Marc 2008 R1 Volume A: Theory And User Information

Marc 2008 r1 ®

Volume A: Theory and User Information

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-A

Main Index

Contents Marc Volume A: Theory and User Information

Contents

Preface About This Manual

20

Purpose of Volume A

20

Contents of Volume A

20

How to Use This Manual

1

21

The Marc System Marc Programs 24 Marc for Analysis 24 Marc Mentat or MD Patran for GUI Structure of Marc 25 Procedure Library 25 Material Library 26 Element Library 26 Program Function Library

26

Features and Benefits of Marc

2

25

26

Program Initiation Marc Host Systems

30

Workspace Requirements 31 Marc Workspace Requirements 31 File Units

33

Program Initiation

36

Examples of Running Marc Jobs Example 1: 39 Example 2: 39

Main Index

39

4 Marc Volume A: Theory and User Information

Example 3: Example 4: Example 5: Example 6: Example 7: Example 8: Example 9:

3

39 39 39 39 39 40 40

Data Entry Input Conventions 42 Input of List of Items 43 Examples of Lists 45 Table Driven Input Table Input 46 Parameters

45

50

Model Definition Options

50

History Definition Options REZONE Option

4

50

51

Introduction to Mesh Definition Direct Input 54 Element Connectivity Data 55 Nodal Coordinate Data 59 Activate/Deactivate 59 User Subroutine Input

59

MESH2D 59 Block Definition 60 Merging of Nodes 60 Block Types 60 Symmetry, Weighting, and Constraints Additional Options 64 Marc Mentat

Main Index

64

63

CONTENTS 5

FXORD Option 65 Major Classes of the FXORD Option 65 Recommendations on Use of the FXORD Option Incremental Mesh Generators Bandwidth Optimization Rezoning

69

69

70

71

Substructure 71 Technical Background 72 Scaling Element Stiffness 74 BEAM SECT Parameter 74 Orientation of the Section in Space Definition of the Section 74 Error Analysis

79

Local Adaptivity 79 Number of Elements Created Boundary Conditions 81 Location of New Nodes 81 Adaptive Criteria 82 Automatic Global Remeshing Remeshing Criteria 90 Remeshing Techniques 91 MD Patran Tetrahedral Mesher

5

74

80

85

93

Structural Procedure Library Linear Analysis 100 Accuracy 101 Error Estimates 102 Adaptive Meshing 102 Fourier Analysis 102 Nonlinear Analysis 105 Geometric Nonlinearities 109 Eulerian Formulation 118 Arbitrary Eulerian-Lagrangian (AEL) Formulation Nonlinear Boundary Conditions 119 Buckling Analysis 122

Main Index

119

6 Marc Volume A: Theory and User Information

Perturbation Analysis 123 Computational Procedures for Elastic-Plastic Analysis 128 AUTO THERM CREEP (Automatic Thermally Loaded Elastic-Creep/ Elastic-Plastic-Creep Stress Analysis) 145 Viscoelasticity 145 Viscoplasticity 146 Fracture Mechanics 147 Linear Fracture Mechanics 148 Nonlinear Fracture Mechanics 150 Numerical Evaluation of the J-integral 151 Numerical Evaluation of the Energy Release Rate with the VCCT Method Automatic Crack Propagation 159 Dynamic Fracture Methodology 163 Modeling Considerations 164 Dynamic Crack Propagation 164 Mesh Splitting

165

Dynamics 165 Eigenvalue Analysis 166 Transient Analysis 168 Harmonic Response 181 Spectrum Response 184 Inertia Relief 185 Rigid Body Mode Evaluation

185

Rigid-Plastic Flow 188 Steady State Analysis 189 Transient Analysis 190 Technical Background 190 Superplasticity

191

Soil Analysis 193 Technical Formulation Mechanical Wear

194 197

Design Sensitivity Analysis

200

Design Optimization 202 Approximation of Response Functions Over the Design Space 204 Improvement of the Approximation 206 The Optimization Algorithm 206 Marc User Interface for Sensitivity Analysis and Optimization 207

Main Index

153

CONTENTS 7

Defined Initial State with Result Data from Previous Analysis (including AXITO3D) 209 Load and Displacement Boundary Conditions Transfer for PRE STATE Option 210 Steady State Rolling Analysis 211 Kinematics 211 Inertia Effect 213 Rolling Contact 213 Steady State Rolling with Marc 213 Structural Zooming Analysis 214 Element Types Supported 215 Cure-Thermal-Mechanically Coupled Analysis Cure Kinetics 217 Cure Shrinkage Strain 219 References

6

216

221

Nonstructural Procedure Library Heat Transfer 226 Thermal Contact 227 Convergence Controls 228 Steady State Analysis 228 Transient Analysis 228 Temperature Effects 230 Initial Conditions 231 Boundary Conditions 231 Surface Energy 236 Thermochemical Ablation and Surface Energy Balance Mathematical Presentation 237 Mechanical Erosion 244 Mechanical Erosion by Other Actions 245 Pyrolysis 245 Coking 249 Presentation of the Energy Equation 253 Ablation 255 Welding 265 Radiation 271 Conrad Gap 285 Channel 286 Output 287

Main Index

237

8 Marc Volume A: Theory and User Information

Diffusion 289 Technical Background

289

Hydrodynamic Bearing 291 Technical Background 293 Electrostatic Analysis 295 Technical Background 297 Magnetostatic Analysis 300 Technical Background 301 Electromagnetic Analysis Technical Background 306

304

Piezoelectric Analysis 309 Technical Background 310 Strain Based Piezoelectric Coupling Acoustic Analysis 312 Rigid Cavity Acoustic Analysis Technical Background 313

312

312

Fluid Mechanics 314 Finite Element Formulation 317 Penalty Method 319 Steady State Analysis 320 Transient Analysis 320 Solid Analysis 320 Solution of Coupled Problems in Fluids Degrees of Freedom 321 Element Types 322

321

Coupled Analyses 323 Thermal Mechanically Coupled Analysis 326 Coupled Acoustic-Structural Analysis 328 Fluid/Solid Interaction – Added Mass Approach 331 Coupled Electrostatic-Structural Analysis 333 Coupled Thermal-Electrical Analysis (Joule Heating) 335 Coupled Electrical-Thermal-Mechanical Analysis 337 Coupled Electromagnetic-Thermal Analysis 341 References

Main Index

343

CONTENTS 9

7

Material Library Linear Elastic Material

346

Composite Material 348 Layered Materials 349 Classical Lamination Theory for Multi-Layered Shells 352 Material Preferred Direction 353 Material Dependent Failure Criteria 357 Interlaminar Shear for Thick Shell, Beam, Solid Shell and 3D Composite Brick Elements 369 The generalized stiffness matrix for the complete section excluding transverse shear terms is given by: 370 Interlaminar Stresses for Continuum Composite Elements 371 Progressive Composite Failure 372 Mixture Model 374 Gasket 378 Constitutive Model

378

Nonlinear Hypoelastic Material

383

Thermo-Mechanical Shape Memory Model 404 Transformation Induced Deformation 406 Constitutive Theory 407 Phase Transformation Strains 407 Experimental Data Fitting for Thermo-mechanical Shape Memory Alloy Mechanical Shape Memory Model 413 Experimental Data Fitting for Mechanical Shape Memory Alloy 417 Conversion from Thermo-Mechanical to Mechanical SMA 418 Elastomer 419 Updated Lagrange Formulation for Nonlinear Elasticity

428

Time-independent Inelastic Behavior 429 Yield Conditions 432 Mohr-Coulomb Material (Hydrostatic Stress Dependence) 437 Buyukozturk Criterion (Hydrostatic Stress Dependence) 439 Powder Material 439 Work or Strain Hardening 441 Flow Rule 446 Constitutive Relations 447 Time-independent Cyclic Plasticity 449

Main Index

409

10 Marc Volume A: Theory and User Information

Time-dependent Inelastic Behavior 453 Creep (Maxwell Model) 456 Oak Ridge National Laboratory Laws 461 Swelling 462 Viscoplasticity (Explicit Formulation) 463 Time-dependent Cyclic Plasticity 464 Viscoelastic Material 465 Narayanaswamy Model 476 Temperature Effects and Coefficient of Thermal Expansion Piecewise Linear Representation 480 Temperature-Dependent Creep 481 Coefficient of Thermal Expansion 482 Time-Temperature-Transformation

479

482

Low Tension Material 485 Uniaxial Cracking Data 485 Low Tension Cracking 486 Tension Softening 486 Crack Closure 487 Crushing 487 Analysis 487 Soil Model 487 Elastic Models 488 Cam-Clay Model 488 Evaluation of Soil Parameters for the Critical State Soil Model Damage Models 499 Ductile Metals 499 Elastomers 501 Cohesive Zone Modeling

504

Nonstructural Materials 512 Heat Transfer Analysis 512 Piezoelectric Analysis 512 Thermo-Electrical Analysis 512 Coupled Electrical-Thermal-Mechanical Analysis 512 Hydrodynamic Bearing Analysis 513 Fluid/Solid Interaction Analysis – Added Mass Approach Electrostatic Analysis 513 Magnetostatic Analysis 513 Electromagnetic Analysis 513

Main Index

513

490

CONTENTS 11

Coupled Electrostatic-Structural Acoustic Analysis 513 Fluid Analysis 514 References

8

513

514

Contact Definition of Contact Bodies Numbering of Contact Bodies

518 521

Motion of Bodies 524 Initial Conditions 526 Detection of Contact 526 Shell Contact 528 Neighbor Relations 529 Implementation of Constraints

530

Friction Modeling 532 Coulomb Friction 533 Shear Friction 542 Glue Model 543 Deact Glue 544 Breaking Glue 544 Separation 544 Release 545 Coupled Analysis Thermal Contact Joule Heating

545 548 548

Contact in an Electrostatic or Piezoelectric Analysis Contact in Magnetostatic Analysis

550

Contact in Electromagnetic Analysis Contact in Soil Analysis

550

Contact in an Acoustic Analysis

Main Index

550

550

549

12 Marc Volume A: Theory and User Information

Element Considerations 2-D Beams 551 3-D Beams 551 Shell Elements 553 Dynamic Impact

550

553

Global Adaptive Meshing and Rezoning Adaptive Meshing

554

Result Evaluation

555

Tolerance Values

556

554

Numerical and Mathematical Aspects of Contact Lagrange Multipliers 557 Penalty Methods 557 Hybrid and Mixed Methods 558 Direct Constraints 558 Lagrange Multiplier Procedure 558 Direct Constraint Procedure 559 Solution Strategy for Deformable Contact 566 Iterative Penetration Checking 567 Instabilities 568 References

9

557

568

Boundary Conditions Loading 571 Loading Types 571 Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations 580 Mechanical Loads 584 Fluid Drag and Wave Loads 587 Cavity Pressure Loading 588 Cyclic Loading 593 Thermal Loads 593 Initial Stress and Initial Plastic Strain 594 Heat Fluxes 595 Mass Fluxes and Restrictors 596 Electrical Currents 597 Electrostatic Charges 597 Acoustic Sources 597

Main Index

CONTENTS 13

Piezoelectric Loads 598 Electrostatic-Structural Loads 598 Magnetostatic Currents 598 Electromagnetic Currents and Charges Kinematic Constraints 599 Boundary Conditions 599 Transformation of Degree of Freedom Shell Transformation 601 Tying Constraint 604 Rigid Link Constraint 613 Shell-to-Solid Tying 614 Rigid Tying to a Surface Patch 615 Overclosure Tying 617 Insert 621 AUTOMSET 621 Support Conditions 621 Bushings 622 Cyclic Symmetry 625 Nastran RBE2 and RBE3 628 Beam - Shell Offsets 632 Pin Code for Beam Elements 636

598

600

Mesh Independent Connection Methods 637 CWELD patch-to-patch connections 639 Parameters for the Projection Process 643 Internal Constraints to Connect Two Surfaces 645 Multiple Surface Connections 646 Coupled Thermo-mechanical Analysis 646 Rules for usage of the GS-node or the GA-, GB-node Pair in the Projection Process 647 CWELD Properties 649 CWELD Input Styles 652 CWELD Error and Warning Messages 653 CWELD Output 655 Two Dimensional Models 655 CFAST Connections 656 CFAST Properties 656 SWLDPRM, Special CWELD/CFAST Parameters 657

Main Index

14 Marc Volume A: Theory and User Information

10 Element Library Truss Elements

666

Membrane Elements

666

Continuum Elements

666

Beam Elements

667

Plate Elements

668

Shell Elements

668

Heat Transfer Elements 668 Acoustic Analysis 669 Electrostatic Analysis 669 Coupled Electrostatic-Structural 669 Fluid/Solid Interaction 669 Hydrodynamic Bearing Analysis 670 Magnetostatic Analysis 670 Electromagnetic Analysis Soil Analysis Fluid Analysis

670

670 670

Piezoelectric Analysis

670

Special Elements 671 Gap-and-Friction Elements 671 Pipe-bend Element 671 Curved-pipe Element 671 Shear Panel Element 671 Cable Element 671 Rebar Elements 672 Interface Elements 672 Incompressible Elements Large Strain Elasticity 672 Large Strain Plasticity 673 Rigid-Plastic Flow 673

672

Constant Dilatation Elements Reduced Integration Elements Continuum Composite Elements

Main Index

673 673 674

CONTENTS 15

Fourier Elements

674

Semi-infinite Elements

674

Cavity Surface Elements

674

Assumed Strain Formulation

675

Follow Force Stiffness Contribution Explicit Dynamics

675

675

Adaptive Mesh Refinement

675

11 Solution Procedures for Nonlinear Systems Considerations for Nonlinear Analysis Behavior of Nonlinear Materials 679 Scaling the Elastic Solution 679 Load Incrementation 679 Selecting Load Increment Size 681 Fixed Load Incrementation 681 Arc Length Method 682 Residual Load Correction 690 Restarting the Analysis 691 Full Newton-Raphson Algorithm

692

Modified Newton-Raphson Algorithm Strain Correction Method Direct Substitution

695

Convergence Controls Singularity Ratio AutoSPC 706

694

695

Arc-length Methods

702

705

Solution of Linear Equations 706 Direct Methods 707 Iterative Methods 707 Mixed Direct-Iterative Solver 708 Preconditioners 708 Storage Methods 709

Main Index

678

693

16 Marc Volume A: Theory and User Information

Nonsymmetric Systems 709 Complex Systems 709 Iterative Solvers 709 Basic Theory 710 Flow Diagram Remarks

711

712

References

713

12 Output Results Workspace Information Increment Information Summary of Loads 720 Timing Information 720 Singularity Ratio 720 Convergence 721

716 720

Selective Printout 721 Options 721 Grid Force Balance 722 User Subroutines 723 Restart

723

Element Information 723 Mentat Computed Element Results 725 Solid (Continuum) Elements 725 Shell Elements 725 Beam Elements 726 Gap Elements 727 Linear and Nonlinear Springs 727 Heat Transfer Analysis 727 Joule Heating Analysis 728 Hydrodynamic Bearing Analysis 728 Electrostatic Analysis 728 Piezoelectric or Electrostatic-Structural Analysis Magnetostatic Analysis 728 Electromagnetics Analysis 728 Acoustic Analysis 728

Main Index

728

CONTENTS 17

Nodal Information 728 Stress Analysis 728 Reaction Forces 729 Residual Loads 729 Dynamic Analysis 729 Heat Transfer Analysis 729 Joule Heating Analysis 729 Rigid-Plastic Analysis 729 Hydrodynamic Bearing Analysis 730 Electrostatic Analysis 730 Magnetostatic Analysis 730 Electromagnetic Analysis 730 Piezoelectric or Electrostatic-Structural Analysis Acoustic Analysis 730 Supplementary Information 730 Contact Analysis 730 Electromagnetic Analysis 730 Post File

731

Forming Limit Parameter (FLP) Program Messages

731

734

Marc HyperMesh Results Interface

735

Marc SDRC I-DEAS Results Interface Marc - ADAMS Results Interface Status File

735

736

738

References

738

13 Parallel Processing Different Types of Machines

740

Supported and Unsupported Features Matrix Solvers Contact

Main Index

742

742

740

730

18 Marc Volume A: Theory and User Information

Domain Decomposition 743 Running a Parallel Job 743 Domain Decomposition Methods

745

14 Code Coupling Interfaces Code Coupling

752

Coupling Regions 754 Time Step Control 756 Shell Elements 756 Parallel Processing 757 References

A

757

Finite Element Technology in Marc Governing Equations of Various Structural Procedures System and Element Stiffness Matrices Load Vectors References

B

762

763 764

Finite Element Analysis of NC Machining Processes General Description

766

NC Files (Cutter Shape and Cutter Path Definition) Intersection Between Finite Element Mesh and Cutter Deactivation of Elements

768

Adaptive Remeshing 768 Typical Features for Machining Input of Initial Stresses References

INDEX

Main Index

760

770

769

769

766 768

Preface

Preface

■ About This Manual

20

■ Purpose of Volume A

20

■ Contents of Volume A

20

■ How to Use This Manual

Main Index

21

20 Marc Volume A: Theory and User Information

About This Manual This manual is Marc Volume A, the first in a series of six volumes documenting the Marc Finite Element program. The documentation of Marc is summarized below. You will find references to these documents throughout this manual. Marc Documentation TITLE

VOLUME

Theory and User Information

Volume A

Element Library

Volume B

Program Input

Volume C

User Subroutines and Special Routines

Volume D

Demonstration Problems

Volume E

Purpose of Volume A The purpose of this volume is: 1. To help you define your finite element problem by describing Marc’s capabilities to model physical problems. 2. To identify and describe complex engineering problems and introduce Marc’s scope and capabilities for solving these problems. 3. To assist you in accessing Marc features that are applicable to your particular problems and to provide you with references to the rest of the Marc literature. 4. To provide you with the theoretical basis of the computational techniques used to solve the problem.

Contents of Volume A This volume describes how to use Marc. It explains the capabilities of Marc and gives pertinent background information. The principal categories of information are found under the following titles:

Main Index

Chapter 1

The Marc System

Chapter 2

Program Initiation

Chapter 3

Data Entry

Chapter 4

Introduction to Mesh Definition

Chapter 5

Structural Procedure Library

Chapter 6

Nonstructural Procedure Library

Chapter 7

Material Library

Chapter 8

Contact

21 Preface

Chapter 9

Boundary Conditions

Chapter 10

Element Library

Chapter 11

Solution Procedures for Nonlinear Systems

Chapter 12

Output Results

Chapter 13

Parallel Processing

Chapter 14

Code Coupling Interfaces

Appendix A Finite Element Technology in Marc Appendix B Finite Element Analysis of NC Machining Processes The information in this manual is both descriptive and theoretical. You will find engineering mechanics discussed in some detail. You will also find specific instructions for operating the various options offered by Marc.

How to Use This Manual Volume A organizes the features and operations of the Marc program sequentially. This organization represents a logical approach to problem solving using Finite Element Analysis. First, the database is entered into the system, as described in Chapter 3. Next, a physical problem is defined in terms of a mesh overlay. Techniques for mesh definition are described in Chapter 4. Chapters 5 and 6 describe the various structural analyses that can be performed by Marc, while Chapter 7 describes the material models that are available in Marc. Chapter 8 describes the contact capabilities. Chapter 9 discusses constraints, in the form of boundary conditions. Chapter 10 explains the type of elements that can be used to represent the physical problem. Chapter 11 describes the numerical procedures for solving nonlinear equations. Chapter 12 describes the results of the analysis in the form of outputs. Chapter 13 describes the use of multiple processors when performing an analysis. Finally, Chapter 14 describes the coupling interface to external solvers that is available through user subroutine programming. This volume is also designed as a reference source. This means that all users will not need to refer to each section of the manual with the same frequency or in the same sequence.

Main Index

22 Marc Volume A: Theory and User Information

Main Index

Chapter 1 The Marc System

1

Main Index

The Marc System

J

Marc for Analysis

J

Marc Mentat or MD Patran for GUI

J

Procedure Library

J

Material Library

26

J

Element Library

26

J

Program Function Library

24

25

26

25

24 Marc Volume A: Theory and User Information

The Marc system contains a series of integrated programs that facilitate analysis of engineering problems in the fields of structural mechanics, heat transfer, and electromagnetics. The Marc system consists of the following programs: • Marc for Analysis • Marc Mentat or MD Patran for GUI (For a detailed description of the supported functionalities by MD Patran, refer to the MD Patran Marc Preference Guide.) These programs work together to: • Generate geometric information that defines your structure (Marc and Marc Mentat or MD Patran) • Analyze your structure (Marc) • Graphically depict the results (Marc and Marc Mentat or MD Patran) Figure 1-1 shows the interrelationships among these programs. Marc Programs discusses the Marc component programs. MARC

Preprocessing

Marc Mentat

or

MD Patran

Marc

Analysis

Postprocessing

Figure 1-1

AFEA

Marc Mentat

or

MD Patran

The Marc System

Marc Programs Marc for Analysis You can use Marc to perform linear or nonlinear stress analysis in the static and dynamic regimes, to perform heat transfer analysis and electromagnetic analysis. The nonlinearities may be due to either material behavior, large deformation, or boundary conditions. An accurate representation accounts for these nonlinearities. Physical problems in one, two, or three dimensions can be modeled using a variety of elements. These elements include trusses, beams, shells, and solids. Mesh generators, graphics, and postprocessing capabilities, which assist you in the preparation of input and the interpretation of results, are all available

Main Index

CHAPTER 1 25 The Marc System

in Marc. The equations governing mechanics and implementation of these equations in the finite element method are discussed in Chapters 5, 6, 7, 8, and 11.

Marc Mentat or MD Patran for GUI Marc Mentat is an interactive computer program that prepares and processes data for use with the finite element method. Interactive computing can significantly reduce the human effort needed for analysis by the finite element method. Graphical presentation of data further reduces this effort by providing an effective way to review the large quantity of data typically associated with finite element analysis. An important aspect of Marc Mentat is that you can interact directly with the program. Marc Mentat verifies keyboard input and returns recommendations or warnings when it detects questionable input. Marc Mentat checks the contents of input files and generates warnings about its interpretation of the data if the program suspects that it may not be processing the data in the manner in which you, the user, have assumed. Marc Mentat allows you to graphically verify any changes the input generates. Marc Mentat can process both two- and three-dimensional meshes to do the following: Generate and display a mesh Generate and display boundary conditions and loadings Perform postprocessing to generate contour, deformed shape, and time history plots The data that is processed includes: Nodal coordinates Element connectivity Nodal boundary conditions Nodal coordinate systems Element material properties Element geometric properties Element loads Nodal loads/nonzero boundary conditions Element and nodal sets

Structure of Marc Marc has four comprehensive libraries, making the program applicable to a wide range of uses. These libraries contain structural procedures, materials, elements, and program functions. The contents of each library are described below.

Procedure Library The structural procedure library contains procedures such as static, dynamic, creep, buckling, heat transfer, fluid mechanics, and electromagnetic analysis. The procedure library conveniently relates these various structural procedures to physical phenomena while guiding you through modules that allow, for example, nonlinear dynamic and heat-transfer analyses.

Main Index

26 Marc Volume A: Theory and User Information

Material Library The material library includes many material models that represent most engineering materials. Examples are the inelastic behavior of metals, soils, and rubber material. Many models exhibit nonlinear properties such as plasticity, viscoelasticity, and hypoelasticity. Linear elasticity is also included. All properties may depend on temperature.

Element Library The element library contains over 200 elements. This library lets you describe any geometry under any linear or nonlinear loading conditions.

Program Function Library The program functions such as selective assembly, user-supplied subroutines, and restart, are tailored for user-friendliness and are designed to speed up and simplify analysis work. Marc allows you to combine any number of components from each of the four libraries and, in doing so, puts at your disposal the tools to solve almost any structural mechanics problem.

Features and Benefits of Marc Since the mid-1970s, Marc has been recognized as the premier general purpose program for nonlinear finite element analysis. The program’s modularity leads to its broad applicability. All components of the structural procedure, material, and element libraries are available for use, allowing virtually unlimited flexibility and adaptability. Marc has helped analyze and influence final design decisions on

Main Index

Automotive parts

Space vehicles

Nuclear reactor housings

Electronic components

Biomedical equipment

Steam-piping systems

Offshore platform components

Engine pistons

Coated fiberglass fabric roof structures

Tires

Rocket motor casings

Jet engine rotors

Ship hulls

Welding, casting, and quenching processes

Elastomeric motor mounts

Large strain metal extrusions

CHAPTER 1 27 The Marc System

Marc’s clients gained the following benefits not attainable through other numerical or experimental techniques. These benefits include: Accurate results for both linear and nonlinear analysis Better designs, which result in improved performance and reliability The ability to model complex structures and to incorporate geometric and material nonlinear behavior Documentation, technical support, consulting, and education provided by MSC.Software Corporation Availability of Marc on most computers Efficient operation

Main Index

28 Marc Volume A: Theory and User Information

Main Index

Chapter 2 Program Initiation

2

Main Index

Program Initiation

J

Marc Host Systems

J

Workspace Requirements

J

File Units

J

Program Initiation

J

Examples of Running Marc Jobs

30 31

33 36 39

30 Marc Volume A: Theory and User Information

Chapter 2 explains how to execute Marc on your computer. Marc runs on many types of machines. All Marc capabilities are available on each type of machine; however, program execution can vary among machine types. The allocation of computer memory depends on the hardware restrictions of the machine you are using.

Marc Host Systems Marc runs on most computers. Table 2-1 summarizes the types of machines and operating systems on which Marc currently runs. Table 2-1

Marc Machines and Operating Systems

Vendor

OS

Hardware

FORTRAN C Version Version

Also Works On

Default MPI

HP-Alpha (DEC)4

Tru64 5.1

Alpha Server 4100 f90 5.5

cc 6.4

HP MPI 2.0

HP (64-bit)2, 4

HPUX 11.11

PA2.0

f90 3.1

A.03.73

HP MPI 2.0

HP (64-bit)2, 4

HPUX 11.23

Itanium 2

f90 2.8.7

A.06.02

HP MPI 2.2

IBM (64-bit)4

AIX 5.2

RS/6000 & RS/6000 SP

xlf 8.1.1

cc 6.0.0

MPICH1

f90 7.4

AIX 5.3

SGI (mips4 64-bit)2, 3, 4

IRIX 6.5

R12000

cc 7.4

MPICH1

SGI (Altix 64-bit)2, 4

Linux 2.4.21 sgi303r2

Itanium 2 (Propack Intel 9.1 3.0)

Intel 9.1

SGI MPT 1.13

Sun (64-bit)4

Solaris 10

UltraSparc III

f90 8.3

cc 5.9

MPICH1

Sun (64-bit)4

Solaris 10

x86

f90 8.3

cc 5.9

SUN HPC 7.1

Linux (32-bit)

RedHat AS 4.0

Intel Pentium III or Intel 9.1 equiv.

Intel 9.1

HP MPI 2.2.5.15

Linux (64 bit)4

RedHat AS 3.0

Itanium 2

Intel 10.1

Intel 10.1

HP MPI 2.2.5.15

RedHat AS 4

Linux (64-bit)

RedHat WS 4.0

AMD Opteron

Intel 9.1

Intel 9.1

Intel MPI 3.16

SuSE 10, Intel 10.1

Linux (64-bit)4

RedHat WS 4.0

Intel EM64T

Intel 9.1

Intel 9.1

Intel MPI 3.16

AMD Opteron, SuSE 10, RedHat 5, Intel 10.1

Intel (32-bit)

Windows XP SP2 Intel Pentium III or Intel 9.1 equiv.

Intel 9.1

Intel MPI 3.1

Intel 10.1

Intel (64-bit)4, 8

Windows Server

Intel 9.1

Intel MPI 3.17

Intel EM64T

2003 x64 1 Hardware MPI version also available (via 2 Supports Solver 6. 3 Supports multi-threading. 4 Supports true 64-bit version. 5 Supports the Intel MPI 3.1. 6 Supports the HP MPI 2.2.5.1. 7 Supports the Microsoft MPI 1.0 (SP1). 8

maintain in /tools directory).

The LP64 (i4) version supports only serial runs. Parallel is enabled for all platforms.

Main Index

Intel 9.1

Propack 4.0

Vista XP 64

CHAPTER 2 31 Program Initiation

Workspace Requirements Computing the amount of workspace required by Marc is a complex function of many variables. The most efficient method is to use the default values for the allocation. The program dynamically acquires memory if necessary and if available. In some situations, it is advantageous to initially allocate an amount of memory as described below. The following sections discuss workspace requirements for Marc.

Marc Workspace Requirements The workspace used by Marc is allocated in separate parts. One part is referred to as general memory and contains items such as element stiffness matrices, assembled global stiffness, and mass matrices and decomposed operator matrix for certain matrix solvers. The initial amount of memory for this part can be entered by the user and the program dynamically allocates more memory if necessary. If no initial memory is specified, it is automatically allocated as needed. Other parts of the dynamically allocated workspace can not be influenced by the user. This includes data for elements, vectors, tables, sets, contact bodies, kinematic boundary conditions, transformations, tying, the so-called incremental backup, solver workspace for certain solvers among other things. These are all allocated separately. The incremental backup is an extra copy of stress tensors and similar quantities and is used for the Newton-Raphson iterations in a non-linear analysis. If the cut-back feature is activated, more data is stored in this part to allow for redoing the increment with a modified time step if a failure occurs. General Memory stored in common/space/ Basic Data

Assembled Stiffness Matrix (2)

Decomposed Stiffness Matrix (3)

Second Group of Memory stored in individual dynamically allocated vectors Element Data (1)

Vectors

Sets

Tables

Incremental Backup (4)

Contact Data

Boundary Conditions

Transformation

Tying

Attach

Decomposed Stiffness Matrix (5)

1. Element Data memory allocation is reduced if ELSTO is used. This also reduces Incremental Backup memory. 2. Assembled stiffness matrix memory allocation is reduced if out-of-core solver is used. 3. Decomposed Stiffness matrix is for solver type 0, 4, and if Cholesky preconditioner is used, solver type 2. 4. Incremental Backup memory allocation is reduced if IBOOC is used. 5. Decomposed Stiffness matrix is for solver type 6 and 8. During the analysis, some of the blocks may grow because of changes in the model. In particular because of local or global adaptive meshing, the Element Data, Vector Data, Assembled Stiffness Matrix, and Decomposed Stiffness Matrix may grow in size because of the addition of elements and nodes. The

Main Index

32 Marc Volume A: Theory and User Information

Assembled Stiffness and Decomposed Stiffness matrices also expand due to changes in the bandwidth of the system. Changes in the bandwidth occur when deformable-deformable or self-contact occur. These changes can have a dramatic effect of the amount of memory required. The program dynamically requests additional memory. If this memory is not available, it activates one or more of the out-of-core options. The amount of memory that can be used by an analysis is limited by the hardware employed in the operating system and by internal restrictions within Marc. On 32 bit systems, it is, in general, not possible to allocate more than two GB of memory for a process. The exception is Windows 2003 Server (which allows three GB). Even on this platform, the size of the largest vector is two GB. If this limit is reached, the memory allocation request by Marc fails. Also, a failure to allocate memory can occur if other processes are using large amounts of memory. A typical output when a memory request fails is memory request of 250000000 words failed This occurs when Marc sends a memory allocation request (using the C function malloc) and the system refuses the request. There is also an internal restriction in the standard version of Marc. It uses standard Fortran 32-bit integers as pointers in vectors, and the largest amount of memory that can be addressed with this is 8 GB on a 64-bit system. This limit applies to each part of the separately allocated memory. For example, in a job where the general memory requires 4 GB, the solver needs 6 GB and the incremental backup needs 4 GB. This job can be run provided that the machine has at least 14 GB of available memory. For a parallel analysis, the 8 GB restriction, as well as the 2 GB limit for 32 bit system, is for each domain of the job since each domain corresponds to a separate process. In a separate set of versions of Marc utilizing 64-bit integers, this 8 GB restriction is removed. The memory allocation for the general memory and matrix solver can be affected by the user. The ALLOCATE parameter specifies the amount of memory that is initially allocated for this part. This

amount is allocated regardless of whether it is used or not. The default is set to a small value and the memory grows as needed. For large problems, you may want to get an estimate of the workspace requirements for running a job without actually executing the analysis. To do this, insert the STOP parameter to exit the program normally after the workspace is allocated. Marc prints out a summary of the memory needed. It should be noted that the reported workspace with this option is only an estimate. Some parts of the memory will grow during the analysis and there is no way to predict this without actually running the analysis. For setting the appropriate initial allocation to avoid memory growth of the general memory (which can be inefficient), one should look at the entry on general memory of the summary printout. Please note that the ALLOCATE parameter value in a parallel run refer to the complete model; the specified amount is divided equally among the domains. Chapter 12 Output Results describes the Marc output related to memory in more detail. By default, the data is stored in-core. There are three out-of-core storage options in Marc. • Out-of-core element data storage (the ELSTO parameter also implies IBOOC) • Out-of-core storage of incremental backup (the IBOOC parameter) • Out-of-core matrix solution The out-of-core element data option stores element arrays (strains, stresses, temperatures, etc.) on a file (Fortran unit 3). Data connected with storage of all element quantities occupy a large amount of space for the more complex shell or three-dimensional elements. Putting this data out-of-core leads to a

Main Index

CHAPTER 2 33 Program Initiation

slowdown of the execution (disk access is, in general, slower than memory access) but the effect of this is usually not severe. The ELSTO parameter is used to set this option. The out-of-core option for incremental backup stores this data in a file (Fortran unit 29). If the element data is out-of-core, the incremental backup is automatically out-of-core as well. The slow-down related to incremental backup out-of-core is much less than the one related to element data out-of-core. The out-of-core matrix solution has a more severe effect on the execution speed. Not all matrix solvers support this option. It is not supported by the iterative sparse solver (Marc solver number 2) and the hardware vendor provided solver by HP (solver 6). The multifrontal direct solver (solver 8) does support out-of-core matrix solution. In the case that a memory allocation request fails, Marc automatically switches to out-of-core storage unless it is too late to do this at the point where the allocation failure occurs. If the memory allocation for element data or incremental backup fails, this part is put out-of-core. The incremental backup part can also automatically be put out-of-core to free up memory for the matrix solver. If the default solver is used (multifrontal, solver 8), there is a special way for checking if out-of-core is needed. The solver workspace is allocated in two parts. One in general memory for the assembly and one in separate memory. If the in-core assembly part takes more than 25% of the available memory, the matrix assembly is done out-of-core. This ensures that this decision is done early enough so there is memory left for other parts of the job. The actual LDU decomposition of the matrix is done out-of-core if the in-core decomposition requires more than the available memory to avoid the usage of swap memory during the decomposition. The available memory is set in the file tools/include (for Windows, tools\include.bat) in the installation directory as the variable MEMLIMIT. For most platforms (Unix/Linux except HP PA-RISC), it is set to the amount of physical memory on the machine using a shell command. This can be set explicitly at the installation or specified with the start-up script run_marc with the option -ml new_memlimit. For Windows and HP PA-RISC, the automatic setting of the amount of physical memory is done in the program.

File Units Marc uses auxiliary files for data storage in various ways. Particular FORTRAN unit numbers are used for certain program functions (for example, ELSTO, RESTART). Table 2-2 lists these file unit numbers. Note:

On most systems, the files are referenced by file names as well as by the file

Several of these files are necessary for solving most problems. The program input file and program output file are always required. Table 2-2

FORTRAN File Units Used by Marc

File name jidname.log jidname.t01 jidname.t02 jidname.t03

Unit

Description 0 1 2 3

*OOC denotes Out-Of-Core solution.

Main Index

Analysis sequence log file Usually contains mesh data OOC* solver scratch file Element data storage (see ELSTO parameter)

File Type sequential access, formatted random access, formatted random access, binary random access, binary

34 Marc Volume A: Theory and User Information

Table 2-2

FORTRAN File Units Used by Marc (continued)

File name

Unit

jidname.dat jidname.out jidname.t08 ridname.t08 jidname.t11 jidname.t12 jidname.t13 jidname.t14 jidname.t15 jidname.t16 ridname.t16 jidname.t18 jidname.fem jidname.t19 ridname.t19 jidname_j_.dat jidname.t22 jidname.t23 pidname.t19

5 6 8 9 11 12 13 14 15 16 17 18 18 19 20 21 22 23 24

pidname.t16

25

jidname.t29

29

sidname.t31 jidname.t32 jidname.t33 sidname.t35 material.mat jidname.g jidname.unv jidname.t41 ridname.t42 jidname.opt

31 32 33 35 38 39 40 41 42 45

jidname.t46 jidname.trk ridname.trk

46 47 48

*OOC denotes Out-Of-Core solution.

Main Index

Description Data input file Output file Restart file, written out Restart file to be read in from a previous job OOC* solver scratch file OOC* solver scratch file OOC* solver scratch file OOC* solver scratch file OOC* solver scratch file Post file, written out Post file to be read in from a previous job Mesh optimization correspondence table From Marc to external mesher Post file, written out Post file to be read in from a previous job Temporary input file when cut-back is used. Subspace iteration scratch file Fluid-solid interaction file Temperature post file for CHANGE STATE or post file from previous analysis for PRE STATE or GLOBALLOCAL. Temperature post file for CHANGE STATE or post file from previous analysis for PRE STATE or GLOBALLOCAL. Incremental backup file when ELSTO, IBOOC is used, or insufficient memory exists. Substructure results file Secant method file Lanczos scratch file Substructure results file Material data base file Intergraph post file I-DEAS Universal post file Post file – Domain Decomposition Post file – Domain Decomposition Duplicate load case data file during design optimization run Design optimization scratch file New particle tracking file Old particle tracking file

File Type sequential access, formatted sequential access, formatted sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary random access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted random access, binary sequential access, binary sequential access, formatted

sequential access, binary

sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, formatted sequential access, formatted sequential access, formatted sequential access, binary sequential access, formatted sequential access, formatted sequential access, binary sequential access, formatted sequential access, formatted

CHAPTER 2 35 Program Initiation

Table 2-2

FORTRAN File Units Used by Marc (continued)

File name

Unit

Description

File Type

userspecified

49

jidname.vfs or jidname_CXX.vfs jidname.lck jidname.cnt jidname.mfd jidname-bbc.mfd jidname.seq jidname.rst jidname.mesh jidname.feb jidname.pass jidname.rms jidname.domesh jidname.donemesh

50

User default file (see Marc Volume C: Program Input, sequential access, formatted Appendix C: Default File) Viewfactors for cavity number xx sequential access, formatted

51 52 52 52 53 54 55 55 56 57 59

Locking of post file Dynamic control file rebar - Mentat interface beam-beam contact - Mentat interface Sequence option Load case data User supplied mesh From 3-D mesher to Marc Auto restart command line 2-D outline file for remeshing Lock files indicating meshing status

sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted

59

“do mesh” and “done mesh” Lock file indicating viewfactor calculation status

sequential access, formatted

jidname.doview jidname.doneview

jidname.sltrk ridname.sltrk jidname.sts bbctch.noconv jidname.t81 jidname.t82 jidname.t83 jidname.t84 jidname.t85 jidname.t86 jidname.t87 jidname.t88 jidname.t89 jidname.t90 jidname.fld jidnamd.stm

60 61 67 80 81 82 83 84 85 86 87 88 89 90 91 91

jidname.rec

96

filename.apt filename.ccl

94 95

*OOC denotes Out-Of-Core solution.

Main Index

New streamline tracking file Old streamline tracking file Analysis progress reporting file beam-beam contact information Multifrontal OOC scratch file Multifrontal OOC scratch file Multifrontal OOC scratch file Multifrontal OOC scratch file Multifrontal DDM scratch file Multifrontal DDM scratch file Multifrontal DDM scratch file Multifrontal DDM scratch file Multifrontal DDM scratch file Multifrontal DDM scratch file Forming Limit input file Output at streamline integration points PYROLYSIS parameter. output file of recession surface ABLATION parameter. APT file - machining option CL file - machining option

sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted random access, binary random access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, binary sequential access, formatted sequential access, formatted sequential access, formatted sequential access, file sequential access, file

36 Marc Volume A: Theory and User Information

Table 2-2

FORTRAN File Units Used by Marc (continued)

File name

Unit 97 98

EXITMSG USRDEF jidname.t08 jidname.grd user specified jidnam-dmig* jidname.hmr jidname.dump

99 103 110 - 119 120 - 130 N/A N/A

Description Exit messages User global default file (see Marc Volume C: Program Input, Appendix C: Default File) Base restart file for DDM Grid Force Balance Output Include files for input DMIG output files. Hypermesh results file Scratch file used during memory reallocation on Windows if in-core reallocation fails.

File Type sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, formatted sequential access, binary C file sequential access, binary C file

*OOC denotes Out-Of-Core solution.

Program Initiation Procedures (shell script) are set up that facilitate the execution of Marc on most computers. These procedures invoke machine-dependent control or command statements. These statements control files associated with a job. This shell script submits a job and automatically takes care of all file assignments. This command must be executed at the directory where all input and output files concerning this Marc job are available. To use this shell script, every Marc job should have a unique name qualifier and all Marc output files connected to that job uses this same qualifier. For restart, post, change state, all default Marc Fortran units should be used. To actually submit a Marc job, the following command should be used: run_marc -prog prog_name -jid job_name -rid rid_name -pid pid_name \ -sid sid_name -queue queue_name -user user_name -back back_value \ -ver verify_value -save save_value -vf view_name -def def_name \ -nprocd number_of_processors (for Single Input file runs, use -nps number_of_processors) -nthread number_of_threads \ -dir directory_where_job_is_processed -itree message_passing_type \ -host hostfile (for running over the network) -pq queue_priority \ -at date_time -comp compatible_machines_on_network -cpu time_limit \ -autorst autorestart_value -ml memory_limit

where the \ provides for continuation of the command line.

Main Index

CHAPTER 2 37 Program Initiation

Table 2-3

Keyword Descriptions*

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)

substructure

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

File name containing user defined default data.

-vf

viewfactor

Name of file containing viewfactors for radiation viewfactor.vfs (Monte Carlo method).

-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.

*Default options are shown in bold.

Main Index

38 Marc Volume A: Theory and User Information

Table 2-3

Keyword Descriptions* (continued)

Keyword

Options

-itree

Description Message passing tree type for domain decomposition.(Normally for internal debugging purposes only.)

-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 no

-cr

yes no

Copy input files automatically to remote hosts for a network run, if necessary. Copy post files automatically from remote hosts used for a network run, if necessary.

-pq

0,1,2,etc

Batch queue only: queue priority.

-at (-a)

date/time

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.

-ml

memlimit

*Default options are shown in bold.

Main Index

Memory limit for deciding if the solver should go out-of-core. Specified in Mbyte. Defaults to the physical amount of memory on the machine.

CHAPTER 2 39 Program Initiation

Examples of Running Marc Jobs Example 1: run_marc -jid e2x1 This runs the job e2x1 in the background using a single processor. The input file is e2x1.dat in the current working directory.

Example 2: run_marc -jid e2x14 -user u2x14 -sav y -nproc 4

This runs the job e2x14 in the background with four processors. The user subroutine is linked with the Marc library and a new execu module is created as u2x14.marc and saved in the current working directory after completion of the job.

Example 3: run_marc -jid e2x14a -prog u2x14 -nproc 4 Use the above saved module u2x14.marc to run the job e2x14a in the background with four processors.

Example 4: run_marc -jid e3x2a -v no -b no -nproc 2 Run the job e3x2a in the foreground with two processors. The job runs immediately without verifying any arguments interactively. If there are any input errors in the arguments, the job does not run and the error message is sent to the screen.

Example 5: run_marc -jid e3x2b -rid e3x2a Run the job e3x2b in the background using a single processor. The job uses e3x2a.t08, which is created from Example 4, as restart file.

Example 6: run_marc -jid e2x1 -nproc 2 Runs a two processor job on a single parallel machine.

Example 7: run_marc -jid e2x1 -nproc 2 -host hostfile Runs a two-processor job over a network. The hosts are specified in the file hostfile.

Main Index

40 Marc Volume A: Theory and User Information

Example 8: run_marc -jid e2x1 -nps 2 Runs a two-processor job on a single parallel machine using a single input file.

Example 9: run_marc -jid e2x1 -nps 2 -host hostfile Runs a two-processor job over a network using a single input file. The hosts are specified in the file hostfile.

Main Index

Chapter 3 Data Entry

3

Main Index

Data Entry

J

Input Conventions

42

J

Table Driven Input

45

J

Parameters

J

Model Definition Options

J

History Definition Options

J

REZONE Option

50

51

50 50

42 Marc Volume A: Theory and User Information

The input data structure is made up of three logically distinct sections: 1. Parameters describe the problem type and size. 2. Model definition options give a detailed problem description. 3. History definition options define the load history. Input data is organized in (optional) blocks. Key words identify the data for each optional block. This form of input enables you to specify only the data for the optional blocks that you need to define your problem. The various blocks of input are “optional” in the sense that many have built-in default values which can be used by Marc in the absence of any explicit input from you.

Input Conventions Marc performs all data conversion internally so that the system does not abort because of data errors made by you. The program reads all input data options alphanumerically and converts them to integer, floating point, or keywords, as necessary. Marc issues error messages and displays the illegal option image if it cannot interpret the option data field according to the specifications given in the manual. When such errors occur, the program attempts to scan the remainder of the data file and ends the run with an exit error message at the END OPTION option or at the end of the input file. Two input format conventions can be used: fixed and free format. You can mix fixed and free format options within a file, but you can only enter one type of format on a single option. The syntax rules for fixed fields are as follows: • You must right-justify integers in their fields. (The right blanks are filled with zeroes). • Give floating point numbers with or without an exponent. If you give an exponent, it must be preceded by the character E or D and must be right-justified. The syntax rules for free fields are as follows: • Check that each option contains the same number of data items that it would contain under standard fixed-format control. This syntax rule allows you to mix fixed-field and free-field options in the data file because the number of options you need to input any data list are the same in both cases. • Separate data items on a option with a comma. The comma can be surrounded by any number of blanks. Within the data item itself, no embedded blanks can appear. • Give floating point numbers with or without an exponent. If you use an exponent, it must be preceded by the character E or D and must immediately follow the mantissa (no embedded blanks). • Give keywords exactly as they are written in the manual. Embedded blanks do not count as separators here (for example, BEAM SECT is one word only). • If a option contains only one free-field data item, follow that item with a comma. For example, the number “1” must be entered as “1,” if it is the only data item on a option. If the comma is omitted, the entry is treated as fixed format and may not be properly right-justified.

Main Index

CHAPTER 3 43 Data Entry

• If the EXTENDED parameter is used, integer data is given using 10 fields as opposed to 5 fields. This allows very large models to be included in Marc. Additionally, real numbers are entered using 20 or 30 fields as opposed to 10 or 15. This allows increased accuracy when reading in data. • All data can be entered as uppercase or lowercase text.

Input of List of Items Marc often requests that you enter a list of items in association with certain program functions. As an example, these items can be a set of elements as in the ISOTROPIC option, or a set of nodes as in the POINT LOAD option. Fourteen types of items can be requested: Element numbers

Curves ids

Node numbers

Surfaces ids

Degree of freedom numbers

Body numbers

Integration point numbers

Edges pairs

Layer numbers

Faces pairs

Increment numbers

Oriented curves

Points ids

Oriented surfaces

This list can be entered using either the OLD format (compatible with the G, H, and J versions of Marc) or the NEW format (the K version). Using the OLD format, you can specify the list of items in three different forms. You can specify: 1. A range of items as: m n p which implies items m through n by p. If p is not specified, the program assumes it is 1. Note that the range can either increase or decrease. 2. A list of items as: -n a1 a2 a3 ... an which implies that you should give n items, and they are a ,...a. 3. A set name as: MYSET which implies that all items previously specified in the set MYSET are used. Specify the items in a set using the DEFINE model definition option. Using the NEW format, you can express the list of items as a combination of one or more sublists. These sublists can be specified in three different forms. The following operations can be performed between sublists: AND INTERSECT EXCEPT

Main Index

44 Marc Volume A: Theory and User Information

When you form a list, subsets are combined in binary operations (from left to right). The following lists are examples. 1. SUBLIST1 and SUBLIST2 This list implies all items in subsets SUBLIST1 and SUBLIST2. Duplicate items are eliminated and the resulting list is sorted. 2. SUBLIST1 INTERSECT SUBLIST2 This list implies only those items occurring both in subsets SUBLIST1 and SUBLIST2; the resulting list is sorted. 3. SUBLIST1 EXCEPT SUBLIST2 This list implies all items in subset SUBLIST1 except those which occur in subset SUBLIST2; the resulting list is sorted. 4. SUBLIST1 AND SUBLIST2 EXCEPT SUBLIST3 INTERSECT SUBLIST4 This list implies the items in subsets SUBLIST1 and SUBLIST2 minus those items that occur in subset SUBLIST3. Then, if the remaining items also occur in subset SUBLIST4, they are included in the list. Sublists can have several forms. You can specify: 1. A range of items as: m TO n BY p or m THROUGH n BY p which implies items m through n BY p. If “BY p” is not included, the program assumes “BY 1”. Note that the range can either increase or decrease. 2. A string of items as: a1 a2 a3 ... an which implies that n items are to be included. If continuation options are necessary, then either a C or CONTINUE should be the last item on the option. 3. A set name as: MYSET which implies that all items you previously specified to be in the set MYSET are used. You specify the items in a set using the DEFINE option. Note:

INTERSECT or EXCEPT cannot be used when defining lists of degrees of freedom.

In a list, edges, faces, oriented curves, and oriented surfaces 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 in Marc Volume C: Program Input, Chapter 1. An oriented curve or an oriented surface is used in conjunction with shell elements to indicate if the top surface or the bottom surface of the shell is to be used.

Main Index

CHAPTER 3 45 Data Entry

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

Examples of Lists This section presents some examples of lists and entry formats. Use the DEFINE model definition option to associate a list of items with a set name with items. Three sets are defined below: FLOOR, NWALL, and WWALL. • DEFINE NODE SET FLOOR contains: 1 TO 15(1,2,3,4,5,6,7,8,9,10,11,12,13,14,15) • DEFINE NODE SET NWALL contains: 5 TO 15 BY 5 AND 20 TO 22(5,10,15,20,21,22) • DEFINE NODE SET WWALL contains: 11 TO 20(11,12,13,14,15,16,17,18,19,20) Some possible lists are: • NWALL AND WWALL, which would contain nodes: 5 10 11 12 13 14 15 16 17 18 19 20 21 22 • NWALL INTERSECT WWALL, which would contain nodes: 15 20 • NWALL AND WWALL EXCEPT FLOOR, which would contain nodes: 16 17 19 20 21 22

Table Driven Input An alternative approach to defining the data which is based upon defining nonlinear material properties and variations in the boundary conditions using tables. This input procedure is activated by use of the TABLE parameter. There are six aspects to this input procedure: 1. The data associated with material properties, boundary conditions, and contact may reference a function of up to four variables defined in the TABLE model definition option. 2. Boundary conditions and initial conditions are input in a consistent manner and are associated with a name. They are not applied unless they have been activated by the LOADCASE model and history definition option. 3. Based upon the use of tables and loadcases, all boundary conditions may be defined in the model definition section. 4. Mechanical boundary conditions are, in general, entered as total values at the end of the loadcase.

Main Index

46 Marc Volume A: Theory and User Information

5. Boundary conditions can be applied to either finite element entities (such as nodes, elements, edges or faces) or they may be applied to geometric entities (such as points, curves, or surfaces). The boundary conditions are applied to the finite element based upon the current attach information. This is updated for local adaptive meshing (2-D or 3-D) or global adaptive meshing in 2-D. 6. Each history definition section provides information on the type of analysis to be performed, the duration, and the active boundary conditions. The LOADCASE history definition option is used to perform the latter.

Table Input Many physical quantities cannot be represented by constants. This includes boundary conditions that are dependent upon spatial location and/or time, material properties dependent upon temperature or material damage, contact parameters such as the coefficient of friction and many more. In previous versions, this data could be input through a variety of options including TEMPERATURE EFFECTS, WORK HARD, STRAIN RATE, by repetitive input of boundary conditions, or, in the most general case, by user subroutines. 1 time

28 contact force F

55 normalized arc distance

2 normalized time

29 contact body M

3 increment number

30

56 distance to other contact surface (near contact only) 57 term of series

4 normalized increment 5 x coordinate 6 y coordinate

31 voltage 32 current

σn (normal stress)

current radius ⎞ 33 ⎛ -----------------------------------⎠ ⎝ radius of throat

7 z coordinate 8 s= 9 10 11 12 13 14

2

2

x +y +z

2

θ angle mode number frequency temperature function fourier

15 ε p (equivalent plastic strain) 16 ε· (equivalent strain rate)

· ⁄ αm (normalized 17 B = m g mass flow rate). 18 arc length 19 relative density (not available for shells)

Main Index

58 hydrostatic stress 59 hydrostatic strain 2

(see THROAT)

· 60 B g, p = m g, p ⁄ αm .

34 χ p (pyrolysis damage).

· 61 B g, w = m g, w ⁄ αm .

35 φ w (water vapor fraction).

62 2nd state variable

36 χ c (coking damage). 37 gasket closure distance 38 displacement magnitude 39 stress rate 40 experimental data 41 porosity 42 void ratio

63 3rd state variable

43 · c (equivalent creep strain rate) ε 44 minor principal total strain

70 1st strain invariant

45 distance from neutral axis (-t/2, +t/2) 46 normalized distance from neutral axis (-1, +1)

72 3rd strain invariant

64 65 66 67 68 69

4th state variable 5th state variable loadcase number degree of cure magnetic field intensity equivalent mechanical strain

71 2nd strain invariant

73 any strain component

CHAPTER 3 47 Data Entry

20 σ (equivalent stress) 21 magnetic induction 22 velocity 23 particle diameter

25 y0 coordinate 26 z0 coordinate 2

2

74 damage 75 accumulated crack growth -1 to parametric variable 1 to 100 -100

50 2nd isoparametric coordinate (not available in this release) 51 wavelength (used in spectral radiation)

24 x0 coordinate

27 s0 =

47 local x-coordinate of layer point for open or closed section beam 48 local y-coordinate of layer point for open or closed section beam 49 1st isoparametric coordinate (not available in this release)

2

x0 + y0 + z0

52 creep strain ε e r 53 pressure or primary quantity in diffusion 54 equivalent strain rate for nonNewtonian viscosity

Using the table driven input procedure, virtually all physical data can reference a table/function. Whenever necessary in the analysis, the table is evaluated based upon the current value of the independent variables and multiplied with the reference value. A table can have as many as four independent variables, as long as that independent variable is physically meaningful, For example, requesting that the Young’s modulus is a function of the equivalent plastic strain is considered a data error because elasticity does not support this behavior. The list of available independent variable types is given in the following table. The function can be input through the TABLE model definition option using either the piecewise linear mode or the equation mode. In the piecewise linear mode, the result is interpolated between the given data values. If the independent variable is outside of the range of data entered, the result will be either extrapolated or the last value will be used. In the second mode, the function may be entered as a mathematical equation. 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 v 1 , v 2 , v 3 , and/or v 4 , 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. + * / ^ ! %

Main Index

addition subtraction multiplication division exponential factor mod

48 Marc Volume A: Theory and User Information

Function

F1

v1

x1

Allowing Extrapolation

x2

x3

x4

No Extrapolation Data Entered

x 1, f 1 x 2, f 2 x 3, f 3 x 4, f 4 Given x 0 with extrapolation

f1 – f2 f 0 = f 1 + ⎛ ------------------⎞ ⋅ ( x 0 – x 1 ) ⎝ x 1 – x 2⎠ without extrapolation

f0 = f1 In addition to v 1 , v 2 , v 3 , and v 4 , the following constants may be used in the equation: pi

π

e

exponent

tz

offset temperature entered via the PARAMETERS model definition option

q

Activation energy entered via MATERIAL DATA model definition option

r

Universal gas constant entered via the PARAMETERS model definition option

sb

Stefan Boltzman constant entered via the PARAMETERS model definition 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

v1

CHAPTER 3 49 Data Entry

dsin

sine (x)

x in degrees

dtan

tangent (x)

x in degrees

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)

The equation is evaluated based upon the current value of the independent variable. It is your responsibility to make sure that the equation may be evaluated for the potential values of the independent values. For example, if the function is 1 ⁄ v 1 , then if v 1 = 0.0 , an error will occur.

Main Index

50 Marc Volume A: Theory and User Information

Parameters This group of parameters allocates the necessary working space for the problem and sets up initial switches to control the flow of the program through the desired analysis, This set of input must be terminated with an END parameter. The input format for these parameters is described in Marc Volume C: Program Input.

Model Definition Options This set of data options enters the initial loading, geometry, and material data of the model and provides nodal point data, such as boundary conditions. Model definition options are also used to govern the error control and restart capability. Model definition options can also specify print-out and postprocessing options. The data you enter on model definition options provides the program with the necessary information for determining an initial elastic solution (zero increment solution). When boundary conditions reference time dependent tables, the transient nonlinear behavior can be defined. The transient period is defined in the history definition section. This group of options must be terminated with the END OPTION option. The input format for these options is described in Marc Volume C: Program Input.

History Definition Options This group of options provides the load incrementation and controls the program after the initial elastic analysis. History definition options also include blocks which allow changes in the initial model specifications. Each set of load sets must be terminated with a CONTINUE option. This option requests that the program perform another increment or series of increments if you request the auto-incrementation features. The input format for these options is described in Marc Volume C: Program Input. A typical input file setup for the Marc program is shown below. • Marc Parameter Terminated by an END parameter • Marc Model Definition Options (Zero Increment) Terminated by an END OPTION option • Marc History Definition Data for the First Increment Terminated by a CONTINUE option • (Additional History Definition Option for the second, third, ..., Increments) Figure 3-1 is a dimensional representation of the Marc input data file.

Main Index

CHAPTER 3 51 Data Entry

Parameter

Figure 3-1

Connectivity Coordinates Fixed Displacements Etc.

Model Definition

Linear Analysis

Requiring Incrementation

Load Incrementation

Proportional Increment Auto Load Etc.

Title Sizing Etc.

The Marc Input Data File

REZONE Option When the REZONE option is inserted into the input file and the manual procedure is used, the program reads additional data options to control the rezoning steps. These options must immediately follow the END OPTION option or a CONTINUE history definition option. You can select as many rezoning steps in one increment as you need. Every rezoning step is defined by the data, starting with the REZONE option and ending with the CONTINUE option. The END REZONE option terminates the complete set of rezoning steps that form a complete rezoning increment. Follow the rezoning input with normal history definition data, or again by rezoning data. The input format for these options is described in Marc Volume C: Program Input.

Main Index

52 Marc Volume A: Theory and User Information

Main Index

Chapter 4 Introduction to Mesh Definition

4

Main Index

Introduction to Mesh Definition

J

Direct Input

J

User Subroutine Input

J

MESH2D

J

Marc Mentat

J

FXORD Option

54

59 64 65

59

54 Marc Volume A: Theory and User Information

This chapter describes the techniques for mesh definition available internally in Marc. Mesh definition is the process of converting a physical problem into discrete geometric entities for the purpose of analysis. Before a body can undergo finite element analysis, it must be modeled into discrete physical elements. An example of mesh definition is shown in Figure 4-1.

Figure 4-1

Structure with Finite Element Mesh

Mesh definition encompasses the placement of geometric coordinates and the grouping of nodes into elements. For Marc to have a valid mesh definition, the nodes must have geometric coordinates and must be connected to an element. First, describe the element by entering the element number, the element type, and the node numbers that make up the element. Next, enter the physical coordinates of the nodal points. Note:

You do not need to enter element numbers and node numbers sequentially or consecutively.

Direct Input You must enter two types of data into Marc for direct mesh definition: connectivity data, which describes the nodal points for each element, and coordinate data which gives the spatial coordinates of each nodal point. This section describes how to enter this data.

Main Index

CHAPTER 4 55 Introduction to Mesh Definition

Element Connectivity Data You can enter connectivity data from either the input option file (FORTRAN unit 5) or from an auxiliary file. Several blocks of connectivity can be input. For example, the program can read one block from tape and subsequently read a block from the input option file. Each block must begin with the word CONNECTIVITY. In the case of duplicate specification, Marc always uses the data that was input last for a particular element. Enter the nodal points of two-dimensional elements in a counterclockwise order. Figure 4-2 illustrates correct and incorrect numbering of element connectivity data. 4

3

2

3

2

1

4

Y,R 1 X,Z Correct Numbering Figure 4-2

Incorrect Numbering

Correct/Incorrect Numbering of Two-Dimensional Element Connectivity of 4-Node Elements

When there are eight nodal points on a two-dimensional element, number the corner nodes 1 through 4 in counterclockwise order. The midside nodes 5 through 8 are subsequently numbered in counterclockwise order. Figure 4-3 illustrates the correct numbering of element connectivity of 8-node elements. 4

Y,R

7

3

6

X,Z 8

1 Figure 4-3

Main Index

5

2

Numbering of Two-Dimensional Element Connectivity for 8-Node Quadrilateral Elements

56 Marc Volume A: Theory and User Information

Lower-order triangular elements are numbered using the counterclockwise rule. 3

X,R

X,Z

1 Figure 4-4

2

Numbering of 3-Node Triangular Element

Note that quadrilateral elements can be collapsed into triangular elements by repeating the last node. The higher order triangular elements have six nodes, the corner nodes are numbered first in a counterclockwise direction. The midside nodes 4 through 6 are subsequently numbered as shown in Figure 4-5. 3

6

1

5

4

Figure 4-5

2 Numbering of 6-Node Triangular Element

Number three-dimensional elements in the same order as two-dimensional elements for each plane. Enter nodes for an 8-node brick in counterclockwise order as viewed from inside the element. First, enter nodes comprising the base; then enter ceiling nodes as shown in Figure 4-6. 8

5

Z

7

6 4

3

Y X Figure 4-6

Main Index

1

2

Numbering of Element Connectivity for 8-Node Brick

CHAPTER 4 57 Introduction to Mesh Definition

A 20-node brick contains two 8-node planes and four nodes at the midpoints between the two planes. Nodes 1 through 4 are the corner nodes of one face, given in counterclockwise order as viewed from within the element. Nodes 5 through 8 are on the opposing face; nodes 9 through 12 are midside nodes on the first face, while nodes 13 through 16 are their opposing midside nodes. Finally, nodes 17 through 20 lie between the faces with node 17 between 1 and 5. Figure 4-7 illustrates the numbering of element connectivity for a 20-node brick. 8

14

16 20

13

5

Z

19 6

4

17

11

12

1

Figure 4-7

3

18 10

Y X

7

15

9

2

Numbering of Three-Dimensional Element Connectivity for 20-Node Brick

The four node tetrahedral is shown in Figure 4-8. 4

3

1 Figure 4-8

2 Numbering of Four-Node Tetrahedral

The ten-node tetrahedral is shown in Figure 4-9. The corner nodes 1-4 are numbered first. The first three midside nodes occur on the first face. Nodes 8, 9, and 10 are between nodes 1 and 4, 2 and 4, and 3 and 4, respectively.

Main Index

58 Marc Volume A: Theory and User Information

4 10 8

3

9 7

1

6

5

Figure 4-9

2 Numbering of 10-Node Tetrahedral

The 6-node pentahedral element is shown in Figure 4-10. 6 4 5 3

1

2 Figure 4-10 6-Node Pentahedral

The 15-node pentahedral element is shown in Figure 4-11. 3 15 6

8

9

11

12

7

1

2

14

13 4

10

5

Figure 4-11 15-Node Pentahedral

Main Index

CHAPTER 4 59 Introduction to Mesh Definition

Nodal Coordinate Data You can enter nodal coordinates directly from the input option file (FORTRAN unit 5) or from an auxiliary file. You can enter several blocks of nodal coordinate data in a file. In the case of duplicate specifications, the program uses data entered last for a particular nodal point in the mesh definition. Direct nodal input can be used to input local corrections to a previously generated set of coordinates. These options give the modified nodal coordinates. The CYLINDRICAL option can be used to transform coordinates given in a cylindrical system to a Cartesian system. Note:

Requires the final coordinate data in terms of a single Cartesian system. Refer to Marc Volume B: Element Library to determine the required coordinate data for a particular element type.

Activate/Deactivate You have the ability to turn on and off elements using this option, which is useful when modeling ablation or excavation. When you enter the mesh connectivity, the program assumes that all elements are to be included in the analysis unless they are deactivated. This effectively removes this material from the model. These elements can be reinstated later by using the ACTIVATE option. If the element is activated, one can select if the level of stress is to be reinstated or set to zero. The use of these options results in nonlinear behavior and have an effect upon convergence.

User Subroutine Input User subroutines can be used to generate or modify the data for mesh definition. User subroutine UFCONN generates or modifies element connectivity data. The UFCONN model definition option activates this subroutine. The user subroutine is called once for each element requested. Refer to Volume D: User Subroutines and Special Routines for a description of the UFCONN user subroutine and instructions for its use. The UFXORD user subroutine generates or modifies the nodal coordinates. The UFXORD model definition option activates this subroutine. The user subroutine is called once for each node requested. Refer to Volume D: User Subroutines and Special Routines for a description of the UFXORD user subroutine and instructions for its use.

MESH2D MESH2D generates a mesh of quadrilateral or triangular elements for a two-dimensional body of any shape. The generated mesh is written to a separate file and must be read with the CONNECTIVITY, COORDINATES, and FIXED DISP, etc., options.

Main Index

60 Marc Volume A: Theory and User Information

Block Definition In MESH2D, a physical object or domain is divided into quadrilateral and/or triangular parts, called “blocks”. Quadrilateral blocks are created by Marc by mapping with polynomials of the third order from a unit square. These blocks can, therefore, be used to approximate curved boundaries. The geometry of a quadrilateral block is defined by the coordinates on 12 nodes shown in Figure 4-12. If the interior nodes on an edge of the block are equal to zero or are not specified, the edge of the block is straight. Triangular blocks have straight edges. The geometry of a triangular block is defined by the coordinates of the three vertices. η 4

10

9

P4

3

P10

P9

P3 P8 P7

P11 11

P2

P12

8

P6

x

2

P1 12

7

1

5

6

2

12

x ( ξ ,η ) =

∑ x ( P 1 )Φ i ( ξ ,η ) i = 1

y ( ξ ,η ) =

∑ y ( P 1 )Φ i ( ξ ,η ) i = 1

2

P5

12

Figure 4-12 Typical Quadrilateral Block

Merging of Nodes Marc creates each block with a unique numbering scheme. The MERGE option fuses all nodes that lie within a small circle, renumbers the nodes in sequence, and then removes all gaps in the numbering system. You can select which blocks are to be merged together, or you can request that all blocks be merged. You must give the closeness distance for which nodes will be merged.

Block Types MESH2D generates two types of quadrilateral blocks. Block Type 1 is a quadrilateral block that is covered by a regular grid. The program obtains this grid by dividing the block edge into M by N intervals. Figure 4-13 illustrates the division of block edges into intervals with M = 4, N = 3. The P1 P4 face of the block is the 1-4 face of triangular elements and the P1 P2 face of the block becomes the 1-2 face of quadrilateral elements.

Main Index

CHAPTER 4 61 Introduction to Mesh Definition

η

P4

16

17

η

18

19

20

P3

24

2/3 17

12

11

13

16 2/3

14

9

7

6

8

2

2/3 1 P1

1

2 1/2

3 1/2

8

1/2

12

5

13

6 7

1

2/3

5 1/2

6

P2

7 4

M=4 Triangular

20

19

11

12 14

7

15 ξ

8

10

5 6

11

ξ N = 3 2/3

9

4 3

18

10

15

16

N = 3 2/3

17

9

1

8

2 2

1/2

9

3 3

1/2

10

4 4

1/2

5 1/2

M=4 Quadrilateral

Figure 4-13 Block Type 1

Block Type 2 is a quadrilateral block that allows the transition of a coarse mesh to a finer one. In one direction, the block is divided into M, 2M, 4M ...; while in the other direction, the block is divided into N intervals. Figure 4-14 illustrates the division of Block Type 2 edges into intervals. The P1 P2 face of the block becomes the 1-2 face of quadrilateral elements, and the P2 P3 face of the block is the 2-3 face of triangular elements. Block Type 3 is a triangular block. The program obtains the mesh for this block by dividing each side into N equal intervals. Figure 4-15 illustrates Block Type 3 for triangular and quadrilateral elements. Block Type 4 is a refine operation about a single node of a block (Figure 4-16). The values of N and M are not used. If quadrilateral elements are used in a triangular block, the element near the P2 P3 face of the block is collapsed by MESH2D in every row. The P1 P2 face of the block is the 1-2 face of the generated elements.

Main Index

62 Marc Volume A: Theory and User Information

η P4 18

P3 19

η

34 2/7

9

10 11

7

12 13

14 15

16

17

1/2 4/7

8

M=2

5

4

N=3

1

6 3

7

8

4

1/2

7

8

x

1/2

9

1

3

10 4

11 6

6

2

4

2

3/7

5

2

3

1

6

2

5

P1 1

1/2

5

1

P2

x

2

3

1 1

1

Triangular

Quadrilateral

Figure 4-14 Block Type 2

13 6 1

2

1

2

6

4

4

9 7

4

P2 5

N=4

P1

Triangular

7 3

2

1 1

5 6

5

8

3

9

8

12

7 3

10

14

11

8

P3

15 16

10 P1

P3

4

3

2

Quadrilateral

Figure 4-15 Block Type 3 5 4

6

1

Figure 4-16 Block Type 4

Main Index

7

3

3

2

1

P2

4

2

CHAPTER 4 63 Introduction to Mesh Definition

Symmetry, Weighting, and Constraints MESH2D contains several features that facilitate the generation of a mesh: use of symmetries, generation of weighted meshes, and constraints. These features are discussed below. MESH2D can use symmetries in physical bodies during block generation. An axis of symmetry is defined by the coordinates of one nodal point, and the component of a vector on the axis. One block can be reflected across many axes to form the domain. Figure 4-17 illustrates the symmetry features of MESH2D.

2 1

1

One Symmetry Axis

Original Block

3 2

3 2 4

1

4 5

1 8 6 7

Two Symmetry Axes

Three Symmetry Axes

Figure 4-17 Symmetry Option Example

A weighted mesh is generated by the program by spacing the two intermediate points along the length of a boundary. This technique biases the mesh in a way that is similar to the weighting of the boundary points. This is performed according to the third order isoparametric mapping function. Note:

If a weighted mesh is to be generated, be cautious not to move the interior boundary points excessively. If the points are moved more than 1/6 of the block length from the 1/3 positions, the generated elements can turn inside-out.

The CONSTRAINT option generates boundary condition restraints for a particular degree of freedom for all nodes on one side of a block. The option then writes the constraints into the file after it writes the coordinate data. The FIXED DISP, etc., option must be used to read the boundary conditions generated from the file.

Main Index

64 Marc Volume A: Theory and User Information

Additional Options Occasionally, you might want to position nodes at specific locations. The coordinates of these nodes are entered explicitly and substituted for the coordinates calculated by the program. This is performed using the SPECIFIED NODES option. Some additional options in MESH2D are: • MESH2D can be used several times within one input file. • The START NUMBER option gives starting node and element numbers. • The CONNECT option allows forced connections and/or disconnections with other blocks. This option is useful when the final mesh has cracks, tying, or gaps between two parts. • The MANY TYPES option specifies different element types.

Marc Mentat Marc Mentat is an interactive program which facilitates mesh definition by generating element connectivity and nodal coordinates. Some of the Marc Mentat capabilities relevant to mesh generation are listed below. • Prompts you for connectivity information and nodal coordinates. Accepts input from a keyboard or mouse. • Accepts coordinates in several coordinate systems (Cartesian, cylindrical, or spherical). • Translates and rotates (partial) meshes. • Combines several pre-formulated meshes. • Duplicates a mesh to a different physical location. • Generates a mirror image of a mesh. • Subdivides a mesh into a finer mesh. • Automatic mesh generation in two- and three-dimensions. • Imports geometric and finite element data from CAD systems. • Smooths nodal point coordinates to form a regular mesh • Converts geometric surfaces to meshes. • Refines a mesh about a point or line. • Expands line mesh into a surface mesh, or a surface mesh into a solid mesh. • Calculates the intersection of meshes. • Maps nodal point coordinates onto prescribed surfaces. • Writes input data file for connectivity and coordinates in Marc format for use in future analyses. • Apply boundary conditions to nodes and elements. • Define material properties. • Submit Marc jobs.

Main Index

CHAPTER 4 65 Introduction to Mesh Definition

FXORD Option The FXORD model definition option (Volume C: Program Input) generates doubly curved shell elements of element type 4, 8, or 24 for the geometries most frequently found in shell analysis. Since the mathematical form of the surface is well-defined, the program can generate the 11 or 14 nodal coordinates needed by element type 8, 24, or 4 to fit a doubly curved surface from a reduced set of coordinates. For example, you can generate an axisymmetric shell by entering only four coordinates per node. The FXORD option automatically generates the complete set of coordinates required by the elements in the program from the mathematical form of the surface. A rotation and translation option is available for all components of the surface to give complete generality to the surface generation. The input to FXORD consists of the reduced set of coordinates given in a local coordinate system and a set of coordinates which orient the local system with respect to the global system used in the analysis. The program uses these two sets of coordinates to generate a structure made up of several shell components for analysis. The FXORD option allows for the generation of several types of geometries. Because you may need to analyze shells with well-defined surfaces not available in this option, you can use the UFXORD user subroutine to perform your own coordinate generation (Volume D: User Subroutines and Special Routines). The FXORD option can also be used to convert cylindrical coordinates or spherical coordinates to Cartesian coordinates for continuum elements.

Major Classes of the FXORD Option The following cases are considered: • • • • • • • •

Shallow Shell (Type I) Axisymmetric Shell (Type 2) Cylindrical Shell Panel (Type 3) Circular Cylinder (Type 4) Plate (Type 5) Curved Circular Cylinder (Type 6) Convert Cylindrical to Cartesian (Type 7) Convert Spherical to Cartesian (Type 8)

Shallow Shell (Type I) Type 1 is a shallow shell with θ 1 = x 1,

θ2 = x2

(4-1)

The middle surface of Figure 4-18 (Type 1) is defined by an equation of the form x 3 = x 3 ( x 1, x 2 )

(4-2)

and the surface is determined when the following information is given at each node. ∂x 3 ∂x 3 ∂ 2 x 3 x 1, x 2, x 3, ---------, --------- , -----------------∂x 1 ∂x 2 ∂x 1 ∂x 2

Main Index

(4-3)

66 Marc Volume A: Theory and User Information

The last coordinate is only necessary for Element Type 4. X3

X3 R f X2

X2

q

X1

Type 2

Type 1 X3

X2

X2 R 3

φ

X1 X1

X3 Type 4

X3 Type 3

Figure 4-18 Classification of Shells

Axisymmetric Shell (Type 2) The middle surface symmetric to the x 3 axis (Figure 4-18, Type 2) is defined as: x 1 = R ( φ ) cos φ cos θ x 2 = R ( φ ) cos φ sin θ

(4-4)

x 3 = R ( φ ) sin φ where φ and θ are the angles shown in Figure 4-18. In this case, the surface is defined by dR θ, φ, R, ------dφ The angles θ and φ are given in degrees.

Main Index

(4-5)

CHAPTER 4 67 Introduction to Mesh Definition

Cylindrical Shell Panel (Type 3) The middle surface is the cylinder defined by Figure 4-18. x1 = x1 ( s ) x2 = x2 ( s )

(4-6)

x3 = x3 The nodal geometric data required is dx 1 dx 2 s, x 3, x 1, x 2, ---------, --------ds ds

(4-7)

Circular Cylinder (Type 4) This is the particular case of Type 3 where the curve x 1 ( s ), x 2 ( s )

(4-8)

is the circle given by Figure 4-18 (Type 4). x 1 = R cos θ

(4-9)

x 2 = R sin θ The only nodal information is now θ, x 3, R

(4-10)

Note that θ is given in degrees and, because R is constant, it needs to be given for the first nodal point only. Plate (Type 5) The shell is degenerated into the plate x3 = 0

(4-11)

The data is reduced to x 1, x 2

Main Index

(4-12)

68 Marc Volume A: Theory and User Information

Curved Circular Cylinder (Type 6) Figure 4-19 illustrates this type of geometry. X3 Shell Middle Surface

q1 q2

R f X2

q X1 Type 6 Figure 4-19 Curved Circular Cylinder

The middle surface of the shell is defined by the equations x 1 = r cos θ x 2 = r sin θ cos φ + R ( 1 – cos φ )

(4-13)

x 3 = ( R + – r sin θ r sin φ ) sin φ The Gaussian coordinates on the surface are θ 1 = rθ θ 2 = Rφ

(4-14)

and form an orthonormal coordinate system. The nodal point information is θ, φ, r, R θ and φ in degrees. You need to specify the radii r and R only for the first nodal point.

Main Index

(4-15)

CHAPTER 4 69 Introduction to Mesh Definition

Convert Cylindrical to Cartesian (Type 7) Type 7 allows you to enter the coordinates for continuum elements in cylindrical coordinates, which are converted by Marc to Cartesian coordinates. In this way, you can enter R , θ , Z and obtain x, y, z where θ is given in degrees and x = R cos θ y = R sin θ z = Z

(4-16)

Convert Spherical to Cartesian (Type 8) Type 8 allows you to enter the coordinates for continuum elements in spherical coordinates, which are converted by Marc to Cartesian coordinates. In this way, you can enter R , θ , φ and obtain x, y, z where θ and φ are given in degrees and x = R cos θ sin φ y = R sin θ cos φ z = R cos φ

(4-17)

Recommendations on Use of the FXORD Option When a continuous surface has a line of discontinuity, for example, a complete cylinder at θ = 0° = 360° , you must place two nodes at each nodal location on the line to allow the distinct coordinate to be input. You must use tying element type 100 to join the degrees of freedom. Generally, when different surfaces come together, you must use the intersecting shell tyings. The FXORD option cannot precede the COORDINATES option, because it uses input from that option.

Incremental Mesh Generators Incremental mesh generators are a collection of options available in Marc to assist you in generating the mesh. Incremental mesh generators generate connectivity lists by repeating patterns and generate nodal coordinates by interpolation. Use these options directly during the model definition phase of the input. During the model definition phase, you can often divide the structure into regions, or blocks, for which a particular mesh pattern can be easily generated. This mesh pattern is established for each region and is associated with a single element connectivity list. Use the CONNECTIVITY option to input this element connectivity list. The incremental mesh generators then generate the remainder of the connectivity lists. Critical nodes define the outline of the regions to be analyzed. Use the COORDINATES option to enter the critical nodes. The incremental mesh generators complete the rest and join the regions by merging nodes. A special connectivity interpolator option generates midside nodes for elements where these nodes have not been specified in the original connectivity. A separate mesh generation run is sometimes required to determine the position of these nodes. This run can be followed by mesh display plotting.

Main Index

70 Marc Volume A: Theory and User Information

The incremental mesh generators are listed below: Element Connectivity Generator – The CONN GENER option repeats the pattern of the connectivity data for previously defined master elements. One element can be removed for each series of elements, allowing the program to generate a tapered mesh. Two elements can be removed for each series with triangular elements. Element Connectivity Interpolator – The CONN FILL option completes the connectivity list by generating midside nodes. You first generate the simpler quadrilateral or brick elements without the midside nodes. You can then fill in the midside nodes with this option. Coordinate Generator – The NODE GENER option creates a new set of nodes by copying the spacing of another specified set of nodes. Coordinate Interpolator – The NODE FILL generates intermediate nodes on a line defined by two end nodes. The spaces between the nodes can be varied according to a geometric progression. Coordinate Generation for Circular Arcs – The NODE CIRCLE option generates the coordinates for a series of nodes which lie on a circular arc. Nodal Merge – The NODE MERGE option merges all nodes which are closer than a specified distance from one another and it eliminates all gaps in the nodal numbers.

Bandwidth Optimization Marc can minimize the nodal bandwidth of a structure in several ways. The amount of storage is directly related to the size of the bandwidth, and the computation time increases in proportion to the square of the average bandwidth. The OPTIMIZE option allows you to choose from several bandwidth optimization algorithms. The minimum degree algorithm should only be used if the direct sparse solver is used. The four available OPTIMIZE options are listed in Table 4-1. Note:

This option creates an internal node numbering that is different from your node numbering. Use your node numbering for all inputs. All output appears with your node numbering. The occurrence of gap or Herrmann elements can change the internal node numbers. On occasion, this change can result in a non optimal node numbering system, but this system is necessary for successful solutions.

Table 4-1

Bandwidth Optimization Options

Option Number

Main Index

Remarks

Solver

2

Cuthill-McKee algorithm

Profile (2)

9

Sloan (Recommended)

Profile (2)

10

Minimum Degree Algorithm

Sparse Direct (4) or Multifrontal (8)

11

Metis (Recommended)

Multifrontal (8)

CHAPTER 4 71 Introduction to Mesh Definition

The nodal correspondence obtained through this process can be saved and then used in subsequent analyses. This eliminates the need to go through the optimization step in later analyses. The correspondence is used to relate the user-defined node (external) numbers to the program-optimized (internal) node numbers and vice versa.

Rezoning The REZONING parameter defines a new mesh and transfers the state of the old mesh to the new mesh. Elements or nodes can be either added to or subtracted from the new mesh. This procedure requires a sub increment to perform the definition of the new mesh. The rezoning capability can be used for two- and three-dimensional continuum elements and for shell elements 22, 75, 138, 139, and 140. See Figure 4-20 for an example of rezoning. Rezoning or remeshing can be carried automatically using the mesh generators. This feature is described in detail in the Automatic Global Remeshing section.

Before Rezoning

After Rezoning

Figure 4-20 Mesh Rezoning

Substructure Marc is capable of multilevel substructuring that includes: Generation of superelements Use of superelements in subsequent Marc analyses Recovery of solutions (displacements, stresses, and strains) in the individual substructures The Marc multilevel procedure allows superelements to be used. One self-descriptive database stores all data needed during the complete analysis. You only have to ensure this database is saved after every step of the analysis. The advantages of substructuring are the following: • • • •

Main Index

Separates linear and nonlinear parts of the model Allows repetition of symmetrical or identical parts of the model for linear elastic analysis Separates large models into multiple, moderate-size models Separates fixed model parts from parts of the model that may undergo design changes

72 Marc Volume A: Theory and User Information

A disadvantage of substructuring is the large amount of data that must be stored on the database. Three steps are involved in a substructuring run. • The superelement generation step is done for every superelement at a certain level. • The use of superelements in subsequent Marc runs is done at the highest level, or is incorporated into Step 1 for the intermediate levels. • Recovery of solutions within a certain superelement can or cannot be done for every superelement. Substructuring in Marc is only possible for static analysis. Nonlinearities are not allowed with a superelement. You, as a user, must ensure that nonlinearities are not present. The maximum number of levels in a complete analysis is 26. The maximum number of substructures in the complete analysis is 676. Each step can be done in an individual run, or an unlimited number of steps can be combined into a single run. During superelement generation in Marc, you can generate a complete new superelement or you can copy a previously defined superelement with identical or newly defined external load conditions. Any number of superelements can be formed in a generation run. Marc offers flexibility in the use of superelements by allowing rotation or mirroring of a superelement. If a run is nonlinear, superelements are treated as linear elastic parts. At every increment, you can perform a detailed analysis of certain substructures by descending down to the desired superelements. Use the normal Marc control algorithm (AUTO INCREMENT, AUTO LOAD, PROPORTIONAL INCREMENT) to control the load on the superelements.

Technical Background The system of equations for a linear static structure is (4-18)

Ku = P When local degrees of freedom (subscripted l ) and external degrees of freedom (subscripted

e

) are

considered, this can be rewritten as K l l K e l ⎛⎜ u l ⎞⎟ = K l e K e e ⎜⎝ u e ⎟⎠

⎛ P ⎞ ⎜ l ⎟ ⎜ P ⎟ ⎝ e ⎠

(4-19)

To obtain both the stiffness matrix and the load vector of the substructure, it is necessary to eliminate u 1 and rewrite the above system with u e as the only unknown splitting the above equation.

Main Index

CHAPTER 4 73 Introduction to Mesh Definition

Kl l ul + Ke l ue = Pl (4-20)

and Kl e ul + Ke e ue = Pe The first equation can be written as u l = – K l–l1 • K e l u e + K l–l1 P l

(4-21)

Substituting this equation into the second – K l e K l–l1 K e l u e + K l e K l–l1 P l + K e e u e = P e

(4-22)

This can be rewritten as K e*e u e = P e*

(4-23)

where –1

K e*e = K e e – K l e K l l K e l

(4-24)

and –1

P e* = P e – K l e K l l P l

(4-25)

K e*e and P e* are solved by the triangularization of K l l , the forward and backward substitution of K e l and P l , respectively, and premultiplication with K l e , K e*e , and P e* are used in the next part of the analysis with other substructures or with another element mesh. That analysis results in the calculation of ue. You can now calculate the local degrees of freedom and/or the stresses using the following procedure: Kl l • ul = Pl – Ke l ue

(4-26)

which can be written as –1

u l = K l l • P l*

(4-27)

where P l* = P e – K e l u e

(4-28)

The displacement of the substructure is, therefore, known, and stresses and strains can be calculated in the normal way.

Main Index

74 Marc Volume A: Theory and User Information

4

Scaling Element Stiffness

Introductio n to Mesh Definition

Occasionally, it is desirable to perform a scalar multiplication of the stiffness, mass, and load matrix to represent a selective duplication of the finite element mesh. The STIFSCALE option can be used to enter the scaling factor for each element. In this case, the global stiffness, mass, and load matrices are formed as follows: K g = Σs i K ie l, M g = Σs i M ie l, and F g = Σs i f ie l

(4-29)

Note that no transformation of the stiffness matrix occurs and that point loads are not scaled.

BEAM SECT Parameter The BEAM SECT parameter inputs data to define the sectional properties for three-dimensional beam elements. Include this option if you are using: element types 13, 77, or 79 element types 14, 25, 76, or 78 with a noncircular section element types 52 or 98 and torsional and shear stiffness must be defined independently element types 52 or 98 with numerical integrated solid cross-section. The convention adopted for the local (beam) coordinate system is: the first and second director (local X and Y) at a point are normal to the beam axis; the third director (local Z) is tangent to the beam axis and is in the direction of increasing distances along the beam. The director set forms a right-handed system.

Orientation of the Section in Space The beam axis in an element is interpolated from the two nodes of the element. dx dy dz x, y, z, ------, ------, -----ds ds ds

(4-30)

where the last three coordinates are only used for element 13. The beam section orientation in an element is defined by the direction of the first director (local X) at a point, and this direction is specified via the coordinates of an additional node or through the GEOMETRY option (see Marc Volume C: Program Input).

Definition of the Section You can include any number of different beam sections in any problem. Data options following the BEAM SECT parameter of the Marc input (see Marc Volume C: Program Input) define each section. The program numbers the sections in the order they are entered. To use a particular section for a beam element, set EGEOM2 (GEOMETRY option, Option 2, Columns 11-20) to the floating-point value of the section number, for example, 1, 2, or 3. The program uses the default circular section for the closed section beam elements (14, 25, 76, 78) if EGEOM1 is nonzero. The program uses the default solid rectangular cross section for elements 52 or 98 if EGEOM1 is nonzero. Figure 4-21 shows how the thin-walled section is defined using the input data.

Main Index

CHAPTER 4 75 Introduction to Mesh Definition

Section 1

Section 2 xl

10 xl 4

3 1

Divisions

1-2 2-3 3-4 4-5 5-6

2

1

2

Branch

yl

20

yl

8

Thickness

8 4 8 4 8

1.0 0.0 0.3 0.0 1.0

1

Branch 1-2 2-3 3-4

10

Branch

60°

R=5

Divisions

Thickness

10 10 10

1.0 1.0 1.0

Section 3

6

2

4

3

6

16

5

8

1-2 2-3 3-4 4-5 5-6

Divisions

Thickness

8 4 8 4 8

0.5 0.5 0.5 0.5 0.5

5

17.85

3

4

xl yl Figure 4-21 Beam Section Definition Examples for Thin-walled Sections

The rules and conventions for defining a thin-walled section are listed below: 1

1

1

1. An x – y coordinate system defines the section, with x the first director at a point of the 1 1 beam. The origin of the x – y system represents the location of the node with respect to the section.

Main Index

76 Marc Volume A: Theory and User Information

2. Enter the section as a series of branches. Branches can have different geometries, but they must form a complete traverse of the section in the input sequence so that the endpoint of one branch is the start of the next branch. It is often necessary for the traverse of the section to double back on itself. To cause the traverse to do this, specify a branch with zero thickness. 3. You must divide each branch into segments. The stress points of the section are the branch division points. The stress points are the points used for numerical integration of a section’s stiffness and for output for stress results. Branch endpoints are always stress points. There must always be an even number of divisions (nonzero) in any branch. Not counting branches of zero thickness, you can use a maximum of 31 stress points (30 divisions) in a complete section. 4. Branch thickness varies linearly between the values given for branch endpoint thickness. The thickness can be discontinuous between branches. A branch is assumed to be of constant thickness equal to the thickness given at the beginning of the branch if the thickness at the end of the branch is given as an exact zero. 1

1

5. The shape of a branch is interpolated as a cubic based on the values of x and y and their directions, in relation to distance along the branch. The data is input at the two ends of the branch. 1

1

If both dx ⁄ ds and dy ⁄ ds are given as exact zeros at both ends of the branch, the branch is assumed to be straight. The section can have a discontinuous slope at the branch ends. The beginning point of one branch must coincide with the endpoint of the previous branch. As a result, 1

1

x and y for the beginning of a branch need to be given only for the first branch of a section. 6. Stress points are merged into one point if they are separated by a distance less than t ⁄ 10 , where t is a thickness at one of these points. Figure 4-21 shows three sections of a beam. Notice the use of zero thickness branches in the traverse of the I section. The program provides the following data: the location of each stress point in the section, the thickness at that point, the weight associated with each point (for numerical integration of the section stiffness), and the warping function at each section. Solid sections can be defined by using one of the standard sections and specifying its typical dimensions or by using quadrilateral segments and specifying the coordinates of the four corner points of each quadrilateral segment in the section. The local axes of a standard section are always the symmetry axes. For the standard sections, the symmetry axes are also the principal axes. The principal axes for each section are shown in Figure 4-22. For the more general sections, it is not required to enter the coordinates of the corner points of the quadrilateral segments with respect to the principal axes. The section is automatically realigned and you can make specifications about how this realignment should be carried out. The details about these orientation methods are described in the Cross-section Orientation and Location of the Local-section Axis sections in Marc Volume B: Element Library. Figure 4-22 shows the standard solid sections, the dimensions needed to specify them, and the orientation of their local axes. If the dimension b is omitted for an elliptical section, the section will be circular. If the dimension b is omitted for a rectangular section, the section will be square. If the dimension c is omitted for a trapezoidal or a hexagonal section, the section will degenerate to a triangle or a diamond. For the elliptical section, the center point is the first integration point. The second is located on the negative y-axis and the points are numbered radially outward and then counterclockwise. For the rectangular, trapezoidal and hexagonal sections the first integration point is nearest to the lower left corner and the last integration point is nearest to the upper right corner. They are numbered from left to

Main Index

CHAPTER 4 77 Introduction to Mesh Definition

right and then from bottom to top. The default integration scheme for all standard solid sections uses 25 integration points. y

y

x

b

x

b

a

a

Elliptical Section Circular (set b = 0)

Rectangular Section Square (set b = 0) c

c y

b

y

[ 2 ( a + c )b ] ⁄ [ 3 ( a + c ) ]

x

b

x

a

a

Trapezoidal Section

Hexagonal Section

Figure 4-22 Standard Solid Section Types with Typical Dimensions

The rules and conventions for defining a general section solid are listed below: 1. Each quadrilateral segment is defined by entering the coordinates of the four corner points in the local xy-plane. The corner points must be entered in a counterclockwise sense. 2. The quadrilateral segments must describe a simply connected region; i.e., there must be no holes in the section, and the section cannot be composed of unconnected “islands” and should not be connected through a single point. 3. The quadrilateral segments do not have to match at the corners. Internally, the edges must, at least, partly match. 4. The segments must not overlap each other (i.e., the sum of the areas of each segment must equal the total area of the segment). 5. Each section can define its own integration scheme and this scheme applies to all segments in the section.

Main Index

78 Marc Volume A: Theory and User Information

6. A section cannot have more than 100 integration points in total. This limits each section to, at most, 100 segments that, by necessity, will use single point integration. If less than 100 segments are present in a section, they may use higher order integration schemes, as long as the total number of points in the section does not exceed 100. 7. Integration points on matching edges are not merged, should they coincide. This method allows you to define an arbitrary solid section in a versatile way, but you must make sure that the conditions of simply connectedness and nonoverlap are met. The assumptions underlying the solid sections are not accurate enough to model sections that are thin-walled in nature. It is not recommended to use them as an alternative to thin-walled sections. Solid sections do not account for any warping of the section and, therefore, overestimate the torsion stiffness as it is predicted by the Saint Venant theory of torsion. The first integration point in each quadrilateral segment is nearest to its first corner point and the last integration point is nearest to its third corner point. They are numbered going from first to second corner point and then from second to third corner point. The segments are numbered consecutively in the order in which they have been entered and the first integration point number in a new segment simply continues from the highest number in the previous segment. There is no special order requirement for the quadrilateral segments. They must only meet the previously outlined geometric requirements. For each section, the program provides the location of the integration points with respect to the principal axes and the integration weight factors of each point. Furthermore, it computes the coordinates of the center of gravity and the principal directions with respect to the input coordinate system. It also computes the area and the principal second moments of area of the cross section. For each solid section, all of this information is written to the output file. All solid sections can be used in a pre-integrated fashion. In that case, the area A and the principal moments of area Ixx and Iyy are calculated by numerical integration. The torsional stiffness is always computed from the polar moment of inertia J=Ixx+Iyy. The shear areas are set equal to the section area A. The stiffness behavior may be altered by employing any of the stiffness factors. In a pre-integrated section, no layer information is computed and is, therefore, not available for output. Pre-integrated sections can only use elastic material behavior and cannot account for any inelasticity (e.g., plasticity). For pre-integrated sections there is no limit on the number of segments to define the section. Figure 4-23 shows a general solid section built up from three quadrilateral segments using a 2 x 2 Gauss integration scheme. It also shows the numbering conventions adopted in a quadrilateral segment and its mapping onto the parametric space. For each segment in the example, the first corner point is the lower-left corner and the corner points have been entered in a counterclockwise sense. The segment numbers and the resulting numbering of the integration points are shown in the figure. Gauss integration schemes do not provide integration points in the corner points of the section. If this is desired, you can choose other integration schemes like Simpson or Newton-Cotes schemes. In general, a 2 x 2 Gauss or a 3 x 3 Simpson scheme in each segment suffices to guarantee exact section integration of linear elastic behavior.

Main Index

CHAPTER 4 79 Introduction to Mesh Definition

η 12

11 3

9

4

8

ξ

2

=>

6

5 3

1 4

1

η

(−1,1)

10

7

1

3

4

y

3

ιint

(−1,−1) 2

1

(1,1)

2

(1,−1)

2 x

Figure 4-23 Beam Section Definition for Solid Section plus Numbering Conventions Adopted

Error Analysis You can determine the quality of the analysis by using the ERROR ESTIMATE option. The ERROR ESTIMATE option can be used to determine the mesh quality (aspect ratio, and skewness), and how they change with deformation. While all of the Marc elements satisfy the patch test, the accuracy of the solution often depends on having regular elements. In analyses where the updated Lagrangian method is used, the mesh often becomes highly distorted during the deformation process. This option tells you when it would be beneficial to perform a rezoning step. This option can also be used to examine the stress discontinuity in the analysis. This is a measure of the meshes ability to represent the stress gradients in the problem. Large stress discontinuities are an indication that the mesh is not of sufficient quality. This can be resolved by increasing the number of elements or choosing a higher order element or using local adaptive meshing.

Local Adaptivity The adaptive mesh generation capability increases the number of elements and nodes to improve the accuracy of the solution. The capability is applicable for both linear elastic analysis and for nonlinear analysis. The capability can be used for lower-order elements, 3-node triangular solids and shells, 4-node quadrilateral solids and shells, 4-node tetrahedrals, 8-node hexahedral elements, and the 8-node solid-shell elements. When used in conjunction with the ELASTIC parameter for linear analysis, a steady-state heat transfer, electrostatic, or magnetostatic, the mesh is adapted and the analysis repeated until the adaptive criteria is satisfied. When used in a nonlinear analysis, an increment is performed. If necessary, this increment is followed by a mesh adjustment which is followed by the analysis of the next increment in time. While this can result in some error, as long as the mesh is not overly coarse, it should be adequate. Local adaptivity is available in a parallel analysis. In this case, the new elements remain in the same domain as the parent element.

Main Index

80 Marc Volume A: Theory and User Information

Number of Elements Created The adaptive meshing procedure works by dividing an element and internally tying nodes to insure compatibility. Figure 4-24 shows the process for a single quadrilateral element.

Original Element

Level 1 Refinement

Level 2 Refinement

Level 3 Refinement

Figure 4-24 Single Quadrilateral Element Process

A similar process occurs for the triangles, tetrahedrons, and hexahedrons elements. You can observe that for quadrilaterals the number of elements expands by four with each subdivision; similarly, the number of elements increases by eight for hexahedrals. For the 8-node solid-shell element, the subdivision is similar to 4-node quadrilaterals; there is no refinement through the thickness. If full refinement occurs, ( level x 2 )

( level x 3 )

you observe that the number of elements is 2 for quadrilaterals and 2 for hexahedrons elements. The number of levels also limits the amount of subdivisions that may occur. Number of Elements Level

Quadrilaterals

Hexahedrals

0

1

1

1

4

8

2

16

64

3

64

512

4

256

4096

For this reason, it is felt that the number of levels should, in general, be limited to three. When adaptive meshing occurs, you can observe that discontinuities are created in the mesh as shown below: E D A

Main Index

B

C

CHAPTER 4 81 Introduction to Mesh Definition

To ensure compatibility node B is effectively tied to nodes A and C, and node D is effectively tied to nodes C and E. All of this occurs internally and does not conflict with other user-defined ties or contact.

Boundary Conditions When mesh refinement occurs, boundary conditions are automatically adjusted to reflect the change in mesh. The rules listed below are followed: 1. Fixed Displacement For both 2-D and 3-D, if both corner nodes on an edge have identical boundary conditions, the new node created on that edge has the same boundary conditions. For 3-D, if all four nodes on a face have identical boundary conditions, the new node created in the center of the face has the same boundary conditions. Note that identical here means the same in the first degree of freedom, second degree of freedom, etc. independently of one another. 2. Point Loads The point loads remain unchanged on the original node number. 3. Distributed Loads Distributed loads are automatically placed on the new elements. Caution should be used when using the FORCEM user subroutine as the element numbers can be changed due to the new mesh process. 4. Contact The new nodes generated on the exterior of a body are automatically treated as potential contact nodes. The elements in a deformable body are expanded to include the new elements created. After the new mesh is created, the new nodes are checked to determine if they are in contact. It should be noted that new nodes on shells that are completely tied to the corresponding edge nodes are not checked for contact. Caution: None of the nodes of an element being subdivided should have a local coordinate system defined through the TRANSFORMATION or COORD SYSTEM option.

Location of New Nodes When an element is refined, the default is that the new node on an edge is midside to the two corner nodes. As an alternative, the POINTS, CURVES, SURFACES, ATTACH EDGE and ATTACH FACE options or the UCOORD user subroutine can be used. The CURVES and SURFACES options can be used to describe the mathematical form of the curve or surface. If the corner nodes of an edge are attached to the surface, the new node is placed upon the actual surface. This option to attach new nodes is available both in a linear as well as a nonlinear analysis. This is illustrated in Figure 4-25 and Figure 4-26, where initially a single element is used to represent a circle. The circle is defined with the CURVES option and the original four nodes are placed on it using the ATTACH EDGE option. Notice that the new nodes are placed on the circle.

Main Index

82 Marc Volume A: Theory and User Information

Figure 4-25 Original Mesh and Surface

Level 1 Refinement

Level 2 Refinement

Level 2 and 3 Refinement Figure 4-26 Levels of Refinement

Adaptive Criteria The adaptive meshing subdivision occurs when a particular adaptive criterion is satisfied. Multiple adaptive criteria can be selected using the ADAPTIVE model definition option. These include: Mean Strain Energy Criterion The element is refined if the strain energy of the element is greater than the average strain energy in a chosen set of elements times a given factor, f 1 . total strain energy element strain energy > ----------------------------------------------- * f 1 number of elements

Main Index

(4-31)

CHAPTER 4 83 Introduction to Mesh Definition

Zienkiewicz-Zhu Criterion The error norm is defined as either 2

π

2

=

∫ ( σ∗ – σ ) dV 2 ------------------------------------------------------------- γ 2

2

∫ σ dV + ∫ ( σ∗ – σ ) dV

2

=

∫ ( E∗ – E ) dV ------------------------------------------------------------2

2

∫ E dV + ∫ ( E∗ – E ) dV

(4-32)

The stress error and strain energy errors are X =

∫ ( σ∗ – σ )

2

dV and Y =

∫ ( E∗ – E )

2

dV

(4-33)

where σ* is the smoothed stress and σ is the calculated stress. Similarly, E is for energy. An element is subdivided if π > f 1 and

(4-34)

X e l > f 2 * X/NUMEL + f 3 * X * f 1 ⁄ π ⁄ NUMEL

(4-35)

or γ > f 1 and

(4-36)

Y e l > f 4 * Y/NUMEL + f 5 * Y * f 1 ⁄ γ ⁄ NUMEL

(4-37)

where NUMEL is the number of elements in the mesh. If f 2 , f 3 , f 4 , and f 5 are input as zero, then f 2 = 1.0 . Zienkiewicz – Zhu Plastic Strain Criterion p

The plastic strain error norm is defined as α

The plastic strain error is A =

∫(ε

p*

2

=

p 2

∫ ( ε * – ε ) dV --------------------------------------------------------------- . ∫ε

p2

p p 2 dV + ∫ ( ε * – ε ) dV

p 2

– ε ) dV . The allowable element plastic strain error is

AEPS = f 2 * A ⁄ NUMEL + f 3 * A * f 1 ⁄ α ⁄ NUMEL . The element will be subdivided when α > f 1 and A e l > AEPS . NUMEL is the number of elements in the mesh.

Main Index

84 Marc Volume A: Theory and User Information

Zienkiewicz-Zhu Creep Strain Criterion c

Zienkiewicz-Zhu creep strain error norm is defined as β

strain error is B =

∫(ε

c*

2

=

c 2

∫ ( ε * – ε ) dV -------------------------------------------------------------- . The creep ∫ε

c2

c c 2 dV + ∫ ( ε * – ε ) dV

c 2

– ε ) dV . The allowable element creep strain error is

AECS = f 2 * B ⁄ NUMEL + f 3 * B * f 1 ⁄ β ⁄ NUMEL . The element will be subdivided when β > f 1 and B e l > AECS . NUMEL is the number of elements in the mesh. Equivalent Values Criterion This method is based upon either relative or absolute testing using either the equivalent von Mises stress, the equivalent strain, equivalent plastic strain or equivalent creep strain. An element is subdivided if the current element value is a given fraction of the maximum (relative) or above a given absolute value.

σ

vm

m ax or σ >f σ >f vm 1 vm 2

m ax or ε ε vm > f 3 σ vm > f 4 vm Node Within A Box, Cylinder, or Sphere Criterion An element is subdivided if it falls within the specified box, cylinder, or sphere, respectively. If all of the nodes of the subdivided elements move outside the box, the elements are optionally merged back together. The location of this box can be repositioned using the UADAPBOX user subroutine. The criteria may also be used in conjunction with the WELD FLUX model definition option. In such cases, the motion of the weld source controls the location of the box. Nodes In Contact Criterion An element is subdivided if one of its nodes is associated with a new contact condition. In the case of a deformable-to-rigid contact, this implies that the node has touched a rigid surface. For deformable-todeformable contact, the node can be either a tied or retained node. Note that if chattering occurs, there can be an excessive number of elements generated. Use the level option to reduce this problem. Temperature Gradient Criterion An element is subdivided if the temperature gradient in the element is greater than a given fraction of the maximum gradient in the solution. This is the recommended method for heat transfer.

Main Index

CHAPTER 4 85 Introduction to Mesh Definition

Pressure Gradient Criterion An element is subdivided if the pressure gradient in the element is greater than a given fraction of the maximum gradient. This is the recommended method for diffusion analysis. Electrical Potential Criterion An element is subdivided if the electrical potential in the element is greater than a given fraction of the maximum gradient. This is the recommended method for electrostatic analysis. Magnetostatic Potential Criterion An element is subdivided if the magnetic potential in the element is greater than a given fraction of the maximum gradient. This is the recommended method for magnetostatic analysis. User-defined Criterion The UADAP user subroutine can be used to prescribe a user-defined adaptive criteria. The user subroutine UADAP2 can be used to prescribe a criterion for merging elements back (unsubdivide). Previously Refined Mesh Criterion Use the refined mesh from a previous analysis as the starting point to this analysis. The information from the previous adapted analysis is read in. Angle Between Shell Elements An element is refined if the change in angle between neighboring shell elements is larger than the given value. For each node, a normal is calculated by averaging shell element normals for elements connected to the node. If an element is to be subdivided, the angle used for checking is two times the angle between the averaged nodal normal and the element normal. Only the change in the normals from the undeformed shape is used to avoid that elements originally connected at an angle get subdivided immediately.

Automatic Global Remeshing In the analysis of metal or rubber, the materials may be deformed from some initial (maybe simple) shape to a final, very often, complex shape. During the process, the deformation can be so large that the mesh used to model the materials become highly distorted, and the analysis cannot go any further without using some special techniques (see Figure 4-27). Remeshing/rezoning in Marc is a useful feature to overcome the difficulties. Although global remeshing can be done manually using the REZONE option, the automatic global remeshing procedure is recommended.

Main Index

86 Marc Volume A: Theory and User Information

Figure 4-27 Mesh Distortion

Global remeshing can only be carried out on a contact body. Therefore, contact bodies are expected in the analysis with global remeshing. The basic steps, which are automatic in global remeshing, are as follows: 1. Analysis checks remeshing criteria at the end of each increment. When one of the remeshing criteria is met, analysis starts the remeshing procedure. 2. The deformed shape of the contact body is extracted. A new mesh is created by calling a stand-alone mesher or an internal mesher. 3. The new mesh is checked and corrected to avoid any penetration or contact loss to other contact bodies. 4. A data mapping is performed to transfer necessary data from the old, deformed mesh to the new mesh. 5. The contact tolerance is recalculated (if not specified by you) and the contact conditions are redefined. 6. Boundary conditions, if any, are transferred to the new mesh. 7. The analysis completes global remeshing and continues its computation based on the new mesh. Global remeshing/rezoning can be used in two- or three-dimensional solid body or a three-dimensional shell body. Most of the linear element types are supported. For shell, element type 75, 138, 139, and 140 are supported. Figure 4-28 shows a simple 3-D rubber seal remeshing. When remeshing/rezoning in 2-D, Marc finds the outline of the body to be rezoned and repairs the outline to remove possible penetration. Marc then calls the mesher to create a new mesh based on the clean outline.

Main Index

CHAPTER 4 87 Introduction to Mesh Definition

2-D Global Remeshing of Rubber Seal Insertion

3-D Global Remeshing of Connecting Rod Forging

Deep Drawing of a Box with Shell Remeshing Figure 4-28 3-D Automatic Remeshing and Rezoning of a Rubber Seal

When remeshing in 3-D with tetrahedral elements, Marc extracts and outputs the surface information together with other contact surface information and the meshing control parameters. A stand-alone 3-D mesher is then called to recreate 3-D surface mesh and the volume mesh. Contact check and volume checks are used to ensure no penetration and loss of volume in the new mesh. In 3-D hexahedral remeshing, hexahedral elements are build from the interior toward the surface. Projections are used to project nodes to the surface.

Main Index

88 Marc Volume A: Theory and User Information

When remeshing with 3-D shell elements, the 3-D mesher is called and surface mesh is created with triangular or quadrilateral elements Contact check is also performed to remove possible penetration. The automatic remeshing/rezoning feature uses the Updated Lagrange formulation by default. For global remeshing controls, the following commands are required: 1. REZONING – parameter to activate global remeshing controls. 2. ADAPT GLOBAL – used in both model definition and history definition options to specify global remeshing criteria, remeshing body, mesh generator, and meshing parameters. The following are the supported features and limitations: 1. Analysis type: Mechanical analysis, thermal-mechanical, thermal Joule mechanical, and electrostatic-structural coupled analysis are supported. 2. Element types: Low order, continuum element types are supported. In 2-D, these include both lower order quadrilateral and triangular elements. In 3-D, only lower order tetrahedral element types are supported including Herrmann type element 157. For 3-D shell elements, triangle element 138 and quadrilateral element 75, 139, and 140 are tested and supported. 3. Contact analysis: The remeshing body is a meshed contact body. Contact information, including boundary conditions defined through contact definitions, is re-determined based on the new mesh. Meshes that are not defined in contact bodies are not supported. • Support Rigid-Deformable contact • Support Deformable-Deformable contact • Support 2-D Self-contact 4. Boundary conditions: Boundary conditions are allowed in a remeshing body. These boundary conditions are transferred to the new mesh after remeshing. The new table style input format is required. These boundary conditions include: • Distributed load, flux, and current • Point load, flux, and current • Fixed displacement, temperature, and potential The above boundary conditions defined in the interior of a contact body are not supported. 5. Local adaptivity meshing is not supported. 6. Parallel computation is not supported. 7. Other analysis options: • PRE STATE model definition option is supported • CYCLIC SYMMETRY model definition option is supported • FLOW LINE and TRACK model definition options are supported

Main Index

CHAPTER 4 89 Introduction to Mesh Definition

Other supported global remeshing features include: 1. Remeshing procedures: • pause and continue: a standalone mesher is called within the analysis process. • stop and continue: analysis is stopped while a standalone mesher is called. This is to save memory usage during the remeshing process. Analysis is automatically resumed after remeshing is complete. 2. Forced remeshing control: • When global remeshing is selected with automatic time stepping scheme, remeshing will be forced when there is an element distortion during the analysis. This is carried out before the end of the increment. 3. Remeshing criteria: • • • • •

Element distortion check Increment frequency check Contact penetration check Equivalent strain change check Immediate meshing

4. Meshing control: • • • • • • • • • •

Based on input element size Based on input number of elements Change element types to triangle (2-D) or tetrahedral elements (3-D) Using Overlay mesher – quadrilateral elements Using advancing front mesher – quadrilateral or triangular elements Using Delauney triangulation mesher – triangular elements Using Hybrid MD Patran mesher – 3-D tetrahedral elements Using MD Patran MOM mesher - 3-D shell elements Using 3-D Overlay mesher – hexahedral elements (SuperForm only) Read user defined mesh files (.mesh)– also supported with RESTART and REAUTO options

5. Refinement and Coarsening control: • Local refinement based on surface curvatures • Local refinement based on thin section (2-D only) • Local refinement based on refinement boxes • Local refinement based on the USIZEOUTL user subroutine – for 2-D advancing front mesher and Delauney triangulation mesher • Interior coarsening using 2-D overlay mesher • Interior coarsening using 3-D Tetrahedral mesher or Hexahedral mesher 6. Special Features: • Support trimming load case to remove part of mesh in a contact body • Support 2-D contact body split using the USPLIT user subroutine.

Main Index

90 Marc Volume A: Theory and User Information

• Support user-defined meshing using the UMAKENET user subroutine. (3-D shell remeshing not supported)

Remeshing Criteria It is possible to choose any remeshing criteria simultaneously. How these criteria work is shown below. Note:

In general, frequent remeshing should be avoided for an effective and computationally efficient analysis. Also, since each remeshing and subsequent rezoning step involves interpolation and extrapolation of element variables, a possibility of error accumulation exists as the analysis progresses when remeshing occurs too frequently.

Increment Remeshing occurs at specified increment frequency. Element Distortion The identified body is remeshed when the distortion in the elements becomes large. For 2-D analysis, the distortion check is based on corner angles. Remeshing is performed if the following conditions are met: • Any inner angle is greater than 175° or less than 5° • Any inner angle change is greater than the user input data For 3-D analysis, a volume ratio is measured to determine if remeshing is required. A volume ratio is calculated based on each corner node and its connecting nodes. If v is the volume of a tetrahedron formed by nodes 1, 2, 3, and 4 and s is the triangle area of nodes 2, 3, and 4, then the ratio: h r = --l l or if h > l , r = --h Where h is the height and l is the equivalent length of the triangle. They can be calculated respectively by 3v h = -----s l =

s

The default control ratio is 0.01. Any volume ratio of each corresponding corner node smaller than this value forces the analysis to perform remeshing. Users can change this number to control the remeshing.

Main Index

CHAPTER 4 91 Introduction to Mesh Definition

Contact Penetration The identified body is remeshed when the curvature of the contact body is such that the current mesh cannot accurately detect penetration. For 2-D analysis, the penetration remeshing criteria is based upon examining the distance between the edge of an element and the contacted body. For 3-D analysis, the penetration is measured from the center of each boundary element face to the contacting surface. By default, remeshing is carried out if the penetration is greater than twice the contact tolerance and less than the target element size, where the contact tolerance is 0.05 of the smallest element length and the target element size is the element size for remeshing. This check does not apply to the self-contact situation. Also, this penetration limit can be given by user input to avoid too many remeshing operations. Remeshing is activated when the penetration distance reaches or exceeds the given penetration tolerance. Immediate The identified body is remeshed before performing any analysis. This control can also be used to change element types from quadrilateral elements to triangular elements or from hexahedral elements to tetrahedral elements. For example, it is possible to use this control to change an initially defined mesh using element type 7 (an 8 node-hexahedral element) to one using element type 157 (5 node-tetrahedral element) in order to use the tetrahedral remeshing capability. Strain Change Equivalent strain measures element deformation. This criterion keeps a record of the strain change after remeshing for each element. When any element of the body has a strain change greater than the control limit, the remeshing will start.

Remeshing Techniques For 2-D analysis, the remeshing techniques include outline extraction and repair and the mesh generation. After the outline is extracted and repaired, the mesh generator is called to create a mesh. For 2-D remeshing, the new mesh is created either through the built-in mesh generator using the overlay method or through a standalone mesh generator. When a standalone mesh generator is called, the program pauses while waiting for the mesh generator to create the new mesh. This can be memory intensive as both program and mesher are using the memory. Alternatively, the program can be stopped automatically while the mesh is being created, freeing the memory for the mesh generation. The program automatically resumes after the meshing is complete. In Marc, this is accomplished by using the AUTO RESTART option, -autorst, through the command line parameter. In Marc Mentat, this is instructed through JOB→JOB PARAMETERS→REMESHING CONTROL→STOP AND RESTART. For 3-D analysis, the outer surface of the contact body is extracted to a data file. This data file also contains remeshing control information. For tetrahedral meshing, a standalone 3-D mesher is called to create the surface mesh with triangles and then mesh the body with the tetrahedral elements. MD Patran

Main Index

92 Marc Volume A: Theory and User Information

mesher is used for the meshing. The new mesh nodes are adjusted to ensure that there is no penetration on the contact surfaces. Mesh Generation There are various 2-D and 3-D mesh generators available in Marc based on Advancing front, Overlay, and Delauney Triangulation techniques. Advancing front mesher This 2-D mesher creates either triangular, quadrilateral, or mixed triangular and quadrilateral mesh. For a given outline boundary, it starts by creating the elements along the boundary. The new boundary front is then formed when the layer of elements is created. This front advances inward until the complete region is meshed. Some smoothing technique is used to improve the quality of the elements. In general, this mesher works with any enclosed geometry and for geometry that has holes inside. The element size can be changed gradually from the boundary to the interior allowing smaller elements near the boundary with no tying constraints necessary (see Figure 4-29).

Figure 4-29 Advancing Front Meshing

Overlay meshing This is a quadrilateral mesh generator. The 2-D overlay mesher is included within Marc. It creates a quadrilateral mesh by forming a regular grid covering the center area of a body. A projection is then used to project all boundary nodes onto the real surface and form the outer layer elements. For the surface that is not in contact with other bodies, a cubic spline line is used to make the outline points smoother. This mesher also allows up to two level refinements on boundary where finer edges are needed to capture the geometry detail, and one level of coarsening in the interior where small elements are not necessary. This refinement and coarsening are performed using the tying constraints (see Figure 4-30).

Main Index

CHAPTER 4 93 Introduction to Mesh Definition

Figure 4-30 Local Refinement and Coarsening

In general, overlay meshing produces good quality elements. However, it does not take geometry with holes inside. It may not create a good mesh with geometry that has a very thin region or very irregular shape. Also, because the regular grid is created based on the global coordinate system, it may create a poor mesh if the geometry is not aligned with the global coordinate system. Delauney Triangulation This mesher creates only the triangular mesh. All the triangles satisfy the Delauney triangulation property. It takes all the seed points on the improved outlines as initial triangulation points. The triangulation is implemented by sequential insertion of new points into the triangulation until all the triangles satisfy the local density and quality requirement. Delauney triangulation algorithm assures the triangular mesh created has the best quality possible for the given set of points. The mesher also allows geometry to have holes inside the body and a variation of the elements with different sizes (Figure 4-31).

Figure 4-31 Meshing with Delauney Triangulation

MD Patran Tetrahedral Mesher MOM (Meshing-On-Mesh) Surface Mesher This is a 3-D surface mesher that creates a surface mesh based on an input mesh. The Meshing-on-mesh technology allows users to input a mesh, which is not good for the analysis, such as a distorted mesh or a mesh from the STL file.

Main Index

94 Marc Volume A: Theory and User Information

Tetrahedral Hybrid Mesher This 3-D mesher is based on Delaunay triangulation and advancing front technology. It generates tetrahedral elements based on an enclosed triangular surface mesh. 2-D Outline Extraction and Repair The outline consists of all the boundary edges of the contact body. Once the outline is extracted from the mesh, it is checked against other contacting bodies. The penetration from other contacting bodies is marked and the outline is corrected according to the penetration. If the outline is to be used for the advancing front or Delaunay mesher, some refinement and corrections are required to obtain better outline points. These outline points become boundary nodes in the new mesh and cannot be altered during the meshing process. The following procedures are taken by the program to prepare the new outline for the remeshing: Step 1:

Marking the hard points: The hard points are those points that represent important features of the original outline. Hard points are points that mark the beginning or end of the boundary portion of the mesh that is in contact or assigned with distributed boundary conditions, and the points that represent a sharp corner (such as 90° angle) or nodal boundary conditions.

Step 2:

Marking the points with target element size and minimum element size: The outline points are placed based on the target element size. The refinements and the user-defined outline points are allowed to change this control. However, the minimum element size is used to make sure the outline segment is not too small for the mesh generation.

Step 3:

Marking the points with curvature consideration: The curvature control is used to allow small outline segments to be used on the boundary where curvature radii are small. Three neighboring outline points are used to calculate the curvature radius. The associate curvature circle can then be formed by a number of line segments. With the same number of line segments used to approximate a circle, the curve with a smaller curvature circle gets a smaller line segment (Figure 4-31). Thus, we have a good variation of mesh size based on the curvature.

r

2πR l = ----------n

R

Figure 4-32 Curvature Consideration

Main Index

Step 4:

Marking the points with thin region consideration: In the area where a thin region is formed, small elements are preferred. This can be done by detecting the thin region and using smaller outline segments in the area. The segment length used for the thin area is to allow at least three elements to be presented across the thin area.

Step 5:

Smoothing the outline points: Smoothing is required on the outline so that the segment

CHAPTER 4 95 Introduction to Mesh Definition

length can gradually vary. Step 6:

Interpolations: Interpolation is the actual process to create a new outline based on the extracted outline and the marking of the outline points. Linear interpolation is used on the contact area to prevent penetration into the other contact bodies. Cubic spline line interpolation is used for the free surfaces.

3-D Surface Extraction and Meshing Similar to the 2-D outline extraction, 3-D surface faces are extracted before calling the mesh generator. If the original mesh is a hexahedral mesh, the boundary element faces are converted into triangles. The contact information on each element face is also extracted and output to a data file. A standalone mesher reads the information and perform the following steps: Step 1:

Construct surface information for contact projection and volume check.

Step 2:

Generate triangle surface mesh using MD Patran surface mesher (MOM). Surface elements are created observing the basic geometry features and contact conditions. Local refinement will be carried out based on the surface curvatures and user defined refinement boxes (see Figure 4-33). Small Elements

Large Elements

Figure 4-33 Local Refinement

Step 3:

Check contact penetration of new nodes and adjust coordinates if penetration is found.

Step 4:

Generate tetrahedral element mesh with MD Patran Hybrid mesher. By default, a coarsening factor is adopted to enlarge interior elements (see Figure 4-34).

Step 5:

Output the mesh to a data file.

Figure 4-34 Interior Coarsening

Main Index

96 Marc Volume A: Theory and User Information

Remeshing Based on the Target Number of Elements Instead of giving the element size, users can give the target number of elements for the remeshing. A uniform mesh assumption is used to compute the element size with the target number of elements. If the target number of elements is not provided, the number of elements in the current mesh is used. For 2-D analysis, the number of elements in the new mesh can also be controlled by using a percentage tolerance to ensure that the new mesh does not have too many or too few elements. However, this tolerance control requires remeshing trials and it cannot be used with the AUTO RESTART option. Remeshing with Boundary Conditions There are two types of boundary conditions that global remeshing needs to transfer from old mesh to the new one: • Contact boundary conditions: This type of boundary conditions includes friction, heat convection, radiation, symmetry or cyclic symmetry conditions. After a new mesh is created, these contact boundary conditions are automatically updated based on the new contact detection using the new mesh. • User defined boundary conditions: If the remeshing body has user defined boundary conditions, such as, point loads, distributed loads or fixed nodal displacements, the boundary conditions are transferred to the new mesh with two different approaches: a. Defined Set Approach This approach allows users to directly apply boundary conditions to the mesh entities, such as, element faces, edges, or nodes. Each boundary condition is arranged in a defined set with a set name and a set type. Currently, the set type can be either a node or an element edge or face set. The element edge sets in 2-D and face sets in 3-D are typically those of distributed boundary conditions. Edges or faces in the set can be continuous or discontinuous. During the remeshing stage, the boundaries of these edges or faces are marked and preserved. This allows the new edges or faces to be created coincident with the old edges or faces in the set. After remeshing, the element edges or faces in the set are replaced with the new element edges or faces (see Figure 4-35). The node ids in nodal sets are automatically replaced with the new node ids (see Figure 4-36).

Figure 4-35 Distributed Loads Transfer

Main Index

CHAPTER 4 97 Introduction to Mesh Definition

Figure 4-36 Point Loads Transfer

The nodal displacement or temperature conditions applying to all the nodes of an element edge or face are treated as an element edge or face boundary condition. This means the new nodes created on the same element edge or face will have the same displacement or temperature boundary conditions. In 2-D, an element edge or face can take up to four boundary condition sets for the remeshing. In 3-D, the number of sets on the same element face is two. There is no limitation on the node set. b. Geometry Attachment Approach Boundary conditions can be assigned to geometry entities, such as points, curves and surfaces. In this approach, these geometry entities are attached to the mesh entities of a remeshing body, such as, a point attached to a node and a curve attached to a set of element edges. During remeshing, mesh entities associated with these geometry entities are marked and preserved. After remeshing, the geometry entities are re-attached to the new mesh entities. By doing so, boundary conditions assigned to these geometry entities are automatically applied to the new mesh (see Figure 4-37). In 3-D, the attached surface ID number cannot exceed 99 and only one surface can be attached to an element face. In 3-D, curves can also be attached to the element edges but only nodal displacement conditions are supported (see Figure 4-38). Geometry attachments are shown.

Figure 4-37 Distributed Load with Curve Attachment

Main Index

98 Marc Volume A: Theory and User Information

Figure 4-38 Geometry Attachment Boundary Conditions in 3-D

History Data Mapping Technique History data such as stress, strain or temperature need to be transferred to the new mesh (dashed red), from the old mesh (solid black). In general, this is carried out in the following steps (see Figure 4-39):

Figure 4-39 Locate New Nodes in Old Mesh

• Store nodal data at the nodal position based on the old mesh • If old mesh is formed of quadrilateral or hexahedral elements, subdivide into triangles or tetrahedrals, respectively. • Extrapolate data from the integration points to the nodal position • If old mesh is formed of quadrilateral or hexahedral elements, determine values at extra nodes • Compute weighted averaged nodal data based on the contributions from different elements • Locate new nodes in the old triangular/tetrahedral region • Determine the value at the new node based upon linear interpolation within triangular/tetrahedral region • Data in the new integration points can be computed based on interpolating from the nodal data in the new mesh After data mapping, new equilibrium is achieved at the end of the new increment.

Main Index

Chapter 5 Structural Procedure Library

5

Main Index

Structural Procedure Library

J

Linear Analysis

J

Nonlinear Analysis

J

Fracture Mechanics

J

Dynamics

J

Inertia Relief

J

Rigid-Plastic Flow

J

Superplasticity

J

Soil Analysis

J

Mechanical Wear

J

Design Sensitivity Analysis

J

Design Optimization

J

Defined Initial State with Result Data from Previous Analysis (including AXITO3D) 209

J

Steady State Rolling Analysis

J

Structural Zooming Analysis

J

Cure-Thermal-Mechanically Coupled Analysis

J

References

100 105 147

165 185 188

191 193

221

197 200

202

211 214 216

100 Marc Volume A: Theory and User Information

This chapter describes the analysis procedures in Marc applicable to structural problems. These procedures range from simple linear elastic analysis to complex nonlinear analysis. A large number of options are available, but you need to consider only those capabilities that are applicable to your physical problem. This chapter provides technical background information as well as usage information about these capabilities.

Linear Analysis Linear analysis is the type of stress analysis performed on linear elastic structures. Because linear analysis is simple and inexpensive to perform and generally gives satisfactory results, it is the most commonly used structural analysis. Nonlinearities due to material, geometry, or boundary conditions are not included in this type of analysis. The behavior of an isotropic, linear, elastic material can be defined by two material constants: Young’s modulus E , and Poisson’s ratio v . Marc allows you to perform linear elastic analysis using any element type in the program. Various kinematic constraints and loadings can be prescribed to the structure being analyzed; the problem can include both isotropic and anisotropic elastic materials. The principle of superposition holds under conditions of linearity. Therefore, several individual solutions can be superimposed (summed) to obtain a total solution to a problem. Linear analysis does not require storing as many quantities as does nonlinear analysis; therefore, it uses the core memory more sparingly. The ELASTIC parameter uses the assembled and decomposed stiffness matrices to arrive at repeated solutions for different loads. Note:

Linear analysis is always the default analysis type in the Marc program.

Linear analysis in Marc requires only the basic input. Table 5-1 shows a subset of the Marc options and parameters which are often used for linear analysis. Table 5-1

Basic Input

Type Parameter

Main Index

Name TITLE SIZING ELEMENTS ELASTIC ALL POINTS CENTROID ADAPTIVE FOURIER END

CHAPTER 5 101 Structural Procedure Library

Table 5-1

Basic Input (continued)

Type Model Definition

Name CONNECTIVITY COORDINATES GEOMETRY ISOTROPIC FIXED DISP DIST LOADS POINT LOAD CASE COMBIN END OPTION

More complex linear analyses require additional data blocks. 1. The ELASTIC parameter allows solutions for the same structural system with different loadings (multiple loading analysis). When using the ELASTIC parameter, you must apply total loads, rather than incremental quantities (for example., total force, total moment, total temperature) in subsequent increments. 2. The RESTART option, used with the ELASTIC parameter and/or CASE COMBIN option, stores individual load cases in a restart file. You can also store the decomposed stiffness matrix for later analyses. 3. The CASE COMBIN model definition option combines the results obtained from different loading cases previously stored in a restart file. 4. The ADAPTIVE option can be used to improve the accuracy of the analysis. 5. The J-INTEGRAL option allows the study of problems of linear fracture mechanics. 6. The FOURIER option allows the analysis of axisymmetric structures subjected to arbitrary loadings. 7. The ORTHOTROPIC or ANISOTROPIC model definition option activates the anisotropic behavior option. In addition, the ANELAS, HOOKLW, ANEXP, and ORIENT user subroutines define the mechanical and thermal anisotropy and the preferred orientations. 8. You can use both the linear SPRINGS and FOUNDATION options in a linear stress analysis.

Accuracy It is difficult to predict the accuracy of linear elastic analysis without employing special error estimation techniques. An inaccurate solution usually exhibits itself through one or more of the following phenomena: • Strong discontinuities in stresses between elements • Strong variation in stresses within an element • Stresses that oscillate from element to element

Main Index

102 Marc Volume A: Theory and User Information

Error Estimates The ERROR ESTIMATE option can also be used to obtain an indication of the quality of the results. You can have the program evaluate the geometric quality of the mesh by reporting the aspect ratios and skewness of the elements. In a large deformation updated Lagrange analysis, you can also observe how these change during the analysis, which indicates mesh distortion. When the mesh distortion is large, it is a good idea to do a rezoning step. The ERROR ESTIMATE option can also be used to evaluate the stress discontinuity between elements. Marc first calculates a nodal stress based upon the extrapolated integration point values. These nodal values are compared between adjacent elements and reported. Large discrepancies indicate an inability of the mesh to capture high stress gradients, in which case you should refine the mesh and rerun the analysis or use local adaptive meshing. The ERROR ESTIMATE option can be used for either linear or nonlinear analysis.

Adaptive Meshing The ADAPTIVE option can be used to insure that a certain level of accuracy is achieved. The elastic analysis is repeated with a new mesh until the level of accuracy requested is achieved.

Fourier Analysis Through Fourier expansion, Marc analyzes axisymmetric structures that are subjected to arbitrary loading. The FOURIER option is available only for linear analysis. During Fourier analysis, a three-dimensional analysis decouples into a series of independent twodimensional analyses, where the circumferential distribution of displacements and forces are expressed in terms of the Fourier series. Both mechanical and thermal loads can vary arbitrarily in the circumferential direction. You can determine the structure’s total response from the sum of the Fourier components. The Fourier formulation is restricted to axisymmetric structures with linear elastic material behavior and small strains and displacements. Therefore, conditions of linearity are essential and material properties must remain constant in the circumferential direction. To use Fourier expansion analysis in Marc, the input must include the following information: • The FOURIER parameter allocates storage for the series expansion. • Fourier model definition blocks for as many series as are needed to describe tractions, thermal loading, and boundary conditions. Number the series sequentially in the order they occur during the FOURIER model definition input. Three ways to describe the series are listed below: • Specify coefficients a 0, a 1, b 1 … on the Fourier model definition blocks. • Describe F ( θ ) (where θ is the angle in degrees about the circumference) in point-wise fashion with an arbitrary number of pairs [ θ, F ( θ ) ] given on the blocks. Marc forms the corresponding series coefficients. • Generate an arbitrary number of [ θ, F ( θ ) ] pairs using the UFOUR user subroutine and let the program calculate the series coefficients.

Main Index

CHAPTER 5 103 Structural Procedure Library

You can obtain the total solution at any position around the circumference by superposing the components already calculated after completion of all increments required by the analysis. The CASE COMBIN option calculates this total solution by summing the individual harmonics which are stored in the restart file. The number of steps or increments needed for analysis depends on the number of harmonics that are chosen. For a full analysis with symmetric and antisymmetric load cases, the total number of increments equals twice the number of harmonics. Table 5-2 shows which Fourier coefficients are used for a given increment. Table 5-2

Fourier Coefficients – Increment Number

LOAD TERMS INC.

1st DOF,Z

2nd DOF,R

3rd DOF,θ

0

a0

a0

0

1

0

0

a0

2

a1

a1

b1

3

b1

b1

a1

.

.

.

.

.

.

.

.

.

.

.

.

2n

an

an

bn

2n + 1

bn

bn

an

The magnitude of concentrated forces should correspond to the value of the ring load integrated around the circumference. Therefore, if the Fourier coefficients for a varying ring load p ( θ ) are found from the [ θ, p ( θ ) ] distribution, where p ( θ ) has the units of force per unit length, the force magnitude given in the point load block should equal the circumference of the loaded ring. If p ( θ ) is in units of force per radian, the point load magnitude should be 2π . The Fourier series can be found for varying pressure loading from [ θ, p ( θ ) ] input with p expressed in force per unit area. Marc calculates the equivalent nodal forces and integrates them around the circumference. The distributed load magnitude in the distributed loads block should be 1.0. Table 5-3 shows the elements in the program that can be used for Fourier analysis.

Main Index

104 Marc Volume A: Theory and User Information

Table 5-3

Elements Used for Fourier Analysis

Element Type

Description

62

8-node

73

8-node with reduced integration

63

8-node for incompressible behavior

74

8-node for incompressible behavior with reduced integration

90

3-node shell

Technical Background The general form of the Fourier series expansion of the function F ( θ ) is shown in the equation below. ∞

F ( θ ) = a0 +

∑

( a n cos nθ + b n sin nθ )

(5-1)

n = 1

This expression expands the displacement function in terms of sine and cosine terms. A symmetric and an antisymmetric problem are formulated for each value of n . The displacements for the symmetric case, expressed in terms of their nodal values, are u n = [ N 1, N 2, … ] cos nθ { u n } e v n = [ N 1, N 2, … ] cos nθ { v n } e wn

= [ N 1, N 2 ,

(5-2)

… ] sin n θ { w n } e

Nodal forces are n

Z = Z0 +

∑ Z n cos nθ 1 n

R = R0 +

∑ R n cos nθ

(5-3)

1 n

T = T0 +

∑ T n sin nθ 1

The value n = 0 is a special case in Fourier analysis. If only the symmetric expansion terms are used, the formulation defaults to the fully axisymmetric two-dimensional analysis. The antisymmetric case for n = 0 yields a solution for the variable θ that corresponds to loading in the tangential direction. Analyze axisymmetric solids under pure torsion in this way.

Main Index

CHAPTER 5 105 Structural Procedure Library

Modal Shapes and Buckling Load Estimations During a Fourier Analysis During a Fourier analysis, Marc can be asked to estimate both the modal shapes and buckling loads for each harmonic in the analysis. In either case, the program performs a Fourier analysis first and then estimates the modal shapes/buckling load at prescribed harmonic numbers. In addition to the input data required for a Fourier analysis (FOURIER parameter and FOURIER model definition option), the following must also be added: DYNAMIC parameter and MODAL INCREMENT model definition option; BUCKLE parameter and BUCKLE INCREMENT model definition option, for Fourier modal shape and Fourier buckling load estimations, respectively. In the Fourier modal analysis, the mass matrix in the eigenvalue equation is a constant matrix. The stiffness matrix in the eigenvalue equation is the one associated with a prescribed harmonic of the Fourier analysis. The expression of the eigenvalue equation is: [ K m ]φ – ω 2 [ M 0 ]φ = 0

(5-4)

m

0

where [ K ] is the stiffness matrix associated with the mth harmonic of the Fourier analysis and [ M ] is a constant matrix. Multiple modes for each harmonic can be extracted. Similarly, in a Fourier buckling analysis, the stiffness matrices in the eigenvalue equation are (respectively); the linear elastic stiffness matrix and the geometric stiffness matrix associated with the prescribed harmonic of the Fourier analysis. The eigenvalue equation is expressed m

m

[ K ]φ – λ [ K g ]φ = 0 m

(5-5) m

where [ K ] is the linear elastic stiffness matrix and [ K g ] is the geometric stiffness matrix, associated with the mth harmonic of the Fourier analysis. The stresses used in the calculation of the geometric stiffness matrix are those associated with the symmetric load case, m = 0 . Multiple buckling load estimations for each harmonic are also available.

Nonlinear Analysis The finite element method can be used for nonlinear, as well as linear, problems. Early development of nonlinear finite element technology was mostly influenced by the nuclear and aerospace industries. In the nuclear industry, nonlinearities are mainly due to the nonlinear, high-temperature behavior of materials. Nonlinearities in the aerospace industry are mainly geometric in nature and range from simple linear buckling to complicated post-bifurcation behavior. Nonlinear finite element techniques have become popular in metal forming manufacturing processes, fluid-solid interaction, and fluid flow. In recent years, the areas of biomechanics and electromagnetics have seen an increasing use of finite elements. A problem is nonlinear if the force-displacement relationship depends on the current state (that is, current displacement, force, and stress-strain relations). Let u be a generalized displacement vector, P a

Main Index

106 Marc Volume A: Theory and User Information

generalized force vector, and K the stiffness matrix. The expression of the force-displacement relation for a nonlinear problem is P = K ( P, u )u

(5-6)

Linear problems form a subset of nonlinear problems. For example, in classical linear elastostatics, this relation can be written in the form P = Ku

(5-7)

where the stiffness matrix K is independent of both u and P . If the matrix K depends on other state variables that do not depend on displacement or loads (such as temperature, radiation, moisture content, etc.), the problem is still linear. Similarly, if the mass matrix is a constant matrix, the following undamped dynamic problem is also linear: P = Mu·· + Ku

(5-8)

There are three sources of nonlinearity: material, geometric, and nonlinear boundary conditions. Material nonlinearity results from the nonlinear relationship between stresses and strains. Considerable progress has been made in attempts to derive the continuum or macroscopic behavior of materials from microscopic backgrounds, but, up to now, commonly accepted constitutive laws are phenomenological. Difficulty in obtaining experimental data is usually a stumbling block in mathematical modeling of material behavior. A plethora of models exist for more commonly available materials like elastomers and metals. Other material model of considerable practical importance are: composites, viscoplastics, creep, soils, concrete, powder, and foams. Figure 5-1 shows the elastoplastic, elasto-viscoplasticity, and creep. Although the situation of strain hardening is more commonly encountered, strain softening and localization has gained considerable importance in recent times. σ

σ

ε

Elasto-Plastic Behavior

ε Elasto-Viscoplastic Behavior

ε

c

σ

Creep Behavior Figure 5-1

Main Index

Material Nonlinearity

t

ε

CHAPTER 5 107 Structural Procedure Library

Geometric nonlinearity results from the nonlinear relationship between strains and displacements on the one hand and the nonlinear relation between stresses and forces on the other hand. If the stress measure is conjugate to the strain measure, both sources of nonlinearity have the same form. This type of nonlinearity is mathematically well defined, but often difficult to treat numerically. Two important types of geometric nonlinearity occur: a. The analysis of buckling and snap-through problems (see Figure 5-2 and Figure 5-3). P

Linear

S

P u

Pc

Neutral Uns

u Figure 5-2

Buckling P

P

u

u Figure 5-3

Snap-Through

b. Large strain problems such as manufacturing, crash, and impact problems. In such problems, due to large strain kinematics, the mathematical separation into geometric and material nonlinearity is nonunique. Boundary conditions and/or loads can also cause nonlinearity. Contact and friction problems lead to nonlinear boundary conditions. This type of nonlinearity manifests itself in several real life situations; for example, metal forming, gears, interference of mechanical components, pneumatic tire contact, and crash (see Figure 5-4). Loads on a structure cause nonlinearity if they vary with the displacements of the structure. These loads can be conservative, as in the case of a centrifugal force field (see Figure 5-5);

Main Index

108 Marc Volume A: Theory and User Information

they can also be nonconservative, as in the case of a follower force on a cantilever beam (see Figure 5-6). Also, such a follower force can be locally nonconservative, but represent a conservative loading system when integrated over the structure. A pressurized cylinder (see Figure 5-7) is an example of this.

Main Index

Figure 5-4

Contact and Friction Problem

Figure 5-5

Centrifugal Load Problem (Conservative)

CHAPTER 5 109 Structural Procedure Library

P

P

Figure 5-6

Follower Force Problem (Nonconservative)

Figure 5-7

Pressurized Cylinder (Globally Conservative)

The three types of nonlinearities are described in detail in the following sections.

Geometric Nonlinearities Geometric nonlinearity leads to two types of phenomena: change in structural behavior and loss of structural stability. There are two natural classes of large deformation problems: the large displacement, small strain problem and the large displacement, large strain problem. For the large displacement, small strain problem, changes in the stress-strain law can be neglected, but the contributions from the nonlinear terms in the strain displacement relations cannot be neglected. For the large displacement, large strain problem, the constitutive relation must be defined in the correct frame of reference and is transformed from this frame of reference to the one in which the equilibrium equations are written.

Main Index

110 Marc Volume A: Theory and User Information

The collapse load of a structure can be predicted by performing an eigenvalue analysis. If performed after the linear solution (increment zero), the Euler buckling estimate is obtained. An eigenvalue problem can be formulated after each increment of load; this procedure can be considered a nonlinear buckling analysis even though a linearized eigenvalue analysis is used at each stage. The kinematics of deformation can be described by the following approaches: A. Lagrangian Formulation B. Eulerian Formulation C. Arbitrary Eulerian-Lagrangian (AEL) Formulation The choice of one over another can be dictated by the convenience of modeling physics of the problem, rezoning requirements, and integration of constitutive equations. Lagrangian Formulation In the Lagrangian method, the finite element mesh is attached to the material and moves through space along with the material. In this case, there is no difficulty in establishing stress or strain histories at a particular material point and the treatment of free surfaces is natural and straightforward. The Lagrangian approach also naturally describes the deformation of structural elements; that is, shells and beams, and transient problems, such as the indentation problem shown in Figure 5-8.

sz

Δu

Figure 5-8

Indentation Problem with Pressure Distribution on Tool

This method can also analyze steady-state processes such as extrusion and rolling. Shortcomings of the Lagrangian method are that flow problems are difficult to model and that the mesh distortion is as severe as the deformation of the object. Severe mesh degeneration is shown in Figure 5-9b. However, recent advances in adaptive meshing and rezoning have alleviated the problems of premature termination of the analysis due to mesh distortions as shown in Figure 5-9c. The Lagrangian approach can be classified in two categories: the total Lagrangian method and the updated Lagrangian method. In the total Lagrangian approach, the equilibrium is expressed with the original undeformed state as the reference; in the updated Lagrangian approach, the current configuration acts as the reference state. The kinematics of deformation and the description of motion is given in Figure 5-10 and Table 5-4.

Main Index

CHAPTER 5 111 Structural Procedure Library

(b) Deformed Mesh Before Rezoning

(a) Original (Undeformed Mesh)

(c) Deformed Mesh After Rezoning Figure 5-9

Rezoning Example

f

Previous

Δu

t=n

Current t=n+1

Fn

un + 1 un

F

Reference t=0 Fn+1 = fFn Figure 5-10 Description of Motion

Depending on which option you use, the stress and strain results are given in different form as discussed below. If the LARGE DISP or LARGE STRAIN parameters are not used, the program uses and prints “engineering” stress and strain measures. These measures are suitable only for analyses without large incremental or total rotation or large incremental or total strains. Using the LARGE DISP parameter, Marc uses the total Lagrangian method. The program uses and prints second Piola-Kirchhoff stress and Green-Lagrange strain. These measures are suitable for analysis with large incremental rotations and large incremental strains.

Main Index

112 Marc Volume A: Theory and User Information

Table 5-4

Kinematics and Stress-Strain Measures in Large Deformation

Configuration Measures

Reference (t = 0 or n)

Current (t = n + 1)

Coordinates

X

x

Deformation Tensor

C (Right Cauchy-Green)

b (Left Cauchy-Green)

Strain Measure

E (Green-Lagrange)

e (Logarithmic)

F (Deformation Gradient) Stress Measure

S (second Piola-Kirchhoff)

σ (Cauchy)

P (first Piola-Kirchhoff)

With the LARGE STRAIN, Marc uses Cauchy stresses and true strains. This is suitable for analyses with large elastic and plastic strains. Stress and strain components are printed with respect to the current state. Theoretically and numerically, if formulated mathematically correct, the two formulations yield exactly the same results. However, integration of constitutive equations for certain types of material behavior (for example, plasticity) make the implementation of the total Lagrange formulation inconvenient. If the constitutive equations are convected back to the original configuration and proper transformations are applied, then both formulations are equivalent. However, for deformations involving excess distortions, ease of rezoning favors the updated Lagrangian formulation. This is reflected in the fact that a rezoned mesh in the current state is mapped back to excessively distorted mesh leading to negative Jacobian in the total Lagrangian formulation. The terminology total and updated Lagrangian has been used with some vagueness [1, 2]. In this document, for a sequence of incremental motions at t = 0, 1, 2, …n and n + 1 , the total Lagrangian formulation entails the use of t = 0 configuration as reference; while in the updated Lagrangian configuration, the t = n + 1 (unequilibriated) configuration is the reference. Total Lagrangian Procedure The total Lagrangian procedure can be used for linear or nonlinear materials, in conjunction with static or dynamic analysis. Although this formulation is based on the initial element geometry, the incremental stiffness matrices are formed to account for previously developed stress and changes in geometry. This method is suitable for the analysis of nonlinear elastic problems (for instance, with the Mooney, Ogden, or NLELAST material behavior or the HYPELA2 user subroutine). The total Lagrangian approach is also useful for problems in plasticity and creep, where moderately large rotations but small strains occur. A case typical in problems of beam or shell bending. However, this is only due to the approximations involved. To activate the large displacement (total Lagrangian approach) option in Marc, use the LARGE DISP parameter. Include the FOLLOW FOR parameter for follower force (for example, centrifugal or pressure load) problems. This parameter forms all distributed loads on the basis of the current geometry. Do not use the CENTROID parameter with this parameter. Always use residual load corrections with this parameter. To input control tolerances for large displacement analysis, use CONTROL model definition option.

Main Index

CHAPTER 5 113 Structural Procedure Library

In the total Lagrangian approach, the equilibrium can be expressed by the principle of virtual work as:

∫

S i j δE i j dV =

V0

∫ V

0

b i δη i dV +

∫ A

0

0

t i δη i dA

(5-9)

0 0

Here S i j is the symmetric second Piola-Kirchhoff stress tensor, E i j , is the Green-Lagrange strain, b i is 0

the body force in the reference configuration, t i is the traction vector in the reference configuration, and η i is the virtual displacements. Integrations are carried out in the original configuration at t = 0 . The strains are decomposed in total strains for equilibrated configurations and the incremental strains between t = n and t = n + 1 as: n+1

Ei j

n

= E i j + ΔE i j

(5-10) n

while the incremental strains are further decomposed into linear, ΔE i j and nonlinear, ΔE i j parts as: n

ΔE i j = ΔEi j + ΔE i j where ΔE is the linear part of the incremental strain expressed as: n ⎛ ∂u kn ⎞ ∂Δu k 1 ∂Δu i ∂Δu j 1 ⎛ ∂u k ⎞ ∂Δu k ΔE = --- ------------ + ------------ + --- ⎜ ---------⎟ ⎛ -------------⎞ + ⎜ ---------⎟ ⎛ -------------⎞ 2 ∂X j ∂X i 2 ⎝ ∂X i⎠ ⎝ ∂X j ⎠ ⎝ ∂X j⎠ ⎝ ∂X i ⎠

The second term in the bracket in Equation (5-11) is the initial displacement effect. ΔE part of the incremental strain expressed as: ΔE

n

1 ∂Δu k ∂Δu k = --- ⎛ -------------⎞ ⎛ -------------⎞ 2 ⎝ ∂X i ⎠ ⎝ ∂X j ⎠

(5-11) n

is the nonlinear

(5-12)

Linearization of equilibrium of Equation (5-9) yields: { K 0 + K 1 + K 2 }δu = F – R where K 0 is the small displacement stiffness matrix defined as ( K0 )i j =

∫ V0

Main Index

0

0

β i m n D m n p q β p q j dV

(5-13)

114 Marc Volume A: Theory and User Information

K 1 is the initial displacement stiffness matrix defined as ( K1 )i j =

∫ V

u

u

u

0

u

u

{ β i m n D m n p q β p q j + β i m n D m n p q β p qj + β i m n D m n p q β p q j } dv

0 0

u

in the above equations, β i m n and β i m n are the constant and displacement dependent symmetric shape function gradient matrices, respectively, and D m n p q is the material tangent, and K 2 is the initial stress stiffness matrix ( K2 )i j =

∫

N i , k N j , l S k l dV

V0

in which S kl is the second Piola-Kirchhoff stresses and N i, k is the shape function gradient matrix. Also, δu is the correction displacement vector. Refer to Chapter 11 in this manual for more details on the solution procedures. F and R are the external and internal forces, respectively. This Lagrangian formulation can be applied to problems if the undeformed configuration is known so that integrals can be evaluated, and if the second Piola-Kirchhoff stress is a known function of the strain. The first condition is not usually met for fluids, because the deformation history is usually unknown. For solids, however, each analysis usually starts in the stress-free undeformed state, and the integrations can be carried out without any difficulty. For viscoelastic fluids and elastic-plastic and viscoplastic solids, the constitutive equations usually supply an expression for the rate of stress in terms of deformation rate, stress, deformation, and sometimes other (internal) material parameters. The relevant quantity for the constitutive equations is the rate of stress at a given material point. It, therefore, seems most obvious to differentiate the Lagrangian virtual work equation with respect to time. The rate of virtual work is readily found as

∫ V

∂v k ∂δη k · S i j δE i j + S i j --------- ------------- dV = ∂X i ∂X j

0

∫ V

0

· b i δη i dV +

∫ A

· t i δη i dA

(5-14)

0

This formulation is adequate for most materials, because the rate of the second Piola-Kirchhoff stress can be written as · · · S i j = S i j ( E k l , S m n, E p q )

(5-15)

For many materials, the stress rate is even a linear function of the strain rate · · S i j = D i j k l ( S m n, E p q )E k l

Main Index

(5-16)

CHAPTER 5 115 Structural Procedure Library

Equation (5-14) supplies a set of linear relations in terms of the velocity field. The velocity field can be solved non iteratively and the displacement can be obtained by time integration of the velocities. The second Piola-Kirchhoff stress for elastic and hyperelastic materials is a function of the GreenLagrange strain defined below: Si j = Si j ( Ek l )

(5-17)

If the stress is a linear function of the strain (linear elasticity) Si j = Di j k l Ek l

(5-18)

the resulting set of equations is still nonlinear because the strain is a nonlinear function of displacement. Updated Lagrangian Procedure The Updated Lagrange formulation takes the reference configuration at t = n + 1 . True or Cauchy stress and an energetically conjugate strain measure, namely the true strain, are used in the constitutive relationship. The updated Lagrangian approach is useful in: a. analysis of shell and beam structures in which rotations are large so that the nonlinear terms in the curvature expressions may no longer be neglected, and b. large strain elasticity and plasticity analysis. In general, this approach can be used to analyze structures where inelastic behavior (for example, plasticity, viscoplasticity, or creep) causes the large deformations. The (initial) Lagrangian coordinate frame has little physical significance in these analyses since the inelastic deformations are, by definition, permanent. The LARGE STRAIN parameter specifies large strain analysis within the framework of Updated Lagrange formulation. It signals Marc to calculate a geometric stiffness matrix and the initial stress stiffness matrix based on the current deformed configuration. Note:

Because large strain analysis involves nonlinearity, the CENTROID parameter must not be used with this option.

For large strain analysis for 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, to overcome the numerical difficulties resulting from the volumetric constraints. 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 incremental strain into an elastic part and a plastic part, together with a mean normal return-mapping algorithm. In this case, volumetric strain in a lower-order plane strain,

Main Index

116 Marc Volume A: Theory and User Information

axisymmetric or 3-D brick element is assumed to be constant for von Mises plasticity to overcome volumetric locking because of the possible large and incompressible plastic deformation. Marc can also use a procedure (LARGE STRAIN parameter with option 2) based on a multiplicative decomposition of deformation gradient into an elastic part and a plastic part together with a radial returnmapping algorithm for large strain elastic-plastic analysis. A mixed formulation is used to deal with the problem associated with volume constraints. This procedure is only available for continuum elements. Because Herrmann elements do not support additive plasticity, Marc internally switches to the multiplicative procedure. Herrmann elements have additional pressure degrees of freedom which increase numerical costs; hence, it is generally more efficient to use displacement-based elements. Marc uses Cauchy stress (true stress) and logarithmic strain with Updated Lagrange formulation. It is instructive to derive the stiffness matrices for the updated Lagrangian formulation starting from the virtual work principle in Equation (5-9). Direct linearization of the left-hand side of Equation (5-9) yields:

∫ V

∫

S i j ( d( δE i j ) ) dV =

∇η i k σ k j ∇Δu i j dv

(5-19)

Vn + 1

0

where Δu and η are actual incremental and virtual displacements respectively, and σ k j is Cauchy stress tensor.

∫ V

∫

dS i j δE i j dV =

s

s

∇ η i j L i j k l ∇ ( Δu k l ) dv

(5-20)

Vn + 1

0 s

∇ denotes the symmetric part of ∇ , which represents the gradient operator in the current configuration. Also, in Equation (5-19) and Equation (5-20), three identities are used: 1 σ i j = --- F i m S m n F j n J s

δE i j = F m i ∇ η m n F n j

(5-21)

and 1 L i j k l = --- F i m F j n F k p F l q D m n p q J in which D m n p q represents the material moduli tensor in the reference configuration which is convected to the current configuration, L i j k . This yields: { K 1 + K 2 }δu = F – R

Main Index

(5-22)

CHAPTER 5 117 Structural Procedure Library

where K 1 is the material stiffness matrix written as

∫

( K1 )i j = V

βi m n Lm n p q βp q j

n+1

in which β i m n is the symmetric gradient operator-evaluated in the current configuration and σ k l is the Cauchy stresses and K 2 is the geometric stiffness matrix written as ( K2 )i j =

∫

σ k l N i, k N j, l dv

Vn + 1

while F and R are the external and internal forces, respectively. Keeping in view that the reference state is the current state, a rate formulation analogous to Equation (5-14) can be obtained by setting: F i j = δ i j,

δE i j = δd i j,

∂ ∂ --------- = --------, ∂X i ∂x i

Si j = σi j

(5-23)

where F is the deformation tensor, and d is the rate of deformation. Hence,

∫ Vn + 1

∂v k ∂δη k ∇ σ i j δd i j + σ i j --------- ------------- dv = ∂x i ∂x j

∫ Vn + 1

· b i δη i dv +

∫

t·i δη i da

(5-24)

An + 1

in which b i and t i is the body force and surface traction, respectively, in the current configuration ∇

In this equation, σ i j is the Truesdell rate of Cauchy stress which is essentially a Lie derivative of Cauchy stress obtained as: · –1 –1 ∇ σ i j = F i n ( JF n k σ k l F m l ) F m j

(5-25)

The Truesdell rate of Cauchy stress is materially objective implying that if a rigid rotation is imposed on the material, the Truesdell rate vanishes, whereas the usual material rate does not vanish. This fact has important consequences in the large deformation problems where large rotations are involved. The constitutive equations can be formulated in terms of the Truesdell rate of Cauchy stress as: ∇ σ i j = Li j k dk

Main Index

(5-26)

118 Marc Volume A: Theory and User Information

Eulerian Formulation In analysis of fluid flow processes, the Lagrangian approach results in highly distorted meshes since the mesh convects with the material. Hence, an alternative formulation, namely Eulerian, is used to describe the motion of the body. In this method, the finite element mesh is fixed in space and the material flows through the mesh. This approach is particularly suitable for the analysis of steady-state processes, such as the steady-state extrusion or rolling processes shown in Figure 5-11.

Figure 5-11 Rolling Analysis

The governing differential equations of equilibrium for fluid flow through an enclosed volume are now written as: D ( ρv i ) ∂σ i j ------------------ = ρb i + ---------∂x j Dt

(5-27)

D where, ------ is the material time derivative of a quantity and v is the velocity of the particle flowing Dt through the mesh. For an incompressible fluid, Equation (5-27) along with continuity equation (mass conservation) yields: ∂σ i j ∂v i ∂v i ρ -------- + ρv j -------- = ρb i + ---------∂t ∂x j ∂x j

(5-28)

The left-hand side of Equation (5-28) represents the local rate of change augmented by the convection effects. The same principle can be called to physically explain the material time derivative of Cauchy stress; that is, Truesdell rate of Cauchy stress. It can be seen from Equation (5-25) that: ∂v j ∂v k ∂v i ∇ · σ i j = σ i j – --------- σ k j – σ i k --------- + σ i j --------∂x k ∂x k ∂x k

(5-29)

The second and third terms on the right-hand side represent the convection effects. The last term vanishes for a completely incompressible material; a condition enforced in the rigid-plastic flow of solids.

Main Index

CHAPTER 5 119 Structural Procedure Library

5

Nonlinear Boundary Conditions

Structur al Procedu re Library

There are three types of problems associated with nonlinear boundary conditions: contact, nonlinear support, and nonlinear loading. The contact problem might be solved through the use of special gap elements or the CONTACT option. Nonlinear support might involve nonlinear springs and/or foundations. Sometimes nonlinearities due to rigid links that become activated or deactivated during an analysis can be modeled through adaptive linear constraints. Nonlinear loading is present if the loading system is nonconservative, as is the case with follower forces or frictional slip effects. Discontinuities are inherent in the nature of many of these nonlinearities, making the solution by means of incremental linear approximations difficult. Some of the most severe nonlinearities in mechanics are introduced by nonlinear boundary conditions. It is, therefore, very important to be aware of potential problem areas and to have a good understanding of the underlying principles. This awareness and understanding enables you to validate numerical answers and to take alternative approaches if an initial attempt fails.

Arbitrary Eulerian-Lagrangian (AEL) Formulation In the AEL formulation referential system, the grid moves independently from the material, yet in a way that is spans the material at any time. Hence, a relationship between derivative with respect to the material and grid derivative is expressed as: · ( ) = ( * ) + c i ( ), i

(5-30) p i

m i

where c i is the relative velocity between the material particle, v and the mesh velocity, v ; for example, p

m

ci = vi – vi

(5-31)

The second or latter term represents the convective effect between the grid and the material. Note that for v

p i

m

= v i , a purely Eulerian formulation is obtained. The equation of momentum, for instance, can

be represented as: ∂σ i j p m ∂v i * ρv - = ---------- + b i i + ρ ( v j – v j ) ------∂x j ∂x j

(5-32)

Due to its strong resemblance to the pure Eulerian formulation, AEL is also called quasi-Eulerian formulation.

Nonlinear Boundary Conditions There are three types of problems associated with nonlinear boundary conditions: contact, nonlinear support, and nonlinear loading. The contact problem might be solved through the use of special gap elements of the CONTACT option. Nonlinear support might involve nonlinear springs and/or

Main Index

120 Marc Volume A: Theory and User Information

foundations. Sometimes nonlinearities due to rigid links that become activated or deactivated during an analysis can be modeled through adaptive linear constraints. Nonlinear loading is present if the loading system is nonconservative, as is the case with follower forces or frictional slip effects. Discontinuities are inherent in the nature of many of these nonlinearities, making the solution by means of incremental linear approximations difficult. Some of the most severe nonlinearities in mechanics are introduced by nonlinear boundary conditions. It is, therefore, very important to be aware of potential problem areas and to have a good understanding of the underlying principles. This awareness and understanding enables you to validate numerical answers and to take alternative approaches if an initial attempt fails. Contact Problems Contact problems are commonly encountered in physical systems. Some examples of contact problems are the interface between the metal workpiece and the die in metal forming processes, pipe whip in piping systems, and crash simulation in automobile designs. Contact problems are characterized by two important phenomena: gap opening and closing and friction. As shown in Figure 5-12, the gap describes the contact (gap closed) and separation (gap open) conditions of two objects (structures). Friction influences the interface relations of the objects after they are in contact. The gap condition is dependent on the movement (displacement) of the objects, and friction is dependent on the contact force as well as the coefficient of (Coulomb) friction at contact surfaces. The analysis involving gap and friction must be carried out incrementally. Iterations can also be required in each (load/time) increment to stabilize the gap-friction behavior.

A

B n

Figure 5-12 Normal Gap Between Potentially Contacting Bodies

Two options are available in Marc for the simulation of a contact problem. A detailed description of these options (gap-friction element and the CONTACT option) is given in Chapter 8 Contact of this manual. Nonlinear Support Marc provides two options for the modeling of support conditions: springs and elastic foundations. Both linear and nonlinear springs can be specified in the input. In a nonlinear problem, the spring stiffness and the equivalent spring stiffness of the elastic foundation can also be modified through a user subroutine. In the nonlinear spring option, the incremental force in the spring is ΔF = K ( Δu 2 – Δu 1 )

Main Index

(5-33)

CHAPTER 5 121 Structural Procedure Library

where K is the spring stiffness, Δu 2 is the displacement increment of the degree of freedom at the second end of the spring, and Δu 1 is the displacement increment of the degree of freedom at the first end of the spring. Use the SPRINGS model definition option for the input of linear and nonlinear spring data. The USPRNG user subroutine may also be used to specify the value of K based on the amount of previous deformation for nonlinear springs. In dynamic analysis, the SPRINGS option can also be used to define a dashpot. In thermal analysis or electrical analysis (heat transfer, Joule heating, heat transfer pass of a coupled analysis), the SPRINGS option can be used to define a thermal or electrical link. In the elastic nonlinear FOUNDATION option, the elements in Marc can be specified as being supported on a frictionless (nonlinear) foundation. The foundation supports the structure with an increment force per unit area given by ΔP n = K ( u n )Δu n

(5-34)

where K is the equivalent spring stiffness of the foundation (per unit surface area), and Δu n is the incremental displacement of the surface at a point in the same direction as ΔP n . To input nonlinear foundation data, use the FOUNDATION model definition option. To specify the value of K for the nonlinear equivalent spring stiffness based on the amount of previous deformation of the foundation, use the USPRNG user subroutine. Nonlinear Loading When the structure is deformed, the directions and the areas of the surface loads are changed. For most deformed structures, such changes are so small that the effect on the equilibrium equation can be ignored. But for some structures such as flexible shell structure with large pressure loads, the effects on the results can be quite significant so that the surface load effects have to be included in the finite element equations. Marc forms both pressure stiffness and pressure terms based on current deformed configuration with the FOLLOW FOR parameter. The FOLLOW FOR parameter should be used with the LARGE DISP or LARGE STRAIN parameters. The CENTROID parameter should not be included due to the use of the

residual load correction. Follower force point loads may be applied by either specifying this in the POINT LOAD option or by applying a transformation which rotates with the displacements of the nodes specified in the COORD SYSTEM option. A special case of nonlinear loading is the resultant pressure due to a gas in an enclosed cavity. In such problems, the pressure changes as the volume changes based upon the ideal gas law. This is discussed in Chapter 9, in the Cavity Pressure Loading section of this manual.

Main Index

122 Marc Volume A: Theory and User Information

Buckling Analysis Buckling analysis allows you to determine at what load the structure will collapse. You can detect the buckling of a structure when the structure’s stiffness matrix approaches a singular value. You can extract the eigenvalue in a linear analyses to obtain the linear buckling load. You can also perform eigenvalue analysis for buckling load in a nonlinear problem based on the incremental stiffness matrices. The buckling option estimates the maximum load that can be applied to a geometrically nonlinear structure before instability sets in. To activate the buckling option in the program, use the BUCKLE parameter. If a nonlinear buckling analysis is performed, also use the LARGE DISP parameter. Use the BUCKLE history definition option to input control tolerances for buckling load estimation (eigenvalue extraction by a power sweep or Lanczos method). You can estimate the buckling load after every load increment. The BUCKLE INCREMENT option can be used if a collapse load calculation is required at multiple increments. The linear buckling load analysis is correct when you take a very small load step in increment zero, or make sure the solution has converged before buckling load analysis (if multiple increments are taken). Linear buckling (after increment zero) can be done without using the LARGE DISP parameter, in which case the restriction on the load step size no longer applies. This value should be used with caution, as it is not conservative in predicting the actual collapse of structures. In a buckling problem that involves material nonlinearity (for example, plasticity), the nonlinear problem must be solved incrementally. During the analysis, a failure to converge in the iteration process or nonpositive definite stiffness signals the plastic collapse. For extremely nonlinear problems, the BUCKLE option cannot produce accurate results. In that case, the AUTO INCREMENT history definition option allows automatic load stepping in a quasi-static fashion for both geometric large displacement and material (elastic-plastic) nonlinear problems. The option can handle elastic-plastic snap-through phenomena. Therefore, the post-buckling behavior of structures can be analyzed. The buckling option solves the following eigenvalue problem by the inverse power sweep method: [ K + λΔK G ( Δu, u, Δσ ) ]φ = 0

(5-35)

where ΔK G is assumed to be a linear function of the load increment ΔP to cause buckling. The geometric stiffness ΔK G used for the buckling load calculation is based on the stress and displacement state change at the start of the last increment. However, the stress and strain states are not updated during the buckling analysis. The buckling load is therefore estimated by: P ( beginning ) + λΔP

(5-36)

where for increments greater than 1, P ( beginning ) is the load applied at the beginning of the increment prior to the buckling analyses, and λ is the value obtained by the power sweep or Lanczos method. The control tolerances for the inverse power sweep method are the maximum number of iterations in the power sweep and the 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. The

Main Index

CHAPTER 5 123 Structural Procedure Library

Lanczos method concludes when the normalized difference between all eigenvalues satisfies the tolerance. The maximum number of iterations and the tolerance are specified through the BUCKLE history definition option.

Perturbation Analysis The buckling mode can be used to perform a perturbation analysis of the structure. In the manual mode, a buckling increment is performed upon request and the coordinates are perturbed by a fraction of the buckling mode or eigenvector. You can enter an individual eigenvector number and the fraction or can request that a combination of modes be used. In the subsequent increments, the coordinates are: φ X = X + f ------ or X = X + φ

φi

∑ fi ------φi

(5-37)

The manual mode can be activated by using the BUCKLE INCREMENT model definition, or BUCKLE load incrementation option. In the automatic mode, the program checks for a nonpositive definite system during the solution phase. When this occurs, it automatically performs a buckle analysis during the next increment and updates the coordinates. The automatic mode can be activated by using the BUCKLE INCREMENT option. Also, be sure to force the solution of the nonpositive definite system through the CONTROL option or PRINT parameter. Material Nonlinearities In a large strain analysis, it is usually difficult to separate the kinematics from the material description. Table 5-5 lists the characteristics of some common materials. Table 5-5

Material Composites

Common Material Characteristics

Characteristics Anisotropic: 1) layered, ds i j = C i j k dε k 21 constants 2) Fiber reinforced, E t S = --- ( T CT – 1 ) 2 one-dimensional strain in fibers

Creep

Main Index

Examples

Marc Models

Bearings, aircraft panels

Composite continuum elements

Tires, glass/epoxy

Rebars

Strains increasing with time under Metals at high constant load. temperatures, polymide films, Stresses decreasing with time semiconductor under constant deformations. materials Creep strains are non-instantaneous.

ORNL Norton Maxwell

124 Marc Volume A: Theory and User Information

Table 5-5

Common Material Characteristics (continued)

Material

Characteristics

Examples

Marc Models

Elastic

Stress functions of instantaneous Small deformation strain only. Linear load(below yield) for most materials: metals, glass, displacement relation. Hookes Law wood

Elastoplasticity

Yield condition flow rule and hardening rule necessary to calculate stress, plastic strain. Permanent deformation upon unloading.

Metals Soils Snow Wood

von Mises Isotropic Cam -Clay Hill’s Anisotropic Generalized MohrCoulomb

Hyperelastic

Stress function of instantaneous Rubber strain. Nonlinear loaddisplacement relation. Unloading path same as loading.

Mooney Ogden Arruda-Boyce Gent NLELAST

Hypoelastic

Rate form of stress-strain law

Concrete

Buyukozturk

Viscoelastic

Time dependence of stresses in elastic material under loads. Full recovery after unloading.

Rubber, Glass, industrial plastics

Simo Model Narayanaswamy

Viscoplastic

Combined plasticity and creep phenomenon

Metals

Power law

Powder

Shima Model

Shape Memory

Superelastic and shape memory Biomedical stents, effect with phase transformations. Satellite antennae

Aurrichio, Thermomechanical

A complete description of the material types mentioned is given in Chapter 7 of this manual. However, some no characteristics and procedural considerations of some commonly encountered materials behavior are listed next. Inaccuracies in experimental data, misinterpretation of material model parameters and errors in userdefined material law are some common sources of error in the analysis from the materials viewpoint. It is useful to check the material behavior by running a single element test with prescribed displacement and load boundary conditions in uniaxial tension and shear. Large Strain Elasticity Structures composed of elastomers, such as tires and bushings, are typically subjected to large deformation and large strain. An elastomer is a polymer, such as rubber, which shows a nonlinear elastic stress-strain behavior. The large strain elasticity capability in Marc deals primarily with elastomeric materials. These materials are characterized by the form of their elastic strain energy function. For a more detailed description of elastomeric material, see Elastomer in Chapter 7 on this manual.

Main Index

CHAPTER 5 125 Structural Procedure Library

For the finite element analysis of elastomers, there are some special considerations which do not apply for linear elastic analysis. These considerations, discussed below, include: • • • •

Large Deformations Incompressible Behavior Instabilities Existence of Multiple Solutions

Large Deformations The formulation is complete for arbitrarily large displacements and strains. When extremely large deformations occur, the element mesh should be designed so that it can follow these deformations without complete degeneration of elements. For problems involving extreme distortions, rezoning must be done. Rezoning can be used with the formulation in the updated Lagrangian framework using conventional displacement based elements. Incompressible Behavior One of the most frequent causes of problems analyzing elastomers is the incompressible material behavior. Lagrangian multipliers (pressure variables) are used to apply the incompressibility constraint. The result is that the volume is kept constant in a generalized sense, over an element. Both the total, as well as updated Lagrange formulations, are implemented with appropriate constraint ratios for lower- and higher-order elements in 2-D and 3-D. For many practical analysis, the LBB (Ladyszhenskaya-Babuska-Brezzi) condition does not have to be satisfied in the strictest sense; for example, four node quadrilateral based on Herrmann principle. For elements that satisfy the LBB condition, error estimates of the following form can be established h

u –u

1

h

+ p –p

where k and

0

= O(h

m i n { k, + 1 }

)

(5-38)

are the orders of displacements and pressure interpolations, respectively. If

K = min { k, + 1 } , the rate of convergence is said to be optimal, and elements satisfying the LBB condition would not lock. The large strain elasticity formulation may also be used with conventional plane stress, membrane, and shell elements. Because of the plane stress conditions, the incompressibility constraint can be satisfied without the use of Lagrange multipliers. Instabilities Under some circumstances, materials can become unstable. This instability can be real or can be due to the mathematical formulation used in calculation. Instability can also result from the approximate satisfaction of incompressibility constraints. If the number of Lagrangian multipliers is insufficient, local volume changes can occur. Under some circumstances, these volume changes can be associated with a decrease in total energy. This type of instability usually occurs only if there is a large tensile hydrostatic stress. Similarly, overconstraints give rise to mesh locking and inordinate increase in total energy under large compressive stresses.

Main Index

126 Marc Volume A: Theory and User Information

Existence of Multiple Solutions It is possible that more than one stable solution exists (due to nonlinearity) for a given set of boundary conditions. An example of such multiple solutions is a hollow hemisphere with zero prescribed loads. Two equilibrium solutions exist: the undeformed stress-free state and the inverted self-equilibrating state. An example of these solutions is shown in Figure 5-13 and Figure 5-14. If the equilibrium solution remains stable, no problems should occur; however, if the equilibrium becomes unstable at some point in the analysis, problems can occur.

y

x Figure 5-13 Rubber Hemisphere

y

x Figure 5-14 Inverted Rubber Hemisphere

When incompressible material is being modeled, the basic linearized incremental procedure is used in conjunction with mixed variational principles similar in form to the Herrmann incompressible elastic formulation. These formulations are incorporated in plane strain, axisymmetric, generalized plane strain, and three-dimensional elements. These mixed elements may be used in combination with other elements in the library (suitable tying may be necessary) and with each other. Where different materials are joined, the pressure variable at the corner nodes must be uncoupled to allow for mean pressure discontinuity. Tying must be used to couple the displacements only.

Main Index

CHAPTER 5 127 Structural Procedure Library

Large Strain Plasticity In recent years there has been a tremendous growth in the analysis of metal forming problems by the finite element method. Although an Eulerian flow-type approach has been used for steady-state and transient problems, the updated Lagrangian procedure, pioneered by McMeeking and Rice, is most suitable for analysis of large strain plasticity problems. The main reasons for this are: (a) its ability to trace free boundaries, and (b) the flexibility of taking elasticity and history effects into account. Also, residual stresses can be accurately calculated. The large strain plasticity capability in Marc allows you to analyze problems of large-strain, elasticplastic material behavior. These problems can include manufacturing processes such as forging, upsetting, extension or deep drawing, and/or large deformation of structures that occur during plastic collapse. The analysis involves both material, geometric and boundary nonlinearities. In addition to the options required for plasticity analysis, the LARGE STRAIN parameter is needed for large strain plasticity analysis. In performing finite deformation elastic-plastic analysis, there are some special considerations which do not apply for linear elastic analysis include: • • • • •

Choice of Finite Element Types Nearly Incompressible Behavior Treatment of Boundary Conditions Severe Mesh Distortion Instabilities

Choice of Finite Element Types Accurate calculation of large strain plasticity problems depends on the selection of adequate finite element types. In addition to the usual criteria for selection, two aspects need to be given special consideration: the element types selected need to be insensitive to (strong) distortion; for plane strain, axisymmetric, and three-dimensional problems, the element mesh must be able to represent nondilatational (incompressible) deformation modes. Nearly Incompressible Behavior Most finite element types tend to lock during fully plastic (incompressible) material behavior. A remedy is to introduce a modified variational principle which effectively reduces the number of independent dilatational modes (constraints) in the mesh. This procedure is successful for plasticity problems in the conventional “small” strain formulation. Zienkiewicz pointed out the positive effect of reduced integration for this type of problem and demonstrates the similarity between modified variational procedures and reduced integration. The lower-order elements, invoking the constant volumetric strain or the lower-order elements, using reduced integration and hourglass control, behave well for nearly incompressible materials. Higher order elements in Marc are formulated to be used in large strain analysis including contact.

Main Index

128 Marc Volume A: Theory and User Information

Treatment of Boundary Conditions In many large strain plasticity problems, specifically in the analysis of manufacturing processes, the material slides with or without friction over curved surfaces. This results in a severely nonlinear boundary condition. The Marc gap-friction element and CONTACT option can model such sliding boundary conditions. Severe Mesh Distortion Because the mesh is attached to the deforming material, severe distortion of the element mesh often occurs, which leads to a degeneration of the results in many problems. The ERROR ESTIMATE option can be used to monitor this distortion. To avoid this degeneration, generate a new finite element mesh for the problem and then transfer the current deformation state to the new finite element mesh. The global adaptive and rezoning procedure in the program is specifically designed for this purpose. Instabilities Elastic-plastic structures are often unstable due to necking phenomena. Consider a rod of a rigid-plastic · incompressible workhardening material. With ε the current true uniaxial strain rate and h the current workhardening, the rate of true uniaxial stress σ is equal to · · σ = Hε

(5-39)

The applied force is equal to F = σA , where A is the current area of the rod. The rate of the force is therefore equal to · F· = σ A + σA·

(5-40)

On the other hand, conservation of volume requires that · Aε + A· = 0

(5-41)

Hence, the force rate can be calculated as · F· = ( H – σ )Aε

(5-42)

Instability clearly occurs if σ > H . For applied loads (as opposed to applied boundary conditions), the stiffness matrix becomes singular (nonpositive definite). For the large strain plasticity option, the workhardening slope for plasticity is the rate of true stress versus the true plastic strain rate. The workhardening curve must, therefore, be entered as the true stress versus the logarithmic plastic strain in a uniaxial tension test.

Computational Procedures for Elastic-Plastic Analysis Three basic procedures for plasticity exist in Marc. In this section, the variational form of equilibrium equations and constitutive relations, and incompressibility are summarized. Issues regarding return mapping procedures for stress calculation in three-dimensional and plane-stress conditions are also discussed.

Main Index

CHAPTER 5 129 Structural Procedure Library

For notational purpose, three configurations are considered at any point, original ( t = 0 ), previous ( t = n ) and current ( t = n + 1 ). An iterative procedure, full or modified Newton-Raphson, secant, or arc-length is used to solve for the equilibrium at t = n + 1 . 1. Small Strain Plasticity (reference configuration: t = 0 ): In this approach, the basis of variational formulation are 2nd Piola-Kirchhoff stress, S and Green-Lagrange strain, E . Equilibrium of the current state can thus be represented by the following virtual work principle:

∫ V

S : δE dV =

∫ A

n

t : δη dA +

n

∫ V

b : δη dV

(5-43)

n

During the increment, all state variables are defined with respect to the state at t = n and are updated at the end of increment upon convergence. The linearized form of constitutive equations is given as: dS = L

ep

: dE – σ.dE – dE.σ

(5-44) ep

in which S is the second Piola-Kirchhoff stress, σ is the Cauchy stress, and L is the elastoplastic moduli. This linearization has the advantage that it is fully independent of the rotation increment, but the disadvantage is that the linearization causes errors equal to the square of the strain increment. Moreover, imposing the incompressibility condition in terms of the trace of Green-Lagrange strains leads to errors in the form of fictitious volume changes in fully developed plastic flow. The above procedure works well in the context of small strain plasticity. However, in many large deformation problems including metal forming processes, the plastic strain increments can be very large and the above procedure can lead to large errors in the results. The two finite strain plasticity formulations to model the large inelastic strains are: rate based (hypoelastic) and total (hyperelastic). 2. Finite Strain Plasticity with additive decomposition of strain rates (reference configuration: t = n + 1 ). This formulation is based on the integration of the constitutive equations in the current configuration. To maintain objectivity, the notion of rotation neutralized stress and strain measures is introduced. All objective stress rates, are manifestation of Lie derivative: · –1 –T T L v ( Σ ) = Φ ( Φ ΣΦ ) Φ

(5-45)

where Φ is a deformation measure; for example, deformation gradient or rotation tensor, R while Σ is a stress measure in the current configuration. The general form for an objective stress rate is:

Main Index

130 Marc Volume A: Theory and User Information

∇ T · σ = σ – σΩ – Ωσ + ασtr ( d )

(5-46)

From Table 5-6, it can be seen that there is a possibility of a number of stress rates. It can be observed that while all the above stress rates are objective, the Truesdell and Durban-Baruch rates would not yield symmetric matrices. Table 5-6

Objective Stress Rates

Ω

α

Truesdell

L

1

Cotter-Rivlin

L

0

Oldroyd

-LT

0

Jaumann-Zaremba-Noll

W

0

Green-McInnis-Nagdhi

· –1 RR

0

1 --- ( D + W ) 2

1

Stress Rates

Durban Baruch

Marc’s implementation of rate formulation involves the use of Jaumann rate of Cauchy stress which is obtained as an average of the Oldroyd and Cotter-Rivlin stress rates. Thus, the Jaumann rate can be written as: · ∇ σ = σ – Wσ + σW

(5-47)

T · ∇ = σ + Ω ⋅ σ + σ ⋅ Ω + tr ( dε )σ σ

(5-48)

∇

where ( · ) is the ordinary rate and ( ) is the objective rate with W is the spin or the antisymmetric part of the velocity gradient, L . The last term is neglected because of the incompressible nature of plasticity. The equilibrium in the current state is given by the virtual work principle at t = n + 1 :

∫ V n+1

σ : δε dv =

∫ A n+1

t . δηda +

∫

b . δη dv

V n+1

Linearization of the above form leads to the variational statement:

Main Index

(5-49)

CHAPTER 5 131 Structural Procedure Library

T

∫ V

[ dσ : δε – 2 ( dε ⋅ σ ) : δε + tr ( dε )σ : δε + σ : { ( ∇ u ) ⋅ ( ∇ η ) } ] dv =

n+1

⎛ d ⎜ ∫ b . δη dv + ⎝V n+1

∫ A

⎞ t . δη da⎟ – ⎠

n+1

(5-50)

∫ V

σ : δε dv

n+1

where, dσ = R ⋅ dσ

RN

⋅R

T

(5-51)

Within the context of rotation neutralized form of constitutive relations, dσ dσ

RN

= L

where, dε ε

RN

RN

RN

: dε

RN

is defined as:

RN

(5-52)

T

= R ⋅ dε ⋅ R . Also, the rotation neutralized strain can be calculated by:

= (U + I)

–T

( F + I )ε

MID

(F + I)(U + I )

–1

MID

with ε being the mid-increment strain, a good approximation for incremental logarithmic strain measure. Where e = U – I is the engineering strain and U is the stretch tensor obtained by the polar decomposition of F . Admitting an error of the order of e 2 in the approximation of the logarithmic strain, one obtains: dσ = L where L

ep

ep

: dε = R ⋅ (R ⋅ L

(5-53) RN

T

⋅R )⋅R

T

(5-54)

During computations, the third term of Equation (5-50), tr ( dε ) ⋅ σ : δε , is neglected due to its nonsymmetric nature. In a fully developed plastic flow, the volumetric part of the energy can become extremely large and lead to volumetric locking. Hence, a special treatment of incompressibility is done to relax the volumetric constraint in an assumed strain format. The volumetric part of deformation gradient is modified such that, the assumed deformation gradient is: 1 --3

F = J J

1 – --3

F

(5-55)

Linearization of F in the original state relates it to the displacement gradients in the current state as: DF = ∇ ( Δu ) F

Main Index

(5-56)

132 Marc Volume A: Theory and User Information

where 1 1 ∇ ( Δu ) = ( Δu ) i, j – --- div ( Δu ) δ i j + --- div ( Δu ) δ i j 3 3

(5-57)

where the first two terms are evaluated at each integration point and the last term is averaged over the element. For a lower order element, the procedure leads to mean or constant dilatation approach. Considering Equations (5-50) to (5-57) the resulting system can be expressed as: s

∫ V

[∇ η : L

ep

s

s

s

T

: ∇ ( Δu ) – 2∇ η ⋅ σ : ∇ ( Δu ) + σ : ∇ ( Δu ) ⋅ ( ∇η ) ] dv =

n+1

⎛ d ⎜ ∫ b . δη dv + ⎝V n+1

∫ A

n+1

⎞ t . δη da⎟ – ⎠

∫ V

s

T

[ ∇ η ] : σ dv

(5-58)

n+1

In the event, the elastic strains become large in an elastic-plastic analysis the rate based constitutive equations do not accurately model the material response. This results from the fact that the elasticity matrix are assumed to have constant coefficients in the current deformed configuration. In the next formulation, the rate of deformation tensor is decomposed multiplicatively into the elastic and plastic parts to resolve these problems. 3. Finite strain plasticity with multiplicative decomposition of deformation gradient. An alternative formulation, based on the multiplicative decomposition of the deformation gradient has been implemented in Marc, namely: e θ p

(5-59)

F = F F F e

θ

p

where F , F , and F are (elastic, thermal, and plastic) deformation gradients, respectively. The thermo-mechanical coupling is implemented using the staggered approach. The above decomposition has a physical basis to it as the stresses are derived from quadratic logarithmic strain energy density function: 1 e 2 e 2 1 W = --- λ ( ln J ) + μ tr ⎛ --- ln b ⎞ ⎝2 ⎠ 2

(5-60)

This function has been chosen due to the availability of the material coefficients from material testing in a small strain case. In the metal forming applications, the elastic strains are negligible and the rate-based (or hypoelastic) as well as the total (or hyperelastic) form of constitutive equations give virtually the same results. However, many polymers, metals subjected to large hydrostatic pressures, high velocity impact loading of metals and processes, where shape changes after deformation need to be evaluated precisely, the hyperelastic formulation yields physically more meaningful results.

Main Index

CHAPTER 5 133 Structural Procedure Library

The return mapping procedure for the calculation of stresses is based on the radial return procedure. With the use of exponential mapping algorithm, the incompressibility condition is imposed exactly: det F

p

(5-61)

= 1

The strain energy is separated into deviatoric and volumetric parts in the framework of mixed formulation. The general form of three-field variational principle is:

∫

π ( u, p , J ) =

V

where, b = J

e

e

e

[W ( b ) + U ( J ) + p ( J – J )] dV

(5-62)

0

2 – --3

(5-63) b

e

W ( b ) and U ( J ) are the deviatoric and elastic volumetric parts of the free energy, p is the e

e

pressure, J and J are elastic pointwise and average elastic Jacobian of the element, respectively. The volumetric free energy can be of any form in Equation (5-61). However, if the incompressibility is enforced in a pointwise fashion and the volumetric free energy is assumed to be of the form: 1 --e 3

2

e 9 U ( J ) = --- K ( J ) – 1 2

(5-64)

the perturbed Lagrangian form of the variational principle can be cast in a two-field framework as:

π ( u, P ) =

∫ V0

1 ⎧ ⎫ --⎪ e 3 ⎪ P2 W ( b ) + 3P ⎨ ( J ) – 1 ⎬ – ------- dV ⎪ ⎪ 2K ⎩ ⎭ 2 --e 3

(5-65)

Note that P = p ( J ) , hence, P is not the true pressure in Equation (5-65). Choice of the volumetric free energy in Equation (5-64) is not arbitrary and is described in more detail in Chapter 7 in the Elastomer section of this manual.

Main Index

134 Marc Volume A: Theory and User Information

Linearization of the equilibrium condition arising from the stationary of the variational principle Equation (5-65), yields:

∫ V

n+1

1 ⎧ ⎛ --⎞⎫ ⎪1⎜ ⎪ e 3⎛1 s ⎞ ∇ η : ⎨ --- C d e v + P ( J ) --- 1 ⊗ 1 – 2I ⎟ ⎬ : ∇ u + ⎜ ⎝3 ⎠⎟ J ⎪ ⎝ ⎠⎪ ⎩ ⎭ s

1 ---

(5-66)

dP e 3 σ : { ( ∇ ( Δu ) ). ( ∇η ) } + ------ ( J ) 1 : ∇η dv = J T

⎛ d ⎜ ∫ b . δη dv + ⎝V n+1

∫ A n+1

⎞ t . δη da⎟ – ⎠

∫ V

s

T

( ∇ η ) : σ dv

n+1

The linearization of the constraint equation defines the term dP in Equation (5-66). The derivation of the spatial tangent C d e v follows by a push forward of the material tangent into the current configuration: –1 d e v

Hence, S = F τ

F

–T

(5-67)

where S is the pull back of the deviatoric Kirchhoff stress tensor. Assuming the entire incremental deformation to be elastic, a symmetric stress tensor, Sˆ can be defined with respect p

to a fixed plastic intermediate configuration F n as: –1

tr tr dev Sˆ = ( F e ) τ ( Fe )

–T

(5-68)

also noting that, 3

Sˆ =

∑ A =

βA S A N A ⊗ N A where Sˆ A = ----------------tr 2 ( λA e ) 1

3

dSˆ =

∑

3

dSˆ A N A ⊗ N A +

A = 1

1 where dSˆ A = ----------------------------------tr 2 tr 2 ( λA e ) ( λB e ) and dN A = Ω A B N B

Main Index

(5-69)

3

∑ ∑

( Sˆ B – Sˆ A ) Ω B A N A ⊗ N B

(5-70)

A = 1B ≠ A

⎛ ∂β A ⎞ tr tr - – 2β A δ A B⎟ λ B e dλ B e ⎜ ----------tr ⎝ ∂ε B e ⎠

(5-71)

(5-72)

CHAPTER 5 135 Structural Procedure Library

3 T

tr tr tr similarly, Cˆ = ( F e ) F e with F e =

∑

tr

λA e nA ⊗ NA

(5-73)

A = 1 3 tr

∑

dCˆ =

tr

2λ B e dλ B e N B ⊗ N B +

B = 1

(5-74) 3

3

∑

∑

A = 1 B≠A

⎧ tr 2 tr 2 ⎫ ⎨ ( λB e ) – ( λB e ) ⎬ ΩB A NA ⊗ NB ⎩ ⎭

The algorithmic elasto-plastic tangent can be obtained as: T T ∂S T T ∂Sˆ C d e v = 2F ⎛ F ------- F ⎞ F = 2 ( F etr ) ( F etr ) ------- ( F etr ) ( F etr ) ⎝ ∂C ⎠ ˆ ∂C

(5-75)

Combining Equations (5-70), (5-75), and (5-76), the spatial form of deviatoric part of the tangent as: 3

⎛ ∂β A ⎞ - – 2β A δ A B⎟ n A ⊗ n A ⊗ n B ⊗ n B ⎜ ----------tr ⎠ 1 B ≠ A ⎝ ∂ε B e 3

∑ ∑

C dev =

A =

+

3

3

∑ ∑

A = 1B ≠ A

tr

2

tr

2

( λA e ) βB – ( λB e ) βA ------------------------------------------------------- ( nA ⊗ nB ⊗ nA ⊗ nB + tr 2 tr 2 ( λB e ) – ( λA e )

(5-76)

nA ⊗ nB ⊗ nB ⊗ nA ) The singularity for two- or three-equal stretch ratios is removed by repeated application of L’Hospital’s rule. Due to separate interpolation of the pressure, a larger system of equations needs to be solved. A static condensation of the element variables is carried out before going in the solver. This step renders the singularity of the system to be inversely proportional to the bulk modulus of the material. Due to the multiplicative split of the deformation gradient and an additive split of the free energy into deviatoric and volumetric parts, this framework is eminently suitable for implementation of general nonlinear elastic as well as inelastic material models. Besides, compressible and nearly incompressible material response can be naturally handled. Finally, the stress calculation is done via return mapping to the yield surface. There are several methods to return the stress. Among them, the popular ones include: Closest point projection (which reduces to radial return for von Mises), mean normal approach, midpoint rule, trapezoidal rule, tangent cutting plane algorithm, and multistage method.

Main Index

136 Marc Volume A: Theory and User Information

Krieg and Krieg (1977) investigated the radial return algorithm which has been proposed by Wilkins (1964). The third algorithm analyzed was the so-called secant stiffness method proposed by Rice and Tracy (1973) which represented a special case of the generalized Trapezoidal rule for nonhardening materials algorithm in contrast to the fully implicit radial return algorithm and the fully explicit tangent stiffness approach. The radial return method (shown in Figure 5-15) was found to be the most accurate among the three analyzed, particularly when large strain increments were used. The radial return and mean normal method are available in Marc and are described next. ′

σ1

Δσ

el

σ fin al σ*

′

′

σ2

σ3

Figure 5-15

Radial Return Method

1. Closest Point Projection procedure: The closest point projection or the backward Euler algorithm reduces to a radial return scheme for cases where there is no anisotropy or plane stress condition. The trial stress is determined as: d

d

σ r r = σ + 2GΔε d

(5-77)

The final stress state is obtained by simply scaling the trial stress by a scale factor, β 2GΔλ where, β = 1 – --------------d σr r

(5-78)

the plastic consistency parameter Δλ , is obtained by solving for consistency condition iteratively. An explicit form of the material tangent for the isotropic, von Mises yield surface can be given as: L

ep

1 ˆ ⊗N ˆ = 2G β ⎛ I – --- 1 ⊗ 1⎞ – 2G γ N ⎝ ⎠ 3

1 where, γ = ------------------ – 1 + β H 1 + ------3G

Main Index

(5-79)

(5-80)

CHAPTER 5 137 Structural Procedure Library

ˆ is the return direction normal to the current yield surface. For the plane stress case, the Here N zero normal stress condition is explicitly imposed in the yield condition. Since the yield surface is not a circle in the plane, the return direction is not radial anymore. 2. Mean-Normal method: Assuming the entire deformation to be elastic in nature, the trial stress is evaluated as: d

d

d

σ m n = σ + 2αGΔε + ( 1 – α )GΔε

d

(5-81)

Due to the use of pressure independent yield function, only the deviatoric stresses are evaluated. As shown in Figure 5-16, ( 1 – α ) represents the fraction of strain increment for which the plastic flow occurs. Δσ e l σ* + σ o + Δσ e l

d

σ1

σ f i n al σ* σo d

σ2

d

σ3

Figure 5-16

Mean-Normal Method

d

σ includes the deviatoric stresses at the previous increment scaled such that it satisfies the yield condition. The yield criterion might not be exactly satisfied due to temperature effects, numerical integration of elastic-plastic relationships, or accumulated numerical inaccuracy. F ( σ ) = 0 indicates that the stress state is exactly on the yield surface. If F ( σ ) > 0 , scale σ by a factor λ such that: F ( λσ ) = 0

0<λ<1

(5-82)

The equivalent plastic strain, plastic strain tensor and the elasto-plastic moduli are obtained as:

Main Index

Δε

p

Δε

p

e ˆ ) : Δεˆ ( 1 – α ) (C : N = ----------------------------------------------------ˆ +H ˆ : Ce : N N p

ˆ = Δε N

(5-83) (5-84)

138 Marc Volume A: Theory and User Information

L

ep

e ˆ ) ⊗ ( Ce : N ˆ) (C : N e = C – ( 1 – α ) --------------------------------------------------e ˆ +H ˆ :C :N N

(5-85)

e

ˆ is the mean-normal direction to the yield surface, H is the hardening modulus and C where, N is the elastic tangent moduli. For nonhardening materials, the mean normal algorithm is a special case of trapezoidal rule. Marc plasticity algorithms are unconditionally stable and accurate for moderate strain increments. However, overall global stability of the system can be dictated by other considerations like contact, buckling which then guide the selection of appropriate load increment size. It should also be recognized that the algorithmically consistent tangent in the closest point projection algorithm is based on the current state, and a lack of embedded directionality (unlike secant methods) in the tangent can lead to divergent solutions unless line search or automatic time stepping algorithms are used. However, when it converges it shows quadratic convergence as compared to linear convergence for the mean-normal scheme. 3. Multistage Return Mapping: The return mapping scheme described in this section is used for isotropic and anisotropic plasticity when LARGE STRAIN is used to describe the Updated Lagrange Procedure. Marc uses this scheme for the Hill and Barlat yield criteria. This scheme is not available for pressure dependent yield criteria like Mohr Coulomb. In a large strain analysis, Marc automatically chooses the return mapping scheme that is most suited for the given material. The increment of Cauchy stress for elasto-plasticity becomes e

Δσˆ = Cˆ : Δεˆ

e

p

e

= Cˆ : ( Δεˆ – Δεˆ ) .

(5-86)

In Equation (5-86), superscript ‘ ˆ ’ means a materially embedded co-rotational coordinate system. For the numerical implementation of Equation (5-86), the general midpoint rule can be expressed as follows: e

ˆn+α σˆ n + 1 = σˆ nT + 1 – λCˆ N

(5-87)

ˆ e Δεˆ where σˆ nT + 1 = σˆ n + C (Case 1) if F ( σˆ nT + 1 ) ≤ 0 , λ = 0 , σˆ n + 1 = σˆ nT + 1 (Case 2) if F ( σˆ nT + 1 ) ≤ 0 , λ = λ such that F ( σˆ nT + 1 ) = 0 where superscript T stands for a trial state. For Case 2, the condition stating that the updated stress p

stays on the strain-hardening curve ( σ = ρ ( ε ) ) provides the following condition: e

ˆ n + α ) – ρ ( ε np + λ ) = 0 . F ( λ ) = σ ( σˆ nT + 1 – λCˆ N Equation (5-88) is a nonlinear equation to solve for λ .

Main Index

(5-88)

CHAPTER 5 139 Structural Procedure Library

5+

If the strain increment is not small enough, it is difficult to obtain the numerical solution of Equation (5-88) even though it has a mathematical solution. Therefore, an iterative scheme, which utilizes the control of the potential residual, is introduced. The method is applicable to a nonquadratic yield function and a general hardening law. For the implementation of the algorithm, Equation (5-88) has been modified to the following relationship with α = 1 ; that is,

Structura l Procedur e Library

ˆ eN ˆ ( k ) ) – ρ ( ε np + λ ( k ) ) = F ( k ) F ( λ ( k ) ) = σ ( σˆ T – λ ( k ) C

(5-89)

where F ( λ( 0 ) = 0 ) = F( 0 ) , { F( k ) F( 0 ) > F( 1 ) > F( k ) > … > F( N ) ( F( N ) = 0 ) , k = 0 ∼ N } , ΔF = ( F k – 1 – F k ) < σ Y ( = ( σ ( ε p = 0 ) ) ) and F k

= 1∼N–1

are prescribed values.

ˆ ( 1 ) is guessed As shown in Equation (5-89) and Figure 5-17, the direction of the first substep N ˆ ( 0 ) , which is normal to the yield surface at the trial stress σˆ T . Then, the exact from the direction N ˆ ( 1 ) can be obtained from the first substep nonlinear solution based on Euler backward direction N ˆ ( i + 1 ) is guessed from the method. In general, the new direction for the second substep N ˆ ( i ) based on the previous substep stress σˆ ( i ) . This procedure is completed when direction N F = F ( N ) ( = 0 ) . In fact, the equation for the Nth step is equivalent to Equation (5-89) and σˆ n + 1 = σˆ ( N ) . Finally, the proportional logarithmic plastic strain remains normal to the yield surface at the final stress σˆ n + 1 ; that is, ∂σ ˆ (N)) . Δεˆ p = Δε p ------- ( σˆ n + 1 ) ( = λ ( N ) N ∂σˆ

(5-90)

T

σ ( σˆ ) σ ( σˆ ( 1 ) )

ˆ (1) N

σ ( σˆ ( 2 ) )

ˆ (2) N ˆ (N) N

σ ( σˆ ( n + 1 ) )

p Δεˆ ( N )

σ ( σˆ ( n ) ) Δσˆ σˆ n + 1 σˆ n Figure 5-17

Main Index

σˆ T

p Δεˆ

p (2) Δεˆ ( 2 )

Schematic View for Multistage Return Mapping Method

140 Marc Volume A: Theory and User Information

Therefore, the normality condition of the incremental deformation theory is satisfied at the current state ( n + 1 ) for α = 1 . In order to solve Equation (5-89), the Euler Backward method is employed to solve the iteration procedure for the kth substep. At each iteration, Δλ (i)

Δλ

(i)

(i)

(i) (k)

(i)

(at ( k ) substep and ( i ) iteration) becomes (i)

ˆ E – 1 g2 ⎛ λ ⎞ + g3 ⎛ λ ⎞ H g1 ⎛ λ ⎞ – N ⎝ ( k )⎠ ⎝ ( k )⎠ ⎝ ( k )⎠ (k) (k) = -------------------------------------------------------------------------------------------------------------------(i) (i) (i) ˆ ˆ E – 1N +H N

(i) (k)

(k)

(k)

(5-91)

( k)

where E

(i)

–1

(k)

=

Cˆ e – 1 + λ

(i)

ˆ ∂N -------

–1

,

( k ) ∂σ ˆ

(i) (i) g 1 ⎛ λ ⎞ = σ ( σˆ ) – ρ ⎛ ε np + λ ⎞ – F ( k ) , ⎝ ⎝ ( k )⎠ ( k )⎠ (i) (i) ˆ , g 2 ⎛ λ ⎞ = Cˆ e – 1 ( σˆ – σˆ T ) + λ N ⎝ ( k )⎠ (k) (i)

(i)

g3 ⎛ λ ⎞ = H ( ρ – ρn ) – λ , ⎝ ( k )⎠ (k) –1

and H is the hardening modulus in stress-strain curve. The detailed derivations of Equation (5-91) are shown in the work of Yoon at al. [Ref. 32]. In order to solve the equilibrium equation iteratively, the elasto-plastic tangent modulus consistent with the current return mapping method is obtained as follows: dσˆ j = dσˆ n + 1 = L e p dεˆ n + 1 where

Lep

ˆ n + α ⊗ CN ˆ n + α⎞ ⎛ CN = ⎜ C – -------------------------------------------------⎟ and C = ˆ n + α + h′⎠ ˆ n + α CN N ⎝

(5-92) ˆn+α ∂N Cˆ e – 1 + λ ------------------∂σˆ n + 1

–1

.

In Equation (5-92), h′ is instantaneous slope and α = 1 is used. CREEP Creep is a time-dependent inelastic behavior that can occur at any stress level, either below or above the yield stress of a material. Creep is an important factor at elevated temperatures. In many cases, creep is also accompanied by plasticity, which occurs above the yield stress of the material.

Main Index

CHAPTER 5 141 Structural Procedure Library

Marc offers two schemes for modeling creep in conjunction with plasticity: a. treating creep strains and plastic strains separately using an explicit procedure (where the creep is treated explicitly) or an implicit procedure (where both creep and plasticity are treated implicitly). These procedures are available with standard options via data input or with userspecified options via user subroutines. More details are provided below. b. modeling creep strains and plastic strains in a unified fashion (viscoplasticity). Both explicit and implicit procedures are again available for modeling unified viscoplasticity. More details are provided in the section titled Viscoplasticity in this chapter. The options offered by Marc for modeling creep are as follows: • Creep data can be entered directly through data input or user subroutine. For explicit creep, the CRPLAW user subroutine is to be used, and for implicit creep, the UCRPLW user subroutine is to be used. • An automatic time stepping scheme can be used to maximize the time step size in the analysis. • Eigenvalues can be extracted for the estimation of creep buckling time. In addition, for explicit creep, the following additional options can be used: • Creep behavior can be either isotropic or anisotropic. • The Oak Ridge National Laboratory (ORNL) rules on creep can be activated. The creep analysis option is activated in Marc through the CREEP parameter. The creep time period and control tolerance information are input through the AUTO CREEP history definition option. This option can be used repeatedly to define a new creep time period and new tolerances. These tolerances are defined in the section on Creep Control Tolerances. Alternatively, a fixed time step can be specified through the CREEP INCREMENT history definition option. In this case, no additional tolerances are checked for controlling the time step. Creep analysis is often carried out in several runs using the RESTART option. Save restart files for continued analysis. The REAUTO option allows you to reset the parameters defined in the AUTO CREEP option upon restart. Adaptive Time Control The AUTO CREEP option takes advantage of the diffusive characteristics of most creep solutions. Specifically, this option controls the transient creep analysis. You specify a period of creep time and a suggested time increment. The program automatically selects the largest possible time increment that is consistent with the tolerance set on stress and strain increments (see Creep Control Tolerances in this chapter). The algorithm is: for a given time step Δt , a solution is obtained. Marc then finds the largest values of stress change per stress, Δσ ⁄ σ , and creep strain change per elastic strain, Δε

cr

el

⁄ ε . It compares

these values to the tolerance values, T s (stress change tolerance) and T e (strain change tolerance), for this period.

Main Index

142 Marc Volume A: Theory and User Information

The value p is calculated as the larger of ( Δσ ⁄ σ ) ⁄ T σ or ( Δε

cr

(5-93)

⁄ εe l ) ⁄ Tε

If p > 1 , the program resets the time step as Δt n e w = 0.8 Δt o l d ⁄ p

(5-94)

The time increment is repeated until convergence is obtained or the maximum recycles control is exceeded. In the latter case, the run is ended. If the first repeat does not satisfy tolerances, the possible causes are: • excessive residual load correction • strong additional nonlinearities such as creep buckling-creep collapse • incorrect coding in the CRPLAW, VSWELL, or UVSCPL user subroutine. Appropriate action should be taken before the solution is restarted. If p < 1 , the solution is stepped forward to t + Δt and the next step is begun. The time step used in the next increment is chosen as Δt n e w = Δt o l d

if

0.8 < p < 1

(5-95)

Δt n e w = 1.25 Δt o l d

if

0.65 < p< 0.8

(5-96)

Δt n e w = 1.5 Δt o l d

if

p < 0.65

(5-97)

Since the time increment is adjusted to satisfy the tolerances, it is impossible to predetermine the total number of time increments for a given total creep time. Creep Control Tolerances Marc performs a creep analysis under constant load or displacement conditions on the basis of a set of tolerances and controls you provide.These are as follows: 1. Stress change tolerance – This tolerance controls the allowable stress change per time step during the creep solution, as a fraction of the total stress at a point. Stress change tolerance governs the accuracy of the transient creep response. If you need accurate tracking of the transient response, specify a tight tolerance of 1 percent or 2 percent stress change per time step. If you need only the steady-state solution, supply a relatively loose tolerance of 10-20 percent. It is also possible to check the absolute rather than the relative stress.

Main Index

CHAPTER 5 143 Structural Procedure Library

2. Creep strain increment per elastic strain – Marc uses either explicit or implicit integration of the creep rate equation. When the explicit procedure is used, the creep strain increment per elastic strain is used to control stability. In almost all cases, the default of 50 percent represents the stability limit, so that you need not provide any entry for this value. It is also possible to check the absolute rather than the relative strain. 3. Maximum number of recycles for satisfaction of tolerances – During AUTO CREEP, Marc chooses its own time step. In some cases, the program recycles to choose a time step that satisfies tolerances, but recycling rarely occurs more than once per step. Excessive recycling can be caused by physical problems such as creep buckling, poor coding of the CRPLAW, VSWELL, or UVSCPL user subroutine or excessive residual load correction that can occur when the creep solution begins from a state that is not in equilibrium. The maximum number of recycles allows you to avoid wasting machine time under such circumstances. If there is no satisfaction of tolerances after the attempts at stepping forward, the program stops. The default of five recycles is conservative in most cases. 4. Low stress cut-off – Low stress cut-off avoids excessive iteration and small time steps caused by tolerance checks that are based on small (round off) stress states. A simple example is a beam in pure bending. The stress on the neutral axis is a very small roundoff-number, so that automatic time stepping scheme should not base time step choices on tolerance satisfaction at such points. The default of five percent of the maximum stress in the structure is satisfactory for most cases. 5. Choice of element for tolerance checking – Creep tolerance checking occurs as a default for all integration points in all elements. You might wish to check tolerances in only 1 element or in up to 14 elements of your choice. Usually, the most highly stressed element is chosen. When you enter the tolerances and controls, the following conventions apply: • All stress and strain measures in tolerance checks are second invariants of the deviatoric state (that is, equivalent von Mises uniaxial values). • You can reset all tolerances and controls upon the completion of one AUTO CREEP sequence. Background Information Creep behavior is based on a von Mises creep potential with isotropic behavior described by the equivalent creep law: · cr ε = f ( σ, ε c r, T, t )

(5-98)

The material behavior is therefore described by: · c r ∂σ Δε c r = ε --------∂σ d

(5-99)

∂σ where --------- is the outward normal to the current von Mises stress surface and ε· c r is the equivalent creep ∂σ d strain rate.

Main Index

144 Marc Volume A: Theory and User Information

There are two numerical procedures used in implementing creep behavior. The default is an explicit procedure in which the above relationship is implemented in the program by an initial strain technique. In other words, a pseudo-load vector due to the creep strain increment is added to the right-hand side of the stiffness equation. KΔu = ΔP +

∫ β T DΔε c r dv

(5-100)

V

where K is the stiffness matrix, and Δu and ΔP are incremental displacement and incremental nodal force vectors, respectively. The integral

∫ β T DΔε c r dv

(5-101)

V

is the pseudo-load vector due to the creep strain increment in which β is the strain displacement relation and D is the stress-strain relation. When plasticity is also specified through a suitably defined yield criterion and yield stress in Marc, the plasticity is treated implicitly while the creep is treated explicitly. As an alternative, an implicit creep procedure can be requested with the CREEP parameter. In this case, the inelastic strain rate has an influence on the stiffness matrix. Using this technique, significantly larger steps in strain space can be used. In Marc, this option is only to be used for isotropic materials with the creep strain rate defined by · cr n cr ε = Aσ f ( ε )g ( T )h ( t ) where A is the creep constant that can be defined through input data or through the UCRPLW user subroutine; power law expression is always to be used for the effective stress with the coefficient provided through the input data or the UCRPLW user subroutine; and power law coefficients or more general expressions can be provided for the creep strain, temperature, and time through the input data or the UCRPLW user subroutine, respectively. When plasticity is also specified through a suitably defined yield stress in conjunction with the von Mises yield criterion, a sub-iterative scheme within each Newton-Raphson cycle is used to determine the plastic strains needed to keep the stress state on the yield surface and the creep strains that develop due to the equivalent stress being greater than a user-defined back stress. The yield stress for the plastic component can be varied as a function of the equivalent plastic strain, temperature and spatial coordinates. Similarly, the back stress for the creep component can be varied as a function of the equivalent creep strain, temperature and spatial coordinates. Creep Buckling Marc also predicts the creep time to buckling due to stress redistribution under given load or repeated cyclic load. The buckling option solves the following equation for the eigenvalue ( K + λK G )Φ = 0

Main Index

(5-102)

CHAPTER 5 145 Structural Procedure Library

The geometric stiffness matrix, K G , is a function of the increments of stress and displacement. These increments are calculated during the last creep time step increment. To determine the creep time to buckle, perform a buckle step after a converged creep increment. Note that the incremental time must be scaled by the calculated eigenvalue, and added to the total (current) time to get an estimate as to when buckling occurs.

AUTO THERM CREEP (Automatic Thermally Loaded Elastic-Creep/Elastic-Plastic-Creep Stress Analysis) The AUTO THERM CREEP option is intended to allow automatic, thermally loaded elastic-creep/elasticplastic-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 the program through the CHANGE STATE option, using input option 3 (post file), and the program creates its own set of temperature steps (increments) based on a temperature change tolerance provided in this option. The times at all temperature steps are calculated by the program for creep analyses. At each temperature step (increment), an elastic/elastic-plastic analysis is carried out first to establish stress levels 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 in this option is reached. Convergence controls are provided on the CONTROL option for elastic-plastic analysis and in the AUTO THERM CREEP option for creep analysis. 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. 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 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. This is based on the fact that the increments of load and displacement correspond to the end of the transient time of the AUTO THERM CREEP input.

Viscoelasticity In a certain class of problems, structural materials exhibit viscoelastic behavior. Two examples of these problems are quenching of glass structures and time-dependent deformation of polymeric materials. The viscoelastic material retains linearity between load and deformation; however, this linear relationship depends on time. Consequently, the current state of deformation must be determined from the entire history of loading. Different models consisting of elastic elements (spring) and viscous elements (dashpot) can be used to simulate the viscoelastic material behavior described in Chapter 7. A special class of temperature dependence known as the Thermo-Rheologically Simple behavior (TRS) is also applicable to a variety of thermal viscoelastic problems. Both the equation of state and the hereditary integral approaches can be used for viscoelastic analysis.

Main Index

146 Marc Volume A: Theory and User Information

To model the thermo-rheologically simple material behavior, the SHIFT FUNCTION model definition option can be used to choose the Williams-Landel-Ferry equation or the power series expression or Narayanaswamy model. In Marc, two options are available for small strain viscoelastic analysis. The first option uses the equation of state approach and represents a Kelvin model. The second option is based on the hereditary integral approach and allows the selection of a generalized Maxwell model. The thermo-rheologically simple behavior is also available in the second option for thermal viscoelastic analysis. The Time-independent Inelastic Behavior section in Chapter 7 discusses these models in detail. Automatic time stepping schemes AUTO CREEP and AUTO STEP can be used in a viscoelastic analysis for first and second options, respectively. The first option for viscoelastic analysis uses the Kelvin model. To activate the generalized Kelvin model in Marc, use the VISCO ELAS or CREEP parameter. To input the matrices [A] and [B] for the Kelvin strain rate computations, use the CRPVIS user subroutine. To input creep time period and the tolerance control for the maximum strain in an increment, use the AUTO CREEP history definition option. The Simo model for large strain viscoelasticity can be used in conjunction with the damage and hyperelastic Mooney or Ogden material model. The large strain viscoelastic material behavior can be simulated by incorporating the VISCELMOON, VISCELOGDEN, or VISCELFOAM model definition option. Viscoelasticity for Mooney and Ogden materials is available in both the total and updated Lagrangian framework. Viscoelasticity for foam materials is available only in the updated Lagrangian framework. Nonlinear structural relaxation behavior of materials can be modeled by the Narayanaswamy model which accounts for memory effect. This model allows simulation of evolution of physical properties of glass subjected to complex time temperature histories. The thermal expansion behavior for the Narayanaswamy model is controlled via the VISCEL EXP model definition option.

Viscoplasticity There are two procedures in Marc for viscoplastic analysis: explicit and implicit. A brief description of each procedure follows: Explicit Method The elasto-viscoplasticity model in Marc is a modified creep model to which a plastic element is added. The plastic element is inactive when the stress is less than the yield stress of the material. You can use the elasto-viscoplasticity model to solve time-dependent plasticity and creep as well as plasticity problems with a nonassociated flow law. The CREEP option in Marc has been modified to enable solving problems with viscoplasticity. The method is modified to allow solving elastic-plastic problems with nonassociated flow rules which result in nonsymmetric stress-strain relations if the tangent modulus method is used. The requirements for solving the viscoplastic problem are: • CREEP parameter and creep controls • Load incrementation immediately followed by a series of creep increments specified by AUTO CREEP

Main Index

CHAPTER 5 147 Structural Procedure Library

• Use of the CRPLAW user subroutine and/or the NASSOC user subroutine The following load incrementation procedure enables a viscoplastic problem to be solved: 1. Apply an elastic load increment that exceeds the steady-state yield stress. 2. Relieve the high yield stresses by turning on the AUTO CREEP option. You may repeat steps 1 and 2 as many times as necessary to achieve the required load history. Note:

The size of the load increments are not altered during the AUTO CREEP process so that further load increments can be effected by using the PROPORTIONAL INCREMENT option.

The viscoplastic approach converts an iterative elastic-plastic method to one where a fraction of the initial force vector is applied at each increment with the time step controls. The success of the method depends on the proper use of the automatic creep time step controls. This means that it is necessary to select an initial time step that will satisfy the tolerances placed on the allowable stress change. The initial time step Δt =

allowable stress change x 0.7 Maximum viscoplastic strain rate x Young’s modulus

The allowable stress change is specified in the creep controls. The most highly stressed element usually yields the maximum strain rate. It is also important to select a total time that gives sufficient number of increments to work off the effects of the initial force vector. A total time of 30 times the estimated Δt is usually sufficient. Marc does not distinguish between viscoplastic and creep strains. A NASSOC user subroutine allows you to specify a nonassociated flow rule for use with the equivalent creep strains (viscoplastic) that are calculated by the CRPLAW user subroutine. A flag is set in the CREEP parameter in order to use the viscoplastic option with a nonassociated flow rule. The viscoplasticity feature can be used to implement very general constitutive relations with the aid of the ZERO and YIEL user subroutines. Since the viscoplasticity model in Marc is a modified creep model, you should familiarize yourself with the creep analysis procedure (see Nonlinear Analysis at the beginning of this chapter). Implicit Method A general unified viscoplastic material law can be implemented through the UVSCPL. user subroutine When using this method, you are responsible for defining the inelastic strain increment and the current stress.

Fracture Mechanics The fracture mechanics capabilities in Marc covers the evaluation of energy release rate and J-integral including automatic crack propagation. Two methods are offered for the evaluation: the mode separation method through the LORENZI option and the Virtual Crack Closure Technique (VCCT) with the VCCT option. The VCCT option also supports automatic crack propagation.

Main Index

148 Marc Volume A: Theory and User Information

Linear Fracture Mechanics Linear fracture mechanics presupposes existence of a crack and examines the conditions under which crack growth occurs. In particular, it determines the length at which a crack propagates rapidly for specified load and boundary conditions. The concept of linear fracture mechanics stems from Griffith’s work on purely brittle materials. Griffith stated that, for crack propagation, the rate of elastic energy release should at least equal the rate of energy needed for creation of a new crack surface. This concept was extended by Irwin to include limited amounts of ductility. In Irwin’s considerations, the inelastic deformations are confined to a very small zone near the tip of a crack. The basic concept presented by Griffith and Irwin is an energy balance between the strain energy in the structure and the work needed to create a new crack surface. This energy balance can be expressed using the energy release rate G as G = Gc

(5-103)

G is defined as dΠ G = – -------da

(5-104)

where Π is the strain energy and a is the crack length. G depends on the geometry of the structure and the current loading. G c is called the fracture toughness of the material. It is a material property which is determined from experiments. Note that the energy release rate is not a time derivative but a rate of change in potential energy with crack length. An important feature of Equation (5-103) is that it can be used as a fracture criterion; a crack starts to grow when G reaches the critical value G c . The stress and strain fields near the tip of a crack are singular for a linear elastic material model. The stresses and strains have the principal form K σ = ------ f ( θ ) r K ε = ------ g ( θ ) r

(5-105)

in a polar coordinate system centered at the crack tip. Thus, a linear elastic material is said to have a 1 ⁄ r singularity near a crack tip. It is easy to demonstrate that in both Griffith’s and Irwin’s considerations, the elastic energy release rate is determined by a single parameter: the strength of the singularity in the elastic stress field at the crack tip. This is the so-called stress intensity factor, and is usually denoted by capital K . The magnitude of K depends on the crack length, the distribution and intensity of applied loads, and the geometry of the structure. Crack propagation occurs when any combination of these factors causes a stress intensity factor K to be equal to or greater than the experimentally determined material property K c , which is equivalent to Equation (5-103). Hence, the objective of linear fracture mechanics calculations is to determine the value of K .

Main Index

CHAPTER 5 149 Structural Procedure Library

There are three possible modes of crack extension in linear elastic fracture mechanics: the opening mode, sliding mode, and tearing mode (see Figure 5-18). y

y

x

x

z

z

(a) Mode I: Opening

(b) Mode II: Sliding y

x z

(c) Mode III: Tearing Figure 5-18 Irwin’s Three Basic Modes of Crack Extension

The opening mode (see Figure 5-18a), Mode I, is characterized by the symmetric separation of the crack surfaces with respect to the plane, prior to extension (symmetric with respect to the X-Y and X-Z planes). The sliding mode, Mode II, is characterized by displacements in which the crack surfaces slide over one another perpendicular to the leading edge of the crack (symmetric with respect to the X-Y plane and skew-symmetric with respect to the X-Z plane). The tearing mode, Mode III, finds the crack surfaces sliding with respect to one another parallel to the leading edge (skew-symmetric with respect to the X-Y and X-Z planes). It is customary to associate a stress intensity factor with each of these mode: K I , K I I , and K I I I . There is also an associated fracture toughness associated with each mode: K I c , K I I c , and K I I I c . The most critical mode is usually mode I and in many cases the other modes are not considered. The connection between the energy release rate and the stress intensity factors is given by 2

2

KI KI I 1 + ν 2 G = ------- + -------- + ------------- K I I I E' E' E

Main Index

(5-106)

150 Marc Volume A: Theory and User Information

where E' = E for plane stress

(5-107)

and E E' = --------------- for plane strain. 1 – ν2

(5-108)

Marc uses the so-called J-integral for evaluating the energy release rate, see below. The J-integral is similar to G but is more general and is also used for nonlinear applications. J is equivalent to G when a linear elastic material model is used.

Nonlinear Fracture Mechanics Nonlinear fracture mechanics is concerned with determining under which conditions crack propagation (growth) occurs. In this sense, nonlinear fracture mechanics is similar to linear fracture mechanics. However, there are additional questions addressed in nonlinear fracture mechanics. Is the crack propagation stable or unstable? If it is stable, at which speed does it occur? After some propagation, is the crack arrested? There also exists a singularity at the crack tip in fracture mechanics problems with nonlinear elasticplastic material behavior, though the singularity is of a different nature. If one takes an exponential hardening law of the form σ ε 1/n ------ = ⎛⎝ -----⎞⎠ σ0 ε0

(5-109)

it can be shown that the singularities in the strain and the stresses at the crack tip are of the form ε = f ( θ )r – n ⁄ ( n + 1 ) σ = g ( θ )r – 1 ⁄ ( n + 1 )

(5-110)

If n approaches infinity, the material behavior becomes perfectly plastic and the singularity in the stresses vanishes. The singularity in the strains, however, takes the form of ε = f ( θ )r – 1

(5-111)

It has not been possible to establish that the strength of the singularity is the only factor that influences initiation of crack propagation for nonlinear situations. In fact, it is doubted that initiation of crack propagation is dependent on only a single factor. The J-integral probably offers the best chance to have a single parameter to relate to the initiation of crack propagation. The J-integral was introduced by Rice as a path-independent contour integral for the analysis of cracks. As previously mentioned, it is equivalent to the energy release rate for a linear elastic material model. It is defined in two dimensions as

Main Index

CHAPTER 5 151 Structural Procedure Library

J =

∂u j

⎛

⎞

- dΓ ∫ ⎝ ( W + T )n 1 – σ i j n i ------∂x 1⎠

(5-112)

Γ

where W is the strain energy density, T is the kinetic energy density, σ i j is the stress tensor and u i is the displacement vector. The

x1

direction is the same as the x direction in the local crack tip system in

Figure 5-19. The integration path Γ is a curve surrounding the crack tip, see Figure 5-19.The J-integral is independent of the path Γ as long as it starts and ends at the two sides of the crack face and no other singularities are present within the path. This is an important feature for the numerical evaluation since the integral can be evaluated using results away from the crack tip.

ni

y

x Γ

Figure 5-19 Definition of the J-integral

Numerical Evaluation of the J-integral The J-integral evaluation in Marc is based upon the domain integration method as described in [Ref. 30]. It is available as the LORENZI model definition option. A direct evaluation of Equation (5-112) is not very practical in a finite element analysis due to the difficulties in defining the integration path Γ . In the domain integration method for two dimensions, the line integral is converted into an area integration over the area inside the path Γ . This conversion is exact for the linear elastic case and also for the nonlinear case if the loading is proportional, that is, if no unloading occurs. By choosing this area as a set of elements, the integration is straightforward using the finite element solution. In two dimensions, the converted expression is J =

⎛

∂u j

⎞

δq 1

- – Wδ 1 i⎠ -------- dA ∫ ⎝ σ i j ------∂x 1 δx i

(5-113)

A

for the simplified case of no thermal strains, body forces or pressure on the crack faces. For the general expression, see [Ref. 1]. A is the area inside Γ and q 1 is a function introduced in the conversion into an area integral. The function q 1 can be chosen fairly generally, as long it is equal to one at the crack tip and zero on Γ . The form of the function chosen in Marc is that it has the constant value of one at all nodes inside Γ , and decreases to zero over the outermost ring of elements in A . It can be interpreted as

Main Index

152 Marc Volume A: Theory and User Information

a rigid translation of the nodes inside Γ while the nodes on Γ remain fixed. Thus, the contribution to Equation (5-113) comes only from the elements in a ring away from the crack tip. This interpretation is that of virtual crack extension and this method can be seen as a variant of such a technique, although it is extended with the effects of thermal strains, body forces, and pressure on the crack faces.The set of nodes moved rigidly is referred to as the rigid region and the function q 1 as the shift function or shift vector. For the evaluation of the J-integral the direction of the shift vector is simply the x axis in the local crack tip system. In three dimensions, the line integral becomes an area integral where the area is surrounding a part of the crack front. In this case, the selection of the area is even more cumbersome than in two dimension. The converted integral becomes a volume integral which is evaluated over a set of elements. The rigid region is a set of nodes which contains a part of the crack front, and the contribution to the integral comes from the elements which have at least one but not all its nodes in the rigid region. Determination of the Rigid Region and the Shift Vector For the evaluation of the J-integral, Marc requires the nodes along the crack front, the shift vector, and the nodes of the rigid region. Marc allows three ways of defining the rigid region. The first is direct input; the nodes or elements in the rigid region are listed explicitly. With this variant, the shift vector is also specified directly. The second and third variants use an automatic search for the nodes of the rigid region. The second variant is based on the mesh topology (connectivity) where a number of regions of increasing size are found by Marc. The first region for two dimensions consists of the nodes of all elements connected to the crack tip node. The second region consists of all nodes in the first region and the nodes of all elements connected to any node in the first region and so on for a given number of regions. This way, contours of increasing size are determined. In the third way of determining the rigid region, a radius is given and all nodes within that radius are part of the rigid region. For the automatic search methods the shift vector can also be determined automatically. It is then determined using the first element edge on the crack face (for meshes with notches see below). Symmetry at the crack face is automatically detected by Marc, also for the case that the symmetry condition is applied by means of a rigid contact body. In three dimensions, it is a bit more complicated. The crack front is defined by an unsorted list of nodes. In order to obtain the variation of the J-integral along the crack front, a disk of nodes with the normal of the disk directed along the tangent to the crack front can be determined. This type of disk can readily be defined if the mesh around the crack front consists of brick elements in a regular mesh. This mesh is typically created from a two-dimensional mesh which is extruded along the crack front. The topology based determination of the rigid region assumes such a mesh and creates disks of increasing size at each crack front node from element faces. The shift vector at each crack front node is automatically determined to be perpendicular to both the tangent to the crack front and the normal to the crack face at each crack front node. At the first and last crack front node, where a free surface is assumed to exist, the shift direction is projected to the tangent to the free surface. This is important since the shift must not change the outer boundary of the model. The geometry based search method here works with a cylinder with the axis aligned with the tangent of the crack front and centered at the crack front node. The length of the cylinder is given as a fraction of the distance to the neighboring crack front nodes. All nodes within the cylinder are part of the rigid region. This method is useful if, for instance, the mesh around the crack front is created with an automatic mesh generator. The shift vector is determined in the same way as for the topology based search method.

Main Index

CHAPTER 5 153 Structural Procedure Library

In elasto-plastic analyses, it is often advantageous to use a mesh where there are several (multiple) nodes at the crack tip. If collapsed elements are used at the crack tip, the nodes are kept separate and a notch is formed as the crack tip deforms. For this kind of mesh, a “multiple nodes” distance is given, which should be smaller than the smallest element at the crack tip. All nodes within that distance are then considered part of the crack tip, and the first contour for the topology based search will consist of all elements connected to any of these nodes (in three-dimensions of element faces connected to any of these nodes). The normal to the crack face used for determining the shift vector is taken as the first face outside the crack tip nodes. Thus, it is also possible to model the crack with an initial notch. Mode Separation For the linear elastic case, Marc automatically calculates and prints the stress intensity factors

KI , KI I ,

and K I I I for the three modes I, II, and III. This evaluation is done using analytical functions for the stress field near the crack tip. The implementation is based upon the procedure outlined in [Ref. 33]. Mode separation is not calculated when nonlinearities like large deformations, nonlinear material, or general contact are present. However, the use of glued contact is allowed to connect different parts of the mesh near the crack front. The material is also not allowed to be temperature dependent. Orthotropic materials are allowed. The calculation of the stress intensity factors is automatically suppressed if unsupported features are used. The stress intensity factors are defined in the local crack tip system, see Figure 5-19. K I will be positive when the crack is opening and negative when it is overlapping. Similarly, K I I is positive when the shear stress is positive ahead of the crack in the local system. Supported Features The LORENZI J-integral option supports the following features: Linear and nonlinear materials. Large deformations. Both total and updated Lagrangian formulation are supported. The crack tip system can undergo finite rotations and translations. Thermal loads. Transient dynamics. Contact between crack faces including friction. Loads on the crack faces. Mode separation for linear elasticity and no loads in the crack region.

Numerical Evaluation of the Energy Release Rate with the VCCT Method The VCCT option offers a simpler but more general way for obtaining the energy release rate. The implementation follows the description in R. Krueger [Ref. 34]. Consider again Equation (5-104). dΠ G = – -------da

Main Index

(5-114)

154 Marc Volume A: Theory and User Information

It states that G is the change in potential energy by a change in crack length. Now, consider the simple finite element model in Figure 5-20. The models A and B are the same, except that in B, the crack has grown by one element edge of length a. Suppose we do one analysis for each one of the two models. We can now calculate the energy release rate G as: Fu G = -----2a

(5-115) a u

F

Model A

Model B

Figure 5-20 Mesh for Illustrating the CCT Method

Here, F is the force (obtained from Model A) that keeps the crack together, and the crack opening, u , is obtained from Model B. In order to obtain these quantities, we would need to perform two analyses and this method is often referred to as CCT (Crack Closure Technique). In the virtual crack closure technique, we only do the analysis with a closed crack (Model A) and use the opening displacement at the closest nodes to the crack tip. Figure 5-21 shows the case of pure mode I. The other modes are treated similarly and separately. The displacements and reactions are transformed into the local crack tip system for this evaluation. a

F u

Figure 5-21 The VCCT Method

Main Index

CHAPTER 5 155 Structural Procedure Library

With x. y, and z denoting the coordinate directions in the local crack tip system (see Figure 5-18), we obtain: F y uy G I = -----------2a

Fx ux G I I = -----------2a

Fz uz G I I I = ----------2a

(5-116)

and the total energy release rate as: (5-117)

Gt o t = GI + GI I + GI I I For higher-order elements, we need to include the contributions from the midside nodes (see Figure 5-22). F 1 u1 + F2 u2 G I = ------------------------------2a

(5-118)

For the case that the midside nodes are not at the middle of the element edges (for example, using the 1/4 point position for increased accuracy, the displacements for these nodes are interpolated to the appropriate locations. a

F1 F2 u1 u2

Figure 5-22 Higher-order Elements

For 3-D solids, we have a situation as shown in Figure 5-23. The situation is similar to the 2-D case, and the evaluation is done separately for each node along the crack front. The area is given by the shaded part in Figure 5-23. For the case of higher-order elements, we obtain the following by using the notation in Figure 5-24. 1 F 1 u 1 + F 2 u 2 + --- ( F 3 u 3 + F 4 u 4 ) 2 G = ------------------------------------------------------------------------------2a

Main Index

(5-119)

156 Marc Volume A: Theory and User Information

u is Crack Opening Displacement At Crack Face Crack Front F

a

Figure 5-23 3-D Mesh for VCCT

u4

u1

u3 u2

F1 F4

F3 F2

Figure 5-24 3-D Mesh for VCCT for Higher-order Elements

The above figures show a regular mesh of hexahedral elements. While a mesh designed like this is advantageous for accuracy, it is not strictly necessary. It is also possible to use a general tetrahedral mesh or a hexahedral mesh with the crack front as defined in Figure 5-25. The latter is typically obtained in the case of crack propagation as described below. The program will find the appropriate nodes to use for the forces and crack opening displacement and calculate an area a. In the current release, the case of higher order tetrahedral elements is not supported.

Main Index

CHAPTER 5 157 Structural Procedure Library

Figure 5-25 Example of Crack Front Not Following Element Edges

The definition of the data involved in the VCCT calculation is done automatically. The user only specifies the crack tip or crack front. In order to check what the program finds there is debug option available. If the PRINT parameter is used with a value of 43, the program will print out the nodes it finds, the corresponding forces, crack opening displacements, and crack areas. Symmetry is automatically detected and accounted for. The symmetry condition can be enforced by boundary conditions or by rigid contact. The mesh in the crack region can contain user tyings or contact. The program automatically detects if the crack tip node is connected to a node, and the node it is connected to is considered part of the crack tip. The supported connections are glued contact, user typing, RBE2 and RROD. For the case that the connection is done node-to-node, it does not matter if the tied or retained node of the tying is selected as the crack node. With glued contact, it is not necessary to connect the parts node-to-node. If the meshes do not match up, the crack will be treated similarly as a case of symmetry. This non-matching glued case is automatically detected and for this case, it is necessary to select the touching node as the crack tip node. A useful option when defining a crack using glued contact is DEACT GLUE. Suppose two parts are glued together and the crack is defined as part of the interface between the bodies. One can then use DEACT GLUE to identify the nodes that should be on the crack faces (see Figure 5-26). These nodes will have regular contact but not be glued.

Main Index

158 Marc Volume A: Theory and User Information

Crack Tip Glued Contact

Nodes Identified with DEACT GLUE Contact Body 1

Contact Body 2

Figure 5-26 Using DEACT GLUE for Defining a Crack

The calculation of VCCT is done in the current geometry in case of large deformations. The updated crack coordinate system is calculated at each increment and the calculations are done in this system. Thus, arbitrary rotations and deformations are allowed. The current crack tip system is available on the post file. The three coordinate axes can be plotted as vectors for verification. The program calculates an estimated crack growth direction for each crack front node. Four methods for defining this are supported: the maximum principal stress criterion ([Ref. 35]), along the pure mode with largest G i – G i c (where i is mode I, II or III), along mode I and along a specified vector. The maximum principal stress criterion states that a crack will grow in the direction normal to the direction of greatest tension. The crack growth direction normal to the direction of greatest tension. The crack growth direction ( d x ,d y ) in the local crack tip system can be expressed in terms of the stress intensity factors in mode I and II as: 2

dx

2

KI I K II 3 -------- + 1 + 8 -------2 2 KI KI = ---------------------------------------------2 KI I 1 + 9 -------2 KI

2

dy

KI I KI I KI I 3 -------- – 3 -------- 1 + 8 -------2 KI KI KI = ---------------------------------------------------------2 KI I 1 + 9 -------2 KI

(5-120)

For the 3-D case, mode III is assumed to have the same effect as mode I so K I + K I I I is used instead of K I in the above equation. It is, thus, assumed that crack growth occurs perpendicular to the crack front tangent. The user can also specify the crack growth direction through the user subroutine UCRACKGROW. Figure 5-27 shows some examples of supported crack configurations. There is a large flexibility in how parts can be tied or glued together to form a crack.

Main Index

CHAPTER 5 159 Structural Procedure Library

Crack Tip Crack Front

Line Crack in Shell

Shell Glued to Shell

Shell Glued to Solid (Line Crack)

3-D Solid

Shell Glued to Solid (Surface Crack)

Figure 5-27 Examples of Supported Crack Types

Remeshing is supported for 2-D solids and shells. A structure containing a crack can be remeshed and the new crack tip is automatically found after remeshing. The crack opening displacement is saved before the remesh, and applied afterwards to make sure that the results are also correct after remeshing takes place. Three-dimensional solids with cracks cannot currently be remeshed. Remeshing can also be used for automatic crack propagation as described below.

Automatic Crack Propagation The VCCT option allows automatic crack propagation to be performed. There are two types of crack propagation analysis types available: fatigue growth and direct growth. There are three methods for how the crack growth is performed: growth during remeshing and growth by releasing tyings or glued contact and growth along element edges. These four options are described in the following. Fatigue Crack Growth Here, the user specifies a fatigue time period. The analysis is performed without crack growth during this period, which can be repeated any number of times. During the time period, it records the maximum and minimum energy release rate and the estimated crack growth direction at the maximum. At the end of each fatigue time period, the crack growth is applied. For the growth, we need to know the distance and direction the crack should grow. The distance is either user specified (possibly scaled by a table) or obtained by Paris’ law. With Paris’ law we use the following expression: a = C [ ( Gm a x –

Main Index

Gm i n )m –

Gt hm ]

(5-121)

160 Marc Volume A: Theory and User Information

This formula is from T. L. Anderson [Ref. 31], modified to use G instead of the stress intensity K. No growth occurs if G m a x – G m i n < G t h or a < a m i n . The ucrack_paris.f user subroutine can be used for specifying the growth increment. The crack growth increment is first calculated with Equation (5-121) and then the user subroutine is called. See UCRACKGROW in Volume D: User Subroutine, Special Routines, and Utility Routines for details. If growth by remeshing is used, the calculated crack growth increment and estimated crack growth direction are used for defining the location of the new crack tip. When release of glued contact or tyings are used, then one element edge at the time is released. Paris’ law for this case. If there are multiple choices available for which element edge to release, then the one closest to the crack growth direction is chosen. Direct Crack Growth For this case, a standard incremental analysis is performed. The user specifies a crack growth resistance (fracture toughness) for each crack. When the crack growth criterion is fulfilled, a propagation is done. This takes place within an increment; the increment will iterate until no further crack growth occurs. For unstable crack growth, this may have the effect that the crack grows through the whole structure within one increment. This ensures that an increment does not show convergence when a crack should grow which would violate the crack growth criterion. With remeshing based growth, the user specifies the crack growth increment to use and the current estimated crack growth direction is used. Repeated remeshing may be used in an increment if more growth is triggered. For the growth by releasing tyings or glued contact, one element edge at the time is released until no more growth occurs. For both methods, the growth only occurs when the increment is otherwise converged. Remeshing Based Growth Crack growth by means of remeshing is available for 2-D solid elements. The model must be set up to do global remeshing, but no specific remeshing criterion needs to be set for the crack propagation. Any specified remeshing criterion will be treated independently from the remeshings due to crack growth. It is, for example, allowed to do remeshings during the fatigue load cycle. When a remeshing occurs in a 2-D analysis, the program first finds the outline of the remeshing body. When a crack is growing, this outline is extended to form a new crack tip location. In order to assure that we obtain a mesh with an element edge in the x direction of the local crack tip system, we extend the outline a little further than to the new crack tip. The new mesh is modified such that the new mesh is correct. This way we avoid meshes as shown in Figure 5-28a. If a crack reaches the boundary of the model, the remeshing body automatically splits. Thus, a crack can grow into another crack, an internal hole of the body, or the external boundary. Due to the outline extension mentioned above, the crack will reach the boundary slightly earlier than one would otherwise expect. The setting of target element length after remeshing will be overridden for the case that it is larger than the growth increment. This ensures that the mesh resolution is large enough to model the new crack tip. The mesh around the crack tip is automatically refined when growth occurs. An example of a remeshed crack is shown in Figure 5-28b.

Main Index

CHAPTER 5 161 Structural Procedure Library

a) poor mesh which is avoided during crack growth

b) refined mesh at current crack tip

Figure 5-28 Meshes after Remeshing.

Growth by Releasing Tyings or Glued Contact For this option, the user needs to specify the crack growth path. The crack can only grow in the direction where there are tyings or glued contact to release. All crack configurations are supported: 2-D, shells and 3-D. For the case of user tyings, there are three types of tyings supported: user tying type 100, RBE2 and RROD. Here, the nodes need to be aligned on both sides of the crack faces. The user specifies only the crack tip node; the program automatically finds the tyings to release. It does not matter if the tied or retained node is selected as the crack tip node or crack front nodes. For glued contact, the meshes do not need to match up. As mentioned in the previous section, a special non-matching glue symmetry case is automatically used if the nodes do not match up. For this case, the tied nodes must be selected as the crack tip nodes. When nodes in glued contact are released due to crack growth, they switch from glued contact to regular contact. The DEACT GLUE option is here used internally. Thus, a node which is released can still contact the new crack face, but it will not glue back again. If higher-order elements are used, the midside node will be released when the corresponding corner node is released. If a crack reaches a model boundary, the crack evaluation for this crack will be turned off and the analysis can continue. The program avoids that a single node is tied at a boundary; if the last element edge is released, then the last node will also be released. If the mesh is designed such that there are multiple choices for which element edge to release, then the one closest to the estimated crack growth direction is chosen.

Main Index

162 Marc Volume A: Theory and User Information

For the 3-D case, it is assumed that the area where the crack grows has a regular mesh. The crack should not grow into areas of irregular mesh. See Figure 5-29 for an illustration. If the crack reaches the point indicated at the top part of the figure, the crack front would have to be extended, which is not supported at this point. Within the regular growth zone the crack can grow irregularly of course. Crack Front Branch

Original Crack Front

Largest Growth Zone

Figure 5-29 Possible Growth Zone for 3-D Crack Propagation

Growth Along Element Edges For this option, the crack can grow along element edges for 2-D and shell elements. The element edge closest to the crack growth direction is used. New nodes are automatically inserted and the element connectivity is changed for elements around the crack tip in order to grow the crack. The new nodes inherit the properties of the respective original node. Crack Growth Criteria and Direction There are currently four different crack growth criteria available: Total G. The crack will grow if G > G c , where G c is the crack growth resistance (also called fracture toughness).

Main Index

CHAPTER 5 163 Structural Procedure Library

Separately for each mode. Crack growth will take place if either of the following is true: G I > G Ic , G I I > G I I c or G I I I > G I I I c . GI n1 G I I n2 G I II n 3 Power law mixed mode criterion ⎛ --------⎞ + ⎛ ----------⎞ + ⎛ -------------⎞ > 1 ⎝ G I c⎠ ⎝ G I I c⎠ ⎝ G II I c⎠ Reeder mixed mode criterion G I + G I I + G II I >1 ---------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------n GI I + GI I I G I I I ⎛ G I I + G I II ⎞ n 1 1 ⎛ ⎞ G I c + ( G I Ic – G I c ) --------------------------------------+ ( G I I I c – G I I c ) ------------------------- ⎜ ---------------------------------------⎟ ⎝ G I + G I I + G I I I⎠ GI I + GI I I ⎝ G + G + G ⎠ I II II I The Reeder mixed mode criterion was suggested in [Ref. 39]. For 2-D, it coincides with the criterion by Benzeggagh and Kenane, see [Ref. 40]. Each of the four methods above are available for the calculation of the crack growth direction.

Dynamic Fracture Methodology In complete similarity with static fracture mechanics concepts, it is assumed that dynamic crack growth processes for linear materials are governed by the following condition: K I ( t ) = R I D ( a· , T, B )

a· ≥ 0

(5-122)

where K I ( t ) is the dynamic stress intensity factor for mode I, a· is the crack velocity, and R I D is the dynamic crack propagation toughness, which is assumed to be a material parameter that in general depends on crack velocity a· , temperature T , and specimen thickness B . The dynamic stress intensity factor depends on crack length ( a ), applied loading ( σ ), time ( t ), specimen dimensions ( D ), temperature ( T ), and initial stress fields ( σ i ) caused by residual stresses or by an initial strain field. The prediction of the crack propagation history and crack arrest event demands complete knowledge of the R I D vs. a· relation. The Dynamic Fracture Methodology procedure consists of the following two phases: 1. Generation phase – in this phase, a crack arrest experiment is performed yielding a crack propagation-versus-time curve. In addition, a numerical simulation of the experiment is carried out by using the measured crack propagation curve. This is used as input for the numerical model. This allows the calculation of dynamic stress intensity factors as a function of time. Combination of the latter relation with the measured crack propagation curve results in a curve, which can be considered the dynamic crack propagation toughness-versus-crack velocity relation.

Main Index

164 Marc Volume A: Theory and User Information

2. Application phase – in order to predict the crack growth and possible crack arrest point in a structural component, the inverse problem is solved. Now, the actual stress intensity factors are calculated for the structural component, that is subjected to a particular loading history, by means of a dynamic finite element analysis. These calculated values are compared to the fracture toughness curve obtained during the generation phase, Equation (5-122), and from this the crack growth is predicted.

Modeling Considerations The main difficulty in the finite element analysis of linear elastic fracture mechanics is representing the solution near the crack front. Typically, a focused mesh is used with the elements in a spider web shape. This gives a mesh with rings of elements in a radial fashion and is particularly useful for studying the variation of the values of J with contour radius. If higher order elements are used for an elastic analysis, it is advantageous to use so-called quarter point elements at the crack tip. These are regular elements where the midside nodes at element sides for which one node is part of the crack tip are shifted towards the crack tip to the quarter point location along the side. This gives a more accurate description of the singularity at the crack tip and is important to use if a coarse mesh is used. In three-dimensions, the mesh along the crack front is typically created from a planar mesh which is extruded along the crack front region as mentioned above. This allows the rigid regions to be created in a regular manner which is advantageous for accuracy. Note that Marc allows rigid contact surfaces to be used for applying symmetry conditions. For a three-dimensional example, see the Marc User’s Guide, Chapter 6.2.

Dynamic Crack Propagation The concepts of fracture mechanics discussed in previous sections have been applied to the prediction of crack initiation, as well as slow stable crack growth of statically loaded structures and for the prediction of fatigue crack growth in cyclically loaded structures. In problems where inertial effects cannot be ignored, application of quasi-static fracture mechanics techniques can lead to erroneous conclusions. The use of dynamic fracture mechanics concepts for these problems is clearly of necessity. The main emphasis on dynamic fracture mechanics is to predict the initiation of stationary cracks in structures, which are subjected to impact loading. It also focuses on the conditions for the continuous growth of fast propagating cracks, and on the conditions under which a crack is arrested. The problem of predicting the growth rate and the possible crack arrest point is quite complicated. It is often treated by means of a so-called dynamic fracture methodology, which requires the combined use of experimental measurements and of detailed finite element analyses. An essential step in this approach is formed by the numerical simulation of propagating cracks by means of the finite element method. The J-integral as implemented in Marc takes into account the effect of inertial and body forces, thermal and mechanical loading and initial strains. The use of the DYNAMIC parameter and the LORENZI model definition option allows for the calculation of dynamic energy release rates for cracked bodies which are subjected to arbitrary thermal and mechanical loadings including initial stresses.

Main Index

CHAPTER 5 165 Structural Procedure Library

Mesh Splitting Marc has the capability to split up the mesh automatically during the analysis. The mesh split can be done at nodes and along element edges (2-D and shells) or element faces (3-D). A new node is created where the split is done. This node inherits the current properties of the original node. The elements at one side of the split are modified to use the new node to create the opening in the mesh. The mesh can also be split by means of the USPLIT_MESH user subroutine. See Marc Volume D: User Subroutines and Special Routines for details. The DELAMIN model definition option allows the specification of mesh splitting between materials and within a material using a stress criterion: σ m σ n ⎛ -----n-⎞ + ⎛ -----t⎞ > 1 ⎝ S n⎠ ⎝ S t⎠

(5-123)

Here σ n is the normal stress, σ t the tangential stress and S n , S t , m and n are user-defined parameters. With the option to split between materials, the program checks all nodes in the interface between the specified materials. The stresses are extrapolated to the nodes and transformed to the material interface. The normal direction is perpendicular to the material interface. With the option to split within a material, it checks all nodes inside a material. The normal direction is perpendicular to each element edge or face. If contact is used, the program recalculates the contact boundary after mesh splitting takes place. This is important in order to avoid penetration between the newly generated free surfaces. Nodal post codes are available for post processing the separate terms in Equation (5-123) as well as the sum. An option is available in the DELAMIN option for inserting interface elements using a cohesive zone material model where the mesh is split. This is automatically done whenever a split takes place. The new elements use the nodes of the surrounding elements. If the split up zone grows, more interface elements are added. The cohesive material properties of the interface elements must be defined in the model. The ELEMENTS parameter defining the element type for the interface elements must be included.

Dynamics Marc’s dynamic analysis capability allows you to perform the following calculations: • • • •

Eigenvalue Analysis Transient Analysis Harmonic Response Spectrum Response

The program contains two methods for eigenvalue extraction and three time integration operators. Nonlinear effects, including material nonlinearity, geometric nonlinearity, and boundary nonlinearity, can be incorporated. Linear problems can be analyzed using modal superposition or direct integration. All nonlinear problems should be analyzed using direct integration methods.

Main Index

166 Marc Volume A: Theory and User Information

In addition to distributed mass, you can also attach concentrated masses associated with each degree of freedom of the system. You can include damping in either the modal superposition or the direct integration methods. You can also include (nonuniform) displacement and/or velocity as an initial condition, and apply time-dependent forces and/or displacements as boundary conditions.

Eigenvalue Analysis Marc uses either the inverse power sweep method or the Lanczos method to extract eigenvalues and eigenvectors. The DYNAMIC parameter is used to determine which procedure to use, and how many modes are to be extracted. The inverse power sweep method is typically used for extracting a few modes while the Lanczos method is optimal for several modes. After the modes are extracted, they can be used in a transient analysis or spectrum response calculation. In dynamic eigenvalue analysis, we find the solution to an undamped linear dynamics problem: ( K – ω 2 M )φ = 0 where K is the stiffness matrix, M is the mass matrix, ω are the eigenvalues (frequencies) and φ are the eigenvectors. In Marc, if the extraction is performed after increment zero, K is the tangent stiffness matrix, which can include material and geometrically nonlinear contributions. The mass matrix is formed from both distributed mass and point masses. Inverse Power Sweep Marc creates an initial trial vector. To obtain a new vector, the program multiplies the initial vector by the mass matrix and the inverse (factorized) stiffness matrix. This process is repeated until convergence is reached according to either of the following criteria: single eigenvalue convergence or double eigenvalue convergence. In single eigenvalue convergence, the program computes an eigenvalue at each iteration. Convergence is assumed when the values of two successive iterations are within a prescribed tolerance. In double eigenvalue convergence, the program assumes that the trial vector is a linear combination of two eigenvectors. Using the three latest vectors, the program calculates two eigenvalues. It compares these two values with the two values calculated in the previous step; convergence is assumed if they are within the prescribed tolerance. When an eigenvalue has been calculated, the program either exits from the extraction loop (if a sufficient number of vectors has been extracted) or it creates a new trial vector for the next calculation. If a single eigenvalue was obtained, Marc uses the double eigenvalue routine to obtain the best trial vector for the next eigenvalue. If two eigenvalues were obtained, the program creates an arbitrary trial vector orthogonal to the previously obtained vectors. After Marc has calculated the first eigenvalue, it orthogonalizes the trial vector at each iteration to previously extracted vectors (using the Gram-Schmidt orthogonalization procedure). Note that the power shift procedure is available with the inverse power sweep method. To select the power shift, set the following parameters: • Initial shift frequency – This is normally set to zero (unless the structure has rigid body modes, preventing a decomposition around the zeroth frequency).

Main Index

CHAPTER 5 167 Structural Procedure Library

• Number of modes to be extracted between each shift – A value smaller than five is probably not economical because a shift requires a new decomposition of the stiffness matrix. • Auto shift parameter – When you decide to do a shift, the new shift point is set to Highest frequency2 + scalar x (highest frequency - next highest frequency)2 You can define the value of the scalar through the MODAL SHAPE option. The Lanczos Method The Lanczos algorithm converts the original eigenvalue problem into the determination of the eigenvalues of a tri-diagonal matrix. The method can be used either for the determination of all modes or for the calculation of a small number of modes. For the latter case, the Lanczos method is the most efficient eigenvalue extraction algorithm. A simple description of the algorithm is as follows. Consider the eigenvalue problem: –ω 2 M u + K u = 0

(5-124)

Equation (5-124) can be rewritten as: 1 ------2 M u = M K – 1 M u ω

(5-125)

Consider the transformation: u = Qη

(5-126) T

Substituting Equation (5-126) into Equation (5-125) and premultiplying by the matrix Q on both sides of the equation, we have 1 ------2 Q T M Q η = Q T M K – 1 M Q η ω

(5-127)

The Lanczos algorithm results in a transformation matrix Q such that: QT M Q = I

(5-128)

Q T M K – 1 MQ = T

(5-129)

where the matrix T is a symmetrical tri-diagonal matrix of the form: α1 β2 T =

β2 α2 β3 βm 0

Main Index

0

βm αm

(5-130)

168 Marc Volume A: Theory and User Information

Consequently, the original eigenvalue problem, Equation (5-125), is reduced to the following new eigenvalue problem: 1 ------ η = T η ω2

(5-131)

The eigenvalues in Equation (5-131) can be calculated by the standard QL-method. Through the MODAL SHAPE option, you can either select the number of modes to be extracted, or a range of modes to be extracted. The Sturm sequence check can be used to verify that all of the required eigenvalues have been found. In addition, you can select the lowest frequency to be extracted to be greater than zero. The Lanczos procedure also allows you to restart the analysis at a later time and extract additional roots. It is unnecessary to recalculate previously obtained roots using this option. Convergence Controls Eigenvalue extraction is controlled by: a. The maximum number of iterations per mode in the power sweep method; or the maximum number of iterations for all modes in the Lanczos iteration method, b. an eigenvalue has converged when the difference between the eigenvalues in two consecutive sweeps divided by the eigenvalue is less than the tolerance, and c. the Lanczos iteration method has converged when the normalized difference between all eigenvalues satisfies the tolerance. Modal Stresses and Reactions After the modal shapes (and frequencies) are extracted, the RECOVER history definition option allows for the recovery of stresses and reactions at a specified mode. This option can be repeated for any of the extracted modes. The stresses are computed from the modal displacement vector φ ; the nodal reactions 2

are calculated from F = Kφ – ω Mφ . The RECOVER option is also used to place eigenvectors on the post file.

Transient Analysis Transient dynamic analysis deals with an initial-boundary value problem. In order to solve the equations of motion of a structural system, it is important to specify proper initial and boundary conditions. You obtain the solution to the equations of motion by using either modal superposition (for linear systems) or direct integration (for linear or nonlinear systems). In direct integration, selecting a proper time step is very important. For both methods, you can include damping in the system. The following sections discuss the seven aspects of transient analysis listed below. • • • • •

Main Index

Modal Stresses and Reactions Direct Integration Time Step Definition Initial Conditions Time-Dependent Boundary Conditions

CHAPTER 5 169 Structural Procedure Library

• Mass Matrix • Damping Modal Superposition The modal superposition method predicts the dynamic response of a linear structural system. In using this method, we assume that the dynamic response of the system can be expressed as a linear combination of the mode shapes of the system. For the principle of superposition to be valid, the structural system must be linear. Damping can be applied to each mode used in the superposition procedure. To select the eigenvalue extraction method and the number of modal shapes, use the DYNAMIC parameter. To select a fraction of critical damping for each mode, use the DAMPING model definition option. The DYNAMIC CHANGE history definition option can be used to select the time step.

Main Index

170 Marc Volume A: Theory and User Information

5

Marc obtains the transient response on the basis of eigenmodes extracted. The number of modes extracted (rather than the choice of time step) governs the accuracy of the solution.

Structur al Procedu re Library

Consider the general linear undamped problem M u·· + K u = f ( t )

(5-132)

and suppose that n eigenvectors φ 1, …, φ n are known. u = Σφ i u i ( t )

(5-133)

The eigenmodes are orthogonal with respect to the M and K matrices. After substitution in Equation (5-132), we find a set of uncoupled dynamic equations m i u·· i + k i u i = f i ( t )

(5-134)

where: m i = φ iT Mφ i

(5-135)

k i = φ iT Kφ i

(5-136)

f i ( t ) = φ iT f ( t )

(5-137)

We can introduce damping on each mode as a fraction of critical damping ( μ i ) for that mode. We can rewrite Equation (5-134) in the form m i u·· i + 2m i ω i μ i u· i + k i u i = f i ( t )

(5-138)

or if we normalize Φ i such that m i = 1 : u·· i + 2ω i μ i u· i + ω i2 u i = f i ( t )

(5-139)

The response of a particular mode is then given by the solution of Equation (5-139) which is: t

ui ( t ) =

∫ f i ( τ )h ( t – τ ) dτ

(5-140)

0

with: 1 – μi ωi t h ( t ) = ------- e sin ( ω id t ) ω id h(t) = 0

Main Index

t<0

t≥0

CHAPTER 5 171 Structural Procedure Library

ω id =

( 1 – μ i2 ) ⋅ ω i

The evaluation of the Duhamel integral, Equation (5-140), can be performed exactly if the load changes linearly in a specific time increment. Hence, if the load changes rapidly in a specific time period, small load steps have to be taken. In case initial displacements u 0 or initial velocities u· 0 are given a transformation to the reduced modal system is needed for those conditions: u i0 = Φ iT ⋅ M ⋅ u 0 and u· i0 = Φ iT ⋅ M ⋅ u· 0 The solution of these initial conditions which must be added to the response given in Equation (5-140) is: ui ( t ) = e

–μ ω t i i

u· i0 + u i0 μ i ω i ------------------------------- ⋅ sin ( ω id ⋅ t ) + u i0 ⋅ cos ( ω id ⋅ t ) ω id

(5-141)

The initial accelerations due to given initial displacements u 0 and initial velocities u· 0 can be obtained by differentiation of Equation (5-141): u·· i0 = – ( ω i2 ⋅ u i0 ) – ( 2 ⋅ μ i ⋅ ω i ⋅ u· i0 ) Direct Integration Direct integration is a numerical method for solving the equations of motion of a dynamic system. It is used for both linear and nonlinear problems. In nonlinear problems, the nonlinear effects can include geometric, material, and boundary nonlinearities. For transient analysis, Marc offers four direct integration operators listed below. • • • •

Newmark-beta Operator Houbolt Operator Generalized-Alpha Operator Central Difference Operator

To select the direct integration operator, use the DYNAMIC parameter. Specify the time step size through the DYNAMIC CHANGE or AUTO STEP option. Direct integration techniques are imprecise; this is true regardless of which technique you use. Each technique exhibits at least one of the following problems: conditional stability, artificial damping, and phase errors. Newmark-beta Operator This operator is probably the most popular direct integration method used in finite element analysis. For linear problems, it is unconditionally stable and exhibits no numerical damping. The Newmark-beta operator can effectively obtain solutions for linear and nonlinear problems for a wide range of loadings. The procedure allows for change of time step, so it can be used in problems where sudden impact makes a reduction of time step desirable. This operator can be used with adaptive time step control. Although this method is stable for linear problems, instability can develop if nonlinearities occur. By reducing the time step and/or adding (stiffness) damping, you can overcome these problems.

Main Index

172 Marc Volume A: Theory and User Information

Houbolt Operator This operator has the same unconditional stability as the Newmark-beta operator. In addition, it has strong numerical damping characteristics, particularly for higher frequencies. This strong damping makes the method very stable for nonlinear problems as well. In fact, stability increases with the time step size. The drawback of this high damping is that the solution can become inaccurate for large time steps. Hence, the results obtained with the Houbolt operator usually have a smooth appearance, but are not necessarily accurate. The Houbolt integration operator, implemented in Marc as a fixed time step procedure, is particularly useful in obtaining a rough scoping solution to the problem. Single Step Houbolt Operator Two computational drawbacks of the Houbolt operator are the requirement of a special starting procedure and the restriction to fixed time steps. In [Ref. 29], a Single Step Houbolt procedure has been presented, being unconditionally stable, second order accurate and asymptotically annihilating. In this way, the algorithm is computationally more convenient compared to the standard Houbolt method, but because of its damping properties, the time steps have to be chosen carefully. This algorithm is recommended for implicit dynamic contact analyses. Generalized Alpha Operator One of the drawbacks of the existing implicit operators is the inability to easily control the numerical dissipation. While the Newmark-Beta method has no dissipation and works well for regular vibration problems, the Single-Step Houbolt method has numerical dissipation and works well for implicit dynamic contact problems. A single scheme that easily allows zero/small dissipation for regular structural dynamic problems and high-frequency numerical dissipation for dynamic contact problems is desirable. In [Ref. 36], a Generalized-alpha method has been presented as an unconditionally stable, second-order algorithm that allows user-controllable numerical dissipation. The dissipation is controlled by choosing either the spectral radius S of the operator or alternatively, two parameters αf and αm. The choice of the parameters provides a family of time integration algorithms that encompasses the Newmark-Beta, Single-Step Houbolt and the Hilber-Hughes-Taylor time integration methods as special cases. Central Difference Operators These explicit operators for IDYN = 4 and IDYN = 5 are only conditionally stable. The program automatically calculates the maximum allowable time step. This method is not very useful for shell or beam structures because the high frequencies result in a very small stability limit. This method is particularly useful for analysis of shock-type phenomena. In this procedure, since the operator matrix is a diagonal mass matrix, no inverse of operator matrix is needed. However, this fact also implies that you cannot use this method in problems having degrees of freedom with zero mass. This restriction precludes use of the Herrmann elements, gap-friction elements, the pipe bend element, shell elements 72 and 89 and beam elements 76 and 77. These shell and beam elements are precluded because they have a rotational degree of freedom, which do not have an associated mass. The mass is updated only if the LARGE STRAIN or UPDATE parameter or the CONTACT option is used. The elastomer capability can be used with explicit dynamics in an updated Lagrange framework where the pressure variables are condensed out before going into the solver.

Main Index

CHAPTER 5 173 Structural Procedure Library

Technical Background Consider the equations of motion of a structural system: Ma + Cv + Ku = F

(5-142)

where M , C , and K are mass, damping, and stiffness matrices, respectively, and a , v , u , and F are acceleration, velocity, displacement, and force vectors. Various direct integration operators can be used to integrate the equations of motion to obtain the dynamic response of the structural system. The technical background of the three direct integration operators available in Marc is described below. Newmark-beta Operator The generalized form of the Newmark-beta operator is u n + 1 = u n + Δtv n + ( 1 ⁄ 2 – β )Δt 2 a n + βΔt 2 a n + 1

(5-143)

v n + 1 = v n + ( 1 – γ )Δta n + γΔta n + 1

(5-144)

where superscript

n

denotes a value at the nth time step and u , v , and a take on their usual meanings.

The particular form of the dynamic equations corresponding to the trapezoidal rule γ = 1⁄2,

β = 1⁄4

results in n 4 4 2 ⎛ ------M + ----- C + K⎞ Δu = F n + 1 – R + M ⎛ a n + ----- v n⎞ + Cv n ⎝ ⎝ Δt 2⎠ Δt ⎠ Δt

(5-145)

where the internal force R is R =

∫ β T σdv

(5-146)

V

Equation (5-145) allows implicit solution of the system u n + 1 = u n + Δu

(5-147)

Notice that the operator matrix includes K , the tangent stiffness matrix. Hence, any nonlinearity results in a reformulation of the operator matrix. Additionally, if the time step changes, this matrix must be recalculated because the operator matrix also depends on the time step. It is possible to change the values of γ and β through the PARAMETERS option. Houbolt Operator The Houbolt operator is based on the use of a cubic fitted through three previous points and the current (unknown) in time. This results in the equations

Main Index

174 Marc Volume A: Theory and User Information

11 1 3 v n + 1 = ⎛ ------ u n + 1 – 3u n + --- u n – 1 – --- u n – 2 ⎞ ⁄ Δt ⎝6 ⎠ 3 2

(5-148)

and a n + 1 = ( 2u n + 1 – 5u n + 4u n – 1 – u n – 2 ) ⁄ Δt 2

(5-149)

Substituting this into the equation of motion results in 2 1 11 ⎛ ------M + --------- C + K⎞ Δu = F n + 1 – R n + -------- ( 3u n – 4u n – 1 + u n – 2 )M + ⎝ Δt 2⎠ 6Δt Δt 2

(5-150)

1 7 3 1 ----- ⎛⎝ --- u n – --- u n – 1 + --- u n – 2⎞⎠ C Δt 6 2 3 This equation provides an implicit solution scheme. By solving Equation (5-147) for Δu , you obtain Equation (5-151), and so obtain v

n+1

and a

n+1

.

u n + 1 = u n + Δu

(5-151)

Equation (5-150) is based on uniform time steps – errors occur when the time step is changed. Also, a special starting procedure is necessary since u

n–1

and u

n–2

appear in Equation (5-150).

Single Step Houbolt Operator The Single Step Houbolt operator according to [Ref. 29] starts with the following equilibrium equation and expressions for the velocity and acceleration: α

m1

Ma

n+1

c1

+ α Cv

n+1

+α

k1

Ku

n+1

f1 n + 1

α F u v

n

n

n+1

= v + γΔta + γ Δta

1

c

n

k

n

= (5-152)

+aF

= u + Δtv + βΔt a + β Δt a n

1

n

f n

n+1

n

2 n

m

+ α Ma + α Cv + α Ku

2 n+1

(5-153)

n+1

(5-154)

Notice that in contrast to the Newmark and the standard Houbolt method, the equilibrium equation also contains terms corresponding to the beginning of the increment. Without loss of generality, the parameter m1

can be set to 1. Based on asymptotic annihilation and second order accuracy, the remaining α parameters can be shown to fulfill:

Main Index

α

k

= 0, β = γ, β

α

c

= – ( 2β + β ) ⁄ 4β

1

1

1

= γ+γ ,α 12

,α

c1

m

= –1 ⁄ 2 , α 1

k1

= ( 2β + 3β ) ⁄ 4β

12

1

= 1 ⁄ 2β , f

k

,α = α ,α

f1

= α

k1

CHAPTER 5 175 Structural Procedure Library

In this way, the number of unknown parameters has been reduced to two. Based on a Taylor series 1

expansion of the displacement about the nth time step, β and β should be related by β + β 1

1

= 1 ⁄ 2,

1

which finally yields γ = 1 ⁄ 2 ( 1 ⁄ 2 – γ ) . According to [Ref. 29], γ should be set to 3/2 (with γ = – 1 ⁄ 2 ) to minimize the velocity error and to 1/2 (with γ = 0 ) to avoid velocity overshoot. The 1

1

default values in Marc are γ = 3 ⁄ 2 and γ = – 1 ⁄ 2 , but the user can modify γ and γ using the PARAMETERS model definition and history definition option. Substitution of the velocity and acceleration into the equilibrium equation results in: c1 1 ⎧ ⎫ α γ 1 n+1 n M + ---------------------- C + K ⎬Δu = F – Ku + ⎨ ----------------------1 2 k1 1 k1 ⎩ β Δt α ⎭ β Δtα

(5-155)

m

n 2 n n α 1 ----------------------- M { Δtv + βΔt a } – -------- Ma – 1 2 k1 k1 β Δt α α 1 c αc 1 ⎧ n n 2 ⎫⎫ n α γ ⎧ C ⎨ v + γΔta – ------------ ⎨ Δtv n + βΔt a n ⎬ ⎬ – --------- Cv -------k1 1 k1 ⎩ ⎭⎭ α α β Δt ⎩

Generalized Alpha Operator From [Ref. 36], the equilibrium equations for the generalized alpha method can be expressed in the form n+1+α

Ma

m

n+1+α

+ Cv

f

n+1+α

+ Ku

f

= F

n + 1 + αf

(5-156)

where u

n + 1 + αf n+1+α

v a

f

n + 1 + αm

= ( 1 + α f )u

n+1

– αf u n

= ( 1 + α f )v

n+1

– αf v

= ( 1 + α m )a

n+1

(5-157)

n

– αm a

(5-158) n

(5-159)

The displacement and velocity updates are identical to those of the Newmark algorithm u n + 1 = u n + Δtv n + ( 1 ⁄ 2 – β )Δt 2 a n + βΔt 2 a n + 1

(5-160)

v n + 1 = v n + ( 1 – γ )Δta n + γΔta n + 1 where, as shown in [Ref. 36], optimal values of the parameters β and γ are related to α f and α m by 2 1 β = --- ( 1 + α m – α f ) 4

Main Index

(5-161)

176 Marc Volume A: Theory and User Information

1 γ = --- + α m – α f 2

(5-162)

In Equation (5-146), α f = α m =0 gives rise to the Newmark-beta method, α m =0, – 0.33 ≤ α f < 0 gives rise to the HHT - a method [Ref. 37], and α f =0, 0 < α m ≤ 1 gives rise to the WBZ - a method [Ref. 38]. It is seen that the α f and α m parameters can be used to control the numerical dissipation of the operator. A simpler measure is the spectral radius S. This is also a measure of the numerical dissipation; a smaller spectral radius value corresponds to greater numerical dissipation. The spectral radius of the generalized alpha operator can be related to the α f and α m parameters as follows S α f = – ------------1+S

(5-163)

1 – 2S α m = ---------------1+S

(5-164)

S varies between 0 and 1. Accordingly, the ranges for the α f and α m parameters are given by – 0.5 ≤ α f ≤ 0.0 and – 0.5 ≤ α m ≤ 1 . α = -0.5, α m = -0.5 corresponds to a spectral radius of 1.0 and f α f = 0, α m = 1 corresponds to a spectral radius of 0.0. By substituting the values in equation (5-145) and comparing with Equation (5-142), it can be noted that the special case of S = 0 ( α f = 0, α m = 1) for the generalized alpha operator is identical to the default single step houbolt operator with γ

1

= 3⁄2

and γ = – 1 ⁄ 2 . It can also be noted that the case of S = 1 has no dissipation and corresponds to a midincrement Newmar- beta operator. In the Marc input file, the generalized alpha operator is flagged through the option 8 on the second field of the DYNAMIC parameter. Options to define the associated generalized alpha parameters are available through the DYNAMIC parameter and the PARAMETERS model definition and history definition option. On the DYNAMIC parameter, a default value of ‘0’ on the 8th field indicates contact-optimized parameters ( α f = 0, α m = 1) and a ‘1’ on the 8th field indicates non-contact optimized parameters ( α f = -0.05, α m = 0). ‘0’ would be recommended for dynamic contact problems or for any problem where high-frequency numerical dissipation is desired. ‘1’ would be recommended for noncontact structural dynamic problems and free-vibration problems where a small amount of numerical dissipation is desired. On the PARAMETERS, the 4th, 5th, and 6th fields of the 5th data block are reserved for α f , α m and S, respectively. S is the main control parameter : 0 ≤ S ≤ 1 indicates that Equations (5-153) and (5-154) are used to calculate α f and α m ; S = -1 indicates that α f and α m remain unchanged from previously set values; S = -2 indicates contact-optimized parameters; S = -3 indicates noncontact optimized parameters; S = -4 indicates that the 4th and 5th fields will be checked and if valid, used to set α f and α m directly.

Main Index

CHAPTER 5 177 Structural Procedure Library

Central Difference Operator The central difference operator assumes a quadratic variation in the displacement with respect to time. a n = ( v n + 1 ⁄ 2 – v n – 1 ⁄ 2 ) ⁄ ( Δt )

(5-165)

v n = ( u n + 1 ⁄ 2 – u n – 1 ⁄ 2 ) ⁄ ( Δt )

(5-166)

so that a n = ( Δu n + 1 – Δu n ) ⁄ ( Δt 2 )

(5-167)

where Δu n = u n – u n – 1

(5-168)

for IDYN=4: M M -------2- Δu n + 1 = F n – R n + -------2- Δu n Δt Δt

(5-169)

for IDYN=5: n+1 n n n M M = F – R + -------- Δu – Cv -------2- Δu 2 Δt Δt

1 n – --2

(5-170)

Since the mass matrix is diagonal, no inverse of the operator matrix is needed. Also, since the operator is only conditionally s, the critical time step is evaluated at the beginning of the analysis. For IDYN = 4, the critical time step is computed by a power sweep for the highest mode in the system only at the beginning of the analysis. For IDYN = 4, no damping is included. For IDYN = 5, an approximated method based on element geometry is used to compute the highest eigenvalue. The critical time step is calculated at a user-specified frequency or every 100 steps. The variable time step can be used only for IDYN = 5. Unless there is significant distortion in an element or material nonlinearity, the change of critical time step is not significant. Time Step Definition In a transient dynamic analysis, time step parameters are required for integration in time. The DYNAMIC CHANGE option can be used for either the modal superposition or the direct integration procedure. The AUTO STEP option can be used for the Newmark-beta, the Single Step Houbolt, and the Generalizedalpha operator to invoke the adaptive time control. Enter parameters to specify the time step size and period of time for this set of boundary conditions. When using the Newmark-beta operator, decide which frequencies are important to the response. The time step in this method should not exceed 10 percent of the period of the highest relevant frequency in the structure. Otherwise, large phase errors will occur. The phenomenon usually associated with too large a time step is strong oscillatory accelerations. With even larger time steps, the velocities start oscillating. With still larger steps, the displacement eventually oscillates. In nonlinear problems, instability usually follows oscillation. When using adaptive dynamics, you should prescribe a maximum time step.

Main Index

178 Marc Volume A: Theory and User Information

As in the Newmark-beta operator, the time step in Houbolt integration should not exceed 10 percent of the period of the highest frequency of interest. However, the Houbolt method not only causes phase errors, it also causes strong artificial damping. Therefore, high frequencies are damped out quickly and no obvious oscillations occur. It is, therefore, completely up to the engineer to determine whether the time step was adequate. For the Generalized-alpha operator, depending on the chosen parameters, the integration scheme can vary between the Newmark-beta operator and the Single-step houbolt operator. For spectral radii < 1, there is artificial damping in the system. Depending on the type of problem, the Generalized-alpha parameters and the associated time step should be carefully chosen to reduce phase errors and effects of artificial damping. In nonlinear problems, the mode shapes and frequencies are strong functions of time because of plasticity and large displacement effects, so that the above guidelines can be only a coarse approximation. To obtain a more accurate estimate, repeat the analysis with a significantly different time step (1/5 to 1/10 of the original) and compare responses. The central difference integration method is only conditionally stable; the program automatically calculates the stable time step. This step size yields accurate results for all practical problems. Initial Conditions In a transient dynamic analysis, you can specify initial conditions such as nodal displacements and/or nodal velocities. To enter initial conditions, use the following model definition options: INITIAL DISP for specified nodal displacements, and INITIAL VEL for specified nodal velocities. As an alternative, you can use the USINC user subroutine.

Dynam ics

Time-Dependent Boundary Conditions Simple time-dependent load or displacement histories can be entered on data blocks. However, in general cases with complex load histories, it is often more convenient to enter the history through a user subroutine. Marc allows the use of the FORCDT and FORCEM user subroutines for boundary conditions. the FORCDT user subroutine allows you to specify the time-dependent incremental point loads and incremental displacements. The FORCEM user subroutine allows you to specify the time-dependent magnitude of the distributed load. Mass Matrix The mass matrix is a discrete representation of the system mass. System mass can be defined through either distributed masses and concentrated masses. Distributed masses are defined for elements through the mass density material property. Marc offers both consistent and lumped element mass matrices. The consistent mass matrix is given by [m] =

∫ ρ[N]

T

[ N ] dV

where ρ is the mass density and [ N ] is the shape function matrix. The lumped mass matrix is flagged through the LUMP parameter. Marc uses the Hinton, Rock, Zienkiewicz lumping scheme to produce a diagonal mass matrix. The salient features of this scheme are as follows: The diagonal coefficients of the consistent mass matrix are computed. The total mass of the element m is also computed. A scale

Main Index

CHAPTER 5 179 Structural Procedure Library

factor s is computed by adding the translational diagonal coefficients that are mutually parallel and in the same direction. All diagonal coefficients are then scaled by m ⁄ s , thereby preserving the total mass of the element. Concentrated masses are defined through the MASSES, CONM1, and/or CONM2 model definition options. The MASSES option allows the placement of particle masses m i at degree of freedom of i at specific nodes. Both translational and rotary masses are allowed. The CONM1 option allows the specification of a diagonal or 6 x 6 symmetric mass matrix at a node in the global cartesian or in a local coordinate system. The local system is specified through a coordinate system ID. The fully coupled 3-D form is given below

M 11 …

[ m conm1 ] =

…

…

M 21 M 22 … sym M 31 M 32 M 33 … M 41 M 42 M 43 M 44

…

…

…

…

…

…

…

…

M 51 M 52 M 53 M 54 M 55 … M 61 M 62 M 63 M 64 M 65 M 66 Each mass term can be varied using tables. Independent variables allowed include time, increment number, coordinates, temperature. When the diagonal form is specified, only the M 11 to M 66 diagonal terms need to be specified. In 2-D, the mass matrix reduces to 3 x 3 and only the M 11 , M 12 …M 33 terms need to be specified. If the CONM1 mass matrix is specified in a local system, then it is transformed to the global system before assembly. The CONM2 option allows a concentrated diagonal mass and the mass moments of inertia with respect to the global cartesian or a local coordinate system. The local system is specified through a coordinate system ID. The mass terms for each degree of freedom at the node are a function of the concentrated mass, the moments of inertia and the distance of the center of mass from the node. The offset distance from the node to the center of mass is given by the vector { V 1 V 2 V 3 } . The 3-D form of the CONM2 matrix is given below:

Main Index

180 Marc Volume A: Theory and User Information

… M 0

M 0 0 [ m conm2 ] =

0

… … M

… … … sym … … … … … a

– MV 3 MV 2

MV 3

0

– MV 2 MV 1

I 11

… …

a

a

a

a

– MV 1 I 21 I 22 … 0

a

I 31 I 32 I 33

where the combined moments of inertia are given as follows: a

2

2

a

2

2

a

2

2

I 11 = I 11 + M ( V 2 + V 3 ) ; I 22 = I 22 + M ( V 1 + V 3 ) ; I 33 = I 33 + M ( V 1 + V 2 ) ; a

a

a

I 21 = – I 21 – MV 1 V 2 ; I 31 = – I 31 – MV 1 V 3 ; I 32 = – I 32 – MV 2 V 3 Each mass coefficient can be varied using tables. Independent variables allowed include time, increment number, coordinates, temperature. In 2-D, the mass matrix reduces to 3 x 3 and only M , I 33 , V 1 , and V 2 are required. If the CONM2 mass matrix is specified in a local system, then it is converted to the global system before assembly. Damping In a transient dynamic analysis, damping represents the dissipation of energy in the structural system. It also retards the response of the structural system. Marc allows you to enter two types of damping in a transient dynamic analysis: modal damping and Rayleigh damping. Use modal damping for the modal superposition method and Rayleigh damping for the direct integration method. For modal superposition, you can include damping associated with each mode. To do this, use the DAMPING option to enter the fraction of critical damping to be used with each mode. During time integration, Marc associates the corresponding damping fraction with each mode. The program bases integration on the usual assumption that the damping matrix of the system is a linear combination of the mass and stiffness matrices, so that damping does not change the modes of the system. For direct integration damping, you can specify the damping matrix as a linear combination of the mass and stiffness matrices of the system. You can specify damping coefficients on an element basis. Stiffness damping should not be applied to either Herrmann elements or gap elements because of the presence of Lagrangian multipliers. Numerical damping is used to damp out unwanted high-frequency chatter in the structure. If the time step is decreased (stiffness damping might cause too much damping), use the numerical damping option to make the damping (stiffness) coefficient proportional to the time step. Thus, if the time step decreases,

Main Index

CHAPTER 5 181 Structural Procedure Library

high-frequency response can still be accurately represented. This type of damping is particularly useful in problems where the characteristics of the model and/or the response change strongly during analysis (for example, problems involving opening or closing gaps). Element damping uses coefficients on the element matrices and is represented by the equation: n

C =

⎧ Δt⎞ ⎫ ⎛ - K ⎨ α i M i + ⎝ β i + γ i ---π ⎠ i ⎬⎭ 1⎩

∑

i =

(5-171)

where C

is the global damping matrix

Mi

is the mass matrix of ith element

Ki

is the stiffness matrix of the ith element

αi

is the mass damping coefficient on the ith element

βi

is the usual stiffness damping coefficient on the ith element

γi

is the numerical damping coefficient on the ith element

Δt

is the time increment

If the same damping coefficients are used throughout the structure, Equation (5-171) is equivalent to Rayleigh damping. The damping associated with springs and mass points can be controlled via the springs and masses input options. The damping on elastic foundations is the same as the damping on the element on which the foundation is applied. For springs, a dashpot can be added for nonlinear analysis.

Harmonic Response Harmonic response analysis allows you to analyze structures vibrating around an equilibrium state. This equilibrium state can be unstressed or statically prestressed. Statically prestressed equilibrium states can include material and/or geometric nonlinearities. You can compute the damped response for prestressed structures at various states. In many practical applications, components are dynamically excited. These dynamic excitations are often harmonic and usually cause only small amplitude vibrations. Marc linearizes the problem around the equilibrium state. If the equilibrium state is a nonlinear, statically prestressed situation, Marc considers all effects of the nonlinear deformation on the dynamic solution. These effects include the following: • initial stress • change of geometry • influence on constitutive law

Main Index

182 Marc Volume A: Theory and User Information

The vibration problem can be solved as a linear problem using complex arithmetic. The analytical procedure consists of the following steps: where De l

are element damping matrices

Dd

are damper contributions

α

mass damping coefficient

β

stiffness damping coefficient

γ

numerical damping coefficient

i

=

ω

= excitation frequencies

u

= u r e + iu i m complex response vector

P

= P re + iP i m complex load vector

–1

If all external loads and forced displacements are in phase and the system is undamped, this equation reduces to ( K – ω 2 M )u r e = P r e

(5-172)

which could be solved without activating the complex arithmetic on the HARMONIC parameter. The values of the damping coefficients ( α , β , γ ) are entered via the DAMPING model definition option. The spring and damper contributions are entered in either the SPRINGS, PFAST, or PBUSH model definition options and mass points are specified in the MASSES, CONM1, or CONM2 model definition options. The element damping matrix ( D e l ) can be obtained for any material with the use of a material damping matrix which is specified in the UCOMPL user subroutine. You specify the material response with the constitutive equation. · σ = Bε + Cε

(5-173)

where B and C can be functions of deformation and/or frequency. The global damping matrix is formed by the integrated triple product. The following equation is used: D =

∑ ∫ el

v

T

β C dV e l

el

where β is the strain-displacement relation.

Main Index

(5-174)

CHAPTER 5 183 Structural Procedure Library

Similarly, the stiffness matrix K is based on the elastic material matrix B . The program calculates the response of the system by solving the complex equations: [ K + iωD – ω 2 M ]u = P

(5-175)

where u now is the complex response vector u = u r e + iu i m

(5-176)

A special application of the harmonic excitation capability involves the use of the elastomeric analysis capability in Marc. Here, the Mooney formulation (used in conjunction with the various Herrmann elements) is used to model the stress-strain behavior of the elastomeric compound. In Marc, the behavior is derived from the third order invariant form of the strain energy density function. W ( I 1, I 2 ) = 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

(5-177)

with the incompressibility constraint (5-178)

I3 = 1

where I 1 , I 2 , and I 3 are the invariants of the deformation. For the harmonic excitation, the constitutive equation has the specific form ΔS i j = [ D i j k l + 2iωφ i j k l ]ΔE k l

(5-179)

with D i j k l as the quasi-static moduli following form the Mooney strain energy density function and φ i j k l = φ 0 [ C i–k1 C j–l1 + C i–l1 C j–k1 ] + φ 1 [ δ i k C j–l1 + C i–l1 δ j k ] + φ 2 [ C i k C j–l1 + C i–l1 C j k ] + φ 0 δ i j C k–l1 + φ 11 δ i j δ k l + φ 12 δ i j C k l + φ 20 C i j C k–l1 + φ 21 C i j δ k l + φ 22 C i j C k l

(5-180)

The output of Marc consists of stresses, strains, displacements and reaction forces, all of which may be complex quantities. The strains are given by ε = β u

(5-181)

and the stresses by · σ = Bε + C ε

(5-182)

The reaction forces are calculated with R = Ku – ω 2 Mu + iωΣD e l u + iωΣD d u 2

where – ω Mu is only included if requested on the HARMONIC parameter.

Main Index

(5-183)

184 Marc Volume A: Theory and User Information

The printout of the nodal values consists of the real and imaginary parts of the complex values, but you can request that the amplitude and phase angle be printed. You do this with the PRINT CHOICE model definition option.

Spectrum Response The spectrum response capability allows you to obtain maximum response of a structure subjected to known spectral base excitation response. This is of particular importance in earthquake analysis and random vibration studies. You can use the spectrum response option at any point in a nonlinear analysis and, therefore, ascertain the influence of material nonlinearity or initial stress. The spectrum response capability technique operates on the eigenmodes previously extracted to obtain the maximum nodal displacements, velocities, accelerations, and reaction forces. You can choose a subset of the total modes extracted by either specifying the lowest n modes or by selecting a range of frequencies. Enter the displacement response spectrum S D ( ω ) for a particular digitized value of damping through the USSD user subroutine. Marc performs the spectrum analysis based on the latest set of modes extracted. The program lumps the mass matrix to produce M . It then obtains the projection of the inertia forces onto the mode φ j Pj = M φj

(5-184)

The spectral displacement response for the jth mode is αj = SD ( ωj ) Pj

(5-185)

Marc then calculates the square roots of the sum of the squares as u =

∑ ( αjφj ) 2

1⁄2

DISPLACEMENT

(5-186)

VELOCITY

(5-187)

ACCELERATION

(5-188)

FORCE

(5-189)

j

v =

∑ ( αj ω j φj ) 2

1⁄2

j

a =

∑ ( αj ωj φj ) 2

1⁄2

j

f =

∑ ( α j ω j2 Mφ j ) 2

1⁄2

j

The internal forces given by Equation 5-189 are identified as reaction forces on the post file. The force transmitted by the structure to the supporting medium (also referred to as base shear) is only reported in the out file and is given by

Main Index

CHAPTER 5 185 Structural Procedure Library

tf =

2

∑ S D ( ω j )ωj2 P j

TRANSMITTED FORCE

(5-190)

j

Inertia Relief Inertia relief refers to an analysis procedure that allows unconstrained systems to be subjected to a quasistatic analysis by taking rigid body inertia forces into account. Examples of such systems include an aircraft in a steady turn, an underwater structure in equilibrium under gravity and buoyancy. Conventional static analysis cannot be performed for such systems since, in the absence of constraints, the stiffness matrix is singular. Inertia relief analysis is applicable to such free bodies. The response is measured relative to a steady accelerating frame induced by the external loads. Two important steps are followed by the solver in an analysis with inertia relief: 1. Rigid Body Mode evaluation: This is the central step in an inertia relief analysis since the rigid body modes are extensively used in the load computations. The Support Method is currently provided in Marc to evaluate the rigid body modes. 2. Inertia Relief Loads evaluation: The loads associated with the rigid body motion of the system are calculated using the rigid body modes and the global lumped mass matrix. The loads are calculated such that they balance the current external load vector in the system. Next, more details on each of the steps are provided.

Rigid Body Mode Evaluation Support Method The Support Method requires the manual specification of nodal degrees of freedom which can be used to evaluate the rigid body modes of the system. Any number of nodal entries can be provided, each with degrees of freedom ranging from 1 to the maximum possible degrees of freedom at each node. These degrees of freedom are referred to as the r-degrees of freedom set. It is the user’s responsibility to ensure that the r-degrees of freedom set is necessary and sufficient to evaluate the rigid body modes of the system. The rigid body modes are evaluated by sequentially setting each r-degrees of freedom to 1 with all other r-degrees of freedom set to 0 and solving for the system of equations [ Kl l ] [ Kl r ] ⎧ [ φl ] ⎫ ⎨ ⎬ = 0 [ K r l ] [ K rr ] ⎩ [ I ] ⎭

(5-191)

where [ I ] is the identity matrix for the r-degrees of freedom and [ φ l ] are the modal amplitudes for the remaining degrees of freedom. Once the rigid body modes are evaluated, the r-degrees of freedom are set to 0 and used as fixed displacement constraints. Other displacement boundary conditions, specified through normal options like FIXED DISP, DISP CHANGE, etc. can be used in conjunction with the rigid body degrees of freedom constraints.

Main Index

186 Marc Volume A: Theory and User Information

The Support Method is computationally inexpensive since the provided Support degrees of freedom are automatically constrained and no additional ties/constraints are needed while calculating the response. It is available for single-processor and multi-processor runs (both single-input and multi-input file formats). The Support Method requires manual input to evaluate the rigid body modes of the system. For direct solvers, the rigid body modes are calculated through repeated back-solves of the factorized matrix. The computation of rigid body modes is more expensive for the conjugate gradient iterative solver. Finally, the Support Method cannot be used in contact problems with dynamically changing rigid body modes. Rigid Body Mode Update In a small displacement analysis, the rigid body modes are evaluated at the first cycle of the first increment of the inertia relief loadcase and are retained through the loadcase. In a large displacement analysis, the rigid body modes are updated at the beginning of each increment by using the current stiffness matrix while solving Equation (5-191). Inertia Relief Loads Evaluation A general derivation for the inertia relief load vector in a nonlinear analysis is presented here. At the i th iteration of the ( n + 1 ) th increment, the total response is given by { u tn, i+ 1 } = { u rn } + { Δu rn, +i –1 1 } + { δu rn, +i 1 } + { u n } + { Δu in–+11 } + { δu in + 1 }

(5-192)

where { u t } is the total response, { u r } is the rigid body response and { u } is the flexible response. Neglecting accelerations associated with the flexible response, the governing equations are given as n+1

n+1

n+1

n+1

[ M i – 1 ] { δu·· r, i } + [ K i – 1 ] { δu i n+1

n+1

n+1

} = { P n + 1 } – { I i – 1 } – { P φ, i – 1 }

(5-193)

n+1

where [ M i – 1 ] and [ K i – 1 ] are the mass and stiffness matrices at the ( i – 1 ) th iteration of ( n + 1 ) th n+1

n+1

increment, { P n + 1 } is the external load vector at the ( n + 1 ) th increment, I i – 1 and { P φ, i – 1 } are the internal load vector and the inertia relief load vector at the ( i – 1 ) th iteration of the ( n + 1 ) th increment, respectively. The change in the rigid body acceleration is computed as follows: { δu·· rn, +i 1 } = [ Φ in–+11 ] { δA φn, +i 1 }

(5-194)

where [ Φ in–+11 ] is the matrix of rigid body modes at the ( i – 1 ) th iteration of the ( n + 1 ) th increment n+1

and { δA φ, i } represents the iterative change in the modal acceleration vector. n+1

Pre-multiplying Equation 5-184 by individual rigid body modes, { φ k, i – 1 } T , and using the fact that the work done by the rigid body modes is 0, one gets

Main Index

CHAPTER 5 187 Structural Procedure Library

n+1

n+1

n+1

[ C i – 1 ] { δA φ, i } = { δR i

}

(5-195)

n+1

where the kl th term of matrix [ C i – 1 ] is given by n+1

n+1

n+1

n+1

C i – 1, k l = { φ k, i – 1 } T [ M i – 1 ] { φ l, i – 1 } n+1

and the k th term of { δR i n+1

δR i, k

n+1

T

= { φ k, i – 1 } [ { P

} is given by

n+1

n+1

n+1

} – { I i – 1 } – { P φ, i – 1 } ]

(5-196) n+1

Note that if the rigid body modes are mass ortho-normalized, matrix [ C i – 1 ] is an identity matrix. n+1

Solving Equation (5-195) for { δA φ, i } , the iterative change in the inertia relief load vector is given by n+1

n+1

n+1

n+1

{ δP φ, i } = [ M i – 1 ] [ Φ i – 1 ] { δA φ, i }

(5-197)

The governing equations in Equation 5-184 can then be rewritten in the form, n+1

n+1

[ K i – 1 ] { δu i

n+1

} = { Pi

n+1

n+1

} – { I i – 1 } – { P φ, i } n+1

where the inertia relief load vector at the i th iteration of the ( n + 1 ) th increment, { P φ, i } , is given by n+1

n+1

n+1

{ P φ, i } = { P φ, i – 1 } + { δP φ, i } Additional items to be kept in consideration for inertia relief analysis in Marc are as follows: Convergence Checking For systems that are unconstrained or just constrained against rigid body motion (statically determinate structures), the reaction forces at nodes are 0 or very close to 0. In this case, using relative residual force checking may lead to unnecessary recycling and possible non-convergence. It would be more appropriate to use displacement checking or absolute residual force checking in such situations. Time Stepping Inertia relief can be used in conjunction with all time stepping procedures used for static analyses. Time step cutback schemes are supported. Inputs specified in either table or non-table formats are also supported.

Main Index

188 Marc Volume A: Theory and User Information

Parallel Processing The Support Method is available for serial and parallel runs. For the multi-input file parallel mode, the Support nodes should be available in all the domains. For the single-input file parallel mode, the inertia relief option should be present in the model definition section itself in order to allow the Support nodes to be added to domains they are not naturally present in. Deactivating Inertia Relief When inertia relief is active during an analysis, and is subsequently turned off, the user has three choices for treating the pre-existing inertia relief load vector. 1. The inertia relief load vector can be retained. No new inertia relief loads are computed, but preexisting inertia relief loads are included in the right-hand side. 2. The inertia relief load vector can be removed instantaneously. Note that this is the option used by Marc if the INERTIA RELIEF option is present in one loadcase and is absent in the next loadcase. This could lead to convergence difficulties at the beginning of the second loadcase due to the large change in load vectors. 3. The inertia relief load vector can be removed gradually. This allows the inertia relief load vector to be removed over the course of the second loadcase. Inertia Relief Ouput Options The nodal inertia relief load and moment vectors are written to the post file by default using nodal post codes 51 and 52, respectively. It should be noted that the inertia relief loads are always written out in the global cartesian system. Also, the command INER can be used on the PRINT NODE option to obtain the inertia relief loads at a particular node. Also, when the NO PRINT option is revoked, a summary of the total inertia relief load is printed in the out file. Limitations for Inertia Relief Analyses 1. All inertia relief analyses provide the uninteresting solution of zero displacements when a uniform mesh is subjected to uniform gravity loads or when a uniform shell mesh is subjected to uniform distributed loads. This is as expected because the inertia relief equations place an inertia load on each node that is equal and opposite to the external load. 2. The Support Method is currently not supported for the CASI iterative solver. 3. The Support Method is capable of dealing with material and geometric non-linearities. However, boundary condition non-linearities like contact between multiple bodies cause the number of rigid body modes to change in the system. These require relative rigid body positions of the bodies to be continuously updated. These cannot be handled by the Support Method.

Rigid-Plastic Flow The rigid-plastic flow analysis is an approach to large deformation analysis which can be used for metal forming problems. Two formulations are available: an Eulerian (steady state) and Lagrangian (transient) approach. The effects of elasticity are not included. If these effects are important, this option should not be used.

Main Index

CHAPTER 5 189 Structural Procedure Library

In the steady state approach, the velocity field (and stress field) is obtained as the solution of a steadystate flow analysis. The time period is considered as 1.0 and, hence, the velocity is equal to the deformation. In the transient formulation, the incremental displacement is calculated. The R-P FLOW parameter invokes the rigid-plastic procedure. This procedure needs to enforce the incompressibility condition, which is inherent to the strictly plastic type of material response being considered. Incompressibility can be imposed in three ways: 1. by means of Lagrange multipliers. Such procedure requires Herrmann elements which have a pressure variable as the Lagrange multiplier. 2. by means of penalty functions. This procedure uses regular solid elements, and adds penalty terms to any volumetric strain rate that develops. It is highly recommended that the constant dilatation formulation be used – by entering a nonzero value in the second field of the GEOMETRY model definition option. Penalty factor can be treated as constant or variable through the R-P FLOW parameter. The penalty value is entered through the PARAMETERS option. 3. In plane stress analysis (shell and membrane elements), the incompressibility constraint is satisfied exactly by updating the thickness. This capability is not available for steady state analysis. In R-P flow analysis, several iterations are required at any given increment, the greatest number occurring in the first increment. Subsequent increments require fewer iterations, since the initial iteration can make use of the solution from the previous increment. Due to the simplicity of the rigid-plastic formulation, it is possible to bypass stress recovery for all iterations but the last in each increment, provided that displacement control is used. In such cases, considerable savings in execution time are achieved. If nodal based friction is used in a contact analysis, then a stress recovery is always performed after each iteration.

Steady State Analysis The steady state R-P flow formulation is based on an Eulerian reference system. For problems in which a steady-state solution is not appropriate, an alternative method is available to update the coordinates. The UPNOD user subroutine is used to update the nodal coordinates at the end of a step according to the relationship. n

x in = x in – 1 + v Δt

(5-198)

where n refers to the step number, v n is the nodal velocity components, and Δt is an arbitrary time step. Δt is selected in such a way as to allow only a reasonable change in mesh shape while ensuring stability with each step. Updating the mesh requires judicious selection of a time step. This requires some knowledge of the magnitude of the nodal velocities that will be encountered. The time step should be selected such that the strain increment is never more than one percent for any given increment.

Main Index

190 Marc Volume A: Theory and User Information

The quantities under the title of ENGSTN in the printouts actually refer to the strain rate at an element integration point. The reaction forces output by the program gives the limit loads on the structure.

Transient Analysis In the transient procedure, there is an automatic updating of the mesh at the end of each increment. During the analysis, the updated mesh can exhibit severe distortion and the solution might be unable to converge. Global adaptive meshing or manual mesh rezoning can be used to overcome this difficulty.

Technical Background The rigid-plastic flow capability is based on iteration for the velocity field in an incompressible, nonNewtonian fluid. The normal flow condition for a nonzero strain rate can be expressed as: ⎛ 2 σ⎞ · · · σ′ i j = ⎜ --- --·-⎟ ε i j = μ ( ε ) ε i j ⎝ 3 ε⎠

(5-199)

where · ε =

2· · --- ε i j ε i j 3

(5-200)

is the equivalent strain rate, σ is the yield stress (which may be rate-dependent) and 1 σ′ i j = σ i j – --- δ i j σ k k 3

(5-201)

gives the deviatoric stress. The effective viscosity is evaluated as: 2 σ μ = --- --·3 ε

(5-202)

· Note that as ε → 0, μ → ∞ . A cutoff value of strain rate is used in the program to avoid this difficulty. · An initial value for ε is necessary to start the iterations. These values can be specified in the PARAMETERS option. The default cut-off value is 10 – 6 , and the default initial strain rate value is 10-4.

The value of the flow stress is dependent upon both the equivalent strain, the equivalent strain rate, and the temperature. This dependence can be given through the WORK HARD, STRAIN RATE, TEMPERATURE EFFECTS, or TABLE options, respectively. For steady state analysis, the UNEWTN user subroutine can be used to define a viscosity. In this manner, a non-Newtonian flow analysis can be performed. For the transient procedure, the URPFLO user subroutine can be used to define the flow stress.

Main Index

CHAPTER 5 191 Structural Procedure Library

Superplasticity Superplasticity is the ability of a material to undergo extensive deformation such as strains of 1000% without necking. Superplastic behavior has been reported in numerous metal, alloys and ceramics. Every instance of superplasticity is associated with: (1) A fine grain size ( 1 – 10 μm ), (2) deformation temperatures > 0.4T m , and (3) a strain-rate sensitivity factor m > 0.3 . Using finite element analysis to simulate superplastic fabrication of complex parts used in the aerospace and automotive industries requires this material behavior and contact with friction. Furthermore, the process pressure needs to be automatically adjusted to keep the material within a target strain rate. The simulation can be used to predict thinning, forming time, areas of void formation, and can ultimately be employed in shape optimization; thus, reducing the number of prototypes of forming trials required to product an acceptable part. Three mechanisms have been proposed to account for the high strain-rate sensitivity found in superplastic materials: (1) Vacancy creep, (2) creep by grain boundary diffusion, and (3) grain boundary sliding. According to Ghosh and Hamilton, the strain-rate sensitivity of metals arises from the viscous nature of the deformation process. The viscosity is a result of the resistance offered by internal obstacles within the material. In dislocation glide and climb processes, the obstacles are a fine dispersion of second phase particles within the grain interior, between which the dislocations are bent around and moved. At high homologous temperatures ( T > 0.4T m ; where T m is the melting temperature), the high diffusivities around grain boundary regions can lead to grain boundary sliding. The overall rate sensitivity of a material is then a result of the rate sensitivities of the grain boundary and the grain interior. The more the material behaves as a viscous liquid, the greater its superplasticity. The superplastic behavior is characterized by the dependence of the flow stress upon the strain-rate, which is usually depicted by the logarithmic relationship shown in Figure 5-30. As indicated in Figure 5-30, the stress-strain rate behavior of a superplastic material can be divided into three regions. Values of strain-rate sensitivity, m (the slope of flow stress versus strain-rate curve) which is a measure of resistance to localized necking, are relatively low in both the low stress-low strain rate region I and the high stress-high strain rate region III and superplasticity is not manifested. Rather, superplasticity is found only in region II, a transition region in which stress increases rapidly with increasing strain-rate. As temperature increases and/or grain size decreases, region II is displaced to higher strain-rates. Moreover, the maximum observed values of m increase with similar changes in these parameters. Certainly the forming process innovations evoked will need to be carefully studied and developed. Forming times are slow, and there will be a critical need for optimizing forming pressures, stress strainrate and deflection in sheet forming. Based on the schematic flow stress-strain rate relationships given above, it is apparent that high values of m are requisite for superplastic materials. Since, for a given material and forming temperature, m , usually varies with strain-rate, it is desirable to control strain-rate during forming so that optimum or at least adequate strain-rate sensitivity is exhibited. Ductility is also dependent upon forming temperature, which must lie within a narrow range. If forming temperatures and

Main Index

192 Marc Volume A: Theory and User Information

pressure cycle are optimum, then unlike conventional ductile materials, superplastic materials are much less susceptible to localized necking. Additionally, under such conditions, the flow stress occurring during forming is much lower than the mechanical yield stress. (a) Flow Stress

Region III ln σ Region II

Region I

Decreasing grain size or increasing temperature

.

ln ε (b) Strain-rate Sensitivity d ln σ m ⎛ = ------------·-⎞ ⎝ ⎠ d ln ε

Decreasing grain size or increasing temperature Region I Region II Region III

.

ln ε Figure 5-30 Function of Strain-rate

Thus, the superplastic materials may be viewed as exhibiting time-dependent inelastic behavior with the yield stress as a function of time, temperature, strain-rate, total stress and total strain. Typical materials used in commercial superplastic forming applications include Ti-6A1-4V titanium alloy and 5083 aluminium alloy. The form of constitutive equation used to simulate superplasticity is given as: ·m σy = ε

(5-203)

The form in Equation (5-203) can be recovered by using appropriate constants in the ISOTROPIC model definition option to define power law or rate power law. Thus,

Main Index

Power Law Model:

·n m σ y = A ( ε o + ε ) + Bε

(5-204)

Rate Power Law Model:

m ·n σ y = Aε ε + B

(5-205)

CHAPTER 5 193 Structural Procedure Library

The superplastic forming process requires the use of the SPFLOW parameter. The use of this parameter automatically activates the FOLLOW FOR and PROCESSOR parameters. The process parameters are controlled by the use of the SUPERPLASTIC history definition option. Typical outputs that are available from the superplastic forming simulation are the thickness distribution for the part, the equivalent plastic strain rate, and the history of the process pressure. The process pressure is automatically calculated during the analysis. The pressure magnitude is adjusted such that the equivalent strain rate in the part is at or close to the user-specified target strain rate. The equivalent strain rate in the part is an average value calculated by sampling a suitable subset of elements. The recommended scheme is one in which elements with a strain rate greater than a cut-off factor times the maximum element strain rate are sampled. This maximum strain rate is based on a smoothing algorithm described below. The cut-off factor can vary between 0 (all elements below the maximum are sampled) and 1 (only the elements with maximum strain rate are sampled). The recommended value for the cut-off factor is 0.7 to 0.9 (default value is 0.8). To reduce undesirable oscillations in the pressuretime history, a pressure smoothing algorithm is incorporated. The basis for this algorithm is a smoothing of the maximum strain rate in the mesh based on the fact that the maximum strain rate should be typically representative of a few elements in the mesh, rather than an isolated individual value. The peak strain rates in a few elements are calculated. The number of elements that are used in this calculation varies with the cut-off factor (for a cut-off factor of 1, only 1 element is used; for the default of 0.8, 10 elements are used; for a cut-off factor of 0, 50 elements are used). The strain rate values are successively disregarded in descending order if the difference from the highest strain rate to the lowest differs by more than 10 percent from the mean. The value of the cut-off factor has significant influence on the maximum strain rate control and on the smoothness of the pressure-time curve. Larger the factor (that is, 0.9 or higher) provides more control on the maximum strain rate, but may potentially cause oscillations in the pressure history. Smaller the factor (that is, 0.7 or lower) provides less control on the maximum strain rate, but causes smoother pressuretime curves. The default of 0.8 should work in most cases - in situations where physically realistic localized strain rates occur and one desires good control on these localized values, a higher value could be used.

Soil Analysis This section has the solution procedure for fluid-soil analysis. In the current formulation, it is assumed that the fluid is of a single phase, and only slightly compressible. This formulation will not be adequate if steam-fluid-solid analysis is required. The dry soil can be modeled using one of the three models: linear elasticity, nonlinear elasticity and the modified Cam-Clay model. There are three types of soil analysis available in Marc. In the first type, you perform an analysis to calculate the fluid pressure in a porous medium. In such analyses, heat transfer elements 41, 42, or 44 are used. The SOIL model definition option is used to define the permeability of the solid and the bulk modulus and dynamic viscosity of the fluid. The porosity is given either through the INITIAL POROSITY or the INITIAL VOID RATIO options and does not change with time. The prescribed pressures can be defined using the FIXED PRESSURE option, while input mass flow rates are given using either the POINT FLUX or DIST FLUXES option.

Main Index

194 Marc Volume A: Theory and User Information

5

In the third type of soil analysis, a fully-coupled approach is used. Element types 32, 33, or 35 are available. These elements are “Herrmann” elements, which are conventionally used for incompressible analysis. In this case, the extra variable represents the fluid pressure. The SOIL option is now used to define both the soil and fluid properties. The porosity is given through the INITIAL POROSITY or the INITIAL VOID RATIO option. The prescribed nodal loads and mass flow rates are given through the POINT LOAD option, while distributed loads and distributed mass flow rates are given through the DIST LOADS option. The FIXED DISP option is used to prescribe either nodal displacements or pore pressures.

Struct Technical Formulation ural In soil mechanics, it is convenient to decompose the total stress σ into a pore pressure component p and Proce the deviatoric or effective stress σ d . dure σ = σ d – pI (5-206) Librar Note the sign convention used; a positive pore pressure results in a compressive stress. The momentum y balance (equilibrium) equations are with respect to the total stresses in the system. ∇σ + f = ρu··

(5-207)

where ρ is the density, and f , u·· are the body force and the acceleration. The equilibrium equation can then be expressed as ∇σ d – ∇p + f = ρu··

(5-208)

The fluid flow behavior can be modeled using D’Arcy’s law, which states that the fluid’s velocity, relative to the soil’s skeleton, is proportional to the total pressure gradient. –K u· f = ------- ( ∇p + ρ f g ) μ

(5-209)

where u· f

is the fluid’s bulk velocity

K

is the soil permeability

μ

is the fluid viscosity

ρf

is the fluid density

g

is the gravity vector.

The fluid is assumed to be slightly compressible. · ρf p· = K ----f ρf

Main Index

(5-210)

CHAPTER 5 195 Structural Procedure Library

where K f is the bulk modulus of the fluid. However, the compressibility is assumed small enough such that the following holds: K K ∇ ⋅ ρ f ---- ( ∇p + ρ f g ) ≈ ρ f ∇ ⋅ ---- ( ∇p + ρ f g ) μ μ

(5-211)

It is also assumed that the bulk modulus of the fluid is constant, introducing the fluid’s compressibility β f . βf = 1 ⁄ Kf

(5-212)

The solid grains are assumed to be incompressible. Under these assumptions, the governing equations for fluid flow is K ∇ ⋅ ---- ( ∇p + ρ f g ) μ

· = φβ f p + ∇u·

(5-213)

where σ is the medium’s porosity. It is important to note that the medium’s porosity is only dependent upon the original porosity and the total strains. Letting V f and V s stand for the fluid and solid’s volume φ = dV f ⁄ ( dV f + dV s ) = 1 – J – 1 ( 1 – φ 0 )

(5-214)

where J is the determinant of the deformation gradient and φ 0 is the original porosity, both with respect to the reference configuration. Introducing the weighting function η u and η p , the weak form, which is the basis for the finite element system, then becomes

∫ Vn + 1

[ η u f – ρη u u·· – ∇η u σ + ∇η u p ]dv +

∫ ηu

t dA = 0

(5-215)

A

where V and A are the conventional volumes and surface area and t is the applied tractions. Note that the applied tractions is the combined tractions from both the effective stress σ d and the pore pressure p . and

∫ V

Main Index

n+1

K ∇η p ---- ( ∇p + ρ f g ) + φβ f η p p· + η p ( ∇u· ) dv – μ

∫ A

n+1

η p q n dA = 0

(5-216)

196 Marc Volume A: Theory and User Information

where the normal volumetric inflow, q n , is: k q n = --- ( ∇p + ρ f g ) ⋅ n μ

(5-217)

The weak form of equilibrium can be written as:

∫

ru = V

[∇

η u p ] dv

(5-218)

⋅

(5-219)

n+1

∫

rp =

⋅

∇η p

Vn + 1

K ---- ( ∇p + ρ f g ) + φβ f η p p· + η p ∇ ⋅ u· dv μ

Application of the directional derivative formula yields: D u ( r u ) ⋅ δu =

d ------ r u ( u + εδu ) dε

(5-220)

ε = 0

Hence,

∫

D u ( r u ) ⋅ δu =

[∇

⋅

Δu ( ∇

⋅

η u p ) + ∇η u

T

⋅

∇Δup ] dv

(5-221)

Vn + 1

Similarly,

∫

D p ( r u ) ⋅ δp =

∇

⋅

η u Δp dv

(5-222)

Vn + 1

∫

D u ( r p ) ⋅ δu = V

n+1

⋅

⎧ ⎨ ∇η p ⎩

K ---- ( ∇p + ρ f g ) + φβ f η p p· + η p ∇ μ

∫ Vn + 1

Main Index

u· ∇

⋅

T Δu – η p ∇u·

⋅ (5-223)

∇Δu + η p ∇ ⋅ Δu· – ∇Δu∇η p D p ( r p ) ⋅ δp =

⋅

∇η p

⋅

⋅

K ---- ( ∇p + ρ f g ) – ∇η p μ

K ---- ∇Δp + φβ f η p Δp· dv μ

⋅

K ---- ( ∇Δu )∇p }dv μ (5-224)

CHAPTER 5 197 Structural Procedure Library

with the displacement and pressures interpolated independently as: Δu =

∑ N i Δu i

and

(5-225) p =

∑ Nj pj

we get a linearized system of equilibrium equation, In the second type of soil analysis, the pore (fluid) pressure is directly defined, and the structural analysis is performed. Element types 27, 28, or 21 are available. In such analyses, the pore pressure is prescribed using the INITIAL PORE and CHANGE PORE options. The characteristics of the soil material are defined using the SOIL option. If an elastic model is used, the Young’s moduli and Poison’s ratio are important. If the Cam-Clay model is used, the compression ratios and the slope of the critical state line is important. For the Cam-Clay model, the preconsolidation pressure is defined using the INITIAL PC option. For this model, it is also important to define an initial (compressive stress) to ensure a stable model. K u u K u p ⎧ δu ⎫ ⎧ Ru ⎫ ⎨ ⎬ = F–⎨ ⎬ K p u K p p ⎩ δp ⎭ ⎩ Rp ⎭

(5-226)

The resulting system of equations is highly nonlinear and nonsymmetric, and is solved by full NewtonRaphson solution scheme. Note that it is assumed that the permeability, porosity, viscosity, and the bulk modulus of the fluid are considered independent of the state variables u and p . It is evident that, in general, this is not the case; however, in the analysis that follows, these dependencies are ignored for tangent purposes. Note that they are included in the calculation of the residuals R u and R p ; hence, convergence is always achieved at the true solution. Three types of analyses can be performed. The simplest is a solution for only the fluid pressure based upon the porosity of the soil. In this case, a simple Poisson type analysis is performed and element types 41, 42, or 44 are used. In the second type of analysis, the pore pressures are explicitly defined and the structural analysis is performed. In this case, the element types 21, 27, and 28 should be used. Finally, a fully-coupled analysis is performed; in which case, you should use element types 32, 33, or 35. Of course, the soil can be combined with any other element types, material properties to represent the structure, such as the pilings.

Mechanical Wear Mechanical wear is an important physical phenomena in any structure subjected to repeated loadings. Often, this behavior is modeled by determining the stress on the surface and using it in a subsequent fatigue calculation. For certain applications, including manufacturing, disk brakes, bearings, gears, tires, and seals, it is important to know the amount of wear and possibly the change in geometry which would influence the behavior. It should be noted that, for some applications such as polishing, surface wear is

Main Index

198 Marc Volume A: Theory and User Information

the positive objective. Wear, which is defined as the removal of material from the surface, may be due to mechanical processes or chemical processes. The latter are not considered but the UWEAR user subroutine may always be used to incorporate these effects. The wear due to mechanical behavior can be classified as: 1. Asperity deformation and removal 2. Plowing of the surface 3. Delamination 4. Adhesive 5. Abrasion 6. Fretting 7. Solid particle impingement These processes lead to either mild wear or severe wear (rough, torn surfaces). The wear model implemented in Marc, based upon Archard equation, is not applicable for severe wear. There are several wear models available beginning with Archard’s equation: Gt w = KF ⋅ ----H where K

is the wear coefficient

F

is the normal force

Gt

is the sliding distance

H

is the hardness

K This is converted into an incremental form and the ---- is combined into a single term. This leads to a series H of models that are written as:

Main Index

w· = A ⋅ F ⋅ V r e l

Force based

w· = A ⋅ σ ⋅ V r e l

Stress based

n m w· = A ⋅ F ⋅ V r e l

Force based; Bayer exponential form

n m w· = A ⋅ σ ⋅ V r e l

Stress based; Bayer exponential form

n m –Q ⁄ R T w· = A ⋅ F ⋅ V r e l exp

Force based; Bayer exponential form with thermal activation

CHAPTER 5 199 Structural Procedure Library

m n –Q ⁄ R T w· = AF V r e l exp

Stress based; Bayer exponential form with thermal activation

w· = A

Simple model

where w·

is the rate of change of wear in the direction normal to the surface

σ

is the normal stress

V r e l is the relative sliding velocity Q

is the activation energy

R

is the universal gas constant

A table may be associated with the coefficient to allow temperature dependence or other effects. As an alternative, the coefficient of friction may be included in the wear model. In the most general form, this results in: m n –Q ⁄ R T w· = μAF V r e l exp

Force based, Bayer exponential form with friction coefficient scaling and thermal activation

m n –Q ⁄ R T w· = μAσ V r e l exp

Stress based, Bayer exponential form with friction coefficient scaling and thermal activation.

The incremental wear calculation is performed at the nodal points that are in contact. Hence, the CONTACT option is required. Furthermore, because nodal forces and possibly the coefficient of friction, is used, a nodal based friction model is required. The incremental wear is calculated as: w· Δt and the wear is accumulated as: w n + 1 = w n + w· Δt . If requested, the nodal coordinates will be updated using u n + 1 = u n + Δu n + w· Δt ⋅ n where n is the normal to the surface. If the amount of wear is large, then remeshing may be required.

Main Index

200 Marc Volume A: Theory and User Information

Design Sensitivity Analysis 5

Design sensitivity analysis is used to obtain the sensitivity of various aspects of a design model with respect to changes in design parameters in order to facilitate structural modifications. The design parameters that are amenable to change are called “design variables”. The two major aspects of the design model for which design sensitivity is considered herein are: a. Design objective b. Design model response As a result, the design sensitivity analysis capability in Marc is currently limited to finite element models of structures with linear response in the computation of 1. Gradients for a. An objective function (or the design objective), if one is defined by you (for example, minimizing the material volume in the model). b. Various types of design model responses under multiple cases of static mechanical loading, or free vibration, in linear behavior. 2. Element contributions to the responses of the model. The gradient of the objective function or of a response function is simply the set of derivatives of such a function with respect to each of the design variables, at a given point in the design space (that is, for a given design). For sensitivity analysis to proceed, the design model, the analysis requirements, the design variables, and the functions for which the gradients are to be found have to be specified by you. The existing design sensitivity analysis capability in Marc can be applied in one of two ways: 1. As a stand-alone feature, where you are concerned only with obtaining sensitivity analysis results. Such an application is completed with the output of the sensitivity analysis results. 2. Within a design optimization process, where you are concerned mainly with the optimization of a design objective related to a finite element model. This type of an application of sensitivity analysis is transparent to you. The design optimization process is completed with the output of design optimization related data, such as the optimized objective function, related values of the design variables, and the analysis results for the optimized design. These two procedures are described below. 1. Sensitivity analysis as a stand-alone feature This type of solution usually aims at obtaining the derivatives of user prescribed response quantities at a given design, with respect to each of multiple design variables specified by the user. This set of derivatives is therefore the gradient of the response function at the given design in the design variable space (or, in short, in the design space). For example, for a prescribed response function r, given the design variables x 1 , x 2 , and x 3 , the gradient is defined as ∇r = ˜

Main Index

dr dr dr --------- --------- --------dx 1 dx 2 dx 3

T

(5-227)

CHAPTER 5 201 Structural Procedure Library

The number of response quantities for which gradients are computed is limited either by the program default or by a user-specified number. If you are interested in obtaining the sensitivity analysis results in order of criticality, the option to sort them in this order is also available. The responses are currently prescribed as constraints with user-defined bounds. If sorting is not required, the bounds can be mostly arbitrary, although they still have to conform to the type of constraint prescribed. However, if sorting is required and is to be meaningful, it is important for you to give realistic bounds on the response. Element contributions to each response quantity are obtained as a by-product of the type of response sensitivity analysis capability in Marc. Thus, the response r can be represented as a sum of these element contributions: N

r =

∑

(5-228)

re + C

e = 1

where the second term, C , involves work done elsewhere, such as in support settlement, if any. This is helpful for a visual understanding of which regions of the model contribute in what manner to each of the response quantities at the given design, since it can be plotted in a manner similar to, say stress contours. Finally, as an option, if you also prescribe an objective function, the gradient of the objective function with respect to the design variables is also computed at the given design. Thus, for the objective function W , Marc obtains ∇W = ˜

dW dW dW --------- --------- … --------dx 1 x 2 dx n

T

(5-229)

2. Sensitivity analysis within a design optimization process: The design optimization algorithm in Marc requires the utilization of gradients of the objective function and of the constraint functions, which are very closely related to the response functions. The current algorithm, described under “design optimization”, ignores your initial prescribed design, but instead begins by generating other designs within the prescribed bounds for the design variables. Once the optimization algorithm is completed and the optimized design is available, if a sensitivity analysis is required at the optimized state, it will be necessary for you to modify the model accordingly and to use sensitivity analysis as a stand alone feature. During design optimization, sensitivity analysis is performed for a maximum number of constraints either indicated by the program default or prescribed by you.

Theoretical Considerations The method currently employed in Marc for response sensitivity analysis is the “virtual load” method. For sensitivity analysis of the objective function, finite differencing on the design variables is performed directly.

Main Index

202 Marc Volume A: Theory and User Information

In the virtual load method, first a design is analyzed for the user-prescribed load cases, and, if also prescribed, for eigenfrequency response. The response of the structure having been evaluated for each of these analyses, the response quantities for which sensitivity analysis is to be performed are then decided upon and collected in a database. In sequence, a virtual load case is generated for each such response quantity. Reanalysis for a virtual load case leads to virtual displacements. The principle of virtual work is then invoked. This defines the element contributed part of the response quantity, for which the virtual load was applied, as a dot product of the structural displacement vector, for the actual load case with which the response is associated, and the virtual load vector itself. The jth response r j can be expressed as the dot product of the actual load vector with the virtual displacement vector as T

rj = p uv

(5-230)

By differentiation of this expression, you can show that the derivative of the response r j with respect to a given design variable x i is given by T

dr j dp v T dp dK -------- = ---------- u + u v ⎛⎝ -------- – -------- u⎞⎠ dx i dx i dx i dx i where K is the stiffness matrix of the structure. The response derivative above is evaluated on the element basis as: dr j -------- = dx i

T

∑ e

dp v T dp dK ---------- u + u v ⎛⎝ -------- – -------- u⎞⎠ dx i dx i dx i

(5-231) e

where the vectors u and p v are the vector of element nodal displacements due to the actual load case and the vector of element nodal forces due to the virtual load, respectively. The case of eigenfrequencies follows the same logic except that an explicit solution for the virtual load case is not necessary. The derivatives are now evaluated at the element level via finite differencing. This is known as the semi-analytical approach. Note that the derivative expression for the virtual load method is quite similar to that for the Adjoint Variable method. In fact, while they are conceptually different approaches, for certain cases they reduce to exactly the same expressions. However, for certain other cases, the terms take on different meanings although the end result is the same.

Design Optimization Design optimization refers to the process of attempting to arrive at certain ideal design parameters, which, when used within the model, satisfy prescribed conditions regarding the performance of the design and at the same time minimize (or maximize) a measurable aspect of the design. In Marc, you can ask to minimize

Main Index

CHAPTER 5 203 Structural Procedure Library

1. total material volume 2. total material mass 3. total material cost. When there is more than one material in the finite element model, the specification of different mass densities and unit costs are taken into account in the computation of the objective function. The performance requirements might not necessarily have to be related to response, but also to different concepts such as packaging, design envelope, even maintenance. The current capability is based on optimization with constraints on response. Also, the lower and upper bounds on the design variables themselves define the limits of design modifications. Hence, the design optimization problem can be posed mathematically in the following format: Minimize

W

Subject to

c j ≥ 0.0

j = 1, …, m

where W is the objective function, and c j is the jth constraint function, either specified as an inequality related to a response quantity or as a limit on a design variable. For example, to limit the x-direction translation component at a node k, the constraint can first be written as ( u x ) k ≤ u x*k Assuming that the displacement is constrained for positive values, the normalized constraint expression c (dropping the subscript

j

) becomes:

( u∗ – u ) ⁄ u∗ ≥ 0.0

(5-232)

with its derivatives as: dc – 1 du ------ = ------ -----dx u∗ dx

(5-233)

Within Marc, the constraints can be imposed on strain, stress, displacement, and eigenfrequency response quantities. For stresses and strains, the constraints are defined as being on the elements, and for displacements, the constraints are defined as being at nodes. Stress and strain components, as well as various functions of these components (the von Mises equivalent stress and principal stresses, stresses on prescribed planes) and generalized stress quantities can be constrained. Similarly, translation and rotation components of displacement, resultant and directed displacements as well as relative displacements between nodes can be constrained. For free vibration response, constraints can be placed on the modal frequencies as well as on differences between modal frequencies. A full listing of such constraints are given in Marc Volume C: Program Input. The upper and lower bounds on the design variables are posed as xi ≤ xu

and

xi ≥ xl

after which they can be transformed into expressions similar to Equation (5-232).

Main Index

(5-234)

204 Marc Volume A: Theory and User Information

The response quantities associated with the model are implicit functions of the design variables. Analyses at sample design points are used to build explicit approximations to the actual functions over the design space. This approach minimizes the number of full scale analyses for problems which require long analysis times such as for nonlinear behavior. This method is summarized next.

Approximation of Response Functions Over the Design Space The design space for the optimization problem is bounded by limits on the design variables of a model to be optimized. The simplest case is that of a single design variable, where the design space is a straight line, bounded at the two ends. For higher number of design variables, say n, the design space can 2

be visualized as a bounded hyperprism with n vertices. For such a construct, you can build approximations to the constraint functions by way of analyses conducted at the vertices. However, this 2

requires n analyses. We now note that the minimum geometrical construct spanning n-dimensional space is a simplex with n + 1 vertices. Thus, an approximation based on analyses at vertices requires only ( n + 1 ) analyses. The simplex has already been used for first order response surface fitting based on only function values [Ref. 3]. However, the use here involves higher order response functions. Like the hyperprism, in one-dimension, the simplex degenerates into a straight line. However, in two dimensions it is a triangle, and in general it is a hyper-tetrahedron. Figure 5-31 compares the simplex to the hyperprism in normalized two-dimensional design space.

n=2 Hyperprism: 22 = 4 vertices Simplex : 2 + 1 = 3 vertices

Figure 5-31 Comparison of the Simplex to the Hyperprism in Two-dimensions

While the orientation of the simplex in the design space appears to be a relatively arbitrary matter, once an origin and the size of the simplex are prescribed, a simple formula will locate all vertices of a simplex in n-dimensions [Ref. 4]. The response gradient information at the simplex vertices is combined with the function values to achieve enhanced accuracy. Thus, an analysis at a vertex can be utilized to yield both response function values and, by way of sensitivity analysis, the response gradients at that vertex.

Main Index

CHAPTER 5 205 Structural Procedure Library

The virtual load method employed in Marc for obtaining the response gradients is discussed under Design Sensitivity Analysis. The response gradients can then easily be converted to constraint gradients for use in an optimization algorithm. As a result, the results of an analysis at a vertex of the simplex can be summarized as the vector of constraint function values c j , and the gradient, ∇c j , of each constraint function ( j ) at that vertex. For the case of a one variable problem, the results of analyses at the two vertices are symbolized in Figure 5-32, for a hypothetical constraint c j . dc j1 -----------dx

E1 Possible Actual Function

c j1 2 1

c j2 E2

dc j2 -----------dx Figure 5-32 Vertex Results for One-dimensional Design Space x

From Figure 5-32, it appears almost natural to fit a cubic function to the four end conditions (two function values and two slopes) depicted in the figure. However, this approach is too rigid, and is not easily generalizable to higher dimensions. On the other hand, the use of two quadratics, which are then merged in a weighted manner gives higher flexibility and potential for increased accuracy. It can be seen that the two equations, E1 and E2 , are designed such that they both satisfy the function values at the two vertices, but E1 satisfies the slope at vertex 1 only, and E2 satisfies the slope at vertex 2 only. Finally, at any design point x , the response function c j can be approximated as c j = ( W1 E1 + W2 E1 ) ⁄ ( W1 + W2 )

(5-235)

where the weight functions W1 and W2 are normally functions of x and possibly some other parameters. This type of approach has the further advantage that it is consistent with the use of the simplex for determining analysis points and approximating constraint functions in the higher dimensional cases. Therefore, for an n-dimensional problem, the simplex having n + 1 vertices, each equation needs to have ( n + 1 ) + n = 2n + 1 unknown parameters. The general quadratic polynomial without the crosscoupling terms satisfies this condition for all n .

Main Index

206 Marc Volume A: Theory and User Information

Improvement of the Approximation When approximations are used, the results of an optimization process need to be checked by means of a detailed analysis. As a result, the approximations can be adjusted and the optimization algorithm can be reapplied. Depending on how accurate the approximations prove to be and how many more detailed analyses are acceptable to you, this process can be applied for a number of cycles in order to improve upon the results.

The Optimization Algorithm The optimization algorithm implemented in Marc is the Sequential Quadratic Programming method [Ref. 5]. This method is employed using the approximation described above. By obtaining response function and gradient values from the approximate equations, the need for full scale analyses is reduced. The method is summarized below. The quadratic programming technique is based on the approximation of the objective function by a quadratic function. When nonlinear constraints exist, as is the case in most practical design optimization problems, the second order approximation concept is extended to the Lagrangian which is a linear combination of the objective function and the constraint functions. The solution method for a quadratic programming problem with nonlinear constraints can be summarized as the following: At each step, modify the design variables vector x by adding a scaled vector x ← x + qs

(5-236)

where s is a search direction and q is the scale factor along the search direction. If the search direction has been determined, the scale factor can be found by some type of line search along the search direction. The determination of the search direction constitutes the major undertaking in the quadratic programming method. If H is the Hessian of the Lagrangian and g is the gradient of the objective function, then the search direction s is that which minimizes the function T

T

g s + ( s Hs ) ⁄ 2

(5-237)

subject to the linearized constraints Js ≥ – c

(5-238)

where J is the Jacobian matrix of the constraints and c is the vector of constraint functions at the current iteration. Due to lack of knowledge about which constraints will be active at the optimum, the Hessian of the Lagrangian is not always readily available. Thus, some iterations take the form of a gradient projection step. The coefficients of the constraint functions in the Lagrangian are the Lagrange multipliers which are unknown before solution has started. At the optimum these multipliers are zero for inactive constraints. Normally, the above problem is solved using only those constraints which appear to be active at or close to the current design point, with the assumption that these constraints will be active at the optimum. The

Main Index

CHAPTER 5 207 Structural Procedure Library

selection of these active constraints is done within the framework of an active set strategy, the set being modified appropriately with the progression of the iterations. Similarly, the arrays g , H , and J are also modified as the iterations proceed.

Marc User Interface for Sensitivity Analysis and Optimization This is discussed under Input, Output, and Postprocessing in the following paragraphs. Input Input features related to design sensitivity and design optimization are similar. However, they differ in the parameter data blocks and in the optional specification of an objective function for the case of sensitivity analysis. Therefore, other than these two items, all discussion of input should be construed to refer to both procedures equally. All design sensitivity and design optimization related parameters and options in a Marc input file start with the word DESIGN. All load cases and any eigenfrequency analysis request associated with sensitivity analysis or optimization should be input as load increments in the history definition section after the END OPTION line. The maximum number of nodes with point loads or the maximum number of distributed load cases should be defined in the DIST LOADS parameter. The type of solution requested from Marc can simply be indicated by the parameter input DESIGN SENSITIVITY or DESIGN OPTIMIZATION. Only one of these lines can appear in the input. These parameters also let you change the sorting of constraints, the maximum number of constraints in the active set, and the maximum number of cycles of design optimization. The first two items are discussed in previous sections. A cycle of design optimization refers to a complete solution employing the sequential quadratic programming technique followed by a detailed finite element analysis to accurately evaluate the new design point reached by way of approximate solution. If required, the approximation is improved using the results of the last finite element analysis, and a new cycle is started. The specification of an objective function, being optional for design sensitivity, is made by use of the model definition option DESIGN OBJECTIVE. This allows you to choose from one of the available design objectives. The DESIGN VARIABLES option allows you to specify the design variables associated with the finite element model. You have a choice of three major types of design variables: 1. Element cross-sectional properties as given by way of the GEOMETRY option. 2. Material properties as given by ISOTROPIC or ORTHOTROPIC options. 3. Composite element properties of layer thickness and ply angle, as given by the COMPOSITE option. The properties which are supported are listed under the DESIGN VARIABLES option. The relevant elements, for which cross-sectional properties can be specified as design variables, each has a section in Marc Volume B: Element Library, describing which properties, if any, can be posed as design variables for that element. Similarly, the list of material properties (currently all related to linear behavior) that can be design variables is given under the DESIGN VARIABLES option. For composite groups, the layer thicknesses and ply angles can be given as design variables for composite groups.

Main Index

208 Marc Volume A: Theory and User Information

Design variables can be linked across finite element entities such that a given design variable controls several entities. An example is the linking of the thicknesses of several plane stress elements by means of a single design variable. Thus, when this variable changes, the thicknesses of all linked elements reflect this change. On the other hand, for the unlinked case, all thicknesses are associated with separate design variables. This feature is controlled by the LINKED and UNLINKED commands. Response quantities, or constraints on response quantities, are specified by means of the DESIGN DISPLACEMENT CONSTRAINTS, DESIGN STRAIN CONSTRAINTS, DESIGN STRESS CONSTRAINTS, and DESIGN FREQUENCY CONSTRAINTS options. There is no limit to the number of constraints. Displacement constraints are posed at nodes or groups of nodes, while the strain and stress constraints are posed over elements or groups of elements, and frequency constraints are posed for free vibration modes. A complete list can be found under the above mentioned options in Marc Volume C: Program Input. When strain or stress constraints are prescribed, it is useful to know that the program evaluates such constraints at all integration points of all layers of an element and proceeds to consider the most critical integration point at the related layer for the element. Thus, a strain or stress constraint on an element normally refers to the most critical value the constraint can attain within the element. During optimization, the most critical location within the element may change and any necessary adjustment takes place internally. For certain responses, the limiting values can be the same in absolute value for both the positive and negative values of the response. For constraints on such response functions, you have the choice of prescribing either separate constraints on the positive and negative values, or a combined constraint on the absolute value. The first approach is more accurate albeit at a higher computational cost. Output For sensitivity analysis, the output file contains the following information: • Echo of input, any warnings or error messages. • A of numbers and definitions for your prescribed design variables. It is important to note that the variable values are always output in the internal numbering sequence which is defined in this. Search for the words ‘Design variable definitions’ to reach this in the output file. • Analysis results for your prescribed design. • The value of the objective function and its gradient with respect to the design variables prescribed by you. • Sensitivity analysis results for the response functions in the default or user-defined set, sorted in order of criticalness (if specified). It should be noted that although the responses are sorted across multiple load cases, the sensitivity results are output for each load case. The related output file consists of a check on the actual response value (obtained by sensitivity analysis) and the gradient of the response with respect to the design variables. For eigenfrequency results, the check values on the response can be somewhat more accurate than the results from eigenfrequency analysis since the latter is iterative, but the check uses the Rayleigh quotient on top of the iteration results. A constraint reference number allows you to track the sensitivity analysis results plots when postprocessing. Search for the word ‘Sensitivity’ to reach this output. For design optimization, the following is written into the output file:

Main Index

CHAPTER 5 209 Structural Procedure Library

• Echo of input, any warnings or error messages. • Certain indications that some analyses are being done, but no analysis results except for the ‘best’ design reached during optimization. • The objective function values and the vector of design variable values: • At each of the simplex vertices. • For the starting simplex vertex (from this point on, the information also includes whether the design is feasible or not). • At the end of each cycle of optimization. • For the ‘best’ design found. • Analysis results for the ‘best’ design. Postprocessing This requires that you ask the program to create a post file. The following plots can be obtained by way of postprocessing. For sensitivity analysis: • Bar charts for gradients of response quantities with respect to the design variables. • Contour plots of element contributions to response quantities. Thus, a finite element model contour plot gives the element contributions to a specific response quantity which was posed in the form of a constraint in the input file. The increment number of the sensitivity analysis results is the highest increment number available in the post file. The information for each response quantity is written out as for a subincrement. The zeroth subincrement corresponds to the objective function information. Numbers for the other subincrements correspond to the constraint reference number(s) in the output file. For design optimization: • Path plots showing the variation of the objective function and of the design variables over the history of the optimization cycles. The best design (feasible or not) is not necessarily the last design point in the plot. The values at the starting vertex are considered as belonging to the zeroth subincrement. Each optimization cycle is then another subincrement. The increment number corresponding to these subincrements is taken as zero. The analysis results for the ‘best’ design start from increment one. • Bar charts where each chart gives the values of the design variables at the optimization cycle corresponding to that bar chart.

Defined Initial State with Result Data from Previous Analysis (including AXITO3D) In many cases, it is necessary to analyze a nonlinear process in several stages. Each stage may involve different contact bodies and boundary conditions, but history data such as temperature, displacement, stress and strain have to be carried over for contact bodies to be passed from one stage to another. In Marc, it is possible to start a numerical simulation as a two-dimensional axisymmetric or plane strain

Main Index

210 Marc Volume A: Theory and User Information

problem and switch to a full three-dimensional analysis in subsequent stages. This makes multiple stage analysis more efficient. The PRE STATE option is designed to read result data from Marc and use the data as initial conditions in the new analysis. For contact analysis, it allows the selection of contact bodies by names. The PRE STATE option includes the capability of the AXITO3D option available in the 2003 release. The methodology of the PRE STATE option can be outlined as the following: • Scan through the result file for the desired time step or time instant. • Collect the list of nodes and elements corresponding to the contact body transfer list. • Collect node and element data as required (see the PRE STATE option in Marc Volume C: Program Input for the data type). • Copy data to the new model as the initial conditions with 2-D to 3-D expansion if applicable. The PRE STATE option takes several steps: • Run first stage analysis. • Open the result file. • Extract and expand (if 2-D to 3-D is required) the mesh from the previous result file at the increment. The expansions of boundary conditions can also be done through Marc Mentat. • Build second stage model based on the mesh extracted and add other contact bodies and conditions. • Specify the PRE STATE option under initial condition menu. • Run 3-D analysis. Most quadrilateral or hexahedral elements (including Herrmann elements) as well as commonly most available materials (such as metal and rubber) can be used in the PRE STATE option. For large deformation problems, either total or updated Lagrangian formulation can be used. Thermal and dynamic effects can also be included. For more detailed information on this feature, see the PRE STATE model definition option, in Marc Volume C: Program Input.

Load and Displacement Boundary Conditions Transfer for PRE STATE Option In general, the PRE STATE option can only transfer history data from the result file as the initial conditions in the new model. Users are responsible for reapplying the boundary and load conditions as well as the material properties. If users use Marc Mentat, the boundary conditions defined in the previous 2-D analysis automatically expand to 3-D when the mesh is expanded from 2-D to 3-D. However, if a load function is used and is required in the new model, curve shifting is required. That is, if, in the previous model, a load is applied from 0 to 10 in the new model based on the last step of the previous analysis, the load is applied starting from 10. For prescribed displacement, as nodal positions are updated to the final configuration in the previous analysis, the load function should start from 0 in the new model.

Main Index

CHAPTER 5 211 Structural Procedure Library

Steady State Rolling Analysis Rolling contact analysis of a cylindrical deformable body in a Lagrangian framework can be computationally expensive because it may require not only time-dependent transient process but also a fine mesh in the entire body to accurately capture contact characteristics. However, some problems involve only fully axisymmetric structures with constant moving/spinning velocities. These problems can be considered steady state if a reference configuration, which moves with the body but does not spin around the rolling axis, is used. Marc provides the capability of steady state rolling analysis. The feature is characterized by a mixed Eulerian/Lagrangian formulation with inertia effects in spinning/cornering deformable bodies. Using a non-spinning reference frame attached to the wheel axel, the analysis becomes purely space dependent. It presents a better alternative to the unnecessary computational burden of arriving at a steady state condition through a transient analysis. Furthermore, a finer mesh only needs to be used in the contact region as opposed to the entire rolling surface.

Kinematics We consider the axisymmetric body shown in Figure 5-33. The body spins at an angular velocity ω s around the axisymmetric axis T s at point P s and, simultaneously rotates with a cornering angular velocity ω c around an axis T c at point P c . Assume that a particle in the body has a location P 0 at time t = 0 . At time t , its motion contains three parts: 1. from P 0 to a location X because of the spinning 2. from X to Y because of a deformation Y = D ( X ) , where D is time independent function resulting from the steady state condition 3. from Y to Z because of the cornering.

Ps Ts

ωs

Tc ωc Pc Figure 5-33 Kinematics

Main Index

212 Marc Volume A: Theory and User Information

The three motions can be described as X = Rs ⋅ ( Po – Ps ) + Ps

(5-239)

Y = D(X)

(5-240)

Z = Rc ⋅ ( Y – Pc ) + Pc

(5-241)

with R s = exp ( ω s t ) and R c = exp ( ω c t )

(5-242)

˜ s and ω c are the skew-symmetric tensors associated with the rotation vectors In Equation (5-242), ω ω s T s and ω c T c , respectively, with ω s ⋅ r = ω s T c × r and ω c ⋅ r = ω c T c × r

(5-243)

for any vector r . Time derivative of Equation (5-242) gives · · R s = ω s ⋅ R s and R c = ω c ⋅ R c

(5-244)

Making use of Equations (5-239), (5-240), (5-243), and (5-244), the velocity of the particle can be obtained by the first time derivative of Equation (5-241) as · ∂D Z = R c ⋅ ω c T c × ( Y – P c ) + ω s ------∂α

(5-245)

where α = ω s t , is the spinning angle. Similarly, the acceleration is obtained by the second derivative of Equation (5-241) with respect to time: ·· ∂D ∂2D Z = R c ⋅ ω c2 ( T c ⊗ T c – 1 ) ⋅ ( Y – P c ) + 2ω s ω c T c × ------- + ω s2 ---------∂α ∂α 2

(5-246)

where ⊗ denotes the tensor product and 1 is the unit tensor. Transformation of Equations (5-245) and (5-246) into the reference configuration defined by X by premultiplying R cT , gives

Main Index

∂D v = ω c T c × ( Y – P c ) + ω s ------∂α

(5-247)

∂D ∂2 D a = ω c2 ( T c ⊗ T c – 1 ) ⋅ ( Y – P c ) + 2ω s ω c T c × ------- + ω s2 ---------∂α ∂α 2

(5-248)

CHAPTER 5 213 Structural Procedure Library

where v and a are velocity and acceleration of the particle with respect to the reference frame.

Inertia Effect The contribution of inertia effect into the right-hand-side of the system equation can be calculated using the weak form δπ =

∫ ρa ⋅ δu dv v

∂D = – ρω c2 ∫ ( T c ⊗ T c – 1 ) ⋅ ( Y – P c ) ⋅ δu dv – 2ρω s ω c ∫ T c × ------- ⋅ δu dv ∂α V

(5-249)

V

∂D ∂δu + ρω s2 ∫ ------- ⋅ --------- dv ∂α ∂α V

where ρ is the density, v is the volume, and u is the displacement. Linearization of Equation (5-249) gives ∂Δu Δδπ = – ρω c2 ∫ Δu ⋅ ( T c ⊗ T c – 1 ) ⋅ δu dv – 2ρω s ω c ∫ T c × ---------- ⋅ δu dv ∂α v

V

∂Δu ∂δu + ρω s2 ∫ ---------- ⋅ --------- dv ∂α ∂α

(5-250)

v

which can be used to calculate the contribution of the inertia effect to stiffness matrix.

Rolling Contact To take into account the rolling effect in contact, the velocity vector in Equation (5-247) is decomposed into a normal and a tangential component, with respect to the contact surface, for all nodes in contact with ground. The normal component is then forced to become zero because of the contact conditions. The relative slipping velocity used in friction calculation is the difference between the tangential component and the ground moving velocity.

Steady State Rolling with Marc The capability of steady state rolling analysis in Marc has taken into account the effects of rolling frictions and the inertia effects resulting from both spinning and cornering. The deformable rolling body can contact with multiple, flat or nonflat rigid surfaces. A typical example is a tire model which is in contact with a rigid rim and a rigid road surface. The spinning effects are involved only for selected contact body pair (for example, tire/road) which is defined with the SS-ROLLING history model definition option. The steady state rolling analysis can follow a static stress analysis with various loadcases and can also combine with any steady state loads. The feature is available for 3-D analysis only.

Main Index

214 Marc Volume A: Theory and User Information

The element types supported for steady state rolling analysis include 7, 9, 18, 21, 35, 57, 61, 84, 117, 120, 146, 147, and 148. The friction type supported in contact for steady state rolling analysis, based on nodal force, is Coulomb friction for rolling. Because the system matrix becomes nonsymmetric in steady state rolling analysis, it is recommended that the multifrontal direct sparse solver be used. The feature requires the so-called streamline along the circumferential direction of the spinning body. Therefore, the 3-D mesh must be generated by revolving its corresponding axisymmetric mesh. For a 3-D brick element, the circumferential direction must be from the element face defined by nodes 1-2-3-4 to the element face defined by nodes 5-6-7-8. Below is a list of options required in a steady state analysis, in addition to the others in a standard static stress analysis. SS-ROLLING:

Parameter activating the steady state rolling analysis

ROTATION A:

Model definition option defining the spinning axis

CORNERING AXIS:

Model definition option defining the cornering axis

SS-ROLLING:

History definition option defining the spinning body, ground body, spinning body motion (spinning/cornering/moving relative to the ground) and others. All velocities/forces defined in the option are total values.

Structural Zooming Analysis Local variations, such as the changes in model geometries or in the degrees of finite element refinement to achieve a better evaluation of the local gradients in the solution, often need a complete re-analysis of the entire model. 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 part with the local changes. It can be realized by applying the existing loads or/and boundary conditions in the local model along with properly defined kinematic conditions to the local boundaries connecting to the global model. A typical structural zooming analysis contains two steps: 1. Global run to obtain a post file containing global 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 next level refinement. The GLOBALLOCAL option (see Marc Volume C: Program Input for details) 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.

Main Index

CHAPTER 5 215 Structural Procedure Library

b. Reading in the global model (element types, node coordinates, element connectivity, thickness if shell elements) and solution of the model from the generated post file in global run. c. Finding out 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. Calculation of 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 storage of the deformation (temperature) history in the format of time-dependent tables. e. Applying the deformation (temperature) history of the connecting nodes to the local model as prescribed kinematic boundary conditions. All the steps above are performed automatically inside Marc once the GLOBALLOCAL option is used in the input file of the local run.

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

One can use composite continuum elements in the local model if the global model had composite continuum elements with the same number of layers or was composed of shell elements See Figure 5-34 for examples from 2-D solid elements to 2-D solid elements and from 3-D shell elements to 3-D solid elements. global model

local model

cracks

Cylinder

(a) 2-D Solid to 2-D Solid Figure 5-34 Structural Zooming

Main Index

(b) 3-D Shell to 3-D Solid

216 Marc Volume A: Theory and User Information

Cure-Thermal-Mechanically Coupled Analysis 5

When resin is used in the manufacturing of composite parts, the curing process during and after the forming processes has a significant effect on the thermal and mechanical behavior of the formed part. The shrinkage caused by curing may severely distort the final geometry of the part. Marc has implemented a capability that allows you to perform cure-thermal-mechanical coupled analysis to predict this behavior.

Structur al Procedu re Library

The curing analysis is incorporated into the existing staggered coupled thermal-mechanical analysis procedure (see Thermal Mechanically Coupled Analysis in Chapter 6: Nonstructural and Coupled Procedure Library). Before the heat transfer analysis pass takes place, the curing analysis is performed based on the estimated temperatures at the beginning and end of the increment. The cure rate is then calculated according to the cure kinetics of the resin materials. Using the cure rate, a heat flux due to cure reaction heat generation is calculated and added into the heat transfer system of equations. Volumetric curing reaction heat flux is calculated according to the cure rate dα Q c = ------- ( 1 – V f )ρ r H r dt

(5-251)

where: Hr

– resin cure reaction heat

ρr

– resin density

α

– resin degree of cure

Vf

– fiber volume fraction

The governing matrix equation for cure-thermal coupled analysis can be expressed as: C ( T )T· + K ( T )T = Q + Q I + Q F + Q C

(5-252)

In Equation (5-252), C ( T ) and K ( T ) are the temperature-dependent heat capacity and thermal conductivity matrices, respectively. T is the nodal temperature vector. T· is the time derivative of the temperature vector, Q is the external heat flux vector, Q I is the heat flux vector due to plastic work, Q F represents the heat generated due to friction, and Q C is the heat generated due to curing. With the CURING parameter included in the input data, Marc first activates the pass to calculate the degree of cure and curing reaction heat flux at the beginning of each cycle of heat transfer analysis. Then, Marc considers the cure shrinkage strain in the mechanical pass of the thermal-mechanical coupled analysis. To include curing into a heat transfer or thermal-mechanical coupled analysis, it is necessary to add the CURING parameter into the input data. In addition, the CURE RATE model definition option is also needed to define the curing properties, usually called cure kinetics, of resin materials as one kind of property for heat transfer analysis.

Main Index

CHAPTER 5 217 Structural Procedure Library

To include cure shrinkage strain into the mechanical pass of a thermal-mechanical coupled analysis, in addition to having both the CURING parameter and the CURE RATE model definition option in the input data, the CURE SHRINKAGE model definition must be included to define the cure shrinkage properties of the resin material. Note that the cure shrinkage effect is calculated based on the degree of cure, so the cure shrinkage effect is ignored if the degree of cure is not calculated during the heat transfer pass.

Cure Kinetics In Marc, the cure kinetics defines the cure rate as a function of the degree of cure and the temperature of resin materials. There are different approaches to define the cure kinetics of resin materials: embedded cure kinetics models, table definition and user subroutine. In a curing analysis, the cure rate is calculated for each time step. Assuming that the cure rate is defined as the function of the degree of cure and temperature of: dα ------- = f ( α ,T ) dt

(5-253)

The time integration of the degree of cure is done using backward Euler method: α ni = Δt ⋅ f ( α ni – 1 ,T ) + α n – 1 where i

– iteration number for cure

n

– current increment number

n–1

– previous increment number

f

– function defined by cure kinetics model

Δt

– time step size of the increment

The four cure kinetics models implemented in Marc are: Cure kinetics model 1: by Lee, Loos and Springer (1982) [Ref. 43]; Cure kinetics model 2: by Scott(1991) [Ref. 50]; Cure kinetics model 3: by Lee, Chiu, and Lin (1992) [Ref. 44]; Cure kinetics model 4: by Johnston and Hubert (1996) [Ref. 52]. Tables 5-7 and 5-8 summarize the details of these cure kinetics models and the definition of the required parameters.

Main Index

(5-254)

218 Marc Volume A: Theory and User Information

Table 5-7

Cure Kinetics Models Embedded in Marc

Model Model 1 Lee, Loos and Springer (1982) [Ref. 43]

Equations dα ------- = ( K 1 + K 2 α ) ( 1 – α ) ( B – α ) dt α ≤ αc dα ------- = K 3 ( 1 – α ) dt Ki = Aie

A 1, A 2, A 3, ΔE 1, ΔE 2, ΔE 3, B, α C, H R

α > αc

–Δ Ei ⁄ ( R T )

dα ------- = Kα m ( 1 – α ) n dt Lee, Chiu, and Lin (1992)[Ref. 44]; White and K = Ae – Δ E ⁄ ( R T ) Hahn (1992) [Ref. 48]

A, ΔE, m, n, H R

(Included in Model 2)

A, ΔE, n, H R

(Included in Model 2)

Kenny (1992) [Ref. 49]; Scott (1991)[Ref. 50]

dα ------- = K ( 1 – α ) n dt K = Ae – Δ E ⁄ ( R T )

Model 2 (combined Model) dα ------- = ( K 1 + K 2 α m ) ( 1 – α ) n dt Scott (1991)[Ref. 50] Ki = Aie Model 3 Lee, Chiu, and Lin (1992)[Ref. 44] Model 4 Johnston and Hubert (1995)[Ref. 52]

A 1, A 2, ΔE 1, ΔE 2, l, m, n, H R

–Δ E ⁄ ( R T ) i

dα Kα m ( 1 – α ) n ------- = --------------------------------------------------------------C {α – (α +α T )} dt C0 CT 1+e Ki = Aie

A 1, A 2, ΔE 1, ΔE 2, m, n, H R

–Δ E ⁄ ( R T ) i

dα ------- = K 1 ( 1 – α ) l + K 2 α m ( 1 – α ) n dt Ki = Aie

Main Index

Parameters

–Δ E ⁄ ( R T ) i

A, ΔE, m, n, C, α C 0, α C T, H R

CHAPTER 5 219 Structural Procedure Library

Table 5-8

Parameters used in the Embedded Resin Cure Kinetics Models

Variable

Description

Units

α

Resin degree of cure.

-

T

Resin temperature

K or R

HR

Total resin heat of reaction (α = 0 to 1)

J/kg or BTU/lbm

Ai

Pre-exponential factor.

/s

ΔE i

Activation energy.

J/mol or BTU/mol

l

Equation superscript.

-

m

Equation superscript.

-

n

Equation superscript.

-

R

Gas constant

J/(mol K) or BTU/(mol R)

C

Diffusion Constant

-

αC 0

Critical Resin Degree of Cure

-

αC T

The Increase in Critical Resin Degree of Cure with Temperature

In Marc, the table definition allows the user to define the cure rate as a function of the degree of cure and temperature if the resin kinetics is not defined by the four embedded models. In addition, the degree of cure and cure rate can also be calculated through the UCURE user subroutine.

Cure Shrinkage Strain The cure shrinkage strain is calculated according to the volumetric shrinkage due to curing process. The S

resin degree of cure shrinkage is defined as the ratio of volumetric cure shrinkage ( V r ) and maximum volumetric cure shrinkage

S∞ ( Vr )

S

of the resin material, as α S

Vr = ----------- . Equation (5-255) then S∞ Vr

calculates the cure shrinkage strain: S 1⁄3

ε rS = ( 1 + V r )

–1

(5-255)

Considering the anisotropic shrinkage behavior of composite with resin, the strain components of the composite are calculated by using the directional Cure Shrinkage Coefficient (CSC) matrix by Equation 5-256.

Main Index

220 Marc Volume A: Theory and User Information

ε iSj = CS ( C i j ⋅ ε rS )

i, j = 1 ,2 ,3

(5-256) S

The calculation of volumetric cure shrinkage, V r , is conducted based on the cure shrinkage models defined by users. Marc has two cure shrinkage models available. Tables 5-9 and 5-10 summarize the details of the cure kinetics models and the definition of the requires parameters. Table 5-9

Resin Cure Shrinkage Models

Model Model 1 Bogetti and Gillespie (1992) [Ref. 42]

Equations α < αC 1

S

V r = 0.0 S∞

S

Vr = A * αS + ( Vr S

2

– A ) * αS

White and Hahn 1992 [Ref. 48]

Table 5-10

V r = V rS ∞ *10 S S

αC 1 ≤ α < αC 2 α ≥ αC 2

B ( α – αc )

α ≤ αC

S∞

V r , α C, B

α > αC

S∞

Vr = Vr

Parameters used in the Resin Cure Shrinkage Models

Variable

Description

Units -

S

Resin volumetric cure shrinkage

Vr

S∞

Total volumetric resin shrinkage from = 0 to 1.

αs

The degree of cure shrinkage.

-

αC 1

Degree of cure after which the resin shrinkage begins (model 1).

-

αC 2

Degree of cure after which the resin shrinkage stops (model 1).

-

A

Linear cure shrinkage coefficient

-

αC

Degree of cure after which the resin shrinkage begins (model 2).

-

B

Cure shrinkage model superscript.

-

Vr

Main Index

S

V r , α C 1 , α C 2, A

S∞

Vr = Vr

α – αC 1 α S – --------------------------αC 2 – αC 1 Model 2

Parameters

-

CHAPTER 5 221 Structural Procedure Library

References 1. Key, S. W. and R. D. Krieg, 1982, “On the Numerical Implementation of Inelastic Time-Dependent, Finite Strain Constitutive Equations in Structural Mechanics”, Computer Methods in Applied Mechanics in Engineering, V.33, pp. 439–452, 1982. 2. Bathe, K. J., E. Ramm, and E. L. Wilson. “Finite Element formulation for Large Deformation Dynamic Analyses”, International Journal for Numerical Methods in Engineering, V. 9, pp. 353386, 1975. 3. Montgomery, D. C., Design and Analysis of Experiments, (2nd ed.) John Wiley and Sons, 1984. 4. Spendley, W., Hext, G. R., Himsworth, F. R., “Sequential Application of Simplex Designs in Optimisation and Evolutionary Operation”, Technometrics, Vol. 4, No. 4, pp. 441-461 (1962). 5. Gill, P. E., Murray, W., Saunders, M. A., Wright, M. H., “Sequential Quadratic Programming Methods for Nonlinear Programming”, NATO-NSF-ARO, Advanced Study Inst. on Computer Aided Analysis and Optimization of Mechanical System Dynamics, Iowa City, IA, Aug. 1-2, 1983, pp. 679-700. 6. Bathe, K. J. Finite Element Procedures Prentice-Hall, 1996. 7. Wilkinson, J. H. The Algebraic Eigenvalue Problem. Oxford: Clarendon Press, 1965. 8. Zienkiewicz, O. C., and Taylor, L. C. The Finite Element Method. Fourth Ed., Vol. 1 & 2. London: McGraw-Hill, 1989. 9. Barsoum, R. S. “On the Use of Isoparametric Finite Elements in Linear Fracture Mechanics.” Int. J. Num. Methods in Engr. 10, 1976. 10. Dunham, R. S. and Nickell, R. E. “Finite Element Analysis of Axisymmetric Solids with Arbitrary Loadings.” No. 67-6. Structural Engineering Laboratory, University of California at Berkeley, June, 1967. 11. Hibbitt, H. D., Marcal, P. V. and Rice, J. R. “A Finite Element Formulation for Problems of Large Strain and Large Displacement.” Int. J. Solids Structures 6 1069-1086, 1970. 12. Houbolt, J. C. “A Recurrence Matrix Solution for the Dynamic Response of Elastic Aircraft.” J. Aero. Sci. 17, 540-550, 1950. 13. McMeeking, R. M., and Rice, J. R. “Finite-Element Formulations for Problems of Large ElasticPlastic Deformation.” Int. J. Solids Structures 11, 601-616, 1975. 14. MARC Update. “The Inverse Power Sweep Method in MARC.” U.S. Ed., vol. 3, no. 1, February, 1984. 15. Simo, J. C., Taylor, R. L., and Pister, K. S. “Variational and Projection Methods for the Volume Constraint in Finite Deformation Elasto-Plasticity,” Comp. Meth. in App. Mech. Engg., 51, 1985. 16. Simo, J. C. and Taylor, R. L. “A Return Mapping Algorithm for Plane Stress Elasto-Plasticity,” Int. J. of Num. Meth. Engg., V. 22, 1986. 17. Wriggers, P., Eberlein, R., and Reese, S. “A Comparison of Three-Dimensional Continuum and Shell Elements for Finite Plasticity,” Int. J. Solids & Structures, V. 33, N. 20-22, 1996.

Main Index

222 Marc Volume A: Theory and User Information

18. Simo, J. C. and Taylor, R. L. “Quasi-Incompressible Finite Elasticity in Principal Stretches, Continuum Basis and Numerical Algorithms,” Comp. Meth. App. Mech. Engg., 85, 1991. 19. Marcal, P. V. “Finite Element Analysis of Combined Problems of Nonlinear Material and Geometric Behavior.” in Proceedings of the ASME Computer Conference, Computational Approaches in Applied Mechanics, Chicago, 1969. 20. Melosh, R. J., and Marcal, P. V. “An Energy Basis for Mesh Refinement of Structural Continua.” Int. J. Num. Meth. Eng. 11, 1083-1091, 1971. 21. Morman, K. N., Jr., Kao, B. G., and Nagtegaal, J. C. “Finite Element Analysis of Viscoelastic Elastomeric Structures Vibrating about Nonlinear Statically Stressed Configurations.” SAE Technical Papers Series 811309, presented at 4th Int. Conference on Vehicle Structural Mechanics, Detroit, November 18-20, 1981. 22. Morman, K. N., Jr., and Nagtegaal, J. C. “Finite Element Analysis of Small Amplitude Vibrations in Pre-Stressed Nonlinear Viscoelastic Solids.” Int. J. Num. Meth. Engng, 1983. 23. Nagtegaal, J. C. “Introduction in Geometrically Nonlinear Analysis.” Int. Seminar on New Developments in the Finite Element Method, Santa Marherita Ligure, Italy, 1980. 24. Nagtegaal, J. C., and de Jong, J. E. “Some Computational Aspects of Elastic-Plastic Large Strain Analysis.” in Computational Methods in Nonlinear Mechanics, edited by J. T. Oden. NorthHolland Publishing Company, 1980. 25. Newmark, N. M. “A Method of Computation for Structural Dynamics.” ASCE of Eng. Mech. 85, 67-94, 1959. 26. Parks, D. M. “A Stiffness Derivative Finite Element Technique for Determination of Elastic Crack Tip Stress Intensity Factors.” International Journal of Fractures 10, (4), 487-502, December 1974. 27. Timoshenko, S., Young, D. H., and Weaver, Jr., W. Vibration Problems in Engineering. John Wiley, New York: 1979. 28. Wilkinson, J. H. The Algebraic Eigenvalue Problem. Oxford: Clarendon Press, 1965. 29. Chung, J. and Hulbert, G.M., “A family of single-step Houbolt time integration algorithms for structural dynamics”, Comp. Meth. in App. Mech. Engg., 118, 1994. 30. Shih, C.F., Moran B. and Nakamura K., “Energy release rate along a three-dimensional crack front in a thermally stressed body”, International Journal of Fracture, vol. 30, pp. 79–102, 1986. 31. Anderson, T.L., Fracture Mechanics: Fundamentals and Applications (2nd ed.) CRC Press, 1995. 32. Yoon, J.W., Yang, D.Y. and Chung, K., “Elasto-plastic finite element method based on incremental deformation theory and continuum based shell elements for planar anisotropic sheet materials”, Comp. Methods Appl. Mech. Eng., 174, 23 (1999). 33. Shih, C.F. and Asaro, R.J., “Elastic-Plastic Analysis of Cracks on Bimaterial Interfaces: Part I – Small Scale Yielding”, Journal of Applied Mechanics, Vol. 110, pp. 299–316, June 1988. 34. Krueger, R., “Virtual Crack Closure Technique: History, Approach and Applications”, Appl. Mech. Rev., Vol. 57:2, pp. 109–143, March 2004. 35. Knops, B., “Numerical Simulation of Crack Growth in Pressurized Fuselages”, Doctoral thesis, Faculty of Aerospace Engineering, Delft University of Technology, The Netherlands, 1994.

Main Index

CHAPTER 5 223 Structural Procedure Library

36. Chung, J. and Hulbert, G.M., “A time integration algorithm for structural dynamics with improved numerical dissipation: The Generalized-α Method”, Journal of Applied Mechanics, Vol. 60, pp. 371 - 375, June 1993. 37. Hilber, H.M., Hughes, T.J.R., and Taylor, R.L., “Improved Numerical Dissipation for Time Integration Algorithms in Structural Dynamics”, Earthquake Engineering and Structural Dynamics, Vol. 5, pp. 283-292, 1977 38. Wood, W.L., Bossak, M., and Zienkiewicz, O.C., “An Alpha Modification of Newmark’s Method”, International Journal for Numerical Methods in Engineering, Vol., 15, pp. 1562-1566, 1981. 39. J. Reeder, 3D Mixed-Mode Delamination Fracture Criteria - An Experimentalist's Perspective. Proceedings of American Society for Composites, 21st Annual Technical Conference, Dearborn, Michigan, 2006. 40. M.L. Benzeggagh and M. Kenane, Measurement of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed-Mode Bending Apparatus, Composites Science and Technology, vol. 56, pp. 439-449, 1996. 41. Yih-Farn Chen, Modeling Analysis of Defect Formation during Thick Laminate Compression Molding Process, Presented at the American Helicopter Society 58th Annual Forum, Montreal, Canada, June 11-13, 2002. 42. Bogetti, T. A., Gillespie, J. W., 1992 Process-Induced Stress and Deformaton in Thick Section thermoset Composite Laminates, Journal of Composite Materials, 26, 626-660. 43. Lee, W.I., A. Loos and G.S. Springer. 1982 Cure Kinetics and Viscosity of Fiberite 976 Resin," Journal of Composite Materials , 21; 243-261. 44. S.N. Lee, M.T. Chiu, and H.S. Lin, 1992 Kinetic Model for the Curing Reaction of a Tetraglycidyl Diamino Diphenyl Methane/Diamino Diphenyl Sulfone (TGDDM/DDS) Epoxy Resin System, Polymer Engineering and Science 32 (15); pp. 1037-1046. 45. T. G. Gutowski, et al. The consolidation of laminate composites, Journal of Composite Materials, Vol. 21, February 1987, pp. 172 – 187. 46. W. B. Young, Consolidation and cure simulations for laminated composites, Polymer Composites, February 1996, Vol. 17, No. 1, pp. 142 – 148 47. Min Li and Charles Tucker, Optimal Curing for Thermoset Matrix Composites : Thermochemical and Consolidation Considerations, Polymer Composites, Aug. 30, 2001 48. S. R. White and H.T. Hahn, 1992 Process Modeling of Composite Materials: Residual Stress Development during Cure. Part I. Model Formulation, Journal of Composite Materials, 26, 24022422. 49. J.M. Kenny, 1992 Integration of Process Models with Control and Optimization of Polymer Composites Fabrication, Proceedings of the Third Conference on Computer Aided Design in Composite Materials Technology, pp. 530-544. 50. E.P. Scott, 1991 Determination of Kinetic Parameters Associated with the Curing of Thermoset Resins Using Dielectric and DSC Data, Composites: Design, Manufacture, and Application, ICCM/VIII, Honolulu, 1991, pp. 10-0- 1-10.

Main Index

224 Marc Volume A: Theory and User Information

51. George S. Springer, Resin Flow During the Cure of Fiber Reinforced Composites, Journal of Composite Materials 1982 16: 400-410. 52. P. Hubert, 1996 Aspects of Flow and Compaction of Laminated Composite Shapes During Cure, Ph.D. Thesis, The University of British Columbia, Vancouver, B.C.

Main Index

Chapter 6 Nonstructural Procedure Library

6

Main Index

Nonstructural Procedure Library J

Heat Transfer

J

Diffusion

J

Hydrodynamic Bearing

J

Electrostatic Analysis

J

Magnetostatic Analysis

J

Electromagnetic Analysis

J

Piezoelectric Analysis

J

Acoustic Analysis

J

Fluid Mechanics

J

Coupled Analyses

J

References

226

289

343

291 295 300 304

309

312 314 323

226 Marc Volume A: Theory and User Information

This chapter describes the nonstructural analysis procedures available in Marc. These are comprised of several areas including heat transfer, hydrodynamic bearing, electrostatic, magnetostatic, electromagnetic, piezoelectric, fluid mechanics, and coupled analysis. This chapter provides the technical background information as well as usage information about these capabilities.

Heat Transfer Marc contains a solid body heat transfer capability for one-, two-, and three-dimensional, steady-state and transient analyses. This capability allows you to obtain temperature distributions in a structure for linear and nonlinear heat transfer problems. The nonlinearities in the problem may include temperaturedependent properties, latent heat (phase change) effect, heat convection in the flow direction, and nonlinear boundary conditions (convection and radiation). The temperature distributions can, in turn, be used to generate thermal loads in a stress analysis. Marc can be applied to solve the full range of two- and three-dimensional transient and steady-state heat conduction and heat convection problems. Marc provides heat transfer elements that are compatible with stress elements. Consequently, the same mesh can be used for both the heat transfer and stress analyses. Transient heat transfer is an initial- boundary value problem, so proper initial and boundary conditions must be prescribed to the problem in order to obtain a realistic solution. Marc accepts nonuniform nodal temperature distribution as the initial condition, and can handle temperature/time-dependent boundary conditions. The thermal conductivity can be isotropic, orthotropic, or anisotropic. Both the thermal conductivity and the specific heat in the problem can be dependent on temperature; however, for conventional heat transfer, the mass density remains constant at all times. Latent heat effects (solid-tosolid, solid-to-liquid phase changes) can be included in the analysis. A time-stepping procedure is available for transient heat transfer analysis. Temperature histories can be stored on a post file and used directly as thermal loads in subsequent stress analysis. User subroutines are available for complex boundary conditions such as nonlinear heat flux, directional heat flux, convection, and radiation. A summary of Marc capabilities for transient and steady-state analysis is given below. • Selection of the following elements that are compatible with stress analysis: 1-D: three-dimensional link (2-node, 3-node) 2-D: planar and axisymmetric element (3-, 4-, and 8-node) 2-D: axisymmetric shells 3-D: solid elements (4-, 6-, 8-, 10-, 15-, and 20-node) 3-D: membrane elements (3-,4-, 6-, and 8-node) 3-D: shell elements (4- and 8-node) • Specification of temperature-dependent materials (including latent heat effects) is performed with the ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, TEMPERATURE EFFECTS, ORTHO TEMP, TABLE, and LATENT HEAT model definition options. • Selection of initial conditions is done using the INITIAL TEMP option. • Selection of the temperature and time-dependent boundary conditions (prescribed temperature history, volumetric flux, surface flux, film coefficients, radiation, change of prescribed temperature boundary conditions during analyses) is done using the FIXED TEMPERATURE, TEMP CHANGE, DIST FLUXES, POINT FLUX, QVECT, and FILMS options. Moving heat sources due to welding can be specified using the WELD FLUX, WELD PATH, and WELD FILL options.

Main Index

CHAPTER 6 227 Nonstructural Procedure Library

• Import of viewfactors calculated by Marc Mentat for radiation analyses. • Selection of time steps using the TRANSIENT or AUTO STEP history definition option. • Application of a tying constraints on nodal temperatures using the TYING model definition option. • Generation of a thermal load (temperature) file using the POST option, which can be directly interfaced with the stress analysis using the CHANGE STATE model definition option. • Use of the ANKOND user subroutines for anisotropic thermal conductivity, FILM or UFILM for convective and radiative boundary conditions or FLUX or QVECT for heat flux boundary conditions. • Selection of nodal velocity vectors for heat convection is done using VELOCITY and VELOCITY CHANGE options. • Use of the UVELOC user subroutines for heat convection. In addition, a number of thermal contact gap and fluid channel elements are available in Marc. These elements can be used for heat transfer problems involving thermal contact gap and fluid channel conditions. The CONRAD GAP option, used in conjunction with 4- and 8-node 2-D continuum elements or 8- and 20-node 3-D continuum elements, provides a mechanism for perfect conduction or radiation/convection between surfaces, depending on the surface temperatures. The perfect conduction capability in the elements allows for the enforcement of equal temperatures at nodal pairs and the radiation/convection capability allows for nonlinear heat conduction between surfaces, depending on film coefficient and emissivity. The perfect conduction is simulated by applying a tying constraint on temperatures of the corresponding nodal points. An automatic tying procedure has been developed for such elements. The radiation/convection capabilities in the elements are modeled by one-dimensional heat transfer in the thickness direction of the elements with variable thermal conductivity. For the purpose of cooling, the CHANNEL option allows coolant to flow through passage ways that often appear in the solid. The fluid channel elements are designed for the simulation of one-dimensional fluid/solid convection conditions based on the following assumptions: 1. Heat conduction in the flow direction can be neglected compared to heat convection; 2. The heat flux associated with transient effects in the fluid (changes in fluid temperature at a fixed point in space) can be neglected. For high velocity air flow, these assumptions are reasonable and the following approach is used: Each cooling channel is modeled using channel elements. On the sides of the channel elements, convection is applied automatically. The film coefficient is equal to the film coefficient between fluid and solid, whereas the sink temperature represents the temperature of the fluid. A two-step staggered solution procedure is used to solve for the weakly coupled fluid and solid temperatures.

Thermal Contact The CONTACT and THERMAL CONTACT options may also be used to define the fluxes entering the surfaces. For more information, see Chapter 8 in this volume.

Main Index

228 Marc Volume A: Theory and User Information

Convergence Controls Use the CONTROL model definition option to input convergence controls for heat transfer analysis. These options are: 1. Maximum allowable nodal temperature change. This is used only for transient heat transfer analysis in conjunction with an automatic time stepping scheme. It controls the time step size. 2. Maximum allowable nodal temperature change before properties are re-evaluated and matrices reassembled. This is used only for transient heat transfer analysis in conjunction with an automatic time stepping scheme. For mildly nonlinear problems, if the time step remains constant, the operator matrix is not reassembled until this value is reached. 3. 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 instance, for latent heat or radiation boundary conditions). When nonzero, this control is used for both steady state and transient heat transfer analysis when either the fixed or adaptive stepping procedures are used.

Steady State Analysis For steady state problems, use the STEADY STATE history definition option. If the problem is nonlinear, use the tolerance for temperature estimate error on the CONTROL model definition set to obtain an accurate solution. You must distinguish between two cases of nonlinearity in steady-state solutions: mild nonlinearities and severe nonlinearities. In the case of mild nonlinearities, variations are small in properties, film coefficients, etc., with respect to temperatures. The steady-state solution can be obtained by iteration. After a small number of iterations, the solution should converge. The technique described above is not suitable for severe nonlinearities. Examples of severe nonlinearities are radiation boundary conditions and internal phase-change boundaries. In these cases, you must track the transient with a sufficiently small time step ( Δt ) to retain stability until the steady-state solution is reached. Clearly, the choice of Δt is dependent on the severity of the nonlinearity. The number of steps necessary to obtain the steady-state solution can often be reduced by judicious choice of initial conditions. The closer the initial temperatures are to the steady-state, the fewer the number of increments necessary to reach steady-state.

Transient Analysis Both fixed stepping and adaptive stepping schemes are available for transient heat transfer analysis. The fixed stepping scheme is TRANSIENT NON AUTO. The adaptive stepping schemes are TRANSIENT and AUTO STEP. In the fixed stepping scheme, the program is forced to step through the transient with a fixed time step that is user specified. Only the error in temperature estimate (convergence control 3) is used with the fixed stepping scheme and the first two convergence controls are not checked.

Main Index

CHAPTER 6 229 Nonstructural Procedure Library

The scheme for the TRANSIENT option is as follows: 1. After the program obtains a solution for a step, it calculates the maximum temperature change in the step and checks this value against the allowable temperature change per step given on the CONTROL option (convergence control 1). 2. If the actual maximum change exceeds the specified value, the program repeats the step with a smaller time step and continues repeating this step until the maximum temperature change is smaller than the specified value or until the maximum number of recycles given on the control option is reached (in which case the program stops). 3. If the actual maximum temperature change is: a. between 80 percent and 100 percent of the specified value, the program goes on to the next step, using the same time step. b. between 65 percent and 80 percent of the specified value, the program tries the next step with a time step of 1.25 times the current step.If the actual maximum is below 65 percent of the specified value, the program tries the next step with a time step that is 1.5 times the current step. The objective of the scheme is to increase the time step as the analysis proceeds. The TRANSIENT option can be used for both heat transfer as well as thermo-mechanical coupled analysis. The time step for coupled analyses is only based on the convergence characteristics of the heat transfer pass. The AUTO STEP option is a unified time-stepping scheme that is available for thermal, mechanical and thermo-mechanically coupled analysis. The time step for coupled analyses is based on the convergence characteristics of each of the heat transfer and structural passes. Details of the AUTO STEP scheme are provided in Chapter 11. Technical Background Let the temperature T ( x ) within an element be interpolated from the nodal values T of the element through the interpolation functions N ( x ) , T ( x ) = N ( x )T

(6-1)

The governing equation of the heat transfer problem is C ( T )T· + K ( T )T = Q

(6-2)

In Equation (6-2), C ( T ) and K ( T ) are the temperature-dependent heat capacity and thermal conductivity matrices, respectively, T is the nodal temperature vector, T· is the time derivative of the temperature vector, and Q is the heat flux vector. The selection of the backward difference scheme for the discretization of the time variable in Equation (6-2) yields the following expression:

Main Index

230 Marc Volume A: Theory and User Information

1 1 ----- C ( T ) + K ( T ) T n = Q n + ----- C ( T )T n – 1 Δt Δt

(6-3)

Equation (6-3) computes nodal temperatures for each time increment Δ ( t ) . For the evaluation of temperature-dependent matrices, the temperatures at two previous steps provide a linear (extrapolated) temperature description over the desired interval τ T ( τ ) = T ( t – Δt ) + ----- ( T ( t – Δt ) – T ( t – 2Δt ) ) Δt

(6-4)

This temperature is then used to obtain an average property of the material f over the interval to be used in Equation (6-3), such that t

1 f = ----Δt

∫

f [ T ( τ ) ]dτ

(6-5)

t – Δt

During iteration, the average property is obtained based on the results of the previous iteration: τ T ( τ ) = T ( t – Δt ) + ----- ( T* ( t ) – T ( t – Δt ) ) Δt

(6-6)

T* ( t ) are the results of the previous iteration.

Temperature Effects The thermal conductivity, specific heat, and emissivity in a heat transfer analysis can depend on temperatures; however, the mass density remains constant. Specify reference temperature values of thermal conductivity, specific heat, mass density, and emissivity with the ISOTROPIC option. Enter temperature variations of both the thermal conductivity and specific heat using the TEMPERATURE EFFECTS or the TABLE option. This option also allows input of latent heat information. The temperature-dependent data can be entered using either the slope-break point representation or the property versus temperature representation. During analysis, an extrapolated/interpolated averaging procedure is used for the evaluation of temperature-dependent properties. Latent heat can be induced because of a phase change that can be characterized as solid-to-solid, solidto-fluid, fluid-to-solid, or a combination of the above, depending on the nature of the process. Phase change is a complex material behavior. Thus, a detailed modeling of this change of material characteristic is generally very difficult. The use of numerical models to simulate these important phenomena is possible; several major factors associated with phase change of certain