAMAGE_INDICATOR user subroutine can be used to implement different damage indicators not supported here.

882 GAP DATA Define Data for Gap Elements

GAP DATA

Define Data for Gap Elements

Description This option allows you to specify all of the data associated with gap elements (types 12 and 97). These data include gap closure distance, gap elastic stiffness, contact coefficient of friction, and momentum ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GAP DATA.

2nd data block 1-5

1st

I

Number of sets of gap data to be input.

6-10

2nd

I

Unit number for reading data. Defaults to input.

The 3rd and 4th data blocks are entered as pairs, once for each set of gap data. 3rd data block 1-10

1st

F

For a fixed direction gap, enter the gap closure distance Ucl. For a true distance gap, enter the minimum distance d between end points. Note:

Main Index

If d > 0, the two end points is never closer than a distance |d| apart. If d < 0, the two end points are never farther apart than |d|.

11-20

2nd

F

μ, the contact coefficient of friction.

21-30

3rd

F

KGAP, the elastic stiffness of the closed gap in the contact direction. Default: Gap is rigid when closed.

31-40

4th

F

KFRICTION, the elastic stiffness of the closed gap in the friction direction. Default: Gap is rigid when closed.

41-50

5th

F

User supplied momentum ratio for first gap node. Default: Marc calculates this ratio internally.

51-60

6th

F

User supplied momentum ratio for fourth gap node. Default: Marc calculates this ratio internally.

GAP DATA 883 Define Data for Gap Elements

Format Fixed 61-65

Free 7th

Data Entry Entry I

Enter 0 for fixed direction gap. Enter 1 for true distance gap. Default is 0.

66-70

8th

I

Enter 0 if gap is open during increment 0. Enter 1 if gap is closed during increment 0. Default is 0.

4th data block Enter a list of gap elements to be associated with this set of gap data.

Main Index

884 COMPOSITE Define Properties for Laminated Composite Materials

COMPOSITE

Define Properties for Laminated Composite Materials

Description This option allows you to define the layer-by-layer material identifications, layer thicknesses, and orientation angles for a laminated composite material and to associate this information with an element number. Property data for each material identification is entered using the ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, HYPOELASTIC, or NLELAST options. If the fast-integrated option is used, the material behavior of each layer must be entered using only the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC options. To specify a user-defined orientation, use the ORIENTATION option. Note that an input error results if the COMPOSITE option is specified for nonlayered elements. This option is available for shell, beams in a plane (type 16), composite solid (types 149-154, 175-180) or solid shell (type 185) elements. It is not available for open and closed-section beam elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word COMPOSITE.

2nd data block 1-5

1st

I

Enter the number of composite group data sets to follow.

6-10

2nd

I

Unit number for input. Defaults to standard input (unit 5).

11-15

3rd

I

Enter 1 to use the 4a data block (default). Enter 2 to use the 4b data block, which allows specification of the ply ID. (Pre-release in 2005r3 release)

3rd data block 1-5

1st

I

Composite group number.

6-10

2nd

I

Number of layers in this group.

11-15

3rd

I

Enter 0 to input actual layer thicknesses in the second field of the 4th data block. (Default is 0; that is, the sum of the layer thicknesses overrides thickness data entered in the GEOMETRY option. This option needs to be used if performing design sensitivity analysis or design optimization. Enter 1 to input percentage of total thickness in the second field of the 4th data block. In this case, element thickness is entered using the GEOMETRY option or the NODAL THICKNESS option.

Main Index

COMPOSITE 885 Define Properties for Laminated Composite Materials

Format Fixed

Free

Data Entry Entry If you are using the variable thickness capability for those elements which have such an option, you must enter 1 here and then enter percentages of total thickness in the second field of the 4th data block below. If a continuum composite element (that is, element types 149-154, 175-180) is used, entering 1 to input the percentage of the total element thickness is preferable. If 0 is entered, the actual layer thickness is converted to the percentage of the total thickness by Marc.

16-25

4th

F

Enter position of user-defined reference plane. This is the value of the local z-coordinate of the user-defined plane with respect to the geometric midplane. Default is 0.

26-30

5th

I

Enter the method for integrating through the thickness of composite shell elements. The default method is that given on the SHELL SECT parameter, if no value is given there, then the default is method 1. Enter 1 for conventional procedure, which supports all material behavior available for composite elements. Enter 2 if stiffness is to be fast-integrated through the thickness based upon classical laminate theory. This reduces the memory requirements and computational costs for elastic shells. Thermal strains and temperature dependent properties are not supported. Enter 3 if stiffness is to be fast-integrated through the thickness based upon classical laminate theory. This reduces the memory requirements and computational costs for elastic shells. This procedure uses more memory and computational time than method 2.

31-40

Note:

6th

F

Enter the allowable bond shear stress. This in only used if the TSHEAR parameter is activated. It may result in additional output and the usage of post codes 110 and 257. Note that the allowable bond shear stress is constant for all layer interfaces.

The user-defined reference plane value is only used to adjust layer positions relative to the geometric midplane of a composite shell element. If the location of the geometric mid-plane itself needs to be adjusted, use the shell offset option in the GEOMETRY option.

Either the 4a or 4b data block is repeated once for each layer defined in the 3rd data block. 4a data block

Main Index

1-5

1st

I

Material identification number for this layer.

6-15

2nd

F

Actual layer thickness if default (0) is used in data block 3, Field 3 (above). If 1, percentage of total thickness.

886 COMPOSITE Define Properties for Laminated Composite Materials

Format Fixed 16-25

Free 3rd

Data Entry Entry F

Ply orientation angle in degrees. Location of principal material axes with respect to element coordinate system measured positive about local zcoordinate, (that is, angle defining orientation of preferred frame w.r.t. element frame). The element orientation is either defined in the ORIENTATION option or defaults to the v1, v2, v3 system defined in element type 75 in the Marc Volume B: Element Library.

4b data block 1-5

1st

I

Enter the ply layer ID.

6-10

2nd

I

Material identification number for this layer.

11-20

3rd

F

Actual layer thickness if default (0) is used in data block 3, Field 3 (above). If 1, percentage of total thickness.

21-30

4th

F

Ply orientation angle in degrees. Location of principal material axes with respect to element coordinate system measured positive about local zcoordinate, (that is, angle defining orientation of preferred frame w.r.t. element frame). The element orientation is either defined in the ORIENTATION option or defaults to the v1, v2, v3 system defined in element type 75 in the Marc Volume B: Element Library.

5th data block Enter a list of elements to be associated with this particular composite group.

Main Index

MIXTURE 887 Define Constituents of Composite Material in Original and Potentially Damaged State

MIXTURE

Define Constituents of Composite Material in Original and Potentially Damaged State

Description This option allows one to create a new material that has multiple components in it. The material behavior will be based upon a “mixture” of the individual components based upon the mixture rule. Several of these mixture rules are only appropriate for linear elastic materials, but are still more than one finds in text books because they will account for temperature dependent material properties. The most sophisticated model (3) allows for the mixture of materials which undergo elastic-plastic behavior. Notes:

1)If void ratio or porosity is defined, it applied to all components in a uniform manner. 2)Model types 1 and 2 only support linear elastic material. 3)Model type 3 can not include the following material laws in any of the components. • Thermo-pore • Gurson damage • Simplified damage models 9 and 10 • Gasket material • Shape memory material • Soils • User defined generalized stress-strain law • ORNL • Rigid-Plastic • Grain size effects • Rubber material • Cohesive

4.) Rebar elements are not supported for type 3. 5.)Design sensitivity and design optimization is not supported for any of the models. 6.)PSHELL option is not supported for any of the models.

One restriction is that within a layer, if the components are orthotropic or anisotropic, the preferred directions are aligned.

Main Index

888 MIXTURE Define Constituents of Composite Material in Original and Potentially Damaged State

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

I

Enter the word MIXTURE.

2nd data block 1-5

1st

I

Enter the number of sets.

6-10

2nd

I

Enter the unit number. Defaults to input file.

Data blocks 3 through 5 are repeated for each data set. 3rd data block 1-5

1st

I

Enter the material ID.

6-10

2nd

I

Enter the number of components/phases.

11-15

3rd

I

Enter the mixture rule. 1 – weighted average of material properties based upon volume fraction (default) The components may be either elastic isotropic or orthotropic. 2 – weighted average of Hooke’s law based upon volume fraction. The components may be either elastic isotropic, orthotropic or anisotropic. 3 – weighted average of nonlinear stress strain curve based upon volume fraction

16-20

4th

I

Flag controlling averaging procedure for thermal expansion. 1 – weighted average based upon volume fraction (default) 2 – details later

21-25

5th

I

Not used, enter zero.

26-30

6th

I

Not used, enter zero.

31-35

7th

I

Not used, enter zero.

36-67

8th

A

Enter material name.

Data block 4 is repeated for each component 4th data block

Main Index

1-5

1st

I

Enter material id of component.

6-10

2nd

I

Not used, enter zero.

MIXTURE 889 Define Constituents of Composite Material in Original and Potentially Damaged State

Format Fixed 11-20

Free 3rd

Data Entry Entry E

Enter the fraction of this component, the sum of the fractions should equal 1.0.

5th data block Enter a list of elements for which this mixture of materials is applied. If composite, then leave blank.

Main Index

890 COHESIVE (with TABLE Input) Define Material Data for Interface Elements

COHESIVE (with TABLE Input)

Define Material Data for Interface Elements

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define material properties for interface elements, which may be used to simulate the onset or progress of delamination, and to associate these material properties with a list of element numbers. The cohesive material is defined using the cohesive energy (also called critical energy release rate), which equals the area below the equivalent traction versus equivalent relative displacement curve. The shape of this curve can be bilinear, exponential, or combined linear-exponential. Mixed mode delamination is incorporated by converting the normal and shear components of the relative displacements into an equivalent relative displacement. The data entered basically refers to the behavior in the normal direction and differences between the behavior in normal and shear direction can be defined using the shear-normal ratios for the maximum stress and the cohesive energy. As an alternative to the standard bilinear, exponential or linear-exponential model, the user can also use this option to trigger the call to the UCOHESIVE user subroutine. Format Format FixeD

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word COHESIVE.

2nd data block 1-5

1st

I

Enter the number of sets of cohesive material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

11-15

3rd

I

Enter 1

if extra data blocks 6 and 7 are used. This entry will be used for all sets of cohesive material data defined below. Default is 0, which means that the extra data blocks 6 and 7 are not used.

Data blocks 3 through 6 are repeated as a set, once for each set of cohesive material defined. 3rd data block 1-5

1st

I

6-10

2nd

I

Material identification number. Enter 1 for the bilinear model (default). Enter 2 for the exponential model. Enter 3 for the combined linear-exponential model.

Main Index

COHESIVE (with TABLE Input) 891 Define Material Data for Interface Elements

Format FixeD

Free

Data Entry Entry Enter -1 to define the cohesive material model via the UCOHESIVE user subroutine

11-15

3rd

I

Enter 1

to deactivate the associated elements if the maximum damage in all the element integration points has been reached. The deactivated elements will remain on the post file.

Enter 2 to deactivate the associated elements if the maximum damage in all the element integration points has been reached. Upon deactivation, the elements are removed from the post file. Default is 0, which implies that the elements will remain active irrespective of the damage level. 16-20

4th

I

Enter 0 (default) if a secant matrix. Enter 1 if a modified tangent matrix has to be used in the global NewtonRaphson iterative procedure. If the modified tangent matrix is selected, one may need to force the solution of a nonpositive definite system via the CONTROL option.

21-32

5th

A

Material name.

4th data block The data entered in the following block are the reference values that are used with tables or are constants. 1-10

1st

F

Cohesive energy.

11-20

2nd

F

Critical opening displacement.

21-30

3rd

F

Maximum opening displacement (linear model only).

31-40

4th

F

Shear-normastress ratio (the ratio of the maximum stress in shear and the maximum stress in tension). Default value is 1.

41-50

5th

F

Exponential decay factor (combined linear-exponential model only). Default value is 1.

51-60

6th

F

Factor for viscous energy dissipation. Default is 0, which implies that there is no viscous energy dissipation.

61-70

7th

F

Reference rate of relative displacement. This is only used if viscous energy dissipation is activated using the 6th field of this data block. Default is 0, which implies that the reference rate will automatically be calculated.

71-80

8th

F

Stiffening factor in compression. Default value is 1.

5th data block

Main Index

1-5

1st

I

Table ID for the cohesive energy. The cohesive energy can be a function of the first five state variables.

6-10

2nd

I

Not used; enter 0.

892 COHESIVE (with TABLE Input) Define Material Data for Interface Elements

Format FixeD

Free

Data Entry Entry

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Not used; enter 0.

Data blocks 6 and 7 are only needed if the third field of the 2nd data block is set to 1. 6th data block 1-10

1st

F

Shear-normal energy ratio (the ratio of the cohesive energy in shear and the cohesive energy in tension). Default value is 1.

I

Not used; enter 0.

7th data block 1-5

1st

8th data block Enter a list of elements associated with this material.

Main Index

COHESIVE 893 Define Mechanical Data for Cohesive Materials

COHESIVE

Define Mechanical Data for Cohesive Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define material properties for interface elements, which may be used to simulate the onset or progress of delamination, and to associate these material properties with a list of element numbers. The cohesive material is defined using the cohesive energy (also called critical energy release rate), which equals the area below the equivalent traction versus equivalent relative displacement curve. The shape of this curve can be bilinear, exponential, or combined linear-exponential. Mixed mode delamination is incorporated by converting the normal and shear components of the relative displacements into an equivalent relative displacement. The data entered basically refers to the behavior in the normal direction and differences between the behavior in normal and shear direction can be defined using the shear-normal ratios for the maximum stress and the cohesive energy As an alternative to the standard linear, exponential, or linear-exponential model, the user can also utilize this option to trigger the call to the UCOHESIVE user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word COHESIVE.

2nd data block 1-5

1st

I

Enter the number of sets of cohesive material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

11-15

3rd

I

Enter 1

if an extra data block 5 is used. This entry will be used for all sets of cohesive material data defined below. Default is 0, which means that the extra data blocks 5 is not used.

Data blocks 3 through 6 are repeated as a set, once for each set of cohesive material defined. 3rd data block 1-5

1st

I

6-10

2nd

I

Material identification number. Enter 1 for the bilinear model (default). Enter 2 for the exponential model. Enter 3 for the combined linear-exponential model.

Main Index

894 COHESIVE Define Mechanical Data for Cohesive Materials

Format Fixed

Free

Data Entry Entry Enter -1 to define the cohesive material model via the UCOHESIVE user subroutine.

11-15

3rd

I

Enter 1

to deactivate the associated elements if the maximum damage in all the element integration points has been reached. Upon deactivation, the elements will remain on the post file.

Enter 2

to deactivate the associated elements if the maximum damage in all the element integration points has been reached. Upon deactivation, the elements will be removed from the post file. Default is 0, which implies that the elements will remain active irrespective of the damage level.

16-20

21-32

4th

5th

I

Enter 0

(default) if a secant matrix.

Enter 1

if a modified tangent matrix has to be used in the global Newton-Raphson iterative procedure. If the modified tangent matrix is selected, one may need to force the solution of a nonpositive definite system via the CONTROL option.

A

Material name.

4th data block 1-10

1st

F

Cohesive energy.

11-20

2nd

F

Critical opening displacement.

21-30

3rd

F

Maximum opening displacement (linear model only).

31-40

4th

F

Shear-normal stress ratio (the ratio of the maximum stress in shear and the maximum stress in tension). Default value is 1.

41-50

5th

F

Exponential decay factor (combined linear-exponential model only). Default value is 1.

51-60

6th

F

Factor for viscous energy dissipation. Default is 0, which implies that there is no viscous energy dissipation.

61-70

7th

F

Reference rate of relative displacement. This is only used if viscous energy dissipation is activated using the 6th field of this data block. Default is 0, which implies that the reference rate will automatically be calculated.

71-80

8th

F

Stiffening factor in compression. Default value is 1.

Data block 5 is only needed if the third field of the 2nd data block is set to 1.

Main Index

COHESIVE 895 Define Mechanical Data for Cohesive Materials

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

Shear-normal energy ratio (the ratio of the cohesive energy in shear and the cohesive energy in tension). Default value is 1.

6th data block Enter a list of elements associated with this material.

Main Index

896 PSHELL Shell Element Property

PSHELL

Shell Element Property

Description This option allows you to define the membrane, bending, transverse shear, and coupling properties of the shell elements independently. This option supports isotropic linear elastic material and anisotropic linear elastic materials. Use of PSHELL for nonlinear analysis is not recommended. If MID1 = 0

membrane or membrane-bending coupling stiffness does not occur.

If MID2 = 0

bending, membrane-bending coupling, or transverse shear stiffness does not occur.

If MID3 = 0

transverse shear flexibility does not occur.

If MID4 = 0

membrane-bending coupling does not occur. This is true in normal cases. However, MID4 is not zero if there is an offset of shell middle surface and/or if the material distribution is not symmetric along the thickness.

Shell made of homogeneous materials can be modeled with PSHELL option by simply setting MID1=MID2=MID3, and MID4=0 if there is no offset of shell middle surface. However, for homogeneous shell structures, it is more efficient to use the standard shell technique, which is relatively easy and inexpensive, generally more accurate, capable to deal with advanced materials. PSHELL is based on the classical lamination theory (also known as equivalent stiffness method, see Marc Volume A: Theory and User Information for details). It is useful for shell structures with layered composite

materials, and gets particularly attractive when the number of composite layers becomes large. By using the option the shell structures contain only one layer with smeared material properties. It is more efficient because analysis of such smeared shell structures uses less computer time and storage space. The smeared material properties are defined as

∫ G dz

h G1 = h2 G4 =

∫ ( – z ) G dz

IG 2 =

∫ z 2 G dz

where

G

is the real material tangent connecting stress and strain tensors; h is the shell thickness; and G 4 are the smeared material tangent matrices defined by MID1, MID2, and MID4, respectively. The generalized stress-strain relations are then given as I = h 3 ⁄ 12 ; G 1 , G 2 ,

⎧ f ⎫ ⎨ ⎬ = ⎩ m ⎭

h G1 h2 G4 ⎧ ε ⎫ ⎨ ⎬ h2 G4 I G2 ⎩ χ ⎭

where f , m , ε , and χ are the membrane and transverse shear forces, the bending moments, strains on the middle surface of the shell, and curvatures, respectively.

Main Index

PSHELL 897 Shell Element Property

in Marc contains both membrane and transverse shear parts. Unless users want to adjust transverse shear stiffness, there is no need to define a new type of materials for it. Set MID3=MID1 to take into account the transverse shear stiffness. Otherwise, set MID3=0. G1

Generally G 1 , G 2 and G 4 can be described by ANISOTROPIC option. However, the tangent matrix defined with ANISOTROPIC is a 6 x 6 matrix for fully 3D cases. The G 1 , G 2 , and G 4 calculated here are 5 x 5 matrices because the third stress component normal to the shell surfaces is zero. Marc requires that all components in the third row and the third column of the 6 x 6 matrix defined in ANISOTROPIC option are entered as zero if the material is used with PSHELL option. In a transient analysis, the structural mass is calculated from the density using the membrane thickness and membrane material properties. If MID1 = 0, then the density is obtained from the MID2 materials. To take into account the effect of thermal expansion, the coefficients of thermal expansion defined by MID1 and MID2 are used. Transverse shear and membrane-bending coupling are not affected. Please note that, if either MID1, MID2, or MID3 is zero, some of diagonal terms in the tangent matrix will be zero. This results in singular stiffness matrix. In this case, the program will automatically fill a small nonzero numbers in these diagonal terms to overcome the problem. PSHELL assumes the constant transverse shear strain distribution through the thickness. Therefore, any input with TSHEAR parameter is ignored for the elements using PSHELL option.

In order to take into account the effect of thermal expansion, the temperature and the gradient of temperature need to be defined. Temperature in Marc is automatically stored as the first state variable. The state variable number used to store temperature gradient is defined in the 3rd data field of the 2nd data block. See the STATE VARS parameter, and the INITIAL STATE and CHANGE STATE options for details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PSHELL.

2nd data block

Main Index

1-5

1st

I

Number of data sets to be read in.

6-10

2nd

I

Unit number for input; defaults to standard input (unit 5).

11-15

3rd

I

State variable number used to store the gradient of temperature through the shell thickness. Must be greater than 1. Otherwise, the temperature gradient is zero.

898 PSHELL Shell Element Property

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

PSHELL property identification number

6-10

2nd

I

MID1

– Material identification number for membrane

11-20

3rd

F

T

– Membrane thickness. Default is the thickness defined using GEOMETRY option

21-25

4th

I

MID2

– Material identification number for bending

26-35

5th

F

12I/T**3 – Ratio of the actual bending moment of inertia of the shell (I) to the bending moment of inertia of a homogeneous shell (T**3/12). The default is 1.0.

36-40

6th

I

MID3

– Material identification number for transverse shear

41-50

7th

F

TS/T

– Ratio of transverse shear thickness TS to membrane thickness of the shell (T). The default is 0.833333.

51-55

8th

I

MID4

– Material identification number for membrane-bending coupling.

56-65

9th

F

Nonstructural mass per unit area.

66-75

10th

F

Fiber distance for stress calculation. Default is on the middle surface.

4th data block Enter a list of elements using this set of PSHELL data.

Main Index

REBAR 899 Define Rebar Positions, Areas, and Orientations

REBAR

Define Rebar Positions, Areas, and Orientations

Description This option defines the rebar positions, areas, and orientations. It can be used with the REBAR user subroutine which allows more general rebar definitions at element integration point level. Any nonzero value defined by the REBAR user subroutine overwrites the corresponding values defined this REBAR option. Rebar Layer Concept

Cord-reinforced composites are characterized by a group of reinforcing cords with arbitrary spatial orientations embedded in various matrix materials. The different constituents may have different mechanical properties. Two typical examples of the cord-reinforces composites are tires and cordreinforced concretes. In modeling such materials, the rebar technique is very useful. The basic idea of rebar layer concept contains that (1) the reinforcing cords and the matrix materials of the composites are represented independently by different types of elements along with different constitutive models, (2) the reinforcing cords within the elements modeling these cords (the so-called rebar elements) are assumed to be in the form of layers, and (3) the rebar elements are then embedded into the matrix elements. The compatibility between the cord elements and the matrix elements is enforced by either of the following two options. 1. Superimposing solid rebar elements on corresponding solid matrix elements using the same element connectivity. A list of solid rebar elements is available (see element types 23, 46, 47, 48, 142, 143, 144, 145, and 146). They are empty 4- or 8-node quadrilaterals (2-D) and 4- or 8-node hexahedrons (3-D). You can place reinforcing cord layers within the elements. Each solid rebar element is then superimposed on a solid matrix element. The two elements share the same space with the same element connectivity (therefore, the same element nodes). The compatibility condition between the reinforcements and the matrix materials is then automatically enforced. 2. Embed membrane rebar elements into solid matrix elements using the INSERT option. A list of membrane rebar elements is available (see element types 147, 148, 165, 166, 167, 168, 169, and 170). They are empty 2- or 3-node line elements (2-D) and 4- or 8-node quadrilaterals (3-D). You can place reinforcing cord layers within these empty elements. These elements are then embedded into their corresponding solid elements representing the matrix materials. Independent meshes can be used for the rebar membrane elements and the matrix elements. The INSERT option is used to enforce the compatibility between two different meshes (see the INSERT model definition option in this manual for details). To model a single reinforcing member, truss elements (for example, element types 9, 51, and 65) can be used with the INSERT option. Option 1 does not introduce additional degrees of freedom because the rebar element shares the same nodes as that of the corresponding matrix element.

Main Index

900 REBAR Define Rebar Positions, Areas, and Orientations

Option 2 may increase the node numbers because of the independent mesh of rebar membrane elements. Though the degrees of freedom of these extra nodes are constrained by the INSERT option, it may still be somewhat more expensive because the INSERT option can increase the bandwidth of the solution matrix. The advantage of Option 2 is that it provides more flexibility in defining arbitrary rebar orientations and in rebar element visualization. Rebar Property Definition

For solid rebar element types (see element types 23, 46, 47, 48, 142, 143, 144, 145, and 146), Figure 3-1 illustrates a single rebar layer within an element. The shape of the rebar layer and its position within the element can be defined by the Rebar Orientation Type of they layer and by the relative position of the layer along the relevant element edges in thickness direction. For membrane rebar element types (see element types 147, 148, 165, 166, 167, 168, 169, and 170), the shape of a rebar layer and its spatial position are the same as those of the element containing the layer. No input on the Rebar Orientation Type or on the relative position of the layer is needed. The maximum number of reinforcing cord layers within a rebar element is 5. By adding more rebar elements in the same spatial location with the same element connectivity, this limit can be extended to a larger number. For each rebar layer, the user is required to define cord material identification number, cross section area of the cords, density of the cords, and an angle α (defining spatial orientation of the cords). α is the angle between the cord and the projection of a predefined reference axis on the rebar layer plane. See Figure 3-2 for a description of the rebar angle of a single rebar layer. A check list of the rebar properties generally required follows: 1. Material identification number. 2. Cross-section of the reinforcing cords. 3. Density of the reinforcing cords. 4. Angle between the cord and the projection of a predefined reference axis on the rebar layer plane. 5. Rebar Orientation Type (not needed for rebar membrane elements). 6. Relative position of the cord layer within the element (not needed for rebar membrane elements). If the properties from items 2 to 6 do not change on the layer, only one set of properties are required. Otherwise, set the 7th field of the 3rd data block to 2 for 2-D or 3 for 3-D and define these properties at all relevant edges (or at corner nodes for rebar membrane elements. See Figure 3-1 for edge definition of solid rebar elements. In many cases, reinforcing cords can only support tensile force. That is the so-called “micro-buckling” behavior of cords. Consideration of the behavior can be activated by entering a 1 in the 8th field of the 3rd data block. Factor to reduce rebar compression stiffness is defined in the 9th field of the 3rd data block.

Main Index

REBAR 901 Define Rebar Positions, Areas, and Orientations

2-D

Edge 2 4

3

4

3

2 1

2

Edge 1 Edge 2

1 1

2 1

Rebar Orientation Type 1

2 Edge 1

Rebar Orientation Type 2

3-D Edge 1

Edge 3

5

8

2

3 1

4

1

Edge 3

2

7

6

3

1 4

8

Edge 4 Edge 4

7

6 Edge 2

5

2

1

2

3

3

Rebar Orientation Type 2

5 Edge 3

Edge 2 7

6

4

8

2

Edge 1

1

1

4

3 2

3 Edge 4

Rebar Orientation Type 3

Main Index

4

Edge 1

Rebar Orientation Type 1

Figure 3-19

4

Description of a Single Rebar Layer Within an Element

Edge 2

902 REBAR Define Rebar Positions, Areas, and Orientations

Direction Normal to the Rebar Layer

Reference Axis Rebar Direction

α z

-α Projection of Reference Axis onto Rebar Layer Plane

y x

Figure 3-20

Description of Rebar Orientation on a Single Rebar Layer

Rebar Pre- and Postprocessing

Marc creates a file named jid_rebar.mfd for rebar layer verification purposes if a 1 is entered in the 3rd field of the 2nd data block. All rebar layers and their orientations can be seen with the Marc Mentat graphic user interface. Directly plotting rebar results with the Marc Mentat graphic user interface can be confusing as there could be multiple rebar layers within one element and different layers could have different spatial orientations. It is recommended to use post codes 471 and 481 (see the POST model definition option for a more detailed description) to output the stress tensors of specific rebar layers into the post file. In the 2nd field of the 3rd data block of the POST option is the global layer identification number which is defined by the REBAR option in the 7th field of the 4th data block. The stress and the direction of rebar can be viewed using the tensor plot option in the Marc Mentat graphic user interface to process the principal values and directions of the rebar stress tensor. The only nonzero principal stress of the stress tensor is the value of the rebar stress on the specific layer. The corresponding principal direction is the rebar direction. Both the principal value and direction are averaged within an element. The angle α between rebar and the project of reference axis on rebar layer plane ( – 90 ≤ α ≤ 90 ) , defined at the 5th field of the 4th data block, changes with the deformation. This angle can be postprocessed with post code 487.

Main Index

REBAR 903 Define Rebar Positions, Areas, and Orientations

Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word REBAR.

2nd data block 1-5

1st

I

Number of data sets to be read in.

6-10

2nd

I

Unit number for input; defaults to standard input (unit 5).

11-15

3rd

I

Enter 1

to create a file named jid_rebar.mfd for rebar layer verification purposes.

Data blocks 3, 4, and 5 are given for each data set. 3rd data block 1-5

1st

I

Rebar data set ID.

6-10

2nd

I

Number of rebar layers to be read in. Maximum is 5.

11-15

3rd

I

Enter 2

if the considered structure is an axisymmetric expansion of cylinders made of bias plies and the cords are nearly inextensible relative to matrix materials. In this case, all parameters below describe the cylinders from which the considered structure was made. The rebar positions, areas, and orientations for real structure is calculated by Marc. When using cylinder expansion option in rebar data definition, the reference axis needs to be the symmetric axis of the original cylinder, and this needs to pass through the origin of the coordinates.

Enter 3

In a 3-D axisymmetric structure with the x-axis (1,0,0) as the asixymmetric axis and the reference axis, if the rebar layer is vertical to (1,0,0), the program internally switches the reference axis to (0,1,0).

16-25

4th

F

First direction cosine of reference axis.

26-35

5th

F

Second direction cosine of reference axis.

36-45

6th

F

Third direction cosine of reference axis. The default reference axis is (1, 0, 0). Notes:

Reference axis should not be perpendicular to rebar layer. If AXITO3D option is used, the reference axis must be (1,0,0). If the rebar layer is vertical to (1,0,0), the program internally switches the reference axis to (0,1,0).

46-50

Main Index

7th

I

Enter 0 (default) if no skew type of rebar layers are to be defined.

904 REBAR Define Rebar Positions, Areas, and Orientations

Format Fixed

Free

Data Entry Entry Enter 2

for 2-D and for 2-D membrane elements (types 165 - 167).

Enter 3

for 3-D and for 3-D membrane elements (types 147 and 148). Set to 0 if the third field of the third data block is 2. to activate the so-called “micro-buckling” behavior of rebar cords in compression.

51-55

8th

I

Enter 1

56-65

9th

F

Factor used to reduce rebar stiffness in compression. Used only if a 1 is entered in the 8th field of the data block. The default if 0.02.

Data block 4 is given for each rebar layer. 4th data block 1-5

1st

I

Material ID.

6-15

2nd

F

p⋅r ----------- , relative position of the rebar layer at edge 1 (ratio of the distance T

between the reference surface (edge) and the rebar layer to the distance across the element); not used for membrane elements. 16-25

3rd

F

A, area of cross section of each rebar at edge 1.

26-35

4th

F

S, number of rebars per unit length in each layer at edge 1. Equivalent thickness of the rebar layer is A ⋅ S .

36-45

5th

F

Angle (α) between the rebar and the projection of the reference axis on rebar layer plane [-90, 90] at edge 1. See Figure 3-2.

46-55

6th

F

Radius of the cylinder; only used when the third field of the 3rd data block is 2.

56-60

7th

I

Enter the global identification number of the rebar layer. Use for postprocessing only.

61-65

8th

I

Enter the rebar layer orientation type. Not used for membrane elements. 2-D

Main Index

Enter 1

if this rebar layer is similar to the 1,2 and 3,4 edges of the element; the “thickness” direction is from the 1,2 edge to 3,4 edge of the element.

Enter 2

if this rebar layer is similar to the 1,4 and 2,3 edges of the element; the “thickness” direction is from the 1,4 edge to 2,3 edge of the element.

REBAR 905 Define Rebar Positions, Areas, and Orientations

Format Fixed

Free

Data Entry Entry 3-D Enter 1

if this rebar layer is similar to the 1,2,3,4 and 5,6,7,8 faces of the element; the “thickness” direction is from the 1,2,3,4 face to 5,6,7,8 face of the element.

Enter 2

if this rebar layer is similar to the 1,4,8,5 and 2,3,7,6 faces of the element; the “thickness” direction is from the 1,4,8,5 face to 2,3,7,6 face of the element.

Enter 3

if this rebar layer is similar to the 2,1,5,6 and 3,4,8,7 faces of the element, the “thickness” direction is from the 2,1,5,6 face to 3,4,8,7 face of the element.

5th data block is only needed when the 7th field of the third data block is not zero. 5th data block 1-10

1st

F

Relative position of the rebar layer at edge 2. Not used for membrane elements.

11-20

2nd

F

Area of cross-section of rebar at edge 2.

21-30

3rd

F

Number of rebars per unit length at edge 2.

31-40

4th

F

Angle between the rebar and the projection of the reference axis on rebar layer plane (-90,90) at edge 2.

6th and 7th data blocks are only needed when the 7th field of the third data block is 3. 6th data block 1-10

1st

F

Relative position of the rebar layer at edge 3. Not used for membrane elements.

11-20

2nd

F

Area of cross-section of rebar at edge 3.

21-30

3rd

F

Number of rebars per unit length at edge 3.

31-40

4th

F

Angle between the rebar and the projection of the reference axis on rebar layer plane (-90,90) at edge 3.

7th data block 1-10

1st

F

Relative position of the rebar layer at edge 4. Not used for membrane elements.

11-20

2nd

F

Area of cross-section of rebar at edge 4.

21-30

3rd

F

Number of rebars per unit length at edge 4.

31-40

4th

F

Angle between the rebar and the projection of the reference axis on rebar layer plane (-90,90) at edge 4.

8th data block Enter a list of elements.

Main Index

906 ORIENTATION Define Orientation of Elements

ORIENTATION

Define Orientation of Elements

Description The ORIENTATION option is used to specify orientation angle data as follows: 1. Edge orientation types (EDGE i-j). For two-dimensional elements (both continuum and shells), you choose a particular element edge with respect to which the preferred coordinates are specified. With these types, the direction vector along the edge from the first to the second edge node is projected onto the surface tangent plane (xy plane if continuum, or each integration point.

˜1˜2 V V

plane if shell) at

The first preferred direction is given by a rotation about the surface normal (z axis if continuum, ˜3 V

axis if shell) equal to the orientation angle. The third preferred direction is given by the surface normal, and the second preferred direction is given by a cross product of the third and first directions. See Figure 3-21. 2. Global intersecting plane types (ij PLANE). These types are also for two-dimensional elements. Here, a particular global coordinate plane (selected by the orientation type) is intersected with the surface tangent plane. The first preferred direction is given by a rotation about the surface normal from this intersection by an amount equal to the orientation angle. The third preferred direction is given by the surface normal and the second direction by a cross product of the third and first. See Figure 3-22. 3. User-defined intersecting plane. These types are also for two-dimensional elements. Here, a plane, defined by you, with one coordinate direction and a user-defined vector or by two userdefined vectors is intersected with the surface tangent plane. The first preferred direction is given by a rotation about the surface normal from this intersection by an amount equal to the orientation angle. The third preferred direction is given by the surface normal and the second direction by a cross product of the third and first. SeeFigure 3-23. 4. Three-dimensional orientation types (3D ANISO). For three-dimensional elements, you directly enter vectors in the first and second preferred directions. The third preferred direction is given by a cross product of the first and second direction. If a nonzero orientation angle is defined, the first and the second preferred directions are given by a rotation of the two corresponding user vectors about the third direction. SeeFigure 3-24. 5. UORIENT orientation type. Here, you define the transformation matrix between global coordinates (if continuum elements) or local coordinates (if beams, plates or shells) directly in the ORIENT user subroutine. 6. Three-dimensional local orientation (3D LOCAL). For hexahedral elements, a local element system is used. This system can be rotated around the three local axes. The local system is defined as follows. See Figure 3-25. The first preferred direction joins the centroids of faces 4-1-5-8 and 3-2-6-7. A second vector joins faces 1-2-6-5 and 4-3-7-8. The third preferred direction is given by the cross product of the first preferred direction and this vector. The second preferred direction is given by the cross product of the third and first preferred directions. This system is then rotated around the three local axes by the three given angles.

Main Index

ORIENTATION 907 Define Orientation of Elements

7. Closest point on curve (CURVE). One or more NURBS curves are used for defining the preferred system. A list of curves are given as input. These curves must be defined with the CURVES model definition option and only the NURBS variant is allowed. Using the centroid of the element, the closest point on any of the given curves is found. The first preferred direction is given by the tangent vector at this point. For 2-D elements, the second preferred direction is given by the cross product of the global z direction and the first preferred direction. For 3-D elements, this option is only supported for solid shell elements and solid composite elements. The third preferred direction is given by the thickness direction and the second preferred direction by the cross product between the third and first preferred direction. The first preferred direction is recalculated as the cross product between the second and third preferred directions to insure that we have an orthogonal system. Notes:

The ORIENTATION option is ignored for 1-D elements, gaps, pipe bend, shear panel and cable elements. The ORIENTATION option is ignored for 2-D continuum composite element types 151-154. The preferred material orientation is obtained by rotating the element local coordinates on an orientation angle about the direction normal to material layers. See the COMPOSITE model definition option and Marc Volume B: Element Library for details. The ORIENTATION option is turned on for composite elements. If no ORIENTATION data is given for these elements, the default is no preferred orientation; that is, the default material orientation of the element. The ORIENTATION option, UORIENT, is turned on for particular material numbers if the IANELS flag is set during data input (see ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, MOONEY and HYPOELASTIC options). You can override this default by entering your own ORIENTATION option. When visualizing the results, one can request that the generalized stresses and strains are in either the element system or the preferred material coordinate system defined here.

Main Index

908 ORIENTATION Define Orientation of Elements

n = Normal to surface tangent plane Node I

Integration point Ω

α

Node J Direction 1 of preferred coordinate system

Z Element surface

Y X

Figure 3-21

Main Index

Edge I-J Orientation Type

Ω = Orientation angle (positive right-hand rotation about n) α = Ply angle (if COMPOSITE)

ORIENTATION 909 Define Orientation of Elements

n - Normal to surface tangent plane

Global ZX plane

Surface tangent plane Ω

α

Direction 1 of preferred coordinate system

Intersection of two planes Z

Y X

Figure 3-22

Main Index

ZX Plane Orientation Type

Element surface

Ω = orientation angle (positive right-hand rotation about n) α = ply angle (if COMPOSITE)

910 ORIENTATION Define Orientation of Elements

n = Normal to surface tangent plane

u = User-defined vector

Surface tangent plane Ω global X

α Direction 1 of preferred coordinate system

Element surface Z

Y X

Figure 3-23

Main Index

W = Orientation angle (positive right-hand rotation about n) α = ply angle (if COMPOSITE)

XU Plane Orientation Type

ORIENTATION 911 Define Orientation of Elements

Direction 2 of preferred coordinate system U2 = User vector 2

Ω

U3 = U1 x U2

Ω

Direction 1 of preferred coordinate system

Z

U1 = User vector 1 Y Ω = Orientation angle X

Figure 3-24

Three-dimensional ANISO Orientation Type

8 7 5

6

4

3

1

2

Figure 3-25

Main Index

3D LOCAL Orientation Type

912 ORIENTATION Define Orientation of Elements

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORIENTATION.

2nd data block 1-5

1st

I

Enter the number of orientation angle data sets to follow.

6-10

2nd

I

Unit number for input. Defaults to input file.

The 3rd and 4th data blocks are entered as pairs, once for each angle data set. 3rd data block 1-10

1st

A

Enter one of the following to specify orientation angle type. EDGE 1-2 EDGE 2-3 EDGE 3-4 EDGE 3-1 EDGE 4-1 XY PLANE YZ PLANE ZX PLANE XU PLANE YU PLANE ZU PLANE UU PLANE UORIENT 3D ANISO COORD SYS 3D LOCAL CURVE

11-20

2nd

F

Orientation angle.

For EDGE style orientations:

Main Index

21-30

3rd

F

First component of user vector 1 in global coordinates.

31-40

4th

F

Second component of user vector 1 in global coordinates.

41-50

5th

F

Third component of user vector 1 in global coordinates.

ORIENTATION 913 Define Orientation of Elements

Format Fixed

Free

Data Entry Entry

51-60

3rd

F

First component of user vector 2 in global coordinates.

61-70

4th

F

Second component of user vector 2 in global coordinates.

71-80

5th

F

Third component of user vector 2 in global coordinates.

For XU PLANE, YU PLANE, ZU PLANE, UU PLANE, and 3-D ANISO, complete the following: 21-30

1st

F

1

31-40

2nd

F

2

41-50

3rd

F

3

component of user vector 1 with respect to global coordinates.

For UU PLANE and 3-D ANISO, complete the following: 51-60

4th

F

1

61-70

5th

F

2

71-80

6th

F

3

component of user vector 2 with respect to global coordinates.

For COORD SYS style orientation: 21-25

3rd

I

Enter the coordinate system ID from COORD SYSTEM option.

For 3D LOCAL, complete the following: 21-30

3rd

F

Rotation around local x axis

31-40

4th

F

Rotation around local y axis

41-50

5th

F

Rotation around local z axis

For CURVE, complete the following: 21-25

3rd

I

Enter 1 to flip the orientation of the curves.

3a data block Enter a list of curves. Only for CURVE option. 4th data block Enter a list of elements to be associated with this orientation angle.

Main Index

914 POWDER (with TABLE input) Define Powder Material Model

POWDER (with TABLE input)

Define Powder Material Model

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to input data associated with Marc’s powder material model. The material parameters can be entered here or through the UPOWDR user subroutine. The influences of temperature and relative density are entered through the TABLE option. The data entered here is at the beginning of the analysis; for example, at the temperatures given through the INITIAL STATE option and the relative density given through the RELATIVE DENSITY option. The yield function for powder material is: 1 3 p2 1 / 2 F = --- ⎛ --- S i j S i j + -----2⎞ – σy γ ⎝2 β ⎠

where s is the deviatoric stresses and p is the hydrostatic stress. γ and β are material properties which can be expressed as: b

b4

q

q4

β = ( b1 + b2 ρ 3 ) γ = ( q1 + q2 ρ 3 )

where ρ is the relative density. This data is entered through this option. Additional details can be found in Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word POWDER.

2nd data block 1-5

1st

I

Enter the number of sets of powder material data to be defined (optional).

6-10

2nd

I

Enter the logical unit number for data input. Defaults to input data file.

Data blocks 3 through 10 are entered as a set, once for each data associated with this material definition.

Main Index

POWDER (with TABLE input) 915 Define Powder Material Model

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Not used.

11-15

3rd

I

Not used.

16-20

4th

I

Not used.

21-32

5th

A

Enter the material name.

4th data block 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Mass density

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Compressive yield stress.

51-60

6th

F

Gamma (γ ).

61-70

7th

F

Beta ( β ).

71-80

8th

F

Viscosity.

5th data block 1-5

1st

I

Enter table ID for Young’s modulus.

6-10

2nd

I

Enter table ID for Poisson’s ratio.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Enter table ID for coefficient of thermal expansion.

21-25

5th

I

Enter table ID for compressive yield stress.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter table ID for viscosity.

6th data block The 5th data block is only required in a coupled thermal-stress analysis.

Main Index

1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

916 POWDER (with TABLE input) Define Powder Material Model

Format Fixed

Free

Data Entry Entry

7th data block The 7th data block is only required in a coupled thermal-stress analysis. 1-5

1st

I

Enter table ID for thermal conductivity.

6-10

2nd

I

Enter table ID for specific heat.

11-15

3rd

I

Enter table ID for mass density.

8th data block 1-10

1st

F

q1

11-20

2nd

F

q2

21-30

3rd

F

q3

31-40

4th

F

q4

9th data block 1-10

1st

F

b1

11-20

2nd

F

b2

21-30

3rd

F

b3

31-40

4th

F

b4

10th data block Enter a list of elements to be associated with this material definition.

Main Index

POWDER 917 Define Powder Material Model

POWDER

Define Powder Material Model

The information provided here is based upon not using the table driven input style. Description This option allows you to input data associated with Marc’s powder material model. The material parameters can be entered here or through the UPOWDR user subroutine. The influences of temperature and relative density are entered through the TEMPERATURE EFFECTS and DENSITY EFFECTS options. The data entered here is at the beginning of the analysis; for example, at the temperatures given through the INITIAL STATE option and the relative density given through the RELATIVE DENSITY option. The yield function for powder material is: 1 3 p2 1 / 2 F = --- ⎛ --- S i j S i j + -----2⎞ – σy γ ⎝2 β ⎠

where s is the deviatoric stresses and p is the hydrostatic stress. γ and β are material properties which can be expressed as: b

b4

q

q4

β = ( b1 + b 2 ρ 3 ) γ = ( q1 + q2 ρ 3)

where ρ is the relative density. This data is entered through this option. Additional details can be found in Marc Volume A: Theory and User Information.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word POWDER.

2nd data block 1-5

1st

I

Enter the number of sets of powder material data to be defined (optional).

6-10

2nd

I

Enter the logical unit number for data input. Defaults to input data file.

Data blocks 3, 4, 5, 6, 7, and 8 are entered as a set, once for each data associated with this material definition.

Main Index

918 POWDER Define Powder Material Model

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Material identification number.

6-10

2nd

I

Not used.

11-15

3rd

I

Not used.

16-20

4th

I

Not used.

21-32

5th

A

Enter the material name.

4th data block 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Mass density.

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Compressive yield stress.

51-60

6th

F

Gamma (γ ).

61-70

7th

F

Beta ( β ).

71-80

8th

F

Viscosity.

5th data block The 5th data block is only required in a coupled thermal-stress analysis. 1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

6th data block 1-10

1st

F

q1

11-20

2nd

F

q2

21-30

3rd

F

q3

31-40

4th

F

q4

7th data block

Main Index

1-10

1st

F

b1

11-20

2nd

F

b2

POWDER 919 Define Powder Material Model

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

b3

31-40

4th

F

b4

8th data block Enter a list of elements to be associated with this material definition.

Main Index

920 DENSITY EFFECTS Define Effects of Density on Powder Materials

DENSITY EFFECTS

Define Effects of Density on Powder Materials

The information provided here is based upon not using the table driven input style. If table driven input is used, the POWDER option should reference tables that provide temperature and density dependent behavior. Description This option defines the variation of powder material data with respect to the relative density. The base values are those read in through the POWDER option at the initial state. The data in this option is used in conjunction with the TEMPERATURE EFFECTS option to give bilinear variations in the material properties. The relative density can be entered using one of the following options: a. The variation of a particular property relative to its base value with respect to the relative density as a piecewise linear curve. Breakpoints must be given in ascending order of relative density. b. The particular value relative to its base value and with respect to the relative density lying on the relevant curve are input directly. Data points must be given in increasing order of relative density. This option is flagged by entering the word DATA on the first block. Note:

In this option, relative density is the density relative to the fully compacted density having the range (0-1). The relative Young’s modulus, Poisson’s ratio, relative conductivity, and relative specific heat are their respective values relative to those given on the POWDER option at the base temperature.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words DENSITY EFFECTS.

16-80

2nd

A

Enter the word DATA to indicate that option B is used.

OPTION A 2a data block

Main Index

1-5

1st

I

Number of slopes of relative Young’s modulus versus relative density curve.

6-10

2nd

I

Number of slopes of relative Poisson’s ratio versus relative density curve.

11-15

3rd

I

Number of slopes of relative Conductivity versus relative density curve (coupled analysis only).

DENSITY EFFECTS 921 Define Effects of Density on Powder Materials

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Number of slopes of relative Specific Heat versus relative density curve (coupled analysis only).

21-25

5th

I

Material type identification number for cross-reference with POWDER model definition option.

3a data block The number entered in the first field of data block 2a defines the number of blocks required in data block 3a. 1-15

1st

F

Enter the slope of relative Young’s modulus versus the relative density curve.

16-30

2nd

F

Enter the relative density at which the above slope becomes operative.

4a data block The number in the second field of data block 2a defines the number of blocks required in data block 4a. 1-15

1st

F

Enter the slope of relative Poisson’s ratio versus the relative density curve.

16-30

2nd

F

Enter the relative density at which the above slope becomes operative.

5a data block The number in the third field of data block 2a defines the number of blocks required in data block 5a. 1-15

1st

F

Enter the slope of relative conductivity versus relative density.

16-30

2nd

F

Enter the relative density at which the above slope becomes operative.

6a data block The number in the fourth field of data block 2a defines the number of blocks required in data block 6a. 1-15

1st

F

Enter the slope of the relative specific heat versus relative density.

16-30

2nd

F

Relative density at which this slope becomes operative.

Option B 2b data block

Main Index

1-5

1st

I

Number of data points on relative Young’s modulus versus relative density curve.

6-10

2nd

I

Number of data points on relative Poisson ratio versus relative density curve.

11-15

3rd

I

Number of data points on relative Conductivity versus relative density curve (coupled analysis only).

16-20

4th

I

Number of data points on relative specific heat versus relative density curve (coupled analysis only).

21-25

5th

I

Material type identification number for cross-reference with POWDER model definition option.

922 DENSITY EFFECTS Define Effects of Density on Powder Materials

Format Fixed

Free

Data Entry Entry

3b data block The number in the first field of data block 2b defines the number of blocks required in data block 3b. 1-15

1st

F

Enter the value of the relative Young’s modulus.

16-30

2nd

F

Enter the associated relative density.

4b data block The number in the second field of data block 2b defines the number of blocks required in data block 4b. 1-15

1st

F

Enter the value of the relative Poisson’s ratio.

16-30

2nd

F

Enter the associated relative density.

5b data block The number in the third field of data block 2b defines the number of blocks required in data block 5b. 1-15

1st

F

Enter the value of the relative conductivity.

16-30

2nd

F

Enter the associated relative density.

6b data block The number in the fourth field of data block 2b defines the number of blocks required in data block 6b.

Main Index

1-15

1st

F

Enter the value of the relative specific heat.

16-30

2nd

F

Enter the associated relative density.

RELATIVE DENSITY 923 Define Initial Relative Density for Stress or Coupled Thermal Stress Analysis

RELATIVE DENSITY

Define Initial Relative Density for Stress or Coupled Thermal Stress Analysis

Description This option allows you to define initial relative density in a powder material analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words RELATIVE DENSITY.

2nd data block 1-5

1st

I

Enter the number of sets to be input with this option.

6-10

2nd

I

Enter the logical unit number of the data input. Defaults to input data file.

The 3rd, 4th and 5th data blocks are entered as pairs, once for each data set. 3rd data block 1-10

1st

F

Initial relative density.

4th data block Enter a list of elements to be associated with the above defined initial relative density. 5th data block Enter a list of integration points for which the defined initial relative density is used.

Main Index

924 SOIL (with TABLE Input) Define Material Properties for Soil Analysis

SOIL (with TABLE Input)

Define Material Properties for Soil Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define material data for soil analysis. It is assumed that the soil skeleton is composed of a collection of randomly oriented grains resulting in effectively isotropic or orthotropic behavior. You must define here both the material properties of the soil and the fluid. For additional details, see Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SOIL.

2nd data block 1-5

1st

I

Enter the number of sets of data used to define the soil data.

6-10

2nd

I

Enter the unit number of input of soil data. Defaults to input.

Data blocks 3 through 14 are entered as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing.

6-15

2nd

A

Enter one of the following soil models: ELASTIC

– linear elastic.

NON LINEAR

– nonlinear elastic via HYPELA2.

CAMCLAY

– Cam clay model.

VON MISES

– von Mises

LIN MOHRC

– Linear Mohr-Coulomb

PBL MOHRC

– Parabolic Mohr-Coulomb

ORTHOTROPIC – orthotropic elastic

Main Index

16-25

3rd

A

Not used.

26-30

4rd

I

Enter 1 if anisotropic linear elastic model is used. Material properties should be entered via the ANELAS or HOOKLW user subroutines.

31-35

5th

I

Not used; enter 0.

SOIL (with TABLE Input) 925 Define Material Properties for Soil Analysis

Format Fixed

Free

Data Entry Entry

36-40

6th

I

Not used; enter 0.

41-52

7th

A

Enter the material name.

The 4th through 7th data blocks are entered only if the second field of the third data block is not orthotropic. 4th data block 1-10

1st

F

Young’s modulus.

11-20

2nd

F

Poisson’s ratio.

21-30

3rd

F

Mass density.

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Yield strength. For Mohr-Coulomb behavior, this is at zero hydrostatic stress.

51-60

6th

F

For Mohr-Coulomb yield criteria,

61-70

7th

F

Bulk modulus of fluid.

71-80

8th

F

Dynamic viscosity of fluid.

α–β

parameter.

5th data block 1-5

1st

I

Table ID for Young’s modulus.

6-10

2nd

I

Table ID for Poisson’s ratio.

11-15

3rd

I

Table ID for mass density.

16-20

4th

I

Table ID for coefficient of thermal expansion.

21-25

5th

I

Table ID for yield strength.

26-30

6th

I

Table ID for Mohr-Coulomb yield criteria,

31-35

7th

I

Table ID for bulk modulus of fluid.

6th data block 1-10

1st

F

Permeability of the soil.

11-20

2nd

F

Virgin compression ratio.

21-30

3rd

F

Recompression ratio.

31-40

4th

F

Slope of critical state line.

7th data block

Main Index

1-5

1st

I

Table ID for permeability of the soil.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

α–β

parameter.

926 SOIL (with TABLE Input) Define Material Properties for Soil Analysis

Format Fixed

Free

Data Entry Entry

The 8th through 13th data blocks are entered only if the second field of the third data block is orthotropic. 8th data block 1-10

1st

F

E11 – Young’s modulus.

11-20

2nd

F

E22 – Young’s modulus.

21-30

3rd

F

E33 – Young’s modulus.

31-40

4th

F

ν12 – Poisson’s ratio.

41-50

5th

F

ν23 – Poisson’s ratio.

51-60

6th

F

ν31 – Poisson’s ratio.

61-70

7th

F

ρ

– Mass density (stress analysis).

9th data block 1-5

1st

I

Table ID for E11.

6-10

2nd

I

Table ID for E22.

11-15

3rd

I

Table ID for E33.

16-20

4th

I

Table ID for ν12.

21-25

5th

I

Table ID for ν23.

26-30

6th

I

Table ID for ν31.

31-35

7th

I

Table ID for mass density.

10th data block 1-10

1st

F

G12 – Shear modulus.

11-20

2nd

F

G23 – Shear modulus.

21-30

3rd

F

G31 – Shear modulus.

31-40

4th

F

α11 – Coefficients of thermal expansion.

41-50

5th

F

α22 – Coefficients of thermal expansion.

51-60

6th

F

α33 – Coefficients of thermal expansion.

11th data block

Main Index

1-5

1st

I

Table ID for G12.

6-10

2nd

I

Table ID for G23.

11-15

3rd

I

Table ID for G31.

SOIL (with TABLE Input) 927 Define Material Properties for Soil Analysis

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Table ID for α11.

21-25

5th

I

Table ID for α22.

26-30

6th

I

Table ID for α33.

12th data block 1-10

1st

F

K11 – Absolute permeability of the soil.

11-20

2nd

F

K22 – Absolute permeability of the soil.

21-30

3rd

F

K33 – Absolute permeability of the soil.

31-40

4th

F

μ

– Dynamic viscosity of fluid.

41-50

5th

F

ρf

– Fluid density.

51-60

6th

F

Kf – Bulk modulus of fluid.

13th data block 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for μ.

21-25

5th

I

Table ID for ρf.

26-30

6th

I

Table ID for Kf.

14th data block Enter a list of elements associated with this particular soil data.

Main Index

928 SOIL Define Material Properties for Soil Analysis

SOIL

Define Material Properties for Soil Analysis

The information provided here is based upon not using the table driven input style. Description This option allows you to define material data for soil analysis. It is assumed that the soil skeleton is composed of a collection of randomly oriented grains resulting in effectively isotropic behavior. You must define here both the material properties of the soil and the fluid. For additional details, see Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word SOIL.

2nd data block 1-5

1st

I

Enter the number of sets of data used to define the soil data.

6-10

2nd

I

Enter the unit number of input of soil data. Defaults to input.

Data blocks 3 through 9 are entered as a set, once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing.

6-15

2nd

A

Enter one of the following soil models: ELASTIC

– linear elastic.

NON LINEAR

– nonlinear elastic via HYPELA2.

CAMCLAY

– Cam clay model.

VON MISES

– von Mises.

LIN MOHRC

– Linear Mohr-Coulomb.

PLB MOHRC

– Parabolic Mohr-Coulomb.

ORTHOTROPIC – Orthotropic elastic.

Main Index

16-25

3rd

A

Not used; enter 0.

26-30

4th

I

Enter 1 if anisotropic linear elastic model is used. Material properties should be entered via the ANELAS or HOOKLW user subroutines.

31-35

5th

I

Not used; enter 0.

SOIL 929 Define Material Properties for Soil Analysis

Format Fixed

Free

Data Entry Entry

36-40

6th

I

Not used; enter 0.

41-52

7th

A

Enter the material name.

The 4th and 5th data blocks are entered only if the second field of the third data block is not orthotropic. 4th data block 1-10

1st

F

Young’s modulus of soil.

11-20

2nd

F

Poisson ratio of soil.

21-30

3rd

F

Mass density.

31-40

4th

F

Coefficient of thermal expansion.

41-50

5th

F

Yield strength. For Mohr-Coulomb behavior, this is at zero hydrostatic stress.

51-60

6th

F

For Mohr-Coulomb yield criteria,

61-70

7th

F

Bulk modulus of fluid.

71-80

8th

F

Dynamic viscosity of fluid.

α–β

parameter.

5th data block 1-10

1st

F

Permeability of the soil.

11-20

2nd

F

Virgin compression ratio.

21-30

3rd

F

Recompression ratio.

31-40

4th

F

Slope of critical state line.

The 6th, 7th, and 8th data blocks are entered only if the second field of the third data block is orthotropic. 6th data block 1-10

1st

F

E11 – Young’s modulus.

11-20

2nd

F

E22 – Young’s modulus.

21-30

3rd

F

E33 – Young’s modulus.

31-40

4th

F

ν12 – Poisson’s ratio.

41-50

5th

F

ν23 – Poisson’s ratio.

51-60

6th

F

ν31 – Poisson’s ratio.

61-70

7th

F

ρ

F

G12 – Shear modulus.

– Mass density (stress analysis).

7th data block 1-10

Main Index

1st

930 SOIL Define Material Properties for Soil Analysis

Format Fixed

Free

Data Entry Entry

11-20

2nd

F

G23 – Shear modulus.

21-30

3rd

F

G31 – Shear modulus.

31-40

4th

F

α11 – Coefficients of thermal expansion.

41-50

5th

F

α22 – Coefficients of thermal expansion.

51-60

6th

F

α33 – Coefficients of thermal expansion.

8th data block 1-10

1st

F

K11 – Absolute permeability of the soil.

11-20

2nd

F

K22 – Absolute permeability of the soil.

21-30

3rd

F

K33 – Absolute permeability of the soil.

31-40

4th

F

μ

41-50

5th

F

ρf – Fluid density.

51-60

6th

F

Kf – Bulk modulus of fluid.

– Dynamic viscosity of fluid.

9th data block Enter a list of elements associated with this particular soil data.

Main Index

INITIAL POROSITY (with TABLE input) 931 Define Initial Porosity

INITIAL POROSITY (with TABLE input)

Define Initial Porosity

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option provides the ability to define the initial porosity. The magnitude and location of the initial porosity is associated with an initial condition name. The LOADCASE model definition option is used to activate this data. For soil analysis, this will be changed during the analysis. For nonsoil analysis, the porosity is an independent (state) variable that may be used in tables. You can either specify the porosity or use the INITIAL VOID RATIO option to specify the void ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PR or INITIAL POROSITY.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the initial porosity.

6-10

2nd

I

Enter the unit number; defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter zero.

11-15

3rd

I

Not used; enter zero.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the initial porosity.

I

Enter the table ID associated with the initial porosity.

4th data block 1-10

1st

5th data block 1-5

Main Index

1st

932 INITIAL POROSITY (with TABLE input) Define Initial Porosity

Format Fixed

Free

Data Entry Entry

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. the geometric entities must all be of the type prescribed in the 6th data block.

INITIAL POROSITY 933 Define Initial Porosity

INITIAL POROSITY

Define Initial Porosity

The information provided here is based upon not using the table driven input style. Description This option provides the ability to initialize the porosity. For nonsoil analysis, the porosity is an independent (state) variable. You can either specify the porosity or use the INITIAL VOID RATIO option to specify the void ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PR or INITIAL POROSITY.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the initial porosity.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. 3rd data block 1-10

1st

F

Enter the initial porosity for the points given below at the start of increment zero.

4th data block Enter a list of elements to which the above porosity is to be applied. 5th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above porosity is to be applied. 6th data block This data block is necessary only when there are either beams or shells in the mesh. Enter a list of layer points to which the above porosity is to be applied.

Main Index

934 POROSITY CHANGE (with TABLE Input - Model Definition) Define Changes in Porosity for Nonsoil Analysis

Define Changes in Porosity for Nonsoil Analysis POROSITY CHANGE (with TABLE Input - Model Definition) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option provides the ability to define the material porosity in nonsoil model. The magnitude and location of the porosity is associated with a boundary condition name. The LOADCASE model definition option is used to activate this data. You can either specify the porosity or use the VOID CHANGE option to specify the void ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words POROSITY CHANGE.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the porosity.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the porosity.

4th data block 1-10

1st

5th data block

Main Index

POROSITY CHANGE (with TABLE Input - Model Definition) 935 Define Changes in Porosity for Nonsoil Analysis

Format Fixed 1-5

Free 1st

Data Entry Entry I

Enter the table ID associated with the porosity.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above porosity is applied. the geometric entities must all be of the type prescribed in the 6th data block.

936 INITIAL VOID RATIO (with TABLE Input) Define Initial Void Ratio for Soil or Diffusion Analysis

INITIAL VOID RATIO (with TABLE Input)

Define Initial Void Ratio for Soil or Diffusion Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option provides the ability to define the initial void ratio model. The magnitude and location of the initial void ratio is associated with an initial condition name. The LOADCASE model definition is used to activate this data. For soil analysis, the void ratio will change during the analysis. For nonsoil analysis, the void ratio is an independent (state) variable that may be used in tables. You can either specify the void ratio or use the INITIAL POROSITY option to specify the porosity. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL VOID.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the initial void ratio.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the initial void ratio.

4th data block 1-10

Main Index

1st

INITIAL VOID RATIO (with TABLE Input) 937 Define Initial Void Ratio for Soil or Diffusion Analysis

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Enter the table ID associated with the initial void ratio.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. the geometric entities must all be of the type prescribed in the 6th data block.

938 INITIAL VOID RATIO Define Initial Void Ratio for Soil or Diffusion Analysis

INITIAL VOID RATIO

Define Initial Void Ratio for Soil or Diffusion Analysis

The information provided here is based upon not using the table driven input style. Description This option provides the ability to initialize the porosity throughout the soil analysis model. You can either specify the void ratio or use the INITIAL POROSITY option to specify the porosity. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL VOID.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the initial void ratio.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. 3rd data block 1-10

1st

F

Enter the initial void ratio for the points given below at the start of increment zero.

4th data block Enter a list of elements to which the above void ratio is to be applied. 5th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above void ratio is to be applied. 6th data block This data block is necessary only when there are either beams or shells in the mesh. Enter a list of layer points to which the above void ratio is to be applied.

Main Index

VOID CHANGE (with TABLE Input - Model Definition) 939 Define Changes in Void Ratio for Nonsoil Analysis

VOID CHANGE (with TABLE Input - Model Definition)

Define Changes in Void Ratio for Nonsoil Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides the ability to define the void ratio in nonsoil analysis model. The magnitude and location of the void ratio is associated with a boundary condition name. The LOADCASE model definition option is used to activate this data. You can either specify the void ratio or use the POROSITY CHANGE option to specify the porosity. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words VOID CHANGE.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the void ratio.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the void ratio.

4th data block 1-10

Main Index

1st

940 VOID CHANGE (with TABLE Input - Model Definition) Define Changes in Void Ratio for Nonsoil Analysis

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Enter the table ID associated with the void ratio.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above void ratio is applied. the geometric entities must all be of the type prescribed in the 6th data block.

INITIAL PC (with TABLE Input) 941 Define Initial Preconsolidation Pressure

INITIAL PC (with TABLE Input)

Define Initial Preconsolidation Pressure

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides the ability to define the preconsolidation pressure throughout the model for soil analysis when using the Cam-Clay model. The magnitude and location of the preconsolidation pressure is associated with an initial condition name. The LOADCASE model definition is used to activate this data. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PC.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the preconsolidation pressure.

6-10

2nd

I

Enter the unit number; defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the preconsolidation pressure.

I

Enter the table ID associated with the preconsolidation pressure.

4th data block 1-10

1st

5th data block 1-5

Main Index

1st

942 INITIAL PC (with TABLE Input) Define Initial Preconsolidation Pressure

Format Fixed

Free

Data Entry Entry

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. the geometric entities must all be of the type prescribed in the 6th data block.

INITIAL PC 943 Define Initial Preconsolidation Pressure

INITIAL PC

Define Initial Preconsolidation Pressure

The information provided here is based upon not using the table driven input style. Description This option provides the ability to define the preconsolidation pressure throughout the model for soil analysis when using the Cam-Clay model. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PC.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the preconsolidation pressure.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. 3rd data block 1-10

1st

F

Initial value of the preconsolidation pressure for the points given below at the start of the zeroth increment.

4th data block Enter a list of elements for which the above data is to be applied. 5th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points for which the data is to be applied. 6th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above data is to be applied.

Main Index

944 SPECIFIC WEIGHT Define Specific Weight Constant for Soil Analysis

SPECIFIC WEIGHT

Define Specific Weight Constant for Soil Analysis

Description This option allows you to enter the specific weight constant with respect to the global coordinate system for soil analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SPECIFIC WEIGHT.

2nd data block

Main Index

1-10

1st

F

Enter gravity constant in first coordinate direction.

11-20

2nd

F

Enter gravity constant in second coordinate direction.

21-30

3rd

F

Enter gravity constant in third coordinate direction.

INITIAL PORE (with TABLE Input) 945 Define Initial Pore Pressure for Soil Analysis

INITIAL PORE (with TABLE Input) Define Initial Pore Pressure for Soil Analysis The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides the ability to initialize the pore pressure throughout the model for an uncoupled soil analysis where the pore pressure is not calculated. In such cases, the 2nd field of the PORE parameter is zero. These initial conditions will be activated using the LOADCASE model definition option. As an alternative, the INITPO user subroutine can be used. Initial Pore Pressure may be used in three different ways with the new table input format. Method 1 is when data is directly input. While not explicitly stated, the data can always be a function of a table, where the independent variables are, e.g., position to allow a nonhomogeneous field. Method 2 is based upon reading the plastic strain from a post file created in a previous stress analysis. Method 3 is using INITPO user subroutine to define initial plastic strain variables. 1. Read the range of elements, integration points and layers and a corresponding value. 2. Read the initial values from a step of the post output file from a previous analysis with Marc. This technique is most common for uncoupled soil analysis to initialize the pore pressure. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 3. Read the initial values through the INITPO user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL PORE.

2nd data block 1-5

1st

I

Number of sets of initial pore pressure data to be entered (optional)

6-10

2nd

I

Unit number for input of initial pore pressure data. Defaults to input file.

3rd data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter the method:

946 INITIAL PORE (with TABLE Input) Define Initial Pore Pressure for Soil Analysis

Format Fixed

Free

Data Entry Entry 3 – use binary post file 5 – use ASCII post file 6 – use data lines (default) 7 – use the INITPO user subroutine.

11-15

3rd

I

If method 3 or 5, enter the step number to read. If method 6, enter the number of geometric types used to define this boundary condition.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-35

7th

A

Enter the unique boundary condition label. This label will be referenced by the LOADCASE option.

4th data block (Used only if method = 6 or 7) 1-10

1st

F

Enter the initial pore pressure.

5th data block (Used only if method = 6 or 7) 1-5

1st

F

Table ID associated with the initial pore pressure.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd field of the 2nd data block (only used if method = 6 or 7). 6th data block 1-5

1st

I

Enter the geometry type: 1 – Element IDs 3 – Volume/Region/Body iDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be al the type prescribed in the 6th data block.

INITIAL PORE 947 Define Initial Pore Pressure for Soil Analysis

INITIAL PORE

Define Initial Pore Pressure for Soil Analysis

The information provided here is based upon not using the table driven input style. Description This option provides the ability to initialize the pore pressure throughout the model for an uncoupled soil analysis where the pore pressure is not calculated. In such cases, the 2nd field of the PORE parameter is zero. Four ways of providing the initial pore pressures are given below. 1. Read the range of elements, integration points and layers, and a corresponding pore pressure. 2. Read the initial values through the INITPO user subroutine. 3. Read the initial values from a step of the binary or formatted post output file from a previous pore pressure analysis with Marc. This technique is most common for uncoupled soil analysis to initialize the pore pressure. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 4. Read a list of elements, integration points and layers and a corresponding pore pressure. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INITIAL PORE.

2nd data block 1-5

1st

I

Enter 1.

6-10

2nd

I

Enter 1 to initialize the pore pressure via block 3 series below. See also the third field on this data block. Enter 2 to initialize the pore pressure via the INITPO user subroutine. This subroutine is now called in a loop on all elements in the mesh. Enter 3 to read the initial values of the pore pressure from the post file written by a previous pore pressure analysis. In this case, the fourth and fifth field must also be defined. Enter 4 to initialize the pore pressure via data blocks 5, 6, 7 and 8 given below. See also the third field on this data block.

Main Index

948 INITIAL PORE Define Initial Pore Pressure for Soil Analysis

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Only nonzero if the second field is set to 3 or 4. Then, this entry gives the number of pairs of blocks in series 3 and 4 or in series 5, 6, 7, 8 used to input the pore pressure.

16-20

4th

I

Only used if the second field is set to 3. Then this entry defines the unit number from which the post file information from the previous pore pressure run is to be read.

21-25

5th

I

Only used if the second field is set to 3. In that case this entry defines the step number on the pore pressure run post file to be used as the definition of the initial pore pressure values.

26-30

6th

31-35

7th

I

If option 3 and a formatted post file, are used, enter 1.

36-40

8th

I

Only nonzero if the second field is set to 2.

Not used; enter 0.

Enter 1 to suppress printout of pore pressure values that are initialized in the INITPO user subroutine. 3rd data block Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of blocks is equal to the number given in the third field above. 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with the value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value.

21-25

5th

I

First layer of cross section point with this value.

26-30

6th

I

Last layer or cross section point with this value can only be bigger than 1 for beam or shell elements.

F

Initial value of the pore pressure for the above range of points.

4th data block 1-10

1st

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

Initial pore pressure for the points given below at the start of the zeroth increment.

6th data block Enter a list of elements to which the above pore pressure is to be applied.

Main Index

INITIAL PORE 949 Define Initial Pore Pressure for Soil Analysis

Format Fixed

Free

Data Entry Entry

7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above pore pressure is to be applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above pore pressure is to be applied.

Main Index

950 CHANGE PORE (with TABLE Input - Model Definition) Define Pore Pressure for Uncoupled Soil Analysis

CHANGE PORE (with TABLE Define Pore Pressure for Uncoupled Soil Analysis Input - Model Definition) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides the ability to initialize the pore pressure throughout the model for an uncoupled soil analysis where the pore pressure is not calculated. The change in the pore pressure will be activated using the LOADCASE model definition option. As an alternative, the NEWPO user subroutine can be used. Initial Pore Pressure may be used in three different ways with the new table input format. Method 1 is when data is directly input. While not explicitly stated, the data can always be a function of a table, where the independent variables are, e.g., position to allow a nonhomogeneous field. Method 2 is based upon reading the plastic strain from a post file created in a previous stress analysis. Method 3 is using the NEWPO user subroutine to define initial plastic strain variables. 1. Read the range of elements, integration points and layers and a corresponding value. 2. Read the initial values from a step of the post output file from a previous analysis with Marc. This technique is most common for uncoupled soil analysis to initialize the pore pressure. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 3. Read the initial values through the NEWPO user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words CHANGE PORE.

2nd data block 1-5

1st

I

Number of sets of pore pressure data to be entered (optional)

6-10

2nd

I

Unit number for input of pore pressure data. Defaults to input file.

3rd data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter the method:

CHANGE PORE (with TABLE Input - Model Definition) 951 Define Pore Pressure for Uncoupled Soil Analysis

Format Fixed

Free

Data Entry Entry 3 – use binary post file 5 – use ASCII post file 6 – use data lines (default) 7 – use the NEWPO user subroutine.

11-15

3rd

I

If method 3 or 5, enter the step number to read. If method 6, enter the number of geometric types used to define this boundary condition.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-35

7th

A

Enter unique boundary condition label. This label will be referenced by the LOADCASE option.

4th data block (Used only if method = 6 or 7) 1-10

1st

F

Enter the pore pressure.

5th data block (Used only if method = 6 or 7) 1-5

1st

F

Table ID associated with the pore pressure.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd field of the 3rd data block (used only if method = 6 or 7). 6th data block 1-5

1st

I

Enter the geometry type: 1 – Element IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above pore pressure are applied. The geometric entities must all be al the type prescribed in the 6th data block.

952 CHANGE PORE (Model Definition) Define Pore Pressures for Uncoupled Soil Analysis

CHANGE PORE (Model Definition)

Define Pore Pressures for Uncoupled Soil Analysis

The information provided here is based upon not using the table driven input style. Description This option provides various ways of changing the pore pressure throughout the model. This option is only used in uncoupled soil analysis. In such cases, the 2nd field of the PORE parameter is zero. Four ways of providing the pore pressures are given below. 1. Read a range of elements, integration points and layers, and corresponding pore pressures for the end of the current step. 2. Read the pore pressure values for the end of the current step through the NEWPO user subroutine. 3. Read the pore pressure values for the end of the current step from a named step of the post file output from a previous pore pressure analysis with Marc. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 4. Read a list of elements, integration points and layers, and corresponding pore pressure. Note:

On this option, total pore pressures are input.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words CHANGE PORE.

2nd data block 1-5

1st

I

Enter 1.

6-10

2nd

I

Enter 1 to change the pore pressure via data block 3 below. In this case, the third field must also be defined. Enter 2 to change the pore pressure via the NEWPO user subroutine. This subroutine is then called in a loop on all the elements in the mesh. Enter 3 to read the initial values of the pore pressure from the post file written by a previous pore pressure analysis. In this case, the fourth and fifth field must also be defined. Enter 4 to change the pore pressure via data blocks 5, 6, 7 and 8 below.

Main Index

CHANGE PORE (Model Definition) 953 Define Pore Pressures for Uncoupled Soil Analysis

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. In that case, this entry gives the number of block sets in series 3 and 4 used to input the new value of the pore pressure (optional).

16-20

4th

I

Only nonzero if the second field is set to 3. Then, this entry defines the unit number from which the post file information from the previous pore pressure run is read.

21-25

5th

I

Only nonzero if the second field is set to 3. In that case, this entry defines the step number on the pore pressure run post file to be read as the definition of the new value of the pore pressure at the end of the current step.

26-30

6th

I

Not used; enter 1.

31-35

7th

I

Enter 1 if a formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2. Set to 1 to suppress printout of pore pressure values that are defined in the NEWPO user subroutine.

Data blocks 3 and 4 are only input if the second field above set to 1. In that case, the number of block sets is equal to the number given in the third field above. 3rd data block 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with this value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value can only be bigger than 1 if the ALL POINTS parameter is used.

21-25

5th

I

First layer or cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value.

F

New value of the pore pressure for the above range of points at the end of the current step.

4th data block 1-10

1st

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

Pore pressure for the points given below at the end of the current increment.

6th data block Enter a list of elements to which the above pore pressure is to be applied.

Main Index

954 CHANGE PORE (Model Definition) Define Pore Pressures for Uncoupled Soil Analysis

Format Fixed

Free

Data Entry Entry

7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above pore pressure is to be applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above pore pressure is to be applied.

Main Index

PRESS FILM (with TABLE Input) 955 Define Pressure Film Boundary Conditions

PRESS FILM (with TABLE Input)

Define Pressure Film Boundary Conditions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows the input of pressure film boundary conditions applied on the surface of the model. The user defines the pressure film coefficients and ambient pressures here. Nonuniform pressure film coefficients or pressures can be specified via the UPRFILM user subroutine (see Marc Volume D: User Subroutines and Special Routines) or by using the TABLE model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the words PRESS FILM.

2nd data block 1-5

1st

I

Number of sets of data used to input pressure films (optional).

6-10

2nd

I

Unit number for input of pressure film data, defaults to input.

Data blocks 3 through 8 are entered for each film input. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define pressure film boundary condition. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the UPRFILM user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used, enter 0.

26-30

6th

I

Enter -1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

956 PRESS FILM (with TABLE Input) Define Pressure Film Boundary Conditions

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Reference value of pressure film coefficient.

11-20

2nd

F

Reference value of ambient pressure (reference values can be modified by the UPRFILM user subroutine).

5th data block - Table IDs 1-5

1st

I

Enter the table ID associated with the pressure film coefficient.

6-10

2nd

I

Enter the table ID associated with the ambient pressure.

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal flow (bottom surface for shells) 10: Normal flow (top surface for shells)

11-15

3rd

I

Enter the face ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID

Main Index

PRESS FILM (with TABLE Input) 957 Define Pressure Film Boundary Conditions

Format Fixed

Free

Data Entry Entry 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention.

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

958 PRESS FILM (Model Definition) Define Pressure Film Coefficient Input

PRESS FILM (Model Definition)

Define Pressure Film Coefficient Input

The information provided here is based upon not using the table driven input style. Description This option allows pressure film coefficients and associated ambient pressures to be input. Nonuniform pressure films or ambient pressures can be specified via the UPRFILM user subroutine (see Marc Volume D: User Subroutines and Special Routines). Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the words PRESS FILM.

2nd data block 1-5

1st

I

Number of sets of data used to input pressure film (optional).

6-10

2nd

I

Unit number for input of pressure film data, defaults to input.

1-5

1st

I

Face identification. Same as for the FLUX user subroutine – see Marc Volume B: Element Library.

6-15

2nd

F

Reference value of pressure film coefficient.

16-25

3rd

F

Reference value of ambient pressure (reference values can be modified by the UPRFILM user subroutine).

3rd data block

4th data block Enter a list of elements to which the above film data is applied.

Main Index

Chapter 3: Model Definition Options 959 Rate Effects

Chapt Rate Effects er 3: This section describes the input of material behavior with rate effects. There are many models which Mode exhibit this behavior and they can be numerically implemented in a variety of way. Rate dependent yield stress is a particular type of rate effects. When used without any of the options l defined in this section, the strain is decomposed into an elastic increment - irreversible plastic increment Defini and thermal increment. The rate dependent yield models include: tion Optio Model Option User Subroutine ns STRAIN RATE or TABLE Piecewise linear

Marc Volume C: Program Input

Cowper Symonds

STRAIN RATE

General

ISOTROPIC/ORTHOTROPIC

Power Law

ISOTROPIC

Rate Power Law

ISOTROPIC

Kumar

ISOTROPIC

Johnson-Cook

ISOTROPIC

YIEL

Strain rate effects may also be included by the following models:

Behavior

Model

Elastic-Deviatoric Creep*

Maxwell

Elastic-Deviatoric Creep*

Kelvin

Implicit/ Explicit Explicit

Parameter CREEP,0

User Model Definition Subroutine CREEP

CRPLAW

(optional) Explicit

CRPVIS

CREEP,0,1

or VISCO ELAS

Elastic-Dilatational Maxwell

Explicit

CREEP,0

Elastic-Deviatoric Creep

Maxwell

Implicit

CREEP,0,0,1

Viscoplasticity

Maxwell

VSWELL CREEP

UCRPLW

(optional) Explicit

CREEP,1,0,0

CREEP

CRPLAW, NASSOC, ZERO. YIEL

* Can be combined with elastic-plastic behavior. ** Can only be used for plane strain, generalized plane strain, axisymmetric, and 3-D elements.

Main Index

960 Marc Volume C: Program Input Rate Effects

Behavior Viscoplasticity**

Model Maxwell

Implicit/ Explicit Implicit

Parameter CREEP,0,0,1

User Model Definition Subroutine ISOTROPIC

UVSCPL

“VISCO PLAS” Isotropic Small Strain Viscoelasticity

Hereditary Implicit Integral

ISOTROPIC VISCELPROP

Orthotropic Small Strain Viscoelasticity

Hereditary Implicit Integral

ORTHOTROPIC

Large Strain Incompressible Viscoelastic (Mooney, Gent, Arruda-Boyce)

Hereditary Implicit Integral

VISCELMOON

Large Strain Viscoelastic (Ogden)

Hereditary Implicit Integral

VISCELOGDEN

Large Strain Viscoelastic Foam

Hereditary Implicit Integral

VISCELFOAM

ThermalRheologically Simple

Implicit

Viscoelastic Thermal Expansion

HOOKVI

VISCELORTH

SHIFT FUNCTION

SHIFT FUNCTION VISCEL EXP

* Can be combined with elastic-plastic behavior. ** Can only be used for plane strain, generalized plane strain, axisymmetric, and 3-D elements.

Main Index

CREEP (with TABLE Input) 961 Define Creep Constitutive Data

CREEP (with TABLE Input)

Define Creep Constitutive Data

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the parameters and material properties used in a creep analysis. The creep data can be specified in either an exponent form or in a piecewise linear curve or an equation. Attention is drawn to the existence of the CRPLAW user subroutine, which allows alternative forms of creep behavior to be programmed indirectly. Further detail on creep is given in Marc Volume D: User Subroutines and Special Routines and Marc Volume A: Theory and User Information. In addition, the CREEP parameter must be included. The three possible modes of input of creep constitutive data are: 1. Using a table or an equation to directly input the creep strain rate. In this case, the first four entries of data block 2 are zero, and data block 3 is used to enter the table ID which may refer to an equation. See Table option. 2. The dependence of equivalent creep strain rate on any independent parameter can be given directly in power law form by giving the appropriate exponent (as a floating-point number) in the first field of blocks 4, 5, 6, or 7. The equivalent creep strain rate is ·c ε = Aσ n ⋅ ( ε c ) n ⋅ T n ⋅ ( nt n – 1 )

Note that the time dependence is specified as a function of total equivalent creep strain. ε c = Atn The power law form is indicated by setting the corresponding field on data block 2 to -1. The multiplier A may have a table associated with it. 3. For a user-supplied creep law (using the CRPLAW subroutine, see Marc Volume D: User Subroutines and Special Routines), set the first five fields of block 2 to 0. Note:

The default numerical procedure for creep analysis is explicit. In case of Norton creep, an alternative implicit procedure can be used. This should be set using the CREEP parameter.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

Main Index

1st

A

Enter the word CREEP.

962 CREEP (with TABLE Input) Define Creep Constitutive Data

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter -1 if creep strain rate is a function of the temperature raised to a power. The exponent is given on the 4th data block.

6-10

2nd

I

Enter -1 if creep strain rate is a function of the equivalent stress raised to a power. The exponent is given on the 5th data block.

11-15

3rd

I

Enter -1 if creep strain rate is a function of the creep strain raised to a power. The exponent is given on the 6th data block.

16-20

4th

I

Enter -1 if the total creep strain is a function of the time raised to a power. The exponent is given on the 7th data block.

21-35

5th

F

Enter the numerical constant in total creep strain relation. Set to zero if a creep law is being supplied through the CRPLAW user subroutine.

36-50

6th

F

Not used; enter 0.

51-65

7th

F

Not used; enter 0.

66-70

8th

I

Enter the unit number for input of creep data, defaults to input.

71-75

9th

I

Material ID number.

3rd data block 1-5

1st

I

No used; enter zero.

6-10

2nd

I

No used; enter zero.

11-15

3rd

I

No used; enter zero.

16-20

4th

I

No used; enter zero.

21-25

5th

I

Enter table ID associated with scalar multiplier A.

4th data block Required only if 1st field, 2nd data block = -1. 1-15

1st

F

Enter the exponent of temperature in the exponential creep law.

4a data block Required only if 2nd field, 2nd data block = -1. 1-15

1st

F

Enter the exponent of stress in the exponential creep law.

6th data block Required only if 3rd field, 2nd data block = -1. 1-15

Main Index

1st

F

Enter the exponent of total equivalent creep strain in the exponential creep law.

CREEP (with TABLE Input) 963 Define Creep Constitutive Data

Format Fixed

Free

Data Entry Entry

7th data block Required only if 4th, 2nd data block = -1. 1-15

Main Index

1st

F

Enter the exponent of time in the exponential creep law.

964 CREEP Define Creep Constitutive Data

CREEP

Define Creep Constitutive Data

The information provided here is based upon not using the table driven input style. Description This option defines the parameters and material properties used in a creep analysis. The creep data can be specified in either an exponent form or in a piecewise linear curve. Attention is drawn to the existence of the CRPLAW user subroutine, which allows alternative forms of creep behavior to be programmed indirectly. Further detail on creep is given in Marc Volume D: User Subroutines and Special Routines and Marc Volume A: Theory and User Information. In addition, the CREEP parameter must be included. The three possible modes of input of creep constitutive data are: 1. Express the dependence of equivalent creep strain rate on any independent parameter through a piecewise-linear relationship. The equivalent creep strain rate is then assumed to be a piecewise linear approximation to ·c dk ( t ) ε = A ⋅ f ( σ ) ⋅ g ( ε c ) ⋅ h ( T ) ⋅ ------------dt

Note that the function k relates total equivalent creep strain to time. Any of the functions f, g, h, or k can be set to unity by setting the number of slopes to zero for that relation on the input data. This is done using one of two methods. Note that these methods cannot be mixed for different functions (f, g, h, k). a. The slopes and breakpoints of the piecewise linear functions are given using data blocks 3a, 4a, 5a, and 6a. Note that the independent variable either σ, εc, T, or t should be given in ascending order. The format is as follows: Column

Field

Entry

1-15

1st

Slope of curve.

16-30

2nd

Breakpoint at which slope begins with the number of blocks describing each curve (up to a maximum of five) given in the appropriate field on block 2 of this set.

b. The data points describing the curve of ε c are given directly using data blocks 3b, 4b, 5b, and 6b. This method is flagged by entering the word “DATA” on the CREEP option. These data points are used to calculate slope breakpoint data. Note that the value of point should equal the value A. The format is as follows:

Main Index

εc

at the lowest data

CREEP 965 Define Creep Constitutive Data

Column

Field

Entry

1-15

1st

Value of

16-30

2nd

Value of either σ, εc, or T for data blocks 3b, 4b, 5b, or 6b

Column

Field

Entry

1-15

1st

Value of

16-30

2nd

Value of t

·c ε

εc

2. The dependence of equivalent creep strain rate on any independent parameter can be given directly in power law form by giving the appropriate exponent (as a floating-point number) in the first field of blocks 3, 4, 5, or 6. The equivalent creep strain rate is ·c ε = Aσ n ⋅ ( ε c ) n ⋅ T n ⋅ ( nt n – 1 )

Note that the time dependence is specified as a function of total equivalent creep strain. ε c = Atn The power law form is indicated by setting the corresponding field on data block 2 to -1. 3. For a user-supplied creep law (using the CRPLAW user subroutine, see Marc Volume D: User Subroutines and Special Routines), set the first five fields of data block 2 to 0. Note:

The default numerical procedure for creep analysis is explicit. In case of Norton creep, an alternative implicit procedure can be used. This should be set using the CREEP parameter.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word CREEP.

11-80

2nd

A

Enter the word DATA to indicate that option B is being used.

2nd data block

Main Index

1-5

1st

I

Number of blocks defining creep-strain rate versus temperature relation.

6-10

2nd

I

Number of blocks defining creep-strain rate versus equivalent stress relation.

11-15

3rd

I

Number of blocks defining creep-strain rate versus equivalent creep-strain curve.

16-20

4th

I

Number of blocks defining total creep-strain increment versus time curve.

966 CREEP Define Creep Constitutive Data

Format Fixed

Free

Data Entry Entry

21-35

5th

F

Enter the numerical constant in total creep strain relation. Set to zero if a creep law is being supplied through the CRPLAW user subroutine.

36-50

6th

F

If the entry in the tenth field is 0, enter tolerance on the creep strain increment relative to the elastic strain. Default = 0.50. A higher value is likely to cause stability problems. If the entry in the tenth field is 1, enter the maximum allowable creep strain increment. Default is .01. Note:

51-65

7th

F

Use of the AUTO CREEP option to input this value is preferred.

If the entry in the tenth field is 0, enter the tolerance on the stress change per stress during creep. Default is 0.10. If the entry in the tenth field is 1, enter the maximum stress increment. Default is 100. This control is included primarily for accuracy purposes. Default value is adequate for creep laws of the type ε = aσn where 3 < n < 6. For lower values of n, tolerance can be increased; for higher values, it should be decreased. Note:

Use of the AUTO CREEP option to input this value is preferred.

66-70

8th

I

Enter the unit number for input of creep data, defaults to input.

71-75

9th

I

Material ID number.

76-80

10th

I

Enter 1 if absolute rather than relative testing is to be performed.

3a data block Slope and breakpoint data for equivalent creep strain rate versus temperature curve. The number entered in the first field of the second data block defines the number of blocks required in data block 3. 1-15

1st

F

Enter the slope of the curve or the exponent of temperature in the exponential creep law.

16-30

2nd

F

Enter the temperature above which the slope (above) becomes operative. This entry is left blank for exponential creep law.

4a data block Enter the slope and breakpoint data for equivalent creep strain rate versus equivalent total stress curve. The number entered in the second field of the second data block defines the number of blocks required in data block 4.

Main Index

1-15

1st

F

Enter the slope of the curve or the exponent of stress in the exponential creep law.

16-30

2nd

F

Enter the equivalent total stress above which the slope becomes operative. This entry is left blank for exponential creep law.

CREEP 967 Define Creep Constitutive Data

Format Fixed

Free

Data Entry Entry

5a data block Slope and breakpoint data for equivalent creep strain rate versus total equivalent creep strain curve. The number entered in the third field of the second data block defines the number of blocks required in data block 5. 1-15

1st

F

Enter the slope of the curve or the exponent of total equivalent creep strain in the exponential creep law.

16-30

2nd

F

Enter the equivalent total creep strain above which the slope becomes operative. This entry is left blank for exponential creep law.

6a data block Slope and breakpoint data for total equivalent creep strain versus time curve. The number entered in the fourth field of the second data block defines the number of blocks required in data block 6. 1-15

1st

F

Enter the slope of the curve or the exponent of time in the exponential creep law.

16-30

2nd

F

Enter the total time above which the slope becomes operative. This entry is left blank for exponential creep law.

3b data block Data points for the equivalent creep strain rate versus temperature curve. The number entered in the first field of the second data block defines the number of blocks required in data block 3. 1-15

1st

F

Enter the equivalent creep strain rate or the exponent of temperature in the exponential creep law.

16-30

2nd

F

Enter the associated temperature. This entry is left blank for exponential creep law.

4b data block Data points for the equivalent creep strain rate versus equivalent total stress curve. The number entered in the second field of the second data block defines the number of blocks required in data block 4. 1-15

1st

F

Enter the equivalent creep strain rate or exponents of stress in the exponential creep law.

16-30

2nd

F

Enter the associated equivalent total stress. This entry is left blank for exponential creep law.

5b data block Data points for the equivalent creep strain rate versus total equivalent creep strain curve. The number entered in the third field of the second data block defines the number of blocks required in data block 5.

Main Index

1-15

1st

F

Enter the equivalent creep strain rate or the exponent of total equivalent creep strain in the exponential creep law.

16-30

2nd

F

Enter the associated total creep strain. This entry is left blank for exponential creep law.

968 CREEP Define Creep Constitutive Data

Format Fixed

Free

Data Entry Entry

6b data block Data point for the equivalent creep strain versus time curve. The number entered in the fourth field of the second data block defines the number of blocks required in data block 6.

Main Index

1-15

1st

F

Enter the equivalent creep strain or the exponent of time in the exponential creep law.

16-30

2nd

F

Enter the associated total time. This entry is left blank for exponential creep law.

PHI-COEFFICIENTS 969 Define Phi-Coefficients for Rubber Viscoelastic Model

PHI-COEFFICIENTS

Define Phi-Coefficients for Rubber Viscoelastic Model

Description This option allows the input of phi function value vs. frequency for one out of the seven possible PHI functions φ0, φ1, φ2, φ11, φ12, φ21, φ22 . This option can be repeated up to seven times to completely define the seven PHI functions. These PHI functions are used in a harmonic analysis with rubber materials using the Mooney material model. This can be used only in the total Lagrange formulation. See Marc Volume A: Theory and User Information for more detail. Note:

For symmetry of the relaxation data, φ12 should equal φ21.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PHI-COEFFI.

2nd data block 1-5

1st

I

Number of different frequencies per PHI function to be read in. If a negative value is entered, the UPHI user subroutine is called to supply PHI coefficients as a function of frequency for all PHI functions.

6-10

2nd

I

PHI function identifier. = 1 for φ0 = 2 for φ1 = 3 for φ2 = 4 for φ11 = 5 for φ12 = 6 for φ21 = 7 for φ22

11-15

3rd

3rd data block (Not

Main Index

I

Material type identifier.

used if the UPHI user subroutine is requested)

1-10

1st

F

Frequency in radians/time unit.

11-20

2nd

F

Real PHI coefficient.

21-30

3rd

F

Imaginary PHI coefficient.

970 VISCELPROP Define Properties for Isotropic Viscoelastic Materials

VISCELPROP

Define Properties for Isotropic Viscoelastic Materials

Description This option is used to specify the time dependent part of the material behavior of a small strain viscoelastic material. Here, only isotropic quantities can be specified. Note that the instantaneous moduli for small-strain viscoelasticity are specified on the ISOTROPIC option. Orthotropic time-dependent behavior can be specified using the VISCELORTH option. Note:

Thermo-rheologically simple behavior is specified with the SHIFT FUNCTION option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VISCELPROP.

2nd data block 1-5

1st

I

Enter the number of distinct sets of viscoelastic properties to be input.

6-10

2nd

I

Enter the unit number for input of viscoelastic properties, default to input.

3rd data block 1-5

1st

I

Material type identification number. This number is used for cross reference with the ISOTROPIC, TEMPERATURE EFFECTS, and SHIFT FUNCTION options.

6-10

2nd

I

Maximum number of terms in the Prony series expansion (maximum value of either the deviatoric terms or the volumetric terms).

11-15

3rd

I

Number of terms in the Prony series expansion for deviatoric behavior.

16-20

4th

I

Number of terms in the Prony series expansion for volumetric behavior.

4th data block Repeated for the maximum number of terms.

Main Index

1-10

1st

F

Shear constant.

11-20

2nd

F

Relaxation time for deviatoric behavior.

21-30

3rd

F

Bulk constant.

31-40

4th

F

Relaxation time for volumetric behavior

VISCELORTH 971 Define Properties for Viscoelastic Orthotropic Materials

VISCELORTH

Define Properties for Viscoelastic Orthotropic Materials

Description This option inputs the time dependent material data used in conjunction with the ORTHOTROPIC option for viscoelastic materials. It can also be used to specify the anisotropic time dependent constants for an anisotropic material exhibiting small strain viscoelastic behavior by use of the HOOKVI user subroutine. The instantaneous elastic behavior is specified on the ORTHOTROPIC option. Note:

Since the material properties for orthotropic materials are independent, it is your responsibility to enter all required data. No defaults are provided by Marc.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VISCELORTH.

2nd data block 1-5

1st

I

Number of sets of VISCELORTH data to read.

6-10

2nd

I

Unit number for reading data, defaults to input.

The 3rd, 4th, and 5th data blocks are entered as a set, once for each set of VISCELORTH data. 3rd data block 1-5

1st

I

Material identification number for cross-referencing with ORTHOTROPIC data.

6-10

2nd

I

Number of terms in the Prony series expansion (note that deviatoric and volumetric behavior are treated together).

4th data block

Main Index

1-10

1st

F

Time constant for this term in the Prony series expansion.

11-20

2nd

F

n E xx

21-30

3rd

F

n E yy

31-40

4th

F

n E zz

41-50

5th

F

n ν xy

51-60

6th

F

n ν yz

61-70

7th

F

n ν zx

972 VISCELORTH Define Properties for Viscoelastic Orthotropic Materials

Format Fixed

Free

Data Entry Entry

5th data block

Main Index

1-10

1st

F

n G xy

11-20

2nd

F

n G yz

21-30

3rd

F

n G zx

VISCELMOON 973 Define Properties for Large Strain Viscoelastic Materials

VISCELMOON

Define Properties for Large Strain Viscoelastic Materials

Description This option is used to input the time dependent data for a Mooney-Rivlin, Gent, or Arruda-Boyce viscoelastic material. The instantaneous elastic behavior is specified using the MOONEY, ARRUDBOYCE, or GENT model definition option, respectively. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VISCELMOON.

2nd data block 1-5

1st

I

Number of sets of VISCELMOON data to read.

6-10

2nd

I

Unit number for reading data. Defaults to input.

The 3rd data block is entered once for each set of VISCELMOON data. 3rd data block 1-5

1st

I

Material ID number for cross-referencing with the rate independent properties.

6-10

2nd

I

Number of terms in the Prony series expansion for deviatoric behavior.

The 4th data block is entered once for each term in the Prony series. 4th data block

Main Index

1-10

1st

F

Multiplier for energy function.

11-20

2nd

F

Relaxation time.

974 VISCELOGDEN Define Properties for Large Strain Viscoelastic Ogden Materials

VISCELOGDEN

Define Properties for Large Strain Viscoelastic Ogden Materials

Description This option is used to input the time dependent data for a Ogden viscoelastic material. The instantaneous elastic behavior is specified using the OGDEN model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VISCELOGDEN.

2nd data block 1-5

1st

I

Number of sets of data to read.

6-10

2nd

I

Unit number for reading data. Defaults to input.

The 3rd data block is entered once for each set of data. 3rd data block 1-5

1st

I

Material ID number for cross-referencing with the OGDEN option.

6-10

2nd

I

Maximum number of terms of either Prony series expansion.

11-15

3rd

I

Number of terms for deviatoric behavior.

16-20

4rd

I

Number of terms for dilatational behavior.

The 4th data block is entered once for each term in the Prony series. 4th data block

Main Index

1-10

1st

F

Multiplier for deviatoric energy function.

11-20

2nd

F

Deviatoric relaxation time.

21-30

3rd

F

Multiplier for dilatational energy function.

31-40

4rd

F

Dilatational relaxation time.

VISCELFOAM 975 Define Properties for Large Strain Viscoelastic Materials

VISCELFOAM

Define Properties for Large Strain Viscoelastic Materials

Description This option is used to input the time dependent data for a foam viscoelastic material. The instantaneous elastic behavior is specified using either the FOAM model definition option or the UELASTOMER user subroutine. This option must be used with LARGE STRAIN; i.e., updated Lagrange formulation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VISCELFOAM.

2nd data block 1-5

1st

I

Number of sets of VISCELFOAM data to read.

6-10

2nd

I

Unit number for reading data. Defaults to input.

The 3rd data block is entered once for each set of VISCELFOAM data. 3rd data block 1-5

1st

I

Material ID number for cross-referencing with the rate independent properties.

6-10

2nd

I

Number of terms in the Prony series expansion for deviatoric behavior.

The 4th data block is entered once for each term in the Prony series. 4th data block

Main Index

1-10

1st

F

Multiplier for energy function.

11-20

2nd

F

Relaxation time.

976 SHIFT FUNCTION Define Properties for Thermo-rheologically Simple Viscoelastic Materials

SHIFT FUNCTION

Define Properties for Thermo-rheologically Simple Viscoelastic Materials

Description This option allows you to define the shift function parameters for viscoelastic material groups that exhibit thermo-rheologically simple behavior. Note that for the Narayanaswamy model, the initial value of the fictive temperature for each term must be specified as the second state variable via the INITIAL STATE option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SHIFT FUNCTION.

2nd data block 1-5

1st

I

Number of sets used to define different shift functions.

6-10

2nd

I

Unit number from which the data block is read. Defaults to block input.

The 3rd and 4th data blocks are entered as pairs, once for each data set. 3rd data block 1-5

1st

I

Material number for cross-referencing with the instantaneous and time dependent viscoelastic properties.

6-10

2nd

I

Enter the code number denoting the shift function type: 1 = Williams-Landel-Ferry equation 2 = Power series expansion 3 = Narayanaswamy model -N = any negative integer value denotes that the shift function is specified in the user subroutine.

11-15

3rd

I

If the second field is 2, enter the number of coefficients in the power series representation. If the second field is 3, enter the number of terms in Prony series expansion.

16-25

4th

E

Enter the reference or glass transition temperature Tg, for this shift function. For the Narayanaswamy model, enter the temperature for stress relaxation data.

Main Index

SHIFT FUNCTION 977 Define Properties for Thermo-rheologically Simple Viscoelastic Materials

Format Fixed

Free

Data Entry Entry

26-35

5th

E

For the Narayanaswamy model, enter the activation energy divided by the gas constant Q/R.

36-45

6th

E

For the Narayanaswamy model, enter the fraction parameter.

46-55

7th

E

For the Narayanaswamy model, enter the temperature shift between your temperature and absolute temperature for calculating fictitive temperatures.

56-65

8th

E

For the Narayanaswamy model, enter the reference temperature for the structural relaxation data.

If Williams-Landel-Ferry form, use the following data block. 4th data block 1-10

1st

F

Enter the constant C1.

11-20

2nd

F

Enter the constant C2.

If power series expansion, use the following data block. If shift function is defined in the TRSFAC user subroutine, the 4th data block is not required. 4th data block 1-80

1st

F

Enter the constants Co to Cm in increasing order of subscript, using additional blocks if necessary to define all constants.

If Narayanaswamy model, use the 4th and 5th data blocks. 4th data block 1-80

1st

F

Enter the weighting factors Wg in increasing order of subscript. Use additional blocks if necessary to define all constants.

F

Enter the relaxation time τi,ref in increasing order of subscript. Use additional blocks if necessary to define all constants.

5th data block 1-80

Main Index

1st

978 VISCEL EXP Viscoelastic Thermal Expansion

VISCEL EXP

Viscoelastic Thermal Expansion

Description This option is used to define the thermal expansion behavior often observed in viscoelastic materials. It is used in conjunction with the viscoelastic material models and the Narayanaswamy thermal rheologically simple shift function. The fictive temperature is stored in the second state variable and can be postprocessed by selecting post code 29. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words VISCEL EXP.

2nd data block 1-5

1st

I

Enter the number of materials to be defined.

6-10

2nd

I

Enter the unit number for input. Defaults to input.

3rd data block

Main Index

1-5

1st

I

Material number for cross-referencing with the instantaneous and time dependent viscoelastic properties.

6-15

2nd

E

Enter the solid coefficient of thermal expansion,

16-25

3rd

E

Enter the liquid coefficient of thermal expansion,

αg . αl .

Chapter 3: Model Definition Options 979 Dynamic Analysis

Chapt Dynamic Analysis er 3: This section describes the data input required for dynamic analysis. There are several options available specifying the initial conditions of the problem. The mass density of the object is specified through Mode for any of the material options. Marc uses this to calculate a consistent mass matrix, which can be converted into a diagonal mass matrix by using the LUMP parameter. This is not recommended for either higherl order elements or shells and beams. In addition, you can apply concentrated masses to particular degrees Defini of freedom using options given in this section. Damping can be specified through either the DAMPING or COEFFICIENT option. Note that stiffness damping should not be applied to either the multi-step tion Herrmann elements or the gap elements. Damping is not recommended when using the multi-step Optio Houbolt operator as this method has significant internal damping. If you want to specify material damping, choose another dynamic operator. If you want to specify material damping, choose another ns dynamic operator.Dashpots can be specified through either the SPRINGS, PBUSH, or PFAST option. In addition, the FLUID SOLID option is included so that you can specify the interface between the fluid and solid boundary. If a response spectrum analysis is to be performed, the spectral density is provided through the RESPONSE SPECTRUM option.

Main Index

980 DAMPING Define Damping Factors

DAMPING

Define Damping Factors

Description This option allows the input of damping factors for use with the dynamic analysis options. Two damping inputs are available depending on your choice of dynamic option. For modal superposition analysis, you give the fraction of critical damping associated with each mode of the solution. For direct integration or harmonic analysis, you input the factors weighting the mass and stiffness matrices to form the damping matrix. In both cases, the damping matrix is assumed to be formed as a linear combination of the mass and stiffness matrices of the system, see Marc Volume A: Theory and User Information. There are two styles for defining the damping coefficients for transient dynamics. In the first style, they are associated with element numbers while the second style is based upon material ID. Using the second style, it is possible to associate a table with the damping coefficients. This may be used to allow the coefficients to be a function of the frequency in a harmonic analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word DAMPING.

11-15

2nd

I

Method to read damping data for direct integration dynamics or harmonics; default = 1. Default; not used for modal analysis, the second data block is used. Enter 1; damping is given on a element basis, data blocks 3, 4, and 5 are used. Enter 2; damping is given based upon the material id, data blocks 3, 6, and 7.

2nd data block For dynamic type 1, transient analysis by modal superposition only. 1-10

1st

F

Fraction of critical damping for 1st mode.

11-20

2nd

F

Fraction of critical damping for 2nd mode.

Etc.

Etc.

Etc.

Etc.

3th data block For direct integration (Newmark-beta, Houbolt, generalized alpha, or central difference) or harmonics.

Main Index

1-5

1st

I

Number of damping sets (NDMPST) to be read in. Either the 4th and 5th data blocks or the 6th and 7th data blocks are given in pairs NDMPST times. Optional.

6-10

2nd

I

Enter the unit number for input of the damping data, defaults to input.

DAMPING 981 Define Damping Factors

Format Fixed

Free

Data Entry Entry

4th data block Use 4th and 5th data blocks if method is 0 or 1 (1st data block, 2nd field). 1-10

1st

F

Multiplier (α) for mass matrix contribution to damping matrix.

11-20

2nd

F

Multiplier (β) for stiffness matrix contribution to damping matrix.

21-30

3rd

F

Multiplier (γ) for numerical damping.

5th data block 1-5

1st

I

First element to have these damping values.

6-10

2nd

I

Last element to have these damping values.

6th data block Use the 6th and 7th data blocks if input method is 2 (1st data block, 2nd field). 1-5

1st

I

Enter the material ID.

6-15

2nd

F

Multiplier (α) for mass matrix contribution to damping matrix.

16-25

3rd

F

Multiplier (β) for stiffness matrix contribution to damping matrix.

26-35

4th

F

Multiplier (γ) for numerical damping.

7th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter the table ID associated with the mass matrix coefficient.

11-15

3rd

I

Enter the table ID associated with the stiffness matrix coefficient.

16-20

4th

I

Enter the table ID associated with the numerical damping coefficient.

In a dynamic analysis, the damping matrix is evaluated as: γ Δt C = αM + ⎛ β + --------⎞ K ⎝ π ⎠

In a harmonic analysis, the damping matrix is evaluated as: 2γ C = αM + ⎛⎝ β + ------⎞⎠ K ω

Main Index

982 FLUID SOLID Define Fluid-Solid Interface

FLUID SOLID

Define Fluid-Solid Interface

Description This option is used with the added mass approach to fluid-solid problems. In such analysis, the fluid is considered incompressible and inviscid. This model definition set is necessary to identify the element faces in the solid which abut the fluid. Note that with this feature, the fluid density is entered on the ISOTROPIC option in the Young’s modulus field for the fluid elements. The fluid region is modeled using heat transfer elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words FLUID SOLID.

2nd data block One data line per solid/fluid interface pair – for each abutting pair specify:

Main Index

1-5

1st

I

Solid element number.

6-10

2nd

I

Solid element face number (as identified for distributed load option).

11-15

3rd

I

Fluid element number.

16-20

4th

I

Fluid element face number (as identified in distributed flux option).

INITIAL DISP (with TABLE Input) 983 Define Initial Displacements

INITIAL DISP (with TABLE Input)

Define Initial Displacements

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides initial displacements for dynamic problems or a spatially varying interference fit in contact analyses. The USINC user subroutine or the TABLE model definition can be used to enter spatially varying initial conditions. The data specified here must be activated using the LOADCASE model definition option. To obtain the initial displacement from the calculated value of a previous analysis, use the PRE STATE option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL DISP.

2nd data block 1-5

1st

I

Enter the number of sets of initial displacements (optional).

6-10

2nd

I

Enter file number for input of initial displacement data, defaults to input.

Data blocks 3 through 7 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the USINC user subroutine is required for this initial condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

984 INITIAL DISP (with TABLE Input) Define Initial Displacements

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Initial displacement in first degree of freedom or the interference fit normal to the contact surface.

11-20

2nd

F

Initial displacement in second degree of freedom.

21-30

3rd

F

Initial displacement in third degree of freedom.

31-40

4th

F

Initial displacement in fourth degree of freedom.

41-50

5th

F

Initial displacement in fifth degree of freedom.

51-60

6th

F

Initial displacement in sixth degree of freedom.

61-70

7th

F

Initial displacement in seventh degree of freedom.

71-80

8th

F

Initial displacement in eighth degree of freedom.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

16-20

4th

I

Table ID associated with the fourth degree of freedom.

21-25

5th

I

Table ID associated with the fifth degree of freedom.

26-30

6th

I

Table ID associated with the sixth degree of freedom.

31-35

7th

I

Table ID associated with the seventh degree of freedom.

36-40

8th

I

Table ID associated with the eighth degree of freedom.

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs

Main Index

INITIAL DISP (with TABLE Input) 985 Define Initial Displacements

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

986 INITIAL DISP Define Initial Displacements

INITIAL DISP

Define Initial Displacements

The information provided here is based upon not using the table driven input style. Description This option provides initial displacements for dynamic problems or a spatially varying interference fit in contact analyses. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL DISP.

I

Enter the number of sets of prescribed displacements (optional).

2nd data block 1-5

1st

If a -1 is entered, the USINC user subroutine is used for all nodes. Data blocks 3 and 4 are not required. 6-10

2nd

I

Enter file number for input of prescribed displacement data, defaults to input.

3rd data block 1-10

1st

F

Initial displacement in first degree of freedom or the interference fit normal to the contact surface.

11-20

2nd

F

Initial displacement in second degree of freedom.

21-30

3rd

F

Initial displacement in third degree of freedom.

31-40

4th

F

Initial displacement in fourth degree of freedom.

41-50

5th

F

Initial displacement in fifth degree of freedom.

51-60

6th

F

Initial displacement in sixth degree of freedom.

61-70

7th

F

Initial displacement in seventh degree of freedom.

71-80

8th

F

Initial displacement in eighth degree of freedom.

Continuation data lines, if necessary, must be in 6E10.3 format. Continuation data lines are needed if there are more than eight degrees of freedom per node in the analysis. 4th data block Enter list of nodes for which the above initial displacements are applied.

Main Index

INITIAL VEL (with TABLE Input) 987 Define Initial Velocity

INITIAL VEL (with TABLE Input)

Define Initial Velocity

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows the input of initial velocity for dynamic problems. The data specified here must be activated using the LOADCASE model definition option. To obtain the initial displacement from the calculated value of a previous analysis, use the PRE STATE option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL VEL.

2nd data block 1-5

1st

I

Enter the number of sets of initial velocity (optional).

6-10

2nd

I

Enter unit number for input of initial velocity data, defaults to input.

Data blocks 3 through 7 are entered as pairs; one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the USINC user subroutine required for this initial condition.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

4th data block

Main Index

1-10

1st

E

Initial velocity in first degree of freedom.

11-20

2nd

E

Initial velocity in second degree of freedom.

988 INITIAL VEL (with TABLE Input) Define Initial Velocity

Format Fixed

Free

Data Entry Entry

21-30

3rd

E

Initial velocity in third degree of freedom.

31-40

4th

E

Initial velocity in fourth degree of freedom.

41-50

5th

E

Initial velocity in fifth degree of freedom.

51-60

6th

E

Initial velocity in sixth degree of freedom.

61-70

6th

E

Initial velocity in seventh degree of freedom.

71-80

6th

E

Initial velocity in eighth degree of freedom.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

16-20

4th

I

Table ID associated with the fourth degree of freedom.

21-25

5th

I

Table ID associated with the fifth degree of freedom.

26-30

6th

I

Table ID associated with the sixth degree of freedom.

31-35

7th

I

Table ID associated with the seventh degree of freedom.

36-40

8th

I

Table ID associated with the eighth degree of freedom.

I

Enter the geometry type:

6th data block 1-5

1st

1: Element IDs 2: Node IDs 3: Volume/Region/Body ids 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention 7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

INITIAL VEL 989 Define Initial Velocity

INITIAL VEL

Define Initial Velocity

The information provided here is based upon not using the table driven input style. Description This option allows the input of initial velocity for dynamic problems. Format Entry Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL VEL.

I

Enter the number of sets of prescribed velocity (optional).

2nd data block 1-5

1st

Enter -1 if the USINC user subroutine is to be used for all nodes. In this case, data blocks 3 and 4 are not used. 6-10

2nd

I

Enter unit number for input of prescribed velocity data, defaults to input.

The 3rd and 4th data blocks are entered as pairs; one for each data set. 3rd data block 1-10

1st

E

Initial velocity in first degree of freedom.

11-20

2nd

E

Initial velocity in second degree of freedom.

21-30

3rd

E

Initial velocity in third degree of freedom.

31-40

4th

E

Initial velocity in fourth degree of freedom.

41-50

5th

E

Initial velocity in fifth degree of freedom.

51-60

6th

E

Initial velocity in sixth degree of freedom.

61-70

7th

E

Initial velocity in seventh degree of freedom.

71-80

8th

E

Initial velocity in eighth degree of freedom.

Continuation data lines, if necessary, must be in 6E10.3 format. Continuation data lines are needed if there are more than eight degrees of freedom per node in the analysis. 4th data block Enter list of nodes for which the above initial velocities are applied.

Main Index

990 FIXED ACCE Define Fixed Acceleration

FIXED ACCE

Define Fixed Acceleration

Description This option defines the fixed accelerations that each specified degree of freedom must take during the first and subsequent increments, unless it is further modified using the ACC CHANGE option. This option can only be used in dynamic analyses. It is usually used to prescribe base motion accelerations. Further detail is given in Marc Volume A: Theory and User Information. See Marc Volume B: Element Library, for a definition of the degrees of freedom for each element type. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED ACCE.

I

Number of sets of boundary condition data lines to be read (optional).

2nd data block 1-5

1st

For each set of boundary conditions, use the 3rd, 4th and 5th data blocks. 3d data block 1-10

1st

E

Prescribed acceleration for first degree of freedom listed in data block 4.

11-20

2nd

E

Prescribed acceleration for second degree of freedom listed in data block 4.

21-30

3rd

E

Prescribed acceleration for third degree of freedom listed in data block 4.

4th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes to which the above accelerations are applied.

Main Index

MASSES 991 Define Concentrated Masses

MASSES

Define Concentrated Masses

Description This option is used to input any concentrated masses for use with the dynamic analysis options. Each concentrated mass is associated with a single degree of freedom. Note:

Rotational degrees of freedom might have mass depending on the element types used in the data.

In a coupled analysis, the lumped capacitance is the concentrated mass multiplied with the lumped capacitance factor, if the lumped mass is given or is the lumped capacitance itself. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word MASSES.

2nd data block 1-5

1st

I

Number of sets of data used to enter mass points (optional).

6-10

2nd

I

Enter unit number for reading mass point data. Defaults to input.

3rd data block 1-5

1st

I

Degree of freedom to which mass is applied.

6-15

2nd

F

Value of concentrated mass.

16-25

3rd

F

Value of concentrated damper.

26-35

4th

F

Lumped capacitance (factor).

36-40

5th

I

Table ID for concentrated mass.

41-45

6th

I

Table ID for concentrated damper.

46-50

7th

I

Table ID for lumped capacitance.

4th data block Enter a list of nodes having the above concentrated masses.

Main Index

992 CONM1 Define a General Concentrated Mass

CONM1

Define a General Concentrated Mass

Description Define a general concentrated mass to be applied to a node. Either a diagonal or a symmetric 6 x 6 mass matrix may be defined with respect to a local coordinate system. This mass is used in dynamic or harmonic analyses only. The TABLE option may be used in conjunction with this option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONM1.

2nd data block 1-5

1st

I

Number of distinct sets of CONM1 entries.

6-10

2nd

I

Enter unit number for input of CONM1 data (default to standard input).

11-15

3rd

I

Enter 1 to suppress printout.

3rd data block 1-5

1st

I

Enter Coordinate System ID (integer ≥ 0).

6-10

2nd

I

Enter method by which mass terms are specified. 1 = only diagonal masses specified on 4a – 5a data blocks. 2 = full 6 x 6 mass specified on 4b – 9b data blocks.

11-15

3rd

I

Enter method by which damping terms are specified. 1 = only diagonal damping specified on 10a – 11a data blocks. 2 = full 6 x 6 damping specified on 10b – 15b data blocks.

16-20

4th

I

Enter method by which capacitance terms are specified. 1 = thermal capacitance factor specified on data block 16a. 2 = thermal capacitance factor specified on data block 16b. 3 = absolute thermal capacitance specified on data block 16a. 4 = absolute thermal capacitance specified on data block 16b.

If the 2nd field of the 3rd data block = 1, include the 4a and 5a data blocks. 4a data block

Main Index

1-10

1st

E

M11

11-20

2nd

E

M22

21-30

3rd

E

M33

CONM1 993 Define a General Concentrated Mass

Format Fixed

Free

Data Entry Entry

31-40

4th

E

M44

41-50

5th

E

M55

51-60

6th

E

M66

5a data block 1–5

1st

I

Table ID for M11.

6-10

2nd

I

Table ID for M22.

11-15

3rd

I

Table ID for M33.

16-20

4th

I

Table ID for M44.

21-25

5th

I

Table ID for M55.

26-30

6th

I

Table ID for M66.

If the 2nd field of the 3rd data block = 2; for 2-D simulation, include the 4b and 5b data blocks (see Remark 2). If the 2nd field of the 3rd data block = 2; for 3-D simulation, include the 4b through 9b data blocks. 4b data block 1-10

1st

E

M11

11-20

2nd

E

M21

21-30

3rd

E

M22

31-40

4th

E

M31

41-50

5th

E

M32

51-60

6th

E

M33

61-70

7th

E

M41

5b data block 1–5

1st

I

Table ID for M11.

6-10

2nd

I

Table ID for M21.

11-15

3rd

I

Table ID for M22.

16-20

4th

I

Table ID for M31.

21-25

5th

I

Table ID for M32.

26-30

6th

I

Table ID for M33.

31-35

7th

I

Table ID for M41.

6b data block

Main Index

1-10

1st

E

M42

11-20

2nd

E

M43

994 CONM1 Define a General Concentrated Mass

Format Fixed

Free

Data Entry Entry

21-30

3rd

E

M44

31-40

4th

E

M51

41-50

5th

E

M52

51-60

6th

E

M53

61-70

7th

E

M54

7b data block 1–5

1st

I

Table ID for M42.

6-10

2nd

I

Table ID for M43.

11-15

3rd

I

Table ID for M44.

16-20

4th

I

Table ID for M51.

21-25

5th

I

Table ID for M52.

26-30

6th

I

Table ID for M53.

31-35

7th

I

Table ID for M54.

8b data block 1-10

1st

E

M55

11-20

2nd

E

M61

21-30

3rd

E

M62

31-40

4th

E

M63

41-50

5th

E

M64

51-60

6th

E

M65

61-70

7th

E

M66

9b data block 1–5

1st

I

Table ID for M55.

6-10

2nd

I

Table ID for M61.

11-15

3rd

I

Table ID for M62.

16-20

4th

I

Table ID for M63.

21-25

5th

I

Table ID for M64.

26-30

6th

I

Table ID for M65.

31-35

7th

I

Table ID for M66.

If the 3rd field of the 3rd data block = 1, include the 10a and 11a data blocks.

Main Index

CONM1 995 Define a General Concentrated Mass

Format Fixed

Free

Data Entry Entry

10a data block 1-10

1st

E

D11

11-20

2nd

E

D22

21-30

3rd

E

D33

31-40

4th

E

D44

41-50

5th

E

D55

51-60

6th

E

D66

11a data block 1–5

1st

I

Table ID for D11.

6-10

2nd

I

Table ID for D22.

11-15

3rd

I

Table ID for D33.

16-20

4th

I

Table ID for D44.

21-25

5th

I

Table ID for D55.

26-30

6th

I

Table ID for D66.

If the 2nd field of the 3rd data block = 2; for 2-D simulation, include the 10b and 11b data blocks (see Remark 2). If the 2nd field of the 3rd data block = 2; for 3-D simulation, include the 10b through 15b data blocks. 10b data block 1-10

1st

E

D11

11-20

2nd

E

D21

21-30

3rd

E

D22

31-40

4th

E

D31

41-50

5th

E

D32

51-60

6th

E

D33

61-70

7th

E

D41

11b data block

Main Index

1–5

1st

I

Table ID for D11.

6-10

2nd

I

Table ID for D21.

11-15

3rd

I

Table ID for D22.

16-20

4th

I

Table ID for D31.

996 CONM1 Define a General Concentrated Mass

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Table ID for D32.

26-30

6th

I

Table ID for D33.

31-35

7th

I

Table ID for D41.

12b data block 1-10

1st

E

D42

11-20

2nd

E

D43

21-30

3rd

E

D44

31-40

4th

E

D51

41-50

5th

E

D52

51-60

6th

E

D53

61-70

7th

E

D54

13b data block 1–5

1st

I

Table ID for D42.

6-10

2nd

I

Table ID for D43.

11-15

3rd

I

Table ID for D44.

16-20

4th

I

Table ID for D51.

21-25

5th

I

Table ID for D52.

26-30

6th

I

Table ID for D53.

31-35

7th

I

Table ID for D54.

14b data block 1-10

1st

E

D55

11-20

2nd

E

D61

21-30

3rd

E

D62

31-40

4th

E

D63

41-50

5th

E

D64

51-60

6th

E

D65

61-70

7th

E

D66

15b data block

Main Index

1–5

1st

I

Table ID for D55.

6-10

2nd

I

Table ID for D61.

11-15

3rd

I

Table ID for D62.

16-20

4th

I

Table ID for D63.

CONM1 997 Define a General Concentrated Mass

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Table ID for D64.

26-30

6th

I

Table ID for D65.

31-35

7th

I

Table ID for D66.

If the 4th field of the 3rd data block = 1 or 2, include the 16a data block. 16a data block 1-10

1st

E

CP (will be multiplied by M11).

11-15

2nd

I

Table ID for CP.

If the 4th field of the 3rd data block = 3 or 4, include the 16b data block. 16b data block 1-10

1st

E

MCP

11-15

2nd

I

Table ID for MCP.

17th data block Enter a list of nodes. Remarks 1. The COORD SYSTEM ID is an integer that is ≥ 0. ID = 0 means that the mass and damping matrix are defined in the global Cartesian system. ID > 0 means that the mass matrix is in a user-defined coordinate system with the same number. 2. For 2-D problems, if the diagonal form is specified, then only M11, M22, and M33 (if rotation degree of freedom is included) are defined. If the full form is specified and there are no rotational degrees of freedom, then M11, M21, and M22 are supported. If the full form is specified and there are rotational degrees of freedom, then M11, M21, M22, M31, M32, and M33 are supported. 3. For heat transfer shells, CP11 is applied to all degrees of freedom through the thickness.

Main Index

998 CONM2 Define a Diagonal Mass/Moment of Inertia

CONM2

Define a Diagonal Mass/Moment of Inertia

Description Define a concentrated diagonal mass contribution and the mass moment of inertia with respect to a local coordinate system. The mass is used in dynamic and harmonic analysis only. The TABLE option may be used in conjunction with this option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONM2.

2nd data block 1-5

1st

I

Number of distinct sets of CONM2 entries.

6-10

2nd

I

Enter unit number for input of CONM2 data (default to standard input).

11-15

3rd

I

Enter 1 to suppress printout.

3rd data block 1-5

1st

I

Enter Coordinate System ID (integer ≥ -1).

6-15

2nd

E

Offset distance component X1.

16-25

3rd

E

Offset distance component X2.

26-35

4th

E

Offset distance component X3.

36-40

5th

I

Table ID for X1.

41-45

6th

I

Table ID for X2.

46-50

7th

I

Table ID for X3.

4th data block

Main Index

1-10

1st

E

M

11-20

2nd

E

I11

21-30

3rd

E

I21

31-40

4th

E

I22

41-50

5th

E

I31

51-60

6th

E

I32

61-70

7th

E

I33

CONM2 999 Define a Diagonal Mass/Moment of Inertia

Format Fixed

Free

Data Entry Entry

5th data block 1–5

1st

I

Table ID for M.

6-10

2nd

I

Table ID for I11.

11-15

3rd

I

Table ID for I21.

16-20

4th

I

Table ID for I22.

21-25

5th

I

Table ID for I31.

26-30

6th

I

Table ID for I32.

31-35

7th

I

Table ID for I33.

6th data block Enter a list of nodes. Remarks 1. The COORD SYSTEM ID is an integer that is ≥ -1. ID = -1 or = 0 both mean that the mass and moments of inertia defined in the 4th data block are in the global Cartesian coordinate system. ID = -1 means that X1, X2, and X3 are the coordinates of the center of gravity in the global Cartesian system. ID = 0 means that X1, X2, and X3 are the offset distances from the grid point in the global Cartesian system. ID > 0 means that the mass and moments of inertia defined in the 4th data block are in the user-defined coordinate system with the same ID. Also, X1, X2, and X3 are the offset distances from the grid point in the same user system. 2. In 2-D problems, M, I33, X1, and X2 alone will need to be entered.

Main Index

1000 RESPONSE SPECTRUM Define Density for Spectral Response

RESPONSE SPECTRUM

Define Density for Spectral Response

Description This option allows you to define the response spectral density. Note that the RESPONSE parameter must also be included. A spectrum response calculation is performed based on the last set of extracted modes when a SPECTRUM history definition option is encountered. Format Format Fixed

Free

Data Entry Entry

1st data block 1-20

A

Enter the words RESPONSE SPECTRUM.

1-5

I

Enter the number of spectral density pairs (optional).

6-10

I

Enter the unit number to read data. Default is to input.

1-10

F

Enter the frequency in cycles per time unit.

11-20

F

Enter the displacement spectral response density.

2nd data block

3rd data block

Main Index

MODAL INCREMENT 1001 Define Increments for Eigenvalue Extraction

MODAL INCREMENT

Define Increments for Eigenvalue Extraction

Description This option allows you to specify at which increments an eigenvalue extraction is performed. It can be used as either a replacement to the MODAL SHAPE history definition option or in conjunction with it. This option allows you to extract modes within an AUTO LOAD, AUTO STEP, AUTO CREEP, or AUTO INCREMENT period. Note that the increment numbers specified here cannot be changed upon restart. Format Format Fixed

Free

Data Entry Entry

1st data block 1-20

1st

A

Enter the words MODAL INCREMENT.

2a data block Data block 2a is used if the inverse power sweep method is selected on the DYNAMIC parameter.

Main Index

1-5

1st

I

Maximum number of iterations per mode in the power sweep. Maximum number of iterations for all modes if subspace iteration is used. Default is 40.

6-15

2nd

F

Convergence tolerance. The power sweep terminates when the difference between the eigenvalues in two consecutive sweeps divided by the eigenvalue is less than the tolerance. Default is 0.0001.

16-25

3rd

F

Initial shift in cycles per time. The power shift is likely to start converging to the eigenvalue closest to this value. Default is 0.

26-35

4th

F

Maximum frequency to be extracted in cycles per time. If this is left blank or zero, the number of modes requested on the DYNAMIC parameter are extracted. If this is nonzero, the extraction ends when this frequency is exceeded or when the number of modes requested on the DYNAMIC parameter is reached, whichever occurs first.

36-40

5th

I

Number of modes extracted per shift. This data field determines if auto shifting occurs. If auto shift is not required, set equal to or greater than number of modes requested on DYNAMIC parameter. Default is 5.

41-50

6th

F

Auto shift parameter. Marc determines the new shift point (in frequency squared) as the highest frequency square plus this entry times the difference between the highest and next highest distinct frequency squared. Default is 1.0.

51-55

7th

I

Enter 1 if eigenvectors are to be written to the post file.

1002 MODAL INCREMENT Define Increments for Eigenvalue Extraction

Format Fixed

Free

Data Entry Entry

2b data block Data block 2b is used if the Lanczos method is selected on the DYNAMIC parameter. 1-10

1st

F

SHFMIN, lowest frequency of mode to be extracted (in cycles/time). This is also the initial shift point. The shift point is SHFMIN∗SHFMIN. If a negative frequency is given, shift point is -SHFMIN∗SHFMIN. This cannot be changed upon restart.

11-20

2nd

F

SHFMAX, highest frequency of modes to be extracted. If set to 0, NSNRM modes are extracted. If not set to zero, all modes between SHFMIN and SHFMAX are extracted and NSNRM is not used. A Strum sequence check is performed to calculate this number. This can be changed upon restart.

21-25

3rd

I

NSNRM, number of requested modes. Only needed if SHFMAX is set equal to 0. This can be increased upon restart.

26-30

4th

I

Not used; enter 0.

31-35

5th

I

Not used; enter 0.

36-40

6th

I

Enter 1 if eigenvectors are to be written to the post file.

3rd data block Enter a list of increment numbers at which modes are to be extracted.

Main Index

BUCKLE INCREMENT 1003 Define Increments for Buckling Analysis

BUCKLE INCREMENT

Define Increments for Buckling Analysis

Description This option allows you to specify at which increments a buckling analysis is performed. It can be used as either a replacement to the BUCKLE history definition option or in conjunction with it. This option allows you to extract modes within an AUTO LOAD, AUTO STEP, AUTO CREEP, or AUTO INCREMENT period. Note that the increment numbers specified here cannot be changed upon restart. Perturbation buckling should not be used with Fourier buckling. Format Format Fixed

Free

Data Entry Entry

1st data block 1-20

1st

A

Enter the words BUCKLE INCREMENT.

2nd data block 1-5

1st

I

Maximum number of iterations per mode in the power sweep. Default is 40.

6-15

2nd

F

Convergence tolerance. The power sweep terminates when the difference between the eigenvalues in two consecutive sweeps divided by the eigenvalue is less than the tolerance. Default is 0.0001.

16-20

3rd

I

Enter 1 if Fourier Buckling is to be performed.

21-25

4th

I

Enter 1 if the eigenvectors are to be written to the post file.

26-30

5th

I

Enter 1 for automatic buckling perturbation. Enter 2 for manual buckling perturbation.

31-35

6th

I

Enter buckling mode to be used in perturbation. Enter negative number of modes if multiple modes are used in perturbation.

36-45

7th

F

Enter the scale factor to be multiplied with the normalized buckle mode and added to coordinates.

3rd data block Used only with Fourier buckling. Enter a list of Fourier harmonics at which to perform extractions. Positive numbers are symmetric modes; negative numbers are antisymmetric modes. Data Block 3a is used only if sixth field of the 2nd data block is negative. Use one line for each mode used for perturbation.

Main Index

1004 BUCKLE INCREMENT Define Increments for Buckling Analysis

Format Fixed

Free

Data Entry Entry

3a data block 1-5

1st

I

Mode number.

6-15

2nd

F

Scale factor.

If automatic buckling perturbation, the fifth field on the 2nd data block equals one, do not enter the 4th data block. 4th data block Enter a list of increment numbers at which modes are to be extracted.

Main Index

Chapter 3: Model Definition Options 1005 Heat Transfer Analysis

Chapt Heat Transfer Analysis er 3: This section describes the input of material data and boundary conditions applicable for heat transfer The boundary conditions discussed in this section are also used for coupled thermalMode problems. mechanical problems or coupled fluid-thermal problems. The ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC options are used to define the conductivity, specific heat and density. If these material l properties are influenced with temperature, this variation can be prescribed by the TABLE, Defini TEMPERATURE EFFECTS or ORTHO TEMP options. In problems where temperature effects are important, a steady-state analysis performed in one increment requires recycling. A transient analysis tion recycles and reassembles based upon the tolerances given in the CONTROL option. The initial Optio temperatures can be prescribed using INITIAL TEMP option. Surface, volumetric or nodal fluxes can be prescribed and convective boundary conditions can be imposed through the FILMS option. ns In Heat Transfer Analysis, data for POINT FLUX, DIST FLUXES, and QVECT should be prescribed as total rather than incremental quantity (as used in Mechanical Analysis). This specification is to be used consistently for the heat transfer portion of analysis in coupled thermal-mechanical (thermal-solid), fluidthermal, and fluid-thermal-solid.

Main Index

1006 FIXED TEMPERATURE (with TABLE Input) Define Fixed Temperature

FIXED TEMPERATURE (with TABLE Input)

Define Fixed Temperature

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the temperature that each node must take. The boundary conditions are specified either by giving the temperature and either a list of nodal numbers, or a list of geometric entries. The prescribed temperature is associated with a boundary condition name and is activated with the LOADCASE history definition option. Note that unless heat transfer shell elements are used, there is only one degree of freedom in a heat transfer analysis. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED TEMPERATURE.

2nd data block 1-5

1st

I

Number of sets of boundary conditions to be read (optional).

6-10

2nd

I

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Maximum number of degrees of freedom specified on the 4th, 5th, and 6th data blocks for heat transfer shells if the number of degrees of freedom is greater than 8.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter a 1 if first prescribed temperature entered is to be applied for all DOF of a heat transfer shell.

FIXED TEMPERATURE (with TABLE Input) 1007 Define Fixed Temperature

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

For conventional heat transfer element, only one degree of freedom is required. For heat transfer shell elements, the 4th, 5th, and 6th data blocks are repeated to satisfy the maximum number specified on the 4th field of the 3rd data block. A maximum of eight degrees of freedom per data block. 4th data block 1-10

1st

F

Prescribed temperature for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed temperature for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed temperature for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed temperatures are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface ids 5: Curve IDs 6: Point IDs 11 Element-Edges IDs

Main Index

1008 FIXED TEMPERATURE (with TABLE Input) Define Fixed Temperature

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED TEMPERATURE 1009 Define Fixed Temperature

FIXED TEMPERATURE

Define Fixed Temperature

The information provided here is based upon not using the table driven input style. Description This option defines the fixed temperature that each node must take during the first and subsequent increments, unless it is further modified using the TEMP CHANGE option. The boundary conditions are specified either by giving the temperature and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Note:

The boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definitions must be arranged accordingly.

For each set of boundary conditions, use the 3a and 4a data blocks or the 3b, 4b, and 5b blocks. (3a); (4a) For analyses which do not include heat transfer shell elements. Format Format Fixed

Free

Data Entry Entry

‘

1st data block 1-19

1st

A

Enter the words FIXED TEMPERATURE.

2nd data block 1-5

1st

I

Number of sets of boundary conditions to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option.

11-15

3rd

I

Unit number used for MESH2D option.

Use 3a,4a for analyses which do not include heat transfer shell elements. 3a data block 1-10

1st

F

Prescribed temperature.

4a data block Enter a list of nodes for which the above temperature is applied.

Main Index

1010 FIXED TEMPERATURE Define Fixed Temperature

Format Fixed

Free

Data Entry Entry

‘

3b data block Use 3b, 4b, and 5b for analyses which include heat transfer shell elements. 1-10

1st

F

Prescribed temperature for first degree of freedom listed in data block 4b.

11-20

2nd

F

Prescribed temperature for second degree of freedom listed in data block 4b.

21-30

3rd

F

Prescribed temperature for third degree of freedom listed in data block 4b. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

4b data block Enter a list of degrees of freedom to which the above prescribed temperatures are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above boundary conditions are applied.

Main Index

FILMS (with TABLE Input - Model Definition) 1011 Define Thermal Boundary Conditions

FILMS (with TABLE Input - Model Definition)

Define Thermal Boundary Conditions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows the input of convection, natural convection, radiation, and applied fluxes on the surface of the model. The user defines the film coefficients, sink temperatures, and fluxes here. Nonuniform films or sink temperatures can be obtained via the UFILM user subroutine (see Marc Volume D: User Subroutines and Special Routines) or by using the TABLE model definition option. As an alternative, the sink temperatures may be prescribed using the SINK POINTS option. This option may also be used to specify a radiation to the environment. The convective boundary condition is associated with a boundary condition name that is activated and deactivated by the LOADCASE history definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word FILMS.

2nd data block 1-5

1st

I

Number of sets of data used to input film (optional).

6-10

2nd

I

Unit number for input of film data, defaults to input.

Data blocks 3 through 8 are entered for each film input. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define film boundary condition. See 7th and 8th data blocks.

6-10

2nd

I

Enter the sum of FILMTYP + TEMTYP where: FILMTYP = 0 if no user subroutine is required. FILMTYP = 1 if the UFILM user subroutine is required for this boundary condition. FILMTYP = 4 if a control node is to be used. FILMTYP = 6 if the environment temperature is a function of the temperature of the control node.

Main Index

1012 FILMS (with TABLE Input - Model Definition) Define Thermal Boundary Conditions

Format Fixed

Free

Data Entry Entry TEMTYP = 0 if temperature dependent convective coefficients based upon temperature at the surface is used. TEMTYP = 10 if temperature dependent convective coefficients based upon average of the temperature of the surface temperature and the ambient temperature is used. TEMTYP = 20 if temperature dependent convective coefficients based upon the ambient temperature is used. Note:

The TEMPTYP 0 and 10 are opposite of the MD Nastran convention, but are necessary to maintain backward compatibility with Marc input files.

11-15

3rd

I

If FILMTYP = 4 or 6, enter the control node to be used.

16-20

4th

I

Enter 0 if environment temperature obtained from 4th data block. Enter the group number containing the sink points which will be used to obtain the environment temperature. If the sink points do not belong to any group, enter 1.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter -1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

If a control node is used (see 4th field) or convection nodes are used (see 5th and 6th fields), the first degree of freedom of this node will always be used even if this node is associated with a heat transfer shell element. 4th data block 1-10

1st

F

Reference value of film coefficient.

11-20

2nd

F

Reference value of sink temperature (reference values can be modified by the UFILM user subroutine). If convection is specified to a node(s), this value is ignored.

21-30

3rd

F

Enter the magnitude of externally applied distributed flux.

31-40

4th

F

Reference value of the film coefficient for natural convection.

41-50

5th

F

Enter the exponent for natural convection.

51-60

6th

F

Enter the emissivity.

61-70

7th

F

Effective View factor (default = 1.0).

5th data block - Table IDs

Main Index

1-5

1st

I

Enter the table ID associated with the film coefficient.

6-10

2nd

I

Enter the table ID associated with the sink temperature.

FILMS (with TABLE Input - Model Definition) 1013 Define Thermal Boundary Conditions

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter the table ID associated with the distributed flux.

16-20

4th

I

Enter the table ID associated with the natural convection.

21-25

5th

I

Enter the table ID associated with the exponent for natural convection.

26-30

6th

I

Enter the table ID for emissivity.

31-35

7th

I

Enter the table ID for view factor.

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 01: Normal flux (bottom surface for shells) 10: Normal flux (top surface for shells)

11-15

3rd

I

Enter the face ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID

Main Index

1014 FILMS (with TABLE Input - Model Definition) Define Thermal Boundary Conditions

Format Fixed

Free

Data Entry Entry 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

FILMS (Model Definition) 1015 Define Convection Film Coefficient Input

FILMS (Model Definition)

Define Convection Film Coefficient Input

The information provided here is based upon not using the table driven input style. Description This option allows film coefficients and associated sink temperatures to be input. Nonuniform films or sink temperatures can be obtained via the FILM user subroutine (see Marc Volume D: User Subroutines and Special Routines). Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word FILMS.

2nd data block 1-5

1st

I

Number of sets of data used to input film (optional).

6-10

2nd

I

Unit number for input of film data, defaults to input.

3rd data block 1-5

1st

I

Face identification. Same as for the FLUX user subroutine – see Marc Volume B: Element Library.

6-15

2nd

F

Reference value of film coefficient.

16-25

3rd

F

Reference value of sink temperature (reference values can be modified by the FILM user subroutine).

26-30

4th

I

Film coefficient index (optional).

31-35

5th

I

Sink temperature index (optional). (Film coefficient and sink temperature indices are to be used in the FILM user subroutine).

4th data block Enter a list of elements to which the above film data is applied.

Main Index

1016 SINK POINTS (with TABLE Input - Model Definition) Define Sink Points

SINK POINTS (with TABLE Input - Model Definition)

Define Sink Points

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option is used to define the temperature at arbitrary points in the environment. The radiative and convective thermal fluxes as entered through the FILMS option are based upon these values. These temperatures may change with time by using either the TABLE model definition option or the USINKPT user subroutine. The program uses the closest eligible sink point to the surface integration point. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SINK POINTS.

2nd data block 1-5

1st

I

Enter the number of sink point groups to be entered.

6-10

2nd

I

Enter the unit number used to read the sink points.

11-15

3rd

I

Enter a 1 to print out sink point data.

16-20

4th

I

Enter the number of real variables associated with sink point, default is 1 (temperature), maximum is 8.

3rd data block 1-10

1st

A

Enter the word GROUP.

11-15

2nd

I

Enter the group number. Default is 1.

16-20

3rd

I

Enter a 1 if the USINKPT user subroutine is used.

Repeat data blocks 4 through 6 for each sink point in this group. 4th data block

Main Index

1-5

1st

I

Enter the sink point id. Only used for the USINKPT user subroutine; otherwise could be zero.

6-15

2nd

E

Enter the first coordinate of sink point.

16-25

3rd

E

Enter the second coordinate of sink point.

26-35

4th

E

Enter the third coordinate of sink point.

SINK POINTS (with TABLE Input - Model Definition) 1017 Define Sink Points

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

E

Enter the sink temperature.

11-20

2nd

E

Enter the second sink variable if the 2nd data block, 4th field is greater than 1. etc.

6th data block 1-5

1st

I

Enter the table ID associated with the sink temperature.

6-10

2nd

I

Enter the table ID associated with the second sink variable if required. etc.

Main Index

1018 DIST FLUXES (with TABLE Input - Model Definition) Define Distributed Fluxes

DIST FLUXES (with TABLE Input - Model Definition)

Define Distributed Fluxes

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines total distributed (surface and volumetric) fluxes by giving the magnitude, location, and associating the information with a boundary condition name. Distributed fluxes are converted to consistent nodal fluxes by Marc. Note that for a given element type, there is an established convention for the application of surface flux on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent fluxes. The applied flux is associated with a boundary condition name that is activated with the LOADCASE history definition option. Note:

If a distributed flux is applied on the bottom of a shell, the flux is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST FLUXES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed flux data, defaults to input.

Data blocks 3 through 8 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter the FLUXTYPE: FLUXTYPE = 0 if no user subroutine is required. FLUXTYPE = 1 if the FLUX user subroutine is required for this boundary condition. FLUXTYPE = 4 if the distributed flux is dependent on a control node.

Main Index

DIST FLUXES (with TABLE Input - Model Definition) 1019 Define Distributed Fluxes

Format Fixed

Free

Data Entry Entry FLUXTYPE = 6 If the tables used to describe a temperature dependent flux are based upon the temperature at the control node, as opposed to the temperature at the surface integration point.

11-15

3rd

I

If the FLUXTYPE = 4 or 6, enter the control node to be used.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option. Note:

If a control node is used (see 3rd field), the first degree of freedom of this node will always be used even if this node is associated with a heat transfer shell element.

4th data block (used if FLUXTYPE = 0, 1, or 4) 1-10

1st

F

Enter the magnitude of this type of distributed fluxes.

5th data block (use if FLUXTYPE = 0, 1, or 4 1-5

1st

I

Enter the table ID associated with the distributed flux.

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal flux (bottom surface for shells) 10: Normal flux (top surface for shells)

11-15

3rd

I

Enter the face ID or edge ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs

Main Index

1020 DIST FLUXES (with TABLE Input - Model Definition) Define Distributed Fluxes

Format Fixed

Free

Data Entry Entry 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation Id 17: Curve ID: orientation id 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

DIST FLUXES (Model Definition) 1021 Define Distributed Fluxes

DIST FLUXES (Model Definition)

Define Distributed Fluxes

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) fluxes to be specified. Distributed fluxes are converted to consistent nodal fluxes by Marc. Note that for a given element type, there is an established convention for the application of surface flux on a particular face. The FLUX user subroutine can be used to input time and spatial dependent fluxes. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST FLUXES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed flux data, defaults to input.

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library.

3rd data block 1-5

1st

Also see distributed flux type 101 under the COUPLE parameter definition. 6-15

2nd

F

Enter the magnitude of this type of distributed fluxes.

16-20

3rd

I

Flux index (optional). (Flux index is to be used in the FLUX user subroutine.)

4th data block Enter a list of elements associated with the above distributed fluxes.

Main Index

1022 POINT FLUX (with TABLE Input - Model Definition) Define Point Fluxes

POINT FLUX (with TABLE Input - Model Definition)

Define Point Fluxes

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines total nodal point fluxes by giving the magnitude, location, and associating the information with a boundary condition name. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent fluxes. The applied flux is associated with a boundary condition name that is activated with the LOADCASE history definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of point fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point flux data, defaults to input.

Data blocks 3 through 7 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter the FLUXTYPE: FLUXTYPE = 0 if no user subroutine is required. FLUXTYPE = 1 if the FORCDT user subroutine is required for this boundary condition. FLUXTYPE = 4 if the point flux is dependent on a control node. FLUXTYPE = 6 If the tables used to describe a temperature dependent flux are based upon the temperature at the control node, as opposed to the temperature at which the flux is applied.

Main Index

11-15

3rd

I

If the FLUXTYPE = 4 or 6, enter the control node to be used.

16-20

4th

I

Not used; enter 0.

POINT FLUX (with TABLE Input - Model Definition) 1023 Define Point Fluxes

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter a 1 if first point flux is to be applied to all degrees of freedom of a heat transfer shell.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option. Notes:

If a control node is used (see 3rd field), the first degree of freedom of this node will always be used even if this node is associated with a heat transfer shell element. If fluxes are applied to multiple degrees of freedom of a heat transfer shell element, the control node will be applied to all degrees of freedom.

For conventional heat transfer element, only one degree of freedom is required. For heat transfer shell elements having more than eight degrees of freedom, the 4th and 5th data blocks are repeated as required, giving eight values per set. 4th data block 1-10

1st

F

Magnitude of point flux in first degree of freedom.

11-20

2nd

F

Magnitude of point flux in second degree of freedom.

21-30

3rd

F

Magnitude of point flux in third degree of freedom.

31-40

4th

F

Magnitude of point flux in fourth degree of freedom.

41-50

5th

F

Magnitude of point flux in fifth degree of freedom.

51-60

6th

F

Magnitude of point flux in sixth degree of freedom.

61-70

7th

F

Magnitude of point flux in seventh degree of freedom.

71-80

8th

F

Magnitude of point flux in eighth degree of freedom.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

16-20

4th

I

Table ID associated with the fourth degree of freedom.

21-25

5th

I

Table ID associated with the fifth degree of freedom.

26-30

6th

I

Table ID associated with the sixth degree of freedom.

31-35

7th

I

Table ID associated with the seventh degree of freedom.

36-40

8th

I

Table ID associated with the eighth degree of freedom.

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field.

Main Index

1024 POINT FLUX (with TABLE Input - Model Definition) Define Point Fluxes

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1: Element ids 2: Nodes ids 3: Volume/Region/Body ids 4: Surface ids 5: Curve ids 6: Point ids 11: Element-Edges ids 12: Element-Faces ids 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

POINT FLUX (Model Definition) 1025 Define Point Fluxes

POINT FLUX (Model Definition)

Define Point Fluxes

The information provided here is based upon not using the table driven input style. Description This option allows total nodal point fluxes to be specified. The FORCDT user subroutine can be used for the time dependent fluxes. Enter an upper bound to the number of nodes with point fluxes on the FLUXES parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of point fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point flux data; defaults to input.

3rd data block 1-10

1st

F

Magnitude of point flux.

11-20

2nd

F

Magnitude of point flux for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point flux for third degree of freedom, (heat transfer shell elements only).

4th data block Enter a list of nodes to which the above nodal sources are applied.

Main Index

1026 QVECT (with TABLE Input - Model Definition) Define Thermal Vector Flux Boundary Conditions

QVECT (with TABLE Input Model Definition)

Define Thermal Vector Flux Boundary Conditions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows the input of thermal vector flux from a distant source into one or more elements. Variations may be given by using either a control node, or using tables. The thermal vector flux boundary condition is associated with a boundary condition name that is activated and deactivated by the LOADCASE history definition option. The absorption is defined via the EMISSIVITY option. The total power into an element is given by: P = – α A * ( e * n ) * Q0 ˜ ˜ P = – α A * ( e * n ) * Q0 * U cntr ln d ˜ ˜

if no control node is given or

e ˜ n ˜

is the user-defined direction cosine.

if a control node is given.

is the normal to the surface

If the temperature of the radiant source is given, then all temperature dependent properties will be a function of this temperature. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word QVECT.

2nd data block 1-5

1st

I

Number of sets of data used to input vector flux (optional).

6-10

2nd

I

Unit number for input of vector flux data; defaults to input.

Data blocks 3 through 8 are entered for each vector flux input. 3rd data block

Main Index

1-5

1st

I

Enter the number of geometric types used to define film boundary condition. See 7th and 8th data blocks.

6-10

2nd

I

Enter the sum of VECFLUXTYPE + TEMTYP + ISIDE where:

QVECT (with TABLE Input - Model Definition) 1027 Define Thermal Vector Flux Boundary Conditions

Format Fixed

Free

Data Entry Entry VECFLUXTYPE = 0 if no user subroutine required. VECFLUXTYPE = 1 if the UQVECT user subroutine is required for this boundary condition. VECFLUXTYPE = 4 if a control node is to be used. VECFLUXTYPE = 6 if the table used to describe the temperature dependent flux is based upon the temperature at the control node. TEMTYP=0

if temperature dependent absorption coefficients based upon temperature at the surface.

TEMTYP=10

if temperature dependent absorption coefficients based upon the average of the surface temperature and the source temperature.

TEMTYP=20

if temperature dependent convective coefficients based upon the source temperature.

If

Q(0 > 0)

then,

ISIDE=0

current default - means heat e∗ n < 0 ˜ ˜ subtracted if e∗ n > 0 ˜ ˜

will be added if will be ISIDE=100

means heat will be added if no heat if

ISIDE=200

e∗ n > 0 ˜ ˜

means no heat if

e∗ n < 0 ˜ ˜

heat will be subtracted if ISIDE=300

e∗ n < 0 ˜ ˜

e∗ n > 0 ˜ ˜

means always add heat; this is the same as using absolute value of e∗ n ˜ ˜

11-15

3rd

I

If VECFLUXTYPE =4 or 6, enter the control node to be used.

16-20

4th

I

Emissivity/Absorption ID. The emissivity/Absorption ID is not required but if given, it reduces the amount of memory required for the analysis.

Main Index

21-25

5th

I

Not used, enter 0.

26-30

6th

I

Not used, enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1028 QVECT (with TABLE Input - Model Definition) Define Thermal Vector Flux Boundary Conditions

Format Fixed

Free

Data Entry Entry Note:

It a control node is used (see 3rd field), the first degree of freedom of this node will be always be used even if this node is associated with a heat transfer shell element.

4th data block 1-10

1st

F

Magnitude of the thermal flux into the face.

11-20

2nd

F

Temperature of the radiant source.

21-30

3rd

F

First direction cosine of thermal flux.

31-40

4th

F

Second direction cosine of thermal flux.

41-50

5th

F

Third direction cosine of thermal flux.

5th data block - Table IDs 1-5

1st

I

Enter the table ID associated with the magnitude of the thermal flux.

6-10

2nd

I

Enter the table ID associated with the temperature of the radiant source.

11-15

3rd

I

Enter the table ID for first direction cosine of thermal flux.

16-20

4th

I

Enter the table ID for second direction cosine of thermal flux.

21-25

5th

I

Enter the table ID for third direction cosine of thermal flux.

6th data block If geometry type is element IDs (1), use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5), use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 01 Flux (bottom surface for shells) 10 Flux (top surface for shells)

11-15

3rd

I

Enter the face ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type 1: Element ids, top side if shell element 4: Surface ids, top side if shell element 5: Curve ids, top side if shell element 11: Element-Edge ids, top side if shell element 12: Element-Face ids, top side if shell element

Main Index

QVECT (with TABLE Input - Model Definition) 1029 Define Thermal Vector Flux Boundary Conditions

Format Fixed

Free

Data Entry Entry 13: Element-Edge IDs - Marc Mentat convention, top side if shell element 14: Element-Face IDs - Marc Mentat convention, top side if shell element. 16: Surface id: orientation id 17: Curve id: orientation id 18: Surface id: orientation ID - Marc Mentat convention 19: Curve id: orientation ID - Marc Mentat convention 21: Element ids, bottom side if shell element 24: Surface ids, bottom side if shell element 25: Curve ids, bottom side if shell element 31: Element-Edge ids, bottom side if shell element 32: Element-Face ids, bottom side if shell element 33: Element-Edge IDs - Marc Mentat convention, bottom side if shell element 34: Element-Face IDs - Marc Mentat convention, bottom side if shell element.

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

1030 WELD FLUX (with TABLE Input - Model Definition) Define Motion and Flux Parameters for Weld Heat Source

WELD FLUX (with TABLE Define Motion and Flux Parameters for Weld Heat Source Input - Model Definition) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows welding (surface and volumetric) fluxes to be specified. Two groups of parameters are used in this option to specify the weld flux. The first group pertains to the initial location and motion of the weld source and the second group pertains to the magnitude and shape of the weld source. The distributed weld fluxes are converted to consistent nodal fluxes by Marc. The default volumetric weld flux has a double ellipsoidal shape and is suitable for deep penetration welding processes like laser welding and electron beam welding. The default surface weld flux has a disc shape and is suitable for welding processes like arc welding. Arbitrary volumetric or surface flux values at integration points along the weld path can be specified through the UWELDFLUX user subroutine. Refer to Marc Volumes A, D, and E for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of distributed fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed flux data, defaults to input.

The 3rd through 7th data blocks are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Weld Flux Index (Index can be used in the UWELDFLUX user subroutine).

11-15

3rd

I

Weld Flux Type: 1 – double ellipsoidal shaped volumetric weld flux. 2 – disc shaped surface weld flux. 3 – user subroutine defined weld flux.

Main Index

16-20

4th

I

Weld Path Index.

21-25

5th

I

Weld Filler Index.

WELD FLUX (with TABLE Input - Model Definition) 1031 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed 26-30

Free 6th

Data Entry Entry I

Initial Position Flag: 0 – Initial weld position is automatically taken as first point of associated weld path. 1 – Initial weld position is specified in the first three fields of the 4th data block.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

X coordinate for initial position of weld flux.

11-20

2nd

F

Y coordinate for initial position of weld flux.

21-30

3rd

F

Z coordinate for initial position of weld flux.

31-40

4th

F

Local X offset from weld path.

41-50

5th

F

Local Y offset from weld path.

51-60

6th

F

Velocity of weld flux.

61-65

7th

I

Table ID for velocity.

Notes:

The initial position defined in fields 1, 2, and 3 of data block 4 is only used if the initial position flag in the 6th field of the 3rd data block is nonzero. Also, the given initial weld position should be along the associated weld path. Else, the program will terminate with exit 20. The defined initial weld position is mandatory when the user subroutine UWELDPATH is used to define the associated weld path. When the same weld flux is specified in multiple loadcases, the initial weld position is only used for the starting loadcase. For subsequent loadcases, the position at the end of the previous loadcase is used as the starting position. The X and Y offsets (fields 4 and 5 in data block 4) are defined in the local coordinate system of the weld flux. They are 0 by default. The Y offset is along the arc direction and the X offset is along the tangent direction. These offsets allow the flux to be located at a specified distance from the associated weld path. The table defining the weld velocity can be a function of time.

5th data block 1-10

1st

F

Power of weld flux.

11-20

2nd

F

Efficiency of weld flux.

21-30

3rd

F

Scale Factor for weld flux.

31-40

4th

F

Width of weld (for volumetric source). Radius of weld (for surface source).

Fields 5 through 7 are only valid for the double ellipsoidal volumetric weld flux: 41-50

Main Index

5th

F

Depth of weld.

1032 WELD FLUX (with TABLE Input - Model Definition) Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

51-60

6th

F

Forward length of weld.

61-70

7th

F

Rear length of weld.

71-80

8th

F

Maximum distance from weld origin for nonzero flux

6th data block 1-5

1st

I

Table ID for Weld Flux Power.

6-10

2nd

I

Table ID for Weld Flux Efficiency.

11-15

3rd

I

Scale Factor Flag: 0 – Use automatic scale factor. 1 – Use manually defined scale factor.

16-20

4th

I

Table ID for Weld Width/Radius.

Fields 5 through 7 are only valid for the double ellipsoidal volumetric weld flux: 21-25

5th

I

Table ID for Weld Depth.

26-30

6th

I

Table ID for Weld Forward Length.

31-35

7th

I

Table ID for Weld Rear Length.

36-40

8th

I

Table ID for Maximum Distance from Weld Origin

Notes:

The 5th and 6th data blocks are directly used for the ellipsoidal and disc shaped weld fluxes. The flux values are defined directly for the user subroutine option. The weld dimensions can still be entered in this case since they are useful for filler element activation, adaptive meshing box definition, etc. The scale factor in the 3rd field of the 5th data block can be manually specified or automatically determined by the program. The scale factor flag in the 3rd field of the 6th data block determines the usage. See Volume A for more details. If the maximum distance from weld origin is not defined (left as 0), then the weld pool dimensions are used to determine which elements receive the weld flux. The tables defining the weld power, efficiency, weld width/radius, depth, forward and rear lengths, and the maximum distance from weld origin can be a function of time or arc length measured along the associated weld path.

7th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

Normal flux (bottom surface for shells)

10: Normal flux (top surface for shells)

Main Index

WELD FLUX (with TABLE Input - Model Definition) 1033 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Enter the face ID or edge ID.

The 8th and 9th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 8th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

9th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 8th data block.

1034 WELD FLUX (Model Definition) Define Motion and Flux Parameters for Weld Heat Source

WELD FLUX (Model Definition)

Define Motion and Flux Parameters for Weld Heat Source

The information provided here is based upon not using the table driven input style. Description This option allows welding (surface and volumetric) fluxes to be specified. Two groups of parameters are used in this option to specify the weld flux. The first group pertains to the initial location and motion of the weld source and the second group pertains to the magnitude and shape of the weld source. The distributed weld fluxes are converted to consistent nodal fluxes by Marc. The default volumetric weld flux has a double ellipsoidal shape and is suitable for deep penetration welding processes like laser welding and electron beam welding. The default surface weld flux has a disc shape and is suitable for welding processes like arc welding. Arbitrary volumetric or surface flux values at integration points along the weld path can be specified through the UWELDFLUX user subroutine. Refer to Marc Volumes A, D, and E for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of weld fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld flux data; defaults to input.

3rd data block 1-5

1st

I

Weld Flux Index (Index is to be used in the UWELDFLUX user subroutine).

6-10

2nd

I

Weld Flux Type: 1 – double ellipsoidal shaped volumetric weld flux. 2 – disc shaped surface weld flux. 3 – user subroutine defined weld flux.

Main Index

11-15

3rd

I

Weld Path Index.

16-20

4th

I

Weld Filler Index.

WELD FLUX (Model Definition) 1035 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed 21-25

Free 5th

Data Entry Entry I

Parameter identifying the type of distributed flux. See library element description in Marc Volume B: Element Library. Note that the parameter in this field should be consistent with the weld flux type specified in the 2nd field.

26-30

6th

I

Initial Position Flag: 0 – Initial weld position is automatically taken as first point of associated weld path. 1 – Initial weld position is specified in the first three fields of the 4th data block.

31-35

7th

I

Weld Flux Activation Flag 0 – Weld Flux boundary condition is active in loadcase 1 – Weld Flux boundary condition is inactive in loadcase

36-67

8th

C

Weld Flux Name (optional)

4th data block 1-10

1st

F

X coordinate for initial position of weld flux.

11-20

2nd

F

Y coordinate for initial position of weld flux.

21-30

3rd

F

Z coordinate for initial position of weld flux.

31-40

4th

F

Local X offset from weld path.

41-50

5th

F

Local Y offset from weld path.

51-60

6th

F

Velocity of weld flux.

61-65

7th

I

Table ID for velocity.

Notes: The initial position defined in fields 1, 2, and 3 of data block 4 is only used if the initial position flag in the 6th field of the 3rd data block is nonzero. Also, the given initial weld position should be along the associated weld path. Else, the program will terminate with exit 20. The defined initial weld position is mandatory when the UWELDPATH user subroutine is used to define the associated weld path. When the same weld flux is specified in multiple loadcases, the initial weld position is only used for the starting loadcase. For subsequent loadcases, the position at the end of the previous loadcase is used as the starting position. The X and Y offsets (fields 4 and 5 in data block 4) are defined in the local coordinate system of the weld flux. They are 0 by default. The Y offset is along the arc direction and the X offset is along the tangent direction. These offsets allow the flux to be located at a specified distance from the associated weld path. The table defining the weld velocity can be a function of time. 5th data block 1-10

Main Index

1st

F

Power of weld flux.

1036 WELD FLUX (Model Definition) Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

11-20

2nd

F

Efficiency of weld flux.

21-30

3rd

F

Scale Factor for weld flux.

31-40

4th

F

Width of weld (for volumetric source). Radius of weld (for surface source).

Fields 5 through 7 are only valid for the double ellipsoidal volumetric weld flux: 41-50

5th

F

Depth of weld.

51-60

6th

F

Forward length of weld.

61-70

7th

F

Rear length of weld.

71-80

8th

F

Maximum distance from weld origin for nonzero flux.

6th data block 1-5

1st

I

Table ID for Weld Flux Power.

6-10

2nd

I

Table ID for Weld Flux Efficiency.

11-15

3rd

I

Scale Factor Flag: 0 – Use automatic scale factor. 1 – Use manually defined scale factor.

16-20

4th

I

Table ID for Weld Width/Radius.

Fields 5 - 7 are only valid for the double ellipsoidal volumetric weld flux: 21-25

5th

I

Table ID for Weld Depth.

26-30

6th

I

Table ID for Weld Forward Length.

31-35

7th

I

Table ID for Weld Rear Length.

36-40

8th

I

Table ID for maximum distance from weld origin.

Notes: The 5th and 6th data blocks are directly used for the ellipsoidal and disc shaped weld fluxes. The flux values are defined directly for the user subroutine option. The weld dimensions can still be entered in this case since they are useful for filler element activation, adaptive meshing box definition, etc. The scale factor in the 3rd field of the 5th data block can be manually specified or automatically determined by the program. The scale factor flag in the 3rd field of the 6th data block determines the usage. See Volume A for more details. If the maximum distance from weld origin is not defined (left as 0), then the weld pool dimensions are used to determine which elements receive the weld flux. The tables defining the weld power, efficiency, weld width/radius, depth, forward and rear lengths, and maximum distance from weld origin can be a function of time or arc length measured along the associated weld path.

Main Index

WELD FLUX (Model Definition) 1037 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

7th data block Enter a list of elements associated with the above weld flux.

Main Index

1038 WELD PATH (Model Definition) Define Path and Arc Orientation for Weld Heat Source

WELD PATH (Model Definition)

Define Path and Arc Orientation for Weld Heat Source

Description This option specifies the weld path to be followed by the weld flux. The orientation of the arc along the path is also defined. The weld path can be specified through nodes or point coordinates of polyline curves in the input file or through point coordinates in a separate text file, or through the UWELDPATH user subroutine. The arc orientation can be specified through nodes, point coordinates of polyline curves, vector components or Euler angles in the input file, point coordinates, vector components, or Euler angles in a separate text file, or through the UWELDPATH user subroutine. The specified path and arc orientation are used to define a moving local coordinate system. The Z axis of the local coordinate system is along the weld path, the Y axis is along the arc orientation and the X axis is along the tangent. X and Y axes that are perpendicular to each other and perpendicular to the given weld path (Z axis) are constructed based on the information provided in this option. See Marc Volume A: Theory and User Information for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD PATH.

2nd data block 1-5

1st

I

Enter the number of sets of weld paths to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld path data, defaults to input.

3rd data block 1-5

1st

I

Weld Path Index (Index is used for cross-referencing with the 3rd data block of the WELD FLUX option)

6-10

2nd

I

Weld Path Type 1 – Weld Path is specified through ordered list of nodes 2 – Weld Path is specified through point coordinates of polyline curves. 4 – Weld Path is specified through text file 5 – Weld Path is specified through the UWELDPATH user subroutine.

11-15

3rd

I

Arc Orientation Type 1 – Arc Orientation is specified through ordered list of nodes. 2 – Arc Orientation is specified through point coordinates of polyline curves.

Main Index

WELD PATH (Model Definition) 1039 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry 3 – Arc Orientation is specified through vector components. 4 – Arc Orientation is specified through Euler angles. 5 – Arc Orientation is specified through the UWELDPATH user subroutine.

16-20

4th

I

Number of curves used to define the Weld Path. This field is only valid when Weld Path Type is 2.

21-25

5th

I

Path Interpolation flag 0 or 1. 0 – Arc Orientation at first point of segment is used for whole segment. 1 – Arc Orientation is linearly interpolated between first and last points of segment.

26-30

6th

I

Not used.

31-62

7th

C

Weld Path Name (optional)

Notes: Weld Path Type 1 can only be used with Arc Orientation Types 1, 3, or 4. Weld Path Type 2 can only be used with Arc Orientation Types 2, 3, or 4. Weld Path Type 4 can only be used with Arc Orientation Type 2, 3, or 4. All quantities are specified via separate text file in this case. Weld Path Type 5 can only be used with Arc Orientation Type 5. The 4th through 7th data blocks depend on the WELD PATH TYPE (2nd field of 3rd data block) and ARC ORIENTATION TYPE (3rd field of 3rd data block). These data blocks are only needed for weld path types 1, 2, and 4. I. WELD PATH TYPE 1 (NODES) 4th data block Enter an unsorted list of nodes or unsorted set of nodes (NDSQ) needed to define the weld path. A. ARC ORIENTATION TYPE 1 (NODES)

5th data block 1-10

1st

F

Angle in degrees by which the ARC-TANGENT plane is rotated about weld path (default is 0).

11-15

2nd

I

Table ID for Angle.

6th data block Enter an unsorted list of nodes or unsorted set of nodes (NDSQ) needed to define the weld orientation.

Main Index

1040 WELD PATH (Model Definition) Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

Notes: The table defining the angle can be a function of the arc length along the weld path or a function of the position coordinates along the weld path. The arc vector is defined as the vector from the weld path node to the weld orientation node. The number of nodes defining the weld orientation has to be either equal to 1 or equal to the number of nodes defining the weld path. If only one node is used, the arc vector is defined as the vector from the weld path node to that node always. B. ARC ORIENTATION TYPE 3 (VECTOR)

5th data block 1-10

1st

F

Component X of Arc Orientation Vector.

11-20

2nd

F

Component Y of Arc Orientation Vector.

21-30

3rd

F

Component Z of Arc Orientation Vector.

31-35

4th

I

Table ID for Component X.

36-40

5th

I

Table ID for Component Y.

41-45

6th

I

Table ID for Component Z.

Note:

The tables defining the arc orientation vector components can be a function of the arclength along the weld path or a function of the position coordinates along the weld path.

C. ARC ORIENTATION TYPE 4 (EULER ANGLES)

5th data block 1-10

1st

F

Rotation of unit vector in X direction about global X axis.

11-20

2nd

F

Rotation of unit vector in X direction about global Y axis.

21-30

3rd

F

Rotation of unit vector in X direction about global Z axis.

31-35

4th

I

Table ID for Rotation about X.

36-40

5th

I

Table ID for Rotation about Y.

41-45

6th

I

Table ID for Rotation about Z.

Note:

Main Index

All rotation values are specified in degrees. If all rotation values are 0, the arc orientation is taken as <1,0,0>; i.e., unit vector in global X direction. Tables defining the Euler angles can be a function of arclength along the weld path or a function of the position coordinates along the weld path.

WELD PATH (Model Definition) 1041 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

II. WELD PATH TYPE 2 (CURVES) Start Loop over Number of Polyline Curves Read Number of Points to define Polyline

(4th data block)

Start Loop over Number of Points to define Path Polyline Read coordinates of each Weld Path Point

(5th data block)

End loop over Points End loop over Polyline Curves

For Each Curve: 4th data block 1-5

1st

I

Weld Curve Type (polyline = 1).

6-10

2nd

I

Number of Points to Define Polyline.

For each point on the Weld Path Curve: 5th data block 1-10

1st

F

X coordinate of point.

11-20

2nd

F

Y coordinate of point.

21-30

3rd

F

Z coordinate of point.

A. ARC ORIENTATION TYPE 2 (CURVES) Start Loop over Number of Polyline Curves Read Angle for Rotation of Tangent-Arc Plane (6th data block) Start Loop over Number of Points to define Arc Polyline Read coordinates of each Weld Orientation Point (7th data block) End Loop over Point End Loop over Polyline Curves

For Each Curve: 6th data block 1-5

1st

I

Arc Curve Type (polyline = 1).

6-15

2nd

F

Angle in degrees by which Arc-Tangent plane is rotated about Weld Path (default = 0).

16-20

3rd

I

Table ID for angle.

For each point on the Arc Orientation Curve:

Main Index

1042 WELD PATH (Model Definition) Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

7th data block 1-10

1st

F

X coordinate of point.

11-20

2nd

F

Y coordinate of point.

21-30

3rd

F

Z coordinate of point.

Notes: Only Polylines (Weld Curve Type = 1, Arc Curve Type = 1) are supported in the current version. The table defining the angle can be a function of the arc length along the weld path or a function of the position coordinates along the weld path. The number of points defining the arc orientation curve has to be equal to the number of points defining the weld path curve. B. ARC ORIENTATION TYPE 3 (VECTOR)

6th data block 1-10

1st

F

Component X of Arc Orientation Vector.

11-20

2nd

F

Component Y of Arc Orientation Vector.

21-30

3rd

F

Component Z of Arc Orientation Vector.

31-35

4th

I

Table ID for Component X.

36-40

5th

I

Table ID for Component Y.

41-45

6th

I

Table ID for Component Z.

Note:

The tables defining the arc orientation vector components can be a function of the arc length along the weld path or a function of the position coordinates along the weld path.

C. ARC ORIENTATION TYPE 4 (EULER ANGLES)

6th data block 1-10

1st

F

Rotation of unit vector in X direction about global X axis.

11-20

2nd

F

Rotation of unit vector in X direction about global Y axis.

21-30

3rd

F

Rotation of unit vector in X direction about global Z axis.

31-35

4th

I

Table ID for Rotation about X.

36-40

5th

I

Table ID for Rotation about Y.

41-45

6th

I

Table ID for Rotation about Z.

Note:

Main Index

All rotation values are specified in degrees. If all rotation values are 0, the arc orientation is taken as <1,0,0> i.e., unit vector in global X direction. Tables defining the euler angles can be a function of arclength along the weld path or a function of the position coordinates along the weld path.

WELD PATH (Model Definition) 1043 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

III. WELD PATH TYPE 4 (Text File) 4th data block Enter name of Text File containing Weld Path and Arc Orientation Information. Note:

Main Index

Columns 1 - 3 of the text file contain weld path information. Columns 4 - 6 of the text file contain arc orientation information. Depending on the arc orientation type (2, 3 or 4) specified on the 3rd data block, columns 4 - 6 can contain point coordinates, vector components or Euler angle values. The entry in each column is a real number of width 10. The columns can be in free or fixed format with commas being used to separate the columns in the free format mode.

1044 WELD FILL (Model Definition) Define Parameters for Weld Filler Elements

WELD FILL (Model Definition)

Define Parameters for Weld Filler Elements

Description This option identifies the weld filler elements that are associated with a particular weld heat source. The method by which the filler elements can potentially participate in the analysis is specified. Two methods can be used: Quiet Element method and Deactivated Element Method. In the Quiet Element Method, the filler elements are always part of the analysis. However, prior to their physical creation, the filler elements are used with scaled down material properties. The regular material properties are restored after the filler elements are physically created by the moving heat source. In the Deactivated Element Method, the filler elements are deactivated at the outset and are automatically activated only when they are physically created by the moving heat source. Filler Bounding Box X, Y, and Z refer to dimensions in the local coordinate system attached to the moving heat source. They are used to identify if filler elements are physically created during the welding process. If these dimensions are not specified on the option (i.e., left at 0), they are related to weld pool dimensions set on the WELD FLUX option: Filler Bounding Box X in the Tangent direction = 1.5 x Weld Width Filler Bounding Box Y in the Arc direction = 2 x Weld Width Filler Bounding Box Z in the Arc Direction = Weld Pool Length See Marc Volume A: Theory and User Information for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD FILL.

2nd data block 1-5

1st

I

Enter the number of sets of weld fillers to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld flux data; defaults to input.

3rd data block 1-5

1st

I

Weld Filler Index (Index is used for cross-referencing with field 4 of the 3rd data block in the WELD FLUX option).

6-10

2nd

I

Initial Activation Flag 0 – Quiet Element Method. 1 – Deactivated Element Method.

Main Index

WELD FILL (Model Definition) 1045 Define Parameters for Weld Filler Elements

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Temperature Boundary Condition Flag 0 – Nodal boundary conditions are applied 1 – Nodal boundary conditions are not applied

16-25

4th

F

Melting Point Temperature

26-35

5th

F

Temperature Activation Time (0 by default)

36-45

6th

F

Material Property Scale Factor (1e-5 by default)

46-77

7th

F

Weld Filler Name (Optional)

Notes: The melting point temperature information in field 4 is only used if the boundary condition flag in field 3 is 0. If nodal boundary conditions are not applied (3rd field = 1), weld fluxes can be applied to the filler elements to ramp up the temperature. A user-specified thermal activation time, specified in field 5, can also be used. The thermal activation time serves two purposes: (1) It defines the time over which the temperature boundary condition is ramped (only valid when field 3 is 0). Default is 0 which means that the temperatures are applied instantaneously. For nonzero time values, the temperatures of the active filler elements are linearly increased from the current value to the specified temperature over the specified time step. (2) It defines the time during which the filler elements only participate in the thermal pass and not in the mechanical pass (valid when field 3 is 0 or 1). Default is 0 which means that if the filler elements are first created at increment n, they only participate on the thermal side at increment n, and then participate in both thermal and mechanical passes at increment n+1. For nonzero time values, the filler elements remain thermally active over the specified time duration and become mechanically active only after the time duration. The property scale factor in field 6 is only used for the quiet element method. 4th data block 1-10

1st

F

Filler Bounding Box in X (weld width) direction

11-20

2nd

F

Filler Bounding Box in Y (weld depth) direction

21-30

3rd

F

Filler Bounding Box in +Z (forward path) direction

31-40

4th

F

Filler Bounding Box in -Z (rear path) direction

41-45

5th

I

Table ID for Filler Bounding Box X

46-50

6th

I

Table ID for Filler Bounding Box Y

51-55

7th

I

Table ID for Filler Bounding Box +Z

56-60

8th

I

Table ID for Filler Bounding Box -Z

Note:

Main Index

The table IDs for the filler bounding boxes can be a function of time or arc length. The arc length is measured along the weld path from the first point to the current position of the weld source. If the bounding box dimensions are not specified, the weld pool dimensions are used to define the box.

1046 WELD FILL (Model Definition) Define Parameters for Weld Filler Elements

Format Fixed

Free

Data Entry Entry

5th data block 1-80

Main Index

1

I

Enter the list of filler elements

THERMAL CONTACT with TABLES (2-D) 1047 Define Two-dimensional Thermal or Electrical Contact Conditions

THERMAL CONTACT with TABLES (2-D)

Define Two-dimensional Thermal or Electrical Contact Conditions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows for the input of 2-D thermal contact definition in heat transfer problems and the definition of conducting bodies for electrostatic and Joule heating analysis. Near thermal contact is only available if the input version is 10 or greater. THERMAL CONTACT should not be used in problems where a mechanical-displacement solution is obtained as there is no checking for changes in contact; use the CONTACT option instead. Note:

Always define heat conduction thermal bodies before heat sink bodies.

If the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used, the film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart: DCONTACT

1st field

3rd data block

Bias factor

2nd field

3rd data block

T1 d T2

If

d < DC ON TACT ,

q = H CT ( T 2 – T 1 )

then contact

if deformable-deformable

q = H CT ( T 2 – T BODY )

If

Main Index

if rigid.

DC ON TACT < d < DQN EAR

and

DQ NEAR

is defined, the last term is only included if

H BL

is defined.

1048 THERMAL CONTACT with TABLES (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

q = H CV ( T 2 – T 1 ) + H NC ( T 2 – T 1 )

B NC

4

4

+ σε f ( T 2 – T 1 )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ ( T 1 ) ⎝ DQN EAR⎠ D QNE A R ⎭ ⎩

If

d > DQN EAR 4

4

q = H CTVE ( T 2 – T SINK ) + σε ( T 2 – T SI NK )

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word THERMAL CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Upper bound to the number of nodes that lie on the periphery of any deformable surface.

16-20

4th

I

Enter 1 to reduce printout of surface definition.

21-25

5th

I

Linearization flag to be used if a contact body consists of quadratic element: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

3rd data block 1-10

1st

F

Distance below which a node is considered touching a body (DCONTACT). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

11-20

2nd

F

Contact tolerance BIAS factor. (0-1)

Data blocks 4th through 20th are repeated once for each body to be defined.

Main Index

THERMAL CONTACT with TABLES (2-D) 1049 Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

Enter 0 for double-sided contact with default search order based upon body id. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined. For conducting bodies, enter 2 if double-sided contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Contact body type (optional): 1: heat sink; 4: heat conduction body. 7: electromagnetic conducting body

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

Main Index

1050 THERMAL CONTACT with TABLES (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed 51-60

Free 6th

Data Entry Entry F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis; Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

7th data block 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

8th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

9th data block The 9th data block is only necessary if heat transfer is included.

Main Index

1-10

1st

F

Heat Transfer coefficient (film) to environment (HCVE).

11-20

2nd

F

Environment sink temperature (TSINK).

21-30

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY). (Required for rigid body only.)

41-50

5th

F

Enter the convection coefficient for near field behavior (HCV).

51-60

6th

F

Enter the natural convection coefficient for near field behavior (HNC).

61-70

7th

F

Enter the exponent associated with natural convection (BNC).

71-80

8th

F

Enter the surface emissivity for near field behavior (ε).

THERMAL CONTACT with TABLES (2-D) 1051 Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

10th data block The 10th data block is only necessary if heat transfer is included. 1-5

1st

I

Enter the table ID for the heat transfer coefficient to environment (HCVE).

6-10

2nd

I

Enter the table ID for the environment sink temperature (TSINK).

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

21-25

5th

I

Enter the table ID for the convection coefficient for near field behavior (HCV).

26-30

6th

I

Enter the table ID for natural convection coefficient for near field behavior (HNC).

31-35

7th

I

Enter the table ID for the exponent associated with natural convection. (BNC).

36-40

8th

I

Enter the table ID for the surface emissivity for near field behavior (ε).

11th data block (Only if heat transfer is included.) 1-10

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

12th data block (Only if heat transfer is included.) 1-5

1st

I

Enter the table ID associated with (HBL).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distance (s) is less than ERROR, bodies are in contact 2. If separation distance (s) is greater than ERROR, but less than not zero. q = H CV ( T B – T A ) + H NC ( T B – T A )

B NC

4

q = H CT ( T B – T A ) .

DQ NEAR ,

and

DQ NEAR

is

4

+ σε ( T B – T A )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H B L -------------------------- ⎬ ( T B – T A ) ⎝ ⎠ D QN EA R DQ NEAR ⎩ ⎭

The last term is only included if HBL is not zero. 3. If separation distance (s) is greater than q = H CVE ( T SI NK – T A ) +

4 σε ( T SI NK

–

DQ NE A R ,

then convection to environment only.

4 TA )

13th data block (Only if Joule Heating is included.) 1-10

Main Index

1st

F

Electrical transfer coefficient to environment.

1052 THERMAL CONTACT with TABLES (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

11-20

2nd

F

Environment sink voltage.

21-30

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage (Required for rigid body only).

41-50

5th

F

Electrical transfer coefficient for near field behavior.

51-60

6th

F

Enter the separation distance dependent electrical transfer coefficient.

14th data block (Only if Joule Heating is included.) 1-5

1st

I

Enter the table ID for the electrical transfer coefficient to environment.

6-10

2nd

I

Enter the table ID for the sink voltage.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

21-25

5th

I

Enter the table ID for the electrical transfer coefficient for near field behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent electrical transfer coefficient.

15th data block (Only used if coupled mass diffusion.) 1-10

1st

E

Enter the mass flow rate coefficient to environment.

11-20

2nd

E

Enter the environment sink pressure (PSINK).

21-30

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure (required for rigid body only).

41-50

5th

E

Enter the mass flow rate coefficient for near field behavior.

51-60

6th

E

Enter separation distance dependent mass flow rate coefficient.

16th data block (Only used if coupled mass diffusion.) 1-5

1st

I

Enter the table ID for the mass flow rate coefficient to environment.

6-10

2nd

I

Enter the table ID for the environment sink pressure (PSINK).

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

21-25

5th

I

Enter the table ID for the mass rate coefficient for near behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent mass flow rate coefficient.

The 17th through 20th data blocks are repeated for as many geometrical data as required (NETTY).

Main Index

THERMAL CONTACT with TABLES (2-D) 1053 Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

A. For 2-D Deformable Bodies

17a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 2-D Rigid Body (Line-Segment)

17b data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 18th data block is repeated once for each point entered. 18b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Circular Arc)

17c data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 18c data block is repeated four times. 18c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (Spline)

17d data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 18d data block is repeated for each point to be entered. 18d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

E. For 2-D Rigid Body (NURBS)

The 17e data block is repeated NPTU times for control points. 17e data block 1-5

Main Index

1st

I

Enter 9 for NURBS.

1054 THERMAL CONTACT with TABLES (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

18e data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 19e data block is repeated NPTU times for homogeneous coordinate. 19e data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 20e data block is repeated NPTU+ NORU times for knot vectors. 20e data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

THERMAL CONTACT (2-D) 1055 Define Two-dimensional Thermal or Electrical Contact Conditions

THERMAL CONTACT (2-D)

Define Two-dimensional Thermal or Electrical Contact Conditions

The information provided here is based upon not using the table driven input style. Description This option allows for the input of 2-D thermal contact definition in heat transfer problems and the definition of conducting bodies for electrostatic and Joule heating analysis. Near thermal contact is only available if the input version is 10 or greater. THERMAL CONTACT should not be used in problems where a mechanical-displacement solution is obtained as there is no checking for changes in contact; use the CONTACT option instead. Note:

Always define deformable surfaces before rigid surfaces.

If the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used, the film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart: DCONTACT

1st field

3rd data block

Bias factor

2nd field

3rd data block

T1 d T2

If

d < DC ON TACT ,

q = H CT ( T 2 – T 1 )

then contact

if deformable-deformable

q = H CT ( T 2 – T BODY )

If

Main Index

if rigid.

DC ON TACT < d < DQN EAR

and

DQ NEAR

is defined, the last term is only included if

H BL

is defined.

1056 THERMAL CONTACT (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

q = H CV ( T 2 – T 1 ) + ( T 2 – T 1 )

B NC

+ σε f ( T 2 – T 1 )

4

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ ( T 1 ) ⎝ DQN EAR⎠ D QN EA R ⎭ ⎩

If

d > DQN EAR 4

4

q = H CTVE ( T 2 – T SINK ) + σε ( T 2 – T SI NK )

The distance below which near contact behavior occurs for thermal and electrical behavior (DQNEAR) needs to be defined in the CONTACT TABLE and can be set for each interface separately. Format Format Fixed

Free

Data En Entry try

1st data block 1-7

1st

A

Enter the word THERMAL CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Upper bound to the number of nodes that lie on the periphery of any deformable surface.

16-20

4th

I

Enter 1 to reduce printout of surface definition.

21-25

5th

I

Linearization flag to be used if a contact body consists of quadratic element: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact. -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

3rd data block 1-10

Main Index

1st

F

Distance below which a node is considered touching a body (DCONTACT). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

THERMAL CONTACT (2-D) 1057 Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

11-20

2nd

Data En Entry try F

Contact tolerance BIAS factor. (0-1)

Data blocks 4 through 15 are repeated once for each body to be defined. 4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

Enter 0 for double-sided contact with default search order based upon body id. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined. For conducting bodies, enter 2 if double-sided contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Contact body type (optional): 1: rigid body; 4: heat -rigid body. 7: electromagnetic conducting body.

41-64

9th

A

Contact body name (optional)

5th data block

Main Index

1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

1058 THERMAL CONTACT (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed 61-70

Free 7th

Data En Entry try F

Third component direction cosine of local axis. Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

7th data block 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

The 8th and 9th data blocks are only necessary for heat transfer. 8th data block 1-10

1st

F

Heat transfer coefficient (film) to environment ( H CVE ).

11-20

2nd

F

Environment sink temperature ( T S INK ).

21-30

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

41-50

5th

F

Enter the convection coefficient for near field behavior ( H CV ).

51-60

6th

F

Enter the natural convection coefficient for near field behavior ( H NC ).

61-70

7th

F

Enter the exponent associated with natural convection ( B NC ).

71-80

8th

F

Enter the surface emissivity for near field behavior or radiation to environment ( ε ).

F

Enter the separation distance dependent heat transfer file coefficient ( H BL ).

9th data block 1-10

1st

10th data block The 10th data block is only necessary for Joule heating.

Main Index

1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30

3rd

F

Contact electrical transfer coefficient.

THERMAL CONTACT (2-D) 1059 Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data En Entry try

31-40

4th

F

Body voltage (required for rigid body only).

41-50

5th

F

Electrical transfer coefficient for near field behavior.

51-60

6th

F

Enter the separation distance dependent electrical transfer coefficient.

A. For 2-D Deformable Bodies The 11th through the 16th data blocks are repeated for each set of body entities (NSURGN). 11a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 2-D Rigid Body (Line-Segment) 11b data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 12b data block is repeated once for each point entered. 12b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Circular Arc) 11c data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 12c data block is repeated four times. 12c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (Spline) 11d data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 12d data block is repeated for each point to be entered. 12d data block 1-10

Main Index

1st

F

First coordinate of point.

1060 THERMAL CONTACT (2-D) Define Two-dimensional Thermal or Electrical Contact Conditions

Format Fixed 11-20

Free 2nd

Data En Entry try F

Second coordinate of point.

E. For 2-D Rigid Body (NURBS) 11e data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 13e data block is repeated NPTU times for control points. 13e data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 14e data block is repeated NPTU times for homogeneous coordinate. 14e data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 15e data block is repeated NPTU+ NORU times for knot vectors. 15e data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

THERMAL CONTACT with TABLES (3-D) 1061 Define Three-dimensional Thermal or Electrical Contact Conditions

THERMAL CONTACT with TABLES (3-D)

Define Three-dimensional Thermal or Electrical Contact Conditions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows for the input of 2-D thermal contact definition in heat transfer problems and the definition of conducting bodies for electrostatic and Joule heating analysis. Near thermal contact is only available if the input version is 10 or greater. THERMAL CONTACT should not be used in problems where a mechanical-displacement solution is obtained as there is no checking for changes in contact; use the CONTACT option instead. Note:

Always define heat conduction thermal bodies before heat sink bodies.

If the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used, the film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart: DCONTACT

1st field

3rd data block

Bias factor

2nd field

3rd data block

T1 d T2

If

d < DC ON TA CT ,

q = H CT ( T 2 – T 1 )

then contact

if deformable-deformable

q = H CT ( T 2 – T BODY )

If

Main Index

if rigid.

DC ON TACT < d < DQN EAR

and

DQ NEAR

is defined, the last term is only included if

H BL

is defined.

1062 THERMAL CONTACT with TABLES (3-D) Define Three-dimensional Thermal or Electrical Contact Conditions

q = H CV ( T 2 – T 1 ) + H NC ( T 2 – T 1 )

B NC

4

4

+ σε f ( T 2 – T 1 )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ ( T 1 ) ⎝ DQN EAR⎠ D QNE A R ⎭ ⎩

If

d > DQN EAR 4

4

q = H CVE ( T SI NK – T A ) + σε ( T SI NK – T A )

Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word THERMAL CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Upper bound to the number of nodes that lie on the periphery of any deformable surface.

16-20

4th

I

Enter 1 to reduce printout of surface definition.

3rd data block 1-10

1st

F

Distance below which a node is considered touching a body (DCONTACT). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

11-20

2nd

F

Contact tolerance BIAS factor. (0-1)Data blocks 4 through 24 are repeated once for each body to be defined.

4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

Enter 0 for double-sided contact with default search order based upon body ID. For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used.

Main Index

THERMAL CONTACT with TABLES (3-D) 1063 Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry Note that, in this case, results are dependent upon the order in which contact bodies are defined. For conducting bodies, enter 2 if double-sided contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Contact body type (optional): 1: heat sink; 4: heat conduction body. 7: electromagnetic conducting body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis; Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

7th data block

Main Index

1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

1064 THERMAL CONTACT with TABLES (3-D) Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

8th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

9th data block The 9th data block is only necessary if heat transfer is included. 1-10

1st

F

Heat Transfer coefficient (film) to environment (HCVE).

11-20

2nd

F

Environment sink temperature (TSINK).

21-30

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY). (Required for rigid body only.)

41-50

5th

F

Enter the convection coefficient for near field behavior (HCV).

51-60

6th

F

Enter the natural convection coefficient for near field behavior (HNC).

61-70

7th

F

Enter the exponent associated with natural convection (BNC).

71-80

8th

F

Enter the surface emissivity for near field behavior (ε).

10th data block The 10th data block is only necessary if heat transfer is included. 1-5

1st

I

Enter the table ID for the heat transfer coefficient to environment (HCVE).

6-10

2nd

I

Enter the table ID for the environment sink temperature (TSINK).

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

21-25

5th

I

Enter the table ID for the convection coefficient for near field behavior (HCV).

26-30

6th

I

Enter the table ID for natural convection coefficient for near field behavior (HNC).

31-35

7th

I

Enter the table ID for the exponent associated with natural convection. (BNC).

36-40

8th

I

Enter the table ID for the surface emissivity for near field behavior (ε).

11th data block (Only if heat transfer is included) 1-10

Main Index

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

THERMAL CONTACT with TABLES (3-D) 1065 Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

12th data block (Only if heat transfer is included) 1-5

1st

I

Enter the table ID associated with (HBL).

The thermal flux can be described between two bodies A and B as follows: 1. If separation distance (s) is less than ERROR, bodies are in contact 2. If separation distance (s) is greater than ERROR, but less than zero. q = H CV ( T B – T A ) + H NC ( T B – T A )

B NC

4

q = H CT ( T B – T A ) .

DQ NE A R ,

and

DQ NE A R

is not

4

+ σε ( T B – T A )

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H B L -------------------------- ⎬ ( T B – T A ) ⎝ D QN EA R⎠ DQ NEAR ⎭ ⎩

The last term is only included if HBL is not zero. 3. If separation distance (s) is greater than q = H CVE ( T SI NK – T A ) +

4 σε ( T SI NK

–

DQ NEAR ,

then convection to environment only.

4 TA )

13th data block (Only if Joule Heating is included.) 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage (Required for rigid body only).

41-50

5th

F

Electrical transfer coefficient for near field behavior.

51-60

6th

F

Enter the separation distance dependent electrical transfer coefficient.

14th data block (Only if Joule Heating is included.) 1-5

1st

I

Enter the table ID for the electrical transfer coefficient to environment.

6-10

2nd

I

Enter the table ID for the sink voltage.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

21-25

5th

I

Enter the table ID for the electrical transfer coefficient for near field behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent electrical transfer coefficient.

15th data block (Only used if coupled mass diffusion.) 1-10

Main Index

1st

E

Enter the mass flow rate coefficient to environment.

1066 THERMAL CONTACT with TABLES (3-D) Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

11-20

2nd

E

Enter the environment sink pressure (PSINK).

21-30

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure (required for rigid body only).

41-50

5th

E

Enter the mass flow rate coefficient for near field behavior.

51-60

6th

E

Enter separation distance dependent mass flow rate coefficient.

16th data block (Only used if coupled mass diffusion.) 1-5

1st

I

Enter the table ID for the mass flow rate coefficient to environment.

6-10

2nd

I

Enter the table ID for the environment sink pressure (PSINK).

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

21-25

5th

I

Enter the table ID for the mass rate coefficient for near behavior.

26-30

6th

I

Enter the table ID for the separation distance dependent mass flow rate coefficient.

The 17th through 24th data blocks are repeated for each set of body entities (NSURGN). A. For 3-D Deformable Body 17a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 3-D Rigid Body (Ruled Surface) 17b data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

21-25

5th

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

Main Index

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

THERMAL CONTACT with TABLES (3-D) 1067 Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

The 18b data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 18b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

C. For 3-D Rigid Body (Surface of Revolution) 17c data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 Method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 18c data block is repeated NPOINT times for surface of revolution. 18c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

19c data block 1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

D. For 3-D Rigid Surface (Bezier Surface) 17d data block

Main Index

1068 THERMAL CONTACT with TABLES (3-D) Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 18d data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 18d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

E. For 3-D Rigid Surface (4-Node Patch) 17e data block 1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

16-20

4th

I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.The 16e data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1)

18e data block 1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 19e data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 19e data block 1-5

Main Index

1st

I

Point number.

THERMAL CONTACT with TABLES (3-D) 1069 Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

F. For 3-D Rigid Surface (Poly-Surface) 17f data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 18f data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 18f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

G. For 3-D Rigid Surface (NURBS) 17g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 18g data block is repeated (NPTU ∗ NPTV) for control points. 18g data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 19g data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 19g data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 20g data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors.

Main Index

1070 THERMAL CONTACT with TABLES (3-D) Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry

20g data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 21g, 22g, 23g, and 24g. 21g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 22g data block is repeated NPTU times for control points. 22g data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 23g data block is repeated NPTU times for homogeneous coordinate. 23g data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 24g data block is repeated NPTU+ NORU times for knot vectors. 24g data block 1-10

1st

F

Component of knot vector between 0 and 1.

H. For 3-D Rigid Surface (Cylinder) 17h data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

18h data block

Main Index

1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface.

THERMAL CONTACT with TABLES (3-D) 1071 Define Three-dimensional Thermal or Electrical Contact Conditions

Format Fixed

Free

Data Entry Entry Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

I. For 3-D Rigid Surface (Sphere) 17i data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

18i data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

1072 THERMAL CONTACT (3-D) Define Three-dimensional Thermal or ElectricalContact Conditions

THERMAL CONTACT (3-D)

Define Three-dimensional Thermal or ElectricalContact Conditions

The information provided here is based upon not using the table driven input style. Description This option allows for the input of 2-D thermal contact definition in heat transfer problems and the definition of conducting bodies for electrostatic and Joule heating analysis. Near thermal contact is only available if the input version is 10 or greater. THERMAL CONTACT should not be used in problems where a mechanical-displacement solution is obtained as there is no checking for changes in contact; use the CONTACT option instead. Note:

Always define deformable surfaces before rigid surfaces.

If the UHTCOEF option and the UHTCOE user subroutine are used, the film coefficient and sink temperature data of a free surface can be skipped. If the UHTCON option and the UHTCON user subroutine are used, the film coefficient data between surfaces in contact can be skipped. The following data can be changed upon restart: DCONTACT

1st field

3rd data block

Bias factor

2nd field

3rd data block

T1 d T2

If

d < DC ON TACT ,

q = H CT ( T 2 – T 1 )

then contact

if deformable-deformable

q = H CT ( T 2 – T BODY )

If

Main Index

if rigid.

DC ON TACT < d < DQN EAR

and

DQ NEAR

is defined, the last term is only included if

H BL

is defined.

THERMAL CONTACT (3-D) 1073 Define Three-dimensional Thermal or ElectricalContact Conditions

q = H CV ( T 2 – T 1 ) + ( T 2 – T 1 )

B NC

+ σεf ( T 2 – T 1 )

4

⎧ ⎫ S S + ⎨ H CT ⎛ 1 – --------------------------⎞ + H BL -------------------------- ⎬ ( T 1 ) ⎝ DQN EAR⎠ D QN EA R ⎭ ⎩

If

d > DQN EAR 4

4

q = H CTVE ( T 2 – T SINK ) + σε ( T 2 – T SI NK )

The distance below which near contact behavior occurs for thermal and electrical behavior (DQNEAR) needs to be defined in the CONTACT TABLE and can be set for each interface separately. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word THERMAL CONTACT.

2nd data block 1-5

1st

I

Number of surfaces to be defined.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Upper bound to the number of nodes that lie on the periphery of any deformable surface.

16-20

4th

I

Enter 1 to reduce printout of surface definition.

3rd data block 1-10

1st

F

Distance below which a node is considered touching a body (DCONTACT). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

11-20

2nd

F

Contact tolerance BIAS factor. (0-1)

Data blocks 4 through 18 are repeated once for each body to be defined. 4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

Enter 0 for double-sided contact with default search order based upon body ID. For rigid surfaces, enter 1 if surface is a symmetry plane.

Main Index

1074 THERMAL CONTACT (3-D) Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed

Free

Data Entry Entry For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined. For conducting bodies, enter 2 if double-sided contact is used with automatic optimization of the contact constraint equations. Notice that this can be overruled per contact body combination by the CONTACT TABLE option.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Contact body type (optional): 1: rigid body; 4: heat -rigid body. 7: electromagnetic conducting body

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

7th data block

Main Index

1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

THERMAL CONTACT (3-D) 1075 Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

The 8th and 9th data blocks are only necessary for heat transfer. 8th data block 1-10

1st

F

Heat transfer coefficient (film) to environment ( H CVE ).

11-20

2nd

F

Environment sink temperature ( T S INK ).

21-30

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

41-50

5th

F

Enter the convection coefficient for near field behavior ( H CV ).

51-60

6th

F

Enter the natural convection coefficient for near field behavior ( H NC ).

61-70

7th

F

Enter the exponent associated with natural convection ( B NC ).

71-80

8th

F

Enter the surface emissivity for near field behavior ( ε ).

F

Enter the separation distance dependent heat transfer file coefficient ( H BL ).

9th data block 1-10

1st

10th data block The 10th data block is only necessary for Joule heating. 1-10

1st

F

Electrical transfer coefficient to environment.

11-20

2nd

F

Environment sink voltage.

21-30

3rd

F

Contact electrical transfer coefficient.

31-40

4th

F

Body voltage (required for rigid body only).

41-50

5th

F

Electrical transfer coefficient for near field behavior.

51-60

6th

F

Enter the separation distance dependent electrical transfer coefficient.

A. For 3-D Deformable Body The 11th through the 18th data blocks are repeated for each set of body entities (NSURGN). 11a data block 1-80

1st

I

Enter a list of elements of which the body is comprised.

B. For 3-D Rigid Body (Ruled Surface) 11b data block

Main Index

1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

1076 THERMAL CONTACT (3-D) Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed 11-15

Free 3rd

Data Entry Entry I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

21-25

5th

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 12b data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 12b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

C. For 3-D Rigid Body (Surface of Revolution) 11c data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 Method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 12c data block is repeated NPOINT times for surface of revolution. 12c data block

Main Index

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

THERMAL CONTACT (3-D) 1077 Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed

Free

Data Entry Entry

13c data block 1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

D. For 3-D Rigid Surface (Bezier Surface) 11d data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 12d data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 12d data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

E. For 3-D Rigid Surface (4-Node Patch) 11e data block 1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

16-20

4th

I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 12e data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1)

Main Index

1078 THERMAL CONTACT (3-D) Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed

Free

Data Entry Entry

12e data block 1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 13e data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 13e data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

F. For 3-D Rigid Surface (Poly-Surface) 11f data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 12f data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 12f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

G. For 3-D Rigid Surface (NURBS) 11g data block

Main Index

1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

THERMAL CONTACT (3-D) 1079 Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 12g data block is repeated (NPTU ∗ NPTV) for control points. 12g data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 13g data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 13g data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 14g data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 14g data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 15g, 16g, 17g, and 18g. 15g data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 16g data block is repeated NPTU times for control points. 16g data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 17g data block is repeated NPTU times for homogeneous coordinate. 17g data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 18g data block is repeated NPTU+ NORU times for knot vectors. 18g data block 1-10

1st

F

Component of knot vector between 0 and 1.

H. For 3-D Rigid Surface (Cylinder) 11h data block 1-5

Main Index

1st

I

Enter 10 for Cylinder.

1080 THERMAL CONTACT (3-D) Define Three-dimensional Thermal or ElectricalContact Conditions

Format Fixed 6-10

Free 2nd

Data Entry Entry I

Number of subdivisions.

12h data block 1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

I. For 3-D Rigid Surface (Sphere) 11i data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

12i data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

INITIAL TEMP (with TABLE Input - Heat Transfer) 1081 Define Initial Temperatures

INITIAL TEMP (with TABLE Input - Heat Transfer) Define Initial Temperatures The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines initial temperatures for heat transfer problems. Associated with an initial condition name will be the magnitude and location of the initial temperature. The initial condition is activated using the LOADCASE model definition option. The USINC user subroutine or the TABLE model definition option can be used to enter spatially varying initial conditions. Unless heat transfer shells are present, there is only one degree of freedom in a heat transfer analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL TEMP.

2nd data block 1-5

1st

I

Enter the number of sets of initial temperatures (optional).

6-10

2nd

I

Enter unit number for input of initial temperatures data, defaults to input.

Data blocks 3 through 7 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if user subroutines USINC required for this initial condition. Enter 2 if initial temperatures are read from post file.

11-15

3rd

I

Only nonzero if the second field is set to 2. Then this entry defines the unit number from which the post file information is read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

16-20

4th

I

Enter the increment number to be read for initial conditions. If -1 is entered, the last step of the post file is used.

Main Index

21-25

5th

I

Enter 1 if a formatted post file is used.

26-30

6th

I

Enter a 1 if the initial temperature is applied to all the degrees of freedom of a heat transfer shell.

1082 INITIAL TEMP (with TABLE Input - Heat Transfer) Define Initial Temperatures

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

The 4th, 5th, 6th, and 7th data blocks are not used if initial temperatures are read from a post file. For conventional heat transfer element, only one degree of freedom is required. For heat transfer shell elements having more than eight degrees of freedom, the 4th and 5th data blocks are repeated as required giving eight values per set. 4th data block 1-10

1st

F

Initial temperature in first degree of freedom.

11-20

2nd

F

Initial temperature in second degree of freedom.

21-30

3rd

F

Initial temperature in third degree of freedom.

31-40

4th

F

Initial temperature in fourth degree of freedom.

41-50

5th

F

Initial temperature in fifth degree of freedom.

51-60

6th

F

Initial temperature in sixth degree of freedom.

61-70

7th

F

Initial temperature in seventh degree of freedom.

71-80

8th

F

Initial temperature in eighth degree of freedom.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

16-20

4th

I

Table ID associated with the fourth degree of freedom.

21-25

5th

I

Table ID associated with the fifth degree of freedom.

26-30

6th

I

Table ID associated with the sixth degree of freedom.

31-35

7th

I

Table ID associated with the seventh degree of freedom.

36-40

8th

I

Table ID associated with the eighth degree of freedom.

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

Main Index

1st

I

Enter the geometry type: 1:

Element IDs

2:

Nodes IDs

3:

Volume/Region/Body IDs

4:

Surface IDs

5:

Curve IDs

INITIAL TEMP (with TABLE Input - Heat Transfer) 1083 Define Initial Temperatures

Format Fixed

Free

Data Entry Entry 6:

Point IDs

11: Element-Edges IDs 12: Element-Faces ids 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

1084 INITIAL TEMP (Heat Transfer) Define Initial Temperatures

INITIAL TEMP (Heat Transfer)

Define Initial Temperatures

The information provided here is based upon not using the table driven input style. Description This option provides initial temperatures for heat transfer problems. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL TEMP.

I

Enter the number of sets of prescribed temperatures (optional).

2nd data block 1-5

1st

Enter -1 if the USINC user subroutine is used. In this case, data blocks 3 and 4 are not used. 6-10

2nd

I

Enter unit number for input of prescribed temperatures data, defaults to input.

11-15

3rd

I

Flag to indicate that initial conditions read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then, this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Enter step number to be read. If -1 is entered, the last step of the post file is used.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter 1 if all degrees of freedom of all nodes have same initial temperature given in the 9th field.

41-50

9th

F

Enter uniform initial temperature.

3a data block (Not used if 8th field = 1) For analyses which do not include heat transfer shell elements: 1-10

Main Index

1st

F

Initial temperature.

INITIAL TEMP (Heat Transfer) 1085 Define Initial Temperatures

Format Fixed

Free

Data Entry Entry

3b data block (Not used if 8th field = 1) For analyses which include heat transfer shell elements: 1-10

1st

F

Initial temperature in first degree of freedom.

11-20

2nd

F

Initial temperature in second degree of freedom.

21-30

3rd

F

Initial temperature in third degree of freedom. Note:

See Marc Volume B: Element Library for the definition of nodal degrees of freedom.

4th data block (Not used if 8th field = 1) Enter list of nodes for which the above initial temperature is applied.

Main Index

1086 ISOTROPIC (with TABLE Input - Thermal) Define Thermal Properties for Isotropic Materials

ISOTROPIC (with TABLE Input Define Thermal Properties for Isotropic Materials - Thermal) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define thermal properties for an isotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the TABLE model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 are repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the ANKOND and ORIENT user subroutines.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file. Enter -8 if data read in US from database.

Main Index

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

ISOTROPIC (with TABLE Input - Thermal) 1087 Define Thermal Properties for Isotropic Materials

Format Fixed

Free

Data Entry Entry

The data entered in data blocks 4 and 5 are the reference values that are used with tables or are constants. 4th data block 1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

31-40

4th

F

Resistivity (for Joule heating analysis).

41-50

5th

F

Emissivity.

51-60

6th

F

Enter the enthalpy of formation.

61-70

7th

F

Enter the reference temperature of enthalpy of formation.

5th data block 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density (heat transfer).

16-20

4th

I

Table ID for electrical resistivity.

21-25

5th

I

Table ID for emissivity.

26-30

6th

I

Table ID for enthalpy of formation.

31-35

7th

I

Table ID for reference temperature of enthalpy of formation.

6th data block Enter a list of elements associated with this material. Note:

Main Index

Do not enter composite elements which use this material in its layers.

1088 ISOTROPIC (Heat Transfer) Define Thermal Properties for Isotropic Materials

ISOTROPIC (Heat Transfer)

Define Thermal Properties for Isotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define thermal properties for an isotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the TEMPERATURE EFFECTS model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to TEMPERATURE EFFECTS option.

6-10

2nd

I

Enter 1 to call the ANKOND and ORIENT user subroutines.

46-55

8th

A

Enter the material name to cross-reference with material data base for temperature dependent properties.

The data entered in data blocks 4 and 5 should be the values at the lowest temperature expected during an analysis, not necessarily at the initial temperature. 4th data block

Main Index

1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

31-40

4th

F

Resistivity (for Joule heating analysis).

41-50

5th

F

Emissivity (for radiation).

ISOTROPIC (Heat Transfer) 1089 Define Thermal Properties for Isotropic Materials

Format Fixed

Free

Data Entry Entry

5th data block Enter a list of elements associated with this material. Note:

Main Index

Do not enter composite elements which use this material in its layers.

1090 ORTHOTROPIC (with TABLE Input - Thermal) Define Thermal Properties for Orthotropic Materials

ORTHOTROPIC (with TABLE Define Thermal Properties for Orthotropic Materials Input - Thermal) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define thermal properties for an orthotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the TABLE model definition option. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPI.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 8 are repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the ANKOND and ORIENT user subroutines.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file.

Main Index

ORTHOTROPIC (with TABLE Input - Thermal) 1091 Define Thermal Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file. Enter -8 if data read in US from database.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

K11 Thermal conductivities.

11-20

2nd

F

K22 Thermal conductivities.

21-30

3rd

F

K33 Thermal conductivities.

31-40

4th

F

ρ

41-50

5th

F

Specific heat per unit mass.

51-60

6th

F

R11 If Joule heating analysis, resistivities.

61-70

7th

F

R22 If Joule heating analysis, resistivities.

71-80

8th

F

R33 If Joule heating analysis, resistivities.

Mass density.

5th data block Only necessary for input format 2 or greater. 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for mass density.

21-25

5th

I

Table ID for specific heat.

26-30

6th

I

Table ID for R11.

31-35

7th

I

Table ID for R22.

36-40

8th

I

Table ID for R33.

6th data block Only required if RADIATION parameter is present or version is greater or equal to 10.

Main Index

1-10

1st

F

Emissivity (for radiation case).

11-20

2nd

F

Enter the enthalpy of formation.

21-30

3rd

F

Enter the reference temperature of enthalpy of formation.

1092 ORTHOTROPIC (with TABLE Input - Thermal) Define Thermal Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

7th data block Only required if RADIATION parameter is present, input format style 2 or greater or version is greater or equal to 10. 1-5

1st

I

Table ID for emissivity.

6-10

2nd

I

Table ID for enthalpy of formation.

11-15

3rd

I

Table ID for reference temperature of enthalpy of formation.

8th data block Enter a list of elements associated with this material. (Do not enter composite elements that use this material in their layers.)

Main Index

ORTHOTROPIC (Thermal) 1093 Define Thermal Properties for Orthotropic Materials

ORTHOTROPIC (Thermal)

Define Thermal Properties for Orthotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define thermal properties for an orthotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature, use the ORTHO TEMP model definition. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. The data entered in the following blocks should be the values at the lowest temperature expected during an analysis, not necessarily at the initial temperature. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to ORTHO TEMP option.

6-10

2nd

I

Enter 1 to call the ANKOND and ORIENT user subroutines.

4th data block

Main Index

1-10

1st

F

K11 Thermal conductivities.

11-20

2nd

F

K22 Thermal conductivities.

21-30

3rd

F

K33 Thermal conductivities.

1094 ORTHOTROPIC (Thermal) Define Thermal Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

31-40

4th

F

ρ

41-50

5th

F

Specific heat per unit mass.

51-60

6th

F

R11

61-70

7th

F

R22 If Joule heating analysis, resistivities.

71-80

8th

F

R33 If Joule heating analysis, resistivities.

Mass density. If Joule heating analysis, resistivities.

5th data block Only required if RADIATION parameter is present. 1-10

1st

F

Emissivity (for radiation).

6th data block Enter a list of elements associated with this material. (Do not enter composite elements that use this material in their layers.)

Main Index

ANISOTROPIC (with TABLE Input - Thermal) 1095 Model Definition Option for Heat Transfer Analysis

ANISOTROPIC (with TABLE Input - Thermal)

Model Definition Option for Heat Transfer Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option specifies thermal properties defined by a call to user subroutines ANKOND and ORIENT. The ANKOND user subroutine must be used for the input of constant or temperature dependent anisotropic thermal conductivities (K11, K22, K33) and/or resistivities (R11, R22, R33) defined in the user coordinate (1,2,3) system. The TABLE model definition option can be used for the definition of material properties with temperatures. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ANISOTROPI.

2nd data block 1-5

1st

I

Enter the number of anisotropic data sets to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 10 are repeated as a set NSET times. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing the ANKOND and ORIENT user subroutines.

6-10

2nd

I

Enter 1 if the ANKOND user subroutine is to be called. Enter 2 if the anisotropic conductivity is to be entered in the 4a data block.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Enter 4 if Marc database is used for flow stress. Enter 5 if MATILDA database is used. Enter 6 if data read in SI-mm from input file. Enter -6 if data read in SI-mm from database. Enter 7 if data read in SI-m from input file. Enter -7 if data read in SI-m from database. Enter 8 if data read in US from input file.

Main Index

1096 ANISOTROPIC (with TABLE Input - Thermal) Model Definition Option for Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry Enter -8 if data read in US from database.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

4th data block 1-10

1st

F

Mass density.

11-20

2nd

F

Specific heat per unit mass.

21-30

3rd

F

Emissivity (for radiation case).

31-40

4th

F

Enter the enthalpy of formation (only required if SURFACE ENERGY is included).

41-50

5th

F

Enter the reference temperature of enthalpy of formation.

5th data block 1-5

1st

I

Table ID for mass density.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for emissivity.

16-20

4th

I

Table ID for enthalpy of formation.

21-25

5th

I

Table ID for reference temperature of enthalpy of formation.

Data blocks 6 to 9 are only required if the second field of the 3rd data block is a 2. 6th data block 1-10

1st

F

K11

11-20

2nd

F

K12

21-30

3rd

F

K13

31-40

4th

F

K22

41-50

5th

F

K23

51-60

6th

F

K33

7th data block

Main Index

1-5

1st

I

K11 Table ID for conductivity.

6-10

2nd

I

K12 Table ID for conductivity.

11-20

3rd

I

K13 Table ID for conductivity.

21-30

4th

I

K22 Table ID for conductivity.

31-40

5th

I

K23 Table ID for conductivity.

41-50

6th

I

K33 Table ID for conductivity.

ANISOTROPIC (with TABLE Input - Thermal) 1097 Model Definition Option for Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

Data blocks 8 and 9 are only required for Joule heating, and the second field of the 3rd data block is a 2. 8th data block 1-10

1st

E

R11 If Joule heating analysis, resistivities.

11-20

2nd

E

R12 If Joule heating analysis, resistivities.

21-30

3rd

E

R13 If Joule heating analysis, resistivities.

31-40

4th

E

R22 If Joule heating analysis, resistivities.

41-50

5th

E

R23 If Joule heating analysis, resistivities.

51-60

6th

E

R33 If Joule heating analysis, resistivities.

9th data block 1-5

1st

I

Table ID for R11.

6-10

2nd

I

Table ID for R12.

11-15

3rd

I

Table ID for R13.

16-20

4th

I

Table ID for R22.

21-25

5th

I

Table ID for R23.

26-30

6th

I

Table ID for R33.

10th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

1098 ANISOTROPIC (Thermal) Model Definition Option for Heat Transfer Analysis

ANISOTROPIC (Thermal)

Model Definition Option for Heat Transfer Analysis

The information provided here is based upon not using the table driven input style. Description This option specifies thermal properties defined by a call to the ANKOND and ORIENT user subroutines. The ANKOND user subroutine must be used for the input of constant or temperature dependent anisotropic thermal conductivities (K11, K22, K33) and/or resistives (R11, R22, R33) defined in the user coordinate (1,2,3) system. The TEMPERATURE EFFECTS model definition option can be used for the input of variations of specific heat with temperatures. Note that the data entered in this option should be the values at the lowest temperature expected during an analysis, not necessarily at the initial temperature. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ANISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of anisotropic data sets to follow (optional)

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 7 are repeated as a set NSET times. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing the ANKOND and ORIENT user subroutines, as well as to the TEMPERATURE EFFECTS option.

6-10

2nd

I

Enter 1 if the ANKOND user subroutine is to be called. Enter 2 if the anisotropic conductivity is to be entered in the 4a data block.

4th data block 1-10

1st

F

Mass density.

11-20

2nd

F

Specific heat per unit mass.

21-30

3rd

F

Emissivity (for radiation).

Data blocks 5 and 6 are only required if the second field of the 3rd data block is a 2.

Main Index

ANISOTROPIC (Thermal) 1099 Model Definition Option for Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

K11

11-20

2nd

F

K12

21-30

3rd

F

K13

31-40

4th

F

K22

41-50

5th

F

K23

51-60

6th

F

K33

Data block 6 is only required for Joule heating. 6th data block 1-10

1st

F

R11

11-20

2nd

F

R12

21-30

3rd

F

R13

31-40

4th

F

R22

41-50

5th

F

R23

51-60

6th

F

R33

7th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

1100 LATENT HEAT Define Latent Heat

LATENT HEAT

Define Latent Heat

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option is used to define the latent heat introduced into the system due to a phase change in the material. It is an alternative input to the TEMPERATURE EFFECTS option when the table driven input format is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words LATENT HEAT.

2nd data block 1-5

1st

I

Number of latent heats.

6-10

2nd

I

Material id.

11-15

3rd

I

Unit number to read input; defaults to standard input.

Repeat 3rd data block for each phase change. 3rd data block

Main Index

1-10

1st

E

Enter the latent heat value.

11-20

2nd

E

Solidus temperature (lower phase change limit).

21-30

3rd

E

Liquids temperature (upper phase change limit).

TEMPERATURE EFFECTS (Heat Transfer) 1101 Define Variation of Material Properties in Heat Transfer Analysis

TEMPERATURE EFFECTS (Heat Transfer)

Define Variation of Material Properties in Heat Transfer Analysis

The information provided here is based upon not using the table driven input style. This option is not available with the table driven input. Description This option defines the variation of material properties (conductivity, specific heat and electrical resistance) with temperature. The values read in through the ISOTROPIC option are those at the lowest temperature specified. Properties are not defined below the lowest temperature. The temperature dependency can be entered using one of the following two options: a. The variation of a particular property with temperature is specified as a piecewise linear curve. Breakpoints must be given in ascending order of temperature. b. The particular property value and temperature lying on the relevant curve are input directly. Data points must be given in ascending order of temperature. This option is flagged by entering the word “DATA” on the first data line. Note:

In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment. The temperature at the end of the increment is an estimated value.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the word TEMPERATURE EFFECTS.

21-80

2nd

A

Enter the word DATA to indicate that Option B is used.

For option A, use data blocks 2a through 7a. For option B, use data blocks 2b through 7b. Option A 2a data block

Main Index

1-5

1st

I

Number of slopes of conductivity versus temperature curve.

6-10

2nd

I

Number of slopes of specific heat versus temperature curve.

11-15

3rd

I

Number of latent heats to be entered.

16-20

4th

I

Number of slopes of resistivity versus temperature curve for Joule heating problem.

1102 TEMPERATURE EFFECTS (Heat Transfer) Define Variation of Material Properties in Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Number of slopes for emissivity versus temperature curve for radiating cavities.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Material type identification (1,2,3...) for cross-reference to the ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to blocks.

3a data block Conductivity variation. Number of blocks as given on data block 2, first field. 1-15

1st

F

Slope of conductivity versus temperature curve.

16-30

2nd

F

Temperature above which above slope becomes operative.

4a data block Specific heat variation. Number of blocks as given on data block 2, second field. 1-15

1st

F

Slope of specific heat versus temperature curve.

16-30

2nd

F

Temperature above which above slope becomes operative.

5a data block Latent heat. Number of blocks given on data block 2, third field. 1-15

1st

F

Latent heat.

16-30

2nd

F

Solidus temperature (lower phase change limit).

31-45

3rd

F

Liquidus temperature (upper phase change limit).

6a data block Resistivity variation for Joule heating problem. Number of blocks given on data block 2, fourth field. 1-15

1st

F

Slope of resistivity versus temperature curve.

16-30

2nd

F

Temperature above which above slope becomes operative.

7a data block Emissivity variation for radiating cavity problems. Number of blocks given on data block 2, fifth field. 1-15

1st

F

Slope of emissivity versus temperature curve.

16-30

2nd

F

Temperature above which the above slope becomes operative.

Option B 2b data block

Main Index

1-5

1st

I

Number of data points on the conductivity versus temperature curve.

6-10

2nd

I

Number of data points on the specific heat versus temperature curve.

11-15

3rd

I

Number of latent heats to be entered.

TEMPERATURE EFFECTS (Heat Transfer) 1103 Define Variation of Material Properties in Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Number of data points on the resistivity versus temperature curve for Joule heating problem.

21-25

5th

I

Number of data points on the emissivity versus the temperature curve.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Material type identification (1,2,3...) for cross-reference to ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to blocks.

3b data block Conductivity variation. Number of blocks as given on data block 2, first field. 1-15

1st

F

Enter the value of the conductivity.

16-30

2nd

F

Enter the associated temperature.

4b data block Specific heat variation. Number of blocks as given on data block 2, second field. 1-15

1st

F

Enter the value of the specific heat.

16-30

2nd

F

Enter the associated temperature.

5b data block Latent heat. Number of blocks given on data block 2, third field. 1-15

1st

F

Latent heat.

16-30

2nd

F

Solidus temperature (lower phase change limit).

31-45

3rd

F

Liquidus temperature (upper phase change limit).

6b data block Resistivity variation for Joule heating problem. Number of blocks given on data block 2, fourth field. 1-15

1st

F

Enter the value of the resistivity.

16-30

2nd

F

Enter the associated temperature.

7b data block Emissivity variation for radiating cavity problem. Number of blocks given on data block 2, fifth field.

Main Index

1-15

1st

F

Enter the value of the emissivity.

16-30

2nd

F

Enter the associated temperature.

1104 ORTHO TEMP (Thermal) Define Variation of Orthotropic Thermal Properties

ORTHO TEMP (Thermal)

Define Variation of Orthotropic Thermal Properties

The information provided here is based upon not using the table driven input style. This option is not available with the table driven input. Description This option defines the variation of all orthotropic thermal properties with temperature. Note that the values read in through the ORTHOTROPIC model definition are those at the lowest temperature defined. Properties at temperatures below this temperature are defined to be equal to properties at this temperature. The variation of a particular property is defined as a piecewise linear curve. Two options are available to define this curve. a. Slope/breakpoint data in ascending order of temperature can be given. b. Property value/temperature data in ascending order of temperature can be given. This option is flagged by entering the word “DATA” after the string ORTHO TEMP on the first data block. Note:

In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment. The temperature at the end of the increment is an estimated value.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the string ORTHO TEMP.

11-80

2nd

A

Enter the word DATA to indicate that option B defined above is to be used. Note:

For option A, use data blocks 2a-11a. For option B, use data blocks 2b-11b.

Option A 2a data block 1-5

1st

I

Number of slopes of K11 vs. temperature curve.

6-10

2nd

I

Number of slopes of K22 vs. temperature curve. Enter -1 to have (K22 vs. temp.) ≡ (K11 vs. temp.).

11-15

3rd

I

Number of slopes of K33 vs. temperature curve. Enter -1 to have (K33 vs. temp.) ≡ (K11 vs. temp.).

Main Index

ORTHO TEMP (Thermal) 1105 Define Variation of Orthotropic Thermal Properties

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Number of slopes of specific heat vs. temperature curve.

21-25

5th

I

Number of latent heats.

26-30

6th

I

In a Joule heating analysis, number of slopes of R11 vs. temperature curve.

31-35

7th

I

In a Joule heating analysis, number of slopes of R22 vs. temperature curve. Enter -1 to have (R22 vs. temp.) ≡ (R11 vs. temp.).

36-40

8th

I

In a Joule heating analysis, number of slopes of R33 vs. temperature curve. Enter -1 to have (R33 vs. temp.) ≡ (R11 vs. temp.)

. 41-45

9th

I

Number of slopes of emissivity vs. temperature curve for radiating cavities.

46-50

10th

I

Enter the material identification (1,2,3, etc.) for this data set.

51-55

11th

I

Enter the unit number for input. Defaults to input file.

3a data block The number of blocks in this series is the number in the 2a data block, first field. 1-15

1st

F

Enter the slope of K11 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

4a data block The number of blocks in this series is n, the number in the 2a data block, second field, or 0 if n = -1. 1-15

1st

F

Enter the slope of K22 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

5a data block The number of blocks in this series is n, the number in the 2a data block, third field, or 0 if n = -1. 1-15

1st

F

Enter the slope of K33 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

6a data block The number of blocks in this series is the number in the 2a data block, fourth field. 1-15

1st

F

Enter the slope of specific heat vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

7a data block The number of blocks in this series is the number in the 3a data block, fifth field.

Main Index

1-15

1st

F

Enter latent heat value.

16-30

2nd

F

Solidus temperature (lower phase change limit).

1106 ORTHO TEMP (Thermal) Define Variation of Orthotropic Thermal Properties

Format Fixed 31-45

Free 3rd

Data Entry Entry F

Liquidus temperature (upper phase change limit).

8a data block The number of blocks in this series is the number in the 2a data block, sixth field. 1-15

1st

F

Enter the slope of R11 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

9a data block The number of blocks in this series is n, the number in the 2a data block, seventh field, or 0 if n = -1. 1-15

1st

F

Enter the slope of R22 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

10a data block The number of blocks in this series is n, the number in the 2a data block, eighth field, or 0 if n = -1. 1-15

1st

F

Enter the slope of R33 vs. temperature curve.

16-30

2nd

F

Temperature at which above slope becomes operative.

11a data block The number of blocks in this series is the number in the 2a data block, ninth field. 1-15

1st

F

Enter the slope of emissivity vs. temperature curve.

16-30

2nd

F

Temperature at which the above slope becomes operative.

Option B 2b data block 1-5

1st

I

Number of data points of K11 vs. temperature curve.

6-10

2nd

I

Number of data points of K22 vs. temperature curve. Enter -1 to have (K22 vs. temp.) ≡ (K11 vs. temp.)

11-15

3rd

I

Number of data points of K33 vs. temperature curve. Enter -1 to have (K33 vs. temp.) ≡ (K11 vs. temp.)

16-20

4th

I

Number of data points of specific heat vs. temperature curve.

21-25

5th

I

Number of latent heats.

26-30

6th

I

In a Joule heating analysis, number of data points of R11 vs. temperature curve.

31-35

7th

I

In a Joule heating analysis, number of data points of R22 vs. temperature curve. Enter -1 to have (R22 vs. temp.) ≡ (R11 vs. temp.).

Main Index

ORTHO TEMP (Thermal) 1107 Define Variation of Orthotropic Thermal Properties

Format Fixed 36-40

Free 8th

Data Entry Entry I

In a Joule heating analysis, number of data points of R33 vs. temperature curve. Enter -1 to have (R33 vs. temp.) ≡ (R11 vs. temp.).

41-45

9th

I

Number of data points of emissivity versus temperature curve.

46-50

10th

I

Enter the material identification (1, 2, 3, etc.) for this data set.

51-55

11th

I

Enter the unit number for input. Defaults to input file.

3b data block The number of blocks in this series is the number in the 2b data block, first field.) 1-15

1st

F

Enter the value of K11.

16-30

2nd

F

Enter the associated temperature.

4b data block The number of blocks in this series is n, the number in the 2b data block, second field, or 0 if n = -1. 1-15

1st

F

Enter the value of K22.

16-30

2nd

F

Enter the associated temperature.

5b data block The number of blocks in this series is n, the number in the 2b data block, third field, or 0 if n = -1. 1-15

1st

F

Enter the value of K33.

16-30

2nd

F

Enter the associated temperature.

6b data block The number of blocks in this series is the number in the 2b data block, fourth field. 1-15

1st

F

Enter the value of specific heat

16-30

2nd

F

Enter the associated temperature.

7b data block The number of blocks in this series is the number in the 2b data block, fifth field. 1-15

1st

F

Enter latent heat value.

16-30

2nd

F

Solidus temperature (lower phase change limit).

31-45

3rd

F

Liquidus temperature (upper phase change limit).

8b data block The number of blocks in this series is the number in the 2b data block, sixth field.

Main Index

1-15

1st

F

Enter the value of R11.

16-30

2nd

F

Enter the associated temperature.

1108 ORTHO TEMP (Thermal) Define Variation of Orthotropic Thermal Properties

Format Fixed

Free

Data Entry Entry

9b data block The number of blocks in this series is n, the number in the 2b data block, seventh field, or 0 if n = -1. 1-15

1st

F

Enter the value of R22.

16-30

2nd

F

Enter the associated temperature.

10b data block The number of blocks in this series is n, the number in the 2b data block, eighth field, or 0 if n = -1. 1-15

1st

F

Enter the value of R33.

16-30

2nd

F

Enter the associated temperature.

11b data block The number of blocks in this series is the number in the 2b data block, ninth field.

Main Index

1-15

1st

F

Enter the value of the emissivity.

16-30

2nd

F

Enter the associated temperature.

CONTROL (Heat Transfer - Model Definition) 1109 Define Control Parameters for Heat Transfer Analysis

CONTROL (Heat Transfer - Define Control Parameters for Heat Transfer Analysis Model Definition) Description This option allows you to input parameters governing the convergence solution and accuracy for heat transfer analysis. For heat transfer analysis, the only data field required to be set is the maximum number of steps, the first field in the second data block. All other fields can, in these cases, be left blank but notice that the 3rd data block must be included. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block

Main Index

1-5

1st

I

Maximum number of load steps in this run. Default is 99999. This is a cumulative number and is usually used to stop the run when RESTART is being used.

6-10

2nd

I

Maximum number of recycles during an increment due to temperature dependent material properties. Default value is 3.

11-15

3rd

I

Minimum number of recycles during an increment. Note that this data field forces this number of recycles to take place in all subsequent increments.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced.

36-40

8th

I

Not used; enter 0.

41-45

9th

I

Not used; enter 0.

46-50

10th

I

Not used; enter 0.

51-55

11th

I

Not used; enter 0.

56-60

12th

I

Assembly flag. If set to 1, the conductivity matrix is assembled each iteration.

1110 CONTROL (Heat Transfer - Model Definition) Define Control Parameters for Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

3rd data block

Main Index

1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are reevaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Maximum change of xsi,p allowed in pyrolysis calculation. Used to control automatic time step scheme.

51-60

6th

F

Maximum change of xsi,v allowed in pyrolysis calculation. Used to control automatic time step scheme.

61-70

7th

F

Maximum change of xsi,c allowed in pyrolysis calculation. Used to control automatic time step scheme.

71-80

8th

F

Maximum change in surface displacement per time step due to recession. This is used to control the time step for the TRANSIENT option.

CONVERT 1111 Define Conversion Factors

CONVERT

Define Conversion Factors

Description This option sets a converting factor when a physical quantity is converted to another physical quantity. This is useful when the units used for the different physics are not consistent (that is, when SI units are not used), or when there are losses in the process. In the coupled thermal-stress analysis, depending on the units used for the passes, different conversion factors must be used. In addition, following the work of Farren and Taylor, not all inelastic work is dissipated into heat; for most metals, about 90% is converted11. This should also be considered when defining this conversion factor. In the Joule heating analysis or coupled electromagnetic thermal analysis, depending on the units used for the passes, different conversion factors must be used. For example, in an Joule heating problem, the heat generation due to the electric current can be expressed in terms of current and resistance as q = I2R. If the units of current and resistance are (amp) and (ohm/ft), respectively, then the unit of heat generation in the electric problem must be (watt/ft). Since 1 (watt) is equal to 3.4129 (btu/hr), a factor of 3.4129 must be used in a Joule heating problem, for the purpose of converting the unit of heat generation from (watt/ft) to (btu/hr-ft) for heat transfer analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONVERT.

2nd data block 1-10

1st

F

Heat generation conversion factor between inelastic mechanical energy and heat transfer flux in a coupled analysis. Default is1.0.

11-20

2nd

F

Heat generation conversion factor between energy due to friction and heat generated in a coupled contact analysis. Defaults to the value given in the first field.

21-30

3rd

F

Heat generation conversion factor between electric current and heat transfer flux. This can be used in both a Joule heating analysis and an electromagnetic thermal analysis. Default is 1.0.

11

Main Index

S. W. Farren, G. I. Taylor. “The Heat Developed During Plastic Extension of Metals”, Proceedings of the Royal Society, London, A107, p. 422, 1925.

1112 CONRAD GAP Define Convection/Radiation Gap

CONRAD GAP

Define Convection/Radiation Gap

Description This option allows you to input emissivity, film coefficient, and gap closure temperature for convection/radiation gap option. The Stefan-Boltzmann and conversion to absolute temperatures is done via the PARAMETERS option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONRAD GAP.

2nd data block 1-5

1st

I

Number of sets of data used to input CONRAD GAP.

6-10

2nd

I

Unit number for input of CONRAD GAP data; defaults to input.

3rd data block 1-5

1st

I

Face identification – see Marc Volume B: Element Library. Note that these identifiers are different from those used for DIST FLUXES.

6-15

2nd

F

Emissivity

16-25

3rd

F

Not used; enter 0.

26-35

4th

F

Not used; enter 0.

36-45

5th

F

Film coefficient.

46-55

6th

F

GAP closure temperature.

56-60

7th

I

Table ID for emissivity.

61-65

8th

I

Table ID for film coefficient.

66-70

9th

I

Table ID for gap closure temperature.

4th data block Enter a list of elements to which the above CONRAD GAP data is applied.

Main Index

CHANNEL 1113 Define Fluid Channel Input

CHANNEL

Define Fluid Channel Input

Description This option allows you to input inlet temperature, fluxes, and film coefficient for a fluid channel in a heat transfer analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CHANNEL.

2nd data block 1-5

1st

I

Number of sets of data used to input fluid channels.

6-10

2nd

I

Unit number for input of fluid channels data; defaults to input.

3rd data block 1-5

1st

I

Face identification – see Marc Volume B: Element Library. Note that these identifiers are different from those used for DIST FLUXES.

6-10

2nd

I

First (inlet) element number in the channel.

11-20

3rd

F

Inlet temperature.

21-30

4th

F

Mass flow rate.

31-40

5th

F

Film coefficient.

41-45

6th

I

Table ID for inlet temperature.

46-50

7th

I

Table ID for mass flow rate.

51-55

8th

I

Table ID for film coefficient.

4th data block Enter a list of elements to which the above fluid channel data is applied.

Main Index

1114 VIEW FACTOR Read in Radiation View Factors

VIEW FACTOR

Read in Radiation View Factors

Description This option initiates the reading of radiation view factors created by Marc Mentat using the Monte Carlo procedure. This file is read as vfid.vfs where vfid is entered using the -vf option when invoking Marc. The RADIATION parameter is required and the 2nd field on this parameter is a 2. Format Format Fixed 1-11

Main Index

Free 1st

Data Entry Entry A

Enter the words VIEW FACTOR.

RADIATING CAVITY 1115 Define Outline of Radiating Cavity

RADIATING CAVITY

Define Outline of Radiating Cavity

Description This option allows for the input of the outlines of radiating cavities. Each cavity outline is defined by a group of nodal points in a counter clockwise direction. The RADIATION parameter is required and the 2nd field on this parameter is a 1. This method may only be used for axisymmetric solid elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-16

1st

A

Enter the word RADIATING CAVITY.

2nd data block 1-5

1st

I

Total number of cavities.

6-10

2nd

I

Unit number for input. Default is 5 (input).

3rd data block Enter a list of nodes defining the outline of a cavity. Repeat for each cavity to be defined. Note:

Main Index

List verbs EXCEPT and INTERSECT are illegal in these nodal lists.

1116 RAD-CAVITY Define Radiation Cavity

RAD-CAVITY

Define Radiation Cavity

Description This option defines a radiation boundary condition. The cavity geometry is specified through the CAVITY DEFINITION option. If required, the view factors will be first calculated. In a coupled analysis, this option may be used to control the frequency of recalculating the view factors. The RADIATION parameter is required and the 2nd field on this parameter is a 3 or a 4. The CAVITY DEFINITION option must also be used to define the shape of the cavity. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words RAD-CAVITY.

2nd data block 1-5

1st

I

Enter the number of sets of radiation boundary conditions to be entered (optional).

6-10

2nd

I

Enter unit number for input of radiation boundary condition data, defaults to input.

3rd data block 1-5

1st

I

Enter number of lines used in card series 6 (default is 1).

6-10

2nd

I

Enter 0 to calculate view factors. Enter 1 to read view factors from a file jid_cnn.vfs, where nn is the cavity ID.

11-15

3rd

I

Enter increment frequency to recalculate view factors.

16-20

4th

I

Enter 0 cavity is closed. Enter 1 cavity is closed and scale view factors. Enter 2 cavity is open.

21-25

5th

I

Enter 1 to make Radiation Exchange Matrix Symmetric. This matrix is defined by A j ⋅ F i j . If 1 is entered, the viewfactors are scaled for closed cavities. Default is 0 and symmetry is not guaranteed.

Main Index

26-30

6th

I

Enter a 1 if a post file is to be created that may be used to visualize the view factors.

31-62

7th

A

Enter the unique label associated with this radiation boundary condition. This label will be referenced by the LOADCASE option.

RAD-CAVITY 1117 Define Radiation Cavity

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

E

Temperature at infinity for an open cavity. If a control node is provided in the CAVITY DEFINITION, the temperature entered here is ignored.

11-20

2nd

E

Enter the change in coordinates before view factors will be recalculated. Only used if 7th field of RADIATION parameter is set to 1.

I

Table ID for Temperature at infinity for an open cavity.

5th data block 1-5

1st

6th data block (Repeat based upon 3rd block, first entry) Enter a list of cavity IDs.

Main Index

1118 CAVITY DEFINITION Define Geometry of a Cavity

CAVITY DEFINITION

Define Geometry of a Cavity

Description This option defines the geometric outline of the cavity, including symmetry surface information. This option is used when the hemi-cube method is used to calculate the view factors, and is used in conjunction with the RAD-CAVITY and EMISSIVITY options. The RADIATION parameter is required and the 2nd field on this parameter is a 3 or a 4. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words CAVITY DEFINITION.

2nd data block 1-5

1st

I

Enter the number of cavities.

6-10

2nd

I

Enter the unit number to read input.

Repeat the 3rd, 4th, 5th, 6th, 7th, 8th, and 9th data blocks for each radiating cavity. 3rd data block 1-5

1st

I

Enter the cavity number.

6-10

2nd

I

Enter the number of geometry types to define cavity.

11-15

3rd

I

Enter the number of symmetry surfaces to be used, maximum is 16.

16-20

4th

I

Control Node ID. Used for determining environment temperature – 1st degrees of freedom is used. If the cavity is closed, this is not used.

4th data block - Enter as many as 16 symmetry surface ids 1-5

1st

I

Enter first symmetry ID If positive number then ID comes from the SYMMETRY option. If negative number then ID comes from the SURFACES option.

6-10

2nd

I

Enter second symmetry ID If positive number then ID comes from the SYMMETRY option. If negative number then ID comes from the SURFACES option.

11-15

3rd

I

Enter third symmetry ID. If positive number then ID comes from the SYMMETRY option. If negative number then ID comes from the SURFACES option.

Main Index

CAVITY DEFINITION 1119 Define Geometry of a Cavity

Format Fixed

Free

Data Entry Entry

5th data block If geometry type is element IDs(1), use either the first or the second and third field. If geometry type is surface(4) or curve(5), use the second field only. 1-5

1st

I

Enter the ibody type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter 1.

11-15

3rd

I

Enter the face ID or edge ID.

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 2nd field. 6th data block 1-5

1st

I

Enter the geometry type 1: Element IDs, top side if shell element 4: Surface IDs, top side if shell element 5: Curve IDs, top side if shell element 11: Element-Edge IDs, top side if shell element 12: Element-Face IDs, top side if shell element 13: Element-Edge IDs - Mentat convention, top side if shell element 14: Element-Face IDs - Mentat convention, top side if shell element 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Mentat convention 19: Curve ID: orientation ID - Mentat convention 21: Element IDs, bottom side if shell element 24: Surface IDs, bottom side if shell element 25: Curve IDs, bottom side if shell element 31: Element-Edge IDs, bottom side if shell element 32: Element-Face IDs, bottom side if shell element 33: Element-Edge IDs - Mentat convention, bottom side if shell element 34: Element-Face IDs - Mentat convention, bottom side if shell element 41: Element IDs, both sides if shell elements 44: Surface IDs, both sides if shell elements 45: Curve IDs, both sides if shell elements

Main Index

1120 CAVITY DEFINITION Define Geometry of a Cavity

Format Fixed

Free

Data Entry Entry 51: Element-Edge IDs, both sides if shell elements 52: Element-Face IDs, both sides if shell elements 53: Element-Edge IDs - Mentat convention, both sides if shell elements 54: Element-Face IDs - Mentat convention, both sides if shell elements.

7th data block 1-80

Main Index

Enter a list of geometric entities to define the cavity. The geometric entities must all be of the type prescribed in the 6th data block.

EMISSIVITY 1121 Define Emissivity

EMISSIVITY

Define Emissivity

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option is used to define the diffuse surface radiation behavior. Separate emissivity and absorption values may be entered. The properties may be a function of the spatial coordinate, the temperature, and/or the frequency. This option is used in conjunction with the CAVITY DEFINITION and RAD-CAVITY options. Note:

If the emissivity is spectral dependent, then the absorption equals the emissivity at each frequency. The wavelength may be given in any units; i.e. m or μm, but the frequency used for table evaluation is based upon the wavelength and the speed of radiation given in the PARAMETERS option. They should be in consistent units. The emissivity is assumed to have a linear variation within each band.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words EMISSIVITY.

2nd data block 1-5

1st

I

Enter the number of data sets.

6-10

2nd

I

Enter the unit number.

11-15

3rd

I

Enter 0 for new style input. Enter 1 for MD Nastran style definition of spectral emissivity.

Repeat the 3rd, 4th, and 5th data blocks for each different surface radiation property. 3rd data block 1-5

1st

I

Enter the emissivity ID.

6-10

2nd

I

Enter the number of geometries that this emissivity will be applied to.

11-15

3rd

I

If input mode 1, then enter the number of wavebands of spectral emissivity.

4th data block

Main Index

1-10

1st

E

Enter the emissivity coefficient.

11-20

2nd

E

Enter the absorption coefficient.

1122 EMISSIVITY Define Emissivity

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Enter the table ID for emissivity coefficient.

6-10

2nd

I

Enter the table ID for absorption coefficient.

6th data block (Only used is input mode is 1 and the spectral emissivity is included. Repeat for each band.) 1-10

1st

E

Enter the wavelength at the start of the band.

11-20

2nd

E

Enter the wavelength at the end of the band.

21-30

3rd

E

Enter the emissivity at the start of the band.

31-40

4th

E

Enter the emissivity at the end of the band.

41-45

5th

I

Enter the table ID associated with the emissivity at the start of the band.

46-50

6th

I

Enter the table ID associated with the emissivity at the end of the band.

7th data block If geometry type is element ids(1), use either the first or the second and third field. If geometry type is surface(4) or curve(5), use the second field only. 1-5

1st

I

Enter the ibody type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter 1.

11-15

3rd

I

Enter the face ID or edge ID.

The 8th and 9th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 2nd field. 8th data block 1-5

1st

I

Enter the geometry type 1: Element IDs, top side if shell element 4: Surface IDs, top side if shell element 5: Curve IDs, top side if shell element 11: Element-Edge IDs, top side if shell element 12: Element-Face IDs, top side if shell element 13: Element-Edge IDs - Marc Mentat convention, top side if shell element 14: Element-Face IDs - Marc Mentat convention, top side if shell element. 16: Surface ID: orientation ID 17: Curve ID: orientation ID

Main Index

EMISSIVITY 1123 Define Emissivity

Format Fixed

Free

Data Entry Entry 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention 21: Element IDs, bottom side if shell element 24: Surface IDs, bottom side if shell element 25: Curve IDs, bottom side if shell element 31: Element-Edge IDs, bottom side if shell element 32: Element-Face IDs, bottom side if shell element 33: Element-Edge IDs - Marc Mentat convention, bottom side if shell element 34: Element-Face IDs - Marc Mentat convention, bottom side if shell element. 41: Element IDs, both sides if shell elements 44: Surface IDs, both sides if shell elements 45: Curve IDs, both sides if shell elements 51: Element-Edge IDs, both sides if shell elements 52: Element-Face IDs, both sides if shell elements 53: Element-Edge IDs - Marc Mentat convention, both sides if shell elements 54: Element-Face IDs - Marc Mentat convention, both sides if shell elements.

9th data block 1-80

Main Index

Enter a list of geometric entities to define the cavity.

1124 VELOCITY (with TABLE Input - Convective Heat Transfer) Define Nodal Velocity Components

VELOCITY (with TABLE Input - Convective Define Nodal Velocity Components Heat Transfer) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows the specification of the nodal velocity components in a heat transfer analysis, where the convective terms are to be included. The convective option is specified by placing a 2 in the fifth field of the HEAT parameter. This activates the nonsymmetric solver as well. The nodal velocity components are defined by specifying the velocity magnitude of a series of components for sets of nodes. Moreover, the velocity values can be specified via the UVELOC user subroutine (see Marc Volume D: User Subroutines and Special Routines). If the motion of the media is to be calculated, a coupled fluid-thermal analysis should be performed. Note:

The convective velocities are not applied to heat transfer shell elements.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words VELOCITY.

2nd data block 1-5

1st

I

Enter the number of sets of velocity (optional).

6-10

2nd

I

Enter unit number for input of velocity data, defaults to input.

Data blocks 3 through 7 are entered as pairs; one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the UVELOC user subroutine required for this initial condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

VELOCITY (with TABLE Input - Convective Heat Transfer) 1125 Define Nodal Velocity Components

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

E

Velocity in first coordinate direction.

11-20

2nd

E

Velocity in second coordinate direction.

21-30

3rd

E

Velocity in third coordinate direction.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first coordinate direction.

6-10

2nd

I

Table ID associated with the second coordinate direction.

11-15

3rd

I

Table ID associated with the third coordinate direction.

I

Enter the geometry type:

6th data block 1-5

1st

1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention 7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

1126 VELOCITY (Convective Heat Transfer) Define Nodal Velocity Components

VELOCITY (Convective Heat Transfer)

Define Nodal Velocity Components

The information provided here is based upon not using the table driven input style. Description This option allows the specification of the nodal velocity components in a heat transfer analysis, where the convective terms are to be included. The convective option is specified by placing a 2 in the fifth field of the HEAT parameter. This activates the nonsymmetric solver as well. The nodal velocity components are defined by specifying the velocity magnitude of a series of components for sets of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the velocity values can be respecified, or initialized if no previous data was entered via user subroutine UVELOC (see Marc Volume D: User Subroutines and Special Routines). A summary of nodal velocities appears in the printout. This can be suppressed by specifying a nonzero value for the print-suppress parameter. If the motion of the media is to be calculated, a coupled fluid-thermal analysis should be performed. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VELOCITY.

2nd data block 1-5

1st

I

Number of data blocks used to input nodal velocity components. If a negative value is entered, the UVELOC user subroutine is called for every node.

6-10

2nd

I

Enter the unit number for input of the velocity field. Default to unit 5, unless the INPUT TAPE parameter has been used.

11-15

3rd

I

Set to 1 to suppress printout of the summary of nodal velocity components.

Data blocks 3, 4 and 5 should be repeated for each data set. 3rd data block 1-10

1st

F

Enter the magnitude of the velocity in the first coordinate-direction for which the velocity is given. Additional velocity components in other coordinate directions must be specified on the same data line in F10 format. The number of components must equal the number of directions.

Main Index

VELOCITY (Convective Heat Transfer) 1127 Define Nodal Velocity Components

Format Fixed

Free

Data Entry Entry

4th data block Enter a list of coordinate directions in which the velocity is specified. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes for which the velocity vector as defined in data blocks 3 and 4.

Main Index

1128 CURE RATE Cure Kinetics

CURE RATE

Cure Kinetics

Description This option is used to define the curing property parameters of materials.This property is used to couple the curing effect for heat transfer or thermal/mechanical problems. There are three choices for this option. Each choice corresponds to its own input data format. Option A: Embedded Models This option allows you to choose one of the four cure models built into the Marc program. Default is a no cure kinetics model. Option B: Table Defined Models This option allows you to define the cure kinetics model in the table format. In this case, the associated table ID should be included. Option C: User-defined Models (through user subroutine) This option allows you to define the cure kinetics model in the UCURE user subroutine. See Marc Volume D: User Subroutines and Special Routines for the description of this subroutine. Note:

This option must be combined with CURING parameter to activate the curing analysis.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CURE RATE.

I

Enter cure kinetics model definition number.

2nd data block 1-5

1st

Enter a negative value if the cure model is defined by the UCURE user subroutine. Enter 0 (default) if no cure kinetics model is defined or if table input is used to define the cure kinetics model. Enter 1 for Lee, Loos and Springer (1982) model;

Main Index

CURE RATE 1129 Cure Kinetics

Format Fixed

Free

Data Entry Entry Enter 2 for Combined model: Lee, Chiu, and Lin (1992); White and Hahn (1992); Kenny (1992); Scott (1991); or Scott (1991) Enter 3 for Lee, Chiu, and Lin (1992) model Enter 4 for Johnston and Hubert (1995) model.

6-10

2nd

I

Enter 0 (default) if the model is not defined by a table, or Enter the table ID number if a table is used to define the cure kinetics model.

11-15

3rd

I

Enter the associated material ID number.

16-20

4th

I

Enter unit number for reading in the data (default is standard input).

Option A (Model 1) 3rd data block 1-10

1st

F

Enter First Pre-Exponential Factor:

11-20

2nd

F

Enter Second Pre-Exponential Factor:

21-30

3rd

F

Enter Third Pre-Exponential Factor:

31-40

4th

F

Enter Activation energy:

Δ E1

41-50

5th

F

Enter Activation energy:

Δ E2 .

51-60

6th

F

Enter Activation energy:

Δ E3

61-70

7th

F

Enter value:

B.

71-80

8th

F

Enter value:

αC .

F

Enter the maximum cure reaction heat.

A1 . A2 .

A3 .

4th data block 1-10

1st

Option A (Model 2) 3rd data block

Main Index

1-10

1st

F

Enter First Pre-Exponential Factor:

11-20

2nd

F

Enter Second Pre-Exponential Factor:

21-30

3rd

F

Enter Activation energy:

Δ E1 .

31-40

4th

F

Enter Activation energy:

Δ E2 .

41-50

5th

F

Enter Exponential Factor:

m.

A1 . A2 .

1130 CURE RATE Cure Kinetics

Format Fixed

Free

Data Entry Entry

51-60

6th

F

Enter Exponential Factor: n .

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Not used; enter 0.

F

Enter the maximum cure reaction heat.

4th data block 1-10

1st

Option A (Model 3) 3rd data block 1-10

1st

F

Enter First Pre-Exponential Factor:

11-20

2nd

F

Enter Second Pre-Exponential Factor:

21-30

3rd

F

Enter Activation energy:

Δ E1 .

31-40

4th

F

Enter Activation energy:

Δ E2 .

41-50

5th

F

Enter Exponential Factor: l .

51-60

6th

F

Enter Exponential Factor:

61-70

7th

F

Enter Exponential Factor: n .

71-80

8th

F

Not used; enter 0.

F

Enter the maximum cure reaction heat.

A1 . A2 .

m.

4th data block 1-10

1st

Option A (Model 4) 3rd data block 1-10

1st

F

Enter Pre-Exponential Factor:

11-20

2nd

F

Enter Activation Energy:

ΔE .

21-30

3rd

F

Enter Exponential Factor:

m.

31-40

4th

F

Enter Exponential Factor: n .

41-50

5th

F

Enter Diffusion Constant:

51-60

6th

F

Enter Critical Resin Degree of Cure:

61-70

7th

F

Enter Increase of Critical Resin Degree of Cure:

71-80

8th

F

Not used; enter 0.

F

Enter the maximum cure reaction heat.

A.

C. α C0 .

4th data block 1-10

Main Index

1st

α CT .

CURE RATE 1131 Cure Kinetics

Format Fixed

Free

Data Entry Entry

Option B 3rd data block 1-10

1st

F

Enter the reference value associated with the table input.

11-20

2nd

F

Enter the maximum cure reaction heat.

Option C The 3rd and 4th data blocks are not needed for Option C.

Main Index

1132 INIT CURE (with TABLE Input) Define Initial Degree of Cure

INIT CURE (with TABLE Input)

Define Initial Degree of Cure

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to enter the initial degree of cure into each elements. The input data is based on the new table driven input data format. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INIT CURE.

2nd data block 1-5

1st

I

Number of sets of initial degree of cure data to be entered (optional)

6-10

2nd

I

Unit number for input of initial degree of cure data. Defaults to input file.

3rd data block 1-10

1st

I

Enter the number of geometry types used to define this initial condition. Default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. The label will be referenced by the LOADCASE option.

F

Enter the magnitude of the initial degree of cure.

I

Enter the table ID associated with the initial degree of cure.

4th data block 1-10

1st

5th data block 1-5

1st

The 6th and 7th data blocks are repeated as many geometry types as specified in the 3rd data block, 1st field.

Main Index

INIT CURE (with TABLE Input) 1133 Define Initial Degree of Cure

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1 - Element IDs 2 - Volume/region/body IDs.

7th data block 1-80

Main Index

1st

I

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

1134 INIT CURE Define Initial Degree of Cure

INIT CURE

Define Initial Degree of Cure

Description This option allows you to enter the initial degree of cure into each elements. The input data is based on the non-table driven input format. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words INIT CURE.

2nd data block 1-5

1st

I

Number of sets of initial degree of cure data to be entered (optional)

6-10

2nd

I

Unit number for input of initial degree of cure data. Defaults to input file.

11-15

3rd

I

Not used; default is set to 0.

The 3rd to 6th data blocks are entered as pairs. 3rd data block 1-10

1st

F

Enter the value of the initial degree of cure.

I

Enter the list of elements for which initial degree of cure prescribed above is applied.

4th data block 1-80

1st

5th data block Only necessary if the CENTROID parameter is not used. 1-80

1st

I

Enter the list of integration points for which the initial degree of cure prescribed above is applied.

6th data block Only necessary for shell or beam analysis. 1-80

Main Index

1st

I

Enter the list of layers for which the initial degree of cure prescribed above is applied.

CURE SHRINKAGE 1135 Shrinkage Property of Resin Material

CURE SHRINKAGE

Shrinkage Property of Resin Material

Description This option is used to define the shrinkage property of resin material and to couple the curing shrinkage effect into thermal/mechanical problems. There are three choices for this option. Each choice corresponds to its own input data format. Option A: Embedded Models: This option is the default method and allows you to choose one of the two cure models built into the Marc program. Default is a no cure kinetics model. Option B: Table Defined Models This option allows you to define the cure kinetics model in the table format. In this case, the associated table ID should be included. Option C: User-defined Models (through user subroutine) This option allows you to define the cure kinetics model in the USHRINKAGE user subroutine. See Marc Volume D: User Subroutines and Special Routines for the description of this subroutine. Note:

This option must be combined with CURING parameter to activate the curing shrinkage analysis.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CURE SHRINKAGE.

I

Enter cure kinetics model definition number. (default is 0).

2nd data block 1-5

1st

Enter a negative value if the cure model is defined by the USHRINKAGE user subroutine. Enter 0 if no cure kinetics model is defined or if table input is used to define the cure kinetics model. Enter 1 for Bogetti and Gillespie (1992) model; Enter 2 for White and Hahn (1992) model.

Main Index

1136 CURE SHRINKAGE Shrinkage Property of Resin Material

Format Fixed 6-10

Free

Data Entry Entry

2nd

I

Enter 0 (default) if the model is not defined by a table, or Enter the table ID number if table is used to define the cure kinetics model.

11-15

3rd

I

Enter the associated material ID number.

16-20

4th

I

Enter unit number for reading in the data (default is standard input).

Option A (Model 1) 3rd data block 1-10

1st

F

11-20

2nd

F

Enter the degree of cure after which the resin shrinkage stops:

α C1 .

21-30

3rd

F

Enter the degree of cure after which the resin shrinkage stops:

α C2 .

31-40

4th

F

Enter the linear cure shrinkage:

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Not used; enter 0.

Enter the total volumetric resin shrinkage:

S∞

Vr

.

A

4th data block 1-10

1st

F

Directional cure shrinkage coefficient:

C SC 11 .

11-20

2nd

F

Directional cure shrinkage coefficient:

C SC 22 .

21-30

3rd

F

Directional cure shrinkage coefficient:

C SC 33 .

31-40

4th

F

Directional cure shrinkage coefficient:

C SC 12 .

41-50

5th

F

Directional cure shrinkage coefficient:

C SC 23 .

51-60

6th

F

Directional cure shrinkage coefficient:

C SC 31 .

Option A (Model 2) 3rd data block

Main Index

1-10

1st

F

11-20

2nd

F

Enter the degree of cure after which the resin shrinkage stops:

21-30

3rd

F

Enter cure shrinkage model superscript:

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Not used; enter 0.

Enter the total volumetric resin shrinkage:

S∞

Vr

B.

. αC .

CURE SHRINKAGE 1137 Shrinkage Property of Resin Material

Format Fixed

Free

Data Entry Entry

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Not used; enter 0.

4th data block 1-10

1st

F

Directional cure shrinkage coefficient:

C SC 11 .

11-20

2nd

F

Directional cure shrinkage coefficient:

C SC 22 .

21-30

3rd

F

Directional cure shrinkage coefficient:

C SC 33 .

31-40

4th

F

Directional cure shrinkage coefficient:

C SC 12 .

41-50

5th

F

Directional cure shrinkage coefficient:

C SC 23 .

51-60

6th

F

Directional cure shrinkage coefficient:

C SC 31 .

F

Enter the reference value associated with the table input.

Option B 3rd data block 1-10

1st

4th data block 1-10

1st

F

Directional cure shrinkage coefficient:

C SC 11 .

11-20

2nd

F

Directional cure shrinkage coefficient:

C SC 22 .

21-30

3rd

F

Directional cure shrinkage coefficient:

C SC 33 .

31-40

4th

F

Directional cure shrinkage coefficient:

C SC 12 .

41-50

5th

F

Directional cure shrinkage coefficient:

C SC 23 .

51-60

6th

F

Directional cure shrinkage coefficient:

C SC 31 .

Option C The 3rd and 4th data blocks are not needed for Option C.

Main Index

1138 THERMO-PORE Define Properties of Thermal Degrading Material

THERMO-PORE

Define Properties of Thermal Degrading Material

Description This option is used to define the material data required for materials subjected to pyrolysis. This format is based upon the different material states, virgin, charred, or coked being previously defined using the ISOTROPIC or ORTHOTROPIC options. The thermal properties of the inert material, the gas, and water, if required, should be defined in the ISOTROPIC option. Notes:

Data that is not required for model A is specified as (NRA), enter 0. Data that is not required for model A or B is specified as (NRAB).

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter word THERMO-PORE.

2nd data block 1-5

1st

I

Enter number of sets of data.

6-10

2nd

I

Enter unit number to read the data from.

The 3rd through 15th data blocks are repeated for each set of material data. 3rd data block 1-5

1st

I

Enter material ID.

6-10

2nd

I

Enter 1 for simple pyrolysis model. Enter 2 for advanced pyrolysis model.

11-15

3rd

I

Set to 3 if BSM database is used.

16-20

4th

I

Enter the material ID for virgin material.

21-25

5th

I

Enter the material ID for charred material.

26-30

6th

I

Enter the material ID for coked material.

31-35

7th

I

Enter the material ID for liquid water.

36-40

8th

I

Enter the material ID for gas.

41-45

9th

I

Enter the material ID for inert material.

46-50

10th

I

Enter the material ID for water vapor.

51-62

11th

A

Enter the material name.

If the BSM database is used, then the 4th through 13th data blocks will be given in the BSM data file.

Main Index

THERMO-PORE 1139 Define Properties of Thermal Degrading Material

Format Fixed

Free

Data Entry Entry

Data block 3b is only used if BSM database is used. 3b data block 1-80

1st

A

Enter path to BSM data section for this option.

I

Enter pyrolysis model (NRA).

4th data block 1-5

1st

0 – No pyrolysis. 1 – Arrhenius law for pyrolysis based upon rho. 2 – Arrhenius law for coking based upon φj. 3 – UPYROLSL user subroutine is used. 6-10

2nd

I

Enter water vapor model (NRA). 0 – No water vapor model included. 1 – Arrhenius law used. 2 – Sullivan and Stokes model. 3 – UWATERSL user subroutine is used.

11-15

3rd

I

Enter coking model (NRA). 0 – No coking model. 1 – Arrhenius coking model based upon Kcg. 2 – Linear model for Kcg. 3 – UCOKSL user subroutine is used.

16-20

4th

I

Enter MATFLG where MATFLG = ICEFF*10+IISO. ICEFF = 0 linear method for calculating effective conductivity. = 1 CMA,PTIMAD weighted average method for calculating effective conductivity. = 2 UPYROLEFF user subroutine used to define effective conductivity. IISO

= 0 if isotropic material is being used. = 1 if orthotropic material is being used. = 2 if anistropic material is being used.

Main Index

21-25

5th

I

Number of terms used in Arrhenius pyrolysis model (NRA).

26-30

6th

I

Number of terms used in Arrhenius water vapor model (NRA). In current model = 1.

1140 THERMO-PORE Define Properties of Thermal Degrading Material

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Number of terms used in Arrhenius coking model (NRA). In current model = 1.

36-40

8th

I

Enter 1 for pressure based upon bulk modulus model. Enter 2 for pressure-temperature based upon Perfect gas law (default).

5th data block 1-10

1st

E

Enter the fraction of pyrolysis when pyrolysis stops and coking begins if present. Default = 0.96.

11-20

2nd

E

Enter the viscosity of the fluid, only required if D’Arcy law

21-30

3rd

E

Enter the volume fraction of the inert material.

31-40

4th

E

Enter the fluid-gas bulk modulus, only required for D’Arcy law.

41-50

5th

E

Enter the molecular weight of the fluid.

6th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Table ID for viscosity, only required if D’Arcy law

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Table ID for fluid-gas bulk modulus.

21-25

5th

I

Table ID for the Molecular weight.

7th data block The 7th data block is only required for the simple model. 1-10

1st

E

Enter reference time associated with the end of the combustion/transformation.

11-20

2nd

E

Enter the pyrolysis temperature.

If the Arrhenius theta model is used for pyrolysis, then for each term - repeat the 8a data block. Do not include for the simple model. 8a data block 1-5

1st

I

Enter term number (j).

6-15

2nd

E

Enter

Bj .

11-25

3rd

E

Enter

E aj .

26-35

4th

E

Enter

ψj .

36-45

5th

E

Enter

Δ ρ s ,p ,c ,j .

If the Arrhenius rho model is used for pyrolysis, then for each term - repeat the 8b data block.

Main Index

THERMO-PORE 1141 Define Properties of Thermal Degrading Material

Format Fixed

Free

Data Entry Entry

8b data block 1-5

1st

I

Enter term number (j).

6-15

2nd

E

Enter

Bj .

16-25

3rd

E

Enter

E aj .

26-35

4th

E

Enter

ψj .

36-45

5th

E

Enter

ρˆ svj .

46-55

6th

E

Enter

ρˆ scj .

56-65

7th

E

Enter

Γj .

If Water vapor model included, use the 9th and 10th data blocks. Do not include for the simple model. 9th data block 1-10

1st

E

Enter initial volumetric mass density of liquid

11-20

2nd

E

Not used; enter 0.

21-30

3rd

E

Boiling point of liquid.

31-40

4th

E

Normalized of

d P sat ⁄ dT

ρ l, o .

(model C only).

10th data block 1-5

1st

I

Enter the table ID for initial volumetric mass density of liquid.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for boiling point of liquid.

16-20

4th

I

Not used; enter 0.

If the Arrhenius water vapor model - 1 terms used for each term include the 11th data block. Do not include for the simple model. 11th data block 1-5

1st

I

Enter term number (j)

6-15

2nd

E

Enter

Bw .

11-25

3rd

E

Enter

E aw .

26-35

4th

E

Enter

ψw .

If the Arrhenius model is used for coking, use the 12th data block. Do not include for the simple model.

Main Index

1142 THERMO-PORE Define Properties of Thermal Degrading Material

Format Fixed

Free

Data Entry Entry

12th data block 1-5

1st

I

Enter term number. Default = 1.

6-15

2nd

E

Enter

Kc .

11-25

3rd

E

Enter

E ac .

26-35

4th

E

Enter

ηc .

36-45

5th

E

Enter K CGE (total mass fraction of the carbon in the pyrolysis gas when chemical equilibrium is achieved).

If the Linear model for

K CG

is used for coking, use the 13th and 14th data blocks.

13th data block 1-10

1st

E

Enter

T

11-20

2nd

E

Enter

K CG

21-30

3rd

E

Enter

TC

31-40

4th

E

Enter

K CGE

low temperature

equilibrium temperature

14th data block 1- 5

1st

I

Enter the table ID associated with

T

6-10

2nd

I

Enter the table ID associated with

K CE

11-15

3rd

I

Enter the table ID associated with

TE .

16-20

4th

I

Enter the table ID associated with

K CGE .

. .

15th data block Enter a list of elements associated with this material.

Main Index

SURFACE ENERGY 1143 Define Surface Energy

SURFACE ENERGY

Define Surface Energy

Description This option allows the user to define the data required for calculating the surface energy balance and to provide the data for the surface recession rate calculation. This option must be used in conjunction with the STREAM DEFINITION option which is used to prescribe the elements/faces associated with a region. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words SURFACE ENERGY.

2nd data block 1-5

1st

I

Enter the number of regions to be defined.

6-10

2nd

I

Enter the unit number to read input data. Defaults to standard input.

The 3rd through 18th data blocks are repeated for each surface region. 3rd data block 1-5

1st

I

Enter the numbers of geometry types used to define the surface energy. Default is 1; see the 17th and 18th data blocks.

6-10

2nd

I

Enter the surface energy ID.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Enter 3 if surface data is to be obtained from BSM database. In this case, card series 4 through 16 will be given in the BSM file.

21-25

5th

I

Enter 1 for simplified heat of ablation model.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with the surface energy. This label will be referenced by the LOADCASE option.

Data block 3b is only used if BSM database is used. 3b data block 1-80

1st

A

Enter path to BSM data section for this option.

If the BSM database is used, then the 4th through 16th data blocks will be given in the BSM file. 4th data block

Main Index

1-5

1st

I

Enter 1 to include diffusion.

6-10

2nd

I

Enter the number of families of particles.

11-15

3rd

I

Enter the number of liquid phases.

1144 SURFACE ENERGY Define Surface Energy

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter 0 if αH = αHo. Enter 1 if αH given by standard calculation. Enter 2 if the UFAH user subroutine is called.

21-25

5th

I

Enter 0 for constant G law (correlation factor). Enter 1 if particles given in card series 12 and 13. Enter 2 if particles defined by the UGLAW user subroutine.

26-30

6th

I

Enter 0 if empirical constant entered. Enter 1 if linear formula used. Enter 2 if arc tan formula. Enter 3 if user subroutine ach06_03.fm: is called.

31-35

7th

I

Enter 1 if the UTIMP user subroutine and/or the UFLUXMEC user subroutine are to be used. Enter 2 if recession rate due to simplified erosion model.

36-40

8th

I

Enter 0 for mixture rule for Hsolid based on Hvirgin, Hcharred. Enter 1 for Hsolid=Hcharred if pyrolysis Hsolid=Hcoked.

41-45

9th

I

Enter table ID that will control diffusion contribution to surface energy. Default is 0; diffusion contribution is always active.

5th data block 1-10

1st

E

Not used; enter 0.

11-20

2nd

E

Not used; enter 0.

21-30

3rd

E

Not used; enter 0.

31-40

4th

E

Not used; enter 0.

41-50

5th

E

Enter the convection coefficient

51-60

6th

E

Enter the diffusion coefficient αM.

61-70

7th

E

Enter the transpiration factor κ.

αH

O

.

6th data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter the table ID for the convection coefficient

αH

O

.

SURFACE ENERGY 1145 Define Surface Energy

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Enter the table ID for the coefficient αM.

31-35

7th

I

Not used; enter 0.

7th data block 1-10

1st

E

Enter the enthalpy of recovery Hrec.

11-20

2nd

E

Enter the enthalpy of the frozen composition He.

21-30

3rd

E

Enter the enthalpy of the wall gas Hw.

31-40

4th

E

Enter the enthalpy of ablation

Δ H a bl

for simple model.

8th data block 1- 5

1st

I

Enter the table ID for the enthalpy of recovery.

6-10

2nd

I

Enter the table ID for the enthalpy of frozen composition.

11-20

3rd

I

Enter the table ID for the enthalpy of the wall gas.

21-25

4th

I

Enter the table ID for the enthalpy of ablation.

E

Enter mass rate of the solid due to ablation by gasses, normalized by B' c = m· s, th, g ⁄ α .

9th data block 1-10

1st

αm

m

11-20

2nd

E

Enter mass rate of the solid due to ablation by particles. If number of families of particles are given, this entry is not used m· s,th,p .

21-30

3rd

E

Enter mass rate of the solid due to ablation by erosion.

31-40

4th

E

Enter amount of ablation due liquid particles Φsolid ablated by liquid.

41-50

5th

E

Enter amount of ablation due to gases Φsolid ablated by gases.

51-60

6th

E

Enter the amount of ablation due to particle impact Φparticles impact.

61-70

7th

E

Enter the amount of pyrolysis at which recession may occur. If zero, recession may occur at all densities.

71-80

8th

E

Surface recession rate due to simplified erosion model.

10th data block

Main Index

1- 5

1st

I

Enter the table ID for

6-10

2nd

I

Enter the table ID for the mass rate of the solid due to ablation by particles.

11-15

3rd

I

Enter the table ID for the mass rate of the solid due to ablation by erosion.

16-20

4th

I

Enter the table ID for the amount of ablation due to liquid particles.

21-25

5th

I

Enter the table ID for the amount of ablation due to gases.

26-30

6th

I

Enter the table ID for the amount of ablation due to particle impact.

B' c .

1146 SURFACE ENERGY Define Surface Energy

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter the table ID for the surface recession rate due to simplified erosion model.

Enter only if diffusion is included in model (not for simple model). 11th data block 1-10

1st

E

Enter H.

11-20

2nd

E

Enter Ze.

21-30

3rd

E

Enter Zs.

31-35

4th

I

Enter the table ID associated with H.

36-40

5th

I

Enter the table ID associated with Ze.

41-45

6th

I

Enter the table ID associated with Zs.

Repeat card series 12th and 13th data blocks as pairs for each family of particles 12th data block 1-10

1st

E

Enter Vx of particle.

11-20

2nd

E

Enter Vy of particle.

21-30

3rd

E

Enter Vz of particle.

31-40

4th

E

Enter diameter of particle.

41-50

5th

E

Enter angle of incidence of particle.

51-60

6th

E

Enter

61-70

7th

E

Enter the correlation factor (G law) if it is constant.

71-80

8th

E

Enter the enthalpy of reaction ΔHr,p.

m·

of particle.

13th data block 1-5

1st

I

Enter the table ID associated with Vx.

6-10

2nd

I

Enter the table ID associated with Vy.

11-15

3rd

I

Enter the table ID associated with Vz.

16-20

4th

I

Enter the table ID associated with the particle diameter.

21-25

5th

I

Enter the table ID associated with angle of incidence of particle.

26-30

6th

I

Enter the table ID associated with

31-35

7th

I

Enter the table ID associated with the correlation factor.

36-40

8th

I

Enter the table ID associated with the enthalpy of reaction.

Include the 14th data block only if particles are included.

Main Index

m·

of particle.

SURFACE ENERGY 1147 Define Surface Energy

Format Fixed

Free

Data Entry Entry

14th data block 1-10

1st

E

Enter the value of the empirical factor fthp.

11-20

2nd

E

Enter the value of temp1, used to define empirical factor.

21-30

3rd

E

Enter the value of temp2 used to define empirical factor.

31-40

4th

E

Enter the value of nfthp.

41-50

5th

E

Enter the value of fmec.

Repeat the 15th and 16th data block for each family of liquid phases. 15th data block 1-10

1st

I

Enter

m· l p .

11-20

2nd

I

Enter

Hl p .

16th data block 1-5

1st

I

Enter the table ID associated with

m· l p .

6-10

2nd

I

Enter the table ID associated with

Hl p .

17th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B, Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 01: Normal flux (bottom surface for shells) 10: Normal flux (top surface for shells)

11-15

3rd

I

Enter the face ID or edge ID.

18th data block The 18th and 19th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 1-5

1st

I

Enter the geometry type: 04: Surface IDs 05: Curve IDs 09: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs

Main Index

1148 SURFACE ENERGY Define Surface Energy

Format Fixed

Free

Data Entry Entry 13: Element-Edges IDs - Mentat convention 14: Element-Faces IDs - Mentat convention

19th data block 1-80

Main Index

Enter a list of geometric entities to which the above surface energy terms are applied. The geometric entities must all be of the type prescribed in the 17th data block.

RECEDING SURFACE 1149 Define Areas where Surface Recedes Due to Thermo-chemical Erosion or Wear Behavior

RECEDING SURFACE

Define Areas where Surface Recedes Due to Thermo-chemical Erosion or Wear Behavior

Description This option allows the user to define where the surface is to recede due to either thermal, chemical, or erosive processes. The process may be defined here, or via the UABLATE or UWEAR user subroutine, or via an advanced model. This data for the advanced thermal model is given in the SURFACE ENERGY option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words RECEDING SURFACE.

2nd data block 1-5

1st

I

Enter the number of sets of data (optional).

6-10

2nd

I

Enter unit number to read data default is standard input.

3rd data block 1-5

1st

I

Enter the number of geometries used to describe this receding surface.

6-10

2nd

I

Enter the recession model: 0 no recession 1 simple thermal ablation model 2 advanced thermal ablation model 3 user subroutine UABLATE 4 wear model based upon nodal force 5 wear model based upon nodal stress 6 wear model based upon nodal force and coefficient of friction 7 wear model based upon nodal stress and coefficient of friction 8 wear model based upon user-defined wear rate 9 wear model based upon user subroutine UWEAR

Main Index

11-15

3rd

I

Enter the table ID for ression model 1 or 8.

16-20

4th

I

Enter the surface ID for the advanced model 2.

1150 RECEDING SURFACE Define Areas where Surface Recedes Due to Thermo-chemical Erosion or Wear Behavior

Format Fixed

Free

Data Entry Entry

For the wear models enter the sum of k1 +k2+k3 +k4 K1 = 0 calculate and apply wear K1 = 10 calculate wear, but do not update coordinates K2 = 0 use values at nodes K2 = 100 use an averaged value of stress or force over the surface K3 = 0 do not include thermal mechanism K3 = 1000 include thermal mechanism K4 = 0 – “Archard” based models K4 = 10000 – “Bayer” based models 21-30

5th

E

For simple model, enter the reference rate of recession. For wear models 4 through 7, enter the wear coefficient. For wear model 8, enter the user-defined wear rate.

31-35

6th

I

Recession Surface ID.

36-40

7th

I

Not used; enter 0.

41-72

8th

A

Enter the name.

4th data block Only required if k4 = 10000 on 3rd data block, 4th field 1-10

1st

E

Enter exponent applied to force or stress term.

11-20

2nd

E

Enter exponent applied to relative velocity term.

I

Enter the geometry type.

5th data block 1-5

1st

1: Element IDs 4: Surface IDs 5: Curve IDs 11: Element-Edge IDs 12: Element-Face IDs 13: Element-Edge IDs - Mentat convention 14: Element-Face IDS - Mentat convention 16: Surface ID: orientation Id 17: Curve ID: orientation id

Main Index

RECEDING SURFACE 1151 Define Areas where Surface Recedes Due to Thermo-chemical Erosion or Wear Behavior

Format Fixed

Free

Data Entry Entry 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

6-10

2nd

I

If geometry type 1, enter the face ID.

6th data block 1-80

Main Index

Enter a list of geometric entities to define the location of the recession. The geometric entities must all be of the type prescribed in the 4th data block.

1152 THROAT Define Coordinates of Throat

THROAT

Define Coordinates of Throat

Description This option is used to provide the reference dimensions of the throat radius and axial position when used with quantities that are dependent upon the radius/throat radius, or quantities that use dual tables based upon the axial coordinate versus the throat axial position. See TABLE option. For independent variable number 33, the ratio used is: 2-D planar ratio = y ( current ) ⁄ radius of the throat 2-D axisymmetric ratio = ( r ( current ) ⁄ radius of the throat ) 2

2

3-D solid ratio = ( y + z ) ⁄ radius of the throat

2

2

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word THROAT.

2nd data block 1-10

1st

E

Enter the axial position of the throat.

11-20

2nd

E

Enter the radius of the throat.

21-25

3rd

I

Enter the recession surface ID used to update the throat radius and axial coordinate. If zero, the reference values are used for the complete calculation.

26-30

4th

I

Number of divisions around circumference for 3-D analysis (default is 36).

31-35

5th

I

Enter 1 for default method to update node at throat point. Enter 2 to update node at throat point based upon upstream points

36-40

Main Index

6th

I

Enter point ID of throat location.

INITIAL PYROLYSIS 1153 Define Initial Pyrolysis

INITIAL PYROLYSIS

Define Initial Pyrolysis

Description This option is used to define the initial material data in an ablating region. For streamline flow model, this is along streamlines; for D’Arcy flow model, it is at conventional integration points. This option is not necessary for model A. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL PYROLYSIS.

2nd data block 1-5

1st

I

Enter the number of sets of data to follow.

6-10

2nd

I

Enter the unit number. Defaults to input file.

The 3rd through 9th data blocks are repeated as a set NSET times. 3rd data block The 3rd data block is only required for D’Arcy flow model. 1-10

1st

E

Enter the initial solid density.

11-20

2nd

E

Enter the initial gas density due to pyrolysis.

21-30

3rd

E

Enter the initial vapor density.

4th data block 1-10

1st

E

Enter the initial value of xsi,p.

11-20

2nd

E

Not used; enter 0.

21-30

3rd

E

Enter the initial value of xsi,c (only required if coking model is included).

31-40

4th

E

If one term Arrhenius water vapor model is used, enter the initial value of φw.

The 5th data block is only used if Arrhenius Pyrolysis model is used. 5th data block 1-10

1st

E

Enter the first term of the initial value of phij.

11-20

2nd

E

Enter the second term of the initial value of phij; continue as necessary for all terms, enter eight terms per line.

The 6th data block is only used if Arrhenius Coking model is used.

Main Index

1154 INITIAL PYROLYSIS Define Initial Pyrolysis

Format Fixed

Free

Data Entry Entry

6th data block 1-10

1st

E

Enter the initial value of Kcg.

The 7th data block is used for flowline model. 7th data block 1-80

Enter a list of regions that has these initial conditions.

The 8th and 9th data blocks is used for D’Arcy flow model. 8th data block 1-80

Enter a list of elements that has these initial conditions.

9th data block 1-80

Main Index

Enter a list of integration points that has these initial conditions.

INITIAL DENSITY (Heat Transfer) 1155 Define Initial Density

INITIAL DENSITY (Heat Transfer)

Define Initial Density

Description This option provides initial density for pyrolysis analyses, using the streamline flow method. For the D’Arcy flow method, use the INITIAL PYROLYSIS option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INITIAL DENSITY.

2nd data block 1-5

1st

I

Enter the number of sets of prescribed temperatures (optional).

6-10

2nd

I

Enter file number for input of prescribed temperatures data; defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine is required. Enter 1 if the USINC user subroutine is used.

11-15

3rd

I

Flag to indicate that initial conditions are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then. this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Enter step number to be read. If -1 is entered, the last step of the post file is used.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

If data is read from post file, the 4th through 7th blocks may be skipped. 4th data block 1-10

Main Index

1st

F

Enter the magnitude of the initial density.

1156 INITIAL DENSITY (Heat Transfer) Define Initial Density

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Enter the table ID associated with the geometric variations in initial density.

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 2 – Node IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial density are applied. the geometric entities must all be of the type prescribed in the 6th data block.

STREAM DEFINITION 1157 Define Stream Definition

STREAM DEFINITION

Define Stream Definition

Description This option allows the user to define the streamline and the reference point for the arc length. The streamlines are used for model B of the thermo-poro analysis. The arc length is only required if the material data and/or boundary conditions are functions of the arc length. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words STREAM DEFINITION.

2nd data block 1-5

1st

I

Enter the number of sets of data.

6-10

2nd

I

Enter the unit number to read in the data.

11-15

3rd

I

Flag to control display of streamlines.

16-25

4th

E

Enter the tolerance distance to match streamlines across regions. Only used if the 10th field of 3rd data block is not zero.

Repeat the 3rd, 4th, and 5th data blocks for each pyrolysis region. 3rd data block 1-5

1st

I

Enter the region ID.

6-10

2nd

I

Enter the contact body ID associated with this streamline region if ablation occurs, and remeshing is required, default is the region ID.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Maximum number of elements through the region.

21-25

5th

I

Enter a 1 if stream definition region is used to define topology for stretch meshers but no pyrolysis occurs in this region, or ABLATION,3 or ABLATION, 4 is used, but no pyrolysis occurs.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Enter the number of streamlines. Only required if an irregular mesh is provided, or if the region is defined using curves.

36-40

8th

I

Enter the maximum number of edges/faces in a region. Only necessary if region will be remeshed of if the region is defined by using curves or surfaces.

41-45

9th

I

Enter 1 if regular region. Enter 2 if irregular region.

Main Index

1158 STREAM DEFINITION Define Stream Definition

Format Fixed

Free

Data Entry Entry Enter 3 if higher-order regular region. Enter 4 if higher-order irregular region.

46-50

10th

I

Enter the previous region id, used to obtain m· at beginning of streamline.Note this ID must be smaller than the current region ID. If a zero is entered

m·

= 0.0 along inside surface.

51-55

11th

I

Enter the curve/surface ID associated with the free surface. If a curve/surface is given, skip the 4th and 5th data blocks.

56-60

12th

I

Enter the curve/surface ID associated with the interior surface. If a curve/surface is given, skip the 6th and 7th data blocks.

61-70

13th

E

Enter used.

71-80

14th

E

Enter m· g, w at beginning of streamline if water model is included, and it is unequal to 0, and 10th field is not used.

m· g, p

at beginning of streamline if unequal to 0 and 10th field is not

4th data block Enter a list of element:edge or element:face pairs for the free surface. 5th data block Enter a list of element:edge or element:face pairs for the interior surface.

Main Index

PRINT STREAMLINE 1159 Control Output of Results along a Streamline

PRINT STREAMLINE

Control Output of Results along a Streamline

Description This option allows the user to control the amount of results that will be placed in the output if the pyrolysis model B is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PRINT STREAM.

2nd data block 1-5

1st

I

Enter the unit number for output; default to .stm file (91).

6-10

2nd

I

Enter frequency to write results into file. -1: don’t write results 0: (default) write results every increment

11-15

3rd

I

0: write values at all SIP 1: write values at extreme SIP points only

Main Index

1160 TRACK STREAMLINE Track Behavior of a Point along a Streamline

TRACK STREAMLINE

Track Behavior of a Point along a Streamline

Description This option allows you to create a file that may be viewed by Mentat, thus gives the results at points along a streamline. This option is often useful when ablation occurs as the conventional streampoints have new locations. The results are written to a file jidname.sltrk. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words TRACK STREAM.

2nd data block 1-5

1st

I

Enter the number for points to be tracked.

6-10

2nd

I

Unit number to read data; default is standard input.

11-15

3rd

I

Enter 1 if stream points are to be entered using 3rd data block. Enter 2 if a list of elements are to be entered using 4th data block.

3rd data block (only used if 2nd data block, 3rd field is a 1) 1-5

1st

I

Enter the region number.

6-10

2nd

I

Enter the streamline number.

11-15

3rd

I

Enter the streamline point.

4th data block (only used if 2nd data block, 3rd field is a 2) Enter a list of elements.

Main Index

Chapter 3: Model Definition Options 1161 Joule Heating Analysis

Chapt Joule Heating Analysis er 3: This section describes the input of additional data required for coupled Joule heating analysis and structural-thermal-electrical analysis. All of the options in the previous subsection referring to Mode coupled heat transfer are also applicable. You have the ability to apply surface, volumetric and nodal currents, and prescribe nodal voltages. All applied boundary conditions should be entered as total values. In addition, l you can input a conversion factor so that you can work in convenient units for both the heat transfer and Defini electrical conduction problems. tion Joule heating analysis is not available for shell elements. Optio ns

Main Index

1162 JOULE Define Conversion Factor for Joule Heating Analysis

JOULE

Define Conversion Factor for Joule Heating Analysis

Description In the analysis of Joule heating, the unit of heat generation computed from the electrical problem is, in general, not consistent with the unit required for the heat transfer analysis. Depending on the units used for the problems, different conversion factors must be used. For example, in an electric problem, the heat generation can be expressed in terms of current and resistance as q = I2R. If the units of current and resistance are (amp) and (ohm/ft), respectively, then the unit of heat generation in the electric problem must be (watt/ft). Since 1 (watt) is equal to 3.4129 (btu/hr), a factor of 3.4129 must be used in a Joule heating problem for the purpose of converting the unit of heat generation from (watt/ft) to (btu/hr-ft) for heat transfer analysis. It is also possible to use the CONVERT model definition option as explained in the Heat Transfer Analysis section to prescribe this factor. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word JOULE.

F

Heat generation unit conversion factor between electrical and heat transfer analyses in a Joule heating problem.

2nd data block 1-10

1st

Default is 1.0.

Main Index

DIST CURRENT (with TABLE Input - Joule Heating) 1163 Define Distributed Currents

DIST CURRENT (with TABLE Input - Joule Heating)

Define Distributed Currents

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent currents. The applied current is associated with a boundary condition name that is activated with the LOADCASE history definition. In the current releases, Joule heating is not available for shell elements. Note:

If a distributed current is applied on the bottom of a shell, the current is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd through 7th data blocks are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

1164 DIST CURRENT (with TABLE Input - Joule Heating) Define Distributed Currents

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of this type of distributed currents.

I

Enter the table ID associated with the distributed current.

4th data block 1-10

1st

5th data block 1-5

1st

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in

6-10

2nd

I

Enter the distributed load type based upon:

Marc Volume B: Element Library.

1: Normal current (bottom surface for shells) 10: Normal current (top surface for shells) 11-15

3rd

I

Enter the face ID or edge id.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID

Main Index

DIST CURRENT (with TABLE Input - Joule Heating) 1165 Define Distributed Currents

Format Fixed

Free

Data Entry Entry 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

1166 DIST CURRENT (Joule Heating - Model Definition) Define Distributed Current

DIST CURRENT (Joule Heating - Model Definition) Define Distributed Current The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) current to be specified. Distributed current is converted to a consistent nodal current by Marc. Note that for a given element type, there is an established convention for the application of surface current of a particular face. The FLUX user subroutine can be used to input time and spatial dependent current. The applied current is associated with a boundary condition name that is activated with the LOADCASE history definition. In the current releases, Joule heating is not available for shell elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd and 4th data blocks are entered in pairs, once for each data block. 3rd data block 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed current.

4th data block Enter a list of elements associated with the above distributed current.

Main Index

POINT CURRENT (with TABLE Input - Joule Heating) 1167 Define Point Currents

POINT CURRENT (with TABLE Input - Joule Heating) Define Point Currents The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows total nodal point currents to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent currents. The applied current is associated with a boundary condition name that is activated with the LOADCASE history definition. In the current releases, Joule heating is not available for shell elements; so, point currents should only be applied to the first degree of freedom. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of point currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of point current data; defaults to input.

Data blocks 3 through 7 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter a 1 if first point current is to be applied to all degrees of freedom of a heat transfer shell.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1168 POINT CURRENT (with TABLE Input - Joule Heating) Define Point Currents

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Magnitude of point current.

11-20

2nd

F

Magnitude of point current for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point current for third degree of freedom, (heat transfer shell elements only).

5th data block 1-5

1st

I

Table ID for point current.

6-10

2nd

I

Table ID for point current for second degree of freedom (Heat transfer shell elements only).

11-15

3rd

I

Table ID for point current for third degree of freedom (Heat transfer shell elements only).

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

POINT CURRENT (Joule - Model Definition) 1169 Define Nodal Point Current

POINT CURRENT (Joule - Model Definition)

Define Nodal Point Current

The information provided here is based upon not using the table driven input style. Description This option allows total nodal point current to be specified. The FORCDT user subroutine can be used for the time dependent current. Format Format Fixed

Free

Data Entry Entry

1st data block A

Enter the words POINT CURRENT.

1-5

I

Enter the number of sets of point currents to be entered (optional).

6-10

I

Enter unit number of input of point current data, defaults to input.

F

Magnitude of point current.

1-10 2nd data block

3rd data block 1-10 4th data block Enter a list of nodes to which the above nodal current are applied.

Main Index

1170 FIXED VOLTAGE (with TABLE Input - Joule Heating) Define Fixed Voltage

FIXED VOLTAGE (with TABLE Input - Joule Heating)

Define Fixed Voltage

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines the fixed voltage that each node must take. The boundary conditions are specified either by giving the voltage and either a list of nodal numbers, or a list of surfaces. Note that unless heat transfer shell elements are used, there is only one degree of freedom in a heat transfer analysis. You must specify it. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. The fixed voltage is associated with a boundary condition name that is activated with the LOADCASE history definition. In the current releases, Joule heating is not available for shell elements; so, the degree of freedom should always be set to one. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED VOLTAGE.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3a data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

FIXED VOLTAGE (with TABLE Input - Joule Heating) 1171 Define Fixed Voltage

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Enter a 1 if first prescribed voltage entered is to be applied for all degrees of freedom of a heat transfer shell.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed voltage for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed voltage for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed voltage for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed temperatures are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11 Element-Edges IDs

Main Index

1172 FIXED VOLTAGE (with TABLE Input - Joule Heating) Define Fixed Voltage

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED VOLTAGE 1173 Define Nodal Fixed Voltage

FIXED VOLTAGE

Define Nodal Fixed Voltage

The information provided here is based upon not using the table driven input style. Description This option defines the fixed voltage that each associated nodal point must take during the first and subsequent increments. Note that a number equal to or exceeding the total number of degrees of freedom constrained must appear on the SIZING parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

A

Enter the words FIXED VOLTAGE.

1-5

I

Number of sets of voltage boundary condition data lines to be read (optional).

6-10

I

Enter unit number for input of voltages;

2nd data block

defaults to input. 3rd data block 1-10

F

Enter the prescribed voltage.

4th data block Enter a list of nodes for which the voltage is prescribed.

Main Index

1174 Chapter 3: Model Definition Options Diffusion Analysis

Chapt Diffusion Analysis er 3: This section defines the options required to perform a diffusion simulation. The solution obtains the (concentration) based upon input of a mass flux across the surfaces or an internally generated Mode pressure mass defined through the DIST MASS or POINT MASS options. Either a steady state or transient analysis may be performed based upon the STEADY STATE, TRANSIENT, or AUTO STEP history definition l options. For a transient analysis, the INITIAL PRESSURE should be used as well. The matrix (solid) Defini material is defined by specifying the permeability on the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC option and the porosity in the INITIAL POROSITY option. In a simple diffusion analysis tion as opposed to a coupled soil simulation performed with the PORE option, the porosity is a state variable Optio and does not change. It is possible to define a new porosity using the CHANGE PORE option. The fluid/gas is defined by giving the viscosity, density, and the bulk modulus. ns

Main Index

INITIAL PRESSURE (with TABLE Input - Diffusion) 1175 Define Initial Pressure

INITIAL PRESSURE (with TABLE Input - Diffusion)

Define Initial Pressure

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines initial pressure for mass diffusion problems. This option provides the magnitude and location, and associates it with an initial condition name. The initial condition is activated with the LOADCASE model definition option. The USINC user subroutine or the TABLE model definition option can be used to enter spatially varying initial conditions. Unless shell elements are used, there is only one degree of freedom in a diffusion analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INIT PRESS.

2nd data block 1-5

1st

I

Enter the number of sets of initial pressure (optional).

6-10

2nd

I

Enter unit number for input of initial pressure data, defaults to input.

Data blocks 3 through 6 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the USINC user subroutine is required for this initial condition.

11-15

3rd

I

Enter 1 if a formatted post file is used.

16-20

4th

I

Only nonzero if the second field is set to 2. Then this entry defines the unit number from which the post file information is read. Defaults to unit 24 for a formatted post file and to unit 25 for a binary post file.

21-25

5th

I

Enter the increment number to be read for initial conditions.

26-30

6th

I

Enter 1 if a formatted post file is used.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

The 4th, 5th, 6th, and 7th data blocks are not used if initial pressure are read from a post file.

Main Index

1176 INITIAL PRESSURE (with TABLE Input - Diffusion) Define Initial Pressure

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Initial pressure in first degree of freedom.

11-20

2nd

F

Initial pressure in second degree of freedom.

21-30

3rd

F

Initial pressure in third degree of freedom. Note:

See Marc Volume B: Element Library for the definition of nodal degrees of freedom.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

FIXED PRESSURE (with TABLE Input - Diffusion) 1177 Define Fixed Pressure

FIXED PRESSURE (with TABLE Input - Diffusion)

Define Fixed Pressure

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This data defines a potential fixed pressure boundary condition. The boundary conditions are specified either by giving the pressure, a list of degrees of freedom, and either a list of nodal numbers or a list of geometric entities. This boundary condition is activated or deactivated using the LOADCASE history definition option. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Unless shell elements are used, there is only one pressure degree of freedom per node in a diffusion analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED PRESS.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

Unit number to read data default is the standard input file.

3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1178 FIXED PRESSURE (with TABLE Input - Diffusion) Define Fixed Pressure

Format Fixed

Free

Data Entry Entry

Data blocks 3 through 8 are repeated for each set. 4th data block - Magnitudes 1-10

1st

E

Prescribed pressure for first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed pressure for second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed pressure for third degree of freedom listed in data block 8.

5th data block - Table IDs 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

DIST MASS (with TABLE Input - Diffusion) 1179 Define Distributed Mass Flux

DIST MASS (with TABLE Input - Diffusion)

Define Distributed Mass Flux

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This block of data defines mass flux (surface and volumetric) type boundary conditions. The user defines a surface distribute mass flux magnitude ( M ⁄ l 2 t ) and the location, and associates this with a boundary condition name. This is activated or deactivated using the LOADCASE history definition option. The FLUX user subroutine can be used for nonuniform, time-dependent distributed mass fluxes or the TABLE model definition option may be used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST MASS.

2nd data block 1-5

1st

I

Enter the number of sets of distributed mass fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed mass fluxes data, defaults to input.

Data blocks 3 through 9 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

1180 DIST MASS (with TABLE Input - Diffusion) Define Distributed Mass Flux

Format Fixed

Free

Data Entry Entry

If a real distributed load is to be defined, data blocks 3 and 4 are used. 4th data block 1-10

1st

F

Enter the magnitude of mass flux.

I

Enter the table ID associated with the mass flux.

5th data block 1-5

1st

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B, Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

Normal

106: Uniform volumetric 107: Nonuniform volumetric 11-15

3rd

I

Enter the face ID.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID

Main Index

DIST MASS (with TABLE Input - Diffusion) 1181 Define Distributed Mass Flux

Format Fixed

Free

Data Entry Entry 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

1182 POINT MASS (with TABLE Input - Diffusion) Define Nodal Mass Flux

POINT MASS (with TABLE Input - Diffusion)

Define Nodal Mass Flux

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This block of data defines nodal mass flux boundary condition. The user specifies a magnitude and location, and associates this with a boundary condition name. This is activated or deactivated using the LOADCASE history definition option. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time or frequency dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT MASS.

2nd data block 1-5

1st

I

Enter number of sets of point mass fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point mass flux data, defaults to input.

Data blocks 3 through 7 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 8th and 9th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

POINT MASS (with TABLE Input - Diffusion) 1183 Define Nodal Mass Flux

Format Fixed

Free

Data Entry Entry

4th data block Magnitude. 1-10

1st

F

Point mass flux associated with first degree of freedom.

11-20

2nd

F

Point mass flux associated with second degree of freedom.

21-30

3rd

F

Point mass flux associated with third degree of freedom.

5th data block - Table ID for Magnitude 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

Data blocks 6 and 7 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1:

Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs

11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 7th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

1184 ISOTROPIC (with TABLE Input - Diffusion) Define Diffusion Properties for Isotropic Materials

ISOTROPIC (with TABLE Input - Define Diffusion Properties for Isotropic Materials Diffusion) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define diffusion properties for an isotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature or pressure, use the TABLE model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 are repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the UPERM and ORIENT user subroutines.

11-15

3rd

I

Enter 1 to use Bulk Modulus. Enter 2 to use perfect gas law.

16-20

4th

I

Data input mode; enter zero.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

The data entered in data blocks 4 and 5 are the reference values that are used with tables or are constants. 4th data block

Main Index

1-10

1st

F

Absolute permeability.

11-20

2nd

F

Fluid dynamic viscosity.

ISOTROPIC (with TABLE Input - Diffusion) 1185 Define Diffusion Properties for Isotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Fluid density.

31-40

4th

F

Fluid bulk modulus.

41-50

5th

F

Porosity if the material is used as a component in the THERMO-PORE option.

5th data block 1-5

1st

I

Table ID for permeability.

6-10

2nd

I

Table ID for viscosity.

11-15

3rd

I

Table ID for fluid density.

16-20

4th

I

Table ID for fluid bulk modulus.

21-25

5th

I

Table ID for porosity.

6th data block Enter a list of elements associated with this material. Note:

Main Index

Do not enter composite elements which use this material in its layers.

1186 ORTHOTROPIC (with TABLE Input - Diffusion) Define Diffusion Properties for Orthotropic Materials

ORTHOTROPIC (with TABLE Define Diffusion Properties for Orthotropic Materials Input - Diffusion) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define diffusion properties for an orthotropic material. You can also associate these material properties with a list of element numbers. To define the dependence of these properties on temperature or pressure, use the TABLE model definition option. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the permeability matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPI.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 7 are repeated for each data set. 3rd data block

Main Index

1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the UPERM and ORIENT user subroutines.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

ORTHOTROPIC (with TABLE Input - Diffusion) 1187 Define Diffusion Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

K11 Absolute permeability.

11-20

2nd

F

K22 Absolute permeability.

21-30

3rd

F

K33 Absolute permeability.

31-40

4th

F

μ

41-50

5th

F

Flui d den sity.

51-60

6th

F

Fluid bulk modulus.

61-70

7th

F

Fluid dynamic viscosity.

Porosity if the material is used as a component in the THERMO-PORE option.

5th data block 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for dynamic viscosity.

21-25

5th

I

Table ID for fluid density.

26-30

6th

I

Table ID for fluid bulk modulus.

27-35

7th

I

Table ID for porosity.

7th data block Enter a list of elements associated with this material. (Do not enter composite elements that use this material in their layers.)

Main Index

1188 ANISOTROPIC (with TABLE Input - Diffusion) Model Definition Option for Diffusion Analysis

ANISOTROPIC (with TABLE Input Model Definition Option for Diffusion Analysis - Diffusion) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option specifies diffusion properties defined by a call to the UPERM and ORIENT user subroutines. The UPERM user subroutine must be used for the input of constant, temperature, or pressure dependent anisotropic permeability (K11, K22, K33) defined in the user coordinate (1,2,3) system. The TABLE model definition option can be used for the input of variations of viscosity with temperatures or pressure. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ANISOTROPI.

2nd data block 1-5

1st

I

Enter the number of anisotropic data sets to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3rd through 8th are repeated as a set NSET times. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-referencing the UPERM and ORIENT user subroutines.

6-10

2nd

I

Enter 1 if the UPERM user subroutine is to be called. Enter 2 if the anisotropic permeability is to be entered in the 6th and 7th data blocks.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

4th data block

Main Index

1-10

1st

F

Fluid Dynamic Viscosity.

11-20

2nd

F

Fluid density.

21-30

3rd

F

Fluid bulk modulus.

ANISOTROPIC (with TABLE Input - Diffusion) 1189 Model Definition Option for Diffusion Analysis

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Table ID for fluid dynamic viscosity.

6-10

2nd

I

Table ID for fluid density.

11-15

3rd

I

Table ID for fluid bulk modulus.

Data block 6 required only if the second fields 6-10 of 3rd data block is a 2. 6th data block - anisotropic absolute permeability 1-10

1st

F

K11

11-20

2nd

F

K12

21-30

3rd

F

K13

31-40

4th

F

K22

41-50

5th

F

K23

51-60

6th

F

K33

7th data block - required only if the second field 6-10 of 3rd data block is a 2 1-5

1st

I

Enter the table ID for K11

6-10

2nd

I

Enter the table ID for K12

11-15

3rd

I

Enter the table ID for K13

16-20

4th

I

Enter the table ID for K22

21-25

5th

I

Enter the table ID for K23

26-30

6th

I

Enter the table ID for K33

8th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

1190 ANISOTROPIC (with TABLE Input - Diffusion) Model Definition Option for Diffusion Analysis

Main Index

Chapter 3: Model Definition Options 1191 Hydrodynamic Bearing Analysis

Chapt Hydrodynamic Bearing Analysis er 3: This section describes the input of data necessary for a hydrodynamic bearing analysis. You have the to define the lubricant film thickness and initial velocity in a variety of ways. In addition, Mode ability restrictors and pump pressures can be imposed on the film pressure. The FIXED PRESSURE or RESTRICTOR model definition option should be used to insure no rigid body modes exist. Lubricant l mass flux may be defined using the POINT MASS or DIST MASS options. FIXED PRESSURE, POINT Defini MASS, and DIST MASS are documented in the Diffusion Analysis section. tion Optio ns

Main Index

1192 VELOCITY (with TABLE Input - Hydrodynamic) Define Nodal Velocity Components

VELOCITY (with TABLE Input Hydrodynamic)

Define Nodal Velocity Components

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows the specification of the nodal velocity components in a bearing analysis, where the convective terms are to be included. The nodal velocity components are defined for sets of nodes. Moreover, the velocity values can be specified via the UVELOC user subroutine (see Marc Volume D: User Subroutines and Special Routines). Note that the velocity in a stationary bearing analysis is specified with respect to the (moving) lubricant. This means that, in case both the adjacent surfaces as well as the lubricant move with respect to some global coordinate system, the velocity vector to be defined equals the sum of both surface velocities relative to the stationary film profile. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words VELOCITY.

2nd data block 1-5

1st

I

Enter the number of sets of velocity (optional).

6-10

2nd

I

Enter unit number for input of velocity data, defaults to input.

Data blocks 3 through 7 are entered as pairs; one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define initial condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the UVELOC user subroutine is required.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

VELOCITY (with TABLE Input - Hydrodynamic) 1193 Define Nodal Velocity Components

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

E

Velocity in first coordinate direction.

11-20

2nd

E

Velocity in second coordinate direction.

5th data block - Table ID 1-5

1st

I

Table ID associated with the first coordinate direction.

6-10

2nd

I

Table ID associated with the second coordinate direction.

I

Enter the geometry type:

6th data block 1-5

1st

1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 7th data block Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

1194 VELOCITY (Hydrodynamic) Define Nodal Velocity Components

VELOCITY (Hydrodynamic)

Define Nodal Velocity Components

The information provided here is based upon not using the table driven input style. Description This option allows the specification of the nodal velocity components in a bearing analysis or a heat transfer analysis, where the convective terms are to be included. The nodal velocity components are defined by specifying the velocity magnitude of a series of components for sets of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the velocity values can be respecified, or initialized if no previous data was entered via UVELOC user subroutine. See Marc Volume D: User Subroutines and Special Routines. A summary of nodal velocities appears in the printout. This can be suppressed by specifying a nonzero value for the print-suppress parameter. Note that the velocity in a stationary bearing analysis is specified with respect to the (moving) lubricant. This means that, in case both the adjacent surfaces as well as the lubricant move with respect to some global coordinate system, the velocity vector to be defined equals the sum of both surface velocities relative to the stationary film profile. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VELOCITY.

2nd data block 1-5

1st

I

Number of data blocks used to input nodal velocity components. If a negative value is entered, the UVELOC user subroutine is called for every node.

6-10

2nd

I

Enter the unit number for input of the velocity field. Default to unit 5, unless the INPUT TAPE parameter has been used.

11-15

3rd

I

Set to 1 to suppress printout of the summary of nodal velocity components.

Data blocks 3, 4 and 5 should be repeated for each data set.

Main Index

VELOCITY (Hydrodynamic) 1195 Define Nodal Velocity Components

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

F

Enter the magnitude of the velocity in the first coordinate-direction for which the velocity is given. Additional velocity components in other coordinate directions must be specified on the same data line in F10 format. The number of components must equal the number of directions.

4th data block Enter a list of coordinate directions in which the velocity is specified. NOTE: List verbs EXCEPT and INTERSECT are illegal here. 5th data block Enter a list of nodes for which the velocity vector as defined in data blocks 3 and 4 applied.

Main Index

1196 THICKNESS (with TABLE Input - Model Definition) Define Lubrication Thickness

THICKNESS (with TABLE Input - Model Definition)

Define Lubrication Thickness

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the thickness of the lubricant film in a bearing analysis. The nodal thicknesses are specified by giving the thickness values for a list of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the nodal thickness values can be respecified, or initialized in case no previous data was input, via the UGROOV user subroutine (see Marc Volume D: User Subroutines and Special Routines). The lubricant thickness is associated with a boundary condition name that is activated with the LOADCASE history definition option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words THICKNESS.

2nd data block 1-5

1st

I

Enter the number of sets of nodal thickness to be entered (optional).

6-10

2nd

I

Enter unit number for input of nodal thickness data, defaults to input.

Data blocks 3 through 7 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define the lubricant thickness, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the UGROOV user subroutine is required to specify thickness.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

THICKNESS (with TABLE Input - Model Definition) 1197 Define Lubrication Thickness

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Nodal thickness.

I

Table ID for nodal thickness.

5th data block 1-5

1st

The 6th and 7th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

1198 THICKNESS Define Lubrication Thickness

THICKNESS

Define Lubrication Thickness

The information provided here is based upon not using the table driven input style. Description This option defines the thickness of the lubricant film in a bearing analysis. The nodal thicknesses are specified by giving the thickness values for a list of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the nodal thickness values can be respecified, or initialized in case no previous data was input, via the UTHICK user subroutine. See Marc Volume D: User Subroutines and Special Routines. A summary of nodal thickness values appears in the printout. This can be suppressed by specifying a nonzero value for the print-suppress parameter. The input of element thicknesses can be done via the GEOMETRY option or by means of the UGROOV user subroutine. Element thickness values usually only have to be defined in case of film discontinuities (grooves). See Marc Volume A: Theory and User Information for a description of the various ways to specify the contributions to the total lubricant film. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word THICKNESS.

2nd data block 1-5

1st

I

Number of data blocks used to input nodal thickness values (optional). If a negative value is entered, the UTHICK user subroutine is called for every node.

6-10

2nd

I

Enter the unit number for input of film thicknesses. Default to unit 5.

11-15

3rd

I

Set to 1 to suppress printout of the nodal thickness summary.

The third and fourth blocks should be entered in pairs, one pair for each distinct nodal data set. 3rd data block 1-10

1st

F

Enter nodal thickness value.

4th data block Enter a list of nodes for which the thickness as specified in data block 3 is applied.

Main Index

RESTRICTOR (with TABLE Input - Model Definition) 1199 Coefficient Input for Bearing Analysis

RESTRICTOR (with TABLE Input - Model Coefficient Input for Bearing Analysis Definition) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows restrictor coefficients and associated pump pressures to be input. Nonuniform restrictors or pump pressures can be obtained via the URESTR user subroutine. See Marc Volume D: User Subroutines and Special Routines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word FILMS.

2nd data block 1-5

1st

I

Number of sets of data used to input film (optional).

6-10

2nd

I

Unit number for input of film data, defaults to input.

Data blocks 3 through 8 are entered for each film input. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define film boundary condition. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the URESTR user subroutine is required for this boundary condition.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used, enter 0.

26-30

6th

I

Not used, enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block

Main Index

1-10

1st

F

Reference value of restrictor coefficient.

11-20

2nd

F

Reference value of pump pressure.

1200 RESTRICTOR (with TABLE Input - Model Definition) Coefficient Input for Bearing Analysis

Format Fixed

Free

Data Entry Entry

5th data block - Table IDs 1-5

1st

I

Enter the table ID associated with the restrictor coefficient.

6-10

2nd

I

Enter the table ID associated with the pump pressure.

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

11-15

3rd

I

Normal flux

Enter the face ID.

The 7th and 8th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

RESTRICTOR 1201 Coefficient Input for Bearing Analysis

RESTRICTOR

Coefficient Input for Bearing Analysis

The information provided here is based upon not using the table driven input style. Description This option allows restrictor coefficients and associated pump pressures to be input. Nonuniform restrictors or pump pressures can be obtained via the URESTR user subroutine. See Marc Volume D: User Subroutines and Special Routines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word RESTRICTOR.

2nd data block 1-5

1st

I

Number data blocks used to input the restrictor coefficient data (optional).

6-10

2nd

I

Enter the unit number for input of restrictor data. Default to unit 5, unless the INPUT TAPE parameter has been used.

Data blocks 3 and 4 are entered in pairs, one pair for each distinct data set. 3rd data block 1-5

1st

I

Face identification. Same as for the FLUX user subroutine. See Marc Volume B: Element Library.

6-15

2nd

F

Reference value of restrictor coefficient.

16-25

3rd

F

Reference value of pump pressure (reference values can be modified by the URESTR user subroutine).

4th data block Enter a list of elements for which restrictor data as defined in data block 3 is applied.

Main Index

1202 CONTROL (Hydrodynamic) Define Maximum Number of Increments for Bearing Analysis

CONTROL (Hydrodynamic)

Define Maximum Number of Increments for Bearing Analysis

Description This option allows you to input the maximum number of increments in a hydrodynamic bearing analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

I

Maximum number of bearing increments in this run. Default is 4.

2nd data block 1-5

1st

3rd data block Not used. Enter a blank data line.

Main Index

ISOTROPIC (with TABLE Input - Hydrodynamic) 1203 Define Lubricant Material Properties

ISOTROPIC (with TABLE Input Hydrodynamic)

Define Lubricant Material Properties

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option is used to define the lubricant material properties for all of the elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of distinct sets of lubricant material properties to be input (optional).

6-10

2nd

I

Enter unit number for input of data. Defaults to input.

Data blocks 3 through 6 should be entered as pairs, one for each distinct data block. 3rd data block 1-5

1st

I

Material identification number (1,2,3, etc.) for cross-reference to the material data base.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material data base.

4th data block

Main Index

1-10

1st

F

Enter the reference value of the viscosity.

11-20

2nd

F

Enter the value of the cavitation pressure.

21-30

3rd

F

Enter the reference value of the mass density of the lubricant.

1204 ISOTROPIC (with TABLE Input - Hydrodynamic) Define Lubricant Material Properties

Format Fixed

Free

Data Entry Entry

5th data block 1-5

1st

I

Table ID for viscosity.

6-10

2nd

I

Table ID for cavitation pressure.

11-15

3rd

I

Table ID for mass density.

• 6th data block

1-80

Main Index

Enter element data set for which the properties specified above are applied.

ISOTROPIC (Hydrodynamic) 1205 Define Lubricant Material Properties

ISOTROPIC (Hydrodynamic)

Define Lubricant Material Properties

The information provided here is based upon not using the table driven input style. Description This option is used to define the lubricant material properties for all of the elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word ISOTROPIC.

I

Enter the number of distinct sets of lubricant material properties to be input (optional).

2nd data block 1-5

1st

For temperature dependent properties, these are values corresponding to the first (lowest temperature) breakpoint (see TEMPERATURE EFFECTS option). A temperature dependent property is undefined below its lowest breakpoint. 6-10

2nd

I

Enter unit number for input of data. Defaults to input.

The 3rd, 4th, and 5th data blocks should be entered as pairs, one for each distinct data block. 3rd data block 1-5

1st

I

Material identification number (1,2,3, etc.) for cross-reference to TEMPERATURE EFFECTS option.

4th data block 1-10

1st

F

Enter the reference temperature value of the viscosity.

11-20

2nd

F

Enter the value of the cavitation pressure.

21-30

3rd

F

Enter the reference value of the mass density of the lubricant.

5th data block Enter element data set for which the properties as specified in data block 3 applies.

Main Index

1206 TEMPERATURE EFFECTS (Hydrodynamic) Define Effect of Temperature in Bearing Analysis

TEMPERATURE EFFECTS (Hydrodynamic)

Define Effect of Temperature in Bearing Analysis

The information provided here is based upon not using the table driven input style. This option is not available with the table driven input. Description This option defines the variation of material property (viscosity) temperature. The values read in through the ISOTROPIC option are those at the lowest temperature specified. Properties are not defined below the lowest temperature. The temperature dependency can be entered using one of the following two options: a. The variation of a particular property with temperature is specified as a piecewise linear curve. Breakpoints must be given in ascending order of temperature. b. The particular property value and temperature lying on the relevant curve are input directly. Data points must be given in ascending order of temperature. This option is flagged by entering the word DATA on the 1st data line. In hydrodynamic bearing analyses, the temperature is defined as the second state variable via the INITIAL STATE and CHANGE STATE options.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words TEMPERATURE EFFECTS.

21-80

2nd

A

Enter the word DATA to indicate that option B is used.

For option A, use data blocks 2a and 3a. For option B, use data blocks 2b and 3b. Option A 2a data block

Main Index

1-5

1st

I

Number of slopes of viscosity versus temperature curve.

6-30

2nd

I

Not used; enter 0.

31-35

3rd

I

Material type identification (1,2,3,...) for cross-reference to the ISOTROPIC option.

36-40

4th

I

Logical unit number for input of this set of data. Defaults to data lines.

TEMPERATURE EFFECTS (Hydrodynamic) 1207 Define Effect of Temperature in Bearing Analysis

Format Fixed

Free

Data Entry Entry

3a data block Viscosity variation. Number of data lines as given on data block 2a, first field. 1-15

1st

16-30

F

Slope of viscosity versus temperature curve.

F

Temperature above which slope becomes operative.

Option B 2b data block 1-5

1st

I

Number of data points on the viscosity versus temperature curve.

6-30

2nd

I

Not used; enter 0.

31-35

3rd

I

Material type identification (1,2,3...) for cross-reference to the ISOTROPIC option.

36-40

4th

I

Logical unit number for input of this set of data. Defaults to data lines.

3b data block Viscosity variation. Number of data lines as given on data block 2b, first field. 1-15

1st

F

Enter the value of the viscosity.

16-30

2nd

F

Enter the associated temperature. Note:

Main Index

Since in bearing analysis no incrementation is performed, the value of the viscosity is always taken at the current temperature. No averaging is performed.

1208 TEMPERATURE EFFECTS (Hydrodynamic) Define Effect of Temperature in Bearing Analysis

Main Index

Chapter 3: Model Definition Options 1209 Acoustic Analysis

Chapt Acoustic Analysis er 3: Marc has two procedures for performing acoustic analysis. One calculates the pressure distribution in a with rigid reflecting surfaces and the other for when the surfaces are deformable. In the first Mode cavity procedure, an eigenvalue analysis is performed, and then modal superposition is used to obtain the transient response. In the second procedure a harmonic analysis is performed. l Defini This section describes the data required for an acoustic analysis where the pressure distribution in a cavity with reflecting surfaces is calculated. For acoustic structural problems, the acoustive and structural tion regions are modeled as separate bodies, and the CONTACT option is used to apply the interface boundary conditions between the two regions. The fluid in the cavity is treated as an inviscid compressible fluid. Optio ns

Main Index

1210 FIXED PRESSURE (with TABLE Input - Acoustic) Define Fixed Pressure

FIXED PRESSURE (with TABLE Input - Acoustic)

Define Fixed Pressure

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This data defines a potential fixed pressure boundary condition. The boundary conditions are specified either by giving the pressure, a list of degrees of freedom, and either a list of nodal numbers or a list of geometric entities. This boundary condition is activated or deactivated using the LOADCASE model or history definition option. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. The FORCDF user subroutine or the TABLE model definition option can be used to enter frequency dependent boundary conditions in a harmonic acoustic analysis. Unless shell elements are used, there is only one pressure degree of freedom per node in a diffusion analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED PRESS.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

Unit number to read data default is the standard input file.

Data blocks 3 through 10 are repeated for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutines are required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

Main Index

FIXED PRESSURE (with TABLE Input - Acoustic) 1211 Define Fixed Pressure

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE model or history definition option.

If a real pressure is to be defined, data blocks 4 and 5 are used. If a complex harmonic pressure is to be defined, data blocks 4 and 5 define the real component or the magnitude, and data blocks 6 and 7 define the imaginary component or the phase. 4th data block - Magnitudes 1-10

1st

E

Prescribed pressure for first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed pressure for second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed pressure for third degree of freedom listed in data block 8.

5th data block - Table IDs 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

The 6th and 7th data blocks are only required if a complex boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of pressure or the phase of the first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed imaginary component of pressure or the phase of the second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed imaginary component of pressure or the phase of the third degree of freedom listed in data block 8.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for imaginary component or phase for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for imaginary component or phase for the third degree of freedom listed.

8th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed.

Main Index

1212 FIXED PRESSURE (with TABLE Input - Acoustic) Define Fixed Pressure

Format Fixed

Free

Data Entry Entry Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 9th and 10th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

10th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

Main Index

FIXED PRESSURE (Acoustic) 1213 Define Nodal Fixed Pressure

FIXED PRESSURE (Acoustic)

Define Nodal Fixed Pressure

The information provided here is based upon not using the table driven input style. Description This option defines the fixed pressure that each node must take during the first and subsequent increments, unless it is further modified using the PRESS CHANGE option. The boundary conditions are specified either by giving the pressure and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED PRESSURE.

2nd data block 1-5

1st

I

Number of sets of boundary condition blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option block. Enter 1 for excitation boundary conditions for harmonic analysis.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly. Enter 1 if harmonic boundary condition is input as magnitude and phase. If blank, real and imaginary values are given.

For each set of boundary conditions, use the 3a and 4a data blocks, or the 3b, 4b, and 5b data blocks. For analyses which do not include heat transfer shell elements, use the 3a and 4a data blocks. 3a data block 1-10

1st

F

Prescribed nodal pressure.

4a data block Enter a list of nodes for which the above pressure is applied. 3b, 4b and 5b data blocks for analyses which include heat transfer shell elements.

Main Index

1214 FIXED PRESSURE (Acoustic) Define Nodal Fixed Pressure

Format Fixed

Free

Data Entry Entry

3b data block 1-10

1st

E

Prescribed pressure for first degree of freedom listed in data block 4b.

11-20

2nd

E

Prescribed pressure for second degree of freedom listed in data block 4b.

21-30

3rd

E

Prescribed pressure for third degree of freedom listed in data block 4b.

See Marc Volume B: Element Library for the definition of nodal degrees of freedom. 4b data block Enter a list of degrees of freedom to which the above prescribed pressures are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above boundary conditions are applied.

Main Index

DIST SOURCES (with TABLE Input - Acoustic) 1215 Define Distributed Sources

DIST SOURCES (with TABLE Input - Acoustic)

Define Distributed Sources

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows distributed (surface and volumetric) sources to be specified. Distributed sources are converted to consistent nodal sources by Marc. Note that for a given element type, there is an established convention for the application of surface source on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent sources. Note:

If a distributed source is applied on the bottom of a shell, the source is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST SOURCES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed sources to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed source data, defaults to input.

Data blocks 3 through 10 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

Main Index

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

1216 DIST SOURCES (with TABLE Input - Acoustic) Define Distributed Sources

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of this type of distributed sources.

I

Enter the table ID associated with the distributed source.

4th data block 1-10

1st

5th data block 1-5

1st

The 6th and 7th data blocks are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of source or phase angle.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase.

8th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

Normal source (bottom surface for shells)

10: Normal source (top surface for shells) 11-15

3rd

I

Enter the face ID or edge ID.

The 9th and 10th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention

Main Index

DIST SOURCES (with TABLE Input - Acoustic) 1217 Define Distributed Sources

Format Fixed

Free

Data Entry Entry 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

10th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

1218 DIST SOURCES (Acoustic - Model Definition) Define Distributed Sources

DIST SOURCES (Acoustic - Model Definition)

Define Distributed Sources

The information provided here is based upon not using the table driven input style. Description This option allows incrementally distributed (surface and volumetric) sources to be specified in an acoustic analysis. Distributed sources are converted to consistent nodal sources by Marc. Note that for a given element type, there is an established convention for the application of surface source on a particular face. The FLUX user subroutine can be used to input time and spatial dependent fluxes. Format Format Fixed

Free

DATA Entry Entry

1st data block 1-10

1st

A

Enter the words DIST SOURCES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed sources to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed source data, defaults to input.

The following 3rd and 4th data blocks are repeated for each set of distributed sources. 3rd data block 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed sources.

16-20

3rd

I

Source index (optional). (Source index is to be used in the FLUX user subroutine.)

4th data block Enter a list of elements associated with the above distributed sources.

Main Index

POINT SOURCE (with TABLE Input - Acoustic) 1219 Define Point Source

POINT SOURCE (with TABLE Input - Acoustic)

Define Point Source

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows total nodal point source to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent source. Either the FORCDF user subroutine or the TABLE model definition option can be used for frequency dependent source loads in a complex harmonic analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT SOURCE.

2nd data block 1-5

1st

I

Enter the number of sets of point source to be entered (optional).

6-10

2nd

I

Enter unit number for input of point source data, defaults to input.

Data blocks 3 through 9 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

Main Index

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter a 1 if first point source is to be applied to all degrees of freedom of a heat transfer shell.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1220 POINT SOURCE (with TABLE Input - Acoustic) Define Point Source

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Magnitude of point source.

11-20

2nd

F

Magnitude of point source for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point source for third degree of freedom, (heat transfer shell elements only).

5th data block 1-5

1st

I

Table ID for point source.

6-10

2nd

I

Table ID for point source for second degree of freedom (Heat transfer shell elements only).

11-15

3rd

I

Table ID for point source for third degree of freedom (Heat transfer shell elements only).

The 6th and 7th data blocks are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of point source or phase.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component or phase.

The 8th and 9th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 8th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs

Main Index

POINT SOURCE (with TABLE Input - Acoustic) 1221 Define Point Source

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

9th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 8th data block.

1222 POINT SOURCE (Acoustic - Model Definition) Define Point Sources

POINT SOURCE (Acoustic - Model Definition)

Define Point Sources

The information provided here is based upon not using the table driven input style. Description This option allows incremental nodal point sources to be specified in an acoustic analysis. The FORCDT user subroutine can be used for the time dependent sources. Enter an upper bound to the number of nodes with point sources on the DIST LOADS parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

A

Enter the words POINT SOURCE.

2nd data block 1-5

1st

I

Enter the number of sets of point sources to be entered (optional).

6-10

2nd

I

Enter 1 is excitation boundary conditions for harmonic analysis.

11-15

3rd

I

Enter 1 if harmonic boundary condition is input magnitude and phase. If blank, real and imaginary values are given.

The following 3rd and 4th data blocks are repeated for each set of distributed sources. 3rd data block 1-10

F

Magnitude of incremental point source.

11-20

F

Magnitude of point source for second degree of freedom, (heat transfer shell elements only).

21-30

F

Magnitude of point source for third degree of freedom, (heat transfer shell elements only).

4th data block Enter a list of nodes to which the above nodal sources are applied.

Main Index

ISOTROPIC (with TABLE Input - Acoustic) 1223 Define Properties for Acoustic Cavity

ISOTROPIC (with TABLE Input Acoustic)

Define Properties for Acoustic Cavity

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define properties for the fluid/gas in the acoustic cavity. You can also associate these material properties with a list of element numbers. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 should be entered as pairs and repeated for each data block. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name.

4th data block 1-10

1st

F

Bulk modulus.

11-20

2nd

F

Enter the mass density.

5th data block 1-5

1st

I

Table ID for bulk modulus.

6-10

2nd

I

Table ID for mass density.

6th data block Enter a list of elements associated with this material.

Main Index

1224 ISOTROPIC (Acoustic) Define Properties for Acoustic Cavity

ISOTROPIC (Acoustic)

Define Properties for Acoustic Cavity

The information provided here is based upon not using the table driven input style. Description This option allows you to define properties for the fluid/gas in the acoustic cavity. You can also associate these material properties with a list of element numbers. Note:

For coupled-structural acoustic analysis or for including fluid drag, you must use ACOUSTIC model definition option to define the properties of the acoustic media.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

The 3rd, 4th, and 5th data blocks should be entered as pairs and repeated for each data block. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

4th data block 1-10

1st

F

Bulk modulus.

11-20

2nd

F

Enter the mass density.

5th data block Enter a list of elements associated with this material.

Main Index

ACOUSTIC (with TABLE Input - Acoustic) 1225 Define Material Properties for Acoustic Analysis

ACOUSTIC (with TABLE Input - Define Material Properties for Acoustic Analysis Acoustic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define material properties for an acoustic medium (fluid). Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ACOUSTIC

2nd data block 1-5

1st

I

Enter the number of sets of acoustic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 to 6 are repeated as a set, once for each set of acoustic material. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

4th data block 1-10

1st

F

Fluid bulk modulus.

11-20

2nd

F

Fluid drag (only used for acoustic-solid coupled harmonic analysis).

21-30

3rd

F

Mass density of fluid.

5th data block 1-5

1st

I

Table ID for fluid bulk modulus.

6-10

2nd

I

Table ID for fluid drag.

11-15

3rd

I

Table ID for mass density.

6th data block Enter a list of elements associated with this material.

Main Index

1226 ACOUSTIC Define Material Properties for Acoustic Analysis

ACOUSTIC

Define Material Properties for Acoustic Analysis

The information provided here is based upon not using the table driven input style. Description This option allows you to define material properties for an acoustic medium (fluid). Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ACOUSTIC

2nd data block 1-5

1st

I

Enter the number of sets of acoustic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 5 are repeated as a set, once for each set of acoustic material. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

4th data block 1-10

1st

F

Fluid bulk modulus.

11-20

2nd

F

Fluid drag (only used for acoustic-solid coupled harmonic analysis).

21-30

3rd

F

Mass density of fluid.

5th data block Enter a list of elements associated with this material.

Main Index

Chapter 3: Model Definition Options 1227 Electrostatic Analysis

Chapt Electrostatic Analysis er 3: This section describes the input of material data and boundary conditions applicable for electrostatic The boundary conditions discussed in this section are also used for coupled electrostaticMode problems. structural problems. The ISOTROPIC and ORTHOTROPIC options are used to define dielectric constants in electrostatic analysis. A steady-state solution can be obtained in one increment using the STEADY l STATE option. In addition, the FLUX user subroutine can be used for variable distributions of charges; Defini the UEPS user subroutine can be used for the anisotropic dielectric constants. tion Optio ns

Main Index

1228 FIXED EL-POT (with TABLE Input - Electrostatic) Define Fixed Potential

FIXED EL-POT (with TABLE Input - Electrostatic)

Define Fixed Potential

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. Note that unless heat transfer shell elements are used, there is only one degree of freedom in a heat transfer analysis. You must specify it. The prescribed potential is associated with a boundary condition name that is activated with the LOADCASE history definition. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED EL-POT.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3a data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter a 1 if first prescribed potential entered is to be applied for all degrees of freedom of a heat transfer shell.

FIXED EL-POT (with TABLE Input - Electrostatic) 1229 Define Fixed Potential

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11 Element-Edges IDs

Main Index

1230 FIXED EL-POT (with TABLE Input - Electrostatic) Define Fixed Potential

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED EL-POT (Electrostatic) 1231 Define Fixed Nodal Potential

FIXED EL-POT (Electrostatic)

Define Fixed Nodal Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each node must take during the first and subsequent increments. The boundary conditions are specified either by giving the potential and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words FIXED EL-POT.

2nd data block 1-5

1st

I

Number of sets of boundary condition blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly.

Data blocks 3a and 4a are for analyses which do not include shell elements. 3rd data block 1-10

1st

F

Prescribed nodal potential.

4a data block Enter a list of nodes for which the above potential is applied. Data blocks 3b, 4b, and 5b are for analyses which include shell elements. 3b data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 4b.

11-20

1st

F

Prescribed potential for second degree of freedom listed in data block 4b.

21-30

2nd

F

Prescribed potential for third degree of freedom listed in data block 4b. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

Main Index

1232 FIXED EL-POT (Electrostatic) Define Fixed Nodal Potential

Format Fixed

Free

Data Entry Entry

4b data block Enter a list of degrees of freedom to which the above prescribed potential is given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above fixed potential conditions are applied.

Main Index

FIXED POTENTIAL (with TABLE Input - Electrostatic) 1233 Define Fixed Potential

FIXED POTENTIAL (with TABLE Input - Electrostatic) Define Fixed Potential The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. Note that unless heat transfer shell elements are used, there is only one degree of freedom in a heat transfer analysis. You must specify it. The prescribed potential is associated with a boundary condition name that is activated with the LOADCASE history definition. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3a data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter a 1 if first prescribed potential entered is to be applied for all degrees of freedom of a heat transfer shell.

1234 FIXED POTENTIAL (with TABLE Input - Electrostatic) Define Fixed Potential

Format Fixed 31-63

Free

Data Entry Entry

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6.

4th data block

(See Marc Volume B: Element Library for the definition of nodal degrees of freedom.) 5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11 Element-Edges IDs

Main Index

FIXED POTENTIAL (with TABLE Input - Electrostatic) 1235 Define Fixed Potential

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

1236 FIXED POTENTIAL (Electrostatic) Define Fixed Nodal Potential

FIXED POTENTIAL (Electrostatic)

Define Fixed Nodal Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each node must take during the first and subsequent increments. The boundary conditions are specified either by giving the potential and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Format Format

Data Entry Entry

1st data block 1-15

1st

A

Enter the words FIXED POTENTIAL.

2nd data block 1-5

1st

I

Number of sets of boundary condition blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly.

Data blocks 3a and 4a are for analyses which do not include shell elements. 3rd data block 1-10

1st

F

Prescribed nodal potential.

4a data block Enter a list of nodes for which the above potential is applied. Data blocks 3b, 4b, and 5b are for analyses which include shell elements. 3b data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 4b.

11-20

1st

F

Prescribed potential for second degree of freedom listed in data block 4b.

21-30

2nd

F

Prescribed potential for third degree of freedom listed in data block 4b. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

Main Index

FIXED POTENTIAL (Electrostatic) 1237 Define Fixed Nodal Potential

Format

Data Entry Entry

4b data block Enter a list of degrees of freedom to which the above prescribed potential is given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above fixed potential conditions are applied.

Main Index

1238 DIST CHARGES (with TABLE Input - Electrosatatic) Define Distributed Charges

DIST CHARGES (with TABLE Input Electrosatatic)

Define Distributed Charges

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface flux on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent charges. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition.

Note:

If a distributed charge is applied on the bottom of a shell, the charge is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

Data blocks 3 through 8 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

DIST CHARGES (with TABLE Input - Electrosatatic) 1239 Define Distributed Charges

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of this type of distributed charges.

I

Enter the table ID associated with the distributed charge.

4th data block 1-10

1st

5th data block 1-5

1st

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal charge (bottom surface for shells) 10: Normal charge (top surface for shells)

11-15

3rd

I

Enter the face ID or edge ID.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID

Main Index

1240 DIST CHARGES (with TABLE Input - Electrosatatic) Define Distributed Charges

Format Fixed

Free

Data Entry Entry 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

DIST CHARGES (Electrostatic) 1241 Define Distributed Charges

DIST CHARGES (Electrostatic)

Define Distributed Charges

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface charge on a particular face. The FLUX user subroutine can be used to input spatially dependent charges. Format Format Fixed

For

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DIST CHARGES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

The 3rd and 4th data blocks are repeated for each set of distributed charges. 3rd data block 1-5

1st

I

Parameter identifying the type of distributed charge. See description of library element in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed charges.

16-20

3rd

I

Charge index (optional). Charge index is to be used in the FLUX user subroutine.

4th data block Enter a list of elements associated with the above distributed charges.

Main Index

1242 POINT CHARGE (with TABLE Input - Electrostatic) Define Point Charges

POINT CHARGE (with TABLE Input - Electrostatic)

Define Point Charges

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows total nodal point charges to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent fluxes. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition.

Format Format Fixed

Free

Data Entry

Entry

1st data block 1-10

1st

A

Enter the words POINT CHARGE.

2nd data block 1-5

1st

I

Enter the number of sets of point charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of point charge data, defaults to input.

Data blocks 3 through 7 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if first point charge is to be applied to all degrees of freedom of a heat transfer shell.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

POINT CHARGE (with TABLE Input - Electrostatic) 1243 Define Point Charges

Format Fixed

Free

Data Entry

Entry

4th data block 1-10

1st

F

Magnitude of point charge.

11-20

2nd

F

Magnitude of point charge for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point charge for third degree of freedom, (heat transfer shell elements only).

5th data block 1-5

1st

I

Table ID for point charge.

6-10

2nd

I

Table ID for point charge for second degree of freedom (Heat transfer shell elements only).

11-15

3rd

I

Table ID for point flux for third degree of freedom (heat transfer shell elements only).

Data blocks 6 and 7 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

1244 POINT CHARGE Define Nodal Point Charges

POINT CHARGE

Define Nodal Point Charges

The information provided here is based upon not using the table driven input style. Description This option allows total nodal point charges to be specified. The FORCDT user subroutine can be used for nonuniform point charges. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words POINT CHARGE.

2nd data block 1-5

1st

I

Enter the number of sets of point charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of point charge data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-10

1st

F

Magnitude of point charge.

11-20

2nd

F

Magnitude of point charge for second degree of freedom (shell elements only).

21-30

3rd

F

Magnitude of point charge for third degree of freedom (shell elements only).

4th data block Enter a list of nodes to which the above nodal charges are applied.

Main Index

ISOTROPIC (with TABLE Input - Electrostatic) 1245 Define Electrical Properties for Isotropic Materials

ISOTROPIC (with TABLE Input Define Electrical Properties for Isotropic Materials - Electrostatic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define electrical properties for an isotropic material. You can also associate these material properties with a list of element numbers. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input data file.

Data blocks 3 through 6 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.)

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

F

Permittivity constant.

I

Table ID for permittivity.

4th data block 1-10

1st

5th data block 1-5

1st

6th data block Enter a list of elements associated with this material.

Main Index

1246 ISOTROPIC (Electrostatic) Define Electrical Properties for Isotropic Materials

ISOTROPIC (Electrostatic)

Define Electrical Properties for Isotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define electrical properties for an isotropic material. You can also associate these material properties with a list of element numbers. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input data file.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.)

F

Permittivity constant.

4th data block 1-10

1st

5th data block Enter a list of elements associated with this material.

Main Index

ORTHOTROPIC (with TABLE Input - Electrostatic) 1247 Define Electrical Properties for Orthotropic Materials

Define Electrical Properties for Orthotropic Materials ORTHOTROPIC (with TABLE Input - Electrostatic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define electrical properties for an orthotropic material. You can also associate these material properties with a list of element numbers. Note:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Library Elements, if necessary). No defaults for this data are provided by Marc.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPI.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the UEPS and ORIENT user subroutines.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

4th data block These values are with respect to the user coordinate (1, 2, 3) system.

Main Index

1-10

1st

F

ε11 Electric permittivity.

11-20

2nd

F

ε22 Electric permittivity.

1248 ORTHOTROPIC (with TABLE Input - Electrostatic) Define Electrical Properties for Orthotropic Materials

Format Fixed 21-30

Free 3rd

Data Entry Entry F

ε33 Electric permittivity.

5th data block 1-5

1st

I

Table ID for ε11.

6-10

2nd

I

Table ID for ε22.

11-15

3rd

I

Table ID for ε33.

6th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

ORTHOTROPIC (Electrical) 1249 Define Electrical Properties for Orthotropic Materials

ORTHOTROPIC (Electrical) Define Electrical Properties for Orthotropic Materials The information provided here is based upon not using the table driven input style. Description This option allows you to define electrical properties for an orthotropic material. You can also associate these material properties with a list of element numbers. Note:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Library Elements, if necessary). No defaults for this data are provided by Marc.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to ORTHO TEMP option.

6-10

2nd

I

Enter 1 to call the UEPS and ORIENT user subroutines.

4th data block These values are with respect to the user coordinate (1, 2, 3) system. 1-10

1st

F

ε11 Electric permittivity

11-20

2nd

F

ε22 Electric permittivity

21-30

3rd

F

ε33 Electric permittivity

5th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

1250 ORTHOTROPIC (Electrical) Define Electrical Properties for Orthotropic Materials

Main Index

Chapter 3: Model Definition Options 1251 Piezoelectric Analysis

Chapt Piezoelectric Analysis er 3: This section describes the input of additional material data and boundary conditions applicable to piezoelectric problems. A piezoelectric analysis is a coupled mechanical-electrostatic analysis. The input Mode for mechanical material data is done using the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC option as described in the section about Material Properties. The PIEZOELECTRIC option is used to define the l piezoelectric coupling matrix and the dielectric constants. The mechanical boundary conditions that can Defini be applied are similar to what is described in the section about Mechanical Analysis. The electrostatic boundary conditions are described here. tion Optio ns

Main Index

1252 FIXED POTENTIAL (with TABLE Input - Piezoelectric) Define Fixed Potential

FIXED POTENTIAL (with TABLE Input - Piezoelectric) Define Fixed Potential The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. The prescribed potential is associated with a boundary condition name that is activated with the LOADCASE history definition. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. The FORCDF user subroutine or the TABLE model definition option can be used to enter nonuniform frequency dependent boundary conditions in a harmonic analysis. Note:

Currently there are no piezoelectric shell elements, so the degree of freedom is always one. You must specify it.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 10 are repeated for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutine required for this boundary condition.

Main Index

FIXED POTENTIAL (with TABLE Input - Piezoelectric) 1253 Define Fixed Potential

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

Data blocks 6 and 7 are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of potential or the phase of the first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed imaginary component of potential or the phase of the second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed imaginary component of potential or the phase of the third degree of freedom listed in data block 8.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

Main Index

1st

I

Enter the table ID for imaginary component or phase for the first degree of freedom listed.

1254 FIXED POTENTIAL (with TABLE Input - Piezoelectric) Define Fixed Potential

Format Fixed

Free

Data Entry Entry

6-10

2nd

I

Enter the table ID for imaginary component or phase for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for imaginary component or phase for the third degree of freedom listed.

8th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 9 and 10 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block

1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

10th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

Main Index

FIXED POTENTIAL (Piezoelectric - Model Definition) 1255 Define Fixed Nodal Potential

FIXED POTENTIAL (Piezoelectric - Model Definition)

Define Fixed Nodal Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each specified node must take during the first and subsequent increments, unless it will be modified using the POTENTIAL CHANGE option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words FIXED POTENTIAL.

I

Number of sets of boundary condition blocks to be read (optional).

2nd data block 1-5

1st

Data blocks 3a and 4a are for analyses which do not include shell elements. 3a data block 1-10

1st

F

Prescribed nodal potential.

4a data block Enter a list of nodes for which the above potential is applied. Data blocks 3b, 4b, and 5b are for analyses which include shell elements. 3b data block 1-10

1st

F

Prescribed nodal potential. NOTE: Currently, there are no piezoelectric shell elements, but it is possible to use mechanical shell elements in a piezoelectric analysis.

4b data block 1-5

1st

I

Enter 1.

5b data block Enter a list of nodes for which the above fixed potential conditions are applied.

Main Index

1256 DIST CHARGES (with TABLE Input - Piezoelectric) Define Distributed Charges

DIST CHARGES (with TABLE Input Piezoelectric)

Define Distributed Charges

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface flux on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent charges. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition.

Note:

If a distributed charge is applied on the bottom of a shell, the charge is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

Data blocks 3 through 10 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

Main Index

4th

I

Not used; enter 0.

DIST CHARGES (with TABLE Input - Piezoelectric) 1257 Define Distributed Charges

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of the distributed charges.

I

Enter the table ID associated with the distributed charge.

4th data block 1-10

1st

5th data block 1-5

1st

Data blocks 6 and 7 are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of the distributed charge or the phase.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component of the distributed charge or the phase.

8th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal charge (bottom surface for shells) 10: Normal charge (top surface for shells)

11-15

3rd

I

Enter the face ID or edge ID.

Data blocks 9 and 10 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs

Main Index

1258 DIST CHARGES (with TABLE Input - Piezoelectric) Define Distributed Charges

Format Fixed

Free

Data Entry Entry 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

10th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

DIST CHARGES (Piezoelectric - Model Definition) 1259 Define Distributed Charges

DIST CHARGES (Piezoelectric - Model Definition) Define Distributed Charges The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface charge on a particular face. The FLUX user subroutine can be used to input spatially dependent charges. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DIST CHARGES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

The 3rd and 4th data blocks are repeated for each set of distributed charges. 3rd data block 1-5

1st

I

Parameter identifying the type of distributed charge. See description of library element in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed charges.

16-20

3rd

I

Charge index (optional). Charge index is to be used in the FLUX user subroutine.

4th data block Enter a list of elements associated with the above distributed charges.

Main Index

1260 POINT CHARGE (with TABLE Input - Piezoelectric) Define Point Charges

POINT CHARGE (with TABLE Input - Piezoelectric)

Define Point Charges

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows total nodal point charges to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent charge. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. The FORCDF user subroutine or the TABLE model definition option can be used to enter nonuniform frequency dependent boundary conditions in a harmonic analysis. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CHARGE.

2nd data block 1-5

1st

I

Enter the number of sets of point charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of point charge data, defaults to input.

Data blocks 3 through 9 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

Main Index

4th

I

Not used; enter 0.

POINT CHARGE (with TABLE Input - Piezoelectric) 1261 Define Point Charges

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Enter a 1 if first point charge is to be applied to all degrees of freedom of a heat transfer shell.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

F

Magnitude of point charge.

I

Table ID for point charge.

4th data block 1-10

1st

5th data block 1-5

1st

Data blocks 6 and 7 are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of point charge or phase.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component of point charge or phase.

Data blocks 8 and 9 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 8th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

9th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 8th data block.

1262 POINT CHARGE (Piezoelectric - Model Definition) Define Nodal Point Charges

POINT CHARGE (Piezoelectric - Model Definition)Define Nodal Point Charges The information provided here is based upon not using the table driven input style. Description This option allows total nodal point charges to be specified. The FORCDT user subroutine can be used for nonuniform point charges. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words POINT CHARGE.

2nd data block 1-5

1st

I

Enter the number of sets of point charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of point charge data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each set of point charges. 3rd data block 1-10

1st

F

Magnitude of point charge.

4th data block Enter a list of nodes to which the above nodal charges are applied.

Main Index

PIEZOELECTRIC (with TABLE Input - Piezoelectric) 1263 Define Electrical Data for Piezoelectric Analysis

PIEZOELECTRIC (with TABLE Input - Piezoelectric)

Define Electrical Data for Piezoelectric Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to specify the coupled electric-mechanical (stress based or strain based) properties eijk, and the electric properties εi for piezoelectric material. A description of the piezoelectric capabilities is included in Marc Volume A: Theory and User Information. Note:

In the current release, the table IDs are not used. All piezoelectric properties are constant.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PIEZOELECTRIC.

2nd data block 1-5

1st

I

Enter the number of sets of piezoelectric material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 12 are repeated as a set; once for each set of piezoelectric material to be input. 3rd data block 1-5

1st

I

Material identification number (1,2,3,etc) for cross-reference to the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC option.

6-10

2nd

I

Flag to indicate if the piezoelectric coupling matrix and the dielectric matrix is stress based or strain based. Enter 0 for stress based, and a 1 for strain based data.

4th data block

Main Index

1-10

1st

F

e111

11-20

2nd

F

e221

21-30

3rd

F

e331

1264 PIEZOELECTRIC (with TABLE Input - Piezoelectric) Define Electrical Data for Piezoelectric Analysis

Format Fixed

Free

Data Entry Entry

31-40

4th

F

e121

41-50

5th

F

e231

51-60

6th

F

e131

5th data block 1-5

1st

I

Table ID for e111

6-10

2nd

I

Table ID for e221

11-15

3rd

I

Table ID for e331

16-20

4th

I

Table ID for e121

21-25

5th

I

Table ID for e231

26-30

6th

I

Table ID for e131

6th data block 1-10

1st

F

e112

11-20

2nd

F

e222

21-30

3rd

F

e332

31-40

4th

F

e122

41-50

5th

F

e232

51-60

6th

F

e132

7th data block 1-5

1st

I

Table ID for e112

6-10

2nd

I

Table ID for e222

11-15

3rd

I

Table ID for e332

16-20

4th

I

Table ID for e122

21-25

5th

I

Table ID for e232

26-30

6th

I

Table ID for e132

8th data block

Main Index

1-10

1st

F

e113

11-20

2nd

F

e223

21-30

3rd

F

e333

31-40

4th

F

e123

PIEZOELECTRIC (with TABLE Input - Piezoelectric) 1265 Define Electrical Data for Piezoelectric Analysis

Format Fixed

Free

Data Entry Entry

41-50

5th

F

e233

51-60

6th

F

e133

9th data block 1-5

1st

I

Table ID for e113

6-10

2nd

I

Table ID for e223

11-15

3rd

I

Table ID for e333

16-20

4th

I

Table ID for e123

21-25

5th

I

Table ID for e233

26-30

6th

I

Table ID for e133

10th data block 1-10

1st

F

ε11 Electric permittivity.

11-20

2nd

F

ε22 Electric permittivity.

21-30

3rd

F

ε33 Electric permittivity.

11th data block 1-5

1st

I

Table ID for ε11 Electric permittivity.

6-10

2nd

I

Table ID for ε22 Electric permittivity.

11-15

3rd

I

Table ID for ε33 Electric permittivity.

12th data block Enter a list of elements associated with this material.

Main Index

1266 PIEZOELECTRIC (Piezoelectric - Model Definition) Define Electrical Data for Piezoelectric Analysis

PIEZOELECTRIC (Piezoelectric - Define Electrical Data for Piezoelectric Analysis Model Definition) The information provided here is based upon not using the table driven input style. Description This option allows you to specify the coupled electric-mechanical (stress based or strain based) properties eijk, and the electric properties εi for piezoelectric material. A description of the piezoelectric capabilities is included in Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PIEZOELECTRIC.

2nd data block 1-5

1st

I

Enter the number of sets of piezoelectric material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 8 are repeated as a set; once for each set of piezoelectric material to be input. 3rd data block 1-5

1st

I

Material identification number (1,2,3,etc) for cross-reference to the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC option.

6-10

2nd

I

Flag to indicate if the piezoelectric coupling matrix and the dielectric matrix is stress based or strain based. Enter 0 for stress based, and a 1 for strain based data.

4th data block

Main Index

1-10

1st

F

e111

11-20

2nd

F

e221

21-30

3rd

F

e331

31-40

4th

F

e121

41-50

5th

F

e231

51-60

6th

F

e131

PIEZOELECTRIC (Piezoelectric - Model Definition) 1267 Define Electrical Data for Piezoelectric Analysis

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

e112

11-20

2nd

F

e222

21-30

3rd

F

e332

31-40

4th

F

e122

41-50

5th

F

e232

51-60

6th

F

e132

6th data block 1-10

1st

F

e113

11-20

2nd

F

e223

21-30

3rd

F

e333

31-40

4th

F

e123

41-50

5th

F

e233

51-60

6th

F

e133

7th data block 1-10

1st

F

ε11 Electric permittivity.

11-20

2nd

F

ε22 Electric permittivity.

21-30

3rd

F

ε33 Electric permittivity.

8th data block Enter a list of elements associated with this material.

Main Index

1268 PIEZOELECTRIC (Piezoelectric - Model Definition) Define Electrical Data for Piezoelectric Analysis

Main Index

Chapter 3: Model Definition Options 1269 Magnetostatic Analysis

Chapt Magnetostatic Analysis er 3: This section describes the input of material data and boundary conditions applicable for magnetostatic problems. The ISOTROPIC and ORTHOTROPIC options are used to define magnetic permeability in Mode magnetostatic analysis. The variation of magnetic permeability with either magnetic field density or magnetic field vector can be prescribed by the B-H RELATION option where the magnetic field intensity l (H) is a function of the magnetic induction (B) with B being the independent variable. This variation of Defini the magnetic permeability can also be described using the table driven option. Then, either the magnetic induction (B) or the magnetic field intensity (H) can be chosen as the independent variable. A steady state tion solution can be obtained in one increment using the STEADY STATE option. In addition, the FLUX user Optio subroutine can be used for variable distributions of currents; the UMU user subroutine can be used for anisotropic magnetic permeabilities. ns

Main Index

1270 FIXED MG-POT (with TABLE Input - Magnetostatic) Define Fixed Potential

FIXED MG-POT (with TABLE Input - Magnetostatic)

Define Fixed Potential

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. In 2-D magnetostatic analysis, a scalar potential is used; hence, only one degree of freedom. In 3-D magnetostatic analysis, a vector potential is used. The fixed potential is associated with a boundary condition name that is activated with the LOADCASE history definition. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED MG-POT.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3th data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

FIXED MG-POT (with TABLE Input - Magnetostatic) 1271 Define Fixed Potential

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11 Element-Edges IDs

Main Index

1272 FIXED MG-POT (with TABLE Input - Magnetostatic) Define Fixed Potential

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED MG-POT (Magnetostatic) 1273 Define Nodal Fixed Potential

FIXED MG-POT (Magnetostatic)

Define Nodal Fixed Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each node must take during the first and subsequent increments. The boundary conditions are specified either by giving the potential and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

2nd data block 1-5

1st

I

Number of sets of boundary condition data blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly.

For each set of boundary conditions, use the 3a and 4a data blocks, or the 3b, 4b, and 5b data blocks. Data blocks 3a and 4a are used for analyses which are planar or axisymmetric. 3a data block 1-10

1st

F

Prescribed potential φ.

4a data block Enter a list of nodes for which the above potential is applied. Data blocks 3b, 4b, and 5b are used for analyses which include solid brick or shell elements.

Main Index

1274 FIXED MG-POT (Magnetostatic) Define Nodal Fixed Potential

Format Fixed

Free

Data Entry Entry

3b data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 4b.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 4b.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 4b. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

4b data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above boundary conditions are applied.

Main Index

FIXED POTENTIAL (with TABLE Input - Magnetostatic) 1275 Define Fixed Potential

FIXED POTENTIAL (with TABLE Input Magnetostatic)

Define Fixed Potential

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. In 2-D magnetostatic analysis, a scalar potential is used; hence, only one degree of freedom. In 3-D magnetostatic analysis, a vector potential is used. The fixed potential is associated with a boundary condition name that is activated with the LOADCASE history definition. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3th data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

1276 FIXED POTENTIAL (with TABLE Input - Magnetostatic) Define Fixed Potential

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

Main Index

1st

I

Enter the geometry type: 1:

Element IDs

2:

Nodes IDs

3:

Volume/Region/Body IDs

4:

Surface IDs

5:

Curve IDs

6:

Point IDs

11

Element-Edges IDs

FIXED POTENTIAL (with TABLE Input - Magnetostatic) 1277 Define Fixed Potential

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

1278 FIXED POTENTIAL (Magnetostatic) Define Nodal Fixed Potential

FIXED POTENTIAL (Magnetostatic)

Define Nodal Fixed Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each node must take during the first and subsequent increments. The boundary conditions are specified either by giving the potential and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

2nd data block 1-5

1st

I

Number of sets of boundary condition data blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data lines are required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly.

For each set of boundary conditions, use the 3a and 4a data blocks, or the 3b, 4b, and 5b data blocks. Data blocks 3a and 4a are used for analyses which are planar or axisymmetric. 3a data block 1-10

1st

F

Prescribed potential φ.

4a data block Enter a list of nodes for which the above potential is applied. Data blocks 3b, 4b, and 5b are used for analyses which include solid brick or shell elements.

Main Index

FIXED POTENTIAL (Magnetostatic) 1279 Define Nodal Fixed Potential

Format Fixed

Free

Data Entry Entry

3b data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 4b.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 4b.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 4b. (See Marc Volume B: Element Library for the definition of nodal degrees of freedom.)

4b data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5b data block Enter a list of nodes for which the above boundary conditions are applied.

Main Index

1280 DIST CURRENT (with TABLE Input - Magnetostatic) Define Distributed Currents

DIST CURRENT (with TABLE Input Magnetostatic)

Define Distributed Currents

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current on a particular face. Either the FLUX user subroutine(2D), the FORCEM user subroutine (3-D), or the TABLE model definition option can be used to input time and spatial dependent currents. The applied current is associated with a boundary condition name that is activated with the LOADCASE history definition. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

Data blocks 3 through 7 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX (2-D) or the FORCEM (3-D) user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

DIST CURRENT (with TABLE Input - Magnetostatic) 1281 Define Distributed Currents

Format Fixed 31-63

Free 7th

Data Entry Entry A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of this type of distributed currents.

4th data block 1-10

1st

For load type 106 or 107, enter the magnitude of this type of distributed current in the first coordinate direction. 11-20

2nd

F

For load type 106 or 107, enter the magnitude of this type if distributed current in the second coordinate direction.

21-30

3rd

F

For load type 106 or 107, enter the magnitude of this type of distributed current in the third coordinate direction.

I

Enter the table ID associated with the distributed current.

5th data block 1-5

1st

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

11-15

3rd

I

Normal current

Enter the face ID or edge ID.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention

Main Index

1282 DIST CURRENT (with TABLE Input - Magnetostatic) Define Distributed Currents

Format Fixed

Free

Data Entry Entry 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

DIST CURRENT (Magnetostatic) 1283 Define Distributed Current

DIST CURRENT (Magnetostatic)

Define Distributed Current

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current of a particular face. The FLUX user subroutine can be used to input spatially dependent current. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element LIbrary.

6-15

2nd

E

Enter the magnitude of this type of distributed current.

16-20

3rd

I

Current index (current index is to be used in the FLUX user subroutine).

4th data block Enter a list of elements associated with the above distributed current.

Main Index

1284 POINT CURRENT (with TABLE Input - Magnetostatic) Define Nodal Point Current

POINT CURRENT (with TABLE Input Magnetostatic)

Define Nodal Point Current

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows total nodal point currents to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for spatially dependent or time dependent currents. The point current is associated with a boundary condition name that is activated with the LOADCASE history definition. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of point currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of point current data, defaults to input.

Data blocks 3 through 7 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

F

Magnitude of point current for first degree of freedom.

4th data block 1-10

Main Index

1st

POINT CURRENT (with TABLE Input - Magnetostatic) 1285 Define Nodal Point Current

Format

Data Entry Entry

Fixed

Free

11-20

2nd

F

Magnitude of point current for second degree of freedom (3-D elements only).

21-30

3rd

F

Magnitude of point current for third degree of freedom (3-D elements only).

5th data block 1-5

1st

I

Table ID for point current for first degree of freedom.

6-10

2nd

I

Table ID for point current for second degree of freedom (3-D elements only).

11-15

3rd

I

Table ID for point current for third degree of freedom (3-D elements only).

Data blocks 6 and 7 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

1286 POINT CURRENT (Magnetostatic) Define Nodal Point Current

POINT CURRENT (Magnetostatic)

Define Nodal Point Current

The information provided here is based upon not using the table driven input style. Description This option allows total nodal point current to be specified. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of point currents to be entered (optional).

6-10

2nd

I

Enter unit number of input of point current data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-10

1st

F

Magnitude of point current.

11-20

2nd

F

Magnitude of point current for second degree of freedom (3-D elements only).

21-30

3rd

F

Magnitude of point current for third degree of freedom (3-D elements only).

4th data block Enter a list of nodes to which the above nodal currents are applied.

Main Index

ISOTROPIC (with TABLE Input - Magnetostatic) 1287 Define Magnetic Properties for Isotropic Materials

ISOTROPIC (with TABLE Input Define Magnetic Properties for Isotropic Materials - Magnetostatic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define magnetic properties for isotropic materials. This can be done by entering one of the following properties: Method Required Data 1

Permeability possibly controlled by a table.

2

Inverse permeability possibly controlled by a table.

3

H-B relation where a table has to be given with B as the independent variable and H as the dependent variable.

4

B-H relation where a table has to be given with H as the independent variable and B as the dependent variable.

You can also associate these material properties with a list of element numbers. Format

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 are repeated for each data set. 3rd data block

Main Index

1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Enter 1 to call the UMU and ORIENT user subroutines.

1288 ISOTROPIC (with TABLE Input - Magnetostatic) Define Magnetic Properties for Isotropic Materials

11-15

3rd

I

Input Mode: Enter 0 for Marc 2005 style or older with table driven input. Enter 1 if permeability is defined. Enter 2 if inverse permeability is defined. Enter 3 if H-B relation with B as the independent variable is defined; a table is also required. Enter 4 if B-H relation with H as the independent variable is defined; a table is also required.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

F

If input mode = 0 or 1, enter permeability.

4th data block 1-10

1st

If input mode = 2, enter inverse permeability. If input mode = 3, enter scale factor for H-B relation. If input mode = 4, enter scale factor for B-H relation. 11-20

2nd

F

If input mode = 0, enter inverse permeability.

I

If input mode = 0 or 1, enter table ID for permeability.

5th data block 1-5

1st

If input mode = 2, enter table ID inverse permeability. If input mode = 3, enter table ID for B-H relation; H is the independent variable. If input mode = 4, enter table ID for H-B relation; B is the independent variable. 6-10

2nd

I

If input mode = 0, enter table ID inverse permeability.

6th data block Enter a list of elements associated with this material.

Main Index

ISOTROPIC (Magnetostatic) 1289 Define Magnetic Properties for Isotropic Materials

ISOTROPIC (Magnetostatic)

Define Magnetic Properties for Isotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define magnetic properties for isotropic materials. You can also associate these material properties with a list of element numbers. Note that either the permeability or its inverse can be entered. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3, 4, and 5 are repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Enter 1 to call the UMU and ORIENT user subroutines.

4th data block 1-10

1st

F

Permeability.

11-20

2nd

F

Inverse permeability.

5th data block Enter a list of elements associated with this material.

Main Index

1290 ORTHOTROPIC (with TABLE Input - Magnetostatic) Define Magnetic Properties for Orthotropic Materials

ORTHOTROPIC (with TABLE Define Magnetic Properties for Orthotropic Materials Input - Magnetostatic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows you to define magnetic properties for an orthotropic material. This can be done by entering one of the following properties in each direction: Method Required Data 1

Permeability possibly controlled by a table.

2

Inverse permeability possibly controlled by a table.

3

H-B relation where a table has to be given with B as the independent variable and H as the dependent variable.

4

B-H relation where a table has to be given with H as the independent variable and B as the dependent variable.

You can also associate these material properties with a list of element numbers. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPI.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 are repeated for each data set. 3rd data block

Main Index

ORTHOTROPIC (with TABLE Input - Magnetostatic) 1291 Define Magnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Enter 1 to call the UMU and ORIENT user subroutines.

11-15

3rd

I

Input Mode (1st component): Enter 0 for Marc 2005 style or older with table driven input. Enter 1 for permeability. Enter 2 for inverse permeability Enter 3 for H-B relation with B as the independent variable; a table is also required. Enter 4 for B-H relation with H as the independent variable; a table is also required.

16-20

4th

I

Input Mode (2nd component): Enter 0 for Marc 2005 style or older with table driven input. Enter 1 for permeability. Enter 2 for inverse permeability. Enter 3 for H-B relation with B as the independent variable; a table is also required. Enter 4 for B-H relation with H as the independent variable; a table is also required.

21-25

5th

I

Input Mode (3rd component): Enter 0 for Marc 2005 style or older with table driven input. Enter 1 for permeability. Enter 2 for inverse permeability. Enter 3 for H-B relation with B as the independent variable; a table is also required. Enter 4 for B-H relation with H as the independent variable; a table is also required.

26-37

6th

A

Enter the material name to cross-reference with material database for temperature dependent properties.

4a data block Use if the input modes for all components are zero.

Main Index

1-10

1st

F

μ11

Magnetic permeability.

11-20

2nd

F

μ22

Magnetic permeability.

1292 ORTHOTROPIC (with TABLE Input - Magnetostatic) Define Magnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

μ33

31-40

4th

F

1/μ11 Inverse magnetic permeability.

41-50

5th

F

1/μ22 Inverse magnetic permeability.

51-60

6th

F

1/μ33 Inverse magnetic permeability.

Magnetic permeability.

4b data block Use if the input modes are not zero. 1-10

1st

F

Data for 1st component: Method 1; enter μ11 (magnetic permeability). Method 2; enter 1/μ11 (inverse magnetic permeability). Method 3; enter scale factor for H-B relation. Method 4; enter scale factor for B-H relation.

11-20

2nd

F

Data for 2nd component: Method 1; enter μ22 (Magnetic permeability). Method 2; enter 1/μ22 (inverse magnetic permeability). Method 3; enter scale factor for H-B relation. Method 4; enter scale factor for B-H relation.

21-30

3rd

F

Data for 3rd component: Method 1; enter μ33 (magnetic permeability). Method 2; enter 1/μ33 (inverse magnetic permeability). Method 3; enter scale factor for H-B relation. Method 4; enter scale factor for B-H relation.

5a data block Use if the input modes for all components are zero.

Main Index

1-5

1st

I

Table ID for μ11

6-10

2nd

I

Table ID for μ22.

11-15

3rd

I

Table ID for μ33.

16-20

4th

I

Table ID for 1/μ11.

21-25

5th

I

Table ID for 1/μ22.

26-30

6th

I

Table ID for 1/μ33.

ORTHOTROPIC (with TABLE Input - Magnetostatic) 1293 Define Magnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

5b data block Use if the input modes are not zero. 1-5

1st

I

Table IDs for 1st component: Method 1; table ID for μ11. Method 2; table ID for 1/μ11. Method 3; table ID for H-B relation; B is the independent variable. Method 4; table ID for B-H relation; H is the independent variable.

6-10

2nd

I

Table IDs for 2nd component: Method 1; table ID for μ22. Method 2; table ID for 1/μ22. Method 3; table ID for H-B relation; B is the independent variable. Method 4; table ID for B-H relation; H is the independent variable.

11-15

3rd

I

Table IDs for 3rd component: Method 1; table ID for μ33. Method 2; table ID for 1/μ33 Method 3; table ID for H-B relation; B is the independent variable. Method 4; table ID for B-H relation; H is the independent variable.

6th data block Enter a list of elements associated with this material.

Main Index

1294 ORTHOTROPIC (Magnetostatic) Define Magnetic Properties for Orthotropic Materials

ORTHOTROPIC (Magnetostatic)

Define Magnetic Properties for Orthotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define magnetic properties for an orthotropic material. You can also associate these material properties with a list of element numbers. Note that either the permeability or the inverse permittivity can be entered. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 8 are repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Enter 1 to call the UMU and ORIENT user subroutines.

4th data block

Main Index

1-10

1st

F

μ11

Magnetic permeability

11-20

2nd

F

μ22

Magnetic permeability

21-30

3rd

F

μ33

Magnetic permeability

ORTHOTROPIC (Magnetostatic) 1295 Define Magnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

31-40

4th

F

1/μ11 Inverse magnetic permeability

41-50

5th

F

1/μ22 Inverse magnetic permeability

51-60

6th

F

1/μ22 Inverse magnetic permeability

5th data block Enter a list of elements associated with this material.

Main Index

1296 B-H RELATION (Magnetostatic) Define Magnetization Curve for Nonlinear Magnetic Material

B-H RELATION (Magnetostatic)

Define Magnetization Curve for Nonlinear Magnetic Material

Description This option can be used to specify the magnetization curve(s) for nonlinear isotropic or orthotropic material. Depending on the material type, a different method of entering data must be used: isotropic material: (OPTION A)

Enter one set of data points (|H|, |B|) representing the magnitude of H as a function of the magnitude of B. For |H| = 0 the value of |B| should be zero. If not, the corresponding offset of the curve is disregarded.

orthotropic material: (OPTION B)

For every component of H, a set of data points (H,B) is entered, relating this component of H to the corresponding component of B. A component of the remanence vector can be specified by choosing a nonzero value of B for H = 0.

Note:

In either cases the curve(s) represented by the data sets must be monotone and uniquely defined. Furthermore, the data points must be given in ascending order of B.

An alternative way of specifying the magnetization curve(s) is to supply the reluctivity 1/μ in the UMU user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words B-H RELATION.

For option A, use data blocks 2a, 3a, 4a, and 5a. For option B, use data blocks 2b, 3b, 4b, and 5b. Option A — Isotropic Behavior 2a data block

Main Index

1-5

1st

I

Number of data points of |H|-|B| curve.

6-10

2nd

I

Not used; 0.

11-15

3rd

I

Not used; 0.

16-20

4th

I

Not used; 0.

21-25

5th

I

Not used; 0.

26-30

6th

I

Not used; 0.

B-H RELATION (Magnetostatic) 1297 Define Magnetization Curve for Nonlinear Magnetic Material

Format Fixed 31-35

Free 7th

Data Entry Entry I

Material type identification (1,2,3...) for cross-reference to ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data blocks.

3a data block |H| - |B| variation. Number of blocks as given on data block 2, first field. 1-15

1st

F

Enter value of |H|.

16-30

2nd

F

Enter value of |B|.

Option B — Orthotropic Behavior 2b data block 1-5

1st

I

Number of data points of H1 - B1 curve.

6-10

2nd

I

Number of data points of H2 - B2 curve.

11-15

3rdt

I

Number of data points of H3 - B3 curve.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-35

7th

I

Material type identification (1,2,3...) for cross-reference to ORTHOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data blocks.

3b data block H1 - B1 variation. Number of blocks given on data block 2, first field. 1-15

1st

F

Enter value of H1.

16-30

2nd

F

Enter value of B1.

4b data block H2 - B2 variation. Number of blocks given on data block 2, second field. 1-15

1st

F

Enter value of H2.

16-30

2nd

F

Enter value of B2.

5b data block H3 - B3 variation. Number of blocks given on data block 2, third field.

Main Index

1-15

1st

F

Enter value of H3.

16-30

2nd

F

Enter value of B3.

1298 PERMANENT (with TABLE Input - Magnetostatic) Define Permanent Magnet

PERMANENT (with TABLE Input - Magnetostatic) Define Permanent Magnet The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides various ways of defining a permanent magnet in parts of the model. The default is that no permanent magnets are present. You need to enter the remanence vector Br, which is the product of the magnet vector M0 and the permeability of the vacuum μ0. The permanent magnet data is associated with a boundary condition name that is activated with the LOADCASE model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PERMANENT.

2nd data block 1-5

1st

I

Number of sets of data to be entered (optional)

6-10

2nd

I

Unit number for input. Defaults to input file.

Data blocks 3 through 7 are repeated once for each data set. 3rd data block

Main Index

1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter zero.

11-15

3rd

I

Not used; enter zero.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

PERMANENT (with TABLE Input - Magnetostatic) 1299 Define Permanent Magnet

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Enter the first component of remanence vector.

11-20

2nd

F

Enter the second component of remanence vector.

21-30

3rd

F

Enter the third component of remanence vector.

5th data block 1-5

1st

F

Table ID associated with the first component of remanence vector.

6-10

2nd

F

Table ID associated with the second component of remanence vector.

11-15

3rd

F

Table ID associated with the third component of remanence vector.

Data blocks 6 and 7 are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1 – Element IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

1300 PERMANENT (Magnetostatic) Define Permanent Magnet

PERMANENT (Magnetostatic)

Define Permanent Magnet

The information provided here is based upon not using the table driven input style. Description This option provides various ways of defining a permanent magnet in parts of the model. The default is that no permanent magnets are present. You need to enter the remanence vector Br, which is the product of the magnet vector M0 and the permeability of the vacuum μ0. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the word PERMANENT.

2nd data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter 1 to initialize the permanent magnet via data blocks 3 and 4 below. See also the third field on this block. Enter 4 to initialize the permanent magnet via data blocks 5, 6, 7, and 8 given below. See also the third field on this block.

11-15

3rd

I

This entry gives the number of pairs of bocks in data blocks 3 and 4 or in data blocks 5, 6, 7, and 8 used to input the permanent magnet.

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of blocks is equal to the number given in the third field above. 3rd data block

Main Index

1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with the value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value.

21-25

5th

I

First layer of cross section point with this value.

26-30

6th

I

Last layer or cross section point with this value can only be bigger than 1 for beam or shell elements.

PERMANENT (Magnetostatic) 1301 Define Permanent Magnet

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

First component of remanence vector.

11-20

2nd

F

Second component of remanence vector.

21-30

3rd

F

Third component of remanence vector.

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

First component of remanence vector.

11-20

2nd

F

Second component of remanence vector.

21-30

3rd

F

Third component of remanence vector.

6th data block Enter a list of elements to which the above state variable is applied. 7th data block This data block is not necessary if CENTROID parameter is used. Enter a list of integration points to which the above remanence is applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above remanence is applied.

Main Index

1302 CONTROL (Magnetostatic) Control for Magnetostatic Analysis

CONTROL (Magnetostatic)

Control for Magnetostatic Analysis

Description This option allows you to input parameters governing the convergence and accuracy for magnetostatic analysis. This option is only required if the B-H RELATION option is used to enter a nonlinear permeability. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of steps in this run. Default is 9999.

6-10

2nd

I

Maximum number of recycles during an increment. Default is 3.

11-15

3rd

I

Minimum number of recycles during an increment.

3rd data block

Main Index

1-10

1st

F

Maximum allowed relative error in residual current.

11-20

2nd

F

Maximum allowed absolute error in residual current.

Chapter 3: Model Definition Options 1303 Electromagnetic Analysis

Chapt Electromagnetic Analysis er 3: This section describes the input of material data and boundary conditions applicable for electromagnetic problems. The ISOTROPIC and ORTHOTROPIC options are used to define magnetic permeability, Mode electrical permittivity, conductivity and susceptibility in the electromagnetic analysis. In addition, the FORCEM user subroutine can be used for variable distributions of currents and charges. l Defini Electromagnetic analysis can be performed using either a harmonic or transient approach. If the harmonic approach is used, the steady state sinusoidal result is obtained. Using this method, the excitation tion frequency is given using the HARMONIC option. If the transient approach is used, the time step is defined Optio using the DYNAMIC CHANGE option. ns

Main Index

1304 FIXED POTENTIAL (with TABLE Input - Electromagnetic) Define Fixed Potential

FIXED POTENTIAL (with TABLE Input Electromagnetic)

Define Fixed Potential

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option defines the fixed potential that each node must take. The boundary conditions are specified either by giving the potential and either a list of nodal numbers, or a list of surfaces. In electromagnetic analysis, the potential consists of vector and scalar potentials, the first three of which are associated with the magnetic vector potential, and the fourth degree of freedom with the scalar potential. The prescribed potential is associated with a boundary condition name that is activated with the LOADCASE history definition.

The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time dependent boundary conditions. The FORCDF user subroutine or the TABLE model definition option can be used to enter frequency dependent boundary conditions in a harmonic electromagnetic analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

I

Number of sets of boundary conditions to be read (optional).

2nd data block 1-5

1st

6-10

2nd

Unit number to read data, default is the standard input file.

Data blocks 3 through 10 are repeated for each set. 3a data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers.

Main Index

FIXED POTENTIAL (with TABLE Input - Electromagnetic) 1305 Define Fixed Potential

Format Fixed

Free

Data Entry Entry Enter 2 if complex value given as magnitude and phase.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

4th data block 1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 6.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 6.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 6.

31-40

4th

F

Prescribed potential for fourth degree of freedom listed in data block 6.

5th data block 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

16-20

4th

I

Enter the table ID for the fourth degree of freedom listed.

The 6th and 7th data blocks are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of potential or the phase of the first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed imaginary component of potential or the phase of the second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed imaginary component of potential or the phase of the third degree of freedom listed in data block 8.

31-40

4th

E

Prescribed imaginary component of potential or the phase of the fourth degree of freedom listed in data block 8.

7th data block - Table IDs for Imaginary Component or Phase Angle

Main Index

1-5

1st

I

Enter the table ID for imaginary component or phase for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for imaginary component or phase for the second degree of freedom listed.

1306 FIXED POTENTIAL (with TABLE Input - Electromagnetic) Define Fixed Potential

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Enter the table ID for imaginary component or phase for the third degree of freedom listed.

16-20

4th

I

Enter the table ID for imaginary component or phase for the fourth degree of freedom listed.

8th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

The 9th and 10th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11 Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces ID - Marc Mentat convention

10th data block Enter a list of geometric entities for which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED POTENTIAL (Electromagnetic) 1307 Define Nodal Fixed Potential

FIXED POTENTIAL (Electromagnetic)

Define Nodal Fixed Potential

The information provided here is based upon not using the table driven input style. Description This option defines the fixed potential that each node must take during the first and subsequent increments. The boundary conditions are specified either by giving the potential and a list of nodal numbers, or by the input of boundary conditions generated during mesh generation (MESH2D). In electromagnetic analysis, the potential consists of vector and scalar potentials, the first three of which are associated with the magnetic vector potential, and the fourth degree of freedom with the scalar potential. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words FIXED POTENTIAL.

2nd data block 1-5

1st

I

Number of sets of boundary condition blocks to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further blocks are required in this option block.

11-15

3rd

I

Unit number used for the MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition options must be arranged accordingly.

Data blocks 3, 4, and 5 are repeated for each set. 3rd data block

Main Index

1-10

1st

F

Prescribed potential for first degree of freedom listed in data block 4.

11-20

2nd

F

Prescribed potential for second degree of freedom listed in data block 4.

21-30

3rd

F

Prescribed potential for third degree of freedom listed in data block 4.

31-40

4th

F

Prescribed potential for fourth degree of freedom list in data block 4.

1308 FIXED POTENTIAL (Electromagnetic) Define Nodal Fixed Potential

Format Fixed

Free

Data Entry Entry

4th data block Enter a list of degrees of freedom to which the above prescribed potentials are given. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes for which the above boundary conditions are applied.

Main Index

DIST CURRENT (with TABLE Input - Electromagnetic) 1309 Define Distributed Currents

DIST CURRENT (with TABLE Input Electromagnetic)

Define Distributed Currents

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time and spatial dependent currents. The applied current is associated with a boundary condition name that is activated with the LOADCASE history definition. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

Data blocks 3 through 10 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

Main Index

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

1310 DIST CURRENT (with TABLE Input - Electromagnetic) Define Distributed Currents

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of this type of distributed currents.

I

Enter the table ID associated with the distributed current.

4th data block 1-10

1st

5th data block 1-5

1st

Data blocks 6 and 7 are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of the distributed current or the phase.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component of the distributed current or the phase.

8th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

11-15

3rd

I

Normal current

Enter the face ID or edge ID.

Data blocks 9 and 10 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 9th data block 1-5

1st

I

Enter the geometry type: 1:

Element IDs

3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs

Main Index

DIST CURRENT (with TABLE Input - Electromagnetic) 1311 Define Distributed Currents

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

10th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 9th data block.

1312 DIST CURRENT (Electromagnetic - Model Definition) Define Distributed Currents

DIST CURRENT (Electromagnetic - Model Definition)

Define Distributed Currents

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current of a particular face. The FORCEM user subroutine can be used to input spatially dependent current. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, repeated for each data set. 3rd data block 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed current.

16-20

3rd

I

Current index (current index is to be used in the FORCEM user subroutine).

4th data block Enter a list of elements associated with the above distributed current.

Main Index

DIST CHARGES (with TABLE Input - Electromagnetic) 1313 Define Distributed Charges

DIST CHARGES (with TABLE Input Electromagnetic)

Define Distributed Charges

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface flux on a particular face. Either the FLUX user subroutine or the TABLE model definition option can be used to input time, frequency, and spatial dependent charges. The prescribed charge is associated with a boundary condition name that is activated with the LOADCASE history definition. Note:

If a distributed charge is applied on the bottom of a shell, the charge is applied to the highest degrees of freedom of the shell.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

Data blocks 3 through 10 are given for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

11-15

3rd

I

Enter 0 if real value given. Enter 1 if complex value given as real and imaginary numbers. Enter 2 if complex value given as magnitude and phase.

16-20

Main Index

4th

I

Not used; enter 0.

1314 DIST CHARGES (with TABLE Input - Electromagnetic) Define Distributed Charges

Format Fixed

Free

Data Entry Entry

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

F

Enter the magnitude of the distributed charges.

I

Enter the table ID associated with the distributed charge.

4th data block 1-10

1st

5th data block 1-5

1st

Data blocks 6 and 7 are only required if a complex harmonic boundary condition. 6th data block - Imaginary Component or Phase Angle 1-10

1st

E

Prescribed imaginary component of the distributed charge or the phase.

7th data block - Table IDs for Imaginary Component or Phase Angle 1-5

1st

I

Enter the table ID for imaginary component of the distributed charge or the phase.

8th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B: Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1: Normal charge (bottom surface for shells) 10: Normal charge (top surface for shells)

11-15

3rd

I

Enter the face ID or edge ID.

Data blocks 9 and 10 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs

Main Index

DIST CHARGES (with TABLE Input - Electromagnetic) 1315 Define Distributed Charges

Format Fixed

Free

Data Entry Entry 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

10th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

1316 DIST CHARGE (Electromagnetic - Model Definition) Define Distributed Charges

DIST CHARGE (Electromagnetic - Model Definition)

Define Distributed Charges

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface charge on a particular face. The FORCEM user subroutine can be used to input spatially dependent charges. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGE.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed charge data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, repeated for each data set. 3rd data block 1-5

1st

I

Parameter identifying the type of distributed charge. See description of library element in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed charges.

16-20

3rd

I

Charge index (optional). Charge index is to be used in the FORCEM user subroutine.

4th data block Enter a list of elements associated with the above distributed charges.

Main Index

POINT CURRENT-CHARGE (with TABLE Input - Electromagnetic) 1317 Define Point Fluxes

POINT CURRENT-CHARGE (with TABLE Input Electromagnetic)

Define Point Fluxes

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows total nodal point fluxes to be specified. Either the FORCDT user subroutine or the TABLE model definition option can be used for the time dependent fluxes. The FORCDF user subroutine or the TABLE model definition option can be used to enter frequency dependent boundary conditions in a harmonic electromagnetic analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of point fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point flux data, defaults to input.

Data blocks 3 through 6 are given in sets. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT or FORCDF user subroutine required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1318 POINT CURRENT-CHARGE (with TABLE Input - Electromagnetic) Define Point Fluxes

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

Magnitude of point current for first degree of freedom.

11-20

2nd

F

Magnitude of point current for second degree of freedom.

21-30

3rd

F

Magnitude of point current for third degree of freedom.

31-40

4th

F

Magnitude of point current for fourth degree of freedom.

5th data block 1-5

1st

I

Table ID for point current for first degree of freedom.

6-10

2nd

I

Table ID for point current for second degree of freedom.

11-15

3rd

I

Table ID for point current for third degree of freedom.

16-20

4th

I

Table ID for point charge.

Data blocks 6 and 7 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1:

Element IDs

2:

Nodes IDs

3:

Volume/Region/Body IDs

4:

Surface IDs

5:

Curve IDs

6:

Point IDs

11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 7th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

POINT CURRENT-CHARGE 1319 Define Nodal Point Currents and Point Charges

POINT CURRENT-CHARGE

Define Nodal Point Currents and Point Charges

The information provided here is based upon not using the table driven input style. Description This option allows nodal point currents and point charges to be specified. The FORCDT user subroutine can be used for nonuniform loading conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CURRENT-CHARGE.

2nd data block 1-5

1st

I

Enter number of sets of point current and charge to be entered (optional).

6-10

2nd

I

Enter unit number for input of point current and charge data; defaults to input.

The 3rd and 4th data blocks should be entered as pairs and repeated for each data set. 3rd data block 1-10

1st

F

Magnitude of point current for first degree of freedom.

11-20

2nd

F

Magnitude of point current for second degree of freedom.

21-30

3rd

F

Magnitude of point current for third degree of freedom.

31-40

4th

F

Nodal charge.

4th data block Enter a list of nodes to which the above point current-charge applies.

Main Index

1320 ISOTROPIC (with TABLE Input - Electromagnetic) Define Electromagnetic Properties for Isotropic Materials

ISOTROPIC (with TABLE Define Electromagnetic Properties for Isotropic Materials Input - Electromagnetic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define electromagnetic properties for an isotropic material. You can also associate these material properties with a list of element numbers. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 6 should be entered as pairs and repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

4th data block Necessary only in coupled electromagnetic-thermal analysis.

Main Index

1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Emissivity.

ISOTROPIC (with TABLE Input - Electromagnetic) 1321 Define Electromagnetic Properties for Isotropic Materials

Format Fixed

Free

Data Entry Entry

5th data block Necessary only in coupled electromagnetic-thermal analysis. 1-10

1st

I

Table ID for thermal conductivity.

11-20

2nd

I

Table ID for specific heat.

21-30

3rd

I

Table ID for mass density.

31-40

4th

I

Not used; enter 0.

41-50

5th

I

Table ID for emissivity.

6th data block 1-10

1st

F

Permeability (μ).

11-20

2nd

F

Permittivity (ε).

21-30

3rd

F

Permeability of air.

31-40

4th

F

Electric conductivity (σ).

7th data block 1-5

1st

I

Table ID for permeability.

6-10

2nd

I

Table ID for permittivity.

11-15

3rd

I

Table ID for permeability of air.

16-20

4th

I

Table ID for electric conductivity.

8th data block Enter a list of elements associated with this material.

Main Index

1322 ISOTROPIC (Electromagnetic) Define Electromagnetic Properties for Isotropic Materials

ISOTROPIC (Electromagnetic)

Define Electromagnetic Properties for Isotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define electromagnetic properties for an isotropic material. You can also associate these material properties with a list of element numbers. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of isotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

The 3rd, 4th, and 5th data blocks should be entered as pairs and repeated for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

4th data block Necessary only in coupled electromagnetic-thermal analysis.

Main Index

1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Emissivity.

ISOTROPIC (Electromagnetic) 1323 Define Electromagnetic Properties for Isotropic Materials

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

Permeability (μ).

11-20

2nd

F

Permittivity (ε).

21-30

3rd

F

Permeability of air.

31-40

4th

F

Electric conductivity (σ).

6th data block Enter a list of elements associated with this material.

Main Index

1324 ORTHOTROPIC (with TABLE Input - Electromagnetic) Define Electromagnetic Properties for Orthotropic Materials

ORTHOTROPIC (with Define Electromagnetic Properties for Orthotropic Materials TABLE Input Electromagnetic) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option allows you to define electrical properties for an orthotropic material. You can also associate these material properties with a list of element numbers. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPI.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow (optional).

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3 through 12 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.).

6-10

2nd

I

Enter 1 to call the UEPS and ORIENT user subroutines.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Data input mode; enter 0.

21-25

5th

I

Not used; enter 0.

26-37

6th

A

Enter the material name to cross-reference with material database.

Data blocks 4 through 7 are only necessary in coupled electromagnetic-thermal analysis.

Main Index

ORTHOTROPIC (with TABLE Input - Electromagnetic) 1325 Define Electromagnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

K11

Thermal conductivities.

11-20

2nd

F

K22

Thermal conductivities.

21-30

3rd

F

K33

Thermal conductivities.

31-40

4th

F

ρ

Mass density.

41-50

5th

F

Specific heat per unit mass.

5th data block 1-5

1st

I

Table ID for K11.

6-10

2nd

I

Table ID for K22.

11-15

3rd

I

Table ID for K33.

16-20

4th

I

Table ID for mass density.

21-25

5th

I

Table ID for specific heat.

6th data block Only required if RADIATION parameter is present or version is greater or equal to 10. 1-10

1st

F

Emissivity (for radiation case).

11-20

2nd

F

Enter the enthalpy of formation.

21-30

3rd

F

Enter the reference temperature of enthalpy of formation.

7th data block Only required if RADIATION parameter is present or version is greater or equal to 10. 1-5

1st

I

Table ID for emissivity.

6-10

2nd

I

Table ID for enthalpy of formation.

11-15

3rd

I

Table ID for reference temperature of enthalpy of formation.

8th data block

Main Index

1-10

1st

F

μ11 Magnetic permeability

1-20

2nd

F

μ22 Magnetic permeability

21-30

3rd

F

μ33 Magnetic permeability

31-40

4th

F

ε11 Permittivity

1-50

5th

F

ε22 Permittivity

51-60

6th

F

ε33 Permittivity

61-70

7th

F

Permeability of air

1326 ORTHOTROPIC (with TABLE Input - Electromagnetic) Define Electromagnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

9th data block 1-10

1st

I

Table ID for μ11 magnetic permeability

1-20

2nd

I

Table ID for μ22 magnetic permeability

21-30

3rd

I

Table ID for μ33 magnetic permeability

31-40

4th

I

Table ID for ε11 permittivity

41-50

5th

I

Table ID for ε22 permittivity

51-60

6th

I

Table ID for ε33 permittivity

61-70

7th

I

Table ID for permeability of air

1-10

F

σ11 Electrical Conductivity

11-20

F

σ22 Electrical Conductivity

21-30

F

σ33 Electrical Conductivity

1-10

I

Table ID for σ11 electrical Conductivity

11-20

I

Table ID for σ22 electrical Conductivity

21-30

I

Table ID for σ33 electrical Conductivity

10th data block

11th data block

12th data block Enter a list of elements associated with this material. (Do not enter composite elements which use this material in its layers.)

Main Index

ORTHOTROPIC (Electromagnetic) 1327 Define Electromagnetic Properties for Orthotropic Materials

ORTHOTROPIC (Electromagnetic)

Define Electromagnetic Properties for Orthotropic Materials

The information provided here is based upon not using the table driven input style. Description This option allows you to define electrical properties for an orthotropic material. You can also associate these material properties with a list of element numbers. Notes:

Since the material properties in an orthotropic material are independent, it is your responsibility to enter all data required to match the dimension of the conductivity matrix for the elements listed below. (See Marc Volume B: Element Library, if necessary). No defaults for this data are provided by Marc. These values are with respect to the user coordinate (1, 2, 3) system.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ORTHOTROPIC.

2nd data block 1-5

1st

I

Enter the number of sets of orthotropic material data to follow.

6-10

2nd

I

Enter the unit number for input. Defaults to input file.

Data blocks 3-8 are repeated once for each data set. 3rd data block 1-5

1st

I

Material identification number (1, 2, 3, etc.) for cross-reference to B-H RELATION option.

6-10

2nd

I

Enter 1 to call the UMU, UEPS, and USIGMA user subroutines.

4th data block Data blocks 4 and 5 are only necessary in coupled electromagnetic-thermal analysis.

Main Index

1-10

1st

F

K11

Thermal conductivities.

11-20

2nd

F

K22

Thermal conductivities.

1328 ORTHOTROPIC (Electromagnetic) Define Electromagnetic Properties for Orthotropic Materials

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

K33

Thermal conductivities.

31-40

4th

F

ρ

Mass density.

41-50

5th

F

Specific heat per unit mass.

5th data block Only required if RADIATION parameter is present or version is greater or equal to 10. 1-10

1st

F

Emissivity (for radiation case).

11-20

2nd

F

Enter the enthalpy of formation.

21-30

3rd

F

Enter the reference temperature of enthalpy of formation.

6th data block 1-10

1st

F

μ11 Magnetic permeability

1-20

2nd

F

μ22 Magnetic permeability

21-30

3rd

F

μ33 Magnetic permeability

31-40

4th

F

ε11 Permittivity

1-50

5th

F

ε22 Permittivity

51-60

6th

F

ε33 Permittivity

61-70

7th

F

Permeability of air

1-10

F

σ11 Electrical Conductivity

11-20

F

σ22 Electrical Conductivity

21-30

F

σ33 Electrical Conductivity

7th data block

8th data block Enter a list of elements associated with this material.

Main Index

B-H RELATION (Electromagnetic) 1329 Define Magnetization Curve for Nonlinear Magnetic Material

B-H RELATION (Electromagnetic)

Define Magnetization Curve for Nonlinear Magnetic Material

Description This option can be used to specify the magnetization curve(s) for nonlinear isotropic or orthotropic material. Depending on the material type, a different method of entering data must be used: isotropic material: (OPTION A)

Enter one set of data points (|H|, |B|) representing the magnitude of H as a function of the magnitude of B. For |H| = 0 the value of |B| should be zero. If not, the corresponding offset of the curve is disregarded.

orthotropic material: (OPTION B)

For every component of H, a set of data points (H,B) is entered, relating this component of H to the corresponding component of B. A component of the remanence vector can be specified by choosing a nonzero value of B for H = 0

Note:

In either case, the curve(s) represented by the data sets must be monotone and uniquely defined. Furthermore, the data points must be given in ascending order of B.

An alternative way of specifying the magnetization curve(s) is to supply the reluctivity 1/μ in the UMU user subroutine. This option is only applicable for transient electromagnetic analysis and is not applicable to harmonic calculations. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words B-H RELATION.

For option A, use data blocks 2a, 3a, 4a, and 5a. For option B, use data blocks 2b, 3b, 4b, and 5b. Option A — Isotropic Behavior 2a data block

Main Index

1-5

1st

I

Number of data points of |H|-|B| curve.

6-10

2nd

I

Not used; 0.

11-15

3rd

I

Not used; 0.

16-20

4th

I

Not used; 0.

21-25

5th

I

Not used; 0.

26-30

6th

I

Not used; 0.

1330 B-H RELATION (Electromagnetic) Define Magnetization Curve for Nonlinear Magnetic Material

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Material type identification (1,2,3...) for cross-reference to ISOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data blocks.

3a data block |H| - |B| variation. Number of blocks as given on data block 2, first field. 1-15

1st

F

Enter value of |H|.

16-30

2nd

F

Enter value of |B|.

Option B — Orthotropic Behavior 2b data block 1-5

1st

I

Number of data points of H1 - B1 curve.

6-10

2nd

I

Number of data points of H2 - B2 curve.

11-15

3rdt

I

Number of data points of H3 - B3 curve.

16-20

4th

I

Not used; enter zero.

21-25

5th

I

Not used; enter zero.

26-30

6th

I

Not used; enter zero.

31-35

7th

I

Material type identification (1,2,3...) for cross-reference to ORTHOTROPIC option.

36-40

8th

I

Logical unit number for input of this set of data. Defaults to data blocks.

3b data block H1 - B1 variation. Number of blocks given on data block 2, first field. 1-15

1st

F

Enter value of H1.

16-30

2nd

F

Enter value of B1.

4b data block H2 - B2 variation. Number of blocks given on data block 2, second field. 1-15

1st

F

Enter value of H2.

16-30

2nd

F

Enter value of B2.

5b data block H3 - B3 variation. Number of blocks given on data block 2, third field.

Main Index

1-15

1st

F

Enter value of H3.

16-30

2nd

F

Enter value of B3.

PERMANENT (Electromagnetic) 1331 Define Permanent Magnet

PERMANENT (Electromagnetic)

Define Permanent Magnet

The information provided here is based upon not using the table driven input style. Description This option provides various ways of defining a permanent magnet in parts of the model. The default is that no permanent magnets are present. You need to enter the remanence vector Bv, which is the product of the magnet vector M and the permeability of the vacuum μ0. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the word PERMANENT.

2nd data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter 1 to initialize the permanent magnet via data blocks 3 and 4 below. See also the third field on this block. Enter 4 to initialize the permanent magnet via data blocks 5, 6, 7, and 8 given below. See also the third field on this block.

11-15

3rd

I

This entry gives the number of pairs of blocks in data blocks 3 and 4 or in data blocks 5, 6, 7, and 8 used to input the permanent magnet.

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of blocks is equal to the number given in the third field above. 3rd data block

Main Index

1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with the value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value.

21-25

5th

I

First layer of cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value can only be bigger than 1 for beam or shell elements.

1332 PERMANENT (Electromagnetic) Define Permanent Magnet

Format Fixed

Free

Data Entry Entry

4th data block 1-10

1st

F

First component of remanence vector.

11-20

2nd

F

Second component of remanence vector.

21-30

3rd

F

Third component of remanence vector.

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

First component of remanence vector.

11-20

2nd

F

Second component of remanence vector.

21-30

3rd

F

Third component of remanence vector.

6th data block Enter a list of elements to which the above state variable is applied. 7th data block This data block is not necessary if CENTROID parameter is used. Enter a list of integration points to which the above remanence is applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above remanence is applied.

Main Index

CONTROL (Electromagnetostatic) 1333 Control for Electromagnetostatic Analysis

CONTROL (Electromagnetostatic)

Control for Electromagnetostatic Analysis

Description This option allows you to input parameters governing the convergence and accuracy for magnetostatic analysis. This option is only required if the B-H RELATION option is used to enter a nonlinear permeability. This option is only applicable for transient electromagnetic analysis and is not applicable to harmonic calculations. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of steps in this run. Default is 9999.

6-10

2nd

I

Maximum number of recycles during an increment. Default is 3.

11-15

3rd

I

Minimum number of recycles during an increment.

3rd data block

Main Index

1-10

1st

F

Maximum allowed relative error in residual current.

11-20

2nd

F

Maximum allowed absolute error in residual current.

1334 CONTROL (Electromagnetostatic) Control for Electromagnetostatic Analysis

Main Index

Chapter 3: Model Definition Options 1335 Fluid Analysis

Chapt Fluid Analysis er 3: This section describes the input of material data and boundary conditions applicable for fluid, fluidfluid-solid and fluid-thermal-solid interaction analyses. The ISOTROPIC option is used to Mode thermal, define the fluid material properties, viscosity, density, and, if necessary, the conductivity and specific heat. Non-Newtonian fluid behavior can be defined through the STRAIN RATE option, while temperature l dependent properties are defined through the TEMPERATURE EFFECTS option. The boundary Defini conditions on a fluid can be either defined through the FIXED VELOCITY, or the POINT LOAD, and DIST LOADS options. The POINT LOAD and DIST LOADS options are described in the Mechanical Analysis tion section. In a fluid-thermal analysis, the additional boundary conditions are FIXED TEMPERATURE, Optio POINT FLUX, DIST FLUXES, and FILMS which are defined in the Heat Transfer Analysis section. In a fluid-solid analysis, the boundary conditions on the solid region are specified using the FIXED DISP, ns POINT LOAD, DIST LOADS, and FOUNDATION options. Initial conditions in a transient analysis can be specified using the INITIAL VEL or INITIAL TEMP options. In Fluid Analysis, data for POINT LOAD and DIST LOADS should be prescribed as total rather than incremental quantity (as used in Mechanical Analysis). Similarly, POINT FLUX and DIST FLUXES for Heat Transfer Analysis are also given as total quantity. This specification is to be used consistently for fluid and/or heat transfer portion of analysis in coupled fluid-solid, fluid-thermal, and fluid-thermalsolid. Note the degrees of freedom in an analysis are dependent upon the type of analysis and the procedure used. This is important when applying boundary conditions in these analyses and is summarized as follows:

Fluid Parameter 2-D-planar 2-D-axisymmetric

Main Index

3-D

Fluid only, mixed

10

vx , vy , p

vz , vr , p

vx , vy , vz , p

Fluid only, penalty

11

vx , vy

vz , vr

vx , vy , vz

Fluid-thermal, mixed, strong coupling

12

vx , vy , p, T

vz , vr , p, T

vx , vy , vz , p, T

Fluid-thermal, penalty, strong coupling

13

vx , vy , T

vx , vr , T

vx , vy , vz , T

Fluid-thermal, mixed, weak coupling

2

vx , v y, p

vz , vr , p

vx , vy , vz , p

T

T

T

Fluid-thermal, penalty, weak coupling

3

vx , vy

vz , vr

vx , vy , vz

T

T

T

Fluid-solid, mixed, weak coupled

40

vx , vy , p

vz , vr , p

vx , vy , vz

ux , uy

uz , ur

ux , uy , uz

Fluid-solid, penalty, weak coupling

41

vx , vy

vz , vr

vx , vy , vz

ux , uy

uz , ur

ux , uy , uz

1336 Chapter 3: Model Definition Options Fluid Analysis

Fluid Parameter 2-D-planar 2-D-axisymmetric Fluid-thermal-solid, mixed, strong-weak

42

Fluid-thermal-solid, penalty, strong-weak

43

Fluid-thermal-solid, mixed, weak-weak

44

Fluid-thermal-solid, penalty, weak-weak

45

3-D

vx , vy , p, T

vx , vr , p, T

vx , vy , vz , p, T

ux , uy

uz , ur

ux , uy , uz

vx , vy , T

vz , vr , T

vx , vy , vz , T

ux , uy

uz , ur

ux , uy , uz

vx , vy , p

vz , vr , p

vx , vy , vz

T

T

T

ux , uy

uz , ur

ux , uy , uz

v x , vy

vz , vr

vx , vy , vz

T

T

T

ux , uy

uz , ur

ux , uy , uz

The fluid region cannot contain any truss, beams, membranes, shells, generalized plain strain, axisymmetric elements with twist or any semi-infinite elements. Element types 155-157 and the higher order tetrahedral elements are also not supported. For a complete list of supported elements, see Marc Volume A: Theory and User Information, Chapter 6: Nonstructural and Coupled Procedure Library, Element Types.

Main Index

REGION (Fluid) 1337 Define Elements in a Region

REGION (Fluid)

Define Elements in a Region

Description This option allows you to define which elements are part of a region. In fluid-solid, or fluid-thermal-solid analysis, it is necessary to divide the model into different regions depending on whether only a fluid analysis is performed in an area or a structural analysis is performed. This is used in conjunction with using the weakly coupled formulations. See Marc Volume A: Theory and User Information for more details. This option is also necessary in an acoustic-solid analysis, where you have to define the parts of the model belonging to the solid and the parts of the model belonging to the acoustic fluid. Format

Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word REGION.

2nd data block 1-5

1st

I

Enter the number of regions.

6-10

2nd

I

Enter the unit number for reading data. Defaults to input file.

Repeat data blocks 3 and 4 for region. 3rd data block 1-5

1st

I

Enter the region type: 1 – solid region 3 – fluid or acoustic region

4th data block Enter a list of elements.

Main Index

1338 COUPLING REGION Define Coupling Regions

COUPLING REGION

Define Coupling Regions

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This data block defines coupling regions and associates them with boundary condition names. These boundary conditions are activated or deactivated using the LOADCASE model or history definition option. Coupling regions, with the accompanying application programming interface (API), provide an interface to couple Marc with external numerical solvers such as computational fluid dynamics codes, via user subroutine programming. A coupling region is that part of the surface or volume of the model where the interaction with the external solver takes place. A surface region consists of a list of edges or geometric curves in 2-D and a list of faces or geometric surfaces in 3-D. A volumetric region consists of a list of elements or contact bodies. On coupling regions, the basic mechanical and thermal quantities (see Table 3-14, Table 3-15, Table 3-16, Table 3-17) can be exchanged with an external solver via API calls. The quantities that will be received from the external solver are applied through appropriate boundary conditions on the coupling region and must be specified on the 4th data block. The code coupling interface may also be used to apply complex boundary conditions on certain regions of the model or to develop dedicated post-processing tools. See Chapter 14 Code Coupling Interface in Marc Volume A: Theory and User Information and Chapter 12 Code Coupling Interface in Marc Volume D: User Subroutines and Special Routines for more information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words COUPLING REGION.

2nd data block 1-5

1st

I

Number of coupling regions to be read (optional).

6-10

2nd

I

Unit number to read data. Default is the standard input file.

Data blocks 3 through 6 are repeated for each coupling region.

Main Index

COUPLING REGION 1339 Define Coupling Regions

Format Fixed

Free

Data Entry Entry

3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 5th and 6th data blocks.

6-10

2nd

I

Enter the number of quantities that will be prescribed on this region. See 4th data block.

11-15

3rd

I

Not used.

16-20

4th

I

Not used.

21-25

5th

I

Not used.

26-30

6th

I

Not used.

31-63

7th

A

Enter the unique label associated with this coupling region. This label will be referenced by the LOADCASE model definition option.

The 4th data block is repeated for as many quantities as specified in the 3rd data block, 2nd field. 4th data block 1-5

1st

I

Enter the ID of the prescribed quantity (see tables below). Only quantities which can be “put” can be selected here. The quantity will be prescribed through appropriate boundary conditions on the region.

The 5th and 6th data blocks are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 5th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

Main Index

1340 COUPLING REGION Define Coupling Regions

Format Fixed

Free

Data Entry Entry

6th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 5th data block. Table 3-14

Global Quantities

Quantity ID

Dimension

Description

1

Scalar

Time Step

2

Scalar

Coupling Time Step

Put

Get

No

Yes

Yes*

No

* Only with the time stepping scheme. If the Coupling Time Step is prescribed on one coupling region, it will be prescribed on all coupling regions in the model.

Table 3-15

Nodal Quantities*

Quantity ID

Dimension

101

Vector

102

Description

Put

Get

Current Coordinates

No

Yes

Vector

Displacement

Yes

Yes

103

Vector

External Force

Yes

Yes

104

Vector

Reaction Force

No

Yes

112

Vector

Displacement (Local)

Yes

Yes

113

Vector

External Force (Local)

Yes

Yes

114

Vector

Reaction Force (Local)

No

Yes

121

Scalar

Displacement X

No

Yes

122

Scalar

Displacement Y

No

Yes

123

Scalar

Displacement Z

No

Yes

124

Scalar

External Force X

No

Yes

125

Scalar

External Force Y

No

Yes

126

Scalar

External Force Z

No

Yes

127

Scalar

Reaction Force X

No

Yes

128

Scalar

Reaction Force Y

No

Yes

129

Scalar

Reaction Force Z

No

Yes

* All mechanical nodal quantities are defined in the global coordinate system, except those tagged with “(Local)”. The latter are defined in the local coordinate systems of the nodes, if such coordinate systems have been defined by the TRANSFORMATION or the COORD SYSTEM model definition option or in the global system, otherwise.

Main Index

COUPLING REGION 1341 Define Coupling Regions

Table 3-15

Nodal Quantities*

Quantity ID

Dimension

161

Scalar

162

Description

Put

Get

Displacement X (Local)

Yes

Yes

Scalar

Displacement Y (Local)

Yes

Yes

163

Scalar

Displacement Z (Local)

Yes

Yes

164

Scalar

External Force X (Local)

Yes

Yes

165

Scalar

External Force Y (Local)

Yes

Yes

166

Scalar

External Force Z (Local)

Yes

Yes

167

Scalar

Reaction Force X (Local)

No

Yes

168

Scalar

Reaction Force Y (Local)

No

Yes

169

Scalar

Reaction Force Z (Local)

No

Yes

201

Scalar

Temperature

Yes

Yes

202

Scalar

External Heat Flux

Yes

Yes

203

Scalar

Reaction Heat Flux

No

Yes

* All mechanical nodal quantities are defined in the global coordinate system, except those tagged with “(Local)”. The latter are defined in the local coordinate systems of the nodes, if such coordinate systems have been defined by the TRANSFORMATION or the COORD SYSTEM model definition option or in the global system, otherwise.

Table 3-16 Quantity ID

Dimension

Put

Get

1101

Scalar

Total Pressure

Yes

No

1102

Vector

Total Traction

Yes

No

1201

Scalar

Heat Flux Density

Yes

No

1202

Scalar

Film Coefficient

Yes

No

1203

Scalar

Environment Temperature

Yes

No

Put

Get

Table 3-17

Main Index

Edge/Face Quantities Description

Element Quantities

Quantity ID

Dimension

Description

10101

Vector

Volume Load

Yes

No

10131

Scalar

Volume Load X

Yes

No

10132

Scalar

Volume Load Y

Yes

No

10133

Scalar

Volume Load Z

Yes

No

1342 FIXED DISP (Fluid) Define Fixed Displacement

FIXED DISP (Fluid)

Define Fixed Displacement

The information provided here is based upon not using the table driven input style. Description This data defines the fixed displacement that each specified degree of freedom must take during the first and subsequent increments, unless it is further modified using the DISP CHANGE option. The boundary conditions are specified either by giving the kinematic displacement and a list of degrees of freedom and a list of nodal numbers or by the input of boundary conditions generated during mesh generation (MESH2D). Note:

In static analysis, the boundary conditions specified must always be sufficient to remove all rigid body modes.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED DISP.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data is required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition data must be arranged accordingly.

For each set of boundary conditions, use the 3rd, 4th and 5th data blocks. 3rd data block 1-10

1st

E

Prescribed displacement for first degree of freedom listed in data block 4.

11-20

2nd

E

Prescribed displacement for second degree of freedom listed in data block 4.

21-30

3rd

E

Prescribed displacement for third degree of freedom listed in data block 4. A maximum of eight kinematic constraints can be specified. Third data block is read as 8E10.3.

Main Index

FIXED DISP (Fluid) 1343 Define Fixed Displacement

Format Fixed

Free

Data Entry Entry

4th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes to which the above boundary conditions are applied.

Main Index

1344 FIXED VELOCITY (with TABLE Input - Fluid) Define Fixed Velocity

FIXED VELOCITY (with TABLE Input - Fluid)

Define Fixed Velocity

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This data block defines potential fixed velocity, including the magnitude, degrees of freedom and applied locations, and associates it with a boundary condition name. This boundary condition is activated or deactivated using the LOADCASE model or history definition option. The boundary conditions are specified either by giving the velocity, a list of degrees of freedom, and either a list of nodal numbers or a list of surfaces. The prescribed velocities are with respect to the degrees of freedom associated with the element, unless they have been transformed to a local coordinate system using either the TRANSFORMATION, COORD SYSTEM, or UTRANFORM options. The FORCDT user subroutines or the TABLE model definition option can be used to enter nonuniform time-dependent boundary conditions. Note:

In steady state analysis, the boundary conditions specified must always be sufficient to remove all rigid body modes.

Further detail is given in Marc Volume A: Theory and User Information. See Marc Volume B: Element Library, for a definition of the degrees of freedom for each element type. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED VELOCITY.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

Unit number to read data default is the standard input file.

Data blocks 3 through 8 are repeated for each set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 7th and 8th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine are required for this boundary condition.

Main Index

FIXED VELOCITY (with TABLE Input - Fluid) 1345 Define Fixed Velocity

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE history definition option.

4th data block - Magnitudes 1-10

1st

E

Prescribed displacement for first degree of freedom listed in data block 8.

11-20

2nd

E

Prescribed displacement for second degree of freedom listed in data block 8.

21-30

3rd

E

Prescribed displacement for third degree of freedom listed in data block 8. A maximum of eight kinematic constraints can be specified.

5th data block - Table IDs 1-5

1st

I

Enter the table ID for the first degree of freedom listed.

6-10

2nd

I

Enter the table ID for the second degree of freedom listed.

11-15

3rd

I

Enter the table ID for the third degree of freedom listed.

6th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs 11: Element-Edges IDs

Main Index

1346 FIXED VELOCITY (with TABLE Input - Fluid) Define Fixed Velocity

Format Fixed

Free

Data Entry Entry 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention

8th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

Main Index

FIXED VELOCITY 1347 Define Fixed Velocity

FIXED VELOCITY

Define Fixed Velocity

The information provided here is based upon not using the table driven input style. Description This data defines the fixed velocity that each specified degree of freedom must take during the first and subsequent increments, unless it is further modified using the VELOCITY CHANGE option in a fluid analysis. The boundary conditions are specified either by giving the kinematic velocity and a list of degrees of freedom and a list of nodal numbers or by the input of boundary conditions generated during mesh generation (MESH2D). Note:

In steady state analysis, the boundary conditions specified must always be sufficient to remove all rigid body modes.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words FIXED VELOCITY.

2nd data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

6-10

2nd

I

This field is set to nonzero to flag input of boundary conditions set during mesh generation (MESH2D). If this field is activated, no further data is required in this option block.

11-15

3rd

I

Unit number used for MESH2D option. Note that the boundary conditions are stored after the connectivity and coordinate data on this file, so that the model definition data must be arranged accordingly.

For each set of boundary conditions, use the 3rd, 4th and 5th data blocks. 3rd data block

Main Index

1-10

1st

E

Prescribed velocity for first degree of freedom listed in data block 4.

11-20

2nd

E

Prescribed velocity for second degree of freedom listed in data block 4.

21-30

3rd

F

Prescribed velocity for third degree of freedom listed in data block 4.

1348 FIXED VELOCITY Define Fixed Velocity

Format Fixed

Free

Data Entry Entry

4th data block Enter a list of degrees of freedom to which the above prescribed velocities are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes to which the above boundary conditions are applied.

Main Index

ISOTROPIC (with TABLE Input - Fluid) 1349 Define Material Properties for Fluid Analysis

ISOTROPIC (with TABLE Input Fluid)

Define Material Properties for Fluid Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option is used to define the fluid properties for all of the elements. To define the dependence of these properties on temperature, use the TEMPERATURE EFFECTS model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word ISOTROPIC.

2nd data block 1-5

1st

I

Enter the number of distinct sets of material properties to be input (optional).

6-10

2nd

I

Enter unit number for input of data. Defaults to input.

The 3rd, 4th, 5th, 6th, 7th, and 8th data blocks should be entered as pairs, one for each distinct data block. 3rd data block 1-5

1st

I

Material identification number (1,2,3, etc.).

6-10

2nd

A

Enter the word FLUID if fluid-solid interaction and this is a fluid region.

4th data block 1-10

1st

F

Enter the reference temperature value of the viscosity.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Enter the reference value of the mass density of the fluid.

31-40

4th

F

Enter the coefficient of volumetric expansion.

5th data block

Main Index

1-5

1st

I

Table ID for viscosity.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Table ID for mass density.

16-20

4th

I

Table ID for coefficient of volumetric expansion.

1350 ISOTROPIC (with TABLE Input - Fluid) Define Material Properties for Fluid Analysis

Format Fixed

Free

Data Entry Entry

6th data block Necessary only in a coupled fluid-thermal analysis or a fluid-thermal-solid analysis. 1-10

1st

F

Thermal conductivity.

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis).

31-40

4th

F

Reference temperature.

7th data block 1-5

1st

I

Table ID for thermal conductivity.

6-10

2nd

I

Table ID for specific heat.

11-15

3rd

I

Table ID for mass density.

8th data block Enter element data set for which the properties as specified in data block 3 applies.

Main Index

ISOTROPIC (Fluid) 1351 Define Material Properties for Fluid Analysis

ISOTROPIC (Fluid)

Define Material Properties for Fluid Analysis

The information provided here is based upon not using the table driven input style. Description This option is used to define the fluid properties for all of the elements. To define the dependence of these properties on temperature, use the TEMPERATURE EFFECTS model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the word ISOTROPIC.

I

Enter the number of distinct sets of material properties to be input (optional).

2nd data block 1-5

1st

For temperature dependent properties, these are values corresponding to the first (lowest temperature) breakpoint (see TEMPERATURE EFFECTS option). A temperature dependent property is undefined below its lowest breakpoint. 6-10

2nd

I

Enter unit number for input of data. Defaults to input.

The 3rd, 4th, and 5th data blocks should be entered as pairs, one for each distinct data block. 3rd data block 1-5

1st

I

Material identification number (1,2,3, etc.) for cross-reference to TEMPERATURE EFFECTS option.

6-10

2nd

A

Enter the word FLUID if fluid-solid interaction and this is a fluid region.

4th data block

Main Index

1-10

1st

F

Enter the reference temperature value of the viscosity.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Enter the reference value of the mass density of the fluid.

31-40

4th

F

Enter the coefficient of volumetric expansion.

1352 ISOTROPIC (Fluid) Define Material Properties for Fluid Analysis

Format Fixed

Free

Data Entry Entry

5th data block Necessary only in a coupled fluid-thermal analysis or a fluid-thermal-solid analysis. 1-10

1st

F

Thermal conductivity

11-20

2nd

F

Specific heat.

21-30

3rd

F

Mass density (heat transfer analysis)

31-40

4th

F

Reference temperature.

6th data block Enter element data set for which the properties as specified in data block 3 applies.

Main Index

STRAIN RATE (Fluid) 1353 Define Strain Rate Dependent Viscosity

STRAIN RATE (Fluid)

Define Strain Rate Dependent Viscosity

Description This option allows the definition of a strain rate dependent viscosity for use in fluid flow problems. It also allows specification of different non-Newtonian viscosity models. The zero strain rate viscosity is given on the ISOTROPIC option. This option must be repeated for each different material for which strain rate data is necessary. The yield stress variation with strain rate is given using the following options: a. The breakpoints and slopes for a piecewise linear approximation to the viscosity strain rate curve are given. The strain rate breakpoints should be in ascending order, or b. The viscosity and stain rate data points lying on the viscosity strain rate curve are input directly. The data is entered in ascending order of strain rate. This method is flagged by entering the word DATA on the first data block. c. Bingham Fluid – enter 3 in the fourth field on the second data block. d. Fluid in the form of Power Law Relation – enter 4 in the fourth field on the second data block. e. Fluid in the form of Generalized Power Law Relation – enter 5 in the fourth field on the second data block. f. Fluid in the form of Carreau Model - enter 6 in the fourth field on the second data block. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words STRAIN RATE.

13-80

2nd

A

Enter the word DATA to indicate that option B is being used.

I

For option A, enter the number of slopes of viscosity versus strain rate curve.

2nd data block 1-5

1st

For option B, enter the number of data points. For other options, enter 0. 6-10

2nd

I

Material type identification (1,2,3...) for cross-reference to ISOTROPICAlphaList.1+option.

11-15

3rd

I

Unit number for input of the set of this block. Defaults to blocks.

16-20

4th

I

Non-Newtonian Viscosity Model type. Enter 0 for piecewise linear (use data block 3a or 3b). Enter 3 for Bingham Fluid (use data block 3c).

Main Index

1354 STRAIN RATE (Fluid) Define Strain Rate Dependent Viscosity

Format Fixed

Free

Data Entry Entry Enter 4 for Power Law Relation (use data block 3d). Enter 5 for Generalized Power Law Relation (use data block 3e). Enter 6 for Carreau model (use data block 3f).

3a data block Data block 3a is used in conjunction with piecewise representations, Option A. The number of blocks in this series is equal to that given in the first field of data block 2. 1-10

1st

F

Enter the slope of the viscosity versus strain rate curve.

11-20

2nd

F

Enter the strain rate value above which the above slope becomes operational. Note, the first strain rate breakpoint must be zero.

3b data block Data block 3b is used in conjunction with piecewise representation, Option B. 1-10

1st

F

Enter the value of the viscosity.

11-20

2nd

F

Enter the associated strain rate. Note that the first strain-rate must be zero.

3c data block Data block 3c is used for Bingham Fluid. 1-10

1st

F

Enter the value of g (stress;

· · · σ i j ′ = μ o γ ij + g γ ij ⁄ γ

if

· σ ≥ g ; γ ij = 0

3d data block Data block 3d is used for Power Law Relation Fluid. · n – 1· σi j ′ = μo K ( γ ) γ ij ).

1-10

1st

F

Enter the value of K (stress;

11-20

2nd

F

Enter the value of N (power; see above equation).

21-30

3rd

F

Enter the value of

μo .

(cutoff shear rate; see above equation).

3e data block Data block 3e is used for Generalized Power Law Relation Fluid. 1-10

1st

F

Enter the value of K.

11-20

2nd

F

Enter the value of N.

21-30

3rd

F

Enter the value of

31-40

4th

F

Enter the value of A1.

41-50

5th

F

Enter the value of A2.

51-60

6th

F

Enter the value of A3.

61-70

7th

F

Enter the value of A4.

then

Main Index

μo .

if

σ < g ).

STRAIN RATE (Fluid) 1355 Define Strain Rate Dependent Viscosity

Format Fixed

Free

Data Entry Entry

· p ow = N + A3 * log ( γ ) + A 4 × T · pow · σ' i j = μ o ⋅ Kγ ⋅ exp ( A 1 * T + A 2 * T 2 )γ ij

3f data block Data block 3f is used for Carreau Model Fluid.

Main Index

2 · 2 (n – 1) ⁄ 2 ). μ = μ∞ + ( μ o – μ∞ ) ( 1 + τ γ )

1-10

1st

F

Enter the value of

11-20

2nd

F

Enter the value of n (power; see above equation).

21-30

3rd

F

Enter the value of

τ

(time constant);

μ∞

(infinite shear viscosity; see above equation).

1356 TEMPERATURE EFFECTS (Coupled Fluid-Thermal) Temperature Effects in Coupled Fluid-Thermal Analysis

TEMPERATURE EFFECTS (Coupled FluidThermal)

Temperature Effects in Coupled Fluid-Thermal Analysis

The information provided here is based upon not using the table driven input style. This option is not available with the table driven input; use the TABLE model definition option instead. Description This option defines the variation of material properties (viscosity, thermal conductivity, specific heat) with temperature for the fluid region. The values read in through the ISOTROPIC option are those at the lowest temperature specified. Properties are not defined below the lowest temperature. The temperature dependency can be entered using one of the following two options: a. The variation of a particular property with temperature is specified as a piecewise linear curve. Breakpoints must be given in ascending order of temperature. b. The particular property value and temperature lying on the relevant curve are input directly. Data points must be given in increasing order of temperature. This option is flagged by entering the word DATA on the 1st data line. Format Format Fixed

Free

Data Entry Entry

1st data block 1-19

1st

A

Enter the words TEMPERATURE EFFECTS.

21-80

2nd

A

Enter the word DATA to indicate that option B is used.

For option A, use data blocks 2a, 3a, 4a, 5a, 6a, 7a and 8a. For option B, use data blocks 2b, 3b, 4b, 5b, 6b, 7b and 8b, below. Option A 2a data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Number of slopes of viscosity versus temperature curve.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Number of slopes of conductivity versus temperature curve

36-40

8th

I

Number of slopes of specific heat versus temperature curve.

TEMPERATURE EFFECTS (Coupled Fluid-Thermal) 1357 Temperature Effects in Coupled Fluid-Thermal Analysis

Format Fixed

Free

Data Entry Entry

41-45

9th

I

Number of latent heats to be entered.

46-50

10th

I

Number of slopes of emissivity versus temperature curve.

51-55

11th

I

Not used; enter 0.

56-60

12th

I

Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

61-65

13th

I

Logical unit number for input of this set of data. Defaults to blocks.

3a data block Slopes/breakpoints for viscosity versus temperature curve. The number in the fifth field of data line 2 defines the number of data lines required in data block 3. 1-15

1st

F

Enter the slope of viscosity versus temperature curve.

16-30

2nd

F

Enter the temperature at which this slope becomes operative.

4a data block Conductivity variation. Number of data lines as given on data line 2, seventh field. 1-15

1st

F

Enter the slope of conductivity versus temperature curve.

16-30

2nd

F

Enter the temperature at which the above slope becomes operative.

5a data block Specific heat variation. Number of data lines as given on data line 2, eighth field. 1-15

1st

F

Enter the slope of specific heat versus temperature curve.

16-30

2nd

F

Temperature above which this slope becomes operative.

6a data block Latent heat. Number of data lines given on data line 2, ninth field. 1-15

1st

F

Enter the latent heat.

16-30

2nd

F

Enter the solidus temperature (lower phase change limit).

31-45

3rd

F

Enter the liquidus temperature (upper phase change limit).

Option B 2b data block

Main Index

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Number of data points on the viscosity versus temperature curve for powder materials.

26-30

6th

I

Not used; enter 0.

1358 TEMPERATURE EFFECTS (Coupled Fluid-Thermal) Temperature Effects in Coupled Fluid-Thermal Analysis

Format Fixed

Free

Data Entry Entry

31-35

7th

I

Number of data points on the conductivity versus temperature curve.

36-40

8th

I

Number of data points on the specific heat versus temperature curve.

41-45

9th

I

Number of latent heats to be entered.

46-50

10th

I

Number of data points on the emissivity versus temperature curve.

51-55

11th

I

Not used; enter 0.

56-60

12th

I

Material type identification (1,2,3,...) for cross-referencing the ISOTROPIC option.

61-65

13th

I

Logical unit number for input of this set of data. Defaults to data lines.

3b data block The number in the fifth field of data line 2 defines the number of data lines required in data block 7. 1-15

1st

F

Enter the value of the viscosity.

16-30

2nd

F

Enter the associated temperature.

4b data block Conductivity variation. Number of data lines as given on data line 2, seventh field. 1-15

1st

F

Enter the value of the conductivity.

16-30

2nd

F

Enter the associated temperature.

5b data block Specific heat variation. Number of data lines as given on data line 2, eighth field. 1-15

1st

F

Enter the value of the specific heat.

16-30

2nd

F

Enter the associated temperature.

6b data block Latent heat. Number of data lines as given on data line 2, ninth field. 1-15

1st

F

Enter the value of the latent heat.

16-30

2nd

F

Enter the solidus temperature (lower phase change limit).

31-45

3rd

F

Enter the liquidus temperature (upper phase change limit).

7b data block Emissivity variation. Number of data lines as given on data line 2, tenth field. 1-15

1st

F

Enter the value of the emissivity.

16-30

2nd

F

Enter the associated temperature. Note:

Main Index

In calculating a particular temperature dependent property, Marc averages the value of this property at the start and at the end of the increment.

CONTROL (Fluid) 1359 Control Option for Fluid Analysis or Fluid-Thermal Analysis

CONTROL (Fluid)

Control Option for Fluid Analysis or Fluid-Thermal Analysis

Description This option allows you to input parameters governing the convergence and the accuracy for fluid analysis. For coupled fluid-thermal analysis, data block 4 must be used in addition to the 3rd data block. For nonlinear analysis, the controls are described in Marc Volume A: Theory and User Information. They do not appear on the restart file, and so must be re-entered on a restart run. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of load steps/increments in this run. Default is 9999. This is a cumulative number and is usually used to stop the run when restart is being used.

6-10

2nd

I

Maximum number of recycles/increments during an increment. Default is 3. If a negative number is entered, then Marc does a maximum of the absolute value entered. If convergence has not been obtained, a warning is given and Marc proceeds to the next increment. This is not recommended.

11-15

3rd

I

Minimum number of recycles during an increment. Default is 0. Note that this data field forces this number of recycles to take place at all subsequent increments.

16-20

4th

I

Flag for convergence testing. 0 or left blank Testing is done on residuals. 1 Testing is done on velocities. Note:

Testing on relative velocity always requires at least one iteration. If nonlinear analysis is done with the CENTROID parameter, the residuals are not calculated and testing is always done on velocities. Fluid analysis with the CENTROID parameter is not recommended.

Main Index

1360 CONTROL (Fluid) Control Option for Fluid Analysis or Fluid-Thermal Analysis

Format Fixed 21-25

Free 5th

Data Entry Entry I

Flag to specify relative or absolute error testing. If equal to 0, testing is done on relative error. If equal to 1, testing is done on absolute value. If set to 2, testing is done on relative error testing unless reactions or incremental velocities are below minimum value in which case absolute tolerances testing is used.

26-30

6th

I

Iterative procedure flag. 1. Full Newton-Raphson (default). 4. Direct substitution.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced. Default in fluid analysis.

36-40

8th

I

No longer used; enter 0.

41-45

9th

I

To print convergence control messages to log file, enter 1.

F

If relative residual checking:

3rd data block 1-10

1st

Maximum allowable value of maximum residual force divided by maximum reaction force. Default is 0.10. If relative velocity checking: Maximum allowable value of the change in velocity increment divided by the velocity increment. Default is 0.10. 11-20

2nd

F

If relative residual checking: Maximum allowable value of maximum residual moment divided by maximum reaction moment. Default is 0.0, in which case, no checking on residual moment occurs. If relative velocity checking: Maximum allowable value of the change in rotational increment divided by the rotational increment. Default is 0.0, in which case, no checking on change in rotational increment occurs.

21-30

3rd

F

If relative residual checking: Minimum reaction force, if reaction force is less than this value, checking is bypassed or absolute testing is performed. If relative velocity checking: Minimum velocity, if velocity increment is less than this value, checking is bypassed or absolute testing is performed.

Main Index

CONTROL (Fluid) 1361 Control Option for Fluid Analysis or Fluid-Thermal Analysis

Format Fixed

Free

Data Entry Entry

4th data block Only necessary for coupled fluid-thermal analysis.

Main Index

1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are reevaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable.

1362 CONTROL (Fluid-Solid) Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis

CONTROL (Fluid- Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis Solid) Description This option allows you to input parameters governing the convergence and the accuracy for fluid-solid or fluid-thermal-solid analysis. For nonlinear analysis, the controls are described in Marc Volume A: User Information. They do not appear on the restart file, and so must be re-entered on a restart run. In fluid-solid or fluid-thermal-solid analysis, there are two areas of the model which are defined using the REGION option. The data given here governs the convergence behavior in these regions. The 2nd and 3rd data blocks control the behavior in the solid region. The 4th and 5th data blocks control the behavior for thermal analysis in either region. The 6th and 7th data blocks control the fluid behavior. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of load steps/increments in this run. Default is 9999. This is a cumulative number and is usually used to stop the run when restart is being used.

6-10

2nd

I

Maximum number of recycles/increments during an increment for solid region. If a negative number is entered, then Marc does a maximum of the absolute value entered. If convergence has not been obtained, a warning is given and Marc proceeds to the next increment. This is not recommended.

11-15

3rd

I

Minimum number of recycles during an increment for plasticity or other tangent modulus nonlinearities in solid region. Default is 0. Note that this data field forces this number of recycles to take place at all subsequent increments.

16-20

4th

I

Flag for convergence testing. 0 or left blank Testing is done on residuals. 1 Testing is done on displacements. 2 Testing is done on strain energy. Note:

Testing on relative displacements or strain energy always requires at least one iteration. If nonlinear analysis is done with the CENTROID parameter, the residuals are not calculated and testing is always done on displacements. Nonlinear analysis with the CENTROID parameter is not recommended.

Main Index

CONTROL (Fluid-Solid) 1363 Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis

Format Fixed 21-25

26-30

Free 5th

6th

Data Entry Entry I

I

Flag to specify relative or absolute error testing. Equal to 0

Testing is done on relative error.

Equal to 1

Testing is done on absolute value.

If set to 2

Testing is done on relative error testing unless reactions or incremental displacements are below minimum value in which case absolute tolerances testing is used.

Iterative procedure flag. 1. Full Newton-Raphson (default). 2. Modified Newton-Raphson (no reassembly during iteration). 3. Newton-Raphson with strain correction modification. 8. Secant method.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced. Note that with use of gap and Herrmann elements, the matrix always is nonpositive definite and this entry has no significance.

36-40

8th

I

No longer used; enter 0.

41-45

9th

I

To print convergence control messages to log file, enter 1.

46-50

10th

I

Control on initial stress stiffness. 0 Normal-full contribution. 1 For Mooney material, reduce contribution of hydrostatic pressure on initial stress stiffness according to: σinitial = σ -fr ⋅ p ⋅ I where σinitial is the stress tensor used in the initial stress stiffness matrix, σ is the current stress tensor, fr is entered through the PARAMETERS option, p is the hydrostatic pressure and I is a unit tensor. 2 No initial stress stiffness. 3 Use stress at beginning of increment, not last iteration. 4 Results in the inclusion of only the positive stresses in the initial stress stiffness during the equilibrium iteration.

51-65

11th

I

Not used; enter 0.

56-60

12th

I

Assembly flag. If set to 1, the stiffness matrix is assembled each iteration. Note that this switches off the modified Newton-Raphson procedure if chosen in the sixth field of this data block.

Main Index

1364 CONTROL (Fluid-Solid) Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

F

If relative residual checking: Maximum allowable value of maximum residual force divided by maximum reaction force. Default is 0.10. If relative displacement checking: Maximum allowable value of the change in displacement increment divided by the displacement increment. Default is 0.10.

11-20

2nd

F

If relative residual checking: Maximum allowable value of maximum residual moment divided by maximum reaction moment. Default is 0.0, in which case, no checking on residual moment occurs. If relative displacement checking: Maximum allowable value of the change in rotational increment divided by the rotational increment. Default is 0.0, in which case, no checking on change in rotational increment occurs.

21-30

3rd

F

If relative residual checking: Minimum reaction force, if reaction force is less than this value, checking is bypassed or absolute testing is performed. If relative displacement checking: Minimum displacement, if displacement increment is less than this value, checking is bypassed or absolute testing is performed.

31-40

4th

F

If relative residual checking: Minimum moment: if moment is less than this value, checking is bypassed or absolute testing is performed. If relative displacement checking: Minimum rotation: if rotation increment is less than this value, checking is bypassed.

41-50

5th

F

If absolute residual testing: Maximum value of residual force. Default is 0.0 in which case, no checking on residual force takes place. If absolute displacement tasking: Maximum value of displacement increment. Default is 0.0; in which case, no checking on displacements takes place.

The 4th and 5th lines are used to control the thermal behavior. In an fluid-structure analysis (no thermal), do not include these blocks.

Main Index

CONTROL (Fluid-Solid) 1365 Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Maximum number of load steps in this run. Default is 99999. This is a cumulative number and is usually used to stop the run when RESTART is being used.

6-10

2nd

I

Maximum number of recycles during an increment due to temperature dependent material properties. Default value is 3.

11-15

3rd

I

Minimum number of recycles during an increment. Note that this data field forces this number of recycles to take place in all subsequent increments.

5th data block 1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are re-evaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable.

6th data block 1-5

1st

I

Maximum number of load steps/increments in this run. Default is 9999. This is a cumulative number and is usually used to stop the run when restart is being used.

6-10

2nd

I

Maximum number of recycles/increments during an increment. If a negative number is entered, then Marc does a maximum of the absolute value entered. If convergence has not been obtained, a warning is given and Marc proceeds to the next increment. This is not recommended.

11-15

3rd

I

Minimum number of recycles during an increment. Default is 0. Note that this data field forces this number of recycles to take place at all subsequent increments.

16-20

4th

I

Flag for convergence testing. If set to 0 or left blank, testing is done on residuals. If set to one, testing is done on velocities. Note that testing on relative velocity always requires at least one iteration. If nonlinear analysis is done with the CENTROID parameter, the residuals are not calculated and testing is always done on velocities. Note that fluid analysis with the CENTROID parameter is not recommended.

21-25

5th

I

Flag to specify relative or absolute error testing. If equal to 0, testing is done on relative error. If equal to 1, testing is done on absolute value. If set to 2, testing is done on relative error testing unless reactions or incremental velocities are below minimum value in which case absolute tolerances testing is used.

Main Index

1366 CONTROL (Fluid-Solid) Control Option for Fluid-Stress or Fluid-Thermal-Stress Analysis

Format Fixed 26-30

Free 6th

Data Entry Entry I

Iterative procedure flag. 1. Full Newton-Raphson (default). 4. Direct substitution.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced. Default in fluid analysis.

36-40

8th

I

No longer used; enter 0.

41-45

9th

I

To print convergence control messages to log file, enter 1.

F

If relative residual checking:

7th data block 1-10

1st

Maximum allowable value of maximum residual force divided by maximum reaction force. Default is 0.10. If relative velocity checking: Maximum allowable value of the change in velocity increment divided by the velocity increment. Default is 0.10. 11-20

2nd

F

If relative residual checking: Maximum allowable value of maximum residual moment divided by maximum reaction moment. Default is 0.0, in which case, no checking on residual moment occurs. If relative velocity checking: Maximum allowable value of the change in rotational increment divided by the rotational increment. Default is 0.0, in which case, no checking on change in rotational increment occurs.

21-30

3rd

F

If relative residual checking: Minimum reaction force, if reaction force is less than this value, checking is bypassed or absolute testing is performed. If relative velocity checking: Minimum velocity, if velocity increment is less than this value, checking is bypassed or absolute testing is performed.

Main Index

END OPTION 1367 Model Definition Data End

END OPTION

Model Definition Data End

Description This option is used to signify the end of all model definition data. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

A

Enter the words END OPTION.

1368 END OPTION Model Definition Data End

Main Index

Chapter 4 History Definition Options List 1369

Chapter 4 History Definition Options List

4

History Definition Options List

History Definition Option

Main Index

Page

ACC CHANGE

1601

ACCUMULATE

1587

ACTIVATE

1508

ACTUATOR

1581

ADAPT GLOBAL

1422

ADD RIGID (2-D)

1527

ADD RIGID (3-D)

1541

ADD RIGID with TABLES (2-D)

1521

ADD RIGID with TABLES (3-D)

1532

ANNEAL

1576

APPROACH

1573

ASSEM LOAD

1507

AUTO CREEP

1585

AUTO INCREMENT

1469

AUTO LOAD

1462

1370

History Definition Option

Main Index

Page

AUTO STEP

1474

AUTO THERM CREEP

1589

AUTO THERM

1487

B2GG, B2PP

1443

BEGIN SEQUENCE

1466

BUCKLE

1501

CHANGE PORE

1496

CHANGE RIGID

1513

CHANGE STATE

1489

COMMENT

1365

CONTACT NODE

1566

CONTACT TABLE

1559

CONTACT TABLE with TABLES

1550

CONTINUE

1680

CONTROL (Heat Transfer)

1623

CONTROL (Mechanical)

1391

CREEP INCREMENT

1584

DAMPING COMPONENTS

1649

DEACTIVATE

1509

DISP CHANGE

1448

DIST CHARGE (Electromagnetic)

1678

DIST CHARGE (Piezoelectric)

1664

DIST CURRENT (Electromagnetic)

1676

DIST CURRENT (Joule Heating)

1633

DIST CURRENT (Magnetostatic)

1668

DIST FLUXES

1607

DIST LOADS

1455

DIST MASS (Diffusion)

1642

DIST SOURCES

1654

Chapter 4 History Definition Options List 1371

History Definition Option

Main Index

Page

DMIG-OUT

1435

DYNAMIC CHANGE (Dynamic)

1598

DYNAMIC CHANGE (Electromagnetic)

1672

ELEMENT SORT

1384

EMCAPAC

1659

EMRESIS

1632

END SEQUENCE

1467

EXCLUDE

1580

EXTRAPOLATE

1588

FILMS

1627

FOUNDATION

1512

GAP CHANGE

1452

GRID FORCE

1380

HARMONIC (Acoustic)

1656

HARMONIC (Dynamic)

1600

HARMONIC (Electromagnetic)

1671

INCLUDE

1368

INERTIA RELIEF

1464

K2GG, K2PP

1440

LOADCASE

1432

M2GG, M2PP

1442

MODAL SHAPE

1594

MOTION CHANGE

1567

MOVE

1574

1372

History Definition Option

Main Index

Page

NEW

1367

NO ELEM SORT

1386

NO NODE SORT

1389

NO PRINT

1375

NO PRINT CONTACT

1377

NO PRINT SPRING

1379

NO SUMMARY

1383

NODE SORT

1387

P2G

1444

PARAMETERS

1397

POINT CHARGE (Piezoelectric)

1663

POINT CURRENT (Electromagnetic)

1675

POINT CURRENT (Joule)

1634

POINT FLUX

1609

POINT LOAD

1460

POINT MASS (Diffusion)

1645

POINT SOURCE (Acoustic)

1655

POINT TEMP

1494

POROSITY CHANGE

1638

POST

1404

POST INCREMENT

1419

POTENTIAL CHANGE (Piezoelectric)

1661

POTENTIAL CHANGE

1673

PRESS CHANGE

1652

PRINT CHOICE

1369

PRINT CONTACT

1376

PRINT ELEMENT

1371

PRINT NODE

1373

PRINT SPRING

1378

PRINT VMASS (History Definition)

1390

PROPORTIONAL INCREMENT

1468

Chapter 4 History Definition Options List 1373

History Definition Option

Main Index

Page

READ FILE

1445

RECOVER

1596

RELEASE NODE

1451

RELEASE

1572

RESET TIME

1500

RESTART INCREMENT

1421

SOLVER

1401

SPECTRUM

1599

SPLINE

1578

SS-ROLLING

1569

STEADY STATE (Electrostatic)

1658

STEADY STATE (Heat Transfer)

1606

STEADY STATE (Magnetostatic)

1667

STIFFNS COMPONENTS

1650

SUMMARY

1382

SUPERELEM (DMIG Applications)

1505

SUPERELEM

1503

SUPERPLASTIC

1483

SYNCHRONIZED

1577

TEMP CHANGE

1625

TERMINATE

1481

THERMAL LOADS

1485

THICKNS CHANGE

1648

TIME STEP

1499

TITLE

1366

TRANSIENT

1604

TYING CHANGE

1454

VELOCITY CHANGE

1628

VOID CHANGE

1640

VOLTAGE CHANGE

1635

1374

History Definition Option

Main Index

Page

WELD FILL

1620

WELD FLUX

1610

WELD PATH

1614

WRITE FILE

1446

Marc Volume C: Program Input Chapter 4 History Definition Options

4

Main Index

History Definition Options

J

General Controls

J

Static, Dynamic, Creep Analysis

J

Rate Dependent Analysis

J

Joule Heating Analysis

J

Diffusion Analysis

J

Hydrodynamic Bearing Analysis

J

Acoustic Analysis

J

Electrostatic Analysis

1671

J

Piezoelectric Analysis

1674

J

Magnetostatic Analysis

J

Electromagnetic Analysis

1378 1461

1597 1645

1651

1665

1680 1684

1661

1376 Marc Volume C: Program Input

The END OPTION ends the initial definition of the problem. All data subsequent to the END OPTION is interpreted as history definition or mesh display options. The input data for the history options controls the flow of Marc for the next loadcase which may consist of a single increment or multiple increments in the case of automatic control of loading. Facilities exist for changing the boundary conditions and the tying data. This new data is read in when the analysis of the previous loadcase is complete. A CONTINUE option terminates the input and initiates the analysis for the series of load increments corresponding to that input. The total number of increments in the analysis (no table input) is controlled by the CONTROL option or by conditions set within these options.

Elastic Analysis When the ELASTIC parameter is includes, all boundary conditions applied are total values that are applied in a single increment. Each loadcase would contain its own DIST LOADS, POINT LOAD, THERMAL LOADS, or CHANGE STATE option and be completed by the CONTINUE option.

Mechanical, Acoustic, Piezoelectric or Electrostatic-Structural or Electromagnetic Analyses All quantities specified for the previous load increment are also applied in the increment unless it is modified by the optional data described below. By judicious choice of the order of the load incrementation options, you can apply many combinations of displacement, traction, and thermal load vectors. You should note here that any new loads applied after the END OPTION are incremental and the total load at the end of any increment corresponds to the zero increment load plus all load increments to that point. Caution:

You must ensure that you zero out load increments that are being switched off since Marc, for some options, does not do this automatically.

Heat Transfer Analysis For heat transfer analysis, total fluxes or temperatures should always be input, and the solution time controlled by the TRANSIENT or AUTO STEP option.

Hydrodynamic Bearing Analysis In a bearing analysis, the lubricant thickness can be modified or the damping or stiffness behavior can be obtained.

Main Index

Chapter 4 History Definition Options 1377

Electrostatic Analysis For electrostatic analysis, total charges or potentials should always be input, and the solution time controlled by the STEADY STATE option.

Magnetostatic Analysis For magnetostatic analysis, total currents or potentials should always be input, and the solution time controlled by the STEADY STATE option.

Table Driven Boundary Conditions When using the table driven boundary conditions, you always enter the total loads at the end of the loadcase. This is done by having the boundary condition reference a table where one of the independent variables is time, normalized time, increment number, or normalized increment number. For the case of loadcases controlled by the arc-length method (AUTO INCREMENT), the independent variable should be the loadcase number. The LOADCASE option is used to activate boundary conditions. If a boundary condition is not named, it is deactivated.

Restart Considerations If a restart is made from one of the increments generated by a multi-increment procedure such as AUTO LOAD, DYNAMIC CHANGE, TRANSIENT, AUTO STEP, AUTO INCREMENT, AUTO THERM, AUTO CREEP, AUTO THERM CREEP, the rest of the increments associated with this procedure are automatically completed before reading of new input. This can be avoided by using the REAUTO option. The completion of an AUTO LOAD by a restart is done using the control parameters specified by Marc used with the RESTART option.

Main Index

1378 Marc Volume C: Program Input General Controls

General Controls This section describes modifications of program controls. The values given here override the values that might have been previously specified either with the model definition options or prior load incrementation data. Note that the CONTROL option is extremely important for specifying the convergence and tolerance controls.

Main Index

COMMENT 1379 Enter Comments

COMMENT

Enter Comments

Description This option allows you to enter informative comments for your own benefit. These data blocks can appear between parameters, model definition and history definition options. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word COMMENT.

11-80

2nd

A

User entered comment.

Alternate Format Format Fixed

Main Index

Free

Data Entry Entry

1-1

1st

A

Enter the $ character.

2-80

2nd

A

User entered comment.

1380 TITLE Output Title Definition

TITLE

Output Title Definition

Description This option defines the output title. There is no limit to the number of the title data read in as long as the word TITLE appears in the first field. However, only the last TITLE data is used as an output header. Due to the free-format processor, do not place commas within the TITLE data (Columns 11-80). Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the word TITLE.

11-80

2nd

A

Enter the title to be output with results.

NEW (History Definition) 1381 Use New Format

NEW (History Definition)

Use New Format

Description This option can be used to switch from input with extended format to the default width or vice-versa. Input is interpreted to be in the format defined here until another NEW history definition option is encountered. This option must not appear embedded inside any history definition option. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word NEW.

11-15

2nd

I

Enter 1 if the default width of the data fields is used for input.This will override the EXTENDED parameter. Enter 2 if the double width of the data fields is used for input.

Main Index

1382 INCLUDE (History Definition) Insert File into the Input File

INCLUDE (History Definition)

Insert File into the Input File

Description Inserts an external file into the input file. The include statement may appear in either the parameter, model definition, or history definition section. In Marc, an include file may reference another include file up to a level of 10 deep. The total length of the file name, including the directory path is limited to 240 characters. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word INCLUDE.

11-80

2nd

A

Physical filename. If the file name is specified without a path, the file should be in the same directory as the input file. If a path is given, the file should be in the path relative to the current working directory. Also, note that the file name is case sensitive.

Main Index

PRINT CHOICE (History Definition) 1383 Define Data to be Printed

PRINT CHOICE (History Definition)

Define Data to be Printed

Description This option allows you the control of the output from Marc. The data given here remains in control until a subsequent PRINT CHOICE set is inserted – such a set can be included with either the model definition or with history definition set. The default values print all elements and all nodes. Element quantities are printed at each integration point or at the centroid only, depending on whether the ALL POINTS or CENTROID parameter is used. For shells, only the extreme fibers are output, plus layers where the inelastic strains or state variables are nonzero. For beams, fibers with inelastic strains or nonzero state variables are printed. In addition, section forces are given for these elements. This option also allows debug output of certain items. The default is no debug printout. All of the above defaults are reset by the PRINT CHOICE option. The PRINT CHOICE option has no effect on the postprocessor file (see Chapter 3). Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words PRINT CHOICE.

2nd data block

Main Index

1-5

1st

I

Number of sets of first and last element numbers to be printed (maximum 10).

6-10

2nd

I

Number of sets of first and last node numbers to be printed (maximum 10).

11-15

3rd

I

Number of integration points to be printed in each element (not used if ALL POINTS is not flagged).

16-20

4th

I

Number of layers to be printed. This is for beams and shells only, and overrides the default described above.

21-25

5th

I

Increments between printout. Default is print every increment.

26-30

6th

I

Enter 1 for complex nodal quantities to be output as magnitude and phase; otherwise, real and imaginary components are given.

31-35

7th

I

Debug print flag. Enter a nonzero value and use data block 7.

36-40

8th

I

Log File Flag: Enter unit number to which log file is to be written.

1384 PRINT CHOICE (History Definition) Define Data to be Printed

Format Fixed

Free

Data Entry Entry

3rd data block Include only if the first field of 2nd data block is not zero. 1-5

1st

I

First element in first set.

6-10

2nd

I

Last element in first set.

11-15

3rd

I

First element in second set.

16-20

4th

I

Last element in second set.

Etc.

Etc. in I5 format.

4th data block Include only if the second field of 2nd data block is not zero. 1-5

1st

I

First node in first set.

6-10

2nd

I

Last node in first set.

11-15

3rd

I

First node in second set.

16-20

4th

I

Last node in second set.

Etc.

Etc. in I5 format.

5th data block Include only if the third field of 2nd data block is not zero. I

Enter the list of integration point to be printed in (16I5) format (number of entries given in the third field of data block 2). This is only used if ALL POINTS is flagged. Be careful with analyses with several different element types.

6th data block Include only if the fourth field of 2nd data block is not zero) I

Enter the list of shell or beam fibers to be printed in (16I5) format. As this over-rides the Marc default, you should be aware that you do not unintentionally miss the plasticity or creep printout.

7th data block Include only if the seventh field is not zero. 1-5

Main Index

1st

I

Enter debug plot code. See the PRINT parameter.

PRINT ELEMENT (History Definition) 1385 Specify Elements to be Included in Output

PRINT ELEMENT (History Definition) Specify Elements to be Included in Output Description This option allows you to choose which elements, and what quantities associated with an element are to be printed. If you do not specify NODE on the first data line, these values are at the integration points. This option can be used to print response quantities for the first 28 integration points of any element. This suffices for all elements, except continuum composite elements (types 149 - 154, 175 - 180) which can have as many as 2040 integration points. For print-outs at integration point numbers greater than 28 for continuum composite elements, use PRINT CHOICE. If you specify the word NODE, these values are the extrapolated nodal values. This extrapolation is currently not available for rebar elements, composite continuum elements, semi-infinite elements, or cavity elements. Note:

This option revokes any NO PRINT that precedes it. Therefore, NO PRINT followed by PRINT ELEMENT and not followed by PRINT NODE results in the selected element printout and full nodal printout. Use PRINT NODE with a blank node list to suppress node output.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PRINT ELEMENT.

11-20

2nd

A

Enter the word NODE (optional).

2nd data block 1-5

1st

I

Enter the number of sets to be given below (optional).

6-10

2nd

I

Increment between printout. Default is print every increment.

11-15

3rd

I

File unit to which output is to be written. Defaults to standard output, unit 6.

Data blocks 3, 4, and, if necessary, 5 and 6 are given once for each data set. 3rd data block 1-80

Main Index

1st

A

Enter one or more of the following: STRAIN

output total strain.

STRESS

output total stress.

PLASTIC

output plastic strain.

CREEP

output creep, swelling and viscoelastic strain.

THERMAL

output thermal strain

1386 PRINT ELEMENT (History Definition) Specify Elements to be Included in Output

Format Fixed

Free

Data Entry Entry ENERGY

output of strain energy densities: • total strain energy • incremental total strain energy • total elastic strain energy • incremental elastic strain energy • plastic strain energy • incremental plastic strain energy

CRACK

output of cracking strain

CAUCHY

output Cauchy stress.

STATE

output state variables.

PREFER

output stresses in preferred system.

ELECTRIC

output electric field and electric flux

MAGNETIC output magnetic field and magnetic flux CURRENT

output current

ALL

output of all of the above.

4th data block Enter a list of elements to be printed. Note:

To suppress all element print-out, enter a blank list for the list of elements.

5th data block If the NODE option is not specified on the 1st data block, enter a list of integration points to be printed. If the NODE option is specified on the 1 data block, enter a list of node positions based upon the CONNECTIVITY option. These node positions range from one to the maximum number of nodes per element. 6th data block Enter a list of layers to be printed. This is only necessary if there are either thin walled beam, shell, rebar, solid composite elements in the mesh, (that is, element types 1, 4, 5, 8, 13, 14, 15, 16, 17, 22, 23, 24, 25, 45,46, 47, 48, 49, 50, 72, 75, 76, 77, 78, 79, 85, 86, 87, 88, 89, 90, 98, 138, 139, 140, 142, 143, 144, 145, 146, 147, 148, 149, 150, 151, 152, 153, 154, 165, 166, 167, 168, 169, 170, 175, 176, 177, 178, 179, 180). It is also necessary to include this data block if there are beam element types 52 or 98 and they are used with integrated solid cross sections.

Main Index

PRINT NODE (History Definition) 1387 Define Nodes and Nodal Quantities to be Printed

PRINT NODE (History Definition)

Define Nodes and Nodal Quantities to be Printed

Description This option allows you to choose which nodes and what nodal quantities are to be printed. The average nodal generalized stresses are obtained via an extrapolation and averaging procedure. If there is a geometric or material discontinuity at a node, this value is not correct unless either double nodes were used and kinematic tying, or you control which elements are to be averaged using the PRINT ELEMENT feature. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words PRINT NODE.

2nd data block 1-5

1st

I

Enter the number of sets to be given below (optional).

6-10

2nd

I

Increment between printout. Default is print every increment.

11-15

3rd

I

File unit to which output is to be written. Default to standard output, unit 6.

Data blocks 3 and 4 are entered as pairs, once for each data set. 3rd data block 1-80

1st

A

Enter one or more of the following: INCR

output incremental displacement or potentials

TOTA

output total displacement or potentials

VELO

output velocity

ACCE

output acceleration

LOAD

output total applied load

REAC

output reaction/residual force

TEMP

output temperature

FLUX

output flux (Fluxes are only available if the HEAT, 0, 0, 2 parameter is used.)

MODE

output eigenvector (modal or buckle)

STRESS output average generalized stresses at nodes

Main Index

VOLT

output voltage (Joule analysis)

PRES

output pressure (bearing analysis)

1388 PRINT NODE (History Definition) Define Nodes and Nodal Quantities to be Printed

Format Fixed

Free

Data Entry Entry COOR

output coordinates (only for rezoning)

ALL

output all relevant quantities

4th data block Enter a list of nodes to be printed. To suppress all nodal printout, enter a blank list for the list of nodes.

Main Index

NO PRINT (History Definition) 1389 Suppress Printing

NO PRINT (History Definition)

Suppress Printing

Description This option suppresses element and nodal output. This option is revoked by using either the PRINT CHOICE, PRINT ELEMENT, or PRINT NODE option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO PRINT.

1390 PRINT CONTACT (History Definition) Prints the Contact Body Summary

PRINT CONTACT (History Definition)

Prints the Contact Body Summary

Description This option ensures that the summary of contact information for each body is printed to the output file even if the NO PRINT option is activated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words PRINT CONTACT.

NO PRINT CONTACT (History Definition) 1391 Suppresses the Contact Body Summary Printout

NO PRINT CONTACT (History Definition)

Suppresses the Contact Body Summary Printout

Description This option deactivates the output of the summary of contact information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO PRINT CONTACT.

1392 PRINT SPRING (History Definition) Controls the Print Out of Springs

PRINT SPRING (History Definition) Description This option controls the output for selected springs. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PRINT SPRING.

2nd data block Enter a list of springs to be printed

Main Index

Controls the Print Out of Springs

NO PRINT SPRING (History Definition) 1393 Deactivates the Printing of All Springs

NO PRINT SPRING (History Definition)

Deactivates the Printing of All Springs

Description This options supresses the output of spring results. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word NO PRINT SPRING.

1394 GRID FORCE (History Definition) Nodal Force Output at Element or Node Level

GRID FORCE (History Definition) Nodal Force Output at Element or Node Level This option allows the user to output the contributions to the nodal force at either an element level or a nodal level. This is useful when constructing a free body diagram of part of the structure. The Marc for grid force balance is with respect to the global coordinate system. In Marc, the following contributions are considered: On an element level the grid force balance is based upon the Internal Forces Distributed Loads Foundation Forces Reaction Force On a nodal basis it is much more complete and includes Internal Forces

Distributed + Point Forces

Foundation Forces

Spring Forces

Contact Normal Forces

Contact Friction Forces

Tying/MPC Forces

Inertia Forces

Damping Forces

DMIG Forces

Reaction Force Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word GRID FORCE.

2nd data block 1-5

1st

I

Frequency (increments) between writing out the grid forces.

6-10

2nd

I

Enter 1 if force output is based upon elements.

11-15

3rd

I

Enter 1 if force output is based upon nodes.

16-20

4th

I

Enter 0 if grid force output is to be written to standard output (default). Enter 1 if grid force output is to be written to file jid.grd.

21-25

5th

I

Enter the number of times that grid force should be output in a load case; if 1 is entered, the output will occur at the last increment of the load case.

3rd and 4th data block are optional (may be repeated multiple number of times)

Main Index

GRID FORCE (History Definition) 1395 Nodal Force Output at Element or Node Level

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

A

Enter the words SELECT ELEMENT

4th data block 1-80

Enter a list of elements for which grid force output will be done

5th and 6th data block are optional (may be repeated multiple number of times) 5th data block 1-10

1st

A

Enter the words SELECT BODY

6th data block 1-80

Enter a list of bodies, grid force on an element level will be given for elements in these bodies.

7th and 8th data block are optional (may be repeated multiple number of times) 7th data block 1-10

1st

A

Enter the words SELECT NODE

8th data block 1-80

Main Index

Enter a list of nodes for which forces will be output on a nodal basis.

1396 SUMMARY (History Definition) Create Summary Report

SUMMARY (History Definition)

Create Summary Report

Description This option produces a summary of the results of the increment and outputs them in a report format. This option is in effect until a NO SUMMARY option is encountered. The summary consists of the maximum and minimum of temperatures, stresses, strains, plastic strains, creep strains, displacements, velocities, accelerations and reaction forces. The option also produces a detailed accounting of both the memory usage and timing information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SUMMARY.

11-15

2nd

I

Enter the unit number to be used for output. Default is standard output, unit 6.

16-20

3rd

I

Enter the increment frequency of summary. Default is every increment.

Main Index

NO SUMMARY (History Definition) 1397 Suppress Summary

NO SUMMARY (History Definition)

Suppress Summary

Description This option turns off the summary feature. The default is off unless the SUMMARY option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO SUMMARY.

1398 ELEMENT SORT (History Definition) Sort Elements for Report

ELEMENT SORT (History Definition)

Sort Elements for Report

Description This option allows various element quantities to be sorted and the output given in report format. This option is in effect until a NO ELEM SORT option is encountered. This option allows you to sort either in ascending or descending order. In addition, you can use either the real numeric value or the absolute value. A range can be given over which to sort. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ELEM SORT.

2nd data block 1-5

1st

I

Enter number of sorts to be performed (optional). One data block, as given below, defines each sort.

6-10

2nd

I

Enter unit number to read sort data.

11-15

3rd

I

Enter the unit number to be used for output, default is standard output, unit 6.

16-20

4th

I

Enter the increment frequency, default is every increment.

3rd data block The 3rd data block is repeated once for each sort. 1-5

1st

I

Enter code indicating type of quantity to be sorted (see Table 4-1).

6-10

2nd

I

Enter 0 for sort in descending order. Enter 1 for sort in ascending order. Default is 0; sort in descending order.

11-15

3rd

I

Enter 1 for sort by real numerical value. Enter 0 for sort by absolute value. Default is 0; sort by absolute value.

Main Index

16-20

4th

I

Enter number of items to be included in sorted list.

21-25

5th

I

Enter lowest element number of range to be sorted. Defaults to 1.

26-30

6th

I

Enter highest element number of range to be sorted. Defaults to last element in mesh.

ELEMENT SORT (History Definition) 1399 Sort Elements for Report

Table 4-1

Element Sort Codes

Code

Description

Description

1 first stress

28 fourth plastic strain

2 second stress

29 fifth plastic strain

3 third stress

30 sixth plastic strain

4 fourth stress

31 equivalent plastic strain

5 fifth stress

32 mean plastic strain

6 sixth stress

33 Tresca plastic strain

7 equivalent stress

34 first principal plastic strain

8 mean stress

35 second principal plastic strain

9 Tresca stress

36 third principal plastic strain

10 first principal stress

37 first creep strain

11 second principal stress

38 second creep strain

12 third principal stress

39 third creep strain

13 first strain

40 fourth creep strain

14 second strain

41 fifth creep strain

15 third strain

42 sixth creep strain

16 fourth strain

43 equivalent creep strain

17 fifth strain

44 mean creep strain

18 sixth strain

45 Tresca creep strain

19 equivalent strain

46 first principal creep strain

20 mean strain

47 second principal creep strain

21 Tresca strain

48 third principal creep strain

22 first principal strain

49 temperature

23 second principal strain

61 voltage

24 third principal strain

73 first gradient

25 first plastic strain

74 second gradient

26 second plastic strain

75 third gradient

27 third plastic strain

Main Index

Code

1400 NO ELEM SORT (History Definition) Do Not Create Report Sorted by Element

NO ELEM SORT (History Definition)

Do Not Create Report Sorted by Element

Description This option turns off the ELEM SORT feature. The default is off unless the ELEM SORT option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO ELEM SORT.

NODE SORT (History Definition) 1401 Sort Nodal Results

NODE SORT (History Definition)

Sort Nodal Results

Description This option allows various nodal quantities to be sorted and the output given in report format. This option is in effect until a NO NODE SORT is encountered. NODE SORT allows you to sort either in ascending or descending order. In addition, you can use either the real numeric value or the absolute value. A range can be given over which to sort. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words NODE SORT.

2nd data block 1-5

1st

I

Enter number of sorts to be performed (optional). One data block as given below defines each sort.

6-10

2nd

I

Enter unit number to read sort data.

11-15

3rd

I

Enter the unit number to be used for output, default is standard output, unit 6.

16-20

4th

I

Enter the increment frequency, default is every increment.

3rd data block The 3rd data block is entered once for each sort.

Main Index

1-5

1st

I

Enter code indicating type of quantity to be sorted (see Table 4-2).

6-10

2nd

I

Enter 0 for sort in descending order. Enter 1 for sort in ascending order. Default is 0, sort in descending value.

11-15

3rd

I

Enter 1 for sort by real numerical value. Enter 0 for sort by absolute value. Default is 0, sort by absolute value.

16-20

4th

I

Enter number of items to be included in sorted list.

21-25

5th

I

Enter lowest node number of range to be sorted. Defaults to 1.

26-30

6th

I

Enter highest node number of range to be sorted. Defaults to last node in mesh.

1402 NODE SORT (History Definition) Sort Nodal Results

Table 4-2 Code

Node Sort Codes Meaning

1-12 sort code I

Main Index

Result Results in the Ith component of the incremental displacement to be sorted.

13-34 sort code I +12

Results in the Ith component of the total displacement to be sorted.

25-36 sort code I + 24

Results in the Ith component of the velocity to be sorted.

37-48 sort code I + 36

Results in the Ith component of the acceleration to be sorted.

48-60 sort code I + 48

Results in the nodal temperature to be sorted.

61-72 sort code I + 60

Results in the Ith component of the reaction force to be sorted.

71-84 sort code I + 72

Results in the Ith component of the contact force to be sorted.

101 101

Sort on magnitude of incremental displacement.

102 102

Sort on magnitude of total displacement.

103 103

Sort on magnitude of velocity.

104 104

Sort on magnitude of acceleration.

105 105

Sort on magnitude of temperature.

106 106

Sort on magnitude of reaction force.

107 107

Sort on magnitude of contact force.

NO NODE SORT (History Definition) 1403 Cancel Report Sorted by Nodes

NO NODE SORT (History Definition)

Cancel Report Sorted by Nodes

Description This option negates the NODE SORT option. The default is off unless the NODE SORT option has been previously invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words NO NODE SORT.

1404 PRINT VMASS (History Definition) Print Element Volumes, Masses, Costs, and Strain Energies

PRINT VMASS (History Definition)

Print Element Volumes, Masses, Costs, and Strain Energies

Description This option allows you to obtain printed output of element volumes, masses, costs and strain energies. Options are provided for you to print the total quantities for each group of elements and the quantities for each element in the group or the total quantities for each group of elements only. In order to have correct mass computations, mass density for each element must be entered through one of the material options. In order to have the correct cost, the cost per unit mass or the cost per unit volume must be defined through the ISOTROPIC/ORTHOTROPIC option. The total strain energy and the plastic strain energy, if applicable, are printed. Note that volumes and masses for some special elements (for example, gap element, semi-infinite element, etc.) is not be computed. These quantities can be written on either standard output file unit 6, or your specified unit. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words PRINT VMASS.

2nd data block 1-5

1st

I

Enter the number of sets to be given below.

6-10

2nd

I

Enter 1 for option to print only total volumes, masses, costs, and strain energy for groups of elements. Default is 0.

11-15

3rd

I

File unit to which output is to be written; default to standard output, unit 6.

Either data block 3a or 3b may be used 3a data block Enter a list of elements to be printed. 3b data block Enter the negative of deformable body number (only one body number per data block).

Main Index

CONTROL (Mechanical - History Definition) 1405 Control Option for Stress Analysis

CONTROL (Mechanical - History Definition) Control Option for Stress Analysis Description This option allows you to input parameters governing the convergence and the accuracy for nonlinear analysis. For heat transfer analysis, see the CONTROL (Heat Transfer) history definition option. For coupled thermal-stress analysis, data block 6 must be used. For coupled electrostatic-stress analysis, data block 7 must be used. For nonlinear static analysis, the controls are described in Marc Volume A: Theory and User Information. They do not appear on the restart file, and so must be re-entered on a restart run. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block 1-5

1st

I

Maximum number of load steps/increments in this run. Default is 9999. This is a cumulative number and is usually used to stop the run when restart is being used. If an ELASTIC parameter is included, this field is ignored and all load cases are analyzed.

6-10

2nd

I

Maximum number of recycles/increments during an increment for plasticity, or other tangent modulus nonlinearities. Default is 3. This should usually be increased to 10 for rigid-plastic flow option. If a negative number is entered, Marc does a maximum of the absolute value entered. If convergence has not been obtained, a warning is given and Marc proceeds to the next increment. This is not recommended.

11-15

3rd

I

Minimum number of recycles during an increment for plasticity or other tangent modulus nonlinearities. Default is 0. Note:

This data field forces this number of recycles to take place at all subsequent increments.

Caution: This value is overwritten by the PROPORTIONAL INCREMENT option. 16-20

4th

I

Flag for convergence testing. 0 or left blank Convergence is achieved when residuals satisfy the criterion. 1 Convergence is achieved when displacements satisfy the criterion.

Main Index

1406 CONTROL (Mechanical - History Definition) Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry 2 Convergence is achieved when strain energy satisfies the criteria. 4 Convergence is achieved when either residual or displacement satisfies the criterion. 5 Convergence is achieved when both residual and displacement satisfies the criterion.

21-25

26-30

5th

6th

I

I

Notes:

Testing on relative displacements or strain energy always requires at least one iteration. If nonlinear analysis is done with the CENTROID parameter, the residuals are not calculated and testing is always done on displacements.

Notes:

Nonlinear analysis with the CENTROID parameter is not recommended.

Notes:

If the fields are set as 0, 1, or 2, only the 3rd data block is needed.

Notes:

If the fields are set as 4 or 5, the 3a data block is also needed. In this case, the 3rd data block is set for residual testing and 3a data block is set for displacements check only.

Flag to specify relative or absolute error testing. If equal to 0

Testing is done on relative error.

If equal to 1

Testing is done on absolute value.

If equal to 2

Testing is done on relative error testing unless reactions or incremental displacements are below minimum value, in which case absolute tolerances testing is used.

Iterative procedure flag. 1 Full Newton-Raphson (default). 2 Modified Newton-Raphson (no reassembly during iteration). 3 Newton-Raphson with strain correction modification (see Marc Volume A: Theory and User Information). 8 Secant method.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced. Note:

Main Index

With use of gap and Herrmann elements, the matrix always is nonpositive definite and this entry has no significance.

36-40

8th

I

No longer used; enter 0.

41-45

9th

I

To print convergence control messages to log file, enter 1.

CONTROL (Mechanical - History Definition) 1407 Control Option for Stress Analysis

Format Fixed

Free

46-50

10th

Data Entry Entry I

Control on initial stress stiffness. 0 Normal-full contribution. 1 For Mooney material, reduce contribution of hydrostatic pressure on initial stress stiffness according to: σ i ni ti al = σ – f r ⋅ p ⋅ I

where σ i ni ti al is the stress tensor used in the initial stress stiffness matrix, σ is the current stress tensor, f r is entered through the PARAMETERS option, p is the hydrostatic pressure and I I is a unit tensor. 2 No initial stress stiffness. 3 Use stress at beginning of increment, not last iteration. 4 Results in the inclusion of only the positive stresses in the initial stress stiffness during the equilibrium iteration. Besides faster convergence, this leads to a stable analysis of very thin shell structures. 51-55

11th

I

Control parameter: 0 Do not allow switching of convergence testing between residuals and displacements. 1 Allow switching of convergence testing between residual and displacements if reaction forces or displacements become extremely small. For more details, see Marc Volume A: Theory and User Information. Note:

Set this parameter to 0 if any kind of absolute value testing is being used.

56-60

12th

I

Assembly flag. If set to 1, the stiffness matrix is assembled each iteration. Note that this switches off the modified Newton-Raphson procedure if chosen in the sixth field of this data block.

61-65

13th

I

For some material models, such as damage, cracking, and Chaboche, there is an inner iteration loop to insure accuracy. The maximum number of iterations allowed can be set here. Default is 50.

3rd data block Include if residual testing is required and the fourth field of the 2nd data block is 0, 4, or 5. 1-10

Main Index

1st

F

If relative residual checking:

1408 CONTROL (Mechanical - History Definition) Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry Maximum allowable value of maximum residual force divided by maximum reaction force. Default is 0.10.

11-20

2nd

F

If relative residual checking: Maximum allowable value of maximum residual moment divided by maximum reaction moment. Default is 0.0, in which case, no checking on residual moment occurs.

21-30

3rd

F

If relative residual checking: Minimum reaction force, if reaction force is less than this value, checking is bypassed or absolute testing is performed.

31-40

4th

F

If relative residual checking: Minimum moment: if moment is less than this value, checking is bypassed or absolute testing is performed.

41-50

5th

F

If absolute residual testing: Maximum value of residual force. Default is 0.0 in which case, no checking on residual force takes place.

51-60

6th

F

If absolute residual testing: Maximum value of residual moment. Default is 0.0 in which case, no checking on residual moments takes place. If absolute displacement testing, maximum value of rotation increment. Default is 0.0; in which case, no checking or rotations take place.

61-70

7th

F

Rigid Link Rotation Tolerance: Maximum allowable value of the change in rotation increment at the retained nodes of RBE2, rigid link (tying type 80) or beam-shell offset nodes. Default is 0.001 radians.

Main Index

Notes:

If the 4th field of the 2nd data block is 4 or 5, the rigid link rotation tolerance entered in the 4th data block circumvents the corresponding value in the 3rd data block.

Notes:

The rigid link rotation tolerance if left at 0, is reset to 0.001 radians by the Marc solver to ensure backward compatibility for RBE2.Theare two ways to by-pass the link rotation check: the rigid link rotation tolerance can be set to a negative number, or the rigid link rotation tolerance can be left as 0.0 with an additional FEATURE,5701 added to the parameter section of the input.

CONTROL (Mechanical - History Definition) 1409 Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry

4th data block Include if displacement testing is required and the fourth field of the 2nd data block is 1, 4, or 5. 1-10

1

F

Maximum allowable value of the change in displacement increment divided by the displacement increment. Default is 0.10.

11-20

2nd

F

Maximum allowable value of the change in rotational increment divided by the rotational increment. Default is 0.0, in which case, no checking on change in rotational increment occurs.

21-30

3rd

F

Minimum displacement, if displacement increment is less than this value, checking is bypassed or absolute testing is performed.

31-40

4th

F

Minimum rotation: if rotation increment is less than this value, checking is bypassed.

41-50

5th

F

Maximum value of displacement increment. Default is 0.0; in which case, no checking on displacements takes place.

51-60

6th

F

Maximum value of rotation increment. Default is 0.0; in which case, no checking on rotations takes place.

61-70

7th

F

Rigid Link Rotation Tolerance: Maximum allowable value of the change in rotation increment at the retained nodes of RBE2, rigid link (tying type 80) or beam-shell offset nodes. Default is 0.001 radians.

Notes:

If the 4th field of the 2nd data block is 4 or 5, the rigid link rotation tolerance entered in the 4th data block circumvents the corresponding value in the 3rd data block.

Notes:

The rigid link rotation tolerance if left at 0, is reset to 0.001 radians by the Marc solver to ensure backward compatibility for RBE2.Theare two ways to by-pass the link rotation check: the rigid link rotation tolerance can be set to a negative number, or the rigid link rotation tolerance can be left as 0.0 with an additional FEATURE,5701 added to the parameter section of the input.

5th data block Include if energy testing is required and the fourth field of the 2nd data block is 2. 1-10

1st

F

Maximum allowable value of the change is energy increment. Default is 0.1.

Main Index

1410 CONTROL (Mechanical - History Definition) Control Option for Stress Analysis

Format Fixed

Free

Data Entry Entry

6th data block Only necessary for coupled thermal-mechanical analysis. 1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are reevaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable. Note:

Only the temperature estimate error (3rd field) is checked for the TRANSIENT NON AUTO fixed stepping procedure. All three fields are checked for the transient adaptive stepping procedure. None of the three fields are checked for the auto step adaptive stepping procedure.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Maximum change of xsi,p allowed in pyrolysis calculation. Used to control automatic time step scheme.

51-60

6th

F

Maximum change of xsi,v allowed in pyrolysis calculation. Used to control automatic time step scheme.

61-70

7th

F

Maximum change of xsi,c allowed in pyrolysis calculation. Used to control automatic time step scheme.

71-80

8th

F

Maximum change in surface displacement per time step due to recession. This is used to control the time step for the TRANSIENT option.

7th data block Only necessary for coupled electrostatic structural analysis.

Main Index

1-10

1st

F

Maximum allowed relative error in residual charge.

11-20

2nd

F

Maximum allowed absolute error in residual charge.

PARAMETERS (History Definition) 1411 Definition of Parameters used in Numerical Analysis

PARAMETERS (History Definition)

Definition of Parameters used in Numerical Analysis

Description There are many parameters that are used in the finite element calculations. These parameters can be customized for your particular application. Some of these constants can be entered in other input blocks as well. The last nonzero value is used for the calculation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word PARAMETERS.

E

Enter the scale factor which, when multiplied with the incremental strain, is used to predict the incremental strain in the next increment.

2nd data block 1-10

1st

Default is 1.0. 11-20

2nd

E

Enter the multiplier used to calculate the penalty factor to impose boundary conditions. The penalty factor is this multiplier times the maximum diagonal value of the operator matrix. Default multiplier is 1 x 109. If the APPBC parameter is used, this option is not used.

21-30

3rd

E

Enter the penalty factor used to satisfy incompressibility in rigid plastic analysis for plane strain, axisymmetric, or solid analysis when displacement elements are used. Default is 100.

31-40

4th

E

Enter the penalty factor used to satisfy incompressibility in fluid analysis when displacement elements are used. Default is 1 x 106.

41-50

5th

E

Beta parameter used in transient dynamic analysis using Newmark-beta procedure. Default is 0.25.

51-60

6th

E

Gamma parameter used in transient dynamic analysis using Newmarkbeta procedure. Default is 0.50.

61-70

Main Index

7th

E

Gamma1 parameter used in transient dynamic analysis using Single Step Houbolt procedure.

1412 PARAMETERS (History Definition) Definition of Parameters used in Numerical Analysis

Format Fixed

Free

Data Entry Entry Default is 1.5.

71-80

8th

E

Gamma parameter used in transient dynamic analysis using Single Step Houbolt procedure. Default is -0.5.

3rd data block 1-10

1st

E

Enter the angle at which a node separates from a convex corner or becomes stuck in a concave corner for two-dimensional contact. Default is 8.625°.

11-20

2nd

E

Enter the angle at which a node separates from a convex corner or becomes stuck in a concave corner for three-dimensional contact. Default is 20.0°.

21-30

3rd

E

Enter the initial strain rate for rigid plastic analysis. Default is 1 x 10-4.

31-40

4th

E

Enter the cutoff strain rate for rigid plastic analysis. Default is 1 x 10-12.

41-50

5th

E

Enter the fraction of the hydrostatic pressure that is subtracted from the stress tensor in the initial stress calculation. See the tenth field of the CONTROL option. Default is 1.0

51-60

6th

E

Enter the factor used to calculate the drilling mode for shell elements type 22, 75, 138, 139, and 140. Default is 0.0001.

61-70

7th

E

Enter the scale factor to the initial incremental displacements estimate for the increment after a rezoning increment. The default value is 1.0, which usually improves friction convergence, but may result in an inside-out element.

4th data block (Optional) 1-10

1st

E

Universal gas constant (R). Default is 8.314 J mol-1K-1.

11-20

2nd

E

Offset temperature between user units and absolute temperature. Default is 273.15°; that is, user input in Centigrade. If user temperature is in Kelvin (K) or Rankine (R), enter a negative value. The offset temperature is then set to zero.

21-30

3rd

E

Thermal Properties Evaluation Weight. Default is 0.5

Main Index

PARAMETERS (History Definition) 1413 Definition of Parameters used in Numerical Analysis

Format Fixed 31-40

Free 4th

Data Entry Entry E

Surface projection factor for single step Houbolt. Default is 0.0.

41-50

5th

E

Stefan Boltzmann Constant. Default is 5.67051 x 10-8 W/m2K4.

51-60

6th

E

Planks second constant. Default is 14387.69 μM°K.

61-70

7th

E

Speed of light in a vacuum. Default is 2.9979 x 1014 μM/s

71-80

8th

E

Maximum change in the incremental displacement in a Newton-Raphson iteration. Default is 1 x 1030.

5th data block (Optional) 1-10

1st

E

Initial friction stiffness (only for friction models 6 and 7). This stiffness will be used during the first cycle of an increment to define the friction stiffness matrix in cases where a touching node has a zero normal force and the amount of sliding does not exceed the elastic sticking limit. If set to zero, Marc will estimate the initial friction stiffness based on the initial average stiffness of the contact body to which the touching node belongs.

Main Index

11-20

2nd

E

Specifies the minimum value that indicates a singularity if a direct solver is used. If a zero is given, that this value is set internally by Marc and depends on the solver being used.

21-30

3rd

E

Specify the maximum change in temperature per iteration in radiation simulations. This is useful to stabilize the solution. The default is 100.

31-40

4th

E

Enter parameter alphaf for the generalized alpha dynamic operator. Note that the value of alphaf defined here may be overruled by defining the spectral radius on the 6th field.

1414 PARAMETERS (History Definition) Definition of Parameters used in Numerical Analysis

Format Fixed

Free

Data Entry Entry

41-50

5th

E

Enter parameter alpham for the generalized alpha dynamic operator. Note that the value of alpham defined here may be overruled by defining the spectral radius on the 6th field.

51-60

6th

E

Define the spectral radius S for the generalized alpha dynamic operator. The following conventions apply: • 0 ≤ S ≤ 1 : the 4th and 5th field are ignored and alphaf and alpham

are calculated based upon the spectral radius according to alphaf = - S /(1+ S ) and alpham = (1-2 S )/(1+ S ) • S = – 1 : the 4th and 5th field are ignored and neither alphaf nor alpham will be changed • S = – 2 : the 4th and 5th field are ignored and the values of alphaf and alpham will be optimized for a dynamic contact analysis • S = – 3 : the 4th and 5th field are ignored and the values of alphaf and alpham will be optimized for an analysis without dynamic

contact • S = – 4 : use the values of alphaf and alpham as entered on the 4th

and 5th field 61-70

Main Index

7th

E

RBE3 conditioning number. If the conditioning number is greater than this value, the RBE3 is probably singular and a warning message is printed. If the value is negative, the analysis is stopped. Default is 1 x 106.

SOLVER (History Definition) 1415 Specify Direct or Iterative Solver

SOLVER (History Definition)

Specify Direct or Iterative Solver

Description This option defines the solver to be used in the analysis. You can specify either the direct or iterative solver. The choice of whether the in-core or out-of-core procedure is used is automatically determined by Marc, based upon the amount of workspace required and the amount of memory that can be allocated. You can also select whether a symmetric or nonsymmetric solver is used. Additionally, you can specify if the solution of a nonpositive definite system is to be obtained. For DDM, an out-of-core procedure is only available for solver type 8. As a convenience, it is necessary to specify the control parameters for the decoupled pre-conditioner only in the first domain file, eliminating unnecessary editing. When the iterative solver, type 2 or type 9, is chosen, additional parameters must be defined which are used to control the accuracy. Note:

It is not recommended to use the iterative solver type 2 for beam or shell models, because these problems are ill conditioned, resulting in a large number of iterations. For a wellconditioned system, the number of iterations should be less than the square root of the total number of degrees of freedom in the system. You control the maximum number of iterations allowed. If this is a positive number, Marc stops if this is exceeded. If this is a negative number, Marc prints a warning and continues to the next Newton-Raphson iteration or increment.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SOLVER.

I

Solver Type, enter:

2nd data block 1-5

1st

0 for Profile Direct Solver. 2 for Sparse Iterative. 4 for Sparse Direct Solver 6 for Hardware Provided Direct Sparse Solver 8 for Multifrontal Direct Sparse Solver. 9 for CASI Iterative solver. 10 for mixed direct/iterative solver.

Main Index

1416 SOLVER (History Definition) Specify Direct or Iterative Solver

Format Fixed

Free

Data Entry Entry

6-10

2nd

I

Enter 1 for solving a nonsymmetric system. Only available for solver types 0 and 8. (Not supported for DDM.)

11-15

3rd

I

Enter 1 if the solution of nonpositive definite system is to be obtained.

16-20

4th

I

Enter 0 if standard pre-conditioner is to be used. Enter 3 if decoupled pre-conditioner is to be used. Default value is 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Enter, in millions, the number of four-byte words to be used by solver type 6, 8, or 10 before going out-of-core. Default is the same behavior as for other solvers. For solver type 6, this option is only available on SGI. For solver type 8 or 10, it is available on all platforms.

41-45

9th

Not used; enter 0.

46-50

10th

Not used; enter 0.

51-55

11th

Not used; enter 0.

56-60

12th

Not used; enter 0.

61-65

13th

Not used; enter 0.

66-70

14th

Enter 1 to activate AUTOSPC when singularity occurs. This is only applicable to the direct solvers. Enter -1 to deactivate AUTOSPC.

The 3rd and 4th data blocks are only required for solver type 2 (sparse iterative) or solver type 9 (CASI). They may also be used with the solver type 10. 3rd data block 1-5

1st

I

Enter maximum number of conjugate-gradient iterations. Default is 1000. For solver type 10, set to 0.

6-10

2nd

I

Enter 1 if the previous solution is to be used as the initial trial solution.

11-15

3rd

I

Solver type 2: Enter 3 for diagonal preconditioner. Enter 4 for scaled-diagonal preconditioner. Enter 5 for incomplete Cholesky preconditioner. Solver type 9: Enter 0 for CASI Primal Preconditioner.

Main Index

SOLVER (History Definition) 1417 Specify Direct or Iterative Solver

Format Fixed

Free

Data Entry Entry Enter 1 for CASI Standard Preconditioner. Solver type 10: Enter 0; not used.

4th data block 1-10

1st

F

Enter tolerance on conjugate gradient convergence for stress analysis. The default for solver type 2 is 1.e-3. The default for solver type 9 is 1.e-8. The default for solver type 10 is 1.e-4.

Main Index

1418 POST (History Definition) Create File for Postprocessing

POST (History Definition)

Create File for Postprocessing

Description This option creates a postprocessor file for time-history or variable versus variable plots using Marc Mentat or your own postprocessing. In the latter case, the file is accessed via the PLDUMP utility given in Marc Volume D: User Subroutines and Special Routines. Note:

In a modal or buckling analysis in addition to POST option, the RECOVER history definition option must be used for storing eigenvectors on post file.

Element data is written to the post file for each integration point of a continuum element or for the integration points on the layer requested; unless, either the CENTROID parameter is used or the average value is requested via the 14th field. Note:

The stresses/strains are generally engineering stresses/strains in an analysis involving only small deformations. In a geometrically nonlinear analysis, if the total Lagrangian formulation is used, the stresses and the strains are the second Piola-Kirchhoff stress and the Green-Lagrange strains, respectively. You can always request to output Cauchy stresses (post code 41-47 and 341) in the post file. If the updated Lagrangian formulation is used in the large deformation analysis, the stresses and the strains are generally Cauchy stresses and the logarithmic strains, respectively.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-4

1st

A

Enter the word POST.

I

Number of element variables to be written on the file (optional)

2nd data block 1-5

1st

For heat transfer, by default, the temperatures are written to a post file. Enter -1 to suppress the default. Enter -2 if both element and nodal post codes are not changed in this loadcase.

Main Index

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

POST (History Definition) 1419 Create File for Postprocessing

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Not used; enter 0.

36-40

8th

I

Not used; enter 0.

41-45

9th

I

Number of increments between writing of post data. Defaults to writing to the post file every increment. Enter -1 if the number of increments is not changed in this loadcase.

46-50

10th

I

Not used; enter 0.

51-55

11th

I

Enter 0 to use the elements in last post option. Enter 1 to select elements to be written to post files. Enter 2 for all elements to be written to post files.

56-60

12th

I

Not used; enter 0.

61-65

13th

I

Not used; enter 0.

66-70

14th

I

Enter 1 if per element only the average element integration point data should be written on the post file. This might considerably reduce the size of the post file, but some significant information might be lost. The default is 0 where the element data is written on the post file for all available integration points. Only needed if the 1st field of the 2nd data block is not a -2.

71-75

15th

I

Enter 1 if automatically generated extra nodes associated with element types 80-84 and 155-157 do not appear on the post file. The default is 0, where all the available nodes are written on the post file. Only needed if the 1st field of the 2nd data block is not a -2.

76-80

16th

I

Enter 1 to exclude forces caused by glued contact from the contact normal and friction forces. The default is 0 where the contact normal and friction forces also contain the contributions due to glued contact. Only needed if the 1st field of the 2nd data block is not a -2.

Data blocks 3 and 4 are used for input of variables to be written on the post file. They are only needed if the 1st field of the 2nd data block is not -2. 3rd data block Use for defining element post codes.

Main Index

1-10

1st

A

Enter the word ELEMENT.

11-15

2nd

I

Enter an element post code. The code numbers are described in Table 4-3.

1420 POST (History Definition) Create File for Postprocessing

Format Fixed 16-20

Free 3rd

Data Entry Entry I

Enter the layer number for shell elements or continuum composite elements. For post codes 471 and 481, enter the global identification number of the rebar layer

21-68

4th

A

Enter a 48-character label associated with this post code for use in postprocessing.

4th data block Use for defining nodal post codes. 1-10

1st

A

Enter the word NODAL.

11-15

2nd

I

Enter a nodal post code. The code numbers are described in Table 4-4.

16-63

3rd

A

Enter a 48-character label associated with this post code for use in postprocessing.

Data blocks 5, 6, and 7 are only needed if the 11th field of the 2nd data block is 1. 5a data block 1-10

1st

A

Enter the words SELECT ELEMENT

I

Enter a list of elements to be written to post file.

5b data block 1-80

1st

6a data block 1-10

1st

A

Enter the words SELECT BODY

11-15

2nd

I

Enter 1 if all elements of the selected contact body are placed on post file (default) Enter 2 if only the elements on the exterior surface are placed on the post file.

6b data block 1-80

I

Enter a list of contact bodies, for which the elements are to be written to post file.

For the 7th data block, these nodes are in addition to nodes based upon element selection; typically, it is used for nodes not associated with elements. 7a data block 1-10

1st

A

Enter the words SELECT NODE

I

Enter a list of nodes to be written to post file.

7b data block 1-80

Main Index

POST (History Definition) 1421 Create File for Postprocessing

Table 4-3

Element Post Codes

Codes 1-6

Components of strain. For rigid-perfectly plastic flow problems, components of strain rate

7

Equivalent plastic strain (integral of equivalent plastic strain rate). For rigid-perfectly plastic flow problems, equivalent plastic strain rate

8

Equivalent creep strain (integral of equivalent creep strain rate)

9

Total temperature

10

Increment of temperature

11-16

Components of stress

17

Equivalent von Mises stress

18

Mean normal stress (tensile positive) for Mohr-Coulomb

19

User-defined variable via the PLOTV user subroutine. See Marc Volume D: User Subroutines and Special Routines.

20

Thickness of element

21-26

Components of plastic strain

27

Main Index

Description

Equivalent plastic strain. ε

p

2--Σ Δ ε ipj ΣΔ ε ijp 3

=

28

Plastic strain rate

29

Total value of second state variable

30

Forming Limit Parameter: FLP = calculated major engineering strain/maximum major engineering strain

31-36

Components of creep strain

37

Equivalent creep strain. ε

38

Total swelling strain (from the VSWELL user subroutine)

39

Total value of third state variable

41-46

Components of Cauchy stress

47

Equivalent Cauchy stress

48

Strain energy density

49

Thickness strain for plane stress: Mooney or Ogden material

51-56

Real components of harmonic stress

57

Equivalent real harmonic stress

58

Elastic strain energy density

59

Equivalent stress/yield stress

60

Equivalent stress/yield stress (at current temperatures)

c

=

2--ΣΔ ε icj Σ Δε ijc 3

1422 POST (History Definition) Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Main Index

Description

61-66

Imaginary components of harmonic stress

67

Equivalent imaginary harmonic stress

68

Plastic strain energy density

69

Current volume

71-76

Components of thermal strain

78

Original volume

79

Grain size

80

Damage indicator for Cockroft-Latham, Oyane, and Principal Stress criteria, and criteria using the UDAMAGE_INDICATOR user subroutine.

81-86

Components of cracking strain (only for stress analysis)

91-107

Failure indices associated with failure criteria

108-109

Interlaminar shear for thick composite shells (TSHEAR parameter must be present)

110

Interlaminar shear bond index for thick composite shells (only available if TSHEAR parameter is present and Allowable Shear Bond Stress, SB, has been prescribed on the COMPOSITE option) = max(Interlaminar shear components given by post codes 108 and 109)/SB

111-116

Components of stress in preferred coordinate system defined by the ORIENTATION option

121-126

Elastic strain

127

Equivalent elastic strain

128

Major engineering strain

129

Minor engineering strain

175

Equivalent viscoplastic strain rate (powder material)

176

Relative density (powder material)

177

Void volume fraction (damage model)

178

Lemaitre damage factor

179

Lemaitre relative damage

<0

User-defined variable via the PLOTV user subroutine. See Marc Volume D: User Subroutines and Special Routines.

241

Gasket Pressure

242

Gasket Closure

243

Plastic Gasket Closure

251

Global components of Interlaminar normal stress; layer n is between n and n+1

254

Global components of Interlaminar shear stress; layer n is between n and n+1

POST (History Definition) 1423 Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Description

257

Interlaminar shear bond index for composite solids (only available if Allowable Shear Bond Stress, SB, has been prescribed on the COMPOSITE option) = magnitude of interlaminar shear vector calculated by post code 254/SB

261

Beam axis (required if beam moment plots are created with Marc Mentat). Orientation axis of CBUSH/CFAST elements 194 and 195.

264

Axial Force

265

Moment Mxx

266

Moment Myy

267

Shear Force Vxz

268

Shear Force Vyz

269

Torque

270

Bimoment

301

Total strains tensor

311

Stress tensor

321

Plastic strain tensor

331

Creep strain tensor

341

Cauchy stress tensor

351

Real harmonic stress tensor

361

Imaginary harmonic stress tensor

371

Thermal strain tensor

381

Cracking strain tensor

391

Stresses in preferred direction tensor

401

Elastic strain tensor

411

Stress in global coordinate system tensor

421

Elastic strain in global coordinate system tensor

431

Plastic strain in global coordinate system tensor

441

Creep strain in global coordinate system tensor

451

Velocity strains (for fluids)

461

Elastic strain in preferred direction tensor

471

Global components of the rebar stresses in the undeformed configuration (Second Piola-Kirchhoff). See Marc Volume B: Element Library for details.

481

Global components of the rebar stress in the deformed configuration (Cauchy). See Marc Volume B: Element Library for details.

Main Index

1424 POST (History Definition) Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Description

487

Rebar angle.

501

Interlaminar normal stress; layer n is between n and n+1. See Marc Volume B: Element Library for details.

511

Interlaminar shear stress; layer n is between n and n+1. See Marc Volume B: Element Library for details.

531

Volume fraction of Martensite.

541

Phase transformation strain tensor.

547

Equivalent Phase Transformation strain PH = ε eq

548

Equivalent TWIN Strain T WIN = ε eq

549

IP 2 ⁄ 3 Σ Δε ijTRI P Σ Δ ε iTR j

Equivalent Plastic Strain in the Multiphase Aggregate: PL = ε eq

Main Index

2 ⁄ 3 ΣΔ ε ijTWI N Σ Δ ε ijTWI N

Equivalent TRIP Strain in the forward transformation T RIP = ε eq

551

2 ⁄ 3 ΣΔ ε ijPH Σ Δ ε ijPH

PL 2 ⁄ 3ΣΔ ε iPL j Σ Δ εi j

552

Equivalent Plastic Strain in the Austenite

553

Equivalent Plastic Strain in the Martensite

557

Yield Stress of Multiphase Aggregate

601-617

Strength ratios based upon FAIL DATA failure modes.

621

Generalized Strain (Harmonic only)

631

Imaginary Generalized Strain (Harmonic only)

641

Generalized Strain - curvatures tensor

661

Generalized Stress - Moments tensor

681

True Strain Tensor (for continuum elements)

691

Element Orientation Vector 1

694

Element Orientation Vector 2

697

Layer Orientation Angle

POST (History Definition) 1425 Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Description

Post Codes for Heat Transfer Analysis 9 or 180

Total temperature

181-183

Components of temperature gradient T

184-186

Components of flux

271

Volumetric Mass density of pyrolysised solid (model C) or nonhomogeneous density

272

Volumetric Mass density of pyrolysis gas (model C)

273

Volumetric Mass density of liquid (model C)

274

χp

(Pyrolysis model B or C)

275

φw

(Pyrolysis model B or C)

276

χc

(Pyrolysis model B or C)

277

ρc

278

k

279

ρ g, w

280

mg

281

· ρ s, p

(Pyrolysis model C only)

282

· ρ s, l

(Pyrolysis model C only)

283

· ρ s, c

(Pyrolysis model C only)

ef f

eff

(Pyrolysis model B or C)

(Pyrolysis model B or C) Pyrolysis Volumetric Mass density of water vapor

(Pyrolysis model B or C)

Post Codes for Bearing Analysis 190

Pressure

191-193

Components of pressure gradient

194-196

Mass flux vector

Post Codes for Joule Heating Analysis 87

Voltage

88

Current

89

Heat generated

197-199

Components of electric potential gradient

577-579

Components of current density

Post Codes for Acoustic Analysis

Main Index

190

Pressure

191-193

Components of pressure gradient

1426 POST (History Definition) Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Description

Post Codes for Electrostatic Analysis 130

Electric potential (V)

561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

Post Codes for Magnetostatic Analysis 140

Magnetic potential (2-D analysis only) (Az)

571-573

Components of magnetic induction (B)

574-576

Components of magnetic field intensity (H)

Post Codes for Transient Electromagnetic Analysis 561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

567-569

Components of Lorentz force

571-573

Components of magnetic induction (B)

574-576

Components of magnetic field intensity (H)

577-579

Components of current density (J)

Post Codes for Harmonic Electromagnetic Analysis 131-133

Real components of electric field intensity (E)

134-136

Real components of electric displacement (D)

137-139

Real components of Lorentz force

141-143

Real components of magnetic induction (B)

144-146

Real components of magnetic field intensity (H)

147-149

Real components of current density (J)

151-153

Imaginary components of electric field intensity (E)

154-156

Imaginary components of electric displacement (D)

157-159

Imaginary components of Lorentz force

161-163

Imaginary components of magnetic induction (B)

164-166

Imaginary components of magnetic field intensity (H)

167-169

Imaginary components of current density (J)

Post Codes for Piezoelectric Analysis (Electrical Part)

Main Index

561-563

Components of electric field intensity (E)

564-566

Components of electric displacement (D)

POST (History Definition) 1427 Create File for Postprocessing

Table 4-3

Element Post Codes (continued)

Codes

Description

Post Codes for Harmonic Piezoelectric Analysis (Electrical Part) 131-133

Real components of electric field intensity (E)

134-136

Real components of electric displacement (D)

151-153

Imaginary components of electric field intensity (E)

154-156

Imaginary components of electric displacement (D)

Post Codes for Soil Analysis 171

Porosity

172

Void ratio

173

Pore pressure

174

Preconsolidation pressure

Post Codes for Cure and Cure Shrinkage Analysis 285

Degree of cure

286

Total cure reaction heat

287

Degree of cure shrinkage

288

Volumetric cure shrinkage of resin

289-294

Cure shrinkage strain components in global coordinate system

295-300

Cure shrinkage strain components in preferred coordinate system

581-586

Cure shrinkage strain tensor in global coordinate system

591-596

Cure shrinkage strain tensor in preferred coordinate system

Notes:

For heat transfer, code 9 is used for all heat transfer elements. When using shells in heat transfer, it is important to enter a code for each layer in chronological order if post file is to be correctly read by the INITIAL STATE or CHANGE STATE options. Note that you do not need to select nodal values (that is, displacement, velocities and accelerations, and temperature for a heat transfer run) as these are automatically written to the post file. Eigenmodes (dynamic analysis) and eigenvectors (buckling analysis) are written to the post file only if indicated by the RECOVER or MODAL INCREMENT/BUCKLE INCREMENT option.

Main Index

1428 POST (History Definition) Create File for Postprocessing

Note that post codes 91-107 refer to failure indices for different failure criteria and post codes 601-617 refer to associated strength ratios. More than 17 quantities are allowed in the analysis but only the first 17 quantities are available for postprocessing. For example. if three failure criteria (say, max. stress, Hoffman and Puck) are flagged, post codes 9197/601-607 would contain the six indices/ratios associated with maximum stress, post code 98 / 608 would contain the one index / ratio associated with Hoffman and post codes 99103 / 609-613 would contain the five indices / ratios associated with Puck criterion. Post codes 691 and 694 provide access to the first and second orientation vectors respectively. These vectors depict the alignment of the material coordinate system at the element level with respect to the global cartesian system. They are available for elements that are either composites, or using materials that are orthotropic/anisotropic / requiring the HOOKLW ANELAS user subroutines, or using the ORIENTATION option to identify the material coordinate system. Note that these element orientation vectors are averaged across all integration points of the element and presented as a single set of vectors at the element centroid. They are always calculated on the current element geometry and any layer IDs associated with post codes 691 and 694 are ignored. Note also that while the normal usage of these post vectors is in conjunction with the ORIENTATION option, if no special material orientation is provided, then they can also be used to obtain the element coordinate system for orthotropic materials, composites, etc. For composites, post code 697 provides access to the fiber angle in any layer. If used without any associated layer id, post code 697 provides access to all layer angles. Else, the user can obtain the angle for a specific layer L by using 697,L as the post code. Note that if there are no composite elements, post code 697 is ignored. The orientation vectors on the post file are available for visualization in Marc Mentat. Either element orientations or layer orientations can be plotted. Note that for layer orientation vectors to be available for a set of layers, the associated layer orientation angle should be available on the post file through post code 697. For post codes 411, 421, 431, and 441, global quantities for shell elements are reported for as many layers as requested and the same layer numbering system is used as for regular shell quantities. Layer 1 is the top surface; layer 2 is the next surface, etc. This convention is followed from MSC.Marc 2000 on.

Main Index

POST (History Definition) 1429 Create File for Postprocessing

Caution has to be exercised in interpreting the results when strain and/or stress tensors are requested for beam and shell elements: 1.For most elements in this category (elastic beam elements 31, 52, 98 are exceptions), stress tensors (post codes 311, 351, 361) or their associated component values (post codes 11-16, 51-56, 61-66) and total strain tensor (post code 301) or its associated component values (post code 1-6) can be requested with or without an associated layer number. When no layer number is requested, the generalized strains (stretches, shear strains) are reported for the strain post values and generalized stresses (axial force, shear forces) are reported for the stress post values. Generalized curvature strains and generalized moments can be requested through post codes 641, 651, 661, and 671 for shells and numerically integrated beams. Note that for shell elements, the generalized stresses are forces per unit length. Refer to Marc Volume B: Element Library for a definition of the generalized strain and stress output for each element type. When a layer number is used, the actual strain and stress components at the requested layer are reported. 2.For elastic beams (types 31, 52, 98), there are no layers - so only the generalized strains and stresses are reported for these elements. Refer to Marc Volume B: Element Library for a definition of the generalized strain and stress output for each element type. Equivalent quantities are not computed for these element types since they do not make physical sense. 3.For other stress tensors (post codes 341, 391, 411) and strain tensors (post codes 321, 331, 371, 381, 401, 421, 431, 441, 461), there are no generalized values and they can only be requested for a particular layer. If no layer number is provided by the user, by default, the tensors are reported for layer number 1. For elastic beams (types 31, 52, 98), only the thermal strain tensor (post code 371) or its associated components (post codes 71-76) are available.

Main Index

1430 POST (History Definition) Create File for Postprocessing

Table 4-4

Nodal Post Codes

Code 1 Displacement 2 Rotation 3 External Force 4 External Moment 5 Reaction Force 6 Reaction Moment 7 Fluid Velocity 8 Fluid Pressure 9 External Fluid Force 10 Reaction Fluid Force 11 Sound Pressure 12 External Sound Source 13 Reaction Sound Source 14 Temperature 15 External Heat Flux 16 Reaction Heat Flux 17 Electric Potential 18 External Electric Charge 19 Reaction Electric Charge 20 Magnetic Potential 21 External Electric Current 22 Reaction Electric Current 23 Pore Pressure 24 External Mass Flux 25 Reaction Mass Flux 26 Bearing Pressure 27 Bearing Force 28 Velocity 29 Rotational Velocity 30 Acceleration 31 Rotational Acceleration 32 Modal Mass

Main Index

Description

POST (History Definition) 1431 Create File for Postprocessing

Table 4-4

Nodal Post Codes (continued)

Code

Description

33 Rotational Modal Mass 34 Contact Normal Stress 35 Contact Normal Force 36 Contact Friction Stress 37 Contact Friction Force 38 Contact Status 39 Contact Touched Body 40 Herrmann Variable 41

ρ sol id

42

M· g

43

· ρ s, p

(Pyrolysis Model B only)

44

· ρ s, l

(Pyrolysis Model B only)

(Pyrolysis Model B only)

(Pyrolysis Model B or C)

46 Tying Force 47 Coulomb Force 48 Tying Moment 49 Generalized Nodal Stress 50 Generalized Nodal Strain 51 Inertia Relief Load 52 Inertia Relief Moment 53 J-Integral 54 Stress Intensity, Mode I 55 Stress Intensity, Mode II 56 Stress Intensity, Mode III 57 Energy Release 58 Energy Release Rate I 59 Energy Release Rate II 60 Energy Release Rate III 61 — 62 Crack System Local X 63 Crack System Local Y 64 Crack System Local Z

Main Index

1432 POST (History Definition) Create File for Postprocessing

Table 4-4

Nodal Post Codes (continued)

Code

Description

65 Near Contact Distance 66 Breaking Index (Normal) 67 Breaking Index (Tangential) 68 Breaking Index 69 Delamination Index (Normal) 70 Delamination Index Tangential) 71 Delamination Index 72 Recession 73 Glue Deactivation Status 74 VCCT Failure Index <0 User-defined nodal quantity via the UPSTNO user subroutine.

Note: The contact status (code 38) can have the following values: 0 if a node is neither in contact nor has tying constraints due to cyclic symmetry. 0.5 if a node is in near contact. 1 if a node is in true contact. 2 if a node has tying constraints due to cyclic symmetry.

Main Index

POST INCREMENT 1433 Define Increments between Writing on Post File

POST INCREMENT

Define Increments between Writing on Post File

Description This option allows you to alter the increments at which data is written to the post file. This option has the same effect as the data in the ninth field of the POST model definition option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POST INCREMENT.

I

Enter the number of increments between writing of post data. Defaults to write post file very increment.

2nd data block 1-5

1st

Enter a -1 to turn off all writing of post data until the next POST INCREMENT option. 6-10

2nd

I

Enter number of times data will be written to the post file for each load case. The step is calculated based on the progress from the total load case time, displacement, or energy. This control is used only if there is no increment frequency control in the first field. Enter 1 if the post file is to be written at the end of the load case only. Default is 0 (no such control).

11-15

3rd

Notes:

I

Not used; enter 0.

Post data is automatically written to the post file at the increment in which the POST INCREMENT option occurs.

This value is not saved upon restart; it must be reset through the POST model definition option or POST INCREMENT option. Example POST INCREMENT 2 writes every other increment to the post file beginning with the current increment.

Main Index

1434 POST INCREMENT Define Increments between Writing on Post File

POST INCREMENT 05 writes five steps in the post file for the current loadcase. Based upon the progress check, the steps that need output will be at about 20%, 40%, 60%, 80%, and 100% of the progress report. Progress check is based upon the total loadcase time, displacement, or energy.

Main Index

RESTART INCREMENT 1435 Define Increments between Writing on Restart File

RESTART INCREMENT

Define Increments between Writing on Restart File

Description This option allows you to alter the increments at which restart data is written to the restart data file. This option has the same effect as the data in the second field of the RESTART model definition option. This does not effect the RESTART LAST option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words RESTART INCREMENT.

I

Enter the number of increments between writing of the restart data.

2nd data block 1-5

1st

It defaults to writing of restart data every increment. Enter -1 to stop all writing of restart data until the next RESTART INCREMENT option.

Notes:

Restart data is automatically written to the restart file at the increments in which the RESTART INCREMENT option occurs.

This value is not saved upon restart; it must be reset through the RESTART model definition or RESTART INCREMENT option. Example RESTART INCREMENT 2 writes every other increment to the restart file beginning with the current increment.

Main Index

1436 ADAPT GLOBAL (History Definition) Define Meshing Parameters Used in Global Remeshing

ADAPT GLOBAL (History Definition)

Define Meshing Parameters Used in Global Remeshing

Description This history definition set provides control parameters used for the global remeshing. The REZONING parameter must also be included in the parameter section. The ADAPT GLOBAL history definition option can also be used to support boundary conditions assigned to the remeshing body for 2-D, 3-D solid (tetrahedral) and 3-D shell. When applying boundary conditions, the new table style input format is preferred. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the words ADAPT GLOBAL.

2nd data block 1-5

1st

I

Enter the number of bodies to be remeshed.

6-10

2nd

I

Enter the unit number to read data; defaults to input.

11-15

3rd

I

Not used.

The 3rd through 5th data blocks are repeated as a set for each body to be remeshed. 3rd data block 1-5

1st

I

Enter 2 for Advancing Front 2-D quad or mixed mesher. Enter 3 for Delaunay 2-D mesher. Enter 4 for 2-D Overlay mesher. Enter 5 for 3-D Overlay Hexahedral mesher. Enter 6 for Delaunay 3-D tetrahedral mesher. Enter 7 for Relax mesh generator. Enter 8 for Stretch mesh generator. Enter 9 for Shave mesh generator. Enter 10 for quadtree mesher. (FEMUTEC externally supplied) Enter 11 for MD Patran 3-D tetrahedral meshers. Enter 12 for triangular shell mesh generator. Enter 18 for reading new mesh from .mesh file. Note:

Main Index

jobid_b*.mesh file name is expected where * is the remeshing body number and jobid is the job name.

ADAPT GLOBAL (History Definition) 1437 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry Enter 19 for quadrilateral shell mesh generator.

6-10

2nd

I

Enter 1 to remesh body (default). Enter 2 if first relax mesh; if that fails, do full remeshing. Enter 3 if relax mesh only.

11-15

3rd

I

Enter the body to be remeshed (default = 1).

16-20

4th

I

Enter the element type; default is to previous element type. Note:

This element type must also be specified on the ELEMENTS parameter.

21-25

5th

I

Enter the number of criteria.

26-30

6h

I

Not used; enter 0.

31-35

7th

I

Echo mode for Overlay Hexahedral Meshing 0 Default; no message print out. 1 Some message print out. 100 Prints out more messages and saves all the meshing input files. For details about these files, see Appendix I: 3-D Remeshing Files.

Repeat the 4th block for each criteria (5th field, 3rd data block). 4th data block 1-5

1st

I

Enter 1 if increment frequency is used. Enter 2 if element distortion is used (2-D only). Enter 3 if angle based. Enter 4 if aspect ratio based. Enter 5 if strain change. Enter 6 if penetration based. Enter 7 if force remeshing at next opportunity. Enter 8 if recession distance based.

6-10

2nd

I

Enter the frequency in increments if criteria 1.

11-20

3rd

E

For criteria 3, enter maximum change in angle from the reference angle for quadrilaterals. Default is 40°. The reference angle is the angle of the current mesh without deformation. For 3-D analysis, enter minimum volume ratio for hexahedral element. Default is 0.1. For criteria 4, enter the maximum aspect ratio allowed. Default is 10.0. For criteria 5, enter maximum change of equivalent strain allowed before remeshing occurs.

Main Index

1438 ADAPT GLOBAL (History Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry Default is 0.4. For criteria 6, enter the penetration limit; default is 2*contact tolerance. For criteria 8, enter the maximum element side reduction fraction before remeshing occurs. If current length divided by the original length < tolerance, remeshing will occur.

21-30

4th

E

For criteria 3, enter maximum change in angle from the reference angle for triangles. Default is 40°. The reference angle is the angle of the current mesh without deformation. For 3-D analysis, enter minimum volume ratio for tetrahedral element. Default is 0.1. For criteria 8, enter the total amount of recession before remeshing occurs.

5th data block (Two-dimensional Advancing Front All Quadrilateral or Mixed Mesher) Mesher type = 2 1-5

1st

I

Enter 0 for all quadrilateral mesh. Enter 1 for mixed quadrilateral/triangular mesh. Enter 2 for all triangular mesh.

6-15

2nd

E

Enter the target element size.

16-25

3rd

E

Enter outline vertex angle of the two adjacent segments. (Default = 120°)

26-30

4th

I

Target number of elements after remeshing; default means no such control. If both the 2nd and 4th fields are default, the number of elements in the previous mesh are used.

31-35

5th

I

Curvature outline control. Enter number of divisions of line segments to fit a curvature circle. Default = 36. Enter -1 to obtain uniform outline points.

Main Index

36-45

6th

E

Outline smoothing ratio range 0 - 1.0; default = 0.8.

46-55

7th

E

Minimum target element size; default = 1/3*target element size.

56-65

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

66-75

9th

E

Not used; enter 0.

76-80

10th

I

Number of local refinement boxes.

ADAPT GLOBAL (History Definition) 1439 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

5th data block (Two-dimensional Delaunay Triangular Mesher) Mesher type = 3 1-5

1st

I

Not used; enter 0.

6-15

2nd

E

Enter the target element size.

16-25

3rd

E

Enter outline vertex angle of the two adjacent segments (default 120°).

26-30

4th

I

Target number of elements after remeshing; default means no such control.

31-35

5th

I

Curvature outline control. Enter number of divisions of line segments to fit a curvature circle. Default = 36. Enter -1 to obtain uniform outline points.

36-45

6th

E

Outline smoothing ratio range 0-1.0; default = 0.8.

46-55

7th

E

Minimum target element size; default = 1/3*target element size.

56-65

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

66-75

9th

E

Not used; enter 0.

76-80

10th

I

Number of local refinement boxes.

5th data block (Two-dimensional Overlay Quadrilateral Mesher) Mesher type = 4 1-10

1st

E

Enter the element target length.

11-15

2nd

I

Enter 1 if elements on the boundary in contact are to be refined one level if necessary. Enter 2 if elements on the boundary in contact are to be refined two levels if necessary.

Main Index

16-20

3rd

I

Enter 1 if elements in the interior can be merged together. Four elements at a time will be merged.

21-25

4th

I

Target number of elements after remeshing; default means no such control.

26-30

5th

I

Not used; enter 0.

31-40

6th

E

Not used; enter 0.

41-50

7th

E

Not used; enter 0.

51-60

8th

E

Percentage of change allowed for the new number of elements created. Default means no such control. Total of five remeshing trials will be used to create the mesh to meet the requirement. Not to be used for the remeshing with the automatic stop-and-restart option.

1440 ADAPT GLOBAL (History Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

5th data block (Three-dimensional Delaunay Tetrahedral Mesher) Mesher type = 6 1-10

1st

E

Enter target atom size (A).

11-20

2nd

E

Enter edge parameter (value is between 0.0 and 1.0). A value of 1 means that all element edges between elements not in the same plane will be considered a hard edge.

21-30

3rd

E

Minimum edge length.

31-40

4th

E

Minimum edge angle.

41-50

5th

E

Gap distance.

51-55

6th

I

Not used; enter 0.

56-60

7th

I

Enter 1 for volume control.

5th data block (Relax Mesh Generator) Mesher type = 7 1-5

1st

I

Enter the number of relaxes to be performed.

6-10

2nd

I

Enter the global direction to relax in, default is all directions.

11-20

3rd

E

Enter the sweep distance, nodes closer than this distance will be swept together.

5th data block (Stretch Generator) Mesher type = 8 1-5

1st

I

Enter the first corner node number, if zero, then the second field gives the streamline region that is used to define the stretching orientation.

6-10

2nd

I

Enter the node increment in first direction, or the streamline region number.

11-15

3rd

I

Enter number of nodes in first direction. Enter the contact body which if nodes contact, they should not be adjusted, if zero all nodes will be adjusted.

16-20

4th

I

Enter the node increment in second direction.

21-25

5th

I

Enter the number of nodes in second direction.

26-30

6th

I

Enter the node increment in third direction (3-D only).

31-35

7th

I

Enter the number of nodes in third direction (3-D only).

5th data block (Shave Mesh Generator) Mesher type = 9 This 5th data block is not required. 5th data block (Three-dimensional MD Patran Tetrahedral Mesher) Mesher type = 11

Main Index

1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

ADAPT GLOBAL (History Definition) 1441 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Number of local refinement boxes; default = 0.

56-60

7th

I

Enter 1 for volume control; default = 1.

61-65

8th

I

Curvature refinement control. Enter number of division to fit a curvature cycle. Default = 0 (no such control).

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Three-dimensional Triangular Shell Mesher) Mesher type = 12 1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Number of local refinement boxes; default = 0.

56-60

7th

I

Not used; enter 0.

61-65

8th

I

Curvature refinement control. Enter number of division to fit a curvature cycle. Default = 0 (no such control).

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Three-dimensional Triangular Shell Mesher) Mesher type = 19

Main Index

1-10

1st

E

Enter target element edge length.

11-20

2nd

E

Minimum element edge length; default 1/3 of the element edge length.

21-30

3rd

E

Feature vertex angle; default 100°.

31-40

4th

E

Feature edge angle; default 60°.

41-50

5th

E

Interior coarsening factor; default 1.5 times.

51-55

6th

I

Not used; enter 0.

56-60

7th

I

Not used; enter 0.

1442 ADAPT GLOBAL (History Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

61-65

8th

I

Not used; enter 0.

66-70

9th

I

Enter number of elements in the target mesh. Default = 0 (no such control).

71-80

10th

E

Enter maximum element edge length. Default = 3*element edge length.

5th data block (Reading .mesh file) Mesher type = 18 1-10

1st

I

Enter mesh file type. Default = 3. Enter 1 for mesh file in .t18 format Enter 2 for mesh file in .feb format Enter 3 for mesh file in .dat format (Marc input format)

5th data block (Three-dimensional Overlay Hexahedral Mesher) Mesher type = 5 1-10

1st

E

Enter target atom size (Ax). For cylindrical grid, Ar.

11-20

2nd

E

Enter target atom size (Ay). For cylindrical grid, AË.

21-30

3rd

E

Enter target atom size (Az).

31-40

4th

E

Enter edge parameter (value is between 0.0 and 1.0). A value of 1 means that all element edges between elements not in the same plane will be considered a hard edge.

41-50

5th

E

Minimum edge length. If an edge length is less than this value, it will not be considered as a hard edge.

51-60

6th

E

Minimum edge angle. If the angle between element faces is less than this value, the common edge will not be considered as a hard edge.

61-70

7th

E

Gap distance.

71-75

8th

I

The template file name is specified on the 9th data block. Enter 1 if grid-based template Enter 2 if mesh-based template. Enter 3 if kernel-based template.

76-80

9th

I

Enter 1 for volume control.

6th data block (Two-dimensional Advancing Front or Delaunay Mesher [If refinement boxes are used]) Repeat for each box (6th field, 5th data block) 1-5

1st

I

Enter refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in box.

Main Index

ADAPT GLOBAL (History Definition) 1443 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

11-15

3rd

I

Body ID 1; if not zero, corner 1 will be attached to this rigid body.

16-20

4th

I

Body ID 2; if not zero, corner 2 will be attached to this rigid body.

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

8th

F

Enter x coordinate of corner 2.

51-60

9th

F

Enter y coordinate of corner 2.

6th data block (Three-dimensional MD Patran Tetrahedral Mesher [If refinement boxes are used]) Repeat for each box (6th field, 5th data block) 1-5

1st

I

Enter refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in box.

11-15

3rd

I

Body ID 1. If not 0, corner 1 will be attached to this rigid body.

16-20

4th

I

Body ID 2. If not 0, corner 2 will be attached to this rigid body.

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

7th

F

Enter z coordinate of corner 1.

51-60

8th

F

Enter x coordinate of corner 2.

61-70

9th

F

Enter y coordinate of corner 2.

71-80

10th

F

Enter z coordinate of corner 2.

6th data block (Two-dimensional Quadtree Mesher or 3-D Hexahedral Mesher) 1-5

1st

I

Number of boxes used for element refinement; entered on 10th series.

6-10

2nd

I

Enter number of levels to coarsen (merge) the interior elements.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 0 for no wedge elements Enter 1 to allow wedge elements. Enter to split hexahedral elements.

31-35

7th

I

Enter 1 to perform shuffle after mesh is snapped to contact surface (default). Enter 2 to avoid shuffle.

Main Index

1444 ADAPT GLOBAL (History Definition) Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

36-40

8th

I

Enter 1 for Coons projection in meshing phase. This improves the accuracy, but increases the cost.

41-45

9th

I

Number of shakes. Default is 10.

46-50

10th

I

Number of tries. Default is 5.

51-55

11th

I

Type of enhancement.

56-60

12th

I

Edge detection: Enter 0 to detect new edges and use contact data. Enter 1 to use contact data only. Enter 2 to detect new edges. Enter 3 to not use edge information. Enter 4 to use previously detected edges, new edges, and contact information. Enter 5 to use contact data and previous edges. Enter 6 to use user edges previously detected and new edges. Enter 7 to use previous edge information only.

7th data block (Three-dimensional Overlay Hexahedral Mesher Only) 1-5

1st

I

Grid type: Enter 1 for Cartesian (default). Enter 2 for cylindrical. Enter 3 for user defined.

6-10

2nd

I

For cylindrical grid: Enter 1 for axis aligned with x-direction. Enter 2 for axis aligned with y-direction. Enter 3 for axis aligned with z-direction.

11-15

3rd

I

Maximum allowed refinement levels.

16-20

4th

I

First user-defined integer parameter.

21-25

5th

I

Second user-defined integer parameter.

26-30

6th

I

Third user-defined integer parameter.

8th data block (Three-dimensional Overlay Hexahedral Mesher Only [Version 11 only])

Main Index

1-10

1st

F

For cylindrical grid, enter the angle of the part.

11-20

2nd

F

Enter the geometric refinement tolerance.

21-30

3rd

F

Enter the surface curvature tolerance.

ADAPT GLOBAL (History Definition) 1445 Define Meshing Parameters Used in Global Remeshing

Format Fixed

Free

Data Entry Entry

31-40

4th

F

First user-defined real parameter.

41-50

5th

F

Second user-defined real parameter.

51-60

6th

F

Third user-defined real parameter.

9th data block (Three-dimensional Overlay Hexahedral Mesher Only and Template-based Mesh Requested) 1-32

1st

A

Enter the template name.

10th data block (Three-dimensional Overlay Hexahedral Mesher [if refinement boxes are used]) One can either specify that refinement is in a box based upon coordinate positions or between two bodies. Repeat for each box (1st field, 6th data block) 1-5

1st

I

Enter the refinement level.

6-10

2nd

I

Enter the refinement type: 0 = refinement in the box. 1 = minimum number of elements in x-direction between bodies. 2 = minimum number of elements in y-direction between bodies. 3 = minimum number of elements in z-direction between bodies. 4 = exact number of elements in x-direction between bodies. 5 = exact number of elements in y-direction between bodies. 6 = exact number of elements in z-direction between bodies.

Main Index

11-15

3rd

I

Body ID 1. If refinement is in the box, corner 1 is attached to this rigid body

16-20

4th

I

Body ID 2. If refinement is in the box, corner 2 is attached to this rigid body

21-30

5th

F

Enter x coordinate of corner 1.

31-40

6th

F

Enter y coordinate of corner 1.

41-50

7th

F

Enter z coordinate of corner 1.

51-60

8th

F

Enter x coordinate of corner 2.

61-70

9th

F

Enter y coordinate of corner 2.

71-80

10th

F

Enter z coordinate of corner 2.

1446 LOADCASE (History Definition) Define Loadcase

LOADCASE (History Definition)

Define Loadcase

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option is used to specify the boundary conditions and initial conditions that are active in this loadcase. This is used to activate or deactivate FIXED DISP, FIXED TEMPERATURE, etc., DIST LOADS, DIST FLUXES, etc., POINT LOAD, POINT FLUX, etc., FOUNDATION, FILMS, INITIAL DISP, INITIAL VEL, INITIAL TEMP, etc. Boundary conditions not explicitly activated are deactivated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word LOADCASE.

11-32

2nd

A

Enter the name of the loadcase (no blanks).

I

Enter the number of labels. This is required.

2nd data block 1-5

1st

3rd data block (Repeat as many times as specified on 2nd data block.) 1-32

1st

A

Enter the boundary condition or initial condition label.

33-40

2nd

I

Enter flag to control application of this boundary condition. This is applicable to FIXED DISP, DIST LOADS, POINT TEMP, and CHANGE STATE only. If a time dependent table (independent variable types 1,2,3,4) is applied to this boundary condition, this flag is ignored and the table is used to control the temporal variations. Enter 0 if load is applied instantaneously, or if boundary condition has been previously activated, it remains constant (default). Enter 1 if point load, distributed load or kinematic load is to be linearly changed from current magnitude to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state.

Main Index

LOADCASE (History Definition) 1447 Define Loadcase

Format Fixed

Free

Data Entry Entry Enter 2 if point load, distributed load or kinematic load is to be linearly changed from zero to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state. If the boundary condition is not included in a subsequent loadcase: point load, distributed load or kinematic load is linearly reduced in magnitude to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”. Enter 3 if point load, distributed load or kinematic load is to be linearly changed from zero to prescribed magnitude, or point temp is to be linearly changed from initial temp to prescribed magnitude, or change state is to be linearly changed from “initial state” to prescribed state. If the boundary condition is not included in a subsequent loadcase: point load, distributed load is linearly reduced in magnitude to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”. Enter -1 or -2 load is removed “gradually”. point load, distributed load or kinematic load is linearly reduced in magnitude to zero, point temperature is linearly changed to the initial temperature, change state is linearly changed to the “initial state”.

Main Index

1448 LOADCASE (History Definition) Define Loadcase

Format Fixed

Free

Data Entry Entry Enter -3 load is removed “gradually”, point load, distributed load is linearly reduced in magnitude to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is linearly ramped to the initial temperatures, change state is linearly ramped to the “initial state”. Enter -4 Load is removed instantaneously, point load, distributed load is instantaneously reduced to zero, kinematic displacements are to be instantaneously removed, and the previous reaction force is linearly reduced to zero, point temperature is instantaneously changed to the initial temperature, change state is instantaneously changed to the “initial state”. When POINT TEMP is used, the initial temperatures are prescribed in the INITIAL TEMP option. When CHANGE STATE is used, the “initial temperatures” are prescribed in the CHANGE STATE option.

Main Index

DMIG-OUT (History Definition) 1449 Output Control of Matrices

DMIG-OUT (History Definition)

Output Control of Matrices

Description This option allows you to control the output of matrices into DMIG format. These matrices may then be read in using the DMIG option and activated using either the B2GG, B2PP, K2GG, K2PP, M2GG, M2PP, and P2G options within Marc or within MD Nastran. To output the substructure matrix, use the SUPERELEM option. In the case of element matrix, they can either be written in the Marc global (MSC.Nastran Basic) or a local coordinate system. Both symmetric and nonsymmetric matrices are supported. Note that the scalar factor associated with the STIFSCALE option is not applied to the element matrices. This option may be repeated in each loadcase. The files created associated with element matrices have the names jidname_dmigXX_inc, where: Jidname

is the job ID name

XX

is the suffix associated with the matrix type

ST

stiffness matrix

DF

differential stiffness matrix

MS

mass matrix

DM

damping matrix

CO

conductivity matrix

SP

specific heat matrix

Inc

is the increment number

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word DMIG-OUT.

The 2nd and 3rd, 4th and 5th, 6th and 7th, 8th and 9th, 10th and 11th, 12th and 13th data blocks are entered as pairs as required. 2nd data block 1-10

1st

A

Enter the word STIFFNESS.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

Main Index

1450 DMIG-OUT (History Definition) Output Control of Matrices

Format Fixed 16-20

Free 3rd

Data Entry Entry I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase. Enter -2 to switch off writing DMIG output.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Enter 0 to output global stiffness in untied state. Enter 1 to output global stiffness in tied state.

36-45

7th

E

Enter minimum value to be written to DMIG. Stiffness values below this value will be ignored.

3rd data block (only required if a list of elements or bodies to be given) 4th data block 1-10

1st

A

Enter the words DIFF MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

Main Index

DMIG-OUT (History Definition) 1451 Output Control of Matrices

Format Fixed

Free

Data Entry Entry

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Stiffness values below this value will be ignored.

5th data block (only required if a list of elements or bodies to be given) 6th data block 1-10

1st

A

Enter the words MASS MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Mass values below this value will be ignored.

7th data block (only required if a list of elements or bodies to be given) 8th data block 1-10

1st

A

Enter the words DAMPING MATRIX.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

Main Index

1452 DMIG-OUT (History Definition) Output Control of Matrices

Format Fixed 21-25

Free 4th

Data Entry Entry I

Enter 1 to output in Marc global, Nastran basic (default). Enter 2 to output in current transformed system. The global matrix is always written in transformed system.

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Damping values below this value will be ignored.

9th data block (only required if a list of elements or bodies to be given) 10th data block 1-10

1st

A

Enter the word CONDUCTIVITY.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default).

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Enter 0 to output global conductivity in untied state. Enter 1 to output global conductivity in tied state.

36-45

7th

E

Enter minimum value to be written to DMIG. Conductivity values below this value will be ignored.

11th data block (only required if a list of elements or bodies to be given)

Main Index

DMIG-OUT (History Definition) 1453 Output Control of Matrices

Format Fixed

Free

Data Entry Entry

12th data block 1-10

1st

A

Enter the word SPECIFIC.

11-15

2nd

I

Enter 1 for element matrices. Enter 2 for global matrix. Enter 3 for element and global matrices.

16-20

3rd

I

Frequency to write (default is every increment). Enter –1 to write out only once in the loadcase.

21-25

4th

I

Enter 1 to output in Marc global (MSC.Nastran basic) (default).

26-30

5th

I

Control of which element matrices are to be written. If only the global matrix is to be written, this option and the next data block is not used. Enter 1 if a list of elements is given (default). Enter 2 if all elements are to be output. Enter 3 if a list of bodies is to be given. Enter 4 if all bodies are to be output.

31-35

6th

I

Not used; enter 0.

36-45

7th

E

Enter minimum value to be written to DMIG. Specific heat values below this value will be ignored.

13th data block (only required if a list of elements or bodies to be given)

Main Index

1454 K2GG, K2PP (History Definition) Selects Direct Input Stiffness Matrix

K2GG, K2PP (History Definition)

Selects Direct Input Stiffness Matrix

Description This option activates or deactivates a stiffness matrix defined by the DMIG option. This option should be in the input file before the matrix is read in by the DMIG option. Note:

If transformation or rigid body rotations of the stiffness matrix are to occur, all degrees of freedom of the nodes must appear on the DMIG file.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word K2GG or K2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

36-40

5th

I

Not used; enter 0.

41-45

6th

I

Enter 0 to suppress the transformation to the stiffness matrix although a transformation has been applied to the node (default - this implies that the stiffness matrix used is provided in the transformed system). Enter 1 to apply transformations to the stiffness matrix.

46-50

7th

I

Enter first node number used to rigidly rotate G stiffness.

51-55

8th

I

Enter second node number used to rigidly rotate stiffness matrix.

56-60

9th

I

Enter third node number used to rigidly rotate stiffness matrix. Note:

Main Index

If only the seventh field is entered, this node must have six degrees of freedom.

K2GG, K2PP (History Definition) 1455 Selects Direct Input Stiffness Matrix

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the stiffness matrix before any constraints are applied. 3. A scale factor may be applied to the stiffness matrix specified here or to all stiffness matrices via the COEFFICIENT model definition option, CK2 entry. 4. If a transformation is to be applied to the stiffness matrix, the DMIG must contain all of the degrees of freedom associated with the node to which the transformation is applied. 5. The 6th and 7th, 8th and 9th entries cannot change in the history definition section.

Main Index

1456 M2GG, M2PP (History Definition) Selects Direction Input Mass Matrix

M2GG, M2PP (History Definition)

Selects Direction Input Mass Matrix

Description This option activates or deactivates a mass matrix defined by the DMIG option in a dynamic analysis. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word M2GG or M2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the mass matrix before any constraints are applied. 3. The matrix must be symmetric and field 4 on DMIG, name entry must contain a 6. 4. M2GG input must either be in consistent mass units or the COEFFICIENT model definition option, CM2 entry may be used.

Main Index

B2GG, B2PP (History Definition) 1457 Selects Direction Input Damping Matrix

B2GG, B2PP (History Definition)

Selects Direction Input Damping Matrix

Description This option activates or deactivates a damping matrix for dynamic or harmonic analysis defined by the DMIG option in a dynamic analysis. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word B2GG or B2PP.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate matrix. Enter -1 to deactivate matrix.

26-35

4th

E

Enter scale factor; default is 1.0.

Remarks 1. DMIG matrices are not used unless selected. 2. Terms are added to the damping matrix before any constraints are applied. 3. The matrix must be symmetric and field 4 on DMIG, name entry must contain the integer 6. 4. A scale factor may be applied to the damping matrix specified here or to all damping matrices via the COEFFICIENT model definition option, CB2 entry.

Main Index

1458 P2G (History Definition) Selects Direction Input Load Vector

P2G (History Definition)

Selects Direction Input Load Vector

Description This option activates or deactivates a load vector defined by the DMIG option. This load vector may be scaled by referencing a table which is a function of time. Format Format Fixed

Free

Data Entry Entry

1-10

1st

A

Enter the word P2G.

11-20

2nd

A

Enter the name of the DMIG. Note that this is case sensitive.

21-25

3rd

I

Enter 0 or 1 to activate the load vector. Enter -1 to deactivate the load vector.

26-30

4th

E

Enter scale factor; default is 1.0.

31-35

5th

I

Enter a table ID.

Remarks 1. Terms are added to the load matrix before any constraints are applied. 2. The matrix must be rectangular in form (i.e., field 4 on DMIG entry - IFO -must contain the integer 9). 3. A scale factor may be applied to the vector specified here or to all vectors via the COEFFICIENT model definition option entry.

Main Index

READ FILE 1459 Read Data Transfer File Used in Contact Decoupled Analysis

READ FILE

Read Data Transfer File Used in Contact Decoupled Analysis

Description This option allows you to define a data transfer file for reading in the analysis performed for tool stress analysis. This option overrides all other loadcases in the same history block and should be placed at the end of that history block before CONTINUE. This option forces analysis to use the loading data in the transfer file and perform a single step loading. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words READ FILE.

A

Enter a full data file name including extension.

2nd data block 1-80 Notes:

1st

The data file is expected in the run directory. This option is used with DECOUPLING,3. If this option is not used, the default data transfer file is jid.t70.

Main Index

1460 WRITE FILE Write Data Transfer File Used in Contact Decoupled Analysis

WRITE FILE

Write Data Transfer File Used in Contact Decoupled Analysis

Description This option allows users to define a data transfer file for writing in contact decoupled analysis. The contact forces are written in the file for every loading increment. This option should be placed in the first loadcase. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WRITE FILE.

A

Enter a full data file name including extension.

2nd data block 1-80 Notes:

1st

The data file is created in the run directory. This option is used with DECOUPLING,1/2. If this option is not used, the default data transfer file is jid.t70.

Main Index

Chapter 4 History Definition Options 1461 Static, Dynamic, Creep Analysis

Chapt Static, Dynamic, Creep Analysis This section describes the application of incremental boundary conditions and/or specifies automatic er 4 Histor multi-increment load control. These boundary conditions include: • kinematic constraint of either zero or specified displacement; y • surface, volumetric or nodal loads; Defini • thermal loads, and tion • modification of tying constraint. Optio These boundary changes are incremental in nature with the following exceptions: ns 1. If the ELASTIC parameter is used, each load case is an independent analysis and the load value are total values. 2. If the FORCEM user subroutine is used with the FOLLOW FOR parameter, the distributed loads given in this routine are total values. 3. If the AUTO INCREMENT option is used, the total load is applied. 4. If the AUTO STEP option is used, the total load at the end of the time period is entered. 5. The table driven input is used to define boundary conditions. There are five possibilities for automatic load control: 1. AUTO LOAD allows you to repeat the same incremental load a prescribed number of times. 2. AUTO INCREMENT divides the incremental mechanical load requested into a series of steps to satisfy the user-prescribed tolerances. 3. AUTO THERM divides the incremental thermal load requested into a series of steps to satisfy the user-prescribed tolerances. 4. AUTO STEP allows automatic time-stepping in dynamic analysis or in coupled thermal-stress analysis with a choice of error criteria. 5. AUTO THERM CREEP divides the requested incremental thermal load into a series of steps and carries out creep analysis between every two steps to satisfy your prescribed tolerances. The BUCKLE option activates the calculation of the collapse loads and eigenvectors. Note that eigenvalues can be extracted at any increment of the analysis. The BACKTOSUBS option allows you to recover the displacements, strains, and stresses from a substructure. The RECOVER option allows the recovery of stresses and reactions for a specified mode during modal analysis.

Main Index

1462 DISP CHANGE Define Displacement Boundary Conditions

DISP CHANGE

Define Displacement Boundary Conditions

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new displacement boundary conditions to be specified or old displacement boundary conditions to be changed. The exact numbering sequence of the boundary conditions is used in some applications of this option. This numbering sequence is output after the boundary condition option is used in the input data describing the problem. This option is used for incrementation of fixed displacement components or for adding or removing displacement constraints. Care should be taken when removing fixed displacement conditions to ensure that the reaction forces are handled properly. The residual load correction should be used to reduce reactions to zero after a constraint has been removed (the LOAD COR parameter might be necessary); however, a constraint force might be too large for the piecewise linear analysis. Note that enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Complex displacement, velocity, or acceleration histories are more conveniently input by user subroutine FORCDT. This option implies a proportional increment of 1.0. Any resetting of this factor (for example, the PROPORTIONAL INCREMENT option used before the next CONTINUE option), proportions these

displacement increments as well. When used in conjunction with harmonic analysis, this boundary change is used for all excitation frequencies until a new boundary change is invoked. In a coupled thermal-stress analysis, use DISP CHANGE for stress and TEMP CHANGE for thermal analysis. When used in conjunction with harmonic analysis, this boundary change is used for all excitation frequencies until a new boundary change is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

Main Index

1st

A

Enter the words DISP CHANGE.

DISP CHANGE 1463 Define Displacement Boundary Conditions

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Set to the number of boundary conditions (specified displacement components to be changed or added). A negative number removes boundary conditions from the end of the boundary condition list. Note:

A zero invokes the FIXED DISP option; a complete set of necessary boundary conditions are then read, using the blocks for that option except for that key word block.

6-10

2nd

I

Enter 1 if excitation boundary conditions for harmonic analysis.

11-15

3rd

I

Enter 1 if harmonic boundary condition is input as magnitude and phase. If blank, real and imaginary values are given.

3a data block Data block 3a is only entered if the number in columns 1 through 5 in data line 2 is positive and then has the number of data lines required by data block 2. 1-5

1st

I

Number of the boundary condition being changed. This number is derived from the “Fixed Boundary Condition Summary” table in the input echo of a Marc run. Boundary conditions being added should be given labels which increment the total count of boundary conditions properly. Note:

A boundary condition in the middle of the list can be removed by specifying that labeled boundary condition as a repeat of some other boundary condition.

6-10

2nd

I

Nodal point to be constrained.

11-15

3rd

I

Degree of freedom to be constrained.

16-30

4th

F

Specified displacement increment (real part).

31-45

5th

F

Specified displacement increment (imaginary part).

Data blocks 3b through 6 are only entered if the number in columns 1 through 5 in data line 2 in zero. 3b data block 1-5

1st

I

Number of sets of boundary condition data to be read (optional).

For each set of boundary conditions use the 4th, 5th, and 6th data blocks. 4a data block Use only if not Fourier Analysis.

Main Index

1-10

1st

E

Prescribed displacement for first degree of freedom listed in data block 5.

11-20

2nd

E

Prescribed displacement for second degree of freedom listed in data block 5.

1464 DISP CHANGE Define Displacement Boundary Conditions

Format Fixed 21-30

Free 3rd

Data Entry Entry F

Prescribed displacement for third degree of freedom listed in data block 5. A maximum of eight kinematic constraints can be specified. The third data block is read as 8E10.3.

4b data block Use for Fourier analysis only. 1-5

1st

I

Enter the series number associated with this boundary condition.

6-15

2nd

F

Prescribed displacement for first degree of freedom listed in data block 5.

16-25

3rd

F

Prescribed displacement for second degree of freedom listed in data block 5.

26-35

4th

F

Prescribed displacement for third degree of freedom listed in data block 5.

36-45

5th

F

Prescribed displacement for fourth degree of freedom listed in data block 5.

46-55

6th

F

Prescribed displacement for fifth degree of freedom listed in data block 5.

5th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

6th data block Enter a list of nodes to which the above boundary conditions are applied.

Main Index

RELEASE NODE 1465 Define Nodes for which the Boundary Condition is Gradually Released

RELEASE NODE

Define Nodes for which the Boundary Condition is Gradually Released

.The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the release node procedure is controlled through the LOADCASE history definition option. Description This option removes a boundary condition constraint from a node in a gradual manner. This option is similar to changing boundary conditions, but it allows the reaction force to be brought to a zero value over a series of increments. The load is reduced in equal steps if used in conjunction with the AUTO LOAD or DYNAMIC CHANGE option. The load is proportionally reduced to zero if used with the AUTO STEP or AUTO INCREMENT option. If the RELEASE NODE and DISP CHANGE are given in the same load incrementation section, the DISP CHANGE option should be given first. Note:

This option should not be applied to nodes in contact with rigid surfaces.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word RELEASE NODE.

2nd data block 1-5

1st

I

Enter the number of sets of data; this must be given.

6-10

2nd

I

Enter unit number for input of release data, defaults to input.

3rd data block Enter a list of degrees of freedom to be released. 4th data block Enter a list of nodes to be released.

Main Index

1466 GAP CHANGE Redefine Data for Gap Elements

GAP CHANGE

Redefine Data for Gap Elements

Description This option allows you to modify the data associated with gap elements. This data includes gap closure distance, gap elastic stiffness, contact coefficient of friction, and momentum ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GAP CHANGE.

2nd data block 1-5

1st

I

Number of sets of gap data to be input.

6-10

2nd

I

Unit number for reading data. Defaults to input.

The 3rd and 4th data blocks are entered as pairs, once for each set of gap data. 3rd data block 1-10

1st

F

For a fixed direction gap, enter the gap closure distance Ucl. For a true distance gap, enter the minimum distance d between end points. Note:

If d > 0, the two end points are never closer than a distance |d| apart. If d<0, the two end points are never farther apart than |d|.

11-20

2nd

F

μ, the contact coefficient of friction.

21-30

3rd

F

KGAP, the elastic stiffness of the closed gap in the contact direction. Default: Gap is rigid when closed.

31-40

4th

F

KFRICTION, the elastic stiffness of the closed gap in the friction direction. Default: Gap is rigid when closed.

41-50

5th

F

User supplied momentum ratio for first gap node. Default: Marc calculates this ratio internally.

51-60

6th

F

User supplied momentum ratio for fourth gap node. Default: Marc calculates this ratio internally.

61-65

7th

I

Enter 0 for fixed direction gap. Enter 1 for true distance gap. Default is 0.

66-70

8th

I

Enter 0 if gap is open during increment 0. Enter 1 if gap is closed during increment 0. Default is 0.

Main Index

GAP CHANGE 1467 Redefine Data for Gap Elements

Format Fixed

Free

Data Entry Entry

4th data block Enter a list of gap elements to be associated with this set of gap data.

Main Index

1468 TYING CHANGE Define Tying Constraints

TYING CHANGE

Define Tying Constraints

Description This allows the number of tying constraints to be modified or a totally new series of tying constraints to be introduced. This option modifies the constraints previously entered on the TYING option. If the number of ties is increased, the TIE parameter is also required. Notes:

The use of TYING CHANGE can increase the bandwidth beyond that calculated for the original space allocation and, therefore, Marc recalculates the nodal bandwidth and the storage allocation for the assembly and solution part of Marc. To completely remove a set of tying constraints, set column 5 to 1 and column 10 to 0.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words TYING CHANGE.

I

Set equal to 1 to reduce the number of tying constraints at this point of the analysis.

2nd data block 1-5

1st

Set equal to 2 to read in an entire new set of tying constraints. If column 5 is set to 1, the new number of tying constraints has to be less than the originally specified number of ties. The tying constraints are deleted from the end of the list to the desired number of remaining ties. The list is in the same sequence as the list of ties in the input file. 6-10

2nd

I

New number of tying constraints. The data lines required by the tying option are read in next if column 5 of this data line is set to 2, except for the key word block.

Main Index

DIST LOADS (History Definition) 1469 Define Distributed Loads

DIST LOADS (History Definition)

Define Distributed Loads

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This block of data allows pressure (surface and volumetric) loads to be specified. These values are incremental values per increment if a fixed time-step procedure is used or the total change over the loadcase if an adaptive time-step procedure is used or the total value of the load if the ELASTIC parameter is used. User subroutine FORCEM can be used for nonuniform, time-dependent distributed loads. Note:

If FOLLOW FOR is included in the input file with DIST LOADS, the input about type of load, magnitude etc. (data blocks 3 and 4) needs to be consistent in the model and history definition options.

If FEATURE,203 is used, then the pressure on an edge (2-D) or face (3-D) is applied, unless all nodes of that edge or face are in contact with another body. If separation occurs, the distributed load is reapplied to the surface. For most distributed load types, one enters a load per unit length (on beams or shell edges) or a load per unit area. There are a few exceptions listed below: Load Type

Main Index

100

Centrifugal

Enter ω2 (ω in radians/time)

102

Gravity

Enter three values (Force/mass)

103

Centrifugal and Coriolis

Enter ω2 (ω in radians/time)

104

Centrifugal

Enter ω (ω in cycles/time)

105

Centrifugal and Coriolis

Enter ω (ω in cycles/time)

106

Uniform Volumetric load

Enter three values force/volume

107

Nonuniform Volumetric load

Enter three values force/volume

110

Uniform load per unit length

Enter three values force/length

111

Nonuniform load per unit length

Enter three values force/length

1470 DIST LOADS (History Definition) Define Distributed Loads

Load Type 112

Uniform load per unit area

Enter three values force/area

113

Nonuniform load per unit area

Enter three values force/area

General traction

Enter three values force/area

-10 to -21

Table 4-5

CID Load Types (Not Table Driven Input)

IBODY

Specify Traction on Edge or Face

User Subroutine

-10

1

No

-11

1

Yes

-12

2

No

-13

3

Yes

-14

3

No

-15

3

Yes

-16

4

No

-17

4

Yes

-18

5

No

-19

5

Yes

-20

6

No

-21

6

Yes

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST LOADS.

2nd data block 1-5

1st

I

Enter the number of sets of distributed loads to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed load data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set.

Main Index

DIST LOADS (History Definition) 1471 Define Distributed Loads

Format Fixed

Free

Data Entry Entry

3a data block Use if conventional Marc input, not Fourier, not applied to a cavity, and not Nastran PLOAD4 style. 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library. For problems with more than one rotation axes, add the rotation axis ID times a thousand.

6-15

2nd

F

Enter the magnitude of this type of distributed load. For load types -10 to -21 or 102 to 113, enter the magnitude of load in first coordinate direction.

16-25

3rd

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in second coordinate direction

26-35

4th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in third coordinate direction

36-40

5th

I

Distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.)

3b data block Use if distributed load is applied to cavity and not Fourier. The CAVITY parameter and CAVITY model definition option is also required. 1-5

1st

I

Enter the value of ibody_cavity. i bo dy _c a vi t y = ic a vi t y * 10000 + i c av it y _t y pe * 1000 + ib od y

where ibody_cavity is the cavity-modified value for the distributed load type. icavity is the cavity ID. icavity_type is the cavity load type: 0: cavity is closed. 1: cavity is loaded with an applied pressure. 2: cavity is loaded with an applied mass. 9: cavity load is defined by the UCAV user subroutine. ibody is the original value for the distributed load type (see library element description in Marc Volume B: Element Library.) 6-15

2nd

F

If icavity_type = 1, enter incremental pressure. If icavity_type = 2, enter incremental mass.

16-25

Main Index

3rd

F

Not used; enter 0.

1472 DIST LOADS (History Definition) Define Distributed Loads

Format Fixed

Free

Data Entry Entry

26-35

4th

F

Not used; enter 0.

36-40

5th

I

Distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.)

41-45

6th

I

Enter -1 if the cavity load is not active.

3c data block Use if Fourier Analysis. 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library. For problems with more than one rotation axes, add the rotation axis ID times a thousand.

6-15

2nd

I

Enter the series number associated with this load.

16-25

3rd

F

Enter the magnitude of this type of distributed load. For load types -10 to -21 or 102 to 113, enter the magnitude of load in first coordinate direction.

26-35

4th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in second coordinate direction.

36-40

5th

F

For load types -10 to -21 or 102 to 113, enter the magnitude of load in third coordinate direction.

3d data block Use if Nastran PLOAD4 style input.

Main Index

1-5

1st

I

Parameter identifying the type of load plus 200. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter P1, the magnitude of load at node 1 of face or edge.

16-25

3rd

F

Enter P2, the magnitude of load at node 2 of face or edge.

26-35

4th

F

Enter P3, the magnitude of load at node 3 of face or edge.

36-45

5th

F

Enter P4, the magnitude of load at node 4 of face or edge. Not required if a triangular face.

46-55

6th

F

Enter first component of direction of load.

56-65

7th

F

Enter second component of direction of load.

DIST LOADS (History Definition) 1473 Define Distributed Loads

Format Fixed

Free

Data Entry Entry

66-75

8th

F

Enter third component of direction of load.

76-80

9th

I

If positive, distributed load index (optional). (Distributed load index is to be used in the FORCEM user subroutine.) If the direction of the load is given with respect to a COORD SYSTEM option, then enter the negative of the coordinate system ID.

Notes:

If the direction of the load is not defined, then the conventional Marc direction is used. If the direction of the load is defined, then it is fixed and not updated even if the FOLLOW FOR parameter is activated.

4th data block Enter a list of elements associated with the above distributed loads.

Main Index

1474 POINT LOAD (History Definition) Define Point Loads

POINT LOAD (History Definition)

Define Point Loads

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows nodal point loads to be specified. The nodal loads can be specified as fixed direction loads or follower loads. For the fixed direction loads, the nodal forces are always specified in vector form. For the follower loads, two options are possible: Option 1 is the MD Nastran style Follower Force wherein the magnitudes of the nodal force and moment are specified and the direction is independently specified using 2 or 4 nodes. Option 2 is the Mesh Based Automated Follower Force wherein the nodal loads are specified in vector form and the initial load orientation with respect to the mesh is maintained as the structure deforms. For more details, refer to Marc Volume A: Theory and User Information. If the number of nodes which have point loads has been changed from the model definition option, you must give an upper bound on the DIST LOADS parameter. Note:

The fourth field of the FOLLOW FOR parameter should be set to 1 when follower force loads are used in the model. When this global parameter for follower force point loads is turned on, the 5th data block is mandatory. The follower force option is not valid for fourier loads or harmonic loads. Also, the follower force capability is not supported for point loads specified through the FORCDT user subroutine.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT LOAD.

11-15

2nd

I

Enter 1 to enter real harmonic load. Enter 2 to enter imaginary harmonic load.

2nd data block

Main Index

1-5

1st

I

Enter number of sets of point loads to be entered (optional).

6-10

2nd

I

Enter logical unit number for input of point load data; defaults to input.

11-15

3rd

I

Enter 1 to signal existence of more than one point load on the same node. The loads are summed in this case.

POINT LOAD (History Definition) 1475 Define Point Loads

Format Fixed

Free

Data Entry Entry

The 3rd and 4th data blocks are entered as pairs, once for each data set. 3rd data block 1-10

1st

F

Nodal load associated with first degree of freedom. Nodal Force magnitude for MD Nastran style follower force.

11-20

2nd

F

Nodal load associated with second degree of freedom. Nodal Moment magnitude for MD Nastran style follower force.

21-30

3rd

F

Nodal load associated with third degree of freedom.

31-40

4th

F

Nodal load associated with fourth degree of freedom.

41-50

5th

F

Nodal load associated with fifth degree of freedom.

51-60

6th

F

Nodal load associated with sixth degree of freedom.

61-70

7th

F

Nodal load associated with seventh degree of freedom.

71-80

8th

F

Nodal load associated with eighth degree of freedom.

Note:

Continuation data line is necessary and must be in 6E10.3 format. Continuation data lines are needed if there are more than eight degrees of freedom per node in the analysis.\ The nodal load vector is valid for fixed direction force or for automated follower force. Only the first two fields are used for the MD Nastran style follower force.

4th data block Enter a list of nodes to which the above point load is applied. 5th data block Used only when 4th field of FOLLOW FOR parameter is 1. For the MD Nastran style follower force, enter as many lines as there are nodes in the 4th data block. 1-5

1st

I

0

= Fixed direction force

-1 = Automated follower force First node for MD Nastran style follower force

Main Index

6-10

2nd

I

Second node for MD Nastran style follower force

11-15

3rd

I

Third node for MD Nastran style follower force

16-20

4th

I

Fourth node for MD Nastran style follower force

1476 AUTO LOAD Define Equal Load Increments

AUTO LOAD

Define Equal Load Increments

Description This option is useful for nonlinear analysis with proportional loads. It generates a specified number of increments. For contact analysis, the TIME STEP history definition option is also needed with AUTO LOAD, so that the incremental displacement of the contact body can be obtained from the velocity. AUTO LOAD primarily controls mechanical loads and kinematic boundary conditions. For uncoupled thermal stress analysis, AUTO LOAD can also be used to control state variables specified by the THERMAL LOADS/CHANGE STATE options or point temperatures specified by the POINT TEMP option.

No Table Driven Input The load increment is the net result of the changes and scalings made to the load increment in all the previous increments, plus the effect of any tractions, proportional increment options, etc., in the current increment. The load increment is the same for all steps in this loadcase. These options should come after the AUTO LOAD option. If the proportional increment option is not included, AUTO LOAD sets the proportionality factor to a default of 1. Table Driven Input When this option is used with the table driven boundary conditions, it is only used to control the number of increments, and with TIME STEP the total time period. The magnitude of the boundary conditions is determined by the table. Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the words AUTO LOAD.

2nd data block 1-5

1st

I

Number of times this load increment is to be applied.

6-10

2nd

I

Reassembly interval for stiffness matrices. Defaults to whenever nonlinearity occurs.

Main Index

AUTO LOAD 1477 Define Equal Load Increments

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Maximum number of allowable time step cuts. = 0 means no automatic restart from the previously converged step. > 1 means maximum number of time step cutbacks allowed if convergence is not achieved. Marc automatically restarts the analysis after each cutback until the maximum number is reached.

Main Index

1478 INERTIA RELIEF (History Definition) Define Inertia Relief

INERTIA RELIEF (History Definition)

Define Inertia Relief

Description This option defines the parameters necessary for conducting an inertia relief analysis. The parameters are used to evaluate the Rigid Body Modes of the system. Once the modes are evaluated, the program evaluates the inertia relief load vector which balances the external load vector acting on the system. For more details of these procedures, you are referred to Inertia Relief in Chapter 5 in the Marc Volume A: Theory and User Information manual. When inertia relief is no longer active in a current loadcase, an option can be provided to remove or retain inertia relief loads from previous loadcases. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words INERTIA RELIEF.

I

Flag for Rigid Body Mode evaluation method:

2nd data block 1-5

1st

0 - Inertia Relief is not active in current loadcase 3 - Support Method 6-10

2nd

I

Flag to retain/remove previous Inertia Relief Loading: 1 - retain load -1 - remove load immediately (default) -2 - remove load gradually

11-15 Note:

3rd

I

Number of Lines containing Support degree of freedom information (default 1)

Field 2 of data block 2 is only used if inertia relief is not active in the current loadcase (i.e., Field 1 of data block 2 is 0). Also, data block 3 is not necessary in this case.

Data block 3 is repeated as many times as specified in the 2nd data block, 3rd field. 3rd data block Use only if 1st field of 2nd data block is 3 (Support Method)

Main Index

1-5

1st

I

Node ID 1.

6-10

2nd

I

Degree of Freedom ID 1.

11-15

3rd

I

Node ID 2.

16-20

4th

I

Degree of Freedom ID 2.

INERTIA RELIEF (History Definition) 1479 Define Inertia Relief

Format Fixed

Data Entry Entry

21-25

5th

I

Node ID 3.

26-30

6th

I

Degree of Freedom ID 3.

31-35

7th

I

Node ID 4.

36-40

8th

I

Degree of Freedom ID 4.

41-5

1st

I

Node ID 5.

46-10

2nd

I

Degree of Freedom ID 5.

51-55

3rd

I

Node ID 6.

56-60

4th

I

Degree of Freedom ID 6.

61-65

5th

I

Node ID 7.

66-70

6th

I

Degree of Freedom ID 7.

71-75

15th

I

Node ID 8.

76-80

16th

I

Degree of Freedom ID 8.

Note:

Main Index

Free

The degrees of freedom in fields 2, 4, etc. of data block 3 refer to the nodal degrees of freedom that define the rigid body motion (r-constraint set). The associated nodes are defined in fields 1,3, etc. The degrees of freedom that form part of the r-constraint set at any particular node can be specified in combined form (e.g., 123, 135, etc.). If all degrees of freedom at node N are to be part of this set, simply specify a negative number in the associated degrees of freedom field.

1480 BEGIN SEQUENCE Initiate a Series of Repeated Load Cases

BEGIN SEQUENCE

Initiate a Series of Repeated Load Cases

Description This option begins a sequence of load cases. All history commands between the BEGIN SEQUENCE and END SEQUENCE are repeated as often as specified here. The input lines are copied to a file named jid.seq. Note:

This does not work with RESTART.

Format Format Fixed

Free

Data Entry Entry

1st data block

Main Index

1-10

1st

A

Enter the words BEGIN SEQUENCE.

11-15

2nd

I

Enter the number of times the following history definition commands are to be repeated.

END SEQUENCE 1481 Terminates a Series of Repeated Load Cases

END SEQUENCE

Terminates a Series of Repeated Load Cases

Description This option is used in conjunction with BEGIN SEQUENCE to terminate a series of repeated load cases. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words END SEQUENCE.

1482 PROPORTIONAL INCREMENT Define Proportional Increments

PROPORTIONAL INCREMENT

Define Proportional Increments

Description Using this option, the previous load increment can be scaled up or down for use in the current load increment. This is most frequently used in elastic-plastic analysis where the first load increment is scaled up to the values that cause first yield. This option governs mechanical loads only; temperature changes are independent of this proportioning. The option can precede or follow all the other options in this optional series. If it precedes a DIST LOADS, POINT LOAD, or DISP CHANGE option, these options reset the proportionality factor to 1.0. If it follows either of these options, it also scales any nonzero load or displacement increments given in these options. Note:

If the SCALE parameter is used, the load increment that is applied in the first increment is the scaled load multiplied by the value given in the second field of the second data block.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-22

1st

A

Enter the words PROPORTIONAL INCREMENT.

2nd data block

Main Index

1-5

1st

I

Minimum number of cycles for each step of one increment; normally 1 (forces recycling n times). Every recycle might cause an assembly and decomposition of the stiffness matrix. Marc automatically recycles if convergence to tolerance is not achieved. The default value of recycles is 0. If this value is set above 1, more cycles are allowed but each increment is forced to cycle at least n times before solution. Use caution that no unnecessary recycling is being forced (for example, in AUTO LOAD). Recycling is usually forced for the first few critical load steps to get convergence and then resume normal condition.

6-20

2nd

F

Ratio of the current increment of load to the previous increment. Only mechanical loads and kinematic boundary conditions are scaled.

AUTO INCREMENT 1483 Define Automatic Load Stepping

AUTO INCREMENT

Define Automatic Load Stepping

Description This option allows automatic load stepping in a quasi-static analysis and is very useful for both geometric (LARGE DISP) and material (elastic-plastic) nonlinear problems. The option is capable of handling elastic/plastic snap-through phenomena; hence, the post-buckling behavior of structures can be analyzed. However, the option cannot be used for thermal loading. You have to specify in the DIST LOADS, POINT LOAD, and/or DISP CHANGE options the total loading at the end of the loadcase, and Marc automatically generates the magnitude of each load step based on an initial load step and the amount of nonlinearity occurring during the loading. The length of the incremental displacement vector (C = ΔuTΔu) is based upon a number of parameters. The analysis is stopped when the total load is reached or when the maximum allowed number of increments is reached. In case of a snap-through problem, the loading can initially increase, decrease after the buckle load has been reached, and increase if the stiffness increases in the post-buckled state. Within the history definition data, the AUTO INCREMENT option can be used as often as desired. For more details, see Marc Volume A: Theory and User Information. When this option is used with table driven boundary conditions, the independent variable should not be time, normalized time, increment number, or normalized increment number. If multiple loadcases are to be used, the boundary condition should be a function of the loadcase number. Notes:

The option cannot be used for thermal loading; use the AUTO THERM option instead. If this option is used for post-buckling analysis, the nonpositive definite flag in the SOLVER model definition option has to be used. This option can be added upon restart.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-14

1st

A

Enter the words AUTO INCREMENT.

F

Fraction (α) of the total load increment that should be applied in the first cycle of the first increment of this AUTO INCREMENT session resulting in Δu1 = K-1αP.

2nd data block 1-10

1st

T

C in = Δ u 1 Δ u 1 .

Main Index

1484 AUTO INCREMENT Define Automatic Load Stepping

Format Fixed

Free

Data Entry Entry Recommendations – If one knows nothing about the problem, this value should be 0.01 to 0.02. If one knows that the initial behavior is relatively linear and the material is elastic, then a higher value may be chosen. Note that in the first increment of the Auto Increment Loadcase, an initial arclength is calculated based upon the initial fraction of the load. This value is used with the data provided in the 5th field of this data block to determine the maximum change in arclength allowed in this loadcase. Hence, if the fraction entered here is small and a small value is given in the 5th field, small increments in displacement will occur.

11-15

2nd

I

Maximum number of increments during this AUTO INCREMENT session. Recommendations – For elastic buckling problems, 500 increments is a conservative number. For nonlinear material behavior, 1000 increments should work for most problems.

16-20

3rd

I

Desired number of recycles per increment. Used to increase or decrease load steps during AUTO INCREMENT session. Default is 3. Please allow for more recycles via CONTROL model definition option. Recommendations – The desired number of recycles of 3 is good for elastic buckling problems. For contact problems, especially if friction is present, the number should be increased to 5. If the convergence criteria is 1% or displacement based convergence checking is preformed, increase this number by 1. Note that this number does not control the number of iterations in this increment, but rather controls how the target arclength will be changed in the next increment. If the actual number of iterations is less than this number, the target arclength will be increased in the next increment. If the actual number of iterations is greater than this number, the target arclength will be decreased. If the value is too high, the target change in arclength becomes too large, but it will hit the upper bound based upon the 5th field.

21-30

4th

F

Maximum fraction of the total load that can be applied in any increment of this AUTO INCREMENT session. Default is 1 if no contact is present. Default is 0.01 if contact is present. If the 10th field is 1 or 2, the default is 0.1 for all simulations. Recommendations – For true buckling simulations, this number should be between 0.01 and 0.025. For mildly nonlinear problems, a value of 0.10 may be used.

Main Index

AUTO INCREMENT 1485 Define Automatic Load Stepping

Format Fixed 31-40

Free 5th

Data Entry Entry F

Maximum multiplier of applied arc length in norm of displacement vector to initial arc length. Cmax/Cin Defaults to maximum fraction of load divided by initial fraction of load. Comments - This number, along with the 1st field, is used to determine the maximum change of arclength in an increment. It is a critical number for the case of stability analyses; unfortunately, it is hard to determine. Recommendations – Typically, a value of 10 should be used. The problem with the default is that the initial arclength based upon the first increment is usually very small, because the initial fraction of load is 1% and the structure is elastic at that point. Hence, the default results in a large number of small displacements.

41-50

6th

F

Total time period to be covered; to be used in conjunction with contact analyses. Default is 1.0.

51-60

7th

F

Fraction of the initial arclength to define a minimal arclength. Cmin/Cin Default is 0.01. Recommendations – The default is acceptable; as the arclength is small, the minimal arclength will be very small.

61-65

8th

I

Arclength root procedure: 1 = Crisfield (quadratic constraint). 2 = Riks/Ramm (linear constraint). 3 = Modified Riks/Ramm (linear constraint) (default). 4 = Crisfield; switch to Modified Riks/Ramm if no real root found. 5 = Scaled Riks/Ramm. Recommendations – The default (Modified Riks/Ramm is good. Though, the Crisfield method with the root selection based upon the sign of the singularity ratio - 3rd data block, 1st field appears to be very effective.

66-70

9th

I

Maximum number of allowable time step cuts. = 0 means no automatic restart from the previously converged step. > 1 means maximum number of time step cutbacks allowed. Marc automatically restarts the analysis after each cutback until the maximum number is reached. Recommendation - A value of 3 should be used.

Main Index

1486 AUTO INCREMENT Define Automatic Load Stepping

Format Fixed

Free

71-75

10th

Data Entry Entry I

Enter 1 or 2 for new Crisfield approach and new defaults. Enter 2 if the 3rd data block is to be entered. This is only available beginning with 2005r3a release.

76-80

11th

I

Enter a 0 if the maximum fraction of the total load is constant over the loadcase (default). Enter a 1 if the maximum fraction of the total load can vary over the loadcase. This requires the 4th data block.

3rd data block (only used if 10th field of 2nd data block is a 2) 1-5

1st

I

For the Crisfield method, select the method to choose the roots. Enter 1 for method used in 2005r3 and previous versions based upon the angle between Δ u n – 1 and Δ u n such that the displacement is in the same direction (default). Enter 2 for selection of root based upon the sign of the singularity ratio. Enter 3 for root selection based upon Falzon. Recommendation – Method 2 appears to be the best for problems that do not have Lagrange multipliers in them; i.e., no Herrmann elements.

6-10

2nd

I

Enter method to modify arclength in next increment. Enter 1 for method used in 2005r3 and pervious versions. The target arclength, λ n + 1 = icydes/ncycle * λ , where icydes is the desired number of cycles (3rd field, 2nd data block) and ncycle is the number of cycles required in the nth increment. Enter 2 for gradual approach of changing target arclength. λ n + 1 = factor * λ n ,

where

factor = 1.5 if 3 < ratio < 5 factor = 1.25 if 1 < ratio < 3 factor = ratio if 0.1 < ratio < 1 factor = 0.1 if ratio < 0.1 where ratio is icydes/ncycle. Recommendation – Use method 2. 11-15

Main Index

3rd

I

Not used; enter 0.

AUTO INCREMENT 1487 Define Automatic Load Stepping

Format Fixed 16-25

Free 4th

Data Entry Entry F

Enter a target incremental displacement. The maximum allowable arclength will be calculated based upon the maximum displacement due to the initial load and this value. This is an alternative to used the 5th field, 2nd data block and is more physical. Recommendation – For shell buckling, enter the thickness of the shell.

26-30

5th

I

Enter 1 to allow the analysis to continue even if the load has reached 100% of the magnitude, but in the opposite direction. Enter 2 to terminate analysis if load has reached 100% of the magnitude, but in the opposite direction. This is the default if this data block is included.

Note:

Upon restart, before reading history definition data, this AUTO INCREMENT session is finished. The maximum number of increments allowed, the desired number of recycles, and the maximum step size for this session can be changed upon restart using the REAUTO model definition option.

4th data block Only required if 11th field of 2nd data block is a one.

Main Index

1-10

1st

E

Maximum fraction of total load to be applied between (MFA) 0% and L1%.

11-20

2nd

E

First percentage cutoff L1.

21-30

3rd

E

MFA between L1% and L2%.

31-40

4th

E

Second percentage cutoff L2.

41-50

5th

E

MFA between L2% and L3%.

51-60

6th

E

Third percentage cutoff L3.

61-70

7th

E

MFA between L3% and L4%.

71-80

8th

E

Fourth percentage cutoff = 100%.

1488 AUTO STEP Adaptive Load Step Control

AUTO STEP

Adaptive Load Step Control

Description This option allows control of the automatic time/load stepping procedure. In this procedure, the time step is adjusted based upon the calculated value of a parameter (strain increment, plastic strain increment, creep strain increment, stress increment, strain rate, strain energy increment, temperature increment, displacement increment, rotation increment) versus a user-defined maximum. More than one criterion can be specified. If the criteria are not satisfied within an increment, recycling occurs with a reduced time/load applied. After the increment has converged based upon tolerances specified on the CONTROL values, the data given here controls the next increment. The enhanced variant (flagged with a 1 in the 9th field of the second data block) allows the scheme to be used with or without a user specified criterion. The default auto step scheme is available for backward compatibility only. The enhanced auto step scheme should be always used for MSC.Marc 2001 and beyond. The time step is adjusted based upon the number of recycles in addition to the user criteria. More details on the scheme can be found in Marc Volume A: Theory and User Information, Chapter 11. The recycling criterion for the enhanced auto step scheme works as follows: For every increment, depending on the starting time step and the minimum time step (specified in the 5th field of the 2nd data block) a maximum number of recycling related cutbacks, N max , are automatically determined by the r program. If an increment converges in less than the desired number of recycles specified in the 8th field of the 2nd data block, the time step for the next increment is scaled up using the factor specified in the 6th field of the 3rd data block S u . If the desired number of recycles are exceeded in the current increment, the time step is scaled back with an automatically determined factor and the actual recycling related cutback count, N r , is updated by 1. The value for the automatic scaleback factor is at least 1 ⁄ S u . For each additional cutback, the magnitude of the scaleback factor is progressively increased such that the minimum time step specified in the 5th field of the 2nd data block is reached on or before N r reaches

max

Nr

.

For the enhanced auto step scheme, user criteria can be prescribed by explicitly defining the criteria (defined in data blocks 4 and 5), or by allowing the program to automatically add appropriate physical criteria (flagged by a 1 or -1 in the 12th field of the 3rd data block), or by doing both. In the last case, the program will only add automatic criteria if there are no competing explicitly defined criteria already. Details of the automatic criteria that are added can be found in Marc Volume A: Theory and User Information, Chapter 11. The user criteria for the enhanced auto step scheme works as follows: After every iteration, the user criteria are checked to see if they are satisfied. If not, the time step is scaled back and the user-criteria related cutback number, N c , is updated by 1. The smallest factor that can be used for reducing the time step is specified by the 3rd field of the 2nd data block. The maximum allowable number of user-criteria related cutbacks, Ncmax, is specified by the 2nd field of the 3rd data block. For each scaleback (recycling related or user-criterion related), the increment is started from the beginning. Scalebacks also occur if any of the following occurs: maximum number of iterations reached

Main Index

AUTO STEP 1489 Adaptive Load Step Control

(exit 3002), elements going inside out (exits 1005, 1009), or a contact node slides off the end of a rigid body (exit 2400). In this case, the time step is divided by a minimum of 2. The enhanced auto step scheme is available for mechanical, thermal and thermo-mechanically coupled analyses. When using table driven input, the 10th field of the 3rd data block is used to determine if the peaks in the tables are to be exactly satisfied. If the table controlling load is based on experimental data, it is suggested that a -1 be used, which will remove the constraint and effectively smooth out the time history of the load. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words AUTO STEP.

E

Enter the initial time step.

2nd data block 1-10

1st

Defaults to 1% of total time period for enhanced scheme. Input is required for old scheme. Recommendations – If one knows nothing about the problem, this value should be 0.01 to 0.02 of the total time period. If one knows that the initial behavior is relatively linear and the material is elastic, a higher value may be chosen. 11-20

2nd

E

Enter the total time period. Defaults to 1.0 for enhanced scheme.

21-30

3rd

E

Enter the smallest ratio between steps. Default is 0.1.

31-40

4th

E

Enter the largest ratio between steps. Default is 10.0. Recommendation – Enter a value of 2.0.

41-50

5th

E

Enter the minimum time step. Defaults to total time/maximum number of steps.

51-60

6th

E

Enter the maximum time step. Defaults to half of the total time period. Recommendation – The default is acceptable except for buckling analyses where a value of 0.025 is more appropriate.

Main Index

1490 AUTO STEP Adaptive Load Step Control

Format Fixed 61-65

Free 7th

Data Entry Entry I

Enter the maximum number of steps allowed. Recommendations – For elastic buckling problems, 200 increments is a conservative number. For nonlinear material behavior, 500 increments should work for most problems. For extremely nonlinear contact problems, 1000 should be used. Normally, a very large number can be used to be conservative.

66-70

8th

I

Controls the iteration criteria. This criteria is not used if the damping energy criteria type 5 is used. Enter the desired number of recycles per increment. Enter -1 if the iteration criteria are not to be used. Recommendations – The desired number of recycles of 3 is good for elastic buckling problems or mildly nonlinear problems. For contact problems, especially if friction is present or highly material nonlinear problems, the number should be increased to 5. If the convergence criteria is 1% or displacement based convergence checking is performed, increase this number by 1. Note:

If the damping method selected in the 10th field is set to 4, this entry is not used and should be set to -1.

71-75

9th

I

Enter 1 to read an extra data block below.

76-80

10th

I

Control of the addition of artificial damping to improve stability. -1 No damping considered. 0 When the time step reaches the minimum time step, increase the time step by a factor of 10 and add damping similar to method 4. 1 Turn on artificial damping if time step is below minimum time step. Reduce time step by a factor of 1000. Damping is based on factor specified in 9th field of data block 3. 2 Always turn on artificial damping. Damping is based on factor specified in 9th field of data block 3. 4 Always turn on artificial damping. Damping is based upon the estimated damping energy and the estimated total strain energy. Estimates are based upon the first increment in this loadcase. Artificial damping strain rate is also controlling the time step. 5 Do not add damping but use the damping energy to control the time step. Recommendation – For buckling or other stability problems, it is recommended that a 4 be entered.

Main Index

AUTO STEP 1491 Adaptive Load Step Control

Format Fixed

Free

Data Entry Entry AUTOSTEP utilizes the desired number of iterations unless the damping

energy criteria type 4 or 5 is used. The 3rd data block is only present if the 9th field of the 2nd data block is equal to 1. 3rd data block 1-5

1st

I

Enter the number of states to put on the post file. These states will be equally spaced in time. By default, the increment based variant as given by the POST option will be used.

6-10

2nd

I

Enter the maximum number of times to cut down the time step in each increment to satisfy any user-specified criteria. Defaults to 10.

11-15

3rd

I

Enter 0 to treat user criteria as limits on behavior within an increment. Enter 1 to treat user criteria as both limits on behavior within an increment and as a target to adjust the time step for the next increment. Recommendation – If user criteria are used, it is recommended that a value of 1 be entered here.

16-20

4th

I

Indicate finish criterion for thermal or coupled analysis. Set to 1 to finish the transient time period when all nodal temperatures fall below the value given in the 5th field (see below). Set to -1 to finish the transient time period when all nodal temperatures exceed the value given in the 5th field (see below). Set to 0 to complete transient time period without any check on temperatures reached.

21-30

5th

E

Finish temperature value to be used in conjunction with flag set above.

31-40

6th

E

Enter scale factor for time step changes other than changes due to user criteria. Defaults to 1.2.

41-45

7th

I

Enter flag to override CREEP and DYNAMIC parameters as specified in the parameter section for this load case. 0 Do not override parameters. 1 Turn off CREEP and DYNAMIC. 2 Turn off CREEP. 3 Turn off DYNAMIC.

46-50

8th

I

Enter table ID for the table that is used for scaling the damping factor. This field is only relevant for artificial damping method 2. Recommendation – This is an advanced feature that would allow the amount of damping to change with time. It is recommended that this field be set to 0.

Main Index

1492 AUTO STEP Adaptive Load Step Control

Format Fixed 51-60

Free 9th

Data Entry Entry E

Enter damping factor for artificial damping. Amount of damping depends on the damping flag in the 10th field of data block 2. If it is 1, the damping matrix is scaled by setting this factor to be the ratio of the initial damping energy to the initial strain energy (defaults to 1e-5). If it is 2, the damping matrix is directly scaled by this factor. If it is 4, the estimated total damping energy in the loadcase will be this factor times the estimated total strain energy. Default value of 2.e-4 is used. Recommendation - Use the defaults.

61-65

10th

I

Enter flag for reaching instances in time from load tables. -1 Ignore points in tables. 0 Reach peak (and valley) points in active load tables (default). 1 Reach all points in active load tables. Recommendation – If there are just a few points, one should enter 0; but if the time history of the boundary condition is generated from experimental data with many points, one should enter -1.

66-70

11th

I

Enter 1 to put states reached by the above flag on the post file.

71-75

12th

I

Enter flag to determine if automatic physical criteria should be added and how analysis should proceed if they are not satisfied. 2 Do not add automatic physical criteria. Stop when any user criteria are not satisfied (default). 1 Add automatic physical criteria. Stop when any user criteria are not satisfied. -1 Add automatic physical criteria. Continue when any user criteria are not satisfied. -2 Do not add automatic physical criteria. Continue when any user criteria are not satisfied. Recommendation - If no user criteria are specified, this should be set to 1. The automatic criteria are:

Main Index

a

Δ ε < 0.5

if large displacement analysis.

b

Δ ε p < 0.1

if PLASTICITY,3 or PLASTICITY,5 or large strain.

c

Δ ε cr ⁄ ε el < 0.5

if creep analysis.

d

Δ σ ⁄ σ < 0.5

if creep analysis.

e

Δ σ t h ⁄ σ < σ < 0.5

if thermal stress analysis.

AUTO STEP 1493 Adaptive Load Step Control

Format Fixed

Free

75-80

13th

Data Entry Entry I

Enter flag to check if dynamic integration error checks should be made while determining time step (only valid for single-step Houbolt and Newmark-Beta operators). 0 Skip error check (default). 1 Include error check. Recommendation – Including error check typically results in smaller time step. For larger models, it is cost effective to enter 0, but physical based criteria should be included to limit the time step. Note:

For dynamic analysis, controlling the time step based upon the number of iterations or the damping energy are not very useful.

Repeat 4rd and 5th data blocks in pairs for each criterion. 4th data block 1-5

1st

I

Enter the criterion ID: Enter 1 for strain increment. (Elements) Enter 2 for plastic strain increment. (Elements) Enter 3 for creep strain increment. (Elements) Enter 4 for normalized creep strain increment. (Elements) Enter 5 for stress increment. (Elements) Enter 7 for strain energy increment. (Elements) Enter 8 for temperature increment. This is only for heat transfer or thermal part of coupled analysis. (Nodes) Enter 9 for displacement increment. (Nodes) Enter 10 for rotation increment. (Nodes) Enter 12 for normalized stress increment (Elements) Enter (13 x 100 + state variable id) for state variable increment. Criterion ID 13, 1300, or 1301 can all be used for temperature. (Elements) Recommendation For buckling or post buckling analysis, it is very useful to cure Criteria type 9 with a displacement increment equal to the shell thickness. For large strain plasticity problems, it is very useful to use criteria type 2 with a requirement of change in plastic strain to be 0.01 or, at most 0.05.

6-80

Main Index

2nd

I

Enter set name of elements/nodes to which this criterion is to be applied.

1494 AUTO STEP Adaptive Load Step Control

Format Fixed

Data Entry Entry

Free

5th data block 1-10

1st

E

ΔYI.

11-20

2nd

E

XMAX1.

21-30

3rd

E

ΔY2.

31-40

4th

E

XMAX2.

41-50

5th

E

ΔY3.

51-60

6th

E

XMAX3.

61-70

7th

E

ΔY4.

71-80

8th

E

XMAX4.

For criteria 1, 2, 3, 4, 5, 6, 7, 8, 9, 10, the time step is adjusted based upon: if X ≤ XMAX1

ΔY calculated/ΔY1

if XMAX1 < X < XMAX2

ΔY calculated/ΔY2

if XMAX2 < X < XMAX3

ΔY calculated/ΔY3

if XMAX3 < X

ΔY calculated/ΔY4

where X

ΔY

1

strain

strain increment

2

plastic strain

plastic strain increment

3

creep strain

creep strain increment

4

creep strain

creep strain increment/elastic strain

5

stress

stress increment

7

strain energy

strain energy increment

8

temperature

temperature increment

9

displacement

displacement increment

10

rotation

rotation increment

12

stress

stress increment/stress

state variable n

increment of state variable n

Criterion

13*100+ n

Main Index

TERMINATE 1495 Terminate Loadcase

TERMINATE

Terminate Loadcase

Description This option terminates the current loadcase defined by the AUTO LOAD and AUTO STEP options if the termination criterion is satisfied. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word TERMINATE.

I

Enter the number of termination criteria; maximum of 10 allowed.

I

Termination Criteria Type.

2nd data block 1-5

1st

3rd data block 1-5

1st

Enter 1 if termination occurs when a percentage of the boundary nodes are in contact. Enter 2 if termination occurs when the maximum force on a rigid body is exceeded. Enter 3 if termination occurs when the displacement of the rigid body exceeds the allowed displacement. Enter 5 if termination occurs when the distance between the reference points of two rigid bodies is less or greater than the specified value. Enter 6 if termination occurs, when any displacement in body, is greater than the specified value. Enter 7 if termination occurs, when the displacement at the node, is greater than the specified value. 6-10

2nd

I

Enter the body number. For criterion type 7, enter the node number.

11-15

3rd

I

For criterion type 1, enter the percentage of nodes to be in contact for termination; default = 100. For criterion type 2, enter direction 1/2/3 for the x, y, z global directions For criterion type 5, enter the second body.

Main Index

1496 TERMINATE Terminate Loadcase

Format Fixed

Free

Data Entry Entry For criterion type 6 or 7, enter the degree of freedom. For criterion type 6 or 7, enter -1 if the total translational displacement. For criterion type 6 or 7, enter -2 if total rotation.

16-25

4th

F

For criterion type 2, enter the critical force. For criterion type 3, enter the critical maximum displacement. For criterion type 5, enter the critical distance. If the value is positive, the termination occurs when the distance is less than the value. If the value is negative, the termination occurs when the distance is greater than the value in a positive sign. For criterion type 6 or 7, enter the critical distance (rotation).

Main Index

SUPERPLASTIC 1497 Superplastic Forming Analysis

SUPERPLASTIC

Superplastic Forming Analysis

Description This option allows you to define the various parameters needed in superplastic forming analysis. The pressure is modified such that the calculated strain rate is approximately equal to the target strain rate. This option is not supported with the table driven input format. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SUPERPLASTIC.

2nd data block This data block controls the prestress options. 1-10

1st

I

Prestress function 1 For a constant application of prestress for a given number of increments. 2 If the prestress is ramped down linearly to 0 in a given number of increments from the prescribed value.

11-20

2nd

I

Number of increments for which prestress is applied.

21-30

3rd

F

Prestress to be applied (applicable for membrane elements only).

3rd data block This data block controls the process control parameters.

Main Index

1-10

1st

F

Target strain rate.

11-20

2nd

F

Strain rate sampling cutoff factor - the use of this factor depends on the sampling method specified by field 5 (ignores any value above this given number for calculating the average strain rate - this helps in ruling out numerical aberrations).

21-30

3rd

F

Minimum pressure for this loadcase.

31-40

4th

F

Maximum pressure for this loadcase.

1498 SUPERPLASTIC Superplastic Forming Analysis

Format Fixed 41-45

Free 5th

Data Entry Entry I

Strain rate sampling method: 0 Sampling is done over elements with strain rate > cut-off factor (field 2) * target strain rate. If no elements exist, sampling is done over all elements. 1 (default) Averaging is done over elements with strain rate > cut-off factor (field 2) * maximum strain rate. The cut-off factor can vary between 0 (all elements will be sampled) and 1 (only elements with maximum strain rate will be sampled). Recommended value range for cut-off factor is 0.7 to 0.9 (default is 0.8). The cut-off factor is also used to smooth out the maximum strain rate in the mesh.

4th data block This data block controls the process driving parameters. 1-10

1st

I

Number of sets to define pressure orientation.

Repeat the 5th and 6th data blocks for the number of sets defined. 5th data block 1-10

1st

I

Pressure orientation

6th data block Enter list of distributed load indices. 7th data block This data block controls the analysis termination criteria. Enter the fraction of the total nodes that must come into contact before the analysis is stopped.

Main Index

THERMAL LOADS (History Definition) 1499 Define Thermal Loads

THERMAL LOADS (History Definition)

Define Thermal Loads

Description This option allows input of temperature and other state variables (see STATE VARS parameter). Used here, the loads are incremental; in that, they are in addition to any loads previously applied. The loads are total loads only if the ELASTIC parameter is used. You can specify either a uniform or nonuniform change in temperature (or other state variables). If a nonuniform change is desired, the change of every state variable at every layer of every integration point of every element must be specified. In this case, Marc calls the CREDE user subroutine for every element in the mesh. (See the THERMAL LOADS model definition option for more information.) If the Fourier decomposition method is being used to analyze an arbitrarily loaded axisymmetric structure, the THERMAL LOADS option must be invoked separately for each Fourier series term that has temperatures (state variables) associated with it. If there is no variation of these variables in the circumferential direction, only the zeroth term of the series should be specified. This option is not supported with the table driven input format; use INITIAL STATE and CHANGE STATE or INITIAL TEMP and POINT TEMP instead. Note:

On a restart run, any THERMAL LOADS option before the END OPTION reads data.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words THERMAL LOADS.

I

Set to 1 if uniform increment temperature (state variable) increment is applied to all elements.

2nd data block 1-5

1st

Set to 2 if nonuniform incremental total temperature (state variable) is read via the CREDE user subroutine. Set to 3 if nonuniform total temperature (state variable) is read via the CREDE user subroutine.

Main Index

1500 THERMAL LOADS (History Definition) Define Thermal Loads

Format Fixed

Free

Data Entry Entry

3rd data block 1-80

1st

F

Include only if the first field of data line 2 is 1; enter the uniform increments in temperature and any additional state variables in (8E10.3) format is applied to all elements.

F

Include only if the first field of data line 2 is 2 or 3, and using the default CREDE user subroutine. Temperature and state variable data to be read in by CREDE. All lines should contain 8 values in (8E10.3) format; do not start a new data line for each element.

4th data block 1-80

Main Index

1st

AUTO THERM 1501 Specify Data for Automatic Thermal Loading

AUTO THERM

Specify Data for Automatic Thermal Loading

Description This option is intended to allow automatic, static, elastic-plastic, thermally loaded stress analysis based on a set of temperatures defined throughout the mesh as a function of time. The temperatures are presented to Marc through the CHANGE STATE option using any of the input possibilities of that option, and Marc then creates its own set of temperature steps based on a temperature change tolerance provided on this option. You should recall that the elastic-plastic stress analysis is time independent, but that the strain increments should be small to obtain accuracy in the integration of the rate equations of plasticity. As a guideline, the maximum thermal strain should be restricted to 20%–50% of the strain to cause yield, depending on how much free thermal expansion is possible. Based on this argument, a temperature change tolerance of 20%–50% of

σ -------- , Eα

where

σ

is the yield stress, E is Young’s modulus and α is the

coefficient of thermal expansion, should be set. Given your temperature change tolerance on this option, Marc proceeds through your definition of the history of the temperatures provided on the CHANGE STATE set, and linearly subdivides or merges together the user-defined steps so as to conform to the tolerance. The automatic thermally loaded analysis continues until all steps indicated on the CHANGE STATE option are completed, so that a typical automatic thermally loaded analysis would have as input: AUTO THERM 30., 0, 0, 4.0, CHANGE STATE 1, 3, 0, 19, 1, 15, 1, In the above case, a temperature change tolerance of 30 is set for the creation of temperature steps by Marc; the total transient time in thermal analysis is 4.0. The data in the CHANGE STATE option indicates that the temperatures are stored in a formatted post file (unit 19) and there are 15 sets of temperatures on the file. Mechanical Loading - No Table Driven Input If no DIST LOADS, POINT LOAD, or PROPORTIONAL INCREMENT options appear with the AUTO THERM set, all mechanical loads and kinematic boundary conditions are held constant during the AUTO THERM. However, DIST LOADS, POINT LOAD, PROPORTIONAL INCREMENT, or DISP CHANGE can be included in the set – the mechanical loads and kinematic boundary conditions, which are then defined, are assumed to change in proportion to the time scale of the temperature history defined by the CHANGE STATE option and are applied accordingly, on the basis that the increments of load and displacement correspond to the end of the transient time (TOTIM) of the AUTO THERM input.

Main Index

1502 AUTO THERM Specify Data for Automatic Thermal Loading

Mechanical Loading - Table Driven Input When table input is used and either FIXED DISP, POINT LOAD, or DIST LOADS references a table which is a function of time, the total mechanical boundary condition will be evaluated based upon the current time. Notes:

All load options must be specified before AUTO THERM. The CHANGE STATE option must follow the AUTO THERM option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words AUTO THERM.

2nd data block 1-10

1st

F

Enter the maximum temperature change to be used per step of stress analysis. Marc linearly subdivides steps or merges steps together to create increments which are close to, but do not exceed, this tolerance.

11-15

2nd

I

Enter the maximum number of increments to be allowed in this AUTO THERM. If this number of increments is exceeded before the temperature history is completed, Marc ends. This is intended as a protection to avoid excessive increments in the case of a data error. Default value is 50 increments if set to 0.

16-20

3rd

I

Reassembly interval for element matrices.

21-30

4th

F

Total transient time, TOTIM. This is used to proportionally scale the incremental boundary conditions. If TOTIM is equal to zero, mechanical loads given with this group are applied for each increment in this group. If TOTIM is unequal to zero, then the mechanical loads specified in this group are linearly scaled. If the temperatures are obtained from a previous heat transfer analysis/post file, enter the total time period of the heat transfer analysis.

31-40

Main Index

5th

F

Maximum time step allowed per step of stress analysis. Marc linearly subdivides steps or merges steps to create increments which are close to, but do not exceed, this tolerance. Both the maximum temperature change allowed and the maximum time step allowed tolerances must be satisfied.

CHANGE STATE (History Definition) 1503 Change State Variables

CHANGE STATE (History Definition)

Change State Variables

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option provides various ways of changing the state variables throughout the model. State variables are initialized in the INITIAL STATE model definition set. The number of state variables per point is defined in the STATE VARS parameter. The default is one with temperature always being the first state variable at a point. If more than one state variable per point has been assigned, this option can be used repeatedly to change the values of all state variables. The default value is no change if this option is not used. In this option, the values of the state variable at the end of the current increment are read in. When the temperature is being defined, the following points should be noted: • For “history following analysis”, the thermal strains are based on temperature change during this

step. • For elastic re-analysis (ELASTIC parameter), the thermal strains are always based on temperature

change between the initial, stress free temperature field and the values read in here. • The AUTO LOAD option is available for specifying a time-varying history of state variables. The

value of the total state variable at the end of each increment is specified. • The AUTO THERM option is available for automatic control of a nonlinear (elastic-plastic)

temperature loaded stress problem, to be used in conjunction with this option. • The THERMAL LOADS option can be used as an alternative to input the change of temperature.

Either incremental or total temperatures can be specified using this option. • The AUTO THERM CREEP option is available for automatic control of a thermally loaded

elastic-plastic-creep problem and is to be used in conjunction with this option. • The AUTO STEP option is available for automatic control of a nonlinear thermally loaded

problem, to be used in conjunction with this option. Time steps based on default recycling criteria and/or user-defined physical criteria are used to determine appropriate state variable increments. Four ways of changing any state variable through CHANGE STATE are possible: • Read a range of elements, integration points, and layers, and a corresponding state variable value

for the end of the current step. • Read the state variable values for the end of the current step through user subroutine NEWSV.

Main Index

1504 CHANGE STATE (History Definition) Change State Variables

• Read the state variable values for the end of the current step from a named step of the post file

output from a previous heat transfer analysis with Marc. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately the user. Providing state variables through the thermal post file is currently supported for AUTO LOAD, AUTO THERM, AUTO THERM CREEP and AUTO STEP. It is not supported other adaptive stepping procedures.

• For AUTO LOAD, a one-to-one correspondence between the thermal increments on the post file and the mechanical increments is assumed between the user-defined starting and ending post increments. • For AUTO THERM or AUTO THERM CREEP, based on the user-defined allowable temperature change, the thermal increments on the post file can be subdivided into many mechanical increments. • For AUTO STEP, thermal values on the post file are used to determine interpolated values of state variables for the mechanical run. The interpolation is based on how the current mechanical loadcase time compares with the times read in from the thermal post file. Use of a state variable criterion to control the temperature increment is optional. The starting increment to be read in from the thermal post file (5th field of the 2nd data block) is user-defined. The number of sets of input to be read in (6th field of the 2nd data block) is not supported for AUTO STEP. Instead, the thermal information is read till the mechanical loadcase time or the thermal post file is completed. The post file is rewound and read from the beginning at the start of each loadcase or at any time a cutback is used by the AUTO STEP algorithm to reduce the current time step. • Read a list of elements, integration points, and layers, and a corresponding state variable value.

It should be noted that the end of the current step is interpreted as the end of the current increment for fixed stepping procedures (AUTO LOAD, DYNAMIC CHANGE, CREEP INCREMENT) and as the end of the loadcase for adaptive stepping procedures (AUTO STEP, AUTO THERM, AUTO INCREMENT, AUTO CREEP). Note:

Main Index

Using this option, total state variable values are input. From Marc 2001 onwards, the incremental change in the state variables is reset to 0 before each new increment if the AUTO LOAD option is used.

CHANGE STATE (History Definition) 1505 Change State Variables

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words CHANGE STATE.

I

Enter the state variable identifier for the state variable being changed (1,2,3,etc.) 1 = temperature. If more than one state variable is being used, the STATE VARS parameter must be included.

2nd data block 1-5

1st

Enter -1 if multiple state variables are read from a post file. In this case, the 9th data block is also required. 6-10

2nd

I

Enter 1 to change the state variable via the 3rd and 4th data blocks below. In this case, the third field must also be defined, and the sixth field if the AUTO THERM option is in use. Enter 2 to change the state variable via the NEWSV user subroutine. This subroutine is now called in a loop on all the elements in the mesh. Enter 3 to read the new values of the state variable from a post file written by a previous heat transfer analysis. In this case, the fourth and fifth field must be defined, and the sixth field if the AUTO THERM option is in use. Enter 4 to change the state variable via data blocks 5, 6, 7, and 8 below.

Main Index

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. In that case, this entry gives the number of data blocks set in data blocks 3 and 4 used to input the new value of the state variable (optional).

16-20

4th

I

Only nonzero if the second field is set to 3. Then. this entry defines the unit number from which the post file information from the previous heat transfer run is read. Defaults to unit 24 for a formatted post file, and to unit 25 for a binary post file.

21-25

5th

I

Only nonzero if the second field is set to 3. In that case, this entry defines the step number on the heat transfer run post file to be read as the definition of the new value of the state variable at the end of the current step. This is currently only supported for AUTO LOAD, AUTO THERM, and AUTO STEP.

26-30

6th

I

Only used if the AUTO LOAD or AUTO THERM options are in use. Give the number of sets of input to be read to define the temperature history. Not used for AUTO STEP.

31-35

7th

I

Enter 1 if formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2.

1506 CHANGE STATE (History Definition) Change State Variables

Format Fixed

Free

Data Entry Entry Set to 1 to suppress printout of state variable values that are defined in NEWSV.

41-45

9th

I

Enter the post code number to be read into this state variable; default is 9 (temperature).

Data blocks 3 and 4 are only input if the second field above is set to 1. In that case, the number of sets is equal to the number given in the third field above. 3rd data block 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with this value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value (11-15 and 16-20 can only be bigger than 1 if ALL POINTS parameter is used).

21-25

5th

I

First layer or cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value (21-25 and 26-30 can only be bigger than 1 for beam or shell elements).

F

New value of this state variable for the above range of points at the end of the current step.

4th data block 1-10

1st

Data blocks 5, 6, 7, and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block 1-10

1st

F

New total value of this state variable for the points given below at the start of the zeroth increment.

6th data block Enter a list of elements to which the above state variable is applied. 7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above state variable is applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above state variable is applied.

Main Index

CHANGE STATE (History Definition) 1507 Change State Variables

Format Fixed

Free

Data Entry Entry

The 9th data block is required only if multiple state variables are read from a post file if the first field of the 2nd data block is -1. 9th data block 1-80

Main Index

I

Enter a list of state variables.

1508 POINT TEMP (History Definition) Define Point Temperatures

POINT TEMP (History Definition)

Define Point Temperatures

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option defines temperatures at nodal points for an uncoupled thermal stress problems at the end of the increment. Note:

For shell analyses, a uniform temperature is used through the thickness direction.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT TEMP.

2nd data block 1-5

1st

I

Enter the number of sets of prescribed temperatures (optional).

6-10

2nd

I

Enter file number for input of prescribed temperatures data; defaults to input.

The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine is required. Enter 1 if the USINC user subroutine is used.

Main Index

11-15

3rd

I

Flag to indicate that temperatures are read from previously generated post file. Set to 1.

16-20

4th

I

Only nonzero if the third field is set to 1. Then, this entry defines the unit number from which the post file information is read.

21-25

5th

I

Enter step number to be read.

POINT TEMP (History Definition) 1509 Define Point Temperatures

Format Fixed

Free

Data Entry Entry

26-30

6th

I

Enter 1 if a formatted post file is used.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

If data is read from post file, the 4th through 7th blocks may be skipped. 4th data block 1-10

1st

F

Enter the magnitude of the temperature.

I

Enter the table ID associated with the temperature.

5th data block 1-5

1st

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 2 - Node IDs 3 - Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above initial conditions are applied. the geometric entities must all be of the type prescribed in the 6th data block.

1510 CHANGE PORE (History Definition) Define Pore Pressures for Uncoupled Soil Analysis

CHANGE PORE (History

Define Pore Pressures for Uncoupled Soil Analysis

Definition) The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option provides various ways of changing the pore pressure throughout the model. This option is only used in uncoupled soil analysis. Given below are four ways of providing the pore pressures. 1. Read a range of elements, integration points and layers, and corresponding pore pressures for the end of the current step. 2. Read the pore pressure values for the end of the current step through the NEWPO user subroutine. 3. Read the pore pressure values for the end of the current step from a named step of the post file output from a previous pore pressure analysis with Marc. With this option, Marc assumes direct correspondence of the post file elements with the elements in the current analysis. Any spatial interpolation must be provided separately by you. 4. Read a list of elements, integration points and layers, and corresponding pore pressure. Note:

On this option, total pore pressures are input.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words CHANGE PORE.

2nd data block 1-5

1st

I

Enter 1.

6-10

2nd

I

Enter 1 to change the pore pressure via data block 3 below. In this case, the third field must also be defined. Enter 2 to change the pore pressure via the NEWPO user subroutine. This subroutine is then called in a loop on all the elements in the mesh.

Main Index

CHANGE PORE (History Definition) 1511 Define Pore Pressures for Uncoupled Soil Analysis

Format Fixed

Free

Data Entry Entry Enter 3 to read the initial values of the pore pressure from the post file written by a previous pore pressure analysis. In this case, the fourth and fifth field must also be defined. Enter 4 to change the pore pressure via data blocks 5, 6, 7 and 8 below.

11-15

3rd

I

Only nonzero if the second field is set to 1 or 4. In that case, this entry gives the number of block sets in series 3 and 4 used to input the new value of the pore pressure (optional).

16-20

4th

I

Only nonzero if the second field is set to 3. Then, this entry defines the unit number from which the post file information from the previous pore pressure run is read.

21-25

5th

I

Only nonzero if the second field is set to 3. In that case, this entry defines the step number on the pore pressure run post file to be read as the definition of the new value of the pore pressure at the end of the current step.

26-30

6th

I

Not used; enter 1.

31-35

7th

I

Enter 1 if a formatted post file is used.

36-40

8th

I

Only nonzero if the second field is set to 2. Set to 1 to suppress printout of pore pressure values that are defined in the NEWPO user subroutine.

Data blocks 3 and 4 are only input if the second field above set to 1. In that case, the number of block sets is equal to the number given in the third field above. 3rd data block 1-5

1st

I

First element with this value.

6-10

2nd

I

Last element with this value.

11-15

3rd

I

First integration point with this value.

16-20

4th

I

Last integration point with this value can only be bigger than 1 if the ALL POINTS parameter is used.

21-25

5th

I

First layer or cross-section point with this value.

26-30

6th

I

Last layer or cross-section point with this value.

F

New value of the pore pressure for the above range of points at the end of the current step.

4th data block 1-10

1st

Data blocks 5, 6, 7 and 8 are only input if the second field above is set to 4. In that case, the number of sets is equal to the number given in the third field above. 5th data block

Main Index

1512 CHANGE PORE (History Definition) Define Pore Pressures for Uncoupled Soil Analysis

Format Fixed 1-10

Free 1st

Data Entry Entry F

Pore pressure for the points given below at the end of the current increment.

6th data block Enter a list of elements to which the above pore pressure is to be applied. 7th data block This data block is not necessary if the CENTROID parameter is used. Enter a list of integration points to which the above pore pressure is to be applied. 8th data block This data block is only necessary if there are either beams or shells in the mesh. Enter a list of layer points to which the above pore pressure is to be applied.

Main Index

TIME STEP 1513 Define Time Step

TIME STEP

Define Time Step

Description This option allows you to enter a time step for static analysis.This option can be used to prescribe the time step in a contact analysis. This time step can be used in conjunction with strain rate effects (CREEP, VISCO ELAS) option. This time step is used for this step or series of steps if AUTO LOAD is used. This time step is not scaled by the proportional increment option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words TIME STEP.

F

Enter time step.

2nd data block 1-10

Main Index

1st

1514 RESET TIME Resets Time to Zero

RESET TIME

Resets Time to Zero

Description In multi-stage forging, it is often useful to consider each stage beginning at time = 0.0. This facilitates the definition of tool velocities, and is useful for postprocessing. This option allows you to reset the time, at the beginning of the increment. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words RESET TIME.

E

Enter the time at beginning of step.

2nd data block 1-10

1st

Default is 0.0.

Main Index

BUCKLE 1515 Specify Buckling Analysis

BUCKLE

Specify Buckling Analysis

Description This sets a flag for the buckling analysis and solves the eigenvalue problem by the inverse power sweep method or the Lanczos method. The number of modes and the procedure used is specified on the BUCKLE parameter. This option can be exercised after every increment of load. The LARGE DISP parameter should be included for nonlinear collapse analysis. This option can also be used to control perturbation analyses. The perturbation is added to the coordinates in the increment following the eigenvalue extraction. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word BUCKLE.

I

Maximum number of iterations allowed.

2nd data block 1-5

1st

Not used for Lanczos. Enter 0. Default is 40. 6-15

2nd

F

Convergence tolerance. The power sweep terminates when the difference between the eigenvalues in two consecutive sweeps divided by the eigenvalue is less than the tolerance. Not used for Lanczos. Enter 0. Default is 0.0001.

16-20

3rd

I

Enter the harmonic number for Fourier buckling; positive number results in cosine terms, negative number results in sine terms. Default is zero.

21-25

4th

I

Enter 1 for buckling perturbation to occur in the next increment.

26-30

5th

I

Enter mode number to be used in the perturbation analysis. Enter negative number of modes if multiple modes are used in the perturbation analysis.

31-40

Main Index

6th

F

Enter the scale factor to be multiplied with the normalized mode and added to the coordinates in the next increment.

1516 BUCKLE Specify Buckling Analysis

Format Fixed 41-50

Free 7th

Data Entry Entry F

Solution scaling factor for linear analysis. If the applied load in increment 0 is too large, the Lanczos procedure may fail; this number is used to scale the solution for numerical reasons. The collapse load will be output based upon the total load applied.

3a data block is used only if 5th field of the 2nd data block is negative. Use one line for each mode. 3a data block

Main Index

1-5

1st

I

Mode number.

6-15

2nd

F

Scale factor.

SUPERELEM (History Definition) 1517 Perform Craig-Bampton Analysis for MD Adams MNF Interface

SUPERELEM (History Perform Craig-Bampton Analysis for MD Adams MNF Interface Definition) Description This option triggers Marc to perform the Craig-Bampton method of Component Mode Synthesis and generate a Modal Neutral File (MNF) that can be uploaded into MD Adams models to represent flexible components. The option allows direct definition of the boundary or interface degrees of freedom. The option also allows automatic definition of interface degrees of freedom of the nodes that get in contact with selected rigid contact bodies. This is very useful for some nonlinear analyses such as tire footprint analysis in which the interface degrees of freedom are not known a priori. It also allows the specification of interface degrees of freedom of the control nodes of selected load-controlled rigid contact bodies. The two control nodes for load-controlled rigid bodies are consolidated into one node with six degrees of freedom before exporting to the MNF. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SUPERELEM.

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter 1 to generate MNF.

2nd data block

The 3rd and 4th data blocks are entered as pairs. Data blocks 3a and 4a may be repeated if needed. A. List of Interface Degrees of Freedom. 3a data block 1-80

1st

I

Enter a list of degrees of freedom.

1st

I

Enter a list of interface nodes.

4a data block 1-80

B. List of Rigid Contact Bodies. All degrees of freedom of all nodes in contact with these bodies will be interface degrees of freedom. 3b data block 1-5

1st

I

Enter -1.

1st

I

Enter a list of rigid contact bodies.

4b data block 1-80

Main Index

1518 SUPERELEM (History Definition) Perform Craig-Bampton Analysis for MD Adams MNF Interface

Format Fixed

Free

Data Entry Entry

C. List of Load-controlled Rigid Contact Bodies. All degrees of freedom of the control nodes of these bodies will be interface degrees of freedom. 3c data block 1-5

1st

I

Enter -2.

1st

I

Enter a list of load-controlled rigid contact bodies.

4c data block 1-80

Main Index

SUPERELEM (DMIG Applications - History Definition) 1519 Create DMIG of Substructure

SUPERELEM (DMIG Applications - History Definition) Create DMIG of Substructure Description This option allows the creation of a DMIG file containing the stiffness associated with the degrees of freedom specified here. This DMIG may be subsequently read into Marc or Nastran. The option allows direct definition of the degrees of freedom. The option also allows automatic definition of interface degrees of freedom of the nodes that get in contact with selected rigid contact bodies. This is very useful for some nonlinear analyses such as tire footprint analysis in which the interface degrees of freedom are not known a priori. It also allows the specification of interface degrees of freedom of the control nodes of selected load-controlled rigid contact bodies. The two control nodes for load-controlled rigid bodies are consolidated into one node with six degrees of freedom before exporting to the DMIG. This option can only occur once in the analysis. However, it may be used in either the model definition or the load increment section. The DMIG will be written to file jidname_dmigst_inc, where: jidname

is the job name

inc

is the increment number

Notes:

If a node is subsequently going to be transformed, all degrees of freedom of all nodes must be specified here. If a rigid body rotation is to be applied to the DMIG, all degrees of freedom of all nodes must be specified here.

This option may only be used with direct solution techniques. Format Format Fixed

Free

Data Entry Entry

1st data block 1st

A

Enter the word SUPERELEM.

1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

1-10 2nd data block

Main Index

1520 SUPERELEM (DMIG Applications - History Definition) Create DMIG of Substructure

Format Fixed 16-20

Free 4th

Data Entry Entry I

Enter 1 to create DMIG file. Enter 3 to create a DMIGB file. DMIGB uses a different output format, which results in a smaller file (about one third of the size of a DMIG file). When a DMIGB file is included in a Marc analysis, the program uses a column-wise storage instead of a full in-core matrix storage. This memory reduction can be important for large DMIG files. The DMIGB format can be used only as input for a Marc analysis; it can not be used in a Nastran analysis.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 0 if all stiffness terms written to DMIG. Enter 1 if terms less than

x f ⋅ K1

Enter 2 if terms less than

xf

are filtered out.

are filtered out.

31-40

7th

F

Enter the value used for filtering

41-50

8th

A

Enter the name of the matrix; default is KAAX which is limited to eight characters.

xf ;

default = 1.e-8.

The 3rd and 4th data blocks are entered as pairs. Data blocks 3a and 4a may be repeated if needed. A.

List of Interface Degrees of Freedom.

3a data block 1-80

1st

I

Enter a list of degrees of freedom.

1st

I

Enter a list of interface nodes.

4a data block 1-80

B. List of Rigid Contact Bodies. All degrees of freedom of all nodes in contact with these bodies will be interface degrees of freedom. 3b data block

1-5

1st

I

Enter -1.

1st

I

Enter a list of rigid contact bodies.

4b data block 1-80

C. List of Load-controlled Rigid Contact Bodies. All degrees of freedom of the control nodes of these bodies will be interface degrees of freedom. 3c data block

Main Index

SUPERELEM (DMIG Applications - History Definition) 1521 Create DMIG of Substructure

Format Fixed 1-5

Free

Data Entry Entry

1st

I

Enter -2.

1st

I

Enter a list of load-controlled rigid contact bodies.

4c data block 1-80

Main Index

1522 ASSEM LOAD Assemble Equivalent Nodal Force Vector

ASSEM LOAD

Assemble Equivalent Nodal Force Vector

Description This option signals Marc to compute only the equivalent nodal force vector for all loads defined in this loadcase. These loads are not applied to the finite element model and no matrix solution takes place for this loadcase. In the case of Marc - MD Adams MNF interface, Marc projects the computed equivalent nodal force vectors onto the modal space and exports them to the MNF as modal loads. MD Adams models can then make use of these modal loads; e.g., by scaling them up or down, before applying them in MD Adams. For MNF generation, all ASSEM LOAD loadcases should appear in the input file before any actual loading is applied to the component. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words ASSEM LOAD.

ACTIVATE 1523 Activate Elements

ACTIVATE

Activate Elements

Description This option allows you to activate elements which were deactivated either before the start of the analysis or during the analysis. Elements, which were deactivated before analysis, have zero internal stress upon activation. Elements, which were used earlier and deactivated during analysis, have an internal stress which is equal to the state when they were deactivated or zero if requested on the DEACTIVATE option. Elements can be activated and deactivated as often as needed. Note that activation of elements results in an increase in the size of the stiffness matrix. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ACTIVATE.

11-20

2nd

A

Enter the word POST to update the post file geometry so the activated elements are shown.

21-30

3rd

A

Enter the word NOPO to not update the post file geometry; the activated elements are not shown.

2nd data block 1-80

Main Index

1st

I

Enter the list of elements that are to be activated at this time.

1524 DEACTIVATE (History Definition) Deactivate Elements

DEACTIVATE (History Definition)

Deactivate Elements

Description The DEACTIVATE option has two choices. Option A This option is the default method. This option allows the manual deactivation of elements during the course of an analysis, which can be useful to model ablation, excavation and other problems. By default, after the elements are deactivated, they demonstrate zero stresses and strains on the post file. However, internally, they retain the stress state in effect at the time of deactivation and this state can be postprocessed or printed at any time. At the later stage in the analysis, the elements can again be activated with the ACTIVATE history definition option. As an alternative, one can use the UACTIVE user subroutine. The stress state is restored in the post file when the elements are reactivated. If this is not desirable, stress/strain states can be permanently set to zero at deactivation by using the additional command line option STRESS/STRAIN. Option B This option allows one to automatically deactivate elements according to the cutter path defined by either Automatically Programmed Tools (APT) source or Cutter Location (CL) data files. This is useful for modeling NC machining (for example, metal cutting or material removal) processes. Marc has an interface to translate the cutter path information into a series of elements to be deactivated. The deactivated elements are not postprocessed or printed. The post file only includes the elements that remain in the model. This method can be chosen by setting the second field of the first data block as CUTTING and specifying the APT/CL file name in the second data block. APT/CL data files should be located in the same directory as the input data file jid.dat. Notes:

The typical definition of APT source file or CL file is shown as below: cutterpath.apt cutterpath.ccl

where the extensions .apt or .ccl are used to distinguish these two types of cutter path data. For example, if the Marc input data specifies the cutter path file name as: cutterpath without either the extension .apt or .ccl, the Marc program looks for either type of cutter path file by adding the extension .apt or .ccl. The first file found existing in the input data directory is used for the analysis. This option must be combined with MACHINING parameter. In the current release, this option can only be used with the AUTO LOAD option.

Main Index

DEACTIVATE (History Definition) 1525 Deactivate Elements

Format Format Fixed

Free

Data Entry Entry

Option A 1st data block 1-10

1st

A

Enter the word DEACTIVATE.

11-20

2nd

A

Enter the word STRESS to set the stresses to zero.

21-30

3rd

A

Enter the word STRAIN to set the strains to zero.

31-40

4th

A

Enter the word POST to update the post file geometry so deactivated elements are not shown.

41-50

5th

A

Enter the word NOPO to not update the post file geometry; the deactivated elements are shown.

2nd data block This is needed for Option A. 1-80

1st

I

Enter the list of elements to be deactivated at this time.

Option B 1st data block 1-10

1st

I

Enter the word DEACTIVATE.

11-20

2nd

A

Enter the word CUTTING if MACHINING feature is to be used.

2nd data block This is needed for Option B. 1-80

1st

A

Enter the name of the file that defines the cutter path.

3rd data block 1-10

1st

I

Enter 0 for NC Machining (default)

11-20

2nd

I

Enter 0 if no time synchronization between the time defined by the load case definition option and the real calculated time based on cutter motion defined by the APT/CL file. Enter 1 if time synchronization is needed between the time defined by the load case definition option and the real calculated time based on cutter motion defined by the APT/CL file. In this case, a factor is applied to the calculated time based on cutter motion.

21-30

3rd

I

Enter the ID of the rigid contact body which is defined by cutter if the user wants to visualize the cutter motion of the cutting process. Default is set to 0.

Main Index

1526 DEACTIVATE (History Definition) Deactivate Elements

Format Fixed 31-40

Free 4th

Data Entry Entry I

Enter 0 if the time spent for rapid cutter motion is to be ignored. Enter 1 if the adaptive remeshing is to be performed for every cutter motion step. Enter 2 if the adaptive remeshing is only performed at the end of the cutting process. Default is set to 0.

41-50

5th

I

Enter 0 if the speed of the rapid cutter motion is the same as the regular cutting speed of cutter. Enter 1 if the speed of the rapid cutter motion is provided by the user. Default is set to 0.

51-65

6th

F

Enter the rapid motion speed of cutter if the fifth field is equal to 1. Default is set to 0.

Main Index

FOUNDATION (History Definition) 1527 Define Foundation Spring Force for Elements

FOUNDATION (History Definition)

Define Foundation Spring Force for Elements

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows the specification of elements and associated foundation spring force to be used with the elastic foundation option (Marc Volume A: Theory and User Information). Nonlinear foundations are available via the USPRNG user subroutine (see Marc Volume D: User Subroutines and Special Routines). Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word FOUNDATION.

2nd data block 1-5

1st

I

Number of sets of data blocks to be used to input the lists of element and foundation stiffnesses (optional).

6-10

2nd

I

Enter unit number for input of foundation data. Defaults to input.

3rd data block The 3rd and 4th data blocks are entered as pairs, once for each list. 1-5

1st

I

Parameter identifying the type of elastic foundation; this is the same parameter as used in the DIST LOADS option. See Marc Volume B: Element Library for a description of the possible distributed load types for each element type in Marc.

6-15

2nd

E

Spring stiffness per unit surface area (or per unit length for beam elements).

4th data block 1-80

Main Index

1st

Enter a list of elements to which the above foundation is applied.

1528 CHANGE RIGID Define New Geometry For a Rigid Contact Surface

CHANGE RIGID

Define New Geometry For a Rigid Contact Surface

Description This option allows for the input of a new geometry for an existing rigid contact surface. The procedure used to control the surface motion (displacement controlled, velocity controlled, or load controlled) will not change. The position of the reference point of the rigid surface is also not changed. It is good engineering practice to first move the rigid surface away from deformable bodies such that it is not in contact before changing the geometry of the rigid body. Otherwise, penetration may occur. This option may be used multiple times to change different contact bodies. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the word CHANGE RIGID.

2nd data block 1-5

1st

I

Body number (must be an existing rigid body).

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY).

11-15

3rd

I

Not used enter 0

16-20

4th

I

Enter 1 if geometry will be defined with respect to original position of this body (default if 0 is entered). Enter 2 if geometry will be defined with respect to current position of this body.

21-25

5th

I

Enter 1 if analytic form is to be used.

A

Contact body name (optional)

3rd data block 1-32

1st

The 4th through 11th data blocks are repeated for as many geometrical data as required (NETTY). A. For 2-D Rigid Body (Line-Segment) 4a data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 5a data block is repeated once for each point entered.

Main Index

CHANGE RIGID 1529 Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

5a data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

B. For 2-D Rigid Body (Circular Arc) 4b data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD).

The 5b data block is repeated four times. 5b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Spline) 4c data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 5c data block is repeated for each point to be entered. 5c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (NURBS) 4d data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 5d data block is repeated NPTU times for control points 5d data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 6d data block is repeated NPTU times for homogeneous coordinate.

Main Index

1530 CHANGE RIGID Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

6d data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 7d data block is repeated NPTU times for knot vectors. 7d data block 1-10

1st

F

Component of knot vector between 0 and 1.

E. For 3-D Rigid Body (Ruled Surface) 4e data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

21-25

5th

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 5e data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 5e data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

F. For 3-D Rigid Body (Surface of Revolution) 4f data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 method to describe the circular arc (METH).

Main Index

CHANGE RIGID 1531 Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 5f data block is repeated NPOINT times for surface of revolution. 5f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

6f data block 1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

G. For 3-D Rigid Surface (Bezier Surface) 4g data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 5g data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 5g data block

Main Index

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

1532 CHANGE RIGID Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

H For 3-D Rigid Surface (4-Node Patch) 4h data block 1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

16-20

4th

I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 5h data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1) 5h data block 1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 6h data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 6h data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

I. For 3-D Rigid Surface (Poly-Surface) 4i data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 5i data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces.

Main Index

CHANGE RIGID 1533 Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

5i data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

J. For 3-D Rigid Surface (NURBS) 4j data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 5j data block is repeated (NPTU ∗ NPTV) for control points. 5j data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 6j data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 6j data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 7j data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 7j data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 8j, 9j, 10j, and 11j. 8j data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 9j data block is repeated NPTU times for control points.

Main Index

1534 CHANGE RIGID Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

9j data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 10j data block is repeated NPTU times for homogeneous coordinate. 10j data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 11j data block is repeated NPTU+ NORU times for knot vectors. 11j data block 1-10

1st

F

Component of knot vector between 0 and 1.

K. For 3-D Rigid Surface (Cylinder) 4k data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

5k data block 1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

L. For 3-D Rigid Surface (Sphere) 4l data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

5l data block

Main Index

1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

CHANGE RIGID 1535 Define New Geometry For a Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

1536 ADD RIGID with TABLES (2-D) Define a New Two-dimensional Rigid Contact Surface

ADD RIGID with TABLES (2-Define a New Two-dimensional Rigid Contact Surface D) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows for the input of a new rigid contact surface. The new body will be velocity controlled. If a load controlled rigid body is added the node number(s) having the degrees of freedom associated with the rigid body must already exist in the model. This option may be used multiple times to add more than one new rigid surface. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the word ADD RIGID.

2nd data block 1-5

1st

I

Body number (must be 1 higher than the current number of bodies).

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY).

11-15

3rd

I

Not used; enter 0.

11-15

3rd

I

Enter 1 if body is a symmetry plane.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block.

Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

Main Index

ADD RIGID with TABLES (2-D) 1537 Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz 36-40

8th

I

Contact body type (optional): 1: rigid body, 3: symmetry body

3rd data block 1-32

1st

A

Contact body name (optional)

4th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of ratio.

31-40

4th

F

Initial Angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0

5th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

6th data block (Only required if a mechanical-displacement analysis)

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Growth factor of rigid surface in first coordinate direction.

1538 ADD RIGID with TABLES (2-D) Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

51-60

6th

F

Growth factor of rigid surface in second coordinate direction.

61-70

7th

F

Growth factor of rigid surface in third coordinate direction.

71-80

8th

F

Friction Coefficient.

7th data block (Only required if a mechanical-displacement analysis) 1-5

1st

I

Enter the table ID for the first component of velocity, or target position of center of rotation.

6-10

2nd

I

Enter the table ID for the second component of velocity, or target position of center of rotation.

11-15

3rd

I

Enter the table ID for the third component of velocity, or target position of center of rotation.

16-20

4th

I

Enter the table ID for the angular velocity.

21-25

5th

I

Enter the table ID for growth factor in first coordinate direction.

26-30

6th

I

Enter the table ID for growth factor in second coordinate direction.

31-35

7th

I

Enter the table ID for growth factor in third coordinate direction.

36-40

8th

I

Enter the table id for the friction coefficient.

8th data block The 8th data block is only necessary if heat transfer is included. 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY).

9th data block The 9th data block is only necessary if heat transfer is included. 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

10th data block (Only if heat transfer is included) 1-10

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

11th data block (Only if heat transfer is included) 1-5

Main Index

1st

I

Enter the table ID associated with (HBL).

ADD RIGID with TABLES (2-D) 1539 Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

12th data block (Only if Joule Heating is included) 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage (Required for rigid body only).

13th data block (Only if Joule Heating is included) 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

14th data block (Only used if coupled mass diffusion) 1-10

1st

E

Not used; enter 0.

11-20

2nd

E

Not used; enter 0.

21-30

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure.

15th data block (Only used if coupled mass diffusion) 1-5

1st

I

Not used; enter 0t.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

16th data block The 16th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

1 ----c1

reactive boundary coefficient.

17th data block The 17th data block is only necessary for harmonic acoustic analysis. 1-5

1st

I

Enter the table ID associated with

1 ----k1

reactive boundary coefficient.

6-10

2nd

I

Enter the table ID associated with

1---c1

reactive boundary coefficient.

The 18th through 21st data blocks are repeated for as many geometrical data as required (NETTY).

Main Index

1540 ADD RIGID with TABLES (2-D) Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

A. For 2-D Rigid Body (Line-Segment) 18a data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 19th data block is repeated once for each point entered. 19a data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

B. For 2-D Rigid Body (Circular Arc) 18b data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 19b data block is repeated four times. 19b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Spline) 18c data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 19c data block is repeated for each point to be entered. 19c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (NURBS) The 18d data block is repeated NPTU times for control points. 18d data block

Main Index

1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

ADD RIGID with TABLES (2-D) 1541 Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

19d data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 20d data block is repeated NPTU times for homogeneous coordinate. 20d data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 21d data block is repeated NPTU+ NORU times for knot vectors. 21d data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

1542 ADD RIGID (2-D) Define a New Two-dimensional Rigid Contact Surface

ADD RIGID (2-D)

Define a New Two-dimensional Rigid Contact Surface

The information provided here is based upon not using the table driven input style. Description This option allows for the input of a new rigid contact surface. The new body will be velocity controlled. If a load controlled rigid body is added the node number(s) having the degrees of freedom associated with the rigid body must already exist in the model. This option may be used multiple times to add more than one new rigid surface. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the word ADD RIGID.

2nd data block 1-5

1st

I

Body number (must be 1 higher than the current number of bodies).

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY).

11-15

3rd

I

Not used; enter 0.

11-15

3rd

I

Enter 1 if body is a symmetry plane.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block.

Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

Main Index

ADD RIGID (2-D) 1543 Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz 36-40

8th

I

Contact body type (optional): 1: rigid body, 3: symmetry body

3rd data block 1-32

1st

A

Contact body name (optional)

1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0.

4th data block

5th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

6th data block The 6th data block is only required for a mechanical-displacement analysis.

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

1544 ADD RIGID (2-D) Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Friction coefficient.

7th data block The 7th data block is only necessary if heat transfer is included. 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

8th data block The 8th data block is only necessary if heat transfer is included. 1-10

1st

F

Enter the separation distance dependent heat transfer film coefficient ( H BL ).

9th data block The 9th data block is only necessary for Joule heating. 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact electrical transfer coefficient.

31-40

4th

F

Body voltage (required for rigid body only).

10th data block The 10th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1---k1

reactive boundary coefficient.

11-20

2nd

F

1---c1

reactive boundary coefficient.

The 11th through 14th data blocks are repeated for as many geometrical data as required (NETTY). A. For 2-D Rigid Body (Line-Segment) 11a data block 1-5

1st

I

Enter 1 for straight line segments (ITYPE).

6-10

2nd

I

Number of points required to define polyline (NPOINT).

The 12a data block is repeated once for each point entered.

Main Index

ADD RIGID (2-D) 1545 Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

12a data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

B. For 2-D Rigid Body (Circular Arc) 11b data block 1-5

1st

I

Enter 2 for circular arc (ITYPE).

6-10

2nd

I

Method of describing circular arc (METHOD). See Figure 3-2 and Figure 3-3.

The 12b data block is repeated four times. 12b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

C. For 2-D Rigid Body (Spline) 11c data block 1-5

1st

I

Enter 3 for spline (ITYPE).

6-10

2nd

I

Number of points required to define spline (NPOINT).

The 12c data block is repeated for each point to be entered. 12c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

D. For 2-D Rigid Body (NURBS) 11d data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 12d data block is repeated NPTU times for control points. 12d data block 1-10

1st

F

First coordinate of point

11-20

2nd

F

Second coordinate of point.

If interpolation scheme is used the following two data blocks are ignored. The 13d data block is repeated NPTU times for homogeneous coordinate.

Main Index

1546 ADD RIGID (2-D) Define a New Two-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

13d data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 14d data block is repeated NPTU+ NORU times for knot vectors. 14d data block 1-10

Main Index

1st

F

Component of knot vector between 0 and 1.

ADD RIGID with TABLES (3-D) 1547 Define a New Three-dimensional Rigid Contact Surface

ADD RIGID with TABLES Define a New Three-dimensional Rigid Contact Surface (3-D) The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option allows for the input of a new rigid contact surface. The new body will be velocity controlled. If a load controlled rigid body is added the node number(s) having the degrees of freedom associated with the rigid body must already exist in the model. This option may be used multiple times to add more than one new rigid surface. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words ADD RIGID.

2nd data block 1-5

1st

I

Body number (must be 1 higher than the current number of bodies).

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY).

11-15

3rd

I

Not used enter 0

11-15

3rd

I

Enter 1 if body is a symmetry plane.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block.

Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

Main Index

1548 ADD RIGID with TABLES (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz 36-40

8th

I

Contact body type (optional): 1: rigid body, 3: symmetry body

3rd data block 1-32

1st

A

Contact body name (optional)

4th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of ratio.

31-40

4th

F

Initial Angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0

5th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach Angular velocity about local axis through center of rotation.

6th data block (Only required if a mechanical-displacement analysis.)

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Growth factor of rigid surface in first coordinate direction.

ADD RIGID with TABLES (3-D) 1549 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

51-60

6th

F

Growth factor of rigid surface in second coordinate direction.

61-70

7th

F

Growth factor of rigid surface in third coordinate direction.

71-80

8th

F

Friction Coefficient.

7th data block (Only required if a mechanical-displacement analysis.) 1-5

1st

I

Enter the table ID for the first component of velocity, or target position of center of rotation.

6-10

2nd

I

Enter the table ID for the second component of velocity, or target position of center of rotation.

11-15

3rd

I

Enter the table ID for the third component of velocity, or target position of center of rotation.

16-20

4th

I

Enter the table ID for the angular velocity.

21-25

5th

I

Enter the table ID for growth factor in first coordinate direction.

26-30

6th

I

Enter the table ID for growth factor in second coordinate direction.

31-35

7th

I

Enter the table ID for growth factor in third coordinate direction.

36-40

8th

I

Enter the table ID for the friction coefficient.

The 8th data block is only necessary if heat transfer is included. 8th data block 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact heat transfer coefficient (HCT).

31-40

4th

F

Body temperature (TBODY).

The 9th data block is only necessary if heat transfer is included. 9th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact heat transfer coefficient (HCT).

16-20

4th

I

Enter the table ID for the body temperature (TBODY).

10th data block (Only if heat transfer is included) 1-10

1st

F

Enter the separation distance dependent heat transfer film coefficient (HBL).

11th data block (Only if heat transfer is included) 1-5

Main Index

1st

I

Enter the table id associated with (HBL).

1550 ADD RIGID with TABLES (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

12th data block (Only if Joule Heating is included) 1-10

1st

F

Not used.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact Electrical transfer coefficient.

31-40

4th

F

Body voltage.

13th data block (Only if Joule Heating is included) 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact electrical transfer coefficient.

16-20

4th

I

Enter the table ID for the body voltage.

14th data block (Only used if coupled mass diffusion) 1-10

1st

E

Not used; enter 0.

11-20

2nd

E

Not used; enter 0.

21-30

3rd

E

Enter the contact mass flow rate coefficient.

31-40

4th

E

Enter the body pressure.

15th data block (Only used if coupled mass diffusion) 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Enter the table ID for the contact mass flow rate coefficient.

16-20

4th

I

Enter the table ID for the body pressure.

16th data block The 16th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

1 ----c1

reactive boundary coefficient.

17th data block The 17th data block is only necessary for harmonic acoustic analysis. 1-5

1st

I

Enter the table id associated with

1 ----k1

reactive boundary coefficient.

6-10

2nd

I

Enter the table id associated with

1---c1

reactive boundary coefficient.

The 18th through 25th data blocks are repeated for each set of body entities (NETTY).

Main Index

ADD RIGID with TABLES (3-D) 1551 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

A. For 3-D Rigid Body (Ruled Surface) 18a data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

21-25

5th

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 19a data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 19a data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

B. For 3-D Rigid Body (Surface of Revolution) 18b data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 19b data block is repeated NPOINT times for surface of revolution.

Main Index

1552 ADD RIGID with TABLES (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

19b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

20b data block 1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

C. For 3-D Rigid Surface (Bezier Surface) 18c data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 19c data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 19c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

D. For 3-D Rigid Surface (4-Node Patch) 18d data block

Main Index

1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

ADD RIGID with TABLES (3-D) 1553 Define a New Three-dimensional Rigid Contact Surface

Format Fixed 16-20

Free 4th

Data Entry Entry I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 19d data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1) 19d data block 1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 20d data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 20d data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

E. For 3-D Rigid Surface (Poly-Surface) 18e data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 19e data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 19e data block

Main Index

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

1554 ADD RIGID with TABLES (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

F. For 3-D Rigid Surface (NURBS) 18f data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 19f data block is repeated (NPTU ∗ NPTV) for control points. 19f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 20f data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 20f data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 21f data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 21f data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 22f, 23f, 24f, and 25f. 22f data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 23f data block is repeated NPTU times for control points. 23f data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 24f data block is repeated NPTU times for homogeneous coordinate.

Main Index

ADD RIGID with TABLES (3-D) 1555 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

24f data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 25f data block is repeated NPTU+ NORU times for knot vectors. 25f data block 1-10

1st

F

Component of knot vector between 0 and 1.

G. For 3-D Rigid Surface (Cylinder) 18g data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

19g data block 1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. Note:

If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

H. For 3-D Rigid Surface (Sphere) 18h data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

19h data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

1556 ADD RIGID (3-D) Define a New Three-dimensional Rigid Contact Surface

ADD RIGID (3-D)

Define a New Three-dimensional Rigid Contact Surface

The information provided here is based upon not using the table driven input style. Description This option allows for the input of a new rigid contact surface. The new body will be velocity controlled. If a load controlled rigid body is added the node number(s) having the degrees of freedom associated with the rigid body must already exist in the model. This option may be used multiple times to add more than one new rigid surface. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words ADD RIGID.

2nd data block 1-5

1st

I

Body number (must be 1 higher than the current number of bodies).

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY).

11-15

3rd

I

Not used enter 0

11-15

3rd

I

Enter 1 if body is a symmetry plane.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block.

Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other.

Main Index

ADD RIGID (3-D) 1557 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz 36-40

8th

I

Contact body type (optional): 1: rigid body, 3: symmetry body

3rd data block 1-32

1st

A

Contact body name (optional)

The 4th through the 15th data blocks are repeated once for each body to be defined. 4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of body entities, NSURGN, to be input for this rigid body. Enter 0 if deformable body.

11-15

3rd

I

For rigid bodies, enter 1 if body is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that in this case, results are dependent upon the order in which contact bodies are defined.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block.

Both nodes of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in the user-defined directions. Note also that it is not necessary for the user-defined directions at the nodes to be identical to each other. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option.

Main Index

1558 ADD RIGID (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

Node 1 has x-, y-, and z-displacement as degrees of freedom 1, 2 and 3 Node 2 has x-,y-, and z-rotation as degrees of freedom 1, 2 and 3 The rotation is defined as: Rx.Ry.Rz 36-40

8th

I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body; 4: heat-rigid body; 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

5th data block 1-10

1st

F

First coordinate of initial position of center of rotation.

11-20

2nd

F

Second coordinate of initial position of center of rotation.

21-30

3rd

F

Third coordinate of initial position of center of rotation.

31-40

4th

F

Initial angular position.

41-50

5th

F

First component direction cosine of local axis. Default = 0.0.

51-60

6th

F

Second component direction cosine of local axis. Default = 0.0.

61-70

7th

F

Third component direction cosine of local axis. Default = 1.0.

6th data block 1-10

1st

F

First component of approach velocity of center of rotation.

11-20

2nd

F

Second component of approach velocity of center of rotation.

21-30

3rd

F

Third component of approach velocity of center of rotation.

31-40

4th

F

Approach angular velocity about local axis through center of rotation.

7th data block The 7th data block is only required for a mechanical-displacement analysis.

Main Index

1-10

1st

F

First component of velocity or target position of center of rotation.

11-20

2nd

F

Second component of velocity or target position of center of rotation.

21-30

3rd

F

Third component of velocity or target position of center of rotation.

ADD RIGID (3-D) 1559 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

31-40

4th

F

Angular velocity or angular position about local axis through center of rotation.

41-50

5th

F

Not used; enter 0.

51-60

6th

F

Not used; enter 0.

61-70

7th

F

Not used; enter 0.

71-80

8th

F

Friction coefficient.

8th data block The 8th data block is only necessary if heat transfer is included. 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact heat transfer coefficient ( H CT ).

31-40

4th

F

Body temperature ( T BODY ). (Required for rigid body only.)

9th data block The 9th data block is only necessary if heat transfer is included. 1-10

1st

F

Enter the separation distance dependent heat transfer file coefficient ( H BL ).

10th data block The 10th data block is only necessary for Joule heating. 1-10

1st

F

Not used; enter 0.

11-20

2nd

F

Not used; enter 0.

21-30

3rd

F

Contact electrical transfer coefficient.

31-40

4th

F

Body voltage (required for rigid body only).

11th data block The 11th data block is only necessary for harmonic acoustic analysis. 1-10

1st

F

1---k1

reactive boundary coefficient.

11-20

2nd

F

1 ----c1

reactive boundary coefficient.

The 12th through 19th data blocks are repeated for as many geometrical data as required (NETTY).

Main Index

1560 ADD RIGID (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

A. For 3-D Rigid Body (Ruled Surface) 12a data block 1-5

1st

I

Enter 4 for ruled surface (ITYPE).

6-10

2nd

I

Entity type of the first surface generator (child) of the surface, JTYPE1.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe first surface generator (NPOINT1). If JTYPE1 = 2 method to describe the circular arc (METH).

16-20

4th

I

Entity type of the second surface generator (child) of the surface (JPOINT2).

21-25

5th

I

If JTYPE1 = 1, 3, 4, 5 enter number of point required to describe second surface generator (NPOINT2). If JTYPE2 = 2 method to describe the circular arc (METH).

26-30

6th

I

Number of subdivisions along first direction (NDIV1), (direction along first and second surface generator).

31-35

7th

I

Number of subdivisions along second direction (NDIV2), (direction from first surface generator to second surface generator).

The 13a data block is repeated (NPOINT1 ∗ NPOINT2) times for ruled surface. 13a data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

B. For 3-D Rigid Body (Surface of Revolution) 12b data block 1-5

1st

I

Enter 5 for surface of revolution (ITYPE).

6-10

2nd

I

Entity type of the surface generator.

11-15

3rd

I

If JTYPE1 = 1, 3, 4, 5 enter number of points required to describe the generator (NPOINT). If JTYPE = 2 method to describe the circular arc (METH).

16-20

4th

I

Number of subdivisions along the first (surface generator) direction (NDIV1).

21-25

5th

I

Number of subdivisions along the second (circumference) direction (NDIV2).

The 13b data block is repeated NPOINT times for surface of revolution.

Main Index

ADD RIGID (3-D) 1561 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

13b data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

14b data block 1-10

1st

F

First coordinate of 1st point on the axis of revolution.

11-20

2nd

F

Second coordinate of 1st point on the axis of revolution.

21-30

3rd

F

Third coordinate of 1st point on the axis of revolution.

31-40

4th

F

First coordinate of 2nd point on the axis of revolution.

41-50

5th

F

Second coordinate of 2nd point on the axis of revolution.

51-60

6th

F

Third coordinate of 2nd point on the axis of revolution.

61-70

7th

F

Total angle (degree) of rotation (Initial position of the surface generator is given on the 9th data block.)

C. For 3-D Rigid Surface (Bezier Surface) 12c data block 1-5

1st

I

Enter 6 for Bezier surface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPONT1).

11-15

3rd

16-20

4th

I

Number of subdivisions along first direction (NDIV1).

21-25

5th

I

Number of subdivisions along second direction (NDIV2).

Number of points along the second direction of surface (NPOINT2).

The 13c data block is repeated (NPOINT1 ∗ NPOINT2) times for Bezier surface. 13c data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

D. For 3-D Rigid Surface (4-Node Patch) 12d data block

Main Index

1-5

1st

I

Enter 7 for a surface consisting of 4-node patches (ITYPE).

6-10

2nd

I

Number of 4-node patches to be read (which makes the entire surface) NSEG.

11-15

3rd

I

Number of points to be read (NPOINT).

1562 ADD RIGID (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed 16-20

Free 4th

Data Entry Entry I

Unit number. Defaults to input. Set KUNIT = -1 if data entered via the DIGEOM user subroutine.

21-25

5th

I

Set to 1 if patch data is to be printed. Default: no printing.

The 13d data block is repeated NSEG times for patches not entered by means of user subroutines (ITYPE = 7 and KUNIT not -1) 13d data block 1-5

1st

I

Patch number (not necessary, can be left blank).

6-10

2nd

I

Not used.

11-15

3rd

I

First point number of this patch.

16-20

4th

I

Second point number of this patch.

21-25

5th

I

Third point number of this patch.

26-30

6th

I

Fourth point number of this patch.

The 14d data block is repeated NPOINT times for patches not entered by means number of user subroutine (ITYPE = 7 and KUNIT not -1). 14d data block 1-5

1st

I

Point number.

6-15

2nd

F

First coordinate of this node.

16-25

3rd

F

Second coordinate of this node.

26-35

4th

F

Third coordinate of this node.

E. For 3-D Rigid Surface (Poly-Surface) 12e data block 1-5

1st

I

Enter 8 for polysurface (ITYPE).

6-10

2nd

I

Number of points along the first direction of surface (NPOINT1).

11-15

3rd

I

Number of points along the second direction of surface (NPOINT2).

The 13e data block is repeated (NPOINT1 ∗ NPOINT2) times for poly-surfaces. 13e data block

Main Index

1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

ADD RIGID (3-D) 1563 Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

F. For 3-D Rigid Surface (NURBS) 12f data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points along u-direction (NPTU).

11-15

3rd

I

Number of control points along v-direction (NPTV).

16-20

4th

I

Order along u-direction (NORU).

21-25

5th

I

Order along v-direction (NORV).

26-30

6th

I

Number of subdivisions along u-direction; default 50.

31-35

7th

I

Number of subdivisions along v-direction; default 50.

36-40

8th

I

Number of trimming curves.

The 13f data block is repeated (NPTU ∗ NPTV) for control points. 13f data block 1-10

1st

F

First coordinate of point.

11-20

2nd

F

Second coordinate of point.

21-30

3rd

F

Third coordinate of point.

The 14f data block is repeated (NPTU ∗ NPTV) for homogeneous coordinate. 14f data block 1-10

1st

F

Homogeneous coordinate (0 ≤ h ≤ 1).

The 15f data block is repeated (NPTU + NORU) + (NPTV + NORV) for knot vectors. 15f data block 1-10

1st

F

Knot vector(0 ≤ k ≤ 1).

For each trimming curve, data blocks 16f, 17f, 18f, and 19f. 16f data block 1-5

1st

I

Enter 9 for NURBS.

6-10

2nd

I

Number of control points (NPTU).

11-15

3rd

I

Order (NORU).

16-20

4th

I

Number of subdivisions; default 50.

The 17f data block is repeated NPTU times for control points. 17f data block 1-10

1st

F

First coordinate of point in isoparametric space.

11-20

2nd

F

Second coordinate of point in isoparametric space.

The 18f data block is repeated NPTU times for homogeneous coordinate.

Main Index

1564 ADD RIGID (3-D) Define a New Three-dimensional Rigid Contact Surface

Format Fixed

Free

Data Entry Entry

18f data block 1-10

1st

F

Homogeneous coordinate between 0 and 1.

The 19f data block is repeated NPTU+ NORU times for knot vectors. 19f data block 1-10

1st

F

Component of knot vector between 0 and 1.

G. For 3-D Rigid Surface (Cylinder) 12g data block 1-5

1st

I

Enter 10 for Cylinder.

6-10

2nd

I

Number of subdivisions.

13g data block 1-10

1st

F

First coordinate of center point on top surface.

11-20

2nd

F

Second coordinate of center point on top surface.

21-30

3rd

F

Third coordinate of center point on top surface.

31-40

4th

F

Radius of top surface

41-50

5th

F

First coordinate of center point on bottom surface.

51-60

6th

F

Second coordinate of center point on bottom surface.

61-70

7th

F

Third coordinate of center point on bottom surface radius of bottom surface.

71-80

8th

F

Radius of bottom surface. NOTE: If the radius is negative value in 4th field the normal of cylinder is outward. Default is inward.

H. For 3-D Rigid Surface (Sphere) 12h data block 1-5

1st

I

Enter 11 for Sphere.

6-10

2nd

I

Number of subdivisions.

13h data block 1-10

1st

F

First coordinate of center point.

11-20

2nd

F

Second coordinate of center point.

21-30

3rd

F

Third coordinate of center point.

31-40

4th

F

Radius of sphere. Note:

Main Index

If the radius is negative value in 4th field, the normal of sphere is outward. Default is inward.

CONTACT TABLE with TABLES (History Definition) 1565 Define Contact Table

CONTACT TABLE with TABLES (History Definition)

Define Contact Table

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option overrides information provided on the CONTACT option to allow the user to give more detailed information concerning the interaction of the bodies. In particular, this option allows you to specify which bodies contact which other bodies, and what is their behavior after contact occurs. If this option is not included, the default for contact analysis is that every body detects the possibility of contact with all other bodies, and itself if it is a flexible body. When the CONTACT TABLE option is entered, the default of detection for every body is overridden. Instead, you specify the relationship of detection between bodies for contact. The touching body does not contact itself unless you request it. This is useful for deactivating or activating bodies to either reduce computational costs, or because the physical process (such as manufacturing) involves multiple stages with different body interactions. Whenever the touched body is a flexible one, by default, the capability of double-sided contact is applied between the contacting bodies. This can be switched off by selecting single-sided contact on the CONTACT option or by setting the searching order in the CONTACT TABLE option. A positive value of the interference closure implies that there is an overlap between the bodies; a negative value implies that a gap exists. In addition, you can invoke the glue option, delayed slide off a deformable body, and stress-free initial contact. In the glue option, when a node contacts a rigid body, the relative tangential displacement is zero. When a node contacts a deformable body, all the translational degrees of freedom are tied. By default, if a node slides off the boundary of a deformable body at a sharp corner by a distance more than the contact tolerance, contact between the node and the contacted body is lost. By invoking the delayed sliding off option, the tangential contact tolerance is increased by a user-defined value. In any static contact analysis, a node contacting a body is projected onto the contacted segment of this body. Due to inaccuracies in the finite element model, this might introduce undesired stress changes, since an overlap or a gap between the node and the contacted segment will be closed. The option for stress-free initial contact forces a change of the coordinates of a node contacting a deformable body, thus avoiding the stress changes. In combination with the glue option, a similar effect can be obtained; however, the overlap or gap remains. The following control variables of contact between bodies can be modified throughout the table: contact tolerance, separation threshold, friction coefficient, interference closure and contact heat transfer and electrical coefficients. For an acoustic-solid analysis, you can also modify the reactive boundary coefficients.

Main Index

1566 CONTACT TABLE with TABLES (History Definition) Define Contact Table

The near thermal contact option can only be invoked using the CONTACT TABLE option. In this case, one must specify the distance at which near thermal contact occurs and the additional parameters to control the thermal (and electrical) flux. The previous value of those control variables is not overridden unless nonzero values are entered here. Notes:

This option should be placed after the CONTACT option. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT TABLE after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONTACT TABLE.

2nd data block 1-5

1st

I

Enter the number of sets of bodies to be input.

6-10

2nd

I

Enter the version number for reading the CONTACT TABLE block. Enter 2 if the 5th, 8th, 9th, 16th, 17th, 18th, and 19th data blocks are to be read to control contact, ungluing, and multiphysics. Default is 0.

The 3rd through the 22nd data blocks are entered once for each set of bodies to be input. 3rd data block 1-5

1st

I

Enter the touching body number.

6-15

2nd

F

Enter the contact tolerance ( E R R OR ).

16-25

3rd

F

Enter the distance below which near thermal or electrical contact behavior occurs ( DQ NE A R ). A 0 entered here indicates that near contact behavior is not included.

26-35

4th

F

Not used; enter 0.

36-45

5th

F

Not used; enter 0.

46-55

6th

F

Not used; enter 0.

56-65

7th

F

Enter 0 (default) if there is no additional constraint on the tangential displacement when contact occurs. No constraints are placed on rotational degrees of freedom. Enter 1 to insure that there is no relative tangential displacement when the node comes into contact. A possible relative normal displacement might originate from an initial gap or overlap between the node and the contacted body, as the node will be projected onto the contacted body.

Main Index

CONTACT TABLE with TABLES (History Definition) 1567 Define Contact Table

Format Fixed

Free

Data Entry Entry Enter 2 to insure that there is no relative tangential and normal displacement when the node comes into contact. An existing initial gap or overlap between the node and the contacted body is not removed, as the node is not projected onto the contacted body. Enter 3 to insure full moment carrying glue when shells contact. The node will be projected onto the contacted body. Enter 4 to insure full moment carrying glue when shells contact. The node will not be projected onto the contact body.

66-70

8th

I

Enter 0 (default) if search order is based upon first checking bodies with lower body number versus bodies with higher body number. Enter 1 to indicate that the searching order for deformable contact bodies is from the touching body to the touched bodies on the 5th data block. This might change the default order for deformable bodies, which is from bodies with a lower number to bodies with a higher number. Enter 2 to let the program decide which searching order is optimal for deformable bodies. This order is set up such that searching is done starting with the body having the smallest element edge. This option forces singlesided contact between the touching and touched bodies: searching is done only from one body to another and not the other way around.

71-75

9th

I

Enter 0 (default) if during initial contact, a projection onto the contact surface induces a stress. Enter 1 to modify the coordinates of a node in contact with a deformable body so that stress-free initial contact can be obtained. Enter 2 to extend the tangential error tolerance at sharp corners of deformable bodies to delay sliding off a contacted segment. Enter 3 to have both 1 and 2 active.

76-80

10th

I

Only relevant if the glue option is invoked and the separation force has not been set. Enter 0 (default) if a node should not separate. Enter 1 to invoke the separation behavior procedure, as specified on the 12th field of the 2nd data block of the CONTACT option. Enter 2 to invoke the breaking glue capability. A node will be released if the break criterion is fulfilled. Then the node will do regular contact with separation instead of being glued. The stress limits for this capability are specified in the 8th data block below.

Main Index

1568 CONTACT TABLE with TABLES (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

4th data block 1-5

1st

I

Not used; enter 0.

6-10

2nd

I

Enter the table ID for the contact tolerance.

11-15

3rd

I

Enter the table ID for the near contact distance.

5th data block Only required if version number is equal to 2. 1-5

1st

I

Enter the boundary description flag for the touching body (entered on the 3rd data block).

6-10

2nd

I

Enter the boundary description flag for the touched body (entered on the 18th data block).

The boundary description flag is given by A+10*B+1000*C, where parameter A is related to continuum elements in a body, parameter B is related to shell elements in a body and parameter C is related to beam elements and/or shell edges in a body. The possible values of these parameters and their meaning are: A = 1:

the outside edges (2-D) or faces (3-D) of continuum elements are included in the boundary description (default).

B = 1:

both top and bottom faces, including thickness offset, are included in the boundary description.

B = 2:

only bottom faces, including thickness offset, are included in the boundary description.

B = 3:

only bottom faces, ignoring thickness offset, are included in the boundary description.

B = 4:

only top faces, including thickness offset, are included in the boundary description.

B = 5:

only top faces, ignoring thickness offset, are included in the boundary description.

B = 6:

both top and bottom faces, ignoring thickness offset, are included in the boundary description. The default value of B depends on the parameter governing the normal direction/thickness contribution of shell elements as entered on the CONTACT option. Note:

Main Index

The choice B = 6 for both bodies in a contact combination is only meaningful for glued contact. If in such cases separation is allowed, separated nodes will not come into contact anymore, unless a new CONTACT TABLE is defined to reset the value of B.

C = 0:

neither beam elements nor shell edges are included in the boundary description.

C = 1:

beam elements are included in the boundary description (allowing for beam-tobeam contact).

CONTACT TABLE with TABLES (History Definition) 1569 Define Contact Table

Format Fixed

Free

Data Entry Entry

C = 10:

shell edges are included in the boundary description.

C = 11:

both beam elements and shell edges are included in the boundary description. If beam-to-beam contact is not activated on the CONTACT option, the default value of C is 0, otherwise the default value is 1.

6th data block Only required if a mechanical-displacement solution is obtained. 1-10

1st

F

Enter the contact separation threshold. The physical meaning of this threshold (a force, a stress, or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block of the CONTACT option.

11-20

2nd

F

Enter the friction coefficient.

21-30

3rd

F

Enter the interference closure amount, normal to the contact surface.

31-40

4th

F

Enter the friction stress limit

σ limit .

This entry is only used for friction type 6 (Coulomb friction using the bilinear model). If the shear stress due to friction reaches this limit value, then the applied friction force will be reduced so that the maximum friction stress is given by min ( μ σ n ,σ limit ) , with μ the friction coefficient and σ n the contact normal stress. Default for this entry is 1.e20.

Main Index

41-50

5th

F

Enter the contact tolerance BIAS factor (0-1). This value will overrule the BIAS factor entered on the 6th field of the 3rd data block of the CONTACT option if nonzero.

51-60

6th

F

Enter the delayed slide off distance (this entry is only used if delayed slide off has been activated by the 9th entry of the 3rd data block). When using the delayed slide off option, a node sliding on a segment will slide off this segment only if it passes the node (2-D) or edge (3-D) at a sharp corner over a distance larger than the delayed slide off distance. By default, the delayed slide off distance is related to the dimensions of the contacted segment by a 20 percent increase of its isoparametric domain.

61-70

7th

F

Enter the hard-soft ratio (this entry is only used if double-sided contact with automatic constraint optimization is used, as defined on the 4th data block of the CONTACT option). The hard-soft ratio can be used by the program if there is a significant difference in the (average) stiffness of the contact bodies (expressed by the trace of the initial stress-strain law). If the ratio of the stiffnesses is larger than the hard-soft ratio, the nodes of the softest body are the preferred slave nodes. By default, the hard-soft ratio is 2.

1570 CONTACT TABLE with TABLES (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

7th data block Only required if a mechanical-displacement solution is obtained. 1-5

1st

I

Enter the table ID for the contact separation threshold.

6-10

2nd

I

Enter the table ID for the friction coefficient.

11-15

3rd

I

Enter the table ID for the interface closure amount.

16-20

4th

I

Enter the table ID for the friction stress limit.

8th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-10

1st

F

Normal stress to break glued contact (SN).

11-20

2nd

F

Tangential stress to break glued contact (ST).

21-30

3rd

F

Enter exponent for breaking normal stress term (m). Default = 2.

31-40

4th

F

Enter exponent for breaking tangential stress term (n). Default = 2. The glue breaks when

m

n

( σ N ⁄ SN ) + ( σ T ⁄ ST ) > 1

9th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-5

1st

I

Enter the table ID associated with normal stress to break glued contact.

6-10

2nd

I

Enter the table ID associated with tangential stress to break glued contact.

11-15

3rd

I

Enter the table ID associated with exponent of normal stress term.

16-20

4th

I

Enter the table ID associated with exponent of tangential stress term.

10th data block Only required if heat transfer is included.

Main Index

1-10

1st

F

Enter the contact heat transfer coefficient. (HCT)

11-20

2nd

F

Enter the convection heat transfer coefficient for near behavior. (HCV)

21-30

3rd

F

Enter the natural convection heat transfer coefficient for near behavior. (HNC)

31-40

4th

F

Enter the exponent associated with the natural convection for near behavior. (BNC)

41-50

5th

F

Enter the surface emissivity. (ε)

51-60

6th

F

Enter the separation distance dependent thermal convection coefficient. (HBL)

CONTACT TABLE with TABLES (History Definition) 1571 Define Contact Table

Format Fixed

Free

Data Entry Entry

11th data block Only required if heat transfer is included. 1-5

1st

I

Enter the table ID for the contact heat transfer coefficient.

6-10

2nd

I

Enter the table ID for the heat transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID for the natural convection heat transfer coefficient for near behavior.

16-20

4th

I

Enter the table ID for the exponent associated with the natural convection for near behavior.

21-25

5th

I

Enter the table ID for the surface emissivity.

26-30

6th

I

Enter the table ID for the separation dependent thermal convection coefficient.

12th data block Only required for Joule heating. 1-10

1st

F

Enter the contact electrical coefficient (coupled Joule analysis only).

11-20

2nd

F

Enter the electrical transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent electrical transfer coefficient.

13th data block Only required for Joule heating. 1-5

1st

I

Enter the table ID associated with the contact electrical coefficient.

6-10

2nd

I

Enter the table ID associated with the electrical transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID associated with the separation distance dependent electrical transfer coefficient.

14th data block Only required for coupled mass diffusion analysis.

Main Index

1-10

1st

F

Enter the contact mass transfer coefficient).

11-20

2nd

F

Enter the mass transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent mass diffusion coefficient.

1572 CONTACT TABLE with TABLES (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

15th data block Only required for coupled mass diffusion analysis. 1-5

1st

I

Enter the table ID associated with the contact mass transfer coefficient.

6-10

2nd

I

Enter the table ID associated with the mass transfer coefficient for near behavior.

11-15

3rd

I

Enter the table ID associated with the separation distance dependent mass diffusion coefficient.

16th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-10

1st

F

Not used; enter 0.

17th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-5

1st

I

Not used; enter 0.

18th data block Only required if magnetostatic analysis is included. 1-10

1st

F

Not used; enter 0.

19th data block Only required if magnetostatic analysis is included. 1-5

1st

I

Not used; enter 0.

20th data block Only required for harmonic acoustic analysis.

Main Index

1-10

1st

F

Enter the

1 ----k1

reactive boundary coefficient.

11-20

2nd

F

Enter the

1 ----c1

reactive boundary coefficient.

CONTACT TABLE with TABLES (History Definition) 1573 Define Contact Table

Format Fixed

Free

Data Entry Entry

21st data block Only required for harmonic acoustic analysis. 1-5

1st

I

Enter the table ID for the

1---k1

reactive boundary coefficient.

6-10

2nd

I

Enter the table ID for the

1 ----c1

reactive boundary coefficient.

22nd data block Enter a list of touched bodies for which the touching body detects contact with the parameters above.

Main Index

1574 CONTACT TABLE (History Definition) Define Contact Table

CONTACT TABLE (History Definition)

Define Contact Table

The information provided here is based upon not using the table driven input style. Description This option overrides information provided on the CONTACT option to allow the user to give more detailed information concerning the interaction of the bodies. In particular, this option allows you to specify which bodies contact which other bodies, and what is their behavior after contact occurs. If this option is not included, the default for contact analysis is that every body detects the possibility of contact with all other bodies, and itself if it is a flexible body. When the CONTACT TABLE option is entered, the default of detection for every body is overridden. Instead, you specify the relationship of detection between bodies for contact. The touching body does not contact itself unless you request it. This is useful for deactivating or activating bodies to either reduce computational costs, or because the physical process (such as manufacturing) involves multiple stages with different body interactions. Whenever the touched body is a flexible one, by default, the capability of double-sided contact is applied between the contacting bodies. This can be switched off by selecting single-sided contact on the CONTACT option or by setting the searching order in the CONTACT TABLE option. A positive value of the interference closure implies that there is an overlap between the bodies; a negative value implies that a gap exists. In addition, you can invoke the glue option, delayed slide off a deformable body, and stress-free initial contact. In the glue option, when a node contacts a rigid body, the relative tangential displacement is zero. When a node contacts a deformable body, all the translational degrees of freedom are tied. By default, if a node slides off the boundary of a deformable body at a sharp corner by a distance more than the contact tolerance, contact between the node and the contacted body is lost. By invoking the delayed sliding off option, the tangential contact tolerance is increased by a user-defined value. In any static contact analysis, a node contacting a body is projected onto the contacted segment of this body. Due to inaccuracies in the finite element model, this might introduce undesired stress changes, since an overlap or a gap between the node and the contacted segment will be closed. The option for stress-free initial contact forces a change of the coordinates of a node contacting a deformable body, thus avoiding the stress changes. In combination with the glue option, a similar effect can be obtained; however, the overlap or gap remains. The following control variables of contact between bodies can be modified throughout the table: contact tolerance, separation threshold, friction coefficient, interference closure and contact heat transfer and electrical coefficients. For an acoustic-solid analysis, you can also modify the reactive boundary coefficients.

Main Index

CONTACT TABLE (History Definition) 1575 Define Contact Table

The near thermal contact option can only be invoked using the CONTACT TABLE option. In this case, one must specify the distance at which near thermal contact occurs and the additional parameters to control the thermal (and electrical) flux. The previous value of those control variables is not overridden unless nonzero values are entered here. Notes:

This option should be placed after the CONTACT option. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT TABLE after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word CONTACT TABLE.

2nd data block 1-5

1st

I

Enter the number of sets of bodies to be input.

6-10

2nd

I

Enter the version number for reading the CONTACT TABLE block. Enter 2 if the 4th, 6th, 10th, and 11th data blocks are to be read to control contact, ungluing, and multiphysics. Default is 0.

The 3rd through the 13th data blocks are entered once for each set of bodies to be input. 3rd data block 1-5

1st

I

Enter the touching body number.

6-15

2nd

F

Enter the contact tolerance ( E R R OR ).

16-25

3rd

F

Enter the distance below which near thermal or electrical contact behavior occurs ( DQ NE A R ). A zero entered here indicates that near contact behavior is not included.

26-35

4th

F

Not used; enter 0.

36-45

5th

F

Not used; enter 0.

46-55

6th

F

Not used; enter 0.

56-65

7th

F

Enter 0 (default) if there is no additional constraint on the tangential displacement when contact occurs. No constraints are placed on rotational degrees of freedom. Enter 1 to insure that there is no relative tangential displacement when the node comes into contact. A possible relative normal displacement might originate from an initial gap or overlap between the node and the contacted body, as the node will be projected onto the contacted body.

Main Index

1576 CONTACT TABLE (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry Enter 2 to insure that there is no relative tangential and normal displacement when the node comes into contact. An existing initial gap or overlap between the node and the contacted body is not removed, as the node is not projected onto the contacted body. Enter 3 to insure full moment carrying glue when shells contact. The node will be projected onto the contacted body. Enter 4 to insure full moment carrying glue when shells contact. The node will not be projected onto the contact body.

66-70

8th

I

Enter 0 (default) if search order is based upon first checking bodies with lower body number versus bodies with higher body number. Enter 1 to indicate that the searching order for deformable contact bodies is from the touching body to the touched bodies on the 8th data block. This might change the default order for deformable bodies, which is from bodies with a lower number to bodies with a higher number. Enter 2 to let the program decide which searching order is optimal for deformable bodies. This order is set up such that searching is done starting with the body having the smallest element edge. This option forces singlesided contact between the touching and touched bodies: searching is done only from one body to another and not the other way around.

71-75

9th

I

Enter 0 (default) if, during initial contact, a projection onto the contact surface induces a stress. Enter 1 to modify the coordinates of a node in contact with a deformable body so that stress-free initial contact can be obtained. Enter 2 to extend the tangential error tolerance at sharp corners of deformable bodies to delay sliding off a contacted segment. Enter 3 to have both 1 and 2 active.

76-80

10th

I

Only relevant if the glue option is invoked and the separation force has not been set. Enter 0 if a node should not separate (default). Enter 1 to invoke the separation behavior procedure, as specified on the 12th field of the 2nd data block of the CONTACT option. Enter 2 to invoke the breaking glue capability. A node will be released if the break criterion is fulfilled. Then the node will do regular contact with separation instead of being glued. The stress limits for this capability are specified in the 20th data block below.

Main Index

CONTACT TABLE (History Definition) 1577 Define Contact Table

Format Fixed

Free

Data Entry Entry

4th data block Only required if version number is equal to 2. 1-5

1st

I

Enter the boundary description flag for the touching body (entered on the 3rd data block).

6-10

2nd

I

Enter the boundary description flag for the touched body (entered on the 11th data block).

The boundary description flag is given by A+10*B+1000*C, where parameter A is related to continuum elements in a body, parameter B is related to shell elements in a body and parameter C is related to beam elements and/or shell edges in a body. The possible values of these parameters and their meaning are: A=1:

the outside edges (2-D) or faces (3-D) of continuum elements are included in the boundary description (default).

B=1:

both top and bottom faces, including thickness offset, are included in the boundary description.

B=2:

only bottom faces, including thickness offset, are included in the boundary description.

B=3:

only bottom faces, ignoring thickness offset, are included in the boundary description.

B=4:

only top faces, including thickness offset, are included in the boundary description.

B=5:

only top faces, ignoring thickness offset, are included in the boundary description.

B=6:

both top and bottom faces, ignoring thickness offset, are included in the boundary description. The default value of B depends on the parameter governing the normal direction/thickness contribution of shell elements as entered on the CONTACT option. Note:

The choice B=6 for both bodies in a contact combination is only meaningful for glued contact. If in such cases separation is allowed, separated nodes will not come into contact anymore, unless a new CONTACT TABLE is defined to reset the value of B.

C=0:

neither beam elements nor shell edges are included in the boundary description.

C=1:

beam elements are included in the boundary description (allowing for beam-tobeam contact).

C=10:

shell edges are included in the boundary description.

C=11:

both beam elements and shell edges are included in the boundary description. If beam-to-beam contact is not activated on the CONTACT option, the default value of C is 0, otherwise the default value is 1.

Main Index

1578 CONTACT TABLE (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

5th data block Only required if a mechanical-displacement solution is obtained. 1-10

1st

F

Enter the contact separation threshold. The physical meaning of this threshold (a force, a stress, or a fraction of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block of the CONTACT option.

11-20

2nd

F

Enter the friction coefficient.

21-30

3rd

F

Enter the interference closure amount; normal to the contact surface.

31-40

4th

F

Enter the friction stress limit

σ limit .

This entry is only used for friction type 6 (Coulomb friction using the bilinear model). If the shear stress due to friction reaches this limit value, then the applied friction force will be reduced so that the maximum friction stress is given by min ( μ σn ,σ limit ) , with μ the friction coefficient and σ n the contact normal stress. Default for this entry is 1.e20.

Main Index

41-50

5th

F

Enter the contact tolerance BIAS factor (0-1). This value will overrule the BIAS factor entered on the 6th field of the 3rd data block of the CONTACT option if nonzero.

51-60

6th

F

Enter the delayed slide off distance (this entry is only used if delayed slide off has been activated by the 9th entry of the 3rd data block). When using the delayed slide off option, a node sliding on a segment will slide off this segment only if it passes the node (2-D) or edge (3-D) at a sharp corner over a distance larger than the delayed slide off distance. By default, the delayed slide off distance is related to the dimensions of the contacted segment by a 20 percent increase of its isoparametric domain.

61-70

7th

F

Enter the hard-soft ratio (this entry is only used if double-sided contact with automatic constraint optimization is used, as defined on the 4th data block of the CONTACT option). The hard-soft ratio can be used by the program if there is a significant difference in the (average) stiffness of the contact bodies (expressed by the trace of the initial stress-strain law). If the ratio of the stiffnesses is larger than the hard-soft ratio, the nodes of the softest body are the preferred slave nodes. By default, the hard-soft ratio is 2.

CONTACT TABLE (History Definition) 1579 Define Contact Table

Format Fixed

Free

Data Entry Entry

6th data block Only required if version number is equal to 2 and a mechanical displacement solution is obtained. 1-10

1st

F

Normal stress to break glued contact (SN).

11-20

2nd

F

Tangential stress to break glued contact (ST).

21-30

3rd

F

Enter exponent for breaking normal stress term (m). Default = 2.

31-40

4th

F

Enter exponent for breaking tangential stress term (n). Default = 2. The glue breaks when

m

n

( σ N ⁄ SN ) + ( σ T ⁄ ST ) > 1

7th data block Only required if heat transfer is included. 1-10

1st

F

Enter the contact heat transfer coefficient ( H T ).

11-20

2nd

F

Enter the convection heat transfer coefficient for near behavior ( H CV ).

21-30

3rd

F

Enter the natural convection heat transfer coefficient for near behavior ( H NC ).

31-40

4th

F

Enter the exponent associated with the natural convection for near behavior ( B NC ).

41-50

5th

F

Enter the surface emissivity ( ε ).

51-60

6th

F

Enter the separation distance dependent thermal convection coefficient ( H BL ).

8th data block Only required for Joule heating. 1-10

1st

F

Enter the contact electrical coefficient (coupled Joule analysis only).

11-20

2nd

F

Enter the electrical transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent electrical coefficient.

9th data block Only required for coupled mass diffusion analysis. 1-10

1st

F

Enter the contact mass transfer coefficient.

11-20

2nd

F

Enter the mass transfer coefficient for near behavior.

21-30

3rd

F

Enter the separation distance dependent mass diffusion coefficient.

10th data block Only required if version number is equal to 2 and electrostatic or piezoelectric analysis is included. 1-10

Main Index

1st

F

Not used; enter 0.

1580 CONTACT TABLE (History Definition) Define Contact Table

Format Fixed

Free

Data Entry Entry

11th data block Only required if magnetostatic analysis is included. 1-10

1st

F

Not used; enter 0.

12th data block Only required for harmonic acoustic analysis. 1-10

1st

F

Enter the

1---k1

reactive boundary coefficient.

11-20

2nd

F

Enter the

1---c1

reactive boundary coefficient.

13th data block Enter a list of touched bodies for which the touching body detects contact with the parameters above.

Main Index

CONTACT NODE (History Definition) 1581 Define Nodes for Surface Contact

CONTACT NODE (History Definition)

Define Nodes for Surface Contact

Description This option is used to define which nodes in a body might potentially contact other surfaces. This option can be used to reduce the computational cost if a body has many exterior nodes and it is known for which nodes contact might occur. If this option is not used, all exterior surface nodes are checked for contact. Notes:

If this option is used and a node number is not explicitly listed, that node might penetrate other bodies. In a restart analysis, if these values are to be changed, use the REAUTO option and specify the CONTACT NODE option after the END OPTION.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words CONTACT NODE.

I

Enter the number of bodies for which exterior nodes are defined

I

Body number.

I

Enter a list of nodes that are potential contact nodes.

2nd data block 1-5

1st

3rd data block 1-5

1st

4th data block 1-80

Main Index

1st

1582 MOTION CHANGE Define Motion of Rigid Surfaces

MOTION CHANGE

Define Motion of Rigid Surfaces

The information provided here is based upon not using the table driven input style. When using the table driven input for contact, the motion of the rigid surfaces can be defined on the CONTACT with TABLES model definition option by referencing tables that are functions of time. Description This option is useful for prescribing the motion of rigid bodies when the CONTACT option is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words MOTION CHANGE.

I

Enter the number of sets of rigid bodies to be input.

2nd data block 1-5

1st

Data blocks 3 and 4 are entered as pairs, once for each data set. 2-D Contact Problems 3rd data block 1-5

1st

I

Enter the rigid body number.

6-10

2nd

I

Enter -1 for position controlled body. Enter 0 for velocity controlled body. Enter 1 for load controlled body.

4th data block (if velocity controlled rigid surface) 1-10

1st

F

First component of velocity of center of rotation (COR).

11-20

2nd

F

Second component of velocity of COR.

21-30

3rd

F

Angular velocity (in radian/unit time) about COR.

31-40

4th

F

Friction coefficient.

4th data block (if position controlled rigid surface)

Main Index

1-10

1st

F

First component of position of COR.

11-20

2nd

F

Second component of position of COR.

21-30

3rd

F

Angular position (in radian) about COR.

31-40

4th

F

Friction coefficient.

MOTION CHANGE 1583 Define Motion of Rigid Surfaces

Format Fixed

Free

Data Entry Entry

3-D Contact Problems 3rd data block 1-5

1st

I

Enter the rigid body number.

6-10

2nd

I

Enter -1 for position controlled body. Enter 0 for velocity controlled body. Enter 1 for load controlled body.

4th data block (if velocity controlled rigid surface) 1-10

1st

F

First component of velocity of COR.

11-20

2nd

F

Second component of velocity of COR.

21-30

3rd

F

Third component of velocity of COR.

31-40

4th

F

Angular velocity (in radian/unit time) about local axis through COR.

41-50

5th

F

Friction coefficient.

4th data block (if position controlled rigid surface)

Main Index

1-10

1st

F

First component of position of COR.

11-20

2nd

F

Second component of position of COR.

21-30

3rd

F

Third component of position of COR.

31-40

4th

F

Angular position (in radian) about local axis through COR.

41-50

5th

F

Friction coefficient.

1584 SS-ROLLING Define the Parameters for Steady State Transport

SS-ROLLING

Define the Parameters for Steady State Transport

Description This option is used to define the spinning, cornering, and ground moving velocities for a body in steady state rolling analysis. Alternatively, this option can also define parameters for a procedure in steady state transport analysis to achieve certain load conditions such as friction force or torque by adjusting spinning velocity. This requires the corresponding degrees of freedom of the ground body being properly constrained (no moving). The torque (friction force) controlled steady state analysis requires iteration to determine the spinning velocity; in addition to Newton-Raphson equilibrium iterations, the convergence is slower compared to the spinning velocity controlled analysis. It is recommended the spinning velocity control option be used if a series of steady state solutions are to be obtained. The torque (friction force) control option is advantageous in case of only one steady state solution at a specific torque (friction force) is required. Start the job with spinning velocity control and switch to torque (friction force) control at a point near to the real solution improves the efficiency of the calculation. This option can be used with either AUTO LOAD or AUTO STEP. The velocities, friction force, or torque defined here are total values. Their values at a given time within the load case are obtained by time interpolating between the values defined here and those at the end of the last case. In the current release, there can be only one spinning body under steady state conditions and it contains all existing elements. The spinning velocity is applied to all elements in the model. The frictional force and torque are associated with the contact body defined here. Refer to Marc Volume A: Theory and User Input, Chapter 5 in the Steady State Rolling Analysis section for more details.

Ps Ts

ωs

Tc ωc

Pc

Figure 4-1

Main Index

Kinematics of a Rolling Body

SS-ROLLING 1585 Define the Parameters for Steady State Transport

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SS-ROLLING.

I

Body ID for spinning body.

2nd data block 1-5

1st

If no contact body is defined, all existing elements are included in the spinning body. 6-10

2nd

I

Body ID for ground.

11-15

3rd

I

jtrncon:flag to input format.

= 0 spinning velocity/ground velocity input = 1 friction force/ground velocity input = 2 torque/ground velocity input Default is 0. 16-25

4th

F

If jtrncon = 0 spinning velocity (cycle/time) = 1 friction force in 0° rolling direction = 2 torque with respect to spinning axis.

26-35

5th

F

Cornering velocity (cycle/time).

36-45

6th

F

x component of ground velocity (in sliding direction).

46-55

7th

F

y component of ground velocity (normal to surface).

56-65

8th

F

z component of ground velocity (in rolling direction).

66-70

9th

F

Used only if jtrncon = 0. If set to 1, friction coefficient increases gradually from 0 to the final value within the load case based on the time increment. In this case only solution at the end of the load case is physically meaningful. This may enhance stability of the analysis, especially for the transition periods from standstill to rolling and from brake to traction. Default is 0.

Main Index

1586 SS-ROLLING Define the Parameters for Steady State Transport

Format Fixed

Free

Data Entry Entry

3rd data block Only needed if the 3rd field in the 2nd data block (jtrncon) is not zero. 1-5

1st

I

Maximum number of adjustments in friction force (torque) - ground velocity input. Default is 20.

6-15

2nd

F

Tolerance ratio of friction force (torque) change in the adjustment over the maximum friction force (torque). Default is 0.02.

Main Index

RELEASE 1587 Define Release Data

RELEASE

Define Release Data

Description This option is useful for the analysis of spring-back after bodies contact one another. The body number is entered and then all of the nodes which contact that body are released at the beginning of the increment. The contact force can either be immediately removed or gradually reduced. In addition, the body must either be moving away to avoid nodes recontacting during the same increment or the CONTACT TABLE option should be used to deactivate contract. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word RELEASE.

11-15

2nd

I

Enter 0 if the contact forces are to be immediately removed (default). Enter 1 if the contact forces are to be reduced to zero over the number of increments specified in this load period.

2nd data block Enter a list of bodies. All nodes contacting these bodies are released.

Main Index

1588 APPROACH Move Rigid Surfaces into Position

APPROACH

Move Rigid Surfaces into Position

Description The APPROACH option allows you to move rigid bodies so that they just make contact with deformable bodies. In the case of multistage forging, you usually have a time period where the first set of bodies are released, followed by a new time period where the second set of bodies are brought into contact. This option is used in conjunction with the CONTACT TABLE option to determine which bodies are now applicable, and the CONTACT (2-D or 3-D), CONTACT with TABLES (2-D or 3-D), or MOTION CHANGE option which prescribes the velocity of the rigid bodies. Marc moves all rigid bodies with nonzero velocities until they come into contact with a deformable body. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

Main Index

1st

A

Enter the word APPROACH.

MOVE (History Definition) 1589 Perform Rigid Body Motion on Model

MOVE (History Definition)

Perform Rigid Body Motion on Model

Description The MOVE option allows you to apply a rigid body motion to either a rigid body, a deformable body, or a collection of elements. In general, use the RELEASE option to separate the moving elements from previously contacting surfaces. You need to use the CONTACT TABLE and/or MOTION CHANGE to control the rigid bodies, and the APPROACH option to position the new rigid bodies. Note:

The MOVE option may not be used with shell or beam elements. One must be very careful if the elements use the ORIENTATION option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word MOVE.

2nd data block 1-5

1st

I

Enter the contact body number. For deformable body, all elements associated with this body are moved. If a zero is entered, the 3rd data block is used.

6-10

2nd

I

Enter 1 to move symmetry bodies that contact the deformable body.

3rd data block (Used only if body number is zero) Enter list of elements to be moved. 4th data block 1-10

1st

E

Translation in first direction.

11-20

2nd

E

Translation in second direction.

21-30

3rd

E

Translation in third direction.

31-40

4th

E

Rotation about first direction.

41-50

5th

E

Rotation about second direction.

51-60

6th

E

Rotation about third direction.

For 2-D planar analysis, rotation about X and Y axis should be zero. For axisymmetric analysis, all rotations should be zero.

Main Index

1590 MOVE (History Definition) Perform Rigid Body Motion on Model

Format Fixed

Free

Data Entry Entry

5th data block

Main Index

1-10

1st

E

First coordinate of center of rotation.

11-20

2nd

E

Second coordinate of center of rotation.

21-30

3rd

E

Third coordinate of center of rotation.

ANNEAL 1591 Modify State of Material

ANNEAL

Modify State of Material

Description This option allows you to simulate an annealing operation at the end of deformation. You can choose to set the stresses and/or strains to zero. Also, an annealing temperature can be set. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word ANNEAL.

2nd data block 1-5

1st

I

Enter 1 to set stresses to zero.

6-10

2nd

I

Enter 1 to set strains to zero.

11-15

3rd

I

Enter 1 to set temperature to anneal temperature.

16-25

4th

E

Enter the anneal temperature.

26-30

5th

I

Enter 0 if a list of elements is entered in the 3rd data block. Enter 1 if a list of deformable contact bodies is entered in the 3rd data block.

3rd data block Enter a list of elements or deformable contact bodies for which this is applied.

Main Index

1592 SYNCHRONIZED Move Rigid Surfaces into Position

SYNCHRONIZED

Move Rigid Surfaces into Position

Description The SYNCHRONIZED option allows you to move rigid bodies so that they just make contact with deformable bodies. (In the case of multistage forging, you usually have a time period where the first set of dies are released, followed by a new time period where the second set of dies are brought into contact. This option is used in conjunction with the CONTACT TABLE option to determine which dies are now applicable, and the CONTACT (2-D or 3-D), CONTACT with TABLES (2-D or 3-D), or MOTION CHANGE option which prescribes the velocity of the rigid dies. Marc all rigid bodies with nonzero velocities until one of the moving rigid surfaces makes contact with a deformable body. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

Main Index

1st

A

Enter the word SYNCHRONIZE.

SPLINE (History Definition) 1593 Analytical Surface used to Represent a Deformable Body

SPLINE (History Definition) Analytical Surface used to Represent a Deformable Body Description In order to improve the accuracy for a deformable-deformable contact analysis, the outer surface of a contacted body can be described based on a spline (2-D) or Coons surface (3-D) description. The analytical surface is then used to calculate the normal to the deformable body and the closest point projection of a contacting node. In 2-D, for a contacted segment, a spline is created based on: tangent at first and second point of segment position of first and second point of segment In 3-D, for a contacted segment, a Coons surface is created based on: tangent vectors at corner points of segment position of corner points of segment zero twist vectors This option should be included in the history definition section if a rezoning step is performed. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word SPLINE.

I

Enter the number of deformable bodies for which the spline description must be applied.

2nd data block 1-5

1st

The 3rd and 4th data blocks are repeated for each deformable body with a spline description. 3rd data block

Main Index

1-5

1st

I

Body number.

6-10

2nd

I

For 3-D analyses only: enter 1 to enforce C0-continuity at edges where the normal vector to the outer contour of the structure shows a discontinuity (also see the 4th data block below).

11-15

3rd

I

Enter 1 to automatically determine nodes (2-D) or edges (3-D) where the normal vector to the outer contour of the structure shows a discontinuity.

1594 SPLINE (History Definition) Analytical Surface used to Represent a Deformable Body

Format Fixed 16-25

Free 4th

Data Entry Entry F

Used only if the 3rd entry of this data block is set to 1; enter the threshold angle to decide if there is a normal vector discontinuity between two adjacent segments of the contact body defined in the first entry of this data block. The threshold angle should be between 0 and 90 degrees; the default value is 60 degrees.

4th data block Enter a list of nodes defining nodes (2-D) or edges (3-D) where the normal vector to the outer contour of the structure shows a discontinuity. Notes: In 3-D, when there is a normal vector discontinuity at an element edge, the corner nodes defining the edge must be entered one after another. If the automatic detection is activated using the 3rd data block above, the nodes/edges with a normal vector discontinuity found by the program will be added to the list defined here. For an example see the SPLINE model definition option.

Main Index

EXCLUDE (History Definition) 1595 Ignore Contact with Certain Regions

EXCLUDE (History Definition)

Ignore Contact with Certain Regions

Description For certain contact problems, you might wish to influence the decision regarding the deformable segment a node contacts. By means of the EXCLUDE option, you can specify a list of nodes defining segments to be excluded from the contacted bodies. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word EXCLUDE.

I

Enter the number of deformable bodies for which the EXCLUDE option must be applied.

2 data block 1-5

1st

The 3rd and 4th data blocks are repeated for each deformable body with the EXCLUDE option. 3rd data block 1-5

1st

I

Body number.

4th data block Enter a list of nodes defining segments to be excluded from contacted bodies. Note:

Main Index

In 2-D, each segment must be defined by two nodes. In 3-D, each segment must be defined by four nodes. If, in 3-D, a segment corresponds to a tetrahedral or a collapsed hexahedral element, the last two nodes of the set of four should be identical.

1596 ACTUATOR Define the Length of the Actuator Link

ACTUATOR

Define the Length of the Actuator Link

Description This option can be used in conjunction with the truss element type 9 to simulate an actuator. This is often used in mechanism analyses to allow the prescription of the relative distance between two points. This option should be used with the LARGE DISP parameter whenever large rotations of the actuator or large displacements are anticipated. The original length of the actuator is given in the fourth field of the GEOMETRY option. The actuator is treated as an elastic link. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word ACTUATOR.

2nd data block 1-5

1st

I

Enter the number of actuators (optional).

6-10

2nd

I

Enter unit number for input of actuator data. Defaults to input.

3rd data block Repeat for each actuator to be modified.

Main Index

1-5

1st

I

Enter the element number

6-15

2nd

F

Enter the new length of the actuator.

16-20

3rd

I

Enter the table ID for the length of the actuator.

Chapter 4 History Definition Options 1597 Rate Dependent Analysis

Chapt Rate Dependent Analysis This section describes the control of the transient aspects of rate dependent analysis. There are several er 4 ways to specify the time step (TIME STEP) in either creep or viscoelastic analysis. Note that the adaptive Histor options AUTO STEP, AUTO CREEP, and AUTO THERM CREEP are recommended. The ACCUMULATE and EXTRAPOLATE options are techniques to allow extrapolation in time based on the results previously y calculated. Note that extrapolation is always a risky procedure. Defini tion Optio ns

Main Index

1598 CREEP INCREMENT Define Creep Increment

CREEP INCREMENT

Define Creep Increment

Description This option allows manual control of the creep time step size. This form of control is not recommended. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words CREEP INCREMENT.

F

Creep time increment.

2nd data block 1-15

Main Index

1st

AUTO CREEP 1599 Control Transient Creep

AUTO CREEP

Control Transient Creep

Description This option controls the transient creep analysis. You specify a total creep time and a suggested time increment. Marc automatically selects the largest possible time increment consistent with the tolerance set on stress and strain increments. You should make sure that load increments are not left on unintentionally, since this would reduce the time step size severely. Information is also input for limiting the total number of time increments. See Marc Volume A: Theory and User Information. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words AUTO CREEP.

2nd data block 1-15

1st

F

Enter the suggested time increment for creep. When the automatic creep control is in use, Marc iterates for the appropriate increment size to satisfy the tolerances placed on stress and strain increments.

16-30

2nd

F

Period of creep time to be covered during this AUTO CREEP option. This value can be changed at restart by using the REAUTO option.

31-35

3rd

I

Maximum number of time increments to be allowed during this part of the creep analysis. Default is 50 increments.

36-40

4th

I

Maximum number iterations allowed to modify the time step during an increment. Default is 5.

41-45

5th

I

Number of increments between stiffness matrix updates. This option is used to prevent unnecessary updating of the stiffness matrix during large displacement creep analysis. If left blank, the stiffness matrix is reformed each step if tangent modulus nonlinearities (for example, plasticity) are present.

Main Index

46-50

6th

I

Not used; enter 0.

51-60

7th

F

Enter stable time step limit, if known. Marc uses stresses and strain change tolerances if this is not used. Stable time step limit is needed for viscoplasticity.

1600 AUTO CREEP Control Transient Creep

Format Fixed

Free

Data Entry Entry

3rd data block 1-10

1st

F

If the fifth field is 0, enter tolerance on the creep strain increment relative to the elastic strain. Default is 0.50. Note that a higher value is likely to cause stability problems. If the fifth field is 1, enter the maximum creep strain increment allowed. Default is .01.

11-20

2nd

F

If the fifth field is 0, enter the tolerance on the stress change per stress during creep. Default is 0.10. If the fifth field is 0, enter the maximum stress increment. Default is 100. This control is included primarily for accuracy purposes. The default value is adequate for creep laws of the type ε = Aσn, where 3
21-30

3rd

F

Tolerance on low stress point cut-off. Points with a stress lower than this ratio relative to the maximum stress in the structure are not used in the creep tolerance checking. Default is 0.05.

31-35

4th

I

Number of the element in which the stress change is checked. Leave blank to check all elements for stress change. If a number of elements (but not all elements) are to be checked, enter the number of elements as a negative number, with 14 as the maximum. In this case, the actual elements are entered on the next data block.

36-40

5th

I

Enter 1 if absolute rather than relative testing is to be performed.

4th data block This series is only required if the entry in the fourth field of the previous block is negative. 1-70

Main Index

1st

I

Enter the elements to be checked in (14I5) format.

ACCUMULATE 1601 Specify Accumulation Option

ACCUMULATE

Specify Accumulation Option

Description This flags the start of accumulation of strains and displacements for use with the extrapolate option. If a new accumulation period is to be started immediately after an extrapolation in the same increment, the ACCUMULATE option must be preceded by the EXTRAPOLATE option. These options are typically used to predict creep behavior at large times. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the word ACCUMULATE.

1602 EXTRAPOLATE Specify Extrapolation Option

EXTRAPOLATE

Specify Extrapolation Option

Description This option uses the accumulation of strains and displacements during one cycle of loading. It takes a linear extrapolation with respect to time or loading of the accumulated quantities. Note:

In order to use this option, the ACCUMULATE parameter must be included. The extrapolation is made from the period starting with the last entry of the ACCUMULATE option and ending at the current increment. If no ACCUMULATE option was used before, the accumulation period starts at the beginning of the analysis. A regular load increment can be applied simultaneously with the EXTRAPOLATE option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the word EXTRAPOLATE.

F

If a positive number is entered: Time to which extrapolation is to be extended.

2nd data block 1-10

1st

If a negative number is entered: Factor with which the previous accumulation period is multiplied to obtain extrapolation period.

Main Index

AUTO THERM CREEP 1603 Automatic, Thermally-Loaded Elastic-Creep Analysis

AUTO THERM CREEP

Automatic, Thermally-Loaded Elastic-Creep Analysis

Description This option is intended to allow automatic, thermally loaded elastic-creep/elastic-plastic-creep stress analysis, based on a set of temperatures defined throughout the mesh as a function of time. The temperatures and transient times are presented to Marc through the CHANGE STATE option, using input option 3 (post file), and Marc then creates its own set of temperature steps (increments) based on a temperature change tolerance provided on this option. The times at all temperature steps are calculated by Marc for creep analyses. At each temperature step (increment), an elastic/elastic-plastic analysis is carried out first to establish stress level in the structure. A creep analysis is performed next on the structure for the time period between current and previous temperature steps (increments). Both the elastic/elastic-plastic stress and the creep analyses are repeated until the total creep time provided on this option is reached. Convergence controls are provided on the CONTROL option for elastic-plastic analysis and on the AUTO THERM CREEP option for creep analysis. You also specify a suggested time increment for creep analysis. Marc automatically selects the largest possible time increment consistent with the tolerance set on stress and strain increments. The analysis can be restarted at temperature steps (increments) or at creep steps (subincrements). The results can be saved on a post file (POST option) for postprocessing. The automatic thermally loaded elastic-creep/elastic-plastic-creep analysis continues until the total creep time is reached. A typical automatic thermally loaded elastic-creep/elastic-plastic-creep analysis has as input: AUTO THERM CREEP 50.,0,0,4.0, 0.1,2.0, 0.,0.,0.,1, CHANGE STATE 1,3,0,19,1,4,1, CONTINUE In the above case, a temperature change tolerance of 50 is set for the creation of temperature steps (increments) by Marc; the total transient time in thermal analysis is equal to 4.0; the suggested time increment for creep analysis is 0.1; and the total creep time (time for the termination of this analysis) is 2.0. Note that the total creep time cannot be greater than the total transient time in the thermal analysis. The data in the CHANGE STATE option indicates that the temperatures are stored in a formatted post file (file 19) and there are four sets of temperatures on the file. Mechanical Loading - No Table Driven Input If no DIST LOADS, POINT LOAD or PROPORTIONAL INCREMENT option appears with the AUTO THERM CREEP set, all mechanical loads and kinematic boundary conditions are held constant during the AUTO THERM CREEP. However, DIST LOADS, POINT LOAD, PROPORTIONAL INCREMENT, or DISP CHANGE can be included in the set. The mechanical loads and kinematic boundary conditions,

Main Index

1604 AUTO THERM CREEP Automatic, Thermally-Loaded Elastic-Creep Analysis

which are then defined, are assumed to change in proportion to the time scale of the temperature history defined by the CHANGE STATE option and are applied accordingly on the basis that the increments of load and displacement correspond to the end of the transient time (TOTIM) of the AUTO THERM CREEP option input. Mechanical Loading - Table Driven Input When table input is used and either FIXED DISP, POINT LOAD, or DIST LOADS references a table which is a function of time, the total mechanical boundary condition will be evaluated based upon the current time. Note:

You must include the CHANGE STATE, option 3 (post file), in conjunction with this option.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-16

1st

A

Enter the words AUTO THERM CREEP.

2nd data block 1-10

1st

F

Enter the maximum temperature change to be used per step of stress analysis. Marc linearly subdivides steps, or merges steps together, to create increments which are close to, but do not exceed, this tolerance.

11-15

2nd

I

Enter the maximum number of increments to be allowed in this AUTO THERM CREEP. If this number of increments is exceeded before the temperature history is completed, Marc ends. This is intended as a protection to avoid excessive increments in the case of a data error. Default value is 50 increments if set to 0.

16-20

3rd

I

Reassembly internal for element matrices.

21-30

4th

F

Total transient time from heat transfer analysis. This is used to proportionally scale the incremental boundary conditions.

3rd data block

Main Index

1-15

1st

F

Enter the suggested time increment for creep. When the automatic creep control is in use, Marc iterates for the appropriate increment size to satisfy the tolerances placed on stress and strain increments by the CREEP model definition option.

16-30

2nd

F

Total creep time to be covered during this AUTO THERM CREEP option. This value can be changed at restart by using the REAUTO option.

AUTO THERM CREEP 1605 Automatic, Thermally-Loaded Elastic-Creep Analysis

Format Fixed 31-35

Free 3rd

Data Entry Entry I

Maximum number of subincrements to be allowed during this part of the creep analysis. Default is 50.

36-40

4th

I

Maximum number of iterations allowed to modify the time step during an increment. Default is 5.

41-45

5th

I

Number of increments between stiffness matrix updates. This reduces the number of updates to the stiffness matrix for mildly nonlinear analyses. This should not be activated if elastic material properties are temperature dependent. If left blank, the stiffness matrix is reformed each step if tangent modulus nonlinearities occur.

4th data block 1-10

1st

F

If the fifth field is a zero, enter tolerance on the creep strain increment relative to the elastic strain. Default is 0.50. Note that a higher value is likely to cause stability problems. If the fifth field is a one, enter the maximum creep strain increment allowed. Default is .01.

11-20

2nd

F

If the fifth field is a zero, enter the tolerance on the stress change per stress during creep. Default is 0.10. If the fifth field is a one, enter the maximum stress increment. Default is 100. This control is included primarily for accuracy purposes. The default value is adequate for creep laws of the type ε = Aσn, where 3
21-30

3rd

F

Tolerance on low stress point cut-off. Points with a stress lower than this ratio relative to the maximum stress in the structure is not used in the creep tolerance checking. Default is 0.05.

Main Index

1606 AUTO THERM CREEP Automatic, Thermally-Loaded Elastic-Creep Analysis

Format Fixed

Free

Data Entry Entry

31-35

4th

I

Number of the element in which the stress change is checked. Leave blank to check all elements for stress change. If a number of elements (but not all elements) are to be checked, enter the number of elements as a negative number, with 14 as the maximum. In this case, the actual elements are entered on the next data line.

36-40

5th

I

Enter 1 if absolute rather than relative testing is to be performed.

5th data block This data block is only required if the entry in the fourth field of the previous data block is negative. 1-70

Main Index

1st

I

Enter the elements to be checked in (14I5) format.

Chapter 4 History Definition Options 1607 Dynamic Analysis

Chapt Dynamic Analysis This section describes the options used to control dynamic analysis. The MODAL SHAPE option requests er 4 Marc calculate the eigenvalues and eigenvectors of the structure. In linear dynamic analysis, this Histor that option immediately follows the END OPTION. It is possible to do a nonlinear static analysis and then perform a modal extraction based on the current deformed state. These modes can then be used to y perform a transient analysis. The DYNAMIC CHANGE option is used to specify the incremental time and Defini the total time period to be covered. An automatic time-stepping scheme (AUTO STEP) is also available for dynamic analysis. The SPECTRUM option allows a spectral response analysis be performed based tion upon the modes previously extracted. In addition, harmonic analysis can be performed at any step in an Optio analysis. The harmonic response is based on the current configuration of the structure. ns

Main Index

1608 MODAL SHAPE Define Modal Shape

MODAL SHAPE

Define Modal Shape

Description This option is used when a modal analysis is indicated on the DYNAMIC parameter or during an acoustic analysis to indicate that eigenmodes are to be extracted. When using the inverse power shift method, this option controls the initial shift and the number of modes to be calculated per shift. The accuracy of the modes calculated is degraded if the number of modes per shift is too high. When using the Lanczos method, if a highest frequency is entered, a Sturm sequence check is performed. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

A

Enter the words MODAL SHAPE.

Option A If inverse power sweep method is used (as specified with the DYNAMIC parameter), use this option. 2nd data block 1-5

1st

I

Maximum number of iterations per mode in the power sweep. Default is 40.

6-15

2nd

F

Convergence tolerance. The power sweep terminates when the difference between the eigenvalues in two consecutive sweeps divided by the eigenvalue is less than the tolerance. Default is 1 x 10-5.

16-25

3rd

F

Initial shift in cycles per time. The power shift is likely to start converging to the eigenvalue closest to this value. Default is 0.

26-35

4th

F

Maximum frequency to be extracted in cycles per time. If this is left blank or zero, the number of modes requested on the DYNAMIC parameter is extracted. If this is nonzero, extraction ends when this frequency is exceeded or when the number of modes requested on the DYNAMIC parameter is reached, whichever occurs first.

36-40

5th

I

Number of modes extracted per shift. This data field determines if auto shifting occurs. If auto shift is not required, set equal to or greater than number of modes requested on the DYNAMIC parameter. Default is 5.

Main Index

MODAL SHAPE 1609 Define Modal Shape

Format Fixed 41-50

Free 6th

Data Entry Entry F

Auto shift parameter. Marc determines the new shift point (in frequency squared) as the highest frequency square plus this entry times the difference between the highest and next highest distinct frequency squared. Default is 1.0.

Option B If the Lanczos method is used (as specified with the DYNAMIC parameter), use the following data blocks. 2nd data block 1-10

1st

F

Lowest frequency of mode to be extracted (in cycles/time). This is also the initial shift point. This cannot be changed upon restart.

11-20

2nd

F

SHFMAX, highest frequency of modes to be extracted. If set to 0, NSNRM modes are extracted. If not set to zero, all modes between SHFMIN and SHFMAX are extracted and NSNRM is not used. A Strum sequence check is performed to calculate this number. This can be changed upon restart.

21-25

3rd

I

NSNRM, number of requested modes. Only needed if SHFMAX is set equal

to 0. This can be increased upon restart.

Main Index

26-30

4th

I

Not used; enter 0.

31-35

5th

I

Not used; enter 0.

1610 RECOVER Recover Option

RECOVER

Recover Option

Description This option allows for: (1) the storing of eigenvectors on the post file, (2) the recovery of reaction forces, or (3) the recovery of stresses and reactions for a specified number of modes during a modal or a buckling analysis. The option should be used after the modal shapes and frequencies or buckling modes have been extracted (MODAL SHAPE or BUCKLE history definition option), and can be repeated as many times as you wish. Additional input data is required on parameters DYNAMIC or BUCKLE for the activation of this option, and the POST model definition option must be included in the input if the eigenvectors are to be stored on a post file. In the RECOVER option, the stresses are computed from the modal displacement vector, φ (eigenvector without normalization), and the nodal reactions are calculated from F = Kφ -ω2 Mφ for the modal analysis or from F = Kφ for buckling analysis. You can choose your normalization by entering the amplitude value of one particular degree of freedom of one particular node in the mesh. The eigenvector is scaled linearly such that the degree of freedom on this node reaches above amplitude. When performing a modal analysis on a structure with rubber material, it is recommended that the modes be scaled so that the amplitude is small relative to the element size if the modal stresses or the reactions are to be calculated. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word RECOVER.

I

Starting mode number.

2nd data block 1-5

1st

Default is 1. 6-10

2nd

I

Ending mode number. Default is modes specified on the DYNAMIC or BUCKLE parameter.

11-15

3rd

I

Set to 0 if only the eigenvectors are to be written to post file. Set to 1 if only reactions are to be calculated. Set to 2 if both stresses and reactions are to be calculated. NOTE: If set to 2, the 4th field of the DYNAMIC parameter or the 3rd field of the BUCKLE parameter must be set equal to 1.

Main Index

RECOVER 1611 Recover Option

Format Fixed 16-20

Free 4th

Data Entry Entry I

Node number of node with respect to which the eigenvector is scaled. Default is 0.

21-25

5th

I

Degree of freedom of node selected in the fourth field with respect to which the eigenvector is scaled. Default is 0.

26-35

6th

E

Reference amplitude of degree of freedom of node selected above. Default is 0, which uses the eigenvector without user scaling.

Main Index

1612 DYNAMIC CHANGE (Dynamic) Define Integration in Time

DYNAMIC CHANGE (Dynamic)

Define Integration in Time

Description This option specifies the parameters required for integration in time when the fixed time step procedure is to be used. It can be used for either the modal or the direct integration procedure. See Marc Volume A: User Information on Dynamic Options and the DYNAMIC, ACOUSTIC, PIEZO, or EL-MA parameter (see Chapter 2). In the case of explicit analysis, IDYN = 5, the time step is adjusted at the given increment interval to insure that the stability limit is not violated. In the case of explicit analysis, IDYN = 4, the time step is adjusted to ensure that the stability limit is not violated at the start of this DYNAMIC CHANGE. Format Format Fixed

Free

Data Entry Entry

1st data block 1-14

1st

A

Enter the words DYNAMIC CHANGE.

2nd data block 1-15

1st

F

Time step size.

16-30

2nd

F

Period of time for this set of boundary conditions.

31-35

3rd

I

Number of time steps in this set of boundary conditions.

36-40

4th

I

Increment frequency to recalculate the time step for IDYN = 5; default is 100.

41-45

5th

I

Reassembly interval for mass and stiffness matrices; for linear problems, set equal to value in the third field. This may be used to reduce the number of updates to the stiffness matrix for mildly nonlinear analysis.

46-50

6th

I

This field is not used; enter 0.

51-60

7th

F

Enter γ for Newmark operator. Default is γ = 0.5 or what was used in previous DYNAMIC CHANGE option.

61-70

8th

F

Enter β for Newmark operator. Default is β = 0.25 or what was used in previous DYNAMIC CHANGE option.

Main Index

SPECTRUM 1613 Initiate Spectral Response Analysis

SPECTRUM

Initiate Spectral Response Analysis

Description This option initiates the spectral response analysis. The calculation is based upon the last set of eigenmodes obtained. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word SPECTRUM.

I

Enter the number of modes to be used.

2nd data block 1-5

1st

Enter 0 if a range of frequencies are given in the second and third field. 6-15

2nd

F

Enter the lowest frequency to be used in response analysis, in cycles per time unit.

16-25

3rd

F

Enter the highest frequency to be used in response analysis, in cycles per time unit.

3rd data block 1-10

1st

F

Weighting factor associated with first degree of freedom.

11-20

2nd

F

Weighting factor associated with second degree of freedom.

21-30

3rd

F

Weighting factor associated with third degree of freedom. Etc.; for higher degrees of freedom–maximum of 8 factors on a data line.

Main Index

1614 HARMONIC (Dynamic) Define Excitation Frequency

HARMONIC (Dynamic)

Define Excitation Frequency

Description This option is necessary to specify the frequency of excitation implemented. The option is used in dynamic harmonic, acoustic, and piezoelectric analyses. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word HARMONIC.

2nd data block 1-10

1st

F

Enter the lowest frequency in cycles per time unit.

11-20

2nd

F

Enter the increment in frequency for each subincrement. If zero, only single frequency is used.

21-30

3rd

F

Enter the highest frequency in cycles per time unit.

31-35

4th

I

Enter 0 for linear increments in frequency (default). Enter 1 for logarithmic increments in frequency.

36-40

5th

I

Enter the number of frequencies (n) if linear intervals, then if n = ( ω HIGH – ω L OW ) ⁄ ( Δ ω ) Δ ω i = entered value of ( ω HI GH – ω L OW ) ⁄ n – 1

If logarithmic increments in frequency ω HIGH ( 1 ⁄ n – 1 ) f ac = ⎛ ----------------⎞ ⎝ ω LOW ⎠ Δ ω i = f ac ** ( i – 1 )

Main Index

n = 0;

ACC CHANGE 1615 Define Acceleration Boundary Conditions

ACC CHANGE

Define Acceleration Boundary Conditions

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new nodal acceleration conditions to be specified in a dynamic analysis. You specify total accelerations through this option. Complex accelerations are more conveniently defined by the FORCDT user subroutine. Note that enough space must be specified on the SIZING parameter on the maximum number of boundary condition field to allow for possible increased storage requirements arising from the use of this option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ACC CHANGE.

I

Enter the number of sets of boundary condition data lines to be read (optional)

2nd data block 1-5

1st

For each set of boundary conditions use the 3rd, 4th, and 5th data blocks. 3rd data block 1-10

1st

E

Prescribed acceleration for first degree of freedom listed in data block 4.

11-20

2nd

E

Prescribed acceleration for second degree of freedom listed in data block 4.

21-30

3rd

E

Prescribed acceleration for third degree of freedom listed in data block 4.

4th data block Enter a list of degrees of freedom to which the above prescribed displacements are prescribed. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes to which the above accelerations are applied.

Main Index

1616

Main Index

Chapter 4 History Definition Options 1617 Heat Transfer Analysis

Chapt Heat Transfer Analysis This section describes the control of both steady-state and transient heat transfer analyses. The er 4 option is available to specify the incremental time and the total time in this set. The default Histor isTRANSIENT that an adaptive time stepping is performed to cover the complete time period, such that the your tolerances are satisfied. These tolerances are given in the CONTROL option. The AUTO STEP option may y also be used to control the time steps in a transient thermal analysis. There are several methods of Defini specifying the fluxes. Note that the total flux is required in a heat transfer analysis. tion Optio ns

Main Index

1618 TRANSIENT Specify Transient or Steady-State Heat Transfer Analysis

TRANSIENT

Specify Transient or Steady-State Heat Transfer Analysis

Description This option controls the transient heat transfer analysis. Marc optionally uses automatic time step controls, based on the maximum nodal temperature change allowed (input on the CONTROL model definition option). You input a suggested initial time step which is adjusted according to the automatic stepping scheme (see Marc Volume A: User Information). The transient period can be ended in one of two ways. A time period is input – the transient solution continues until this period is completed. You can also give a finish temperature, and a flag which indicates that the transient solution should end when all nodal point temperatures are below (or above) this finish temperature. This second technique for ending the transient is optional and does not disable the first option, so that an adequately long time period should be allowed if the finish temperature option is to govern the solution. In addition, you should supply a maximum number of steps to be allowed. This is intended to prevent an excessive number of increments in case of a data error. If Marc analyzes this number of increments before completing the time period (or reaching the finish temperature), it stops any further analysis. For steady-state solutions, use the TRANSIENT NON AUTO option with one “infinite” time step (set specific heat to zero if problem is linear). Use the recycling tolerance for property evaluation for nonlinear steady-state solutions. In addition, the STEADY STATE option is also available for steady-state solution. The first line must be in fixed format. Format Format Fixed

Free

Data Entry Entry

1st data block 1-9

1st

A

Enter the word TRANSIENT.

11-18

2nd

A

Leave blank to use automatic time stepping. Enter the words NON AUTO to suppress automatic time stepping, and complete total period with a uniform time step.

21-28

3rd

A

Enter the words NO SOLID to suppress performing a structural analysis during this period in a coupled analysis.

2nd data block

Main Index

1-10

1st

F

Suggested initial time step. This is be adjusted by the automatic timestepping scheme (see Marc Volume A: User Information).

11-20

2nd

F

Time period. Marc continues the transient solution until this time period is completed, unless the finish temperature option is flagged.

TRANSIENT 1619 Specify Transient or Steady-State Heat Transfer Analysis

Format Fixed 21-25

Free 3rd

Data Entry Entry I

Maximum number of steps to be allowed in this transient period. Marc stops the analysis if this number of steps is exceeded. This data field is intended to be used to avoid excessive steps in the automatic control. Default (if left blank) is time period divided by suggested step.

26-30

4th

I

Not used; enter 0.

31-35

5th

I

Reassembly interval – number of increments between reassessment of element (material) properties based on temperature or time dependency. For purely linear problems (constant properties), a large number should be given here to avoid reassembly. Default value (if left blank) is automatic reassembly controlled by the temperature change given on the CONTROL option, data line 3, second field. Note that if a material property or film coefficient changes, reassembly is needed.

36-40

6th

I

Set to 1 to finish the transient when all nodal temperatures fall below the value given in the seventh field (see below). Set to -1 to finish the transient when all nodal temperatures exceed the value given in the seventh field (see below). Set to 0 to complete transient time period without any check on temperatures reached. Set to 2 to indicate that a steady-state analysis is to be performed in one increment.

41-50

Main Index

7th

F

Finish temperature value to be used in conjunction with flag set above.

1620 STEADY STATE (Heat Transfer) Specify Steady-State Heat Transfer Analysis

STEADY STATE (Heat Transfer)

Specify Steady-State Heat Transfer Analysis

Description This option allows the solution of the steady-state heat transfer problem. This procedure uses less computation time than using the TRANSIENT NON AUTO option with a large time step. If temperature dependent properties or boundary conditions are included, the recycling tolerance for property evaluation must be used so that iteration is performed. Marc begins execution of the step when a CONTINUE option is encountered. Multiple steady-state steps can be performed to solve quasi-steady-state problems. The first line must be in fixed format. Format Format Fixed

Main Index

Free

Data Entry Entry

1-10

1st

A

Enter the words STEADY STATE.

21-28

2nd

A

Enter the words NO SOLID to suppress performing a structural analysis during this period in a coupled analysis.

DIST FLUXES (History Definition) 1621 Define Distributed Fluxes

DIST FLUXES (History Definition)

Define Distributed Fluxes

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows distributed (surface and volumetric) fluxes to be specified. Distributed fluxes are converted to consistent nodal fluxes by Marc. For a given element type, there is an established convention for the application of surface flux on a particular face. The FLUX user subroutine can be used to input and spatial dependent fluxes. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST FLUXES.

2nd data block 1-5

1st

I

Enter the number of sets of distributed fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed flux data, defaults to input.

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library.

3rd data block 1-5

1st

Also see distributed flux type 101 under the COUPLE parameter definition. 6-15

2nd

F

Enter the magnitude of this type of distributed fluxes.

16-20

3rd

I

Flux index (optional). (Flux index is to be used in the FLUX user subroutine.)

4th data block Enter a list of elements associated with the above distributed fluxes.

Main Index

1622

Main Index

POINT FLUX (History Definition) 1623 Define Point Fluxes

POINT FLUX (History Definition)

Define Point Fluxes

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows total nodal point fluxes to be specified. The FORCDT user subroutine can be used for the time dependent fluxes. If the number of nodes which have point fluxes has been changed from the model definition option, you must give an upper bound on the FLUXES parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of point fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point flux data; defaults to input.

3rd data block 1-10

1st

F

Magnitude of point flux.

11-20

2nd

F

Magnitude of point flux for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point flux for third degree of freedom, (heat transfer shell elements only).

4th data block Enter a list of nodes to which the above nodal sources are applied.

Main Index

1624 WELD FLUX (History Definition) Define Motion and Flux Parameters for Weld Heat Source

WELD FLUX (History

Define Motion and Flux Parameters for Weld Heat Source

Definition) The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows welding (surface and volumetric) fluxes to be specified. Two groups of parameters are used in this option to specify the weld flux. The first group pertains to the initial location and motion of the weld source and the second group pertains to the magnitude and shape of the weld source. The distributed weld fluxes are converted to consistent nodal fluxes by Marc. The default volumetric weld flux has a double ellipsoidal shape and is suitable for deep penetration welding processes like laser welding and electron beam welding. The default surface weld flux has a disc shape and is suitable for welding processes like arc welding. Arbitrary volumetric or surface flux values at integration points along the weld path can be specified through the UWELDFLUX user subroutine. Refer to Marc Volumes A, D, and E for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD FLUX.

2nd data block 1-5

1st

I

Enter the number of sets of weld fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld flux data; defaults to input.

3rd data block 1-5

1st

I

Weld Flux Index (Index is to be used in the UWELDFLUX user subroutine).

6-10

2nd

I

Weld Flux Type: 1 – double ellipsoidal shaped volumetric weld flux. 2 – disc shaped surface weld flux. 3 – user subroutine defined weld flux.

11-15

Main Index

3rd

I

Weld Path Index.

WELD FLUX (History Definition) 1625 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

16-20

4th

I

Weld Filler Index.

21-25

5th

I

Parameter identifying the type of distributed flux. See library element description in Marc Volume B: Element Library. Note that the parameter in this field should be consistent with the weld flux type specified in the 2nd field.

26-30

6th

I

Initial Position Flag: 0 – Initial weld position is automatically taken as first point of associated weld path. 1 – Initial weld position is specified in the first three fields of the 4th data block.

31-35

7th

I

Weld Flux Activation Flag 0 – Weld Flux boundary condition is active in loadcase 1 – Weld Flux boundary condition is inactive in loadcase

36-67

8th

C

Weld Flux Name (optional)

4th data block 1-10

1st

F

X coordinate for initial position of weld flux.

11-20

2nd

F

Y coordinate for initial position of weld flux.

21-30

3rd

F

Z coordinate for initial position of weld flux.

31-40

4th

F

Local X offset from weld path.

41-50

5th

F

Local Y offset from weld path.

51-60

6th

F

Velocity of weld flux.

61-65

7th

I

Table ID for velocity.

Notes: The initial position defined in fields 1, 2, and 3 of data block 4 is only used if the initial position flag in the 6th field of the 3rd data block is nonzero. Also, the given initial weld position should be along the associated weld path. Else, the program will terminate with exit 20. The defined initial weld position is mandatory when the UWELDPATH user subroutine is used to define the associated weld path. When the same weld flux is specified in multiple loadcases, the initial weld position is only used for the starting loadcase. For subsequent loadcases, the position at the end of the previous loadcase is used as the starting position. The X and Y offsets (fields 4 and 5 in data block 4) are defined in the local coordinate system of the weld flux. They are 0 by default. The Y offset is along the arc direction and the X offset is along the tangent direction. These offsets allow the flux to be located at a specified distance from the associated weld path. The table defining the weld velocity can be a function of time.

Main Index

1626 WELD FLUX (History Definition) Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

5th data block 1-10

1st

F

Power of weld flux.

11-20

2nd

F

Efficiency of weld flux.

21-30

3rd

F

Scale Factor for weld flux.

31-40

4th

F

Width of weld (for volumetric source). Radius of weld (for surface source).

Fields 5 through 7 are only valid for the double ellipsoidal volumetric weld flux: 41-50

5th

F

Depth of weld.

51-60

6th

F

Forward length of weld.

61-70

7th

F

Rear length of weld.

71-80

8th

F

Maximum distance from weld origin for nonzero flux.

6th data block 1-5

1st

I

Table ID for Weld Flux Power.

6-10

2nd

I

Table ID for Weld Flux Efficiency.

11-15

3rd

I

Scale Factor Flag: 0 – Use automatic scale factor. 1 – Use manually defined scale factor.

16-20

4th

I

Table ID for Weld Width/Radius.

Fields 5 - 7 are only valid for the double ellipsoidal volumetric weld flux:

Main Index

21-25

5th

I

Table ID for Weld Depth.

26-30

6th

I

Table ID for Weld Forward Length.

31-35

7th

I

Table ID for Weld Rear Length.

36-40

8th

I

Table ID for maximum distance from weld origin.

WELD FLUX (History Definition) 1627 Define Motion and Flux Parameters for Weld Heat Source

Format Fixed

Free

Data Entry Entry

Notes: The 5th and 6th data blocks are directly used for the ellipsoidal and disc shaped weld fluxes. The flux values are defined directly for the user subroutine option. The weld dimensions can still be entered in this case since they are useful for filler element activation, adaptive meshing box definition, etc. The scale factor in the 3rd field of the 5th data block can be manually specified or automatically determined by the program. The scale factor flag in the 3rd field of the 6th data block determines the usage. See Volume A for more details. If the maximum distance from weld origin is not defined (left as 0), then the weld pool dimensions are used to determine which elements receive the weld flux. The tables defining the weld power, efficiency, weld width/radius, depth, forward and rear lengths, and maximum distance from weld origin can be a function of time or arc length measured along the associated weld path. 7th data block Enter a list of elements associated with the above weld flux.

Main Index

1628 WELD PATH (History Definition) Define Path and Arc Orientation for Weld Heat Source

WELD PATH (History

Define Path and Arc Orientation for Weld Heat Source

Definition) Description This option specifies the weld path to be followed by the weld flux. The orientation of the arc along the path is also defined. The weld path can be specified through nodes or point coordinates of polyline curves in the input file or through point coordinates in a separate text file, or through the UWELDPATH user subroutine. The arc orientation can be specified through nodes, point coordinates of polyline curves, vector components or Euler angles in the input file, point coordinates, vector components, or Euler angles in a separate text file, or through the UWELDPATH user subroutine. The specified path and arc orientation are used to define a moving local coordinate system. The Z axis of the local coordinate system is along the weld path, the Y axis is along the arc orientation and the X axis is along the tangent. X and Y axes that are perpendicular to each other and perpendicular to the given weld path (Z axis) are constructed based on the information provided in this option. See MARC Volume A: Theory and User Information for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD PATH.

2nd data block 1-5

1st

I

Enter the number of sets of weld paths to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld path data, defaults to input.

3rd data block 1-5

1st

I

Weld Path Index (Index is used for cross-referencing with the 3rd data block of the WELD FLUX option)

6-10

2nd

I

Weld Path Type 1 – Weld Path is specified through ordered list of nodes 2 – Weld Path is specified through point coordinates of polyline curves. 4 – Weld Path is specified through text file 5 – Weld Path is specified through the UWELDPATH user subroutine.

11-15

3rd

I

Arc Orientation Type 1 – Arc Orientation is specified through ordered list of nodes. 2 – Arc Orientation is specified through point coordinates of polyline curves.

Main Index

WELD PATH (History Definition) 1629 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry 3 – Arc Orientation is specified through vector components. 4 – Arc Orientation is specified through Euler angles. 5 – Arc Orientation is specified through the UWELDPATH user subroutine.

16-20

4th

I

Number of curves used to define the Weld Path. This field is only valid when Weld Path Type is 2.

21-25

5th

I

Path Interpolation flag 0 or 1. 0 – Arc Orientation at first point of segment is used for whole segment. 1 – Arc Orientation is linearly interpolated between first and last points of segment.

26-30

6th

I

Not used.

31-62

7th

C

Weld Path Name (optional)

Notes: Weld Path Type 1 can only be used with Arc Orientation Types 1, 3, or 4. Weld Path Type 2 can only be used with Arc Orientation Types 2, 3, or 4. Weld Path Type 4 can only be used with Arc Orientation Type 2, 3, or 4. All quantities are specified via separate text file in this case. Weld Path Type 5 can only be used with Arc Orientation Type 5. The 4th through 7th data blocks depend on the WELD PATH TYPE (2nd field of 3rd data block) and ARC ORIENTATION TYPE (3rd field of 3rd data block). These data blocks are only needed for weld path types 1, 2, and 4. I. WELD PATH TYPE 1 (NODES) 4th data block Enter an unsorted list of nodes or unsorted set of nodes (NDSQ) needed to define the weld path. A. ARC ORIENTATION TYPE 1 (NODES)

5th data block 1-10

1st

F

Angle in degrees by which the ARC-TANGENT plane is rotated about weld path (default is 0).

11-15

2nd

I

Table ID for Angle.

6th data block Enter an unsorted list of nodes or unsorted set of nodes (NDSQ) needed to define the weld orientation.

Main Index

1630 WELD PATH (History Definition) Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

Notes: The table defining the angle can be a function of the arc length along the weld path or a function of the position coordinates along the weld path. The arc vector is defined as the vector from the weld path node to the weld orientation node. The number of nodes defining the weld orientation has to be either equal to 1 or equal to the number of nodes defining the weld path. If only one node is used, the arc vector is defined as the vector from the weld path node to that node always. B. ARC ORIENTATION TYPE 3 (VECTOR)

5th data block 1-10

1st

F

Component X of Arc Orientation Vector.

11-20

2nd

F

Component Y of Arc Orientation Vector.

21-30

3rd

F

Component Z of Arc Orientation Vector.

31-35

4th

I

Table ID for Component X.

36-40

5th

I

Table ID for Component Y.

41-45

6th

I

Table ID for Component Z.

Note:

The tables defining the arc orientation vector components can be a function of the arclength along the weld path or a function of the position coordinates along the weld path.

C. ARC ORIENTATION TYPE 4 (EULER ANGLES)

5th data block 1-10

1st

F

Rotation of unit vector in X direction about global X axis.

11-20

2nd

F

Rotation of unit vector in X direction about global Y axis.

21-30

3rd

F

Rotation of unit vector in X direction about global Z axis.

31-35

4th

I

Table ID for Rotation about X.

36-40

5th

I

Table ID for Rotation about Y.

41-45

6th

I

Table ID for Rotation about Z.

Note:

Main Index

All rotation values are specified in degrees. If all rotation values are 0, the arc orientation is taken as <1,0,0>; i.e., unit vector in global X direction. Tables defining the Euler angles can be a function of arclength along the weld path or a function of the position coordinates along the weld path.

WELD PATH (History Definition) 1631 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

II. WELD PATH TYPE 2 (CURVES) Start Loop over Number of Polyline Curves Read Number of Points to define Polyline

(4th data block)

Start Loop over Number of Points to define Path Polyline Read coordinates of each Weld Path Point

(5th data block)

End loop over Points End loop over Polyline Curves

For Each Curve: 4th data block 1-5

1st

I

Weld Curve Type (polyline = 1).

6-10

2nd

I

Number of Points to Define Polyline.

For each point on the Weld Path Curve: 5th data block 1-10

1st

F

X coordinate of point.

11-20

2nd

F

Y coordinate of point.

21-30

3rd

F

Z coordinate of point.

A. ARC ORIENTATION TYPE 2 (CURVES) Start Loop over Number of Polyline Curves Read Angle for Rotation of Tangent-Arc Plane (6th data block) Start Loop over Number of Points to define Arc Polyline Read coordinates of each Weld Orientation Point (7th data block) End Loop over Point End Loop over Polyline Curves

For Each Curve: 6th data block

Main Index

1-5

1st

I

Arc Curve Type (polyline = 1).

6-15

2nd

F

Angle in degrees by which Arc-Tangent plane is rotated about Weld Path (default = 0).

16-20

3rd

I

Table ID for angle.

1632 WELD PATH (History Definition) Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

For each point on the Arc Orientation Curve: 7th data block 1-10

1st

F

X coordinate of point.

11-20

2nd

F

Y coordinate of point.

21-30

3rd

F

Z coordinate of point.

Notes: Only Polylines (Weld Curve Type = 1, Arc Curve Type = 1) are supported in the current version. The table defining the angle can be a function of the arc length along the weld path or a function of the position coordinates along the weld path. The number of points defining the arc orientation curve has to be equal to the number of points defining the weld path curve. B. ARC ORIENTATION TYPE 3 (VECTOR)

6th data block 1-10

1st

F

Component X of Arc Orientation Vector.

11-20

2nd

F

Component Y of Arc Orientation Vector.

21-30

3rd

F

Component Z of Arc Orientation Vector.

31-35

4th

I

Table ID for Component X.

36-40

5th

I

Table ID for Component Y.

41-45

6th

I

Table ID for Component Z.

Note:

The tables defining the arc orientation vector components can be a function of the arc length along the weld path or a function of the position coordinates along the weld path.

C. ARC ORIENTATION TYPE 4 (EULER ANGLES)

6th data block 1-10

1st

F

Rotation of unit vector in X direction about global X axis.

11-20

2nd

F

Rotation of unit vector in X direction about global Y axis.

21-30

3rd

F

Rotation of unit vector in X direction about global Z axis.

31-35

4th

I

Table ID for Rotation about X.

36-40

5th

I

Table ID for Rotation about Y.

41-45

6th

I

Table ID for Rotation about Z.

Note:

Main Index

All rotation values are specified in degrees. If all rotation values are 0, the arc orientation is taken as <1,0,0> i.e., unit vector in global X direction. Tables defining the euler angles can be a function of arclength along the weld path or a function of the position coordinates along the weld path.

WELD PATH (History Definition) 1633 Define Path and Arc Orientation for Weld Heat Source

Format Fixed

Free

Data Entry Entry

III. WELD PATH TYPE 4 (Text File) 4th data block Enter name of Text File containing Weld Path and Arc Orientation Information. Note:

Main Index

Columns 1 - 3 of the text file contain weld path information. Columns 4 - 6 of the text file contain arc orientation information. Depending on the arc orientation type (2, 3 or 4) specified on the 3rd data block, columns 4 - 6 can contain point coordinates, vector components or Euler angle values. The entry in each column is a real number of width 10. The columns can be in free or fixed format with commas being used to separate the columns in the free format mode.

1634 WELD FILL (History Definition) Define Parameters for Weld Filler Elements

WELD FILL (History Definition)

Define Parameters for Weld Filler Elements

Description This option identifies the weld filler elements that are associated with a particular weld heat source. The method by which the filler elements can potentially participate in the analysis is specified. Two methods can be used: Quiet Element method and Deactivated Element Method. In the Quiet Element Method, the filler elements are always part of the analysis. However, prior to their physical creation, the filler elements are used with scaled down material properties. The regular material properties are restored after the filler elements are physically created by the moving heat source. In the Deactivated Element Method, the filler elements are deactivated at the outset and are automatically activated only when they are physically created by the moving heat source. Filler Bounding Box X, Y, and Z refer to dimensions in the local coordinate system attached to the moving heat source. They are used to identify if filler elements are physically created during the welding process. If these dimensions are not specified on the option (i.e., left at 0), they are related to weld pool dimensions set on the WELD FLUX option: Filler Bounding Box X in the Tangent direction = 1.5 x Weld Width Filler Bounding Box Y in the Arc direction = 2 x Weld Width Filler Bounding Box Z in the Arc Direction = Weld Pool Length See Marc Volume A: Theory and User Information for more details. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words WELD FILL.

2nd data block 1-5

1st

I

Enter the number of sets of weld fillers to be entered (optional).

6-10

2nd

I

Enter unit number for input of weld flux data; defaults to input.

3rd data block 1-5

1st

I

Weld Filler Index (Index is used for cross-referencing with field 4 of the 3rd data block in the WELD FLUX option).

6-10

2nd

I

Initial Activation Flag 0 – Quiet Element Method. 1 – Deactivated Element Method.

Main Index

WELD FILL (History Definition) 1635 Define Parameters for Weld Filler Elements

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Temperature Boundary Condition Flag 0 – Nodal boundary conditions are applied 1 – Nodal boundary conditions are not applied

16-25

4th

F

Melting Point Temperature

26-35

5th

F

Temperature Activation Time (0 by default)

36-45

6th

F

Material Property Scale Factor (1e-5 by default)

46-77

7th

F

Weld Filler Name (Optional)

Notes: The melting point temperature information in field 4 is only used if the boundary condition flag in field 3 is 0. If nodal boundary conditions are not applied (3rd field = 1), weld fluxes can be applied to the filler elements to ramp up the temperature. A user-specified thermal activation time, specified in field 5, can also be used. The thermal activation time serves two purposes: (1) It defines the time over which the temperature boundary condition is ramped (only valid when field 3 is 0). Default is 0 which means that the temperatures are applied instantaneously. For nonzero time values, the temperatures of the active filler elements are linearly increased from the current value to the specified temperature over the specified time step. (2) It defines the time during which the filler elements only participate in the thermal pass and not in the mechanical pass (valid when field 3 is 0 or 1). Default is 0 which means that if the filler elements are first created at increment n, they only participate on the thermal side at increment n, and then participate in both thermal and mechanical passes at increment n+1. For nonzero time values, the filler elements remain thermally active over the specified time duration and become mechanically active only after the time duration. The property scale factor in field 6 is only used for the quiet element method. 4th data block 1-10

1st

F

Filler Bounding Box in X (weld width) direction

11-20

2nd

F

Filler Bounding Box in Y (weld depth) direction

21-30

3rd

F

Filler Bounding Box in +Z (forward path) direction

31-40

4th

F

Filler Bounding Box in -Z (rear path) direction

41-45

5th

I

Table ID for Filler Bounding Box X

46-50

6th

I

Table ID for Filler Bounding Box Y

51-55

7th

I

Table ID for Filler Bounding Box +Z

56-60

8th

I

Table ID for Filler Bounding Box -Z

Note:

Main Index

The table IDs for the filler bounding boxes can be a function of time or arc length. The arc length is measured along the weld path from the first point to the current position of the weld source. If the bounding box dimensions are not specified, the weld pool dimensions are used to define the box.

1636 WELD FILL (History Definition) Define Parameters for Weld Filler Elements

Format Fixed

Free

Data Entry Entry

5th data block 1-80

Main Index

1

I

Enter the list of filler elements

CONTROL (Heat Transfer - History Definition) 1637 Define Controls for Heat Transfer Analysis

CONTROL (Heat Transfer - History

Define Controls for Heat Transfer Analysis

Definition) Description This option allows you to input parameters governing the convergence solution and accuracy for heat transfer analysis. For transient heat transfer, the only data field required to be set is the maximum number of steps, the first field in the second data block. All other fields can, in these cases, be left blank, but notice that the third data block must be included. For coupled thermal-stress analysis, see CONTROL option for stress analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-7

1st

A

Enter the word CONTROL.

2nd data block

Main Index

1-5

1st

I

Maximum number of load steps in this run. Default is 99999. This is a cumulative number and is usually used to stop the run when RESTART is being used.

6-10

2nd

I

Maximum number of recycles during an increment due to temperature dependent material properties. Default value is 3.

11-15

3rd

I

Minimum number of recycles during an increment. Note that this data field forces this number of recycles to take place in all subsequent increments.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-35

7th

I

Nonpositive definite flag. If set to 1, solution of nonpositive definite system is forced.

36-40

8th

I

Not used; enter 0.

41-45

9th

I

Not used; enter 0.

46-50

10th

I

Not used; enter 0.

51-55

11th

I

Not used; enter 0.

56-60

12th

I

Assembly flag. If set to 1, the conductivity matrix is assembled each iteration.

1638 CONTROL (Heat Transfer - History Definition) Define Controls for Heat Transfer Analysis

Format Fixed

Free

Data Entry Entry

3rd data block

Main Index

1-10

1st

F

Maximum nodal temperature change allowed. Used to control automatic time step scheme for heat transfer. Default value of 20.

11-20

2nd

F

Maximum nodal temperature change allowed before properties are reevaluated and matrices reassembled. Default value of 100.

21-30

3rd

F

Maximum error in temperature estimate used for property evaluation. This control provides a recycling capability to improve accuracy in highly nonlinear heat-transfer problems (for example, latent heat, radiation boundary conditions). Default is 0, which bypasses this test. Set to maximum temperature error which is considered acceptable.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Maximum change of xsi,p allowed in pyrolysis calculation. Used to control automatic time step scheme.

51-60

6th

F

Maximum change of xsi,v allowed in pyrolysis calculation. Used to control automatic time step scheme.

61-70

7th

F

Maximum change of xsi,c allowed in pyrolysis calculation. Used to control automatic time step scheme.

71-80

8th

F

Maximum change in surface displacement per time step due to recession. This is used to control the time step for the TRANSIENT option.

TEMP CHANGE 1639 Specify or Change Fixed Temperatures

TEMP CHANGE

Specify or Change Fixed Temperatures

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new fixed temperature to be specified or old fixed temperatures to be changed. The exact numbering sequence of the fixed temperatures is used in some applications of this option. This numbering sequence is output after the fixed temperature option is used in the input data describing the problem. This option is used to change fixed temperatures in heat transfer. Note that enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Complex temperature histories are more conveniently input by the FORCDT user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words TEMP CHANGE.

I

Set to the number of fixed temperatures to be changed or added.

2nd data block 1-5

1st

A negative number removes fixed temperatures from the end of the fixed temperature list. A zero activates the FIXED TEMPERATURE option; a complete set of necessary fixed temperatures are then read, using the data blocks for that option except for that key word block.

Main Index

1640 TEMP CHANGE Specify or Change Fixed Temperatures

Format Fixed

Free

Data Entry Entry

3rd data block Data block 3 is only entered if columns 1 through 5 in data block 2 are a positive number and then has the number of data lines required by data block 2. 1-5

1st

I

Number of the boundary condition being changed. This number is derived from the “Fixed Boundary Condition Summary” table in the input echo of a Marc run. Boundary conditions being added should be given labels which increment the total count of boundary conditions properly. Note that a boundary condition in the middle of the list can be removed by specifying that labeled boundary condition as a repeat of some other boundary condition.

Main Index

6-10

2nd

I

Nodal point to be constrained.

11-15

3rd

I

Degree of freedom to be constrained.

FILMS (History Definition) 1641 Define Film Coefficients and Sink Temperatures

FILMS (History Definition)

Define Film Coefficients and Sink Temperatures

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows film coefficients and associated sink temperatures to be input. Nonuniform films or sink temperatures can be obtained via the FILM user subroutine, see Marc Volume D: User Subroutines and Special Routines. Format Format Fixed

Free

Data Entry Entry

1st data block 1-5

1st

A

Enter the word FILMS.

2nd data block 1-5

1st

I

Number of sets of data used to input film (optional).

6-10

2nd

I

Unit number for input of film data, defaults to input.

3rd data block 1-5

1st

I

Face identification. Same as for the FLUX user subroutine – see Marc Volume B: Element Library.

6-15

2nd

F

Reference value of film coefficient.

16-25

3rd

F

Reference value of sink temperature (reference values can be modified by the FILM user subroutine).

26-30

4th

I

Film coefficient index (optional).

31-35

5th

I

Sink temperature index (optional). (Film coefficient and sink temperature indices are to be used in the FILM user subroutine).

4th data block Enter a list of elements to which the above film data is applied.

Main Index

1642 VELOCITY CHANGE Modify Nodal Velocity Components

VELOCITY CHANGE

Modify Nodal Velocity Components

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows the specification of the nodal velocity components in a heat transfer analysis, where the convective terms are to be included. The convective option is specified by placing a 2 in the fifth field of the HEAT parameter. This activates the nonsymmetric solver as well. The nodal velocity components are defined by specifying the velocity magnitude of a series of components for sets of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the velocity values can be respecified or initialized if no previous data was entered via the UVELOC user subroutine. See Marc Volume D: User Subroutines and Special Routines. A summary of nodal velocities appears in the printout. This can be suppressed by specifying a nonzero value for the print-suppress parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word VELOCITY CHANGE.

2nd data block 1-5

1st

I

Number of sets of data lines used to input nodal velocity components. If a negative value is entered, the UVELOC user subroutine is called for every node.

6-10

2nd

I

Enter the unit number for input of the velocity field. Default to unit 5, unless the INPUT TAPE parameter has been used.

11-15

3rd

I

Set to 1 to suppress printout of the summary of nodal velocity components.

Data blocks 3, 4, and 5 should be repeated for each data set. 3rd data block 1-10

Main Index

1st

F

Enter the magnitude of the velocity in the first coordinate-direction for which the velocity is to be given.

VELOCITY CHANGE 1643 Modify Nodal Velocity Components

Format Fixed

Free

Data Entry Entry Additional velocity components in other coordinate directions must be specified on the same data line in F10 format. The number of components must equal the number of directions.

4th data block Enter a list of coordinate directions in which the velocity is specified. Note:

List verbs EXCEPT and INTERSECT are illegal here.

5th data block Enter a list of nodes for which the velocity vector, as defined in data blocks 3 and 4, is applied.

Main Index

1644

Main Index

Chapter 4 History Definition Options 1645 Joule Heating Analysis

Chapt Joule Heating Analysis This section describes the input of data necessary for a Joule heating analysis. All of the options in the er 4 subsections referring to heat transfer are also applicable. Both the applied currents and the nodal Histor previous voltages can be specified in this section. In Joule heating analysis, these are total values. y Defini tion Optio ns

Main Index

1646 EMRESIS Select Conducting Bodies to be used in a Resistance Calculation

EMRESIS

Select Conducting Bodies to be used in a Resistance Calculation

Description The purpose of this option is to define a group of conductors that will be used in a resistance calculation. This option is to be used only in conjunction with the THERMAL CONTACT model definition option. You can select all conductor bodies or a sub-set of these bodies for resistance computation. This option may only be used in a Joule Heating analysis. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word EMRESIS.

2nd data block 1-5

1st

I

Enter 0; not used.

3rd data block Enter a list of body IDs.

Main Index

DIST CURRENT (Joule Heating - History Definition) 1647 Define Distributed Current

DIST CURRENT (Joule Heating - History Definition)

Define Distributed Current

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows distributed (surface and volumetric) current to be specified. Distributed current is converted to a consistent nodal current by Marc. Note that for a given element type, there is an established convention for the application of surface current of a particular face. The FLUX user subroutine can be used to input time and spatial dependent current. In the current releases, Joule heating is not available for shell elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd and 4th data blocks are entered in pairs, once for each data block. 3rd data block 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed current.

4th data block Enter a list of elements associated with the above distributed current.

Main Index

1648 POINT CURRENT (Joule - History Definition) Define Nodal Point Current

POINT CURRENT (Joule - History Definition)

Define Nodal Point Current

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows total nodal point current to be specified. The FORCDT user subroutine can be used for the time dependent current. If the number of nodes which have point currents has been changed from the model definition option, you must give an upper bound on the DIST LOADS parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

A

Enter the words POINT CURRENT.

1-5

I

Enter the number of sets of point currents to be entered (optional).

6-10

I

Enter unit number of input of point current data, defaults to input.

F

Magnitude of point current.

2nd data block

3rd data block 1-10 4th data block Enter a list of nodes to which the above nodal current are applied.

Main Index

VOLTAGE CHANGE 1649 Define or Change Voltage for Joule Heating Analysis

VOLTAGE CHANGE

Define or Change Voltage for Joule Heating Analysis

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new voltage conditions to be specified or old voltage conditions to be changed in a Joule heating analysis. The exact numbering sequence of the voltage conditions is used in some applications of this option. This numbering sequence is output after the voltage conditions governing increment zero are read by Marc. This option is used for Joule heating analysis. Enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Complex time dependent voltage histories are more conveniently input by the FORCDT user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words VOLTAGE CHANGE.

I

Set to the number of specified voltage conditions to be changed or added.

2nd data block 1-5

1st

A negative number removes voltage conditions from the end of the voltage condition list. A zero activates the voltage option; a complete set of voltages are then read, using the data blocks for that option as described in the model definition section, except for that key word block.

Main Index

1650 VOLTAGE CHANGE Define or Change Voltage for Joule Heating Analysis

Format Fixed

Free

Data Entry Entry

3rd data block Data block 3 is only entered if the first field in data block 2 is a positive number determining the number of blocks required in this series. 1-5

1st

I

Number of the boundary condition being changed. This number is derived from the “Fixed Voltage Condition Summary” table in the input echo of a Marc run. Voltage conditions being added should be given labels which increment the total count of voltage conditions properly. A voltage condition in the middle of the list can be removed by specifying that labeled boundary condition as a repeat of some other boundary condition.

Main Index

6-10

2nd

I

Nodal point to be constrained.

11-15

3rd

I

Set to 1.

16-30

4th

F

Specified voltage.

Chapter 4 History Definition Options 1651 Diffusion Analysis

Chapt Diffusion Analysis This section describes the input of data necessary for a transient diffusion simulation with changing er 4 Histor boundary conditions or porosity. y Defini tion Optio ns

Main Index

1652 POROSITY CHANGE Define Changes in Porosity for Nonsoil Analysis

POROSITY CHANGE

Define Changes in Porosity for Nonsoil Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option.

Description This option provides the ability to change the porosity in nonsoil model. You can either specify the porosity or use the VOID CHANGE option to specify the void ratio. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words POROSITY CHANGE.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the porosity.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the porosity.

I

Enter the table id associated with the porosity.

4th data block 1-10

1st

5th data block 1-5

1st

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field.

Main Index

POROSITY CHANGE 1653 Define Changes in Porosity for Nonsoil Analysis

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above porosity is applied. the geometric entities must all be of the type prescribed in the 6th data block.

1654 VOID CHANGE Define Changes in Void Ratio for Nonsoil Analysis

VOID CHANGE

Define Changes in Void Ratio for Nonsoil Analysis

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This option provides the ability to change the void ratio in a nonsoil analysis model. You can either specify the void ratio or use the POROSITY CHANGE option to specify the porosity. Format Format Fixed

Free

Data Entry Entry

1st data block 1-13

1st

A

Enter the words VOID CHANGE.

2nd data block 1-5

1st

I

Enter the number of sets of data required to define the void ratio.

6-10

2nd

I

Enter the unit number; defaults to input.

The number of sets is equal to the number given in the first field above. The 3rd through 7th data blocks are entered as pairs. 3rd data block 1-5

1st

I

Enter the number of geometry types used to define this initial condition, default is 1. See the 6th and 7th data blocks.

6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this initial condition. This label will be referenced by the LOADCASE option.

F

Enter the magnitude of the void ratio.

I

Enter the table id associated with the void ratio.

4th data block 1-10

1st

5th data block 1-5

1st

The 6th and 7th data blocks are repeated for as many geometry types as specified in the 3rd data block, 1st field.

Main Index

VOID CHANGE 1655 Define Changes in Void Ratio for Nonsoil Analysis

Format Fixed

Free

Data Entry Entry

6th data block 1-5

1st

I

Enter the geometry type: 1 – Elements IDs 3 – Volume/Region/Body IDs

7th data block 1-80

Main Index

Enter a list of geometric entities to which the above void ratio is applied. the geometric entities must all be of the type prescribed in the 6th data block.

1656 DIST MASS (Diffusion) Define Distributed Mass Flux

DIST MASS (Diffusion)

Define Distributed Mass Flux

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This block of data defines mass flux (surface and volumetric) type boundary conditions. The user defines a surface distribute mass flux magnitude ( M ⁄ l 2 t ) and the location, and associates this with a boundary condition name. This is activated or deactivated using the LOADCASE history definition option. The FLUX user subroutine can be used for nonuniform, time-dependent distributed mass fluxes or the TABLE model definition option may be used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST MASS.

2nd data block 1-5

1st

I

Enter the number of sets of distributed mass fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed mass fluxes data, defaults to input.

Data blocks 3 through 9 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 9th and 10th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FLUX user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Enter 1 to exclude applied load when the edge (2-D) or face (3-D) is fully in contact.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label is referenced by the LOADCASE option.

DIST MASS (Diffusion) 1657 Define Distributed Mass Flux

Format Fixed

Free

Data Entry Entry

If a real distributed load is to be defined, data blocks 3 and 4 are used. 4th data block 1-10

1st

F

Enter the magnitude of mass flux.

I

Enter the table ID associated with the mass flux.

5th data block 1-5

1st

6th data block If geometry type is element IDs (1) use either the first field or the second and third field. If geometry type is volume (3), surface (4), or curve (5) use the second field only. 1-5

1st

I

Enter the distributed load type based upon element library description in Marc Volume B, Element Library.

6-10

2nd

I

Enter the distributed load type based upon: 1:

Normal

106: Uniform volumetric 107: Nonuniform volumetric 11-15

3rd

I

Enter the face ID.

Data blocks 7 and 8 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 7th data block 1-5

1st

I

Enter the geometry type: 1: Element IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 9: Polycurve IDs 10: Polysurface IDs 11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 16: Surface ID: orientation ID

Main Index

1658 DIST MASS (Diffusion) Define Distributed Mass Flux

Format Fixed

Free

Data Entry Entry 17: Curve ID: orientation ID 18: Surface ID: orientation ID - Marc Mentat convention 19: Curve ID: orientation ID - Marc Mentat convention

8th data block 1-80

Main Index

Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 7th data block.

POINT MASS (Diffusion) 1659 Define Nodal Mass Flux

POINT MASS (Diffusion)

Define Nodal Mass Flux

The information provided here is based upon table driven input. See the TABLE parameter to activate this input option. Description This block of data defines nodal mass flux boundary condition. The user specifies a magnitude and location, and associates this with a boundary condition name. This is activated or deactivated using the LOADCASE history definition option. The FORCDT user subroutine or the TABLE model definition option can be used to enter nonuniform time or frequency dependent boundary conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT MASS.

2nd data block 1-5

1st

I

Enter number of sets of point mass fluxes to be entered (optional).

6-10

2nd

I

Enter unit number for input of point mass flux data, defaults to input.

Data blocks 3 through 7 are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Enter the number of geometric types used to define boundary condition, default is 1. See 8th and 9th data blocks.

6-10

2nd

I

Enter 0 if no user subroutine required. Enter 1 if the FORCDT user subroutine is required for this boundary condition.

Main Index

11-15

3rd

I

Not used; enter 0.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Not used; enter 0.

26-30

6th

I

Not used; enter 0.

31-63

7th

A

Enter the unique label associated with this boundary condition. This label will be referenced by the LOADCASE option.

1660 POINT MASS (Diffusion) Define Nodal Mass Flux

Format Fixed

Free

Data Entry Entry

4th data block Magnitude. 1-10

1st

F

Point mass flux associated with first degree of freedom.

11-20

2nd

F

Point mass flux associated with second degree of freedom.

21-30

3rd

F

Point mass flux associated with third degree of freedom.

5th data block - Table ID for Magnitude 1-5

1st

I

Table ID associated with the first degree of freedom.

6-10

2nd

I

Table ID associated with the second degree of freedom.

11-15

3rd

I

Table ID associated with the third degree of freedom.

Data blocks 6 and 7 are repeated in pairs for as many geometry types as specified in the 3rd data block, 1st field. 6th data block 1-5

1st

I

Enter the geometry type: 1:

Element IDs 2: Nodes IDs 3: Volume/Region/Body IDs 4: Surface IDs 5: Curve IDs 6: Point IDs

11: Element-Edges IDs 12: Element-Faces IDs 13: Element-Edges IDs - Marc Mentat convention 14: Element-Faces IDs - Marc Mentat convention 7th data block Enter a list of geometric entities to which the above boundary conditions are applied. The geometric entities must all be of the type prescribed in the 6th data block.

Main Index

Chapter 4 History Definition Options 1661 Hydrodynamic Bearing Analysis

Chapt Hydrodynamic Bearing Analysis The purpose of bearing analysis history definition options are mainly to activate the calculation of er 4 bearing characteristics like damping and stiffness coefficients for a particular film profile. In addition, it Histor is possible to solve the lubrication problem for a new film profile. The history definition options used are: y • THICKNS CHANGE to specify a variation of the thickness field. Defini • DAMPING COMPONENTS to activate the calculation of damping coefficients based on the defined thickness change. tion • STIFFNS COMPONENTS to activate the calculation of stiffness coefficients based on the Optio defined thickness change. ns The calculation of damping and stiffness properties is performed within subincrements. If only the THICKNS CHANGE option is activated within an increment, the defined thickness change is added to the current film profile. The lubrication problem is then solved for the current film thickness.

Main Index

1662 THICKNS CHANGE Define Thickness Variations

THICKNS CHANGE

Define Thickness Variations

Description This option defines the thickness variations of the lubricant film in a bearing analysis. The nodal thickness changes are specified by giving the thickness increments for a list of nodes. This data can be input from data blocks or from an auxiliary input device. Moreover, the nodal thickness changes can be respecified or initialized, in case no previous data was input, via the UTHICK user subroutine. See Marc Volume D: User Subroutines and Special Routines. A summary of nodal thickness changes appears in the printout. This can be suppressed by specifying a nonzero value for the print-suppress parameter. The THICKNS CHANGE option enables the solution of the lubrication problems for a modified film profile. The defined thickness variation is added to the previously defined film profile. In case this option is combined with either the DAMPING COMPONENTS or STIFFNS COMPONENTS option, no updating is performed and damping or stiffness components are calculated within a subincrement based on the specified thickness variation. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word THICKNS CHANGE.

I

Number of sets of data lines used to input nodal thickness changes.

2nd data block 1-5

1st

If a negative value is entered, the UTHICK user subroutine is called for every node. 6-10

2nd

I

Enter the file number for input of film thickness variations. Default to unit 5, unless the INPUT TAPE parameter has been used.

11-15

3rd

I

Set to 1 to suppress printout of the summary of nodal thickness increments.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-10

1st

F

Enter nodal thickness increment.

4th data block Enter a list of nodes for which the nodal thickness variation as specified in data block 3 applied.

Main Index

DAMPING COMPONENTS 1663 Define Damping Coefficients

DAMPING COMPONENTS

Define Damping Coefficients

Description This option activates the calculation of damping coefficients for bearing analysis. Based on the thickness variation specified in the THICKNS CHANGE option, an incremental pressure distribution due to the thickness variation per unit time is calculated for the current bearing configuration within a subincrement. The resulting bearing force represents the damping properties pertaining to the specified rate of thickness change for the current film profile. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the words DAMPING COMPONENTS.

1664 STIFFNS COMPONENTS Define Stiffness Coefficients

STIFFNS COMPONENTS

Define Stiffness Coefficients

Description This option activates the calculation of stiffness coefficients for bearing analysis. Based on the thickness variation specified in the THICKNS CHANGE option, an incremental pressure distribution due to the thickness variation is calculated for the current bearing configuration within a subincrement. The resulting bearing force represents the stiffness properties pertaining to the specified thickness change for the current film profile. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word STIFFNS COMPONENTS.

Chapter 4 History Definition Options 1665 Acoustic Analysis

Chapt Acoustic Analysis This section describes options for the control of an acoustic analysis in a cavity with rigid boundaries. In er 4 an acoustic analysis, you would first extract the eigenmodes of the cavity using the MODAL SHAPE Histor option. The time step during the transient option would be controlled by the DYNAMIC CHANGE option. These two options are previously discussed in this chapter. The DIST SOURCES, POINT SOURCE, and y PRESS CHANGE options are available to specify the data to allow Marc to calculate the fundamental Defini frequencies of the cavity as well as the pressure distribution in the cavity. Incremental load information is provided here. tion Optio ns

Main Index

1666 PRESS CHANGE Define Fixed Pressures

PRESS CHANGE

Define Fixed Pressures

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new fixed pressures to be specified or old fixed pressures to be changed. The exact numbering sequence of the fixed pressures is used in some applications of this option. This numbering sequence is output after the fixed pressure option is used in the input data describing the problem. This option is used to change fixed pressures in acoustic transfer. Enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Complex pressure histories are more conveniently input by the FORCDT user subroutine. Format Format Fixed

Free

Data Entry Entry

1st data block 1-15

1st

A

Enter the words PRESS CHANGE.

I

Set to the number of fixed pressure to be changed or added.

2nd data block 1-5

1st

A negative number removes fixed pressures from the end of the fixed pressure list. A zero activates the FIXED PRESSURE option; a complete set of necessary fixed pressures are then read, using the blocks for that option except for that key word block. 3rd data block Data block 3 is only entered if columns 1 through 5 in data block 2 is a positive number and then has the number of data lines required by data block 2. 1-5

Main Index

1st

I

Number of the boundary condition being changed. This number is derived from the “Fixed Boundary Condition Summary” table in the input echo of a Marc run. Boundary conditions being added should be given labels which increment the total count of boundary conditions properly.

PRESS CHANGE 1667 Define Fixed Pressures

Format Fixed

Free

Data Entry Entry A boundary condition in the middle of the list can be removed by specifying that labeled boundary condition as a repeat of some other boundary condition.

Main Index

6-10

2nd

I

Nodal point to be constrained.

11-15

3rd

I

Degree of freedom to be constrained.

16-30

4th

F

Specified pressure.

1668 DIST SOURCES (History Definition) Define Incremental Distributed Sources

DIST SOURCES (History Definition)

Define Incremental Distributed Sources

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows incrementally distributed (surface and volumetric) sources to be specified in an acoustic analysis. Distributed sources are converted to consistent nodal sources by Marc. Note that for a given element type, there is an established convention for the application of surface source on a particular face. The FLUX user subroutine can be used to input time and spatial dependent fluxes. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST SOURC.

11-15

2nd

I

Enter 1 if distributed source is to be applied as excitation load in a harmonic analysis.

2nd data block 1-5

1st

I

Enter the number of sets of distributed sources to be entered (optional).

6-10

2nd

I

Enter file number for input of distributed source data. Defaults to input.

The following 3rd and 4th data blocks are given as pairs; once for each data set. 3rd data block 1-5

1st

I

Parameter identifying the type of load. See library element description in Marc Volume B: Element Library.

6-15

2nd

E

Enter the magnitude of this type of distributed sources.

16-20

3rd

I

Source index (optional). Source index is to be used in the FLUX user subroutine.

4th data block Enter a list of elements associated with the above distributed sources.

Main Index

POINT SOURCE (Acoustic - History Definition) 1669 Define Incremental Nodal Point Sources

POINT SOURCE (Acoustic - History Definition)

Define Incremental Nodal Point Sources

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows incremental nodal point sources to be specified in an acoustic analysis. The FORCDT user subroutine can be used for the time dependent sources. If the number of nodes which have point source has been changed from the model definition option, you must give an upper bound on the DIST LOADS parameter. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT SOUR.

11-15

2nd

I

Enter 1 to enter real harmonic load. Enter 2 to enter imaginary harmonic load.

2nd data block 1-5

1st

I

Enter the number of sets of point sources to be entered (optional).

6-10

2nd

I

Enter file number for input of point source data. Defaults to input.

The following 3rd and 4th data blocks are given in pairs, once for each data set. 3rd data block 1-10

1st

F

Magnitude of incremental point source.

11-20

2nd

F

Magnitude of point source for second degree of freedom, (heat transfer shell elements only).

21-30

3rd

F

Magnitude of point source for third degree of freedom, (heat transfer shell elements only).

4th data block Enter a list of nodes to which the above nodal sources are applied.

Main Index

1670 HARMONIC (Acoustic - History Definition) Define Excitation Frequency

HARMONIC (Acoustic - History Definition)

Define Excitation Frequency

Description This option is necessary to specify the frequency of excitation implemented. The option is used in dynamic harmonic, acoustic, and piezoelectric analyses. Note:

This history definition option cannot be used in modal or transient acoustic analysis.

Format

1st data block 1-10

1st

A

Enter the word HARMONIC.

2nd data block 1-10

1st

F

Enter the lowest frequency in cycles per time unit.

11-20

2nd

F

Enter the increment in frequency for each subincrement. If zero, only single frequency is used.

21-30

3rd

F

Enter the highest frequency in cycles per time unit.

31-35

4th

I

Enter 0 for linear increments in frequency (default). Enter 1 for logarithmic increments in frequency.

36-40

5th

I

Enter the number of frequencies (n) if linear intervals, then if n = ( ω HIGH – ω L OW ) ⁄ ( Δ ω ) Δ ω i = entered value of ( ω HI GH – ω L OW ) ⁄ n – 1

If logarithmic increments in frequency ω HIGH f ac = ⎛ ----------------⎞ ⎝ ω LOW ⎠

(1 ⁄ n – 1)

Δ ω i = f ac ** ( i – 1 )

Main Index

n = 0;

Chapter 4 History Definition Options 1671 Electrostatic Analysis

Chapt Electrostatic Analysis In an electrostatic analysis, the boundary conditions are charges given in the POINT CHARGE and DIST er 4 CHARGES option, and the potential given in the FIXED POTENTIAL option. The history definition Histor consists of the STEADY STATE option and the CONTINUE option which initiates the analysis. The analysis is linear, so no iterations occur. y Defini For a coupled electrostatic structural analysis a static or a dynamic transient analysis type are possible. For the static analysis the application of the mechanical boundary conditions, and how to specify tion automatic multi-increment load control is similar to what was described in the subsection Static, Optio Dynamic, Creep Analysis. Options which are used to control the dynamic transient analysis are described in the subsection Dynamic Analysis. For nontable driven input, the electrostatic boundary ns conditions are charges given in the POINT CHARGE and DIST CHARGE option, and the potential given in the POTENTIAL CHANGE option. Incremental values are required for coupled electrostatic structural analyses.

Main Index

1672 STEADY STATE (Electrostatic) Specify Steady-State Electrostatic Analysis

STEADY STATE (Electrostatic)

Specify Steady-State Electrostatic Analysis

Description This option allows the solution of the steady-state electrostatic problem. Marc begins execution of the step when a CONTINUE option is encountered. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words STEADY STATE.

EMCAPAC 1673 Select Conducting Bodies to be used in a Capacitance Calculation

EMCAPAC

Select Conducting Bodies to be used in a Capacitance Calculation

Description The purpose of this option is to select a group of conductors that will be used in a capacitance calculation in this increment. This option is to be used only in conjunction with the THERMAL CONTACT model definition option. You can select all conductor bodies or a subset of these bodies for capacitance computation. The chosen conductor bodies are used for the capacitance matrix calculation in Marc. This option may only be used with electrostatic analysis. No two conductors should touch each other. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word EMCAPAC.

2nd data block 1-5

1st

I

Enter 0; not used.

6-10

2 nd

I

Enter the increment frequency at which the capaciatnce calculation should be done. Default is 1.

3rd data block Enter a list of body IDs.

Main Index

1674 EMCAPAC Piezoelectric Analysis

Chapt Piezoelectric Analysis This section describes options used to control a piezoelectric analysis. Possible analysis types are static, er 4 modal, dynamic transient, and dynamic harmonic. For static analysis the application of the Histor dynamic mechanical boundary conditions, and how to specify automatic multi-increment load control is similar to what was described in the subsection Static, Dynamic, Creep Analysis. Options which are used to y control the dynamic modal, dynamic transient, or dynamic harmonic analysis are described in the Defini subsection Dynamic Analysis. The electrical boundary conditions are charges given in the POINT CHARGE and DIST CHARGE option, and the potential given in the POTENTIAL CHANGE option. tion Optio ns

Main Index

POTENTIAL CHANGE (Piezoelectric - History Definition) 1675 Define Potential Boundary Conditions

POTENTIAL CHANGE (Piezoelectric History Definition)

Define Potential Boundary Conditions

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new potential boundary conditions to be specified or old potential boundary conditions to be changed. The change in potential is incremental. Care should be taken, when removing fixed potential conditions, to ensure that the reaction forces are handled properly. Note that enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Time dependent potentials are more conveniently input by the FORCDT user subroutine. When used in conjunction with harmonic analysis, this boundary change is used for all excitation frequencies until a new boundary change is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POTENTIAL CHANGE.

2nd data block 1-5

1st

I

Enter 0. This activates the FIXED POTENTIAL option; a complete set of necessary fixed potential boundary conditions are then read, replacing the existing fixed potential boundary conditions.

6-10

2nd

I

Enter 1 if excitation boundary conditions for harmonic analysis.

11-15

3th

I

Enter 1 if harmonic boundary condition is input as magnitude and phase. If blank, real and imaginary values are given.

I

Number of the boundary condition blocks to be read (optional).

3rd data block 1-5

1st

Data blocks 4a and 5a are for analyses which do not include shell elements.

Main Index

1676 POTENTIAL CHANGE (Piezoelectric - History Definition) Define Potential Boundary Conditions

Format Fixed

Free

Data Entry Entry

4a data block 1-10

1st

F

Prescribed potential or amplitude or real part of potential for harmonic analysis.

11-20

2nd

F

Phase or imaginary part of potential for harmonic analysis.

5a data block Enter a list of nodes for which the above boundary conditions are applied. Data blocks 4b, 5b, and 6b are for analyses which include shell elements. 4b data block 1-10

1st

F

Prescribed potential, or amplitude or real part of potential for harmonic analysis.

11-20

2nd

F

Enter 0.

21-30

3rd

F

Phase or imaginary part of potential for harmonic analysis. Note:

Currently, there are no piezoelectric shell elements, but it is possible to use mechanical shell elements in a piezoelectric analysis.

5b data block 1-5

1st

I

Enter 1.

6b data block Enter a list of nodes for which the above potential change conditions are applied.

Main Index

POINT CHARGE (Piezoelectric - History Definition) 1677 Define Nodal Point Charges

POINT CHARGE (Piezoelectric - History Definition)

Define Nodal Point Charges

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows nodal point charges to be specified. The FORCDT user subroutine can be used for nonuniform loading conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CHARGE.

11-15

2nd

I

Enter 1 to enter real harmonic charge. Enter 2 to enter imaginary harmonic charge.

2nd data block 1-5

1st

I

Enter the number of sets of point charge to be entered (optional).

6-10

2nd

I

Enter file number for input of point charge data; defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-10

1st

F

Magnitude of point charge.

4th data block Enter a list of nodes to which the above nodal charges are applied.

Main Index

1678 DIST CHARGE (Piezoelectric - History Definition) Define Distributed Charges

DIST CHARGE (Piezoelectric - History Definition) Define Distributed Charges The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. For a given element type, there is an established convention for the application of surface charge of a particular face. The FLUX user subroutine can be used to input spatially dependent charge. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGES.

11-15

2nd

I

Enter 1 if distributed charge is to be applied as excitation load in a harmonic analysis.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter file number for input of distributed charge data; defaults to input.

The 3rd and 4th data blocks are given in pairs; once for each data set. 3a data block 1-5

1st

I

Parameter identifying the type of distributed charge. See description of library element in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed charges.

16-20

3rd

I

Charge index. Charge index is to be used in the FLUX user subroutine.

3b data block Use if harmonic analysis.

Main Index

1-5

1st

I

Parameter identifying the type of charge. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the real component of this type of distributed charge.

DIST CHARGE (Piezoelectric - History Definition) 1679 Define Distributed Charges

Format Fixed

Free

Data Entry Entry

16-25

3rd

F

Enter the imaginary component of this type of distributed charge.

25-30

4th

I

Charge index. Charge index is to be used in the FLUX user subroutine.

4th data block Enter a list of elements associated with the above distributed charges.

Main Index

1680 DIST CHARGE (Piezoelectric - History Definition) Magnetostatic Analysis

Chapt Magnetostatic Analysis In a magnetostatic, the boundary conditions are currents given to the POINT CURRENT and DIST er 4 options and the potential given in the FIXED POTENTIAL option. The history definition Histor CURRENT consists of the STEADY STATE and the CONTINUE options which initiate the analysis. If a nonlinear material is present, defined through the B-H RELATION option, iteration is required as specified in the y CONTROL option; otherwise, no iterations occur. Defini tion Optio ns

Main Index

STEADY STATE (Magnetostatic) 1681 Specify Steady-State Magnetostatic Analysis

STEADY STATE (Magnetostatic)

Specify Steady-State Magnetostatic Analysis

Description This option allows the solution of the steady-state magnetostatic problem. If nonlinear magnetic properties are included, the recycling tolerance for property evaluation must be used so that iteration is performed. Marc begins execution of the step when a CONTINUE option is encountered. Format Format Fixed 1-10

Main Index

Free

Data Entry

1st

A

Enter the words STEADY STATE.

1682 DIST CURRENT (Magnetostatic) Define Distributed Current

DIST CURRENT (Magnetostatic)

Define Distributed Current

The information provided here is based upon not using the table driven input style. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. Note that for a given element type, there is an established convention for the application of surface current of a particular face. The FLUX user subroutine for 2-D and the FORCEM user subroutine for 3-D can be used to input spatially dependent current. Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words DIST CURRENT.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter unit number for input of distributed current data, defaults to input.

The 3rd and 4th data blocks are entered as pairs, one for each data set. 3rd data block 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element LIbrary.

6-15

2nd

E

Enter the magnitude of this type of distributed current.

16-20

3rd

I

Current index (current index is to be used in the FLUX for 2-D and FORCEM for 3-D user subroutine).

3b data block The following block is only used if the parameter identifying the type of current is 106 or 107.

Main Index

1-5

1st

I

Parameter identifying the type of current (106 or 107). See library element description in Marc Volume B: Element LIbrary.

6-15

2nd

E

Enter the magnitude of this type of distributed current in the first coordinate direction.

16-25

3rd

E

Enter the magnitude of this type of distributed current in the second coordinate direction.

DIST CURRENT (Magnetostatic) 1683 Define Distributed Current

Format Fixed

Free

Data Entry Entry

26-35

4th

E

Enter the magnitude of this type of distributed current in the third coordinate direction.

36-40

3rd

I

Current index (current index is to be used in the FORCEM user subroutine).

4th data block Enter a list of elements associated with the above distributed current.

Main Index

1684 DIST CURRENT (Magnetostatic) Electromagnetic Analysis

Chapt Electromagnetic Analysis This section describes options used to control both transient and harmonic electromagnetic analysis. The er 4 DYNAMIC CHANGE option is used to specify the time step, while the HARMONIC option is used to Histor control the excitation frequency. Note that all loads are incremental in nature. y For a coupled electromagnetic thermal analysis a harmonic electromagnetic analysis is combined with a Defini thermal analysis. To activate this analysis chose the HARMONIC option to set the excitation frequency of the electromagnetic pass, and either STEADY STATE, TRANSIENT, or AUTO STEP, for the thermal pass. tion For the thermal boundary conditions like DIST FLUXES, POINT FLUX, TEMP CHANGE, and FILMS see Optio the Heat Transfer Analysis section. ns

Main Index

HARMONIC (Electromagnetic - History Definition) 1685 Define Excitation Frequency

HARMONIC (Electromagnetic - History Definition)

Define Excitation Frequency

Description This option is necessary to specify the frequency of excitation implemented. The option is used in dynamic harmonic, acoustic, and piezoelectric analyses. This can be used if the harmonic flag (1) has been set on the EL-MA parameter. For a coupled electromagnetic thermal analysis enter only one excitation frequency. Format

1st data block 1-10

1st

A

Enter the word HARMONIC.

2nd data block 1-10

1st

F

Enter the lowest frequency in cycles per time unit.

11-20

2nd

F

Enter the increment in frequency for each subincrement. If zero, only single frequency is used.

21-30

3rd

F

Enter the highest frequency in cycles per time unit.

31-35

4th

I

Enter 0 for linear increments in frequency (default). Enter 1 for logarithmic increments in frequency.

36-40

5th

I

Enter the number of frequencies (n) if linear intervals, then if n = ( ω HIGH – ω L OW ) ⁄ ( Δ ω ) Δ ω i = entered value of ( ω HI GH – ω L OW ) ⁄ n – 1

If logarithmic increments in frequency ω HIGH ( 1 ⁄ n – 1 ) f ac = ⎛ ----------------⎞ ⎝ ω LOW ⎠ Δ ω i = f ac ** ( i – 1 )

Main Index

n = 0;

1686 DYNAMIC CHANGE (Electromagnetic - History Definition) Define Dynamic Change

DYNAMIC CHANGE (Electromagnetic - History Definition)

Define Dynamic Change

Description This option specifies the parameters required for integration in time. This can be used if the transient flag (0) has been set on the EL-MA parameter. The Newmark-beta procedure with a fixed time step is used. Format Format Fixed

Free

Data Entry Entry

1st data block 1-14

1st

A

Enter the words DYNAMIC CHANGE.

2nd data block

Main Index

1-15

1st

F

Time step size.

16-30

2nd

F

Period of time for this set of boundary conditions.

31-35

3rd

I

Number of time steps in this set of boundary conditions.

36-40

4th

I

This field is not used.

41-45

5th

I

Reassembly interval for mass and stiffness matrices; for linear problems, set equal to value in the seventh field.

POTENTIAL CHANGE 1687 Define or Redefine Potential Boundary Conditions

POTENTIAL CHANGE

Define or Redefine Potential Boundary Conditions

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows new potential boundary conditions to be specified or old potential boundary conditions to be changed. The exact numbering sequence of the boundary conditions is used in some applications of this option. This numbering sequence is output after the boundary condition option is used in the input data describing the problem. This option is used for incrementation of fixed potential components or for adding or removing potential constraints. Care should be taken, when removing fixed potential conditions, to ensure that the reaction forces are handled properly. Note that enough space must be specified on the SIZING parameter in the maximum number of boundary condition fields to allow for possible increased storage requirements arising from use of this option. Time dependent potentials are more conveniently input by the FORCDT user subroutine. When used in conjunction with harmonic analysis, this boundary change is used for all excitation frequencies until a new boundary change is invoked. Format Format Fixed

Free

Data Entry Entry

1st data block 1-11

1st

A

Enter the words POTENTIAL CHANGE.

I

Set to the number of boundary conditions (specified potential components to be changed or added).

2nd data block 1-5

1st

A negative number removes boundary conditions from the end of the boundary condition list. A zero activates the FIXED POTENTIAL option; a complete set of necessary boundary conditions are then read, using the blocks for that option except for that key word block. 6-10

Main Index

2nd

I

Enter 1 if excitation boundary conditions for harmonic analysis.

1688 POTENTIAL CHANGE Define or Redefine Potential Boundary Conditions

Format Fixed 11-15

Free 3rd

Data Entry Entry I

Enter 1 if harmonic boundary condition is input as magnitude and phase. If blank, real and imaginary values are given.

3rd data block Data block 3 is only entered if the number in columns 1 through 5 in data block 2 is positive and then has the number of data lines required by data block 2. 1-5

1st

I

Number of the boundary condition being changed. This number is derived from the “Fixed Boundary Condition Summary” table in the input echo of a Marc run. Boundary conditions being added should be given labels which increment the total count of boundary conditions properly.

6-10

2nd

I

Nodal point to be constrained.

11-15

3rd

I

Degree of freedom to be constrained. Note that a boundary condition in the middle of the list can be removed by specifying that labeled boundary condition as a repeat of some other boundary condition.

Main Index

16-30

4th

F

Specified potential increment (real part).

31-45

5th

F

Specified potential increment (imaginary part).

POINT CURRENT (Electromagnetic - History Definition) 1689 Define Point Current and/or Charge

POINT CURRENT (Electromagnetic History Definition)

Define Point Current and/or Charge

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows nodal point currents and point charges to be specified. The FORCDT user subroutine can be used for nonuniform loading conditions. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words POINT CURRENT.

11-15

2nd

I

Enter 1 to enter real harmonic current and charge. Enter 2 to enter imaginary harmonic current and charge.

2nd data block 1-5

1st

I

Enter number of sets of point current and charge to be entered (optional).

6-10

2nd

I

Enter file number for input of point current and charge data. Defaults to input.

The following 3rd and 4th data blocks are entered as pairs; once for each data set. 3rd data block 1-10

1st

F

Magnitude of point current for first degree of freedom.

11-20

2nd

F

Magnitude of point current for second degree of freedom.

21-30

3rd

F

Magnitude of point current for third degree of freedom.

31-40

4th

F

Magnitude of point charge.

4th data block Enter a list of nodes to which the above point current-charge applies.

Main Index

1690 DIST CURRENT (Electromagnetic - History Definition) Define Distributed Current

DIST CURRENT (Electromagnetic - History Definition)

Define Distributed Current

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows distributed (surface and volumetric) currents to be specified. Distributed currents are converted to consistent nodal currents by Marc. For a given element type, there is an established convention for the application of surface current of a particular face. The FORCEM user subroutine can be used to input spatially dependent current. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CURRENT.

11-15

2nd

I

Enter 1 if distributed current is to be applied as excitation load in a harmonic analysis.

2nd data block 1-5

1st

I

Enter the number of sets of distributed currents to be entered (optional).

6-10

2nd

I

Enter file number for input of distributed current data. Defaults to input.

The following 3rd and 4th data blocks are given in pairs; once for each data set. 3a data block Use if not harmonic analysis.

Main Index

1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the magnitude of this type of distributed current.

16-20

3rd

I

Current index. Current index is to be used in the FORCEM user subroutine.

DIST CURRENT (Electromagnetic - History Definition) 1691 Define Distributed Current

Format Fixed

Free

Data Entry Entry

3b data block Use if harmonic analysis. 1-5

1st

I

Parameter identifying the type of current. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the real component of distributed current.

16-25

3rd

F

Enter the imaginary component of distributed current.

26-30

4th

I

Current index. Current index is to be used in the FLUX user subroutine.

4th data block Enter a list of elements associated with the above distributed current.

Main Index

1692 DIST CHARGE (Electromagnetic - History Definition) Define Distributed Charges

DIST CHARGE (Electromagnetic - History Definition)

Define Distributed Charges

The information provided here is based upon not using the table driven input style. When using the table driven input for boundary conditions, the variation with time or increment number should be specified in the table. If this boundary condition is applied as a harmonic excitation, it may be defined as a function of the frequency. The complete definition of the boundary condition can be specified in the model definition section. Description This option allows distributed (surface and volumetric) charges to be specified. Distributed charges are converted to consistent nodal charges by Marc. Note that for a given element type, there is an established convention for the application of surface charge on a particular face. The FORCEM user subroutine can be used to input spatially-dependent charges. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words DIST CHARGE.

11-15

2nd

I

Enter 1 if distributed charge is to be applied as excitation load in a harmonic analysis.

2nd data block 1-5

1st

I

Enter the number of sets of distributed charges to be entered (optional).

6-10

2nd

I

Enter file number for input of distributed charge data. Defaults to input.

The following 3rd and 4th data blocks are given as pairs; once for each data set. 3a data block Use if not harmonic analysis.

Main Index

1-5

1st

I

Parameter identifying the type of distributed charge. See description of library element in Marc Volume B: Element Library.

6-15

2nd

E

Enter the magnitude of this type of distributed charges.

16-20

3rd

I

Charge index (optional). Charge index is to be used in the FORCEM user subroutine.

DIST CHARGE (Electromagnetic - History Definition) 1693 Define Distributed Charges

Format Fixed

Free

Data Entry Entry

3b data block Use if harmonic analysis. 1-5

1st

I

Parameter identifying the type of charge. See library element description in Marc Volume B: Element Library.

6-15

2nd

F

Enter the real component of distributed charge.

16-25

3rd

F

Enter the imaginary component of distributed charge.

26-30

4th

I

Charge index. Charge index is to be used in the FORCEM user subroutine.

4th data block Enter a list of elements associated with the above distributed charge.

Main Index

1694 CONTINUE (History Definition) End Loadcase

CONTINUE (History Definition)

End Loadcase

Description The CONTINUE option is necessary to indicate that all data for this increment or series of increments has been read in. The analysis is then initiated. Format Format Fixed 1-8

Main Index

Free 1st

Data Entry Entry A

Enter the word CONTINUE.

Chapter 5 Rezoning Options List

5

Main Index

Rezoning Options List

Rezoning Options

Page

CONNECTIVITY CHANGE

1690

CONTACT CHANGE

1702

CONTINUE

1711

COORDINATE CHANGE

1699

END REZONE

1712

GAP DATA CHANGE

1697

GEOMETRY CHANGE

1691

MOVE

1701

ORIENTATION CHANGE

1695

PRINT CHOICE

1708

REZONE

1686

1696

Rezoning Options

Main Index

Page

SECTIONING

1688

SPLIT BODIES

1687

UFRORD

1700

URCONN

1710

Chapter 5 Rezoning Options Marc Volume C: Program Input

5

Rezoning Options

J

Main Index

Rezoning Options

1699

1698 Marc Volume C: Program Input

For the analysis of metal forming problems, Marc utilizes the updated Lagrange approach. In this approach, the state at the beginning of an increment serves as the reference state for the calculation of the incremental values. At each subsequent increment, the reference state is updated. This analysis method has several advantages, but it has a limit on the maximum deformation attainable. Due to the large deformations, the element mesh can degenerate strongly, and, in the updated approach, this means that the analysis of subsequent increments is carried out with a very poor mesh. This effect can even be so serious that elements locally turn inside out, which makes further analysis impossible. In order to continue the analysis with sufficient accuracy, it is necessary to use a new mesh. The state in the old mesh must be transferred to the new mesh. Such a transfer is, of course, only possible if the state in the old mesh is defined with respect to the current configuration. Hence, if you use the updated Lagrange approach, you might be required to rezone the mesh to successfully complete a given analysis. This process involves two steps, defining a new mesh or remeshing and transferring the results from the old mesh to the new mesh. This section defines the used-controlled process of creating a new mesh. As an alternative, the ADAPT GLOBAL option may be used. This procedure automatically creates a new mesh and is preferred because the meshing automatically occurs when necessary. When using the “manual” procedure discussed in this chapter, one increment is required to perform this definition of the new mesh using a complete set of input options, as defined in the following sections of this chapter. The rezoning capability is available for the following element types: • Continuum 2-D and 3-D displacement elements (except semi-infinite). • Shell elements 22 and 75. • Herrmann elements 80-84, 118-120, and 155-157 using techniques defined under the SECTIONING option. • Heat transfer continuum elements.

Main Index

Chapter 5 Rezoning Options 1699 Rezoning Options

Rezoning Options When you insert the REZONE option into a typical data setup of a problem, Marc is able to read a selection of the rezoning option format to control the rezoning steps. These rezoning option formats are described on the following pages. These options must follow immediately after a load incrementation CONTINUE option. If you do not want any rezoning steps, Marc reinterprets the input as load incrementation data. You can select as many rezoning steps in one increment as are needed. Every rezoning step is defined by the data starting with the REZONE option and ending with the CONTINUE option. The complete set of rezoning steps that form a complete rezoning increment is terminated by the END REZONE option. The rezoning input is followed by normal load incrementation data or again by rezoning data.

Main Index

1700 REZONE Specify Rezoning Input

REZONE

Specify Rezoning Input

Description This option starts the rezoning input and should be present in the rezoning input data. If this option is not encountered, no rezoning step is performed and the option read in is interpreted as a history definition option. This option must be repeated for every rezoning step; if the rezoning increment consists of more than one step, this option must be repeated. Format Format Fixed

Free

Data Entry Entry

1-6

1st

A

Enter the word REZONE.

11-15

2nd

I

Enter 1 if the total displacements in subsequent increments are to be printed with respect to the original configuration; otherwise, they are with respect to the updated coordinate position defined in this rezoning step. For the regions modeled using Mooney, Ogden, or powder materials, this should be set to 1.

Main Index

SPLIT BODIES 1701 Defines Rezoned Data of Contact Nodes

SPLIT BODIES

Defines Rezoned Data of Contact Nodes

Description This option is very useful in ensuring correct rezoning in bodies involved in deformable to deformable contact. In case of slight penetration of the contact node (allowed by the contact zone tolerance) of one body into another, the rezoned data of the contact nodes is correctly defined with this option. This option is currently available for 4-node quadrilateral in two-dimensional analysis and 8-node hexahedral in three-dimensional analysis. Note:

Main Index

This option must immediately follow the REZONE option and is necessary only in the increment with rezoning.

1702 SECTIONING (Rezoning) Define Sections for Rezoning

SECTIONING (Rezoning)

Define Sections for Rezoning

Description This option allows rezoning of parts of the mesh. Three input definitions are allowed for specifications of the mesh part to be rezoned. Only one of the following sectioning options can be used during a rezoning step definition. a. Selection by element numbers – a list of element numbers must be supplied. b. Selection by element type – the element type must be supplied. c. Selection by material type – the material type must be supplied. If Herrmann elements are to be used in a rubber rezoning, they should be selected using method B described above. Only Herrmann element types 80-84, 118-120, and 155-157 can be rezoned. Note:

Only one of the above sectioning options can be used during a rezoning step definition.

If the sectioning option is not used, the complete mesh is taken into account during the current rezoning step which can cause problems. If discontinuities in material type or element thickness are present, not all element variables are continuous across element boundaries. In that case, SECTIONING should be used to divide the regions. If continuum and shell elements are to be rezoned, two rezoning steps should be taken and the SECTIONING option used to separate the element types. Caution:

If an analysis has both Herrmann elements and displacement elements and a rezoning step is to be performed, it is necessary to have double nodes at the interface and to tie all the displacement degrees of freedom. See note on COORDINATE CHANGE option on definition of coordinate points

Note:

For an analysis with 2-D deformable to deformable contact, the SPLIT BODIES option must be used if rezoning is required for the contacting bodies.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

Main Index

1st

A

Enter the word SECTIONING.

SECTIONING (Rezoning) 1703 Define Sections for Rezoning

Format Fixed

Free

Data Entry Entry

2nd data block 1-5

1st

I

Enter the number of lists of elements to be given in data block 3. If either option B or C are used, enter 0.

6-10

2nd

I

If a particular element type is selected enter the element type number to be selected.

11-15

3rd

I

If a particular material type is selected enter the material type to be selected.

3rd data block The 3rd data block is repeated once for each list of elements. Enter a list of elements to be taken into account during this rezoning step.

Main Index

1704 CONNECTIVITY CHANGE Define or Change Connectivity

CONNECTIVITY CHANGE

Define or Change Connectivity

Description This option provides the possibility of changing the connectivity of a number of elements or to delete and/or add some elements. If elements are added, you must ensure that all the other element quantities (for example, GEOMETRY) are initialized for this element number in the model definition data and that the element number to be added is smaller than the maximum number of elements given on the SIZING parameter. If elements are deleted, you must enter element type 0 in this option. Caution:

If this option is used, the bandwidth of the system matrix might change and this makes a renewed calculation of the bandwidth necessary. This is automatically done by Marc.

Format

1st data block 1-19

1st

A

Enter the words CONNECTIVITY CHANGE.

2nd data block 1-5

1st

I

Enter the number of elements to be change with this option (optional).

6-10

2nd

I

Enter the file number for input of connectivity. Defaults to input.

11-15

3rd

I

Set to 1 to suppress printing of element connectivity list during this option.

3rd data block One data block per element. 1-5

1st

I

Element number.

6-10

2nd

I

Element type. Enter 0 if this element is to be deleted. In the latter case, no nodes have to be read in for this option.

11-15

3rd

I

First nodal point.

16-20

4th

I

Second nodal point.

etc.

Main Index

etc.

Repeat until all nodes for this element type are read in. Continuation, if necessary, is in format 16I5.

GEOMETRY CHANGE 1705 Specify New Geometry

GEOMETRY CHANGE

Specify New Geometry

Description This option can be used to specify the GEOMETRY model definition data for changed or added elements. Format Format Fixed

Free

Data Entry Entry

1st data block 1-8

1st

A

Enter the words GEOMETRY CHANGE.

2nd data block 1-5

1st

I

Number of distinct sets of element geometries to be input (optional).

6-10

2nd

I

Enter file number for input of geometry data. Defaults to input.

3rd data block Element geometries. The 3rd through 6th data blocks are entered as pairs, one for each distinct data set. 1-10

1st

F

EGEOM1

11-20

2nd

F

EGEOM2

21-30

3rd

F

EGEOM3

31-40

4th

F

EGEOM4

41-50

5th

F

EGEOM5

51-60

6th

F

EGEOM6

61-70

7th

F

EGEOM7

71-80

8th

F

EGEOM8 For beam and shells, EGEOM8 is the negative of the sum of three numbers = -(ioffset + iorien + ipin) ioffset

=

0 – no offsets 10 – offsets with beams; include the 5a data block 2 – offsets with shells; include the 5b data block

iorien

=

0 – conventional definition of local beam orientation, beam axis given in 4th through 6th field in global system 10 – the local beam orientation is given with respect to the coordinate system of the first beam node.

Main Index

1706 GEOMETRY CHANGE Specify New Geometry

Format Fixed

Free

Data Entry Entry ipin

=

0 – no pin codes are used

Note:

iorien and ipin are only valid for beam elements.

100 – pin codes are used; include the 4th data block See library element descriptions in “Quick Reference” of Marc Volume B: Element Library for the meaning of EGEOM1, etc. for each element type. 4th data block Necessary only if ipin = 100 1-5

1st

I

Enter the pin code associated with the first node of the beam.

6-10

2nd

I

Enter the pin code associated with the second node of the beam. The degrees of freedom are defined in the element’s coordinate system and the pin flags are applied at the offset ends of the beam. The pin code is a packed integer of up to five unique integers 1 through 6 with no embedded blanks.

5a data block Necessary only if ioffset = 1 1-10

1st

F

X component of offset vector at beam node 1

11-20

2nd

F

Y component of offset vector at beam node 1

21-30

3rd

F

Z component of offset vector at beam node 1

31-40

4th

F

X component of offset vector at beam node 2

41-50

5th

F

Y component of offset vector at beam node 2

51-60

6th

F

Z component of offset vector at beam node 2

61-65

7th

I

Interpolation flag for higher-order beams 0 – no interpolation of offset vector for midside node (Offset vector at midside node set to 0.). 1 – linear interpolation of offset vector for midside node

66-70

8th

I

Coordinate system flag for offset vector at beam node 1 0 – vector in global coordinate system 1 – vector in element coordinate system 2 – vector along associated shell normal at node 3 – vector in local coordinate system at node 1.

Main Index

GEOMETRY CHANGE 1707 Specify New Geometry

Format Fixed 71-75

Free 9th

Data Entry Entry I

Coordinate system flag for offset vector at beam node 2 0 – vector in global coordinate system 1 – vector in element coordinate system 2 – vector along associated shell normal at node 3 – vector in local coordinate system at node 2.

5b data block Necessary only if ioffset = 2 1-10

1st

F

Offset magnitude at corner node 1

11-20

2nd

F

Offset magnitude at corner node 2

21-30

3rd

F

Offset magnitude at corner node 3

31-40

4th

F

Offset magnitude at corner node 4

41-45

5th

I

Interpolation flag for higher-order shells 0 – no interpolation of offset for mid-side nodes 1 – linear interpolation of offset for mid-side nodes

46-50

6th

I

Constant Offset flag 0 – offset magnitude is variable. Four data fields are used to specify offset magnitudes at corner nodes. 1 – offset magnitude is constant. First data field is used to specify offset magnitudes at corner nodes.

6th data block Enter a list of elements to which the above geometry is applied. Notes: For elements 7, 10, 11, and 19, enter 1 in the EGEOM2 field to activate the constant dilatation option. This improves the behavior of the element for nearly incompressible analysis. See Marc Volume B: Element Library for further details. For elements 3, 7, and 11, enter 1 in the EGEOM3 field to activate the assumed strain formulation. This improves the element bending behavior. This is an alternative to the ASSUMED STRAIN parameter. For elements 109 and 110, the penalty factor used to add the constraint for the vector potential (Marc Volume A: Theory and User Information) to the set of equations for magnetostatic calculations can be set in the EGEOM2 field.

Main Index

1708 GEOMETRY CHANGE Specify New Geometry

Format Fixed

Free

Data Entry Entry

Beam offset capability is possible for elements 5, 14, 25, 36, 45, 52, 65, 76, 77, 78, 79, 98. Enter -1 in the EGEOM8 field and the offset information via the 4a data block. See Marc Volume B: Element Library for further details. The components of the local x-axis for beam elements are entered in the EGEOM4-EGEOM6 fields. These components can be entered in the global Cartesian coordinate system (default) or in a local coordinate system. In the latter case, the local coordinate system used to define the beam x-axis is flagged through the EGEOM8 field and is taken to be the coordinate system defined at the first nodal point of the beam element using the TRANSFORMATION, CYLINDRICAL, or COORD SYSTEM options. Enter ‘--10 or -11 in the EGEOM8 field to indicate that the fields EGEOM4-EGEOM6 are in the local coordinate system. If EGEOM8 is -11, it further indicates that the beam elements are offset and that the nodal offset vectors are provided via the 4a data block. Shell offset capability is possible for elements 1, 22, 50, 75, 85, 86, 87, 88, 89, 138, 139, 140. Enter -2 in the EGEOM8 field and the offset information via the 4b data block. See Marc Volume B: Element Library for further details.

Main Index

ORIENTATION CHANGE 1709 Redefine Orientation

ORIENTATION CHANGE

Redefine Orientation

Description This option allows redefinition of the internal material orientation data for the new rezoned mesh. See the discussion of the ORIENTATION model definition option in Chapter 3. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words ORIENTATION CHANGE.

2nd data block 1-5

1st

I

Enter the number of orientation angle data sets to follow.

6-10

2nd

I

Unit number for input. Defaults to input file.

Data blocks 3 and 4 are repeated as pairs; once for each angle data set. 3rd data block 1-10

1st

A

Enter one of the following to specify orientation angle type: EDGE 1-2 EDGE 2-3 EDGE 3-4 EDGE 3-1 EDGE 4-1 XY PLANE YZ PLANE ZX PLANE XU PLANE YU PLANE ZU PLANE UU PLANE UORIENT 3D ANISO COORD SYS 3D LOCAL CURVE

Main Index

1710 ORIENTATION CHANGE Redefine Orientation

Format Fixed 11-20

Free

Data Entry Entry

2nd

Enter orientation angle.

For EDGE style orientations: 21-30

3rd

F

First component of user vector 1 in global coordinates.

31-40

4th

F

Second component of user vector 1 in global coordinates.

41-50

5th

F

Third component of user vector 1 in global coordinates.

51-60

3rd

F

First component of user vector 2 in global coordinates.

61-70

4th

F

Second component of user vector 2 in global coordinates.

71-80

5th

F

Third component of user vector 2 in global coordinates.

For XU PLANE, YU PLANE, ZU PLANE, UU PLANE, and 3D ANISO, complete the following: 21-30

1st

F

1

31-40

2nd

F

2 component of user vector 1 with respect to global coordinates.

41-50

3rd

F

3

For UU PLANE, 3D ANISO, complete the following: 51-60

4th

F

1

61-70

5th

F

2 component of user vector 2 with respect to global coordinates.

71-80

6th

F

3

For COORD SYS style orientation: 21-25

3rd

I

Enter the coordinate system ID from COORD SYSTEM option.

4th data block Enter a list of elements associated with this orientation angle.

Main Index

GAP DATA CHANGE 1711 Redefine Gap Data

GAP DATA CHANGE

Redefine Gap Data

Description This option allows redefinition of gap data for the new rezoned mesh. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the words GAP DATA CHANGE.

2nd data block 1-5

1st

I

Number of sets of gap data to be input.

6-10

2nd

I

Unit number for reading data. Defaults to input format.

Data blocks 3, 4, and 5 are entered as a set; once for each set of gap data materials. 3rd data block 1-10

1st

F

For a fixed direction gap, enter the gap closure distance Ucl. For a true distance gap, enter the minimum distance between end points |d|. Notes: If d>0, the two end points are never closer than a distance |d| apart. If d<0, the two end points are never farther apart than |d|.

11-20

2nd

F

μ, the contact coefficient of friction.

21-30

3rd

F

KGAP’, the elastic stiffness of the closed gap in the contact direction. Default: gap is rigid when closed.

31-40

4th

F

KFRICTION’, the elastic stiffness of the closed gap in the friction direction. Default: gap is rigid when closed.

Main Index

41-50

5th

F

User-supplied momentum ratio for first gap node. Default: Marc calculates this ratio internally.

51-60

6th

F

User-supplied momentum ratio for fourth gap node. Default: Marc calculates this ratio internally.

1712 GAP DATA CHANGE Redefine Gap Data

Format Fixed 61-65

Free 7th

Data Entry Entry I

Enter 1 for true distance gap. Default is 0: fixed direction gap.

66-70

8th

I

Enter 1 if gap is closed during increment 0. Default is 0: gap is open during increment 0.

4th data block Enter a list of gap elements associated with this set of gap data.

Main Index

COORDINATE CHANGE 1713 Redefine Node Coordinates

COORDINATE CHANGE

Redefine Node Coordinates

Description This option allows redefinition of the coordinates of a number of nodes to redefine the mesh. If the LARGE STRAIN parameter is used or a rubber rezoning analysis using element types 80-84, 118120, or 155-157 is preformed, the new coordinates to be read in by this option are the updated coordinates. Marc itself divides this into new coordinates and new total displacements. If LARGE STRAIN is not used, the coordinates to be read in are the actual new coordinates without considering the displacements. Format

1st data block 1-17

1st

A

Enter the words COORDINATE CHANGE.

I

Enter the maximum number of coordinate directions to be read in per node.

2nd data block 1-5

1st

Defaults to the number of coordinates per node. 6-10

2nd

I

Enter the number of nodal points for which the new coordinates are read in this block (optional).

11-15

3rd

I

Enter the unit number to read coordinates. Defaults to input.

16-20

4th

I

Enter 1 to suppress printout of nodal coordinate list.

3rd data block One data block per nodal point. Input six coordinates per data block; CONTINUE options in format 6E10. 1-5

1st

I

Nodal point number.

6-15

2nd

F

Coordinate 1.

16-25

3rd

F

Coordinate 2.

26-35

4th

F

Coordinate 3.

etc.

Main Index

etc.

Number of coordinates per node to read in.

1714 UFRORD Use Subroutine UFRORD

UFRORD

Use Subroutine UFRORD

Description This option calls the UFRORD user subroutine to generate or modify nodal coordinates. See Marc Volume D: User Subroutines and Special Routines. The option can be repeated as often as necessary. If coordinates must be modified, this option should follow the COORDINATE CHANGE option. If coordinates must be defined, this option can be used alone. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word UFRORD.

2nd data block Enter a list of nodes for which the UFRORD user subroutine is to be called.

Main Index

MOVE (Rezoning) 1715 Redefine Node Coordinates

MOVE (Rezoning)

Redefine Node Coordinates

Description This option allows you to apply a uniform translation to a list of elements, redefining the coordinates of all nodes in the elements. This translation is applied to the last value of the coordinates, excluding any displacement. This option can be repeated as often as necessary. Format Format Fixed

Free

Data Entry Entry

1st data block 1-10

1st

A

Enter the word MOVE.

I

Enter the number of lists to be entered.

2nd data block 1-5

1st

3rd data block 1-10

1st

F

The amount of translation in the first coordinate direction.

11-20

2nd

F

The amount of translation in the second coordinate direction.

21-30

3rd

F

The amount of translation in the third coordinate direction.

4th data block This data block is entered once for each list. Enter a list of element numbers to which the above translation is applied.

Main Index

1716 CONTACT CHANGE Change Surface Contact after Rezoning

CONTACT CHANGE

Change Surface Contact after Rezoning

Description This option allows changes to a deformable surface definition (rezoned mesh) in 2-D and 3-D contact problems after rezoning occurs. Changes to the rigid surfaces should be made in the next loadcase using the CHANGE RIGID option. It also allows changes to friction type, choice of Coulomb friction calculation, maximum number of separations in each increment, suppression of splitting of increment. In addition, relative sliding velocity for sticking condition, contact tolerance, separation force, as well as average and cut-off strain rates in rigid-plastic analysis, can also be changed. Note:

See the SPLIT BODIES option if the analysis has deformable-to-deformable contact.

Format Format Fixed

Free

Data Entry Entry

1st data block 1-14

1st

A

Enter the words CONTACT CHANGE.

I

Number of surfaces to be defined.

2nd data block 1-5

1st

(Must be same value as before rezoning.) 6-10

2nd

I

Not used; enter 0.

11-15

3rd

I

Upper bound to the number of nodes that lie on the periphery of any deformable surface.

16-20

4th

I

Friction type 0: No Friction 1: Shear Friction 2: Coulomb 3: Shear Friction for Rolling 4: Coulomb Friction for Rolling 5: Stick-slip Coulomb Friction 6: Bilinear Coulomb Friction 7: Bilinear Shear Friction (Same value as before rezoning.)

Main Index

CONTACT CHANGE 1717 Change Surface Contact after Rezoning

Format Fixed 21-25

Free 5th

Data Entry Entry I

Enter 0 for the calculation of Coulomb friction based on nodal stress. Enter 1 for the calculation of Coulomb friction based on nodal force instead of nodal stress. Default is 0. This can only be activated for friction types 1 to 4. Friction types 5 to 7 always used nodal force.

26-30

6th

I

Maximum number of separations allowed in each increment. Default is 9999.

31-35

7th

I

Enter 0 (default) to use the increment splitting procedure for the fixed time step procedures (AUTO LOAD, DYNAMIC CHANGE, TRANSIENT NON AUTO). Enter 1 for the suppression of the splitting of an increment in fixed time step procedure. Enter 2 for adaptive time step procedure. Default is 0. Enter 3 to use contact procedure which does not require increment splitting (iterative penetration checking procedure). Note:

The iterative penetration checking procedure is not available for dynamic problems using the AUTO STEP option.

36-40

8th

I

Enter 3 to not reset NCYCLE = 0 when separation occurs; this speeds up the solution but might result in instabilities.

41-45

9th

I

Control separations within an increment. When 0 is entered, if the force on a node is greater than the separation force, the node separates and an iteration occurs. When 1 is entered, if a node, which was in contact at the end of the previous increment, has a force greater than the separation force, the node does not separate in this increment, but separates at the beginning of the next increment. When 2 is entered, if a new node comes into contact during this increment, it is not allowed to separate during this increment (prevents chattering). When 3 is entered, both (1) and (2) above are in effect.

46-50

10th

I

Parameter governing normal direction/thickness contribution of shell (ISH). Enter 0 – Check Node Contact with top and bottom surface Enter 1 – Nodes only come into contact with bottom layer Enter 2 – Nodes only come into contact with bottom layer and ignore shell thickness

Main Index

1718 CONTACT CHANGE Change Surface Contact after Rezoning

Format Fixed

Free

Data Entry Entry Enter -1 – Nodes only come into contact with top layer Enter -2 – Nodes only come into contact with top layer and ignore shell thickness

51-55

11th

I

Enter 1 to reduce printout of surface definition.

56-60

12th

I

Separation flag. This flag is related to the separation threshold entered on the 5th field of the 3rd data block and may have the following values: 0: Separation is based on nodal forces. If the contact normal force on a node in contact exceeds the threshold, the node separates. 1: Separation is based on absolute nodal stresses where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 2: Separation is based on absolute nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold, the node separates. 3: Separation is based on relative nodal stresses, where a nodal stress is calculated as a force divided by an equivalent area. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. 4: Separation is based on relative nodal stresses, where a nodal stress is determined by extrapolating and averaging integration point values. If the contact normal stress on a node in contact exceeds the threshold times the maximum contact normal stress, the node separates. The default value is 0. Notice that for true quadratic contact, only stressbased separation (2 or 4) can be used.

61-65

13th

I

Not used; enter 0.

66-70

14th

I

Linearization flag, to be used if a contact body consists of quadratic elements: 1: The outer boundary of a contact body is described based on the corner nodes only. In the contact area, the midside nodes are linearly tied to the corresponding corner nodes. Midside nodes cannot come into contact.

Main Index

CONTACT CHANGE 1719 Change Surface Contact after Rezoning

Format Fixed

Free

Data Entry Entry -1: The outer boundary of a contact body is described using a quadratic field. If a node touches a quadratic segment, a full quadratic multipoint constraint is set up. Both corner and midside nodes can come into contact. The default value is 1.

71-75

15th

I

Not used; enter 0.

76-80

16th

I

Enter 1 to get the tying information due to initial contact written into the jid.t01 file. This file can be included in a second analysis, so that (glued) contact conditions can be obtained without actually defining contact bodies in the second analysis. Enter 3 to write out the tying information due to contact each increment to a file called jid.comnpc_xxx where xxx is the increment number the Marc format is used. Enter 4 to write out the tying information due to contact each increment to a file called jid.conmpc_xxx. The MD Nastran MPC format is used.

3rd data block 1-10

1st

F

For friction types 1, 2, 3, or 4 enter the relative sliding velocity between bodies below which sticking is simulated (RVCNST). Default = 1.0. For friction type 5, enter the slip-to-stick transition region (β); Default is 1.e-6.

11-20

2nd

F

Distance below which a node is considered touching a body (ERROR). Leave blank if you want Marc to calculate it. This number is also used to divide splines. If splines are used, this must be defined.

21-30

3rd

F

Not used; enter 0.

31-40

4th

F

Not used; enter 0.

41-50

5th

F

Separation threshold. The physical meaning of this threshold (a force, a stress or a percentage of the maximum contact normal stress) depends on the separation flag entered on the 12th field of the 2nd data block. Notice that the CONTACT TABLE option offers the possibility to define a separation threshold per pair of contact bodies.

51-60

6th

F

Contact tolerance BIAS factor. (0-1)

61-70

7th

F

For stick-slip model, enter the friction coefficient multiplier (α). Defaults to 1.05

71-80

8th

F

For stick-slip model, enter the friction force tolerance (e). Defaults to 0.05.

Main Index

1720 CONTACT CHANGE Change Surface Contact after Rezoning

Format Fixed

Free

Data Entry Entry

For two- and three-dimensional contact problems The data blocks 4 and 5 are repeated once for each data set. 4th data block 1-5

1st

I

Body number.

6-10

2nd

I

Number of sets of geometrical data to be input for this rigid body (NETTY). Enter 0 if deformable body.

11-15

3rd

I

For rigid surfaces, enter 1 if surface is a symmetry plane. For deformable bodies, enter 1 if single-sided deformable-deformable contact is used. Note that, in this case, results are dependent upon the order in which contact bodies are defined.

16-20

4th

I

Not used; enter 0.

21-25

5th

I

Enter 1 if analytic form is to be used.

26-30

6th

I

Enter -1 if body is position controlled. Enter 0 (default) if body is velocity controlled. Enter a positive number if load controlled. The number entered is the node number which has the displacement degrees of freedom of the body. The position of this node is at the center of rotation given in the 5th data block.

31-35

7th

I

Enter a positive number if load controlled and rotations are allowed. The number is the node number which has the rotation(s) of the body as degrees of freedom. The position of this node is at the center of rotation given in the 5th data block. The first node of a load-controlled body may use the TRANSFORMATION or COORD SYSTEM option to allow for movement in user-defined directions. The load controlled body node(s) may have FIXED DISP/POINT LOAD or connections with environment/other structures using the SPRINGS option. Node 1 has x- and y-displacement as degree of freedom 1 and 2 Node 2 has z-rotation as degree of freedom 1

36-40

8th

I

Contact body type (optional): 1: rigid body; 2: deformable body; 3: symmetry body; 4: heat-rigid body;

Main Index

CONTACT CHANGE 1721 Change Surface Contact after Rezoning

Format Fixed

Free

Data Entry Entry 5: workpiece; 6: acoustic body.

41-64

9th

A

Contact body name (optional)

The 5th data block is only necessary if the surface is deformable; if the surface is rigid, no additional data is required. 5th data block Enter a list of elements of which the surface is comprised.

Main Index

1722 PRINT CHOICE (Rezoning) Select Print Settings

PRINT CHOICE (Rezoning)

Select Print Settings

Description This option allows control of the output from Marc. The data given here remains in control until a subsequent PRINT CHOICE set is inserted – such a set can be included with either the model definition or the history definition data options. The default values print all elements and all nodes. Element quantities are printed at each integration point or at the centroid only, depending on whether ALL POINTS parameter was used. For shells, only the extreme fibers are output, plus layers where the inelastic strains or state variables are nonzero. For beams, fibers with inelastic strains or nonzero state variables are printed. In addition, section forces are given for these elements. This option also allows debug output of certain items. The default is no debug printout. All of the above defaults are reset by the PRINT CHOICE option. The PRINT CHOICE option has no effect on the postprocessor file (see the POST model definition option). Format Format Fixed

Free

Data Entry Entry

1st data block 1-12

1st

A

Enter the words PRINT CHOICE.

2nd data block 1-5

1st

I

Number of sets of first and last element numbers to be printed (maximum 10).

6-10

2nd

I

Number of sets of first and last node numbers to be printed (maximum 10).

11-15

3rd

I

Number of integration points to be printed in each element (not used if ALL POINTS parameter not flagged).

16-20

4th

I

Number of layers to be printed. This is for beams and shells only, and overrides the default described above.

21-25

5th

I

Increments between printout. Default is print every increment.

Main Index

26-30

6th

I

Enter 1 for complex nodal quantities to be output as magnitude and phase; otherwise, real and imaginary components are given.

31-35

7th

I

Debug print flag. Enter a nonzero value and use data block 7.

36-40

8th

I

Log File Flag: Enter unit number to which log file is to be written.

PRINT CHOICE (Rezoning) 1723 Select Print Settings

Format Fixed

Free

Data Entry Entry

3rd data block Include only of the first field of 2nd data block is not zero. 1-5

1st

I

First element in first set.

6-10

2nd

I

Last element in first set.

11-15

3rd

I

First element in second set.

16-20

4th

I

Last element in second set.

Etc.

Etc. in I5 format.

4th data block Include only if the second field of 2nd data block is not zero. 1-5

1st

I

First node in first set.

6-10

2nd

I

Last node in first set.

11-15

3rd

I

First node in second set.

16-20

4th

I

Last node in second set.

Etc.

Etc. in I5 format.

5th data block Include only if the third field of 2nd data block is not zero. Enter the list of integration points to be printed in (16I5) format (number of entries given in the third field of cards series 2). This is only used if ALL POINTS parameter is flagged. Be careful with analyses with several different element types. 6th data block Include only if the fourth field of the 2nd data block is not zero. Enter the list of shell or beam fibers to be printed in (16I5) format. This over-rides Marc’s default, so that you should be aware that you do not unintentionally miss plasticity or creep printout. 7th data block Include only if the seventh field of the 2nd data block is not zero 1-5

Main Index

Enter debug plot code. See the PRINT parameter.

1724 URCONN Invoke User Subroutine URCONN

URCONN

Invoke User Subroutine URCONN

Description This option calls the URCONN user subroutine to generate or modify element connectivity (see Marc Volume D: User Subroutines and Special Routines.) The option can be repeated as often as necessary. This option must follow the connectivity change option. Format Format Fixed

Free

Data Entry Entry

1st data block 1-6

1st

A

Enter the word URCONN.

2nd data block Enter a list of elements for which the URCONN user subroutine is called.

Main Index

CONTINUE (Rezoning) 1725 End Rezoning Input

CONTINUE (Rezoning)

End Rezoning Input

Description This option closes the input for this rezoning step and gives control back to the executing routine. Format Format Fixed 1-8

Main Index

Free 1st

Data Entry Entry A

Enter the word CONTINUE.

1726 END REZONE End Input for Rezoning Increment

END REZONE

End Input for Rezoning Increment

Description This option closes the input for the rezoning increment. It must follow the CONTINUE option of the last defined rezoning step of the increment. If this option is read, control is given back to the main control routine of Marc, and the next input is interpreted as either mesh plot data or as history definition data. Format Format Fixed 1-10

Main Index

Free 1st

Data Entry Entry A

Enter the words END REZONE.

Marc Volume C: Program Input Appendix A Program Messages

A

Program Messages

J

Main Index

Marc Exits

1728

1728 Marc Volume C: Program Input Marc Exits

Marc Exits Marc provides an exit number when execution terminates, unless a system abort interrupts execution first. These exits are grouped as follows: Exit Number Classification 1-1000

Simple data errors detected during initial data input (before END OPTION).

1001-2000

Errors detected during stiffness assembly or load distribution.

2001-3000

Errors detected during solution of stiffness matrix or boundary condition or constraint application.

3001-4000

Exits during load incrementation control and output. Most normal exits are in this range.

4001-5000

System I/O Errors.

5001-6000

Errors detected during adaptive meshing.

The following subsections list the current exit numbers with their corresponding description and probable cause.

Exit Numbers 1-1000 Exit Number Explanation

Main Index

1

The number of elements associated with a distributed load exceeds the maximum number given on the SIZING, DIST LOADS, or FLUXES parameters. This usually happens in the history definition when a new distributed load is added or the number of elements is increased. Increase the value on the parameter. Note that this cannot be done in a restarted analysis, it must be done beginning with increment zero.

2

A line being read as a parameter line is unidentifiable. This may be caused by illegal data or a mistyped line.

3

The compilation of a user subroutine failed. The log file contains information about the failure. This error is given by the start-up script run_marc before the execution of Marc has started.

4

The number of fixed displacement boundary conditions input with the BC FILL or BC GENER options exceeds the maximum specified with the SIZING parameter. Check the data and change the maximum specification as necessary.

6

The analysis cannot be run in the memory space available. Either increase the work space on the SIZING parameter or modify the input.

Appendix A Program Messages 1729 Marc Exits

Exit Number Explanation Adding the ELSTO parameter stores the element data on the disk, thus reducing the amount of memory necessary. Reducing the number of layers associated with beam and shell elements and/or switching to reduced integration elements also reduces the amount of memory necessary. Be sure that the best solver has been chosen for your problem and that the bandwidth is being minimized. 7

Normal finish caused by setting the STOP parameter. Try to request larger work space on the SIZING parameter than the required work space mentioned in the output file, remove the STOP parameter, and resubmit the analysis.

9

Too many points (more than 60) used in the BEAM SECT parameter. Either the number of branches in a beam section is large, or the number of points per branch is large. Reduce the relevant number(s).

13

Data errors have been detected during data input. Refer to output for location of error. Likely causes are misspelled keywords, mistyped lines, or invalid input options.

14

Negative relative density during equilibrium iterations for the POWDER model. Decrease the load increment or use AUTO STEP or AUTO INCREMENT schemes. If the problem still occurs, check the material properties in the input data.

17

Conjugate gradient solver (2) or Hardware solver (6) cannot be combined with the OOC (out-of-core) parameter, or there is not enough available memory to use this solver in-core, or Memory Allocation Failed for CASI solver

18

Error with MACHINING (METAL CUTTING) is found. Possible reason and solution: 1. Features that MACHINING does not support yet are used. Turn off the unsupported feature if possible. 2. Error in cutter path data. Check the APT/CCL file. 3. If cutter motion type other than a. Point to Point (GOTO/) b. Cycle motion (CYCLE/DRILL) has been used, use the correct CATIA setting to convert it into one of the above motion types. 4. Wrong loadcase definition option is used. 5. Wrong load case definition option is used.

Main Index

1730 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 19

Error in welding simulation. Inconsistency in WELD FLUX, WELD PATH, and WELD FILL data. 1. Check that weld flux id exists. 2. Check that weld path id associated with weld flux exists. 3. Check that weld filler id associated with weld flux exists. 4. Check that weld flux type (volumetric or surface) is consistent with distributed flux index.

20

Error in welding simulation. Position of weld flux is not within specified weld path. 1. Check initial position of weld flux specified on WELD FLUX option. 2. Weld flux may be moving out of range of the specified weld path. Check weld velocity and/or WELD FLUX data. Extrapolation flag may be set to continue beyond last point on WELD FLUX option.

23

The wave front optimization scheme has lost continuity. This indicates that the mesh is not continuous. Two or more distinct bodies are defined in the same problem, and the wave front renumbering scheme cannot handle this case. Switch to the Sloan optimizer.

Main Index

24

No elements, springs or ties exist; the analysis cannot be meaningful. Check your input, it is possible that the input file is empty.

25

Internal renumbering scheme for Lagrange multipliers does not converge. Check if there are Herrmann elements where all displacement degrees of freedom are prescribed. Try a different optimization scheme. Otherwise, Marc system error; consult with an MSC software analyst.

26

No element type chosen. Include ELEMENTS or SIZING parameter.

27

Failure in transformation, most probably due to bad coordinates data.

28

The contacting body is moving away from the bottom dead center. Check current position and the bottom dead center in the output file (jidname.out) and adjust your input data.

29

The contacting body is not moving at all. Either the bottom dead center is reached or the zero moving velocity is encountered. Check current position and the bottom dead center or the velocity in the output file (jidname.out) and adjust the input data.

30

Selected surface entity not allowable in CONTACT model definition option. Check the input data.

31

A surface has more entities than the maximum declared. Increase the maximum number of entities on the CONTACT model definition option.

32

Circle segment data not consistent. Likely cause is that radii calculated are not consistent with the given input. Check input.

Appendix A Program Messages 1731 Marc Exits

Exit Number Explanation

Main Index

33

There are more boundary nodes than the upper bound declared. Increase the upper bound to the number of boundary nodes on the CONTACT model definition option.

34

Error in CONTACT model definition option. Either no deformable body has been defined, or there are rigid surfaces defined before deformable bodies. There must be at least one deformable body on the CONTACT option. All deformable bodies should be specified before rigid bodies.

35

During initial surface approach, velocities were set to zero before initial contact occurred.

36

Data error in supplying the surface profile for a 2-D deformable body. Check that elements specified for the body form a continuous path. Make sure that there are no inside-out or upside-down elements.

37

Friction calculations with the CONTACT option are being attempted without defining the relative sliding velocity below which sticking is simulated. Input the relative sliding velocity below which sticking is simulated on the CONTACT option.

38

The CONTACT model definition option is being exercised without a time increment being defined. Enter the time period using either TIME STEP, AUTO TIME, AUTO STEP, AUTO INCREMENT, DYNAMIC CHANGE, or TRANSIENT history definition options.

39

Attempt to change contact data during a REZONE increment. Only the elements associated with a deformable body can be changed during rezoning. Other changes must be done through the MOTION CHANGE or CONTACT TABLE history definition options.

40

During the approach stage of a contact analysis, a rigid body did not contact a deformable body within 1000 trials. The time step per trial is chosen in such a way that the displacement of the rigid body does not exceed 100 times the error tolerance calculated by Marc. The initial distance between the rigid and deformable contact bodies is probably too large or the rigid body velocity has an incorrect direction.

41

Error in determining normal direction to a contact surface; potential conflict with boundary condition. Try to remove boundary conditions on nodes that come into contact. It is better to use symmetry surfaces.

42

The number of subdivisions of a 3-D arc must be greater than 1. Change your input in the CONTACT model definition option.

43

The number of data points of a 3-D curve must be less than or equal to the number of subdivisions. Change your input in the CONTACT model definition option.

44

The number of data points on a polyline must be equal to the number of subdivisions minus 1. Change your input in the CONTACT model definition option.

45

The number of spline data points should be greater than 3 and less than 30. If the number is less than 3, convert the spline segment into a line. If the number of points is greater than 30, consider breaking the spline segment into multiple spline segments.

1732 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 46

The number of Bezier data points should be greater than 3. If the number of points is 2, treat entity as a 4-node patch (Type 7).

47

The input data points are either too close or colinear. Could not convert input to proposed surface type. Check input in the CONTACT model definition option.

48

The current patch is too small for program to find its normal. Check input of rigid contact surfaces. It is also possible that deformation has caused a surface of a deformable body to become very small.

50

The normal direction of the tied node in deformable-deformable contact has the same direction as a boundary condition. Try to remove boundary conditions of nodes that come into contact. It is better to use symmetry surfaces.

51

END parameter is missing. This must be included in the input file.

57

In a contact body used in the beam-to-beam contact model definition option a branch is detected. This is not supported in the current version of the program.

58

An analysis feature requested is currently not supported by the parallel version of Marc but will be in the near future.

59

An analysis feature requested is currently not supported by the parallel version of Marc. Unsupported features in the current parallel version of Marc are: acoustic, adaptive, auto therm creep, axisymmetric to 3-D data transfer (AXITO3D), bearing, buckling, beam-to-beam contact, design sensitivity and optimization, electromagnetics, explicit dynamics, fluid and its coupled analysis, gap elements, harmonic, hydrodynamics, JIntegral, out-of-core solver, radiation, response spectrum, and rezoning.

60

The listed contact body contains elements from the acoustic region and elements from other regions.

61

The listed contact body contains a combination of different element types (solid + shell or solid + beam or beam + shell). This is not supported.

62

Beam bodies in the current version cannot touch both beam bodies and other bodies.

67

Marc password security has determined that you are not allowed to run on this machine; possible reasons are: 1. The choice of machine or current OS level is not compliant with the passwords. 2. The file “license.dat” in the Marc subdirectory “security” contains wrong information. 3. The directory “security” has wrong access permissions. 4. All available licenses are in use - contact your local MSC software office to purchase additional licenses.

Main Index

Appendix A Program Messages 1733 Marc Exits

Exit Number Explanation 68

Marc password security has determined that you are not allowed to run on this machine; possible reasons are: 1. The license has expired. 2. The file “license.dat” in the Marc subdirectory wrong information.

Main Index

“security” contains

69

A third party solver requested is not supported in this version of Marc on this platform or in multi-processor mode.

70

Attempt to run a model larger than 500 nodes or 500 elements using the demo version of Marc.

71

While extracting outlines for remeshing, Marc found more than 100 closed loops in one body. The closed loops should be smaller than 100 at this time.

72

While extracting outlines for remeshing, Marc found more than 1000 nodes penetrating a contact body. The slave surface probably has a very coarse mesh compared with the master contact surface.

75

More than 1 outline found for the 2-D overlay mesher. Use other meshers, such as the advancing front mesher, in order to overcome the problem.

76

Incompatible view factor data has been read in. The number of segments read in is not consistent with the number required.

77

Error in restart run. There is an illegal change in parameter or model definition options in the input file of the restart run, such that the core allocation has changed. This may also occur if restart data utilized is from a different version of Marc.

78

Error in restart run with user provided mesh data.

79

Error in memory allocation.

80

Lap formation encountered during the analysis.

81

Error in remeshing. Nodes belonging to a body which is being remeshed have boundary conditions which cannot be transported correctly to the new mesh.

82

Number of faces of a cavity exceeds maximum estimated value. Increase maximum number on CAVITY parameter.

83

Error determining streamline. Check the input in the STREAM DEFINITION option. Make sure that the number of edges is consistent between inner and outer surface, and that the outer surface is truly the outer surface of this body.

84

The density at the surface is less than or equal to zero in recession/ablation calculation. Enter initial value of density was not provided, or charred density was not provided, or pyrolysis calculation is incorrect. Check input data.

85

The program is trying to perform an incremental data backup for a nonlinear analysis. However, the ELASTIC or SUBSTRUC parameter indicates that this is a linear elastic analysis. This is a conflict.

1734 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 100

Viewpoint chosen for plotting causes excessive distortion. Probable causes are that the viewpoint chosen is either within the body or too close to it.

666

The Powder model data input is incomplete. Check the input in the POWDER option.

Exit Numbers 1001-2000 Exit Number Explanation 1001

Connectivity exceeded at the node given in the message: MORE THAN MAXNP JOINED TO NODE... during in-core assembly of elements. This aborts Marc at that point. If this occurs during a contact analysis, try to activate single-sided contact on the CONTACT option. This can also occur if a contacted element has a user-defined tying on the contacted patch or edge. Otherwise, Marc system error; consult with an MSC software analyst.

1002

Connectivity exceeded at the node given in the message: MORE THAN MAXNP JOINED TO NODE... during out-of-core assembly of elements. This aborts Marc at that point. If this occurs during a contact analysis, try to activate single-sided contact on the CONTACT option. This can also occur if a contacted element has a user-defined tying on the contacted patch or edge.Otherwise, Marc system error; consult with an MSC software analyst.

1003

Too many nodes joined to node in forming fluid coupling matrix. Marc system error; consult with an MSC software analyst.

1004

Error occurred when calculating equivalent nodal loads. This is either due to an incorrect load type, or the element going inside out. Check input for valid load type for this element type or reduce step size.

1005

Errors during stiffness or mass matrix generation. The output reveals which element has a particular problem. If this occurs during the first assembly, it is due to input errors associated with the COORDINATES, GEOMETRY or the CONNECTIVITY model definition options. If this occurs during a later increment, it is due to excessive deformation in the element. Note that this can occur during the iterative process, so that it is not always possible to visualize the excessive deformation. Check the material behavior and the magnitude of the incremental loads. Suggestion: Activate the cut-back feature if using the AUTO LOAD, AUTO STEP, or AUTO INCREMENT solution schemes. This will allow the analysis to automatically cut down the time step and try again from the end of the last converged increment. For the AUTO LOAD procedure, the increment numbers are maintained as specified in the input.

Main Index

Appendix A Program Messages 1735 Marc Exits

Exit Number Explanation 1006

Elastic reanalysis attempted with nonzero displacement boundary conditions and boundary condition enforcement by row/column elimination. This is not possible. Remove the APPBC option.

1007

Incorrect Film or Foundation load type given. See additional messages in output to indicate which element and correct input.

1009

Error encountered in stress recovery. The output reveals which element has a particular problem. The error is usually due to excessive deformation in the element. This can occur during the iterative process, so that it is not always possible to visualize the excessive deformation. Check the material behavior and the magnitude of the incremental loads. Suggestion: Activate the cut-back feature if using the AUTO LOAD, AUTO STEP, or AUTO INCREMENT solution schemes. This will allow the analysis to automatically cut down the time step and to try again from the end of the last converged increment. For the AUTO LOAD procedure, the increment numbers are maintained as specified in the input.

Main Index

1010

Error occurred because emissivity was not defined for an element edge or face that is used in a radiating cavity. Correct input file.

1021

Error in adding fluid mass to node. Marc system error; consult with an MSC software analyst.

1030

Reference vector obtained by intersection of tangent plane and orientation plane has zero length; cannot determine preferred orientation. Check input in the ORIENTATION model definition option.

1031

Error while determining view factors in cavity. Make sure that node numbers defining cavity are in consecutive order in the input file.

1040

Maximum number of element groups exceeded while using EBE iterative solver. Increase the maximum number of groups allowed in the SOLVER option.

1041

Error in calculation of the spline constants during the reading of the material database.

1042

Material database file could not be opened.

1043

Too many materials from database used.

1044

Curves in material database have too many points.

1045

Error in calculation of the spline constants during the reading of the material database. Total number of curves read from material database is too large.

1050

Radiation is using an element type that is not supported by CAVITY option - output indicates element type. Remove elements of this type from CAVITY DEFINITION.

1051

Error in calculating pyrolysis damage. Damage indicator is less than 0 or greater than 1.0

1736 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 1052

The pyrolysis appears to begin on the colder side. Possibly the definition of interior and exterior surfaces is incorrect.

1053

The mass density is less than or equal to zero; either the initial mass density was not defined via INITIAL PYROLYSIS or the pyrolysis calculation is incorrect.

1054

Too much ablation occurred within this increment and the fixed time stepping procedure is used. Either switch to adaptive time stepping or reduce the time step or increase the amount of ablation allowed per time step.

1055

Attempt to use table ID which has not been defined.

1111

An error occurred during the outline search of a 2-D contact body. In planar problems, check for correct anti-clockwise numbering of all elements in the body. Otherwise, Marc system error; consult with an MSC software analyst.

1112

An error occurred during the adding of load provided in DMIG. Marc system error; consult MSC software analyst.

1113

An error occurred during adaptive meshing. Marc system error; consult MSC software analyst.

Exit Numbers 2001-3000 Exit Number Explanation

Main Index

2004

The determinant of the stiffness matrix becomes zero or negative when the indicated node has been reached during the Gaussian elimination phase of the solution process. This means that the stiffness matrix is nonpositive definite. If this happens at the start of the analysis, the condition is usually caused by the existence of rigid body modes. It may also be caused by incorrect material properties (for example, Poisson's ratio greater than 0.5; note that these situations may arise through temperature dependence of properties). In nonlinear cases, the structure may have buckled or reached a plastic limit load. In rubber analysis, it may also be due to the strain state being in a region where the input data for the strain energy function is invalid. In contact analysis with friction, lack of normal forces may result in friction being absent. If desired, Marc may be forced to continue by use of the PRINT parameter or the CONTROL model (or history) definition option. Either one of these procedures may be used for restart. Whenever a nonpositive definite situation occurs one must exercise caution, as the resultant numerical solution may be infeasible.

2006

System error in multifrontal sparse solver. Marc system error; consult with an MSC software analyst.

2007

System error in CASI iterative solver. The output gives additional messages. The problem may be due to rigid body modes in the system. Switch to the multifrontal direct solver if possible.

Appendix A Program Messages 1737 Marc Exits

Exit Number Explanation 2008

Maximum connectivity has been exceeded during application of tying constraints. If tyings are included, check the TYING model definition and TYING CHANGE history definition options. This may also occur because of inconsistencies in deformabledeformable contact; switch to single-sided (K3 style) contact. Marc system error; consult with an MSC software analyst.

2009

Not enough space to convert system from nodal blocks to row format. Marc system error; consult with an MSC software analyst.

2011

Errors encountered during application of TYING equations. Printout indicates specific problem.

2012

One of the surface directions in Tying Type 22 (intersecting shells of type 22) has zero length. This is caused by bad surface normal coordinates at one of the nodes being tied.

2014

Search vector for eigen extraction is zero. Caused by inadequate guess vector, or by asking for more eigenvalues than the system contains. Do not attempt to extract more modes than exist in the system. The number of modes is the total number of degrees of freedom minus the number of boundary conditions. Remember that contact to rigid bodies effectively apply boundary conditions to the system, hence removing potential modes.

2015

Not enough work space for the fluid/solid interface calculations. Increase the space specified on the SIZING parameter,

2016

Not enough work space for the fluid/solid interface calculations. Increase the space specified on the SIZING parameter.

2017

Not enough work space for the fluid/solid interface calculations. Increase the space specified on the SIZING parameter.

2020

Conjugate gradient iterative solver fails to converge within the required number of iterations. This may be due to the fact that there are rigid body modes in the system, or that the system is numerically ill-conditioned, such as with shell or membrane structures. Possible things to do: 1. Add pre-conditioner, incomplete Cholesky preferred. 2. Increase the number of iterations. 3. Set the number of iterations to a negative number. This forces Marc to continue. If the solution is truly poor, Marc does not converge in the outer Newton-Raphson iterations.

2030

Main Index

Unable to perform dynamic memory allocation for hardware-provided direct sparse solver. Decrease the amount of memory requested on the SIZING parameter down to the number printed in the output file (jidname.out). Use reduced integration elements and reduce the number of layers of shell elements. If you still get this message, either increase the amount of virtual/real memory on the computer, switch to the multifrontal sparse solver, or switch to the sparse iterative solver.

1738 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 2031

Error occurred during initialization or factorization process with hardware provided direct sparse solver. Switch to one of the Marc solvers. Consult with an MSC software analyst.

2032

The number of entries including fill-in is too large for the sky-line solver. Use another solver.

2033

Memory allocation error; not enough memory to perform internal nodal renumbering with METIS. To avoid this error, try using either a different solver or nodal optization routine.

2109

Mode with zero energy is found during transient modal response analysis. Probable cause is failure to use MODAL SHAPE history definition option before DYNAMIC CHANGE is used. Check input file.

2201

Attempt to recover a substructure, before solving the one level higher superstructure.

2304

Cannot use AUTO INCREMENT with boundary conditions using table input that is a function of time. either switch to AUTO STEP or remove time dependent table - load will be controlled by AUTO INCREMENT procedure.

2400

A node on the boundary of a deformable body tried to slide out of surface definition in a contact analysis. Either the segment of a rigid body is not large enough, in which case increase the length, or the nodal points in the area of contact have a large incremental displacement due to possible instability. In the latter case, the suggestion below may help under certain circumstances. Suggestion: Activate the cut-back feature if using the AUTO LOAD, AUTO STEP, or AUTO INCREMENT solution schemes. This allows the analysis to automatically cut down the time step and to try again from the end of the last converged increment. For the AUTO LOAD procedure, the increment numbers are maintained as specified in the input.

Main Index

2401

In a 3-D contact analysis, a node touching a 3-D NURBS cannot be projected on the NURBS. Marc system error: consult with an MSC software analyst.

2402

A growing rigid body may have different growing factors in x, y, and z-direction in this release only if it is not rotating.

2404

A growing rigid body should have relative size of 1.0 at time 0.0 You should scale the initial size in the modelling phase of your analysis.

Appendix A Program Messages 1739 Marc Exits

Exit Numbers 3001-4000 Exit Number Explanation 3001

The maximum number of increments specified on the CONTROL option has been reached. Note that increment zero has to be considered as an increment as well.

3002

Analysis has failed to converge to required convergence tolerances. One of several error conditions has been detected and the run aborted. The output specifies additional messages.

3003

Analysis could not be finished because the maximum number of increments defined in an adaptive loading procedure has been reached or the calculated step is too small. The user should increase the number of increments allowed during the automatic loading procedure.

3004

This is a successful completion to a Marc analysis, indicating that no additional incremental data was found and the analysis is complete.

3005

This is a successful completion to a Marc analysis when the CASE COMBIN(ATION) model definition option is used.

3006

This is a successful completion to a Marc analysis when the user has requested that the restart file is to be read and that either the results are to be printed or a post file is to be created.

3007

A restart analysis has been requested at an increment that is not on the restart file. The previous output will give the message RESTART DATA AT INCREMENT XX The new input file should specify the increment number XX on the RESTART model definition option.

Main Index

3008

Contact caused the restarting of an increment an excessive number of times. This may be due to separation or increment splitting. Increase the separation force or reduce the size of the step. An alternative is to increase the number of recycles allowed.

3009

Time step size becomes too small to continue the analysis. This may be due to having too many cutback times in current increment. An alternative is to increase the allowed maximum number of cutback times.

3010

Successful completion of design sensitivity analysis.

3011

Successful completion of design optimization process.

3012

No constraints activated at vertex of design space. Enter bounds on design variables, as these are probably missing.

3013

User element is not supported in design sensitivity analysis or design optimization process.

3014

For design optimization with composite layer thicknesses as design variables, the initial thicknesses may not be given in terms of percentages. Enter only estimated values, as it is not necessary to enter accurate values in this case.

1740 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 3015

Unable to reduce the time step below the minimum value allowed, and to still satisfy the user criteria in the AUTO STEP history definition option. Either change the criteria or reduce the minimum time step allowed.

3016

The element chosen is not supported in the Lorenzi j-integral calculation. This element type must not be used in the crack region of the model, but it can be used outside the crack region.

3017

DESIGN SENSITIVITY cannot be used with rebar elements.

3018

This is a successful completion of an analysis to generate an MD Adams MNF database file.

3019

MD Adams MNF database file generation failed.

3020

Job stopped immediately due to user intervention.

3021

Job stopped at end of increment due to user intervention.

3022

This is a successful completion of an analysis to generate a DMIG file of a substructure.

3023

This analysis needs the use of solver 8.

3025

Normal ending of Marc-reader.

3026

Marc-reader does not support substructures or superelements.

3027

Marc-reader does not support: 1. UFCONN user subroutine; 2. Element type chosen. 3. Reading of a restart file. Set relevant field to 1 in Marc input file.

Main Index

3030

Job has created brake squeal DMIG matrices as requested.

3031

Job has created contact interface file as requested.

3032

Job has been terminated in an AUTO INCREMENT loadcase because the load has reached over 100% of desired load in opposite direction. It is likely that the wrong branch in bifurcation analysis has been taken. Change the AUTO INCREMENT procedure and/or tighten the convergence testing.

3300

The eigenvalue extraction did not converge within the maximum number of iterations allowed. Increase the maximum number of cycles or tolerance in the MODAL SHAPE, MODAL INCREMENT, BUCKLE, or BUCKLE INCREMENT options or, if applicable, change from the inverse power sweep to the Lanczos method using the BUCKLE parameter.

3301

Eigenvalue analysis requested, but either mass is zero or initial stress stiffness is zero. For dynamic modal analysis, make sure that there is mass in the system. This can be from either entering a mass density or mass points. For buckling analysis, make sure that load has been previously applied to the structure, such that stresses are present.

Appendix A Program Messages 1741 Marc Exits

Exit Number Explanation 3302

Nonpositive definite system occurred during Lanczos eigenvalue extraction for buckling analysis. Decrease the applied load before the buckling analysis is performed or switch to the inverse power sweep method using the BUCKLE parameter.

3303

Either eigenvalue extraction for modal analysis or buckling analysis cannot be performed immediately after the activation or de-activation or local adaptive meshing or global rezoning of elements or the number of modes below the specified maximum frequency is zero. You should perform at least one extra increment before the eigenvalue extraction can be performed or change the maximum frequency.

3304

In an inertia relief analysis using the Kinematic method, only free directions specified for inertia relief loading can be left unconstrained. If non-inertia relief directions are unconstrained, the system has a singularity. You should constrain the non-inertia relief directions OR you should specify the unconstrained directions as free inertia relief directions.

3305

Eigenvalue extraction for modal analysis using the Lanczos method did not converge. A possible cause is that the model contains rigid body modes and the value of the lowest frequency to be extracted (defined on the MODAL SHAPE option) is either zero or very small. Try to specify this value to be around 10% of the first nonzero eigenfrequency. If you specify a positive value, you will only find the positive eigenmodes; if you specify a negative value also, the rigid body modes will be found.

Main Index

3401

Errors in torque (or friction force) controlled steady state rolling analysis. Check the error messages in the output file for details.

3402

In a structural zooming analysis, the local analysis time exceeds the maximum time available in global post file. Either rerun the global analysis with a wider time range in post file, or use extrapolation option defined under GLOBALLOCAL.

3403

Errors in a structural zooming analysis when read in the global post file. Check the error messages in output file for details.

3410

The thermal solution has become unstable. If using fixed time step procedure reduce time step and/or reduce the maximum error in the temperature estimate allowed. If using adaptive time step procedure reduce the maximum temperature change allowed nd/or reduce the maximum error in the temperature estimate allowed.

1742 Marc Volume C: Program Input Marc Exits

Exit Numbers 4001-5000 Exit Number Explanation 4001

Sequential I/O error: problems with opening, reading or writing files. Check file access permissions and available disk space. If on a restart or post file, there was an attempt to read an increment which is not on file. Otherwise, Marc system error; consult with an MSC software analyst.

4002

Cannot find jidname.pass file which is needed for automatic restart run. This is an internal file and should not be removed.

4003

Cannot read any “continue” statement in jidname.rst file for the automatic restart run. Check jidname.dat to make sure there are loadcases to run the problem.

4004

Cannot find the jidname.rst file which is needed for automatic restart run. This is an internal file and should not be removed.

4009

Sequential I/O error, unable to open file. Either a file requested is not found, or there is a system protection against opening the file. Make sure that you have read/write permission in the current directory or that the file has not been opened by another process; for example, Marc Mentat. If this is a mesh data file, the mesher may have failed to create a mesh.

4031

Unable to obtain the memory requested during a dynamic memory request. This can be due to the following reasons: 1. The maximum allowed amount of memory is exceeded. This is specified by the MAXSIZE variable in the include file in the tools directory in the Marc install directory. MAXSIZE specifies the memory in million words, multiply by 4 to get the amount in megabytes. 2. There is not enough free memory on the system. If the memory available is not enough for an in-core solution, Marc attempts to perform the solution out-of-core. In this case, some data which normally would be stored in memory is stored on the hard disk (which could slow down the analysis considerably). The memory request fails if there is still not enough memory for the analysis.

Main Index

4032

The maximum amount of memory in the job is exceeded and it was not possible at this point to switch over to an out-of-core solution.

4209

The option of reading radiation view factors from a file is specified in the related model definition option, but either the given file could not be opened (for example, no read permission) or, the input option -vf was not used to specify the file.

4210

Restart requested, but no restart file was provided. Add “-rid” parameter when submitting the job.

4211

Substructure analysis requested, but no database was found. Add “-sid” parameter when submitting the job.

4212

AUTO STEP does not support electromagnetics analysis. Try to use other auto loading strategies.

Appendix A Program Messages 1743 Marc Exits

Exit Number Explanation 4213

AUTO STEP does not support soil material models. Try to use other auto loading

strategies. 4214

AUTO STEP does not support powder material models. Try to use other auto loading

strategies.

Exit Numbers 5001-6000 Exit Number Explanation

Main Index

5001

The number of nodes created during adaptive meshing is greater than the number specified on the ADAPTIVE parameter. Either increase the number on the ADAPTIVE parameter or reduce the number of levels allowed with the ADAPTIVE model definition option. The analysis can be forced to continue using the ADAPTIVE parameter.

5002

The number of elements created during adaptive meshing is greater than the number specified on the ADAPTIVE parameter. Either increase the number on the ADAPTIVE parameter or reduce the number of levels allowed with the ADAPTIVE model definition option. The analysis can be forced to continue using the ADAPTIVE parameter.

5003

Adaptive meshing is not available for the element type used. Either use a valid element type, remove ADAPTIVE option or use ADAPTIVE option with a set specifying elements of a valid type.

5004

Adaptive meshing is not available for the element type used. Either use a valid element type, remove ADAPTIVE option or use ADAPTIVE option with a set specifying elements which are of a valid type.

5005

Number of boundary conditions created during adaptive meshing exceeds the number specified on the SIZING parameter. Increase the number of boundary conditions specified on the SIZING parameter.

5006

The number(s) of nodes and/or elements created during adaptive meshing is greater than the numbers specified on the ADAPTIVE parameter. Either increase the numbers on the ADAPTIVE parameter or increase the element edge length on the ADAPT GLOBAL option. The analysis can be forced to continue using the ADAPTIVE parameter.

5007

Error in performing adaptive meshing with elastic foundations or films; Marc system error; consult with an MSC software analyst.

5008

The number of elastic foundations or films created during adaptive meshing exceeds the number specified on the ADAPTIVE parameter. Add FOUNDATION model (or history) or FILMS model (or history) definition option.

5009

Error in memory allocation while performing adaptive meshing. Marc system error; consult with an MSC software analyst.

1744 Marc Volume C: Program Input Marc Exits

Exit Number Explanation 5010

System error during adaptive meshing. Marc system error; consult with an MSC software analyst.

5011

Unable to find surface for adaptive meshing with shells if the ATTACH NODE model definition option is used. Check definition of surfaces.

5012

Unable to find surface normal when using the ATTACH NODE model definition option with 3-D adaptive meshing. Check definition of surfaces.

5013

The command string to call mesher is too long. It is likely that your path to the mesher is too long or your filename is too long.

5024

Not enough space on SIZING parameter to perform rezoning. Increase workspace available.

5025

The node being printed is used in the TRANSFORMATION or COORD SYSTEM model definition option and also belongs to an element which is subdivided in the ADAPTIVE option. This is not allowed.

5050

Number of divisions in the x-direction exceeds maximum needed. Increase the element target length on ADAPT GLOBAL option.

Main Index

5051

Number of divisions in the y-direction exceeds maximum needed. Increase the element target length on ADAPT GLOBAL option.

5052

Something is wrong with start point in mesher. Reduce the element target length on ADAPT GLOBAL option.

5053

Something is wrong with projection in mesher. Reduce the element target length on ADAPT GLOBAL option.

5054

Something is wrong with start point in mesher. Marc system error; consult with an MSC software analyst.

5055

Something is wrong with the mesh outline; outline is not complete. Marc system error; consult with an MSC software analyst.

5056

Cannot mesh with current edge length. Try smaller edge length and, if necessary, increase maximum number of elements and nodes on the ADAPTIVE parameter.

5057

Error found from 3-D hexmesher. Check error message in file jidname.log.

5058

2-D overlay mesher failed to create a mesh after many trials. This may be due to small element size or wrong outlines.

5059

The mesher failed to create a mesh. Check error messages in the output file (jidname.out) or in the log file.

5060

Cannot find the mesh data file. The mesher might be hanging due to memory problem or the disk space is full.

5061

The mesh data file is not complete. The mesher might be hanging due to memory problem or the disk space is full.

Appendix A Program Messages 1745 Marc Exits

Exit Number Explanation 5062

The solver has been waiting for remeshing status file. Check if Run_sleep program is running properly.

5063

The element size for remeshing is found to be zero. You need to specify the element size or number of elements needed for remeshing. Check input.

5064

2-D trimming fails because of the above error. Check your input and redesign your trimmer.

5065

Bad elements are found after remeshing check if the mesher creates a good mesh. Contact with MSC Support.

5066

Trimming operation is not supported in Marc release.

5067

During the rezoning process, a new node is found outside the previous mesh. It is not possible to transfer data to the new mesh. Contact Support.

5091

Stand alone view factor program failed; consult Software analyst.

5092

The solver has been waiting for view factor status file. Check if Run_sleep program is running properly.

5093

The command string to call viewfactor program is too long. It is likely that your path to the bin directory is too long or your filename is too long.

5094

Cannot find the view factor data file. The view factor program might be hanging due to memory problem or the disk space is full.

5095

The view factor file is not complete. The view factor might be hanging due to memory problem or the disk space is full or the view factor file does not output the required data.

Exit Numbers 6001-7000 Exit Number Explanation 6001-6999

Main Index

Reserved for auto restart exit.

1746 Marc Volume C: Program Input Marc Exits

Exit Numbers 9001-10000 Exit Number 9991

Explanation Error in 2-D contact code. This is usually related to excessive iterative displacements which cause difficulties in finding the correct new position of nodes in contact. Possible remedies are: – use the iterative penetration checking procedure; – reduce the load incrementation; – define the maximum change in the incremental displacement to be equal to, e.g., a characteristic element length; – for incompressible materials, only use the tensile stresses in the geometric stiffness matrix. If the problem remains, consult an MSC software analyst.

9992

Error in 3-D contact code. This is usually related to excessive iterative displacements which cause difficulties in finding the correct new position of nodes in contact. Possible remedies are: – use the iterative penetration checking procedure; – reduce the load incrementation; – define the maximum change in the incremental displacement to be equal to, e.g., a characteristic element length; – for incompressible materials, only use the tensile stresses in the geometric stiffness matrix. If the problem remains, consult an MSC software analyst.

9993

Main Index

Error in equation intepretor or evaluator; used by TABLE option.

Appendix B Workspace Definition and the Sizing Option

B

Main Index

Workspace Definition and the Sizing Option J

I/O With Marc

J

Estimating File Sizes

J

Running Marc

1749

1752

1750

1748 Estimating Workspace Sizes for Marc Jobs

Finite element analysis requires the generation of a large amount of data including element quantities, nodal quantities, input data and the stiffness matrix. Under ideal circumstances, all of this data can be stored in core. Marc uses dynamic memory management in performing the analysis. The memory used by Marc is allocated in separate parts. One part is what is referred to as “general memory” and contains much of the data used in the analysis. The largest parts are the assembled stiffness matrix and, possibly, the decomposed stiffness matrix. Solvers 6 (hardware provided), 8 (multifrontal sparse), and 9 (CASI) allocate the main part of the memory separately. Another part of the memory allocation is the so-called incremental backup. This is a copy of part of the element data and is needed for a nonlinear analysis. Other parts allocated separately are the element data, vector data, contact data, tyings, transformations and data for boundary conditions. The memory allocation is automatically done for the amount of memory needed. When more memory is needed, additional memory is allocated. Only the general memory part can be affected by the user. At the beginning of the job, Marc allocates the amount of memory specified by the SIZING parameter in the Marc input file (if no sizing value is specified, it uses 5,000,000). This memory is among other things used for storing data that is read in. After the model data is read, more memory is allocated for the general memory as needed. This additional allocation of memory can be limited by means of the variable MAXSIZE defined in the file include (include.bat on Windows) in the tools directory of the Marc installation. In the case that the amount specified by MAXSIZE, or that there is no more memory to allocate, Marc attempts to put part of the memory on disk. It then activates either the ELSTO parameter or the out-of-core solver option, or both. The ELSTO parameter places the element quantities on the disk. This option substantially reduces the memory requirements with only a small penalty to the performance. For models that require an amount of memory close to the memory limit, it is advantageous to specify a sizing value high enough to avoid that additional allocation is necessary. The memory allocation in Marc is done via a C routine called calloc. When additional memory is needed the memory portion is extended via the C routine realloc. This part is handle by the operative system. During the realloc phase both the old and the new memory needs to be kept in virtual memory. Thus, it is important that the system is set up with enough swapping (paging) space. For efficiency, it is usually best to avoid realloc of large memory segments. The amount used for general memory is reported at the end of the analysis in the output file under “memory usage:” as the item “general memory (sizing)”. This printout can also be obtained during the analysis by means of the control file, see Appendix D. A test run for determining the memory usage without running the whole job can be done by using the STOP parameter in the input file. Unfortunately, because of deformable-deformable contact the global bandwidth may increase, hence requiring additional memory allocation. There is no way to predict this.

Estimating Workspace Sizes for Marc Jobs Unfortunately, there is no easy method for estimating how much workspace is needed by Marc, as the space computation is a complicated function of many variables. The most efficient method is to select a workspace to handle as large a variety of runs as possible, without at the same time sacrificing efficiency or wasted core space.

Main Index

Appendix B Workspace Definition and the Sizing Option 1749 I/O With Marc

Marc presents some complications to estimating sizing as both in-core and out-of-core solutions are possible. It is also possible to have the storage of elements data out-of-core through the use of the ELSTO parameter. Normally, you have no direct control over whether the solution is in-core or out-of-core except the OOC parameter may be used to force out-of-core assembly. If the memory limitation is exceeded, the job goes out-of-core. If the disk space limitation is exceeded, the job stops. The program now comes with defaults sufficient to run well-sized problems, so simply setting the SIZING parameter to zero (0) allows these defaults to take over.

I/O With Marc In this section, the input and output (I/O) that Marc performs during an analysis are discussed. The machine dependent specifics are discussed in subsequent sections. In many cases, it is your responsibility to preserve one or more of the files written out for subsequent analysis. Marc’s execution is performed in a noninteractive manner; that is, input data is placed in a file and is not modified during the execution of the problem. During the execution of this job, this file and others are either read, written, or both written and read. The primary data file is the “input” file and is normally read from FORTRAN unit 5. This file is a socalled card image file, referring to the days when input was prepared as punch card decks. It is necessary for all analyses. The results of the finite element analysis containing the stresses, strains, displacements, reactions, etc. are normally written to FORTRAN unit 6. This is the “output” file. This file is always created by Marc. If you request a “restart” file, it is written by default to unit 8. Upon restarting the analysis, this previously generated file is, by default, read from as unit 9. The restart files are binary sequential files containing the results of one or more increments. You can control the frequency with which the restart information is written. The information written for each increment contains control information, element and nodal data. Normally, you should request that a subset of the results be written to an auxiliary file labeled the post file. This information is typically used for postprocessing by Marc. Mentat and MD Patran use this information to produce either deformation, contour, x-y, or time history plots. The PLDUMP program, as discussed in Marc Volume D: User Subroutines and Special Routines, can also be used to examine this information. This file is used to transfer temperature data from a heat transfer analysis to a stress analysis. You select the post file to be either a binary or formatted (ASCII) file. Either type of a file is a sequential file. By default, the binary file is written to unit 16 and the formatted file is written to unit 19. The advantage of generating a binary file is that the I/O time is faster and the resultant file is smaller. The advantage of generating a formatted file is that the results can be more readily transferred to another machine for postprocessing. The PLDUMP program can be used to translate the post file from one format to the other. One or more increments of analysis can be written to this file. Upon restart, you can request that Marc make a new post file that contains either the information from both previous and restart analyses (continuous) or the data from the restart analysis only. If the RESTART option appears before the POST option, a continuous post file is written. In such an analysis, the old post

Main Index

1750 Estimating File Sizes

file is read from units 17 or 20 depending on whether a binary or formatted file was made, respectively. The creation of a continuous post file results in a much larger file. If the CHANGE STATE option is used in a thermal stress analysis, the post files previously generated in a heat transfer analysis is read from unit 24 (formatted) or unit 25 (binary). If the PRE STATE option is used, the post files previously generated is read from unit 24 (formatted) or unit 25 (binary). If the GLOBALLOCAL option is used, the post files previously generated is read from unit 24 (formatted) or unit 25 (binary). The use of substructures/superelements requires I/O on multiple files. The primary data base is a direct access binary file written to unit 31. Optionally, you can place the bulk of the information required in substructure analysis to auxiliary sequential binary files. In this case, each formed superelement is placed in its own file. The direct access database is still required. Marc also uses additional files for scratch purposes depending on the type of the analysis or options selected, as discussed below. If you include the ELSTO parameter, the information associated with element quantities is stored on a binary direct access file on unit 3. These element quantities are stresses, strains, plastic strains, etc. Marc may automatically switch on the ELSTO parameter if the workspace specified on the SIZING parameter is not adequate to store the information in core. The global stiffness matrix typically requires the largest amount of data. If the amount of data exceeds the available workspace, Marc automatically utilizes the out-of-core solver. The out-of-core assembly and solver utilize as many as five files. Some of the files are used for multiple purposes during this process. Files 11, 12, 13, and 15 are binary sequential files, while file 14 is a binary direct access file. Marc also uses files 12 and 13 during the iteration process of nonlinear analysis. If the Lanczos eigenvalue extraction procedure is used, the eigenvectors are stored in a binary sequential file on unit 22.

Estimating File Sizes In an out-of-core solution using the symmetric profile solver, units 11 and 12 have approximately the same storage space requirements. The number of single-precision words needed is: NUMNP*(MAXBW*NDEG*2+3)*NDEG where NUMNP = number of nodes in the mesh

Main Index

MAXB W

= average nodal half-bandwidth

NDEG

= number of degrees of freedom per node

Appendix B Workspace Definition and the Sizing Option 1751 Estimating File Sizes

The other two out-of-core solution files, units 13 and 15, are also approximately the same regarding total disk space usage. The number of single- precision words is: MAXBW2 * NDEG2 where

MAXBW and NDEG are defined as above. Also important is the need to have some idea of how large the files created by the POST or RESTART options are going to be. For the POST option, the approximate number of words written per increment is: (NUMV*INTEL*NUMEL)+(NUMNP*JNODE*NDEG) where NUMV

= number of element variables per integration point

INTEL

= maximum number of integration points per element

NUMEL = number of elements NUMNP = number of nodes JNODE

= number of types of nodal vectors written to the post file.

NDEG

= number of degrees of freedom per node

Note:

INOD = JNODE * NDEG. Also see Block 502nn for PLDUMP 2000 in the same chapter

mentioned above. The format of a restart file is much more complicated and changes somewhat with every new feature added. Therefore, an accurate estimate of space requirements is very difficult. The amount of data output depends, to some extent, on the options within Marc that have been selected. However, the largest amount of data on the file is formed from three parts: 1. Space for element variables (connectivity, stresses, etc.). 2. Space for the storage of the displacement, load and coordinate vectors. The space for the first two can be found by examining the output of a Marc run. About one-third of the way down the page entitled “Key to Strain, Stress, and Displacement Output”, there is a section “Internal Core Allocation Parameters”. In this section, the total space required in words for element and vector storage is printed. When these two numbers are added together, you will have a rough idea of how many words per increment are written to the restart file. When a large analysis of many increments is run, the total number of words in the restart file is quite large. Note that since all these files contain unformatted variable-length records, some extra space must be added to the above figures to determine the total disk space. Also, Marc requires some additional space

Main Index

1752 Running Marc

for internal control variables, thereby increasing the total space even more. Thus, any estimates should be at least doubled to provide a sufficient safety margin.

Running Marc This section describes the use of Marc on UNIX- and Linux-based and Windows platforms. Marc is mainly controlled by a shell script program called run_marc (run_marc.bat for Windows platforms) which is stored in the subdirectory tools. If you have used the option to create a link during the installation, this shell script is also known system wide as marc. It is designed to handle practically all possible options. The shell script submits a job and automatically takes care of the file assignments provided that use is made of the default FORTRAN file units as specified in Table B-1. Note that Marc automatically opens all needed file units. For the single processor case, the shell script must be executed in the directory where all relevant input and output files concerning the job are available. To use the shell script, each Marc job should have a unique name qualifier and, as a result, all Marc output files connected to that job use this same qualifier. For domain decomposition based parallel processing on the same platform, see the -nprocd option in Table . For parallel processing over a number of machines refer to the Parallel Installation and User Notes for the Parallel Network version of Marc on UNIX or NT. Table B-1

FORTRAN File Units Used by Marc

File Name

Unit

Description

jidname.log

0

Analysis sequence log file

sequential access, formatted

jidname.t01

1

Usually contains mesh data

random access, formatted

jidname.t02

2

OOC* solver scratch file

random access, binary

jidname.t03

3

Element data storage (see ELSTO parameter)

random access, binary

jidname.dat

5

Data input file

sequential access, formatted

jidname.out

6

Output file

sequential access, formatted

jidname.t08

8

Restart file, written out

sequential access, binary

ridname.t08

9

Restart file to be read in from a previous job

sequential access, binary

jidname.t11

11

OOC* solver scratch file

sequential access, binary

jidname.t12

12

OOC* solver scratch file

sequential access, binary

jidname.t13

13

OOC* solver scratch file

sequential access, binary

jidname.t14

14

OOC* solver scratch file

random access, binary

jidname.t15

15

OOC* solver scratch file

sequential access, binary

*OOC denotes Out-Of-Core solution.

Main Index

File Type

Appendix B Workspace Definition and the Sizing Option 1753 Running Marc

Table B-1

FORTRAN File Units Used by Marc (continued)

File Name

Unit

Description

File Type

jidname.t16

16

Post file, written out

sequential access, binary

ridname.t16

17

Post file to be read in from a previous job

sequential access, binary

jidname.t18

18

Mesh optimization correspondence table

sequential access, formatted

jidname.fem

18

From Marc to external mesher

sequential access, formatted

jidname.t19

19

Post file, written out

sequential access, formatted

ridname.t19

20

Post file to be read in from a previous job

sequential access, formatted

jidname_j_.dat

21

Temporary input file when cutback is used.

sequential access, formatted

jidname.t22

22

Subspace iteration scratch file.

random access, binary

jidname.t23

23

Fluid-solid interaction file.

sequential access, binary

pidname.t19

24

Temperature post file for

sequential access, formatted

CHANGE STATE or post file from previous analysis for PRE STATE or GLOBALLOCAL.

pidname.t16

25

Temperature post file for

sequential access, binary

CHANGE STATE or post file from previous analysis for PRE STATE or GLOBALLOCAL.

jidname.t29

29

Incremental backup file when

sequential access, binary

ELSTO, IBOOC is used, or

insufficient memory exists. sidname.t31

31

Substructure results file

sequential access, binary

jidname.t32

32

Secant method file

sequential access, binary

jidname.t33

33

Lanczos scratch file

sequential access, binary

sidname.t35

35

Substructure results file

sequential access, binary

material.mat

38

Material data base file

sequential access, formatted

jidname.g

39

Intergraph post file

sequential access, formatted

jidname.unv

40

I-DEAS Universal post file

sequential access, formatted

jidname.t41

41

Post file – Domain Decomposition

sequential access, binary

*OOC denotes Out-Of-Core solution.

Main Index

1754 Running Marc

Table B-1

FORTRAN File Units Used by Marc (continued)

File Name

Unit

Description

ridname.t42

42

Post file – Domain Decomposition

sequential access, formatted

jidname.opt

45

Duplicate loadcase data file during design optimization run

sequential access, formatted

jidname.t46

46

Design optimization scratch file sequential access, binary

jidname.trk

47

New particle tracking file

sequential access, formatted

ridname.trk

48

Old particle tracking file

sequential access, formatted

userspecified

49

User defaults file (see Appendix C: Default File)

sequential access, formatted

jidname.vfs

50

Viewfactors

sequential access, formatted

jidname.lck

51

Locking of post file

sequential access, formatted

jidname.cnt

52

Dynamic control file

sequential access, formatted

jidname.mfd

52

rebar - Marc Mentat interface

sequential access, formatted

jidnamebbc.mfd

52

beam-beam contact - Marc Mentat interface

sequential access, formatted

jidname_spline .mfd

52

Contact with spline - Marc Mentat interface

sequential access, formatted

jidname.seq

53

Sequence option

sequential access, formatted

jidname.rst

54

Loadcase data

sequential access, formatted

jidname.mesh

55

User supplied mesh

sequential access, formatted

jidname.feb

55

From 3-D mesher to Marc

sequential access, formatted

jidname.pass

56

Auto restart command line

sequential access, formatted

jidname.rms

57

2-D outline file for remeshing

sequential access, formatted

jidname.domesh

59

Lock files indicating meshing status

sequential access, formatted

jidname.doneme sh

“do mesh” and “done mesh”

jidname.sltrk

60

New streamline tracking file

sequential access, formatted

ridname.sltrk

61

Old streamline tracking file

sequential access, formatted

jidname.sts

67

Analysis progress reporting file sequential access, formatted

bbctch.noconv

80

beam-beam contact information sequential access, formatted

jidname.t81

81

multifrontal OOC scratch file

random access, binary

jidname.t82

82

multifrontal OOC scratch file

random access, binary

*OOC denotes Out-Of-Core solution.

Main Index

File Type

Appendix B Workspace Definition and the Sizing Option 1755 Running Marc

Table B-1

FORTRAN File Units Used by Marc (continued)

File Name

Unit

Description

File Type

jidname.t83

83

multifrontal OOC scratch file

sequential access, binary

jidname.t84

84

multifrontal OOC scratch file

sequential access, binary

jidname.t85

85

multifrontal DDM scratch file

sequential access, binary

jidname.t86

86

multifrontal DDM scratch file

sequential access, binary

jidname.t87

87

multifrontal DDM scratch file

sequential access, binary

jidname.t88

88

multifrontal DDM scratch file

sequential access, binary

jidname.t89

89

multifrontal DDM scratch file

sequential access, binary

jidname.t90

90

multifrontal DDM scratch file

sequential access, binary

jidname.fld

91

Forming Limit input file

sequential access, binary

filename.apt

94

APT file - machining option

sequential access, file

filename.ccl

95

CL file - machining option

sequential access, file

EXITMSG

97

Exit messages

sequential access, formatted

USRDEF

98

User global defaults file (see Appendix C: Default File)

sequential access, formatted

jidname.t08

99

Base restart file for DDM

sequential access, formatted

jidname.grd

103

Grid Force Balance Output

sequential access, formatted

user specified

110 - 119 Include files for input

sequential access, formatted

jidnam-dmig*

120 - 130 DMIG output files.

sequential access, formatted

jidname.hmr

N/A

Hypermesh results file

sequential access, binary C file

jidname.dump

N/A

Scratch file used during memory reallocation on Windows if in-core reallocation fails.

sequential access, binary C file

*OOC denotes Out-Of-Core solution. Marc input files should always be named job_name.dat, whereby the prefix job_name (or jidname, as in Table B-1; also see -jid below) is the name qualifier which you are free to choose. The suffix .dat is obligatory. To actually submit a Marc job from the command line, the following command should be used. The single input line is split over multiple lines for clarity: run_marc

Main Index

(required as minimum)

-jid

job_name

-rid

restart_name

-pid

post_name

1756 Running Marc

-sid

job_name containing solution of the external nodes

-prog

program_name

-user

user_subroutine_name

-save

save_user_executable

-queue

queue_name

-back

alternative for -queue

-ver

verification_flag

-def

data_name

-vf

viewfactor

-nprocd

domains

-nthread

threads

-dir

directory where job I/O takes place

-sdir

directory where job scratch files are placed

-itree

message passing type

-host

hostfile (for running over the network)

-comp

compatible machines on a network

-pq

Batch queue only: queue priority

-at

Batch queue only: delay time for start of job

-cpu

Batch queue only: cpu time limit

-autorst

autorestart_value.

Table B-2 describes the meanings of these input options and Table B-3 gives examples.

Main Index

Appendix B Workspace Definition and the Sizing Option 1757 Running Marc

Table B-2

run_marc Input Options*

Keyword

Options

Description

-jid (-j)

job_name

Input file (and, therefore, job) name identification. Requires job_name.dat for all programs except the curve fit and neutral plot programs.

-prog (-pr)

progname

Run marc with or without user subroutine.

Run the post file conversion program pldump. Run saved executable progname.marc from a previous job (see -user and -save). -user (-u)

user_name

User subroutine user_name.f is used to generate a new executable program called user_name.marc (see -save and -prog).

-save (-sa)

no

Do not save the new executable program user_name.marc.

yes

Save the executable program user_name.marc for a next time (see -prog and -user).

-rid -(r)

restart_name

For marc or progname: identification of previous job_name that created restart file.

-pid (-pi)

post_name

For marc or progname: identification of previous job_name that created the post file containing temperature data.

-sid (-si)

super

Identify the job that contains the solution to the external nodes of the superelement.

-queue (-q)

background

Run Marc in the background.

foreground

Run Marc in the foreground.

queue name

Submit to batch queue the queue name. Only available for machines with batch queue; for example, Convex, Cray. Queue names and submit command syntax can differ from site to site, adjust run_marc if necessary.

yes

Alternative for -queue: run Marc in the background.

no

Run Marc in the foreground.

yes

Ask for confirmation of these input options before starting the job. Start the job immediately.

-back (-b)

-ver (-v)

no -def (-de)

data_name

*Default options are shown in bold.

Main Index

File name containing user defined default data.

1758 Running Marc

Table B-2

run_marc Input Options* (continued)

Keyword

Options

Description

-vf

viewfactor

Name of file containing viewfactors for radiation viewfactor.vfs.

-nprocd

number

Number of domains for parallel processing.

-nprods

number

Number of domains for parallel processing using a Single Input file.

-nthread

number

Number of threads per task. Message passing tree type for domain decomposition.(Normally for internal debugging purposes only.)

-itree

-dir

directory_name

Pathname to directory where the job I/O should take place. Defaults to current directory.

-sdir

directory_name

Directory where scratch files are placed.

-host (-ho)

hostfile

Specify the name of the host file for running over a network (default is execution on one machine only in which case this option is not needed).

-comp (-co)

yes

When machines are compatible in a run over the network. Examples of compatible machines are:

no 1.

Two or more SGI, SUN, IBM, HP, and DEC with exactly the same processor type and OS.

2.

One SGI R8000/Irix 6.2 and one SGI R10000/Irix 6.5 machine.

3.

One SUN Ultra/Solaris 2.5 and one SUN Ultra/Solaris 2.6.

4.

One HP J Class/HPUX-10.20 and one HP C Class/HPUX-10.20.

This option is only needed when user subroutines are used. -ci

yes

Copy input files automatically to remote hosts for a network run, if necessary.

no -cr

yes

Copy post files automatically from remote hosts used for a network run, if necessary.

no -pq

0,1,2,etc

*Default options are shown in bold.

Main Index

Batch queue only: queue priority.

Appendix B Workspace Definition and the Sizing Option 1759 Running Marc

Table B-2

run_marc Input Options* (continued)

Keyword -at (-a)

Options date/time

Description Batch queue only: delay time for start of job. Syntax: January,1,1994,12:30 or:

today,5pm

-cpu

sec

Batch queue only: CPU time limit.

-autorst

0 or 1

If 0 when remeshing is required, the analysis program goes into a wait state until meshing is complete. If 1 when remeshing is required, the analysis program stops, the mesher begins, and the analysis program automatically restarts. Using the default procedure (0) uses more memory, but less I/O. Using the restart procedure (1), invokes the RESTART LAST option.

*Default options are shown in bold. Table B-3

Examples of Running Marc Jobs

Examples of Running Marc Jobs run_marc -jid e2x1

Description: Runs the job e2x1 in the background. The input file e2x1.dat resides in the current working directory.

run_marc -jid e2x14 -user u2x14 -save yes Runs the job e2x14 in the background,

using the user subroutine u2x14.f and the input file e2x14.dat. An executable program named u2x14.marc is saved after completion of the job.

Main Index

run_marc -jid e2x14a -prog u2x14

Runs the job e2x14a in the background using the executable produced by job e2x14.

run_marc -jid e3x2a -ver no -back no

Runs the job e3x2a in the foreground. The job runs immediately without verifying interactively.

run_marc -jid e3x2b -rid e3x2a

Performs a restart job in the background using the results of the previous job e3x2a.

run_marc -jid e3x29 -nprocd 2

Runs the two domain job in the background over two processors. Asks for verification.

1760 Running Marc

Main Index

Marc Volume C: Program Input Appendix C Default File

C

Main Index

Default File

1762 Marc Volume C: Program Input

Marc allows commonly used options to be stored in a file, so that it is not necessary to include them into the input file. This can be done in two ways. First, an organization could have a file that has options that are commonly used and shared by all users. The file name is defined by an environment variable named USRDEF (see Appendix B, Table B-1, Unit 98). This default file is read first. Second, you can specify a file when you are running an analysis. This is done when submitting a job using the -def option (see Appendix B, Table B-1, Unit 49). This file is read second. Values of data previously read can be overwritten. Your actual model data specified by -jid is read last. It can also overwrite previously defined data. The form of the file containing the defaults is the same as the standard Marc input file (it must include an END parameter and an END OPTION model definition option), but is restricted to selective options. These options include:

Parameters All parameters can be put in the default file.

Model Definition Options ADAPTIVE CONTROL CONVERT NO PRINT OPTIMIZE POST RESTART RESTART LAST SOLVER SUMMARY END OPTION

Main Index

Marc Volume C: Program Input Appendix D Control File

D

Main Index

Control File

1764 Marc Volume C: Program Input

Marc allows you to change the controls while the analysis is being performed. This is done by creating a file named jid.cnt where jid is the job id name. This file supports the following options. STOP

Stops the job as soon as the current operation is complete; goes through the Marc quit procedure to correctly close files.

STOP NEXT

Stops the job after the completion of the current increment. As you can change the restart frequency or post frequency, you can make sure that his last increment is saved.

CONTROL

Same as normal CONTROL history definition option; can be used to change tolerances, etc.

POST INCREMENT Same as normal POST INCREMENT option; can be used to change post tape frequency.

Main Index

RESTART IN

Same as normal RESTART INCREMENT option; can be used to change restart file frequency.

RESTART NOW

Writes a restart file at the end of the current increment.

ADAPT GLOBAL

Same as normal ADAPT GLOBAL option; can be used to change global remeshing settings.

MEMORY

Prints out a memory usage summary similar to the one printed at the end of the analysis.

TIMING

Prints out a timing summary similar to the one printed at the end of the analysis.

Marc Volume C: Program Input Appendix E Environment Variables

E

Main Index

Environment Variables

1766 Marc Volume C: Program Input

Marc has introduced user-controlled environment variables. They can be put into your login shell script or the run_marc shell script. However, it is not recommended that you change any of these default settings. These environment variables include: EXITMSG

Name of file containing centralized exit messages. The default is set in run_marc or run_marc.bat.

USRDEF

Name of file containing default input options/data. Change is not recommended. There is no default setting for this variable. The default input options/data are set internally in Marc.

AFMATDAT

Name of file containing material data base. The default is set in run_marc or run_marc.bat.

IBIG

Set to 1 for reading integers in I5 format, reals in F10 format. Set to 2 for reading integers in I10 format, reals in F20 format. This setting is not necessary if the EXTENDED parameter is used in the Marc input file. There is no default setting for this variable.

NPROCDS

Set to the number of domains when using the single input data file for parallel processing using DDM.

MSC_MMEM

Set to the maximum number of elements or nodes in the model. Default is one million.

If you need to reset these variables: For UNIX environments, you typically use csh and similar:

setenv USRDEF myfile.dat

sh, ksh and similar: USRDEF=myfile.dat export USRDEF For Windows, you typically define the environmental variable under the Control Panel or define at a Command Prompt: set USRDEF=myfile.dat

Main Index

Marc Volume C: Program Input Appendix F Material Database

F

Main Index

Material Database

1768 Marc Volume C: Program Input

To enter a new material into the database, the following steps would be performed. Please use the name convention followed in Marc to be certain that Marc reads your material data file properly. Using the convention, Marc exits with error if the file with the material name does not exist in the directory. The user-defined material data should use the prefix of usr_ and the file extension for the flow stress data should be .mat. Eight characters are allowed after usr_. For example, if you name your material as usr_material, you will create one use_material.mud or use_material.mfd file for Marc Mentat database and one flow stress data file, usr_material.mat for the analysis. You have to place the Marc Mentat database file in mentat/materials/directory. You can put the flow stress file in your current job directory or in marc/AF_flowmat directory if you want to share it with other users. Once you have done the preparation for the material database, you can use it in setting up your finite element model file in the future. Step 1 Collect all experimental data for the new material. This includes the following data: Young’s modulus Poisson’s ratio mass density instantaneous coefficient of thermal expansion yield stress conductivity specific heat latent heats (if applicable) The above properties may be dependent on the temperature. For the yield stress, it is dependent upon the equivalent plastic strain and optionally with strain rate. For the yield behavior of materials, the data must be in the form of Cauchy (true) stress versus logarithmic (true) strain. Therefore, if your data is in any other form, it is necessary to convert the data. Make sure your material data is in a consistent set of units. Step 2 Begin with a new database, use the FILES>NEW to clear out old data. Use SAVE AS to create a database with the material name you desire. Material name must be no more than eight characters. Step 3 Use the MATERIAL and TABLE menus to define the material properties except for the flow stress. Enter a 1 for the initial yield stress. Step 4 Save database for this material. This file will be called usr_material.mfd, or usr_material.mud.

Main Index

Appendix F Material Database 1769

Step 5 If you have the write permissions, move this database into mentat/materials/. Be sure that you don’t overwrite a material that has been previously defined. Step 6 Use the editor to define a file for the flow stress. This file should be called usr.material.mat. The structure of this file is as follows: Data structure in x_xxxxcc.mat 1. data card:

2. data card: where

3. data card:

Material name beginning in column one with the material identification number Format

: character*40

Example

: 3.2318 AlMgSi 1

ncurves, npoints, ntemps, nerates, number of : ncurves

: number of curves in input

(Max. 400)

npoints

: number of data points in each curve

(Max. 100)

ntemps

: number of reference temperatures

(Max. 20)

nerates

: number of reference strain rates

(Max. 20)

Format

: four integer in free format

Example

: 30, 13, 5, 6

eqpemin, eqpemax,

equivalent plastic strain range of the material described in this input eqpemin must be = 0.0, logarithmic strain measure

4. data card:

5. data card:

Main Index

Format

: two real in free format

Example

: 0.0, 7.0,

eratmin, eratmax,

equivalent plastic strain rate range of the material described in this input

Format

: two real in free format

Example

: 0.2, 10.0,

eratmin, eratmax,

Temperature range of the material described in this input

Format

: two real in free format

Example

: 350.0, 550.0,

1770 Marc Volume C: Program Input

The following data are repeated “ncurves” time (See card 2) 6. 0 data card :

documentation text, character*80

6. 1 data card :

icurve, temp., erate, sequential curve identification number, Temperature and equivalent plastic strain rate

6. 2 data card :

eqpmin, eq_stress,

logarithmic equivalent plastic strain and equivalent von mises (true) stress (first point)

6. n data card :

eqpmax, eq_stress,

logarithmic equivalent plastic strain and equivalent von mises (true) stress (npoint’th point, see card 2)

Format

:

character*80

Example

:

=== CURVE_01 Sig_Yiel, T=350. C, Eps_dot=0.2 1/s

Format

:

one integer, two real in free format

Example

:

1, 350.0, 0.20,

Format

:

two real in free format

Example

:

0.00, 78.0,

Format

:

two real in free format

Example

:

11.75, 59.0,0,

Format

:

two real in free format

Example

:

7.00, 52.0,

6.0 : 6.1 : 6.2 : 6.i : 6.n :

• • • Step 7 Save file and move file into marc/AF_flowmat/. Step 8 Your new material can now be read from: material properties>Read>Read other materials.

Main Index

Marc Volume C: Program Input Appendix G Flow Line FIle Format

G

Main Index

Flow Line File Format

1772 Marc Volume C: Program Input

This appendix defines the syntax of the flow line file if the user desires to specify an initial geometry for the flow lines. This data is entered into a file called jidnam.flw. All data entered is in free format. Format Format Fixed

Free

Data Entry Entry

1st data block 1st

I

Enter number of flow lines.

1st

I

Enter flow line ID.

2nd

I

Enter flow line type:

2nd data block

0 – straight line 1 – 2-D circle 3rd

I

Enter number of divisions of the flow line.

3rd data block For 2-D analysis, if flow line type = 0 (straight line) 1st

E

Starting point X-coordinate.

2nd

E

Starting point Y-coordinate.

3rd

E

Starting point Z-coordinate.

4th

E

End point X-coordinate.

5th

E

End point Y-coordinate.

6th

E

End point Z-coordinate.

For 2-D analysis, if flow line type = 1 (circle)

Note:

1st

E

Center point X-coordinate.

2nd

E

Center point Y-coordinate.

3rd

E

Center point Z-coordinate.

4th

E

Radius.

For 2-D flow line, the Z-coordinate equals 0.

For 3-D analysis, if flow line type = 0 (straight line)

Main Index

1st

E

Starting point X-coordinate.

2nd

E

Starting point Y-coordinate.

3rd

E

Starting point Z-coordinate.

Appendix G Flow Line FIle Format 1773

Format Fixed

Main Index

Free

Data Entry Entry

4th

E

End point X-coordinate.

5th

E

End point Y-coordinate.

6th

E

End point Z-coordinate.

1774 Marc Volume C: Program Input

Main Index

Marc Volume C: Program Input Appendix H: 3-D Remeshing Files

H

Main Index

3-D Remeshing Files

1776 Marc Volume C: Program Input

During the automatic 3-D remeshing phase, several files are created depending on the value of the verbose flag. These files may be viewed within the GUI to observe the remeshing process. The file names are based upon the following syntax, jid_bnn.fe?, where jid is the job name, nn is the body number, and the suffix fe? is described below.

.fem

This file is created by the analysis program containing the mesh of the deformed body, contact information, and meshing information. It is created every time there is a remeshing operation. Normally, the current working directory contains the last one created. If the verbose flag is set to greater than 20, files are saved for each meshing operation. They have the syntax jid_bnn_ll.fem. Here ll, is the number of times this body has been remeshed. Note that this is not the same as the increment number.

.fen

This file contains the previous edge information, which may be used to create the new mesh. If the verbose flag is set to greater than 20, files are saved for each meshing operation. They have the syntax jid_bnn_11.fen.

.feb

This file is created by the mesher containing the new meshing data. This includes the connectivity, coordinated, and contact node information. This is the mesh that MSC.SuperForm uses for the next increment.

.fee

This file contains information about what edges have been detected. If one observes small edges with discontinuities between them, one should increase the minimum edge length.

.fei

This file shows the surface of the workpiece after checking for penetration with the tools, but before remeshing. Only saved if verbose > 40.

.feik

This file shows the surface of tool number k. Only saved if verbose > 40.

.fek

This file contains the kernel of the mesh. The kernel should do a good job representing the volume of the body and be smooth. If the kernel is too far from the surface, it is necessary to reduce the target element size.

.fes

This file contains the surface of the final mesh. This is useful for quick visualization. Only saved if verbose > 2.

To visualize the intermediate files go into the FILE menu, and select NEW, and then type *read_marc filename.

Main Index

Marc Volume C: Program Input Appendix I: Units

I

Units

J

Main Index

Tables of Units

1778

1778 Marc Volume C: Program Input Tables of Units

Tables of Units Marc has no units built into it. Therefore, the units chosen must be self-consistent. The International System of units (SI) is an example of a self-consistent set of units but there are more sets of units supported by Marc tabulated below:

SI

mm/tonne/s/K or SI-mm

Imperial

US Common

Length

m

mm

in

in

Time

s

s

s

s

Quantity

Mass

kg

tonne

Force

kg-m/s2

tonne-mm/s2

N

N

kg/m3

tonne/mm3

2

lbf-s /in

pound (lb)

lbf

pound force (lbf)

lbf-s2/in4

lb/in3

lbf/in2

p.s.i.

lbf-in

lbf-in

Mg

Density

Mg/mm3 Stress

Energy

Temperature Spec. Heat Capacity

kg/m/s2

tonne/mm/s2

N/m2

MPa or N/mm2

kg-m2/s2

tonne-mm2/s2

J

MJ or N-mm

K

C

R

F

m2/s2/K

mm2/s2/C

in2/s2/R

Btu/lb/F

kg/s3/K

tonne/s3/C

lbf/in/s/R

Btu/in2/s/F

W/m2/C

N/s/°K/mm lbf/s/R

Btu/in/s/F

in/in/R

in/in/F

J/kg/C Heat Convection

Thermal Conductivity

Thermal Expansion

3

kg-m/s /K

tonne-mm/s3/C

W/m/C

N/s/K

m/m/K

mm/mm/C

Sometimes the standard units are not convenient to work with. For example, Young’s modulus is frequently specified in terms of MegaPascals (MPa or, equivalently,

Main Index

Appendix I: Units 1779 Tables of Units

N/mm2) where 1 Pascal is 1 N/m2. As shown in the table below, SI units are fundamental units with only conversion factors for stress and temperature.

Quantity

Common Units

to

SI Units

Multiplication Factor

Length

meter (m)

meter (m)

1.0

Time

second (s)

second (s)

1.0

Mass

kilogram (kg)

kilogram (kg)

1.0

kg/m3

1.0

kg-m/s2

1.0

Density Force

kg/m

3

Newton (N)

Stress Temperature Spec. Heat Capacity Heat Convection

2

MegaPascal (MPa)

kg/m/s

Celsius (C)

Kelvin (K)

J/kg/K W/m /C

Thermal Conductivity

W/m/C

Thermal Expansion

m/m/C

K = C + 273.15

m2 2

1.0

3

1.0

/s /K

2

1.0x106

kg/s /K kg-m/s3

/K

m/m/K

1.0 1.0

However, Imperial or American units can cause confusion since the naming conventions are not as clear as in the SI system. The American units are not consistent and require the user to give a conversion factor in coupled analyses. Below you can find a conversion table which will help you to derive Imperial units from common US units:

Quantity Length Time

to

Imperial

Multiplication Factor

inch (in)

inch (in)

1.0

second (s)

second (s)

1.0

pound (lb)

lbf-s /in

2.590076x10-3

lb/in3

lbf-s2/in4

2.590076x10-3

Force

pound force (lbf)

pound force (lbf)

1.0

Stress

lbf/in2

lbf/in

Fahrenheit (F)

Rankine (R)

Mass Density

Temperature Spec. Heat Capacity Heat Convection Thermal Conductivity Thermal Expansion

Main Index

Common Units

Btu/lb/F

2

in

2

2/s2/R

1.0 R = 459.67 + F 3.605299x106

Btu/in2/sec/F

lbf/in/s/R

9336.0

Btu/in/s/F

lbf/s/R

9336.0

in/in/F

in/in/R

1.0

1780 Marc Volume C: Program Input Tables of Units

The following is a table to convert from SI(mm) to either Imperial or common US units.

Quantity

SI(mm)

Length Time Mass Density

Imperial

mm

inch

s

s

Mg

lbf-s2/in

Mg/mm

3

2

lbf-s /in

Factor

US

Factor

inch

3.9370x10-2

1.0

s

1.0

5.7101

pound(lb)

3.9370x10

4

lb/in

3.6127x104

lbf/in2

145.04

lbf

0.22481

lbf-in

8.8508x10-3

F

9/5*C+32

Btu/lb/F

2.3883x10-10

N/mm2

lbf/in2

145.04

Force

N

lbf

0.22481

MJ(Nmm)

lbf-in

3

8.8508x10

F

2204.6

93.573

Stress Energy

-2

-3

Temperature

C

Spec. Heat Capacity

2 2

mm /s /C

in /s /F

Heat Convection

N/s/C/mm

lbf/in/s/F

3.1723

Btu/in2/s/F

3.3979x10-4

Heat Conductivity

N/s/C

lbf/s/F

0.12489

Btu/in/s/F

1.3377x10-5

Thermal Expansion

l/C

l/F

0.55556

l/F

0.55556

2 2

9/5*C+32 8.6111x10

-4

Finally, it is often necessary to convert between US and SI units for which the following table may used.

General Conversion Factors (to five significant digits) Quantity Length

US Units 1 in

0.025400 m

1 ft

0.30480 m

1 mile Area

Volume

Main Index

SI Equivalent

2

1609.3 m

1 in

0.64516x10-3 m2

1 ft2

0.092903 m2

1 acre

4046.9 m2

1 in3

0.016387x10-3 m3

1 ft3

0.028317 m3

1 US gallon

3.7854x10-3 m3

Appendix I: Units 1781 Tables of Units

Conversion Factors for Stress Analysis Quantity Density

US Units

SI Equivalent

1 slug/ft3 = 1 lbf s2/ft4

515.38 kg/m3

1 lbf s2/in4

10.687x106 kg/m3

Energy

1 ft lbf

1.3558 J (N m)

Force

1 lbf

4.4482 N (kg m/s2)

Mass

1 slug = 1 lbf s2/ft

14.594 kg (N s2/m)

1 lbf s2/in

175.13 kg

1 lb

0.45359 kg

Power

1 ft lbf/s

Pressure, Stress

1.3558 W (N m/s) 2

1 psi (lbf/in )

6894.8 Pa (N/m2)

Conversion Factors for Heat Transfer Analysis Conductivity

1 Btu/ft hr F

1.7307 W/m C

1 Btu/in hr F

20.769 W/m C

Density

1 lb/in3

27680.0 kg/m3

Energy

1 Btu

1055.1 J

Heat flux density

1 Btu/in hr

454.26 W/m2

Power

1 Btu/hr

0.29307 W

Specific heat

1 Btu/lb F

4186.8 J/kg C

Temperature

1F

5/9 C

Temp F

9/5 x Temp C + 32°

2

9/5 x Temp K–459.67° Important Constants Absolute zero

-459.67 F

-273.15 C

Acceleration of gravity

32.174 ft/s2

9.8066 m/s2

Stefan-Boltzmann constant

0.1714x10-8 Btu/hr ft2 R4

5.669x10-8 W/m2 K4

where R = F + 459.67

Main Index

where K = C + 273.15

1782 Marc Volume C: Program Input Tables of Units

Main Index

Marc Volume C: Program Input Appendix J: Parameters List

J

Parameters List

Links to Parameter $NO LIST

ABLATION ACCUMULATE ACOUSTIC ADAPTIVE ALIAS ALL POINTS ALLOCATE APPBC ASSUMED STRAIN AUTOMSET AUTOSPC

BEAM SECT BEARING

Main Index

1784 Marc Volume C: Program Input

Links to Parameter BOOC BOUNDARY CONDITIONS BUCKLE

CAVITY CENTROID COMMENT CONSTANT DILATATION COUPLE CREEP CURING

DECOUPLING DESIGN OPTIMIZATION DESIGN SENSITIVITY DIFFUSION DIST LOADS DYNAMIC

ELASTIC ELASTICITY ELECTRO ELEMENTS EL-MA ELSTO END EXTENDED

FEATURE FILMS FINITE FLUID FLUXES

Main Index

Appendix J: Parameters List 1785

Links to Parameter FOLLOW FOR FOURIER

HARMONIC HEAT

INCLUDE INPUT TAPE ISTRESS

JOULE

LARGE DISP LARGE STRAIN LINEAR LOAD COR LUMP

MACHINING MAGNETO MNF MPC-CHECK

NEW NO ECHO NO LOADCOR NOTES

OOC

PIEZO PLASTICITY PORE

Main Index

1786 Marc Volume C: Program Input

Links to Parameter PREALLOC PRINT PROCESSOR PYROLYSIS

RADIATION RBE RESPONSE RESTRICTOR REZONING R-P FLOW

SCALE SHELL SECT SIZING SPFLOW SS-ROLLING STATE VARS STOP STRUCTURAL

TABLE THERMAL TIE TITLE TSHEAR T-T-T

UNIT UPDATE USER

Main Index

Appendix J: Parameters List 1787

Links to Parameter VERSION VISCO ELAS

WELDING

Main Index

1788 Marc Volume C: Program Input

Main Index

Marc Volume C: Program Input Appendix K: Options List

K

Options List

Links to Options ACC CHANGE ACCUMULATE ACOUSTIC (with TABLE Input - Acoustic) ACOUSTIC ACTIVATE ACTUATOR ACTUATOR ADAPT GLOBAL (History Definition) ADAPT GLOBAL (Model Definition) ADAPTIVE ADD RIGID (2-D) ADD RIGID (3-D) ADD RIGID with TABLES (2-D) ADD RIGID with TABLES (3-D) ANISOTROPIC (Mechanical) ANISOTROPIC (Thermal) ANISOTROPIC (with TABLE Input - Diffusion)

Main Index

1790

Marc Volume C: Program Input

Links to Options ANISOTROPIC (with TABLE Input - Mechanical) ANISOTROPIC (with TABLE Input - Thermal) ANNEAL APPROACH ARRUDBOYCE (with TABLE Input) ARRUDBOYCE ASSEM LOAD ATTACH EDGE ATTACH FACE ATTACH NODE AUTO CREEP AUTO INCREMENT AUTO LOAD AUTO STEP AUTO THERM CREEP AUTO THERM AXITO3D (Model Definition)

B2GG, B2PP (History Definition) B2GG, B2PP (Model Definition) BEGIN SEQUENCE B-H RELATION (Electromagnetic) B-H RELATION (Magnetostatic) BLOCKS BOUNDARY BUCKLE INCREMENT BUCKLE

CASE COMBIN CAVITY DEFINITION CAVITY CFAST CHANGE PORE (History Definition) CHANGE PORE (Model Definition) CHANGE PORE (with TABLE Input - Model Definition)

Main Index

Appendix K: Options List 1791

Links to Options CHANGE RIGID CHANGE STATE (History Definition) CHANGE STATE (Model Definition) CHANGE STATE (with TABLE Input - Model Definition) CHANNEL COEFFICIENT COHESIVE (with TABLE Input) COHESIVE COMMENT COMPOSITE CONM1 CONM2 CONN FILL CONN GENER CONNECT CONNECTIVITY CHANGE CONNECTIVITY CONRAD GAP CONSTRAINT CONTACT (2-D) CONTACT (3-D) CONTACT CHANGE CONTACT NODE (History Definition) CONTACT NODE (Model Definition) CONTACT TABLE (History Definition) CONTACT TABLE (Model Definition) CONTACT TABLE with TABLES (History Definition) CONTACT TABLE with TABLES (Model Definition) CONTACT with TABLES (2-D) CONTACT with TABLES (3-D) CONTINUE (History Definition) CONTINUE (Rezoning) CONTROL (Electromagnetostatic) CONTROL (Fluid) CONTROL (Fluid-Solid)

Main Index

1792

Marc Volume C: Program Input

Links to Options CONTROL (Heat Transfer - History Definition) CONTROL (Heat Transfer - Model Definition) CONTROL (Hydrodynamic) CONTROL (Magnetostatic) CONTROL (Mechanical - History Definition) CONTROL (Mechanical - Model Definition) CONVERT COORD SYSTEM COORDINATE CHANGE COORDINATES CORNERING AXIS COUPLING REGION CRACK DATA (with TABLE Input) CRACK DATA CREEP (with TABLE Input) CREEP INCREMENT CREEP CURE RATE CURE SHRINKAGE CURVES CWELD CYCLIC SYMMETRY CYLINDRICAL

DAMAGE DAMPING COMPONENTS DAMPING DEACT GLUE (Model Definition) DEACTIVATE (History Definition) DEACTIVATE (Model Definition) DEFINE (Mesh2D Block Type) DEFINE (Sets) DELAMINATION DENSITY EFFECTS DESIGN DISPLACEMENT CONSTRAINTS

Main Index

Appendix K: Options List 1793

Links to Options DESIGN FREQUENCY CONSTRAINTS DESIGN OBJECTIVE DESIGN STRAIN CONSTRAINTS DESIGN STRESS CONSTRAINTS DESIGN VARIABLES DISP CHANGE DIST CHARGE (Electromagnetic - History Definition) DIST CHARGE (Electromagnetic - Model Definition) DIST CHARGE (Piezoelectric - History Definition) DIST CHARGES (Electrostatic) DIST CHARGES (Piezoelectric - Model Definition) DIST CHARGES (with TABLE Input - Electromagnetic) DIST CHARGES (with TABLE Input - Electrosatatic) DIST CHARGES (with TABLE Input - Piezoelectric) DIST CURRENT (Electromagnetic - History Definition) DIST CURRENT (Electromagnetic - Model Definition) DIST CURRENT (Joule Heating - History Definition) DIST CURRENT (Joule Heating - Model Definition) DIST CURRENT (Magnetostatic) DIST CURRENT (Magnetostatic) DIST CURRENT (with TABLE Input - Electromagnetic) DIST CURRENT (with TABLE Input - Joule Heating) DIST CURRENT (with TABLE Input - Magnetostatic) DIST FLUXES (History Definition) DIST FLUXES (Model Definition) DIST FLUXES (with TABLE Input - Model Definition) DIST LOADS (History Definition) DIST LOADS (Model Definition) DIST LOADS (with TABLE Input - Model Definition) DIST MASS (Diffusion) DIST MASS (with TABLE Input - Diffusion) DIST SOURCES (Acoustic - Model Definition) DIST SOURCES (History Definition) DIST SOURCES (with TABLE Input - Acoustic) DMIG

Main Index

1794

Marc Volume C: Program Input

Links to Options DMIG-OUT (History Definition) DMIG-OUT (Model Definition) DYNAMIC CHANGE (Dynamic) DYNAMIC CHANGE (Electromagnetic - History Definition) ELEMENT SORT (History Definition) ELEMENT SORT (Model Definition) EMISSIVITY END OPTION END REZONE END SEQUENCE ERROR ESTIMATE EXCLUDE (History Definition) EXCLUDE (Model Definition) EXTRAPOLATE

FACE IDS FAIL DATA (with TABLE Input) FAIL DATA FILMS (History Definition) FILMS (Model Definition) FILMS (with TABLE Input - Model Definition) FIXED ACCE FIXED DISP (Fluid) FIXED DISP (Mechanical) FIXED DISP (with TABLE Input - Mechanical) FIXED EL-POT (Electrostatic) FIXED EL-POT (with TABLE Input - Electrostatic) FIXED MG-POT (Magnetostatic) FIXED MG-POT (with TABLE Input - Magnetostatic) FIXED POTENTIAL (Electromagnetic) FIXED POTENTIAL (Electrostatic) FIXED POTENTIAL (Magnetostatic) FIXED POTENTIAL (Piezoelectric - Model Definition) FIXED POTENTIAL (with TABLE Input - Electromagnetic)

Main Index

Appendix K: Options List 1795

Links to Options FIXED POTENTIAL (with TABLE Input - Electrostatic) FIXED POTENTIAL (with TABLE Input - Magnetostatic) FIXED POTENTIAL (with TABLE Input - Piezoelectric) FIXED PRESSURE (Acoustic) FIXED PRESSURE (with TABLE Input - Acoustic) FIXED PRESSURE (with TABLE Input - Diffusion) FIXED TEMPERATURE (with TABLE Input) FIXED TEMPERATURE FIXED VELOCITY (with TABLE Input - Fluid) FIXED VELOCITY FIXED VOLTAGE (with TABLE Input - Joule Heating) FIXED VOLTAGE FLOW LINE FLUID DRAG FLUID SOLID FOAM (with TABLE Input) FOAM FORCDT FORMING LIMIT FOUNDATION (History Definition) FOUNDATION (Model Definition) FOUNDATION (with TABLE Input - Model Definition) FOURIER FXORD

GAP CHANGE GAP DATA CHANGE GAP DATA GASKET GENERATE GENT (with TABLE Input) GENT GEOMETRY CHANGE GEOMETRY GLOBALLOCAL

Main Index

1796

Marc Volume C: Program Input

Links to Options GRAIN SIZE GRID FORCE (History Definition) GRID FORCE (Model Definition)

HARMONIC (Acoustic - History Definition) HARMONIC (Dynamic) HARMONIC (Electromagnetic - History Definition) HOLD NODES HYPERMESH HYPOELASTIC (with TABLE Input) HYPOELASTIC

INCLUDE (History Definition) INCLUDE (Model Definition) INERTIA RELIEF (History Definition) INERTIA RELIEF (Model Definition) INIT CURE (with TABLE Input) INIT CURE INIT STRESS (with TABLE Input) INIT STRESS INITIAL DENSITY (Heat Transfer) INITIAL DISP (with TABLE Input) INITIAL DISP INITIAL PC (with TABLE Input) INITIAL PC INITIAL PLASTIC STRAIN (with TABLE Input) INITIAL PLASTIC STRAIN INITIAL PORE (with TABLE Input) INITIAL PORE INITIAL POROSITY (with TABLE input) INITIAL POROSITY INITIAL PRESSURE (with TABLE Input - Diffusion) INITIAL PYROLYSIS INITIAL STATE (with TABLE Input) INITIAL STATE

Main Index

Appendix K: Options List 1797

Links to Options INITIAL TEMP (Heat Transfer) INITIAL TEMP (Thermal Stress) INITIAL TEMP (with TABLE Input - Heat Transfer) INITIAL TEMP (with TABLE Input - Thermal Stress) INITIAL VEL (with TABLE Input) INITIAL VEL INITIAL VOID RATIO (with TABLE Input) INITIAL VOID RATIO INSERT IRM ISLAND REMOVAL ISOTROPIC (Acoustic) ISOTROPIC (Electromagnetic) ISOTROPIC (Electrostatic) ISOTROPIC (Fluid) ISOTROPIC (Heat Transfer) ISOTROPIC (Hydrodynamic) ISOTROPIC (Magnetostatic) ISOTROPIC (Stress) ISOTROPIC (with TABLE Input - Acoustic) ISOTROPIC (with TABLE Input - Diffusion) ISOTROPIC (with TABLE Input - Electromagnetic) ISOTROPIC (with TABLE Input - Electrostatic) ISOTROPIC (with TABLE Input - Fluid) ISOTROPIC (with TABLE Input - Hydrodynamic) ISOTROPIC (with TABLE Input - Magnetostatic) ISOTROPIC (with TABLE Input - Stress) ISOTROPIC (with TABLE Input - Thermal) J-INTEGRAL JOULE K2GG, K2PP (History Definition) K2GG, K2PP (Model Definition)

Main Index

1798

Marc Volume C: Program Input

Links to Options LATENT HEAT LOADCASE (History Definition) LOADCASE (Model Definition) LORENZI M2GG, M2PP (History Definition) M2GG, M2PP (Model Definition) MANY TYPES MAPPER MASSES MATERIAL DATA MERGE (Model Definition) MERGE SELECTIVE MESH2D MIXTURE MNF UNITS MODAL INCREMENT MODAL SHAPE MOONEY (with TABLE Input) MOONEY MOTION CHANGE MOVE (History Definition) MOVE (Rezoning) NEW (History Definition) NEW (Model Definition) NLELAST NO ELEM SORT (History Definition) NO ELEM SORT (Model Definition) NO NODE SORT (History Definition) NO NODE SORT (Model Definition) NO PRINT (History Definition) NO PRINT (Model Definition) NO PRINT CONTACT (History Definition) NO PRINT CONTACT (Model Definition)

Main Index

Appendix K: Options List 1799

Links to Options NO PRINT SPRING (History Definition) NO PRINT SPRING (Model Definition) NO SUMMARY (History Definition) NO SUMMARY (Model Definition) NODAL THICKNESS NODE CIRCLE NODE FILL NODE GENER NODE MERGE NODE SORT (History Definition) NODE SORT (Model Definition) OGDEN (with TABLE Input) OGDEN OPTIMIZE ORIENTATION CHANGE ORIENTATION ORTHO TEMP (Structural) ORTHO TEMP (Thermal) ORTHOTROPIC (Electrical) ORTHOTROPIC (Electromagnetic) ORTHOTROPIC (Magnetostatic) ORTHOTROPIC (Mechanical) ORTHOTROPIC (Thermal) ORTHOTROPIC (with TABLE Input - Diffusion) ORTHOTROPIC (with TABLE Input - Electromagnetic) ORTHOTROPIC (with TABLE Input - Electrostatic) ORTHOTROPIC (with TABLE Input - Magnetostatic) ORTHOTROPIC (with TABLE Input - Mechanical) ORTHOTROPIC (with TABLE Input - Thermal) P2G (History Definition) P2G (Model Definition) PARAMETERS (History Definition) PARAMETERS (Model Definition) PBUSH

Main Index

1800

Marc Volume C: Program Input

Links to Options PERMANENT (Electromagnetic) PERMANENT (Magnetostatic) PERMANENT (with TABLE Input - Magnetostatic) PFAST PHI-COEFFICIENTS PIEZOELECTRIC (Piezoelectric - Model Definition) PIEZOELECTRIC (with TABLE Input - Piezoelectric) PIN CODE POINT CHARGE (Piezoelectric - History Definition) POINT CHARGE (Piezoelectric - Model Definition) POINT CHARGE (with TABLE Input - Electrostatic) POINT CHARGE (with TABLE Input - Piezoelectric) POINT CHARGE POINT CURRENT (Electromagnetic - History Definition) POINT CURRENT (Joule - History Definition) POINT CURRENT (Joule - Model Definition) POINT CURRENT (Magnetostatic) POINT CURRENT (with TABLE Input - Joule Heating) POINT CURRENT (with TABLE Input - Magnetostatic) POINT CURRENT-CHARGE (with TABLE Input - Electromagnetic) POINT CURRENT-CHARGE POINT FLUX (History Definition) POINT FLUX (Model Definition) POINT FLUX (with TABLE Input - Model Definition) POINT LOAD (History Definition) POINT LOAD (Model Definition) POINT LOAD (with TABLE Input - Model Definition) POINT MASS (Diffusion) POINT MASS (with TABLE Input - Diffusion) POINT SOURCE (Acoustic - History Definition) POINT SOURCE (Acoustic - Model Definition) POINT SOURCE (with TABLE Input - Acoustic) POINT TEMP (History Definition) POINT TEMP (Model Definition) POINT TEMP (with TABLE Input - Model Definition)

Main Index

Appendix K: Options List 1801

Links to Options POINTS POROSITY CHANGE (with TABLE Input - Model Definition) POROSITY CHANGE POST (History Definition) POST (Model Definition) POST INCREMENT POTENTIAL CHANGE (Piezoelectric - History Definition) POTENTIAL CHANGE POWDER (with TABLE input) POWDER PRE STATE PRESS CHANGE PRESS FILM (Model Definition) PRESS FILM (with TABLE Input) PRINT CHOICE (History Definition) PRINT CHOICE (Model Definition) PRINT CHOICE (Rezoning) PRINT CONTACT (History Definition) PRINT CONTACT (Model Definition) PRINT ELEMENT (History Definition) PRINT ELEMENT (Model Definition) PRINT NODE (History Definition) PRINT NODE (Model Definition) PRINT SPRING (History Definition) PRINT SPRING (Model Definition) PRINT STREAMLINE PRINT VMASS (History Definition) PRINT VMASS (Model Definition) PROPORTIONAL INCREMENT PRTCONNECT PSHELL PWELD QVECT (with TABLE Input - Model Definition)

Main Index

1802

Marc Volume C: Program Input

Links to Options RAD-CAVITY RADIATING CAVITY RBE2 RBE3 READ FILE REAUTO REBAR RECEDING SURFACE RECOVER REGION (Fluid) RELATIVE DENSITY RELEASE NODE RELEASE RESET TIME RESPONSE SPECTRUM RESTART INCREMENT RESTART LAST RESTART RESTRICTOR (with TABLE Input - Model Definition) RESTRICTOR REZONE ROTATION A RROD

SDRC SECTIONING (Rezoning) SERVO LINK SHAPE MEMORY (with TABLE Input) SHAPE MEMORY SHELL TRANSFORMATION SHIFT FUNCTION SINK POINTS (with TABLE Input - Model Definition) SOIL (with TABLE Input) SOIL SOLVER (History Definition)

Main Index

Appendix K: Options List 1803

Links to Options SOLVER (Model Definition) SPECIFIC WEIGHT SPECIFIED NODES SPECTRUM SPLINE (History Definition) SPLINE (Model Definition) SPLIT BODIES SPRINGS SS-ROLLING START NUMBER STEADY STATE (Electrostatic) STEADY STATE (Heat Transfer) STEADY STATE (Magnetostatic) STIFFNS COMPONENTS STIFSCALE STRAIN RATE (Fluid) STRAIN RATE (Material Properties) STREAM DEFINITION STRING SUMMARY (History Definition) SUMMARY (Model Definition) SUPERELEM (DMIG Applications - History Definition) SUPERELEM (DMIG Applications - Model Definition) SUPERELEM (History Definition) SUPERELEM (Model Definition) SUPERPLASTIC SURFACE ENERGY SURFACES SWLDPRM SYMMETRY SYNCHRONIZED

TABLE TEMP CHANGE TEMPERATURE EFFECTS (Coupled Fluid-Thermal)

Main Index

1804

Marc Volume C: Program Input

Links to Options TEMPERATURE EFFECTS (Coupled Thermal-Stress) TEMPERATURE EFFECTS (Heat Transfer) TEMPERATURE EFFECTS (Hydrodynamic) TEMPERATURE EFFECTS (Stress) TERMINATE THERMAL CONTACT (2-D) THERMAL CONTACT (3-D) THERMAL CONTACT with TABLES (2-D) THERMAL CONTACT with TABLES (3-D) THERMAL LOADS (History Definition) THERMAL LOADS (Model Definition) THERMO-PORE THICKNESS (with TABLE Input - Model Definition) THICKNESS THICKNS CHANGE THROAT TIME STEP TIME-TEMP TITLE TRACK STREAMLINE TRACK TRANSFORMATION TRANSIENT TYING CHANGE TYING

UDUMP UFCONN UFRICTION UFRORD UFXORD UHTCOEF UHTCON UMOTION URCONN

Main Index

Appendix K: Options List 1805

Links to Options USDATA UTRANFORM VCCT VELOCITY (Convective Heat Transfer) VELOCITY (Hydrodynamic) VELOCITY (with TABLE Input - Convective Heat Transfer) VELOCITY (with TABLE Input - Hydrodynamic) VELOCITY CHANGE VIEW FACTOR VISCEL EXP VISCELFOAM VISCELMOON VISCELOGDEN VISCELORTH VISCELPROP VOID CHANGE (with TABLE Input - Model Definition) VOID CHANGE VOLTAGE CHANGE

WELD FILL (History Definition) WELD FILL (Model Definition) WELD FLUX (History Definition) WELD FLUX (Model Definition) WELD FLUX (with TABLE Input - Model Definition) WELD PATH (History Definition) WELD PATH (Model Definition) WORK HARD WRITE FILE WRITE

Main Index

1806

Marc Volume C: Program Input

Main Index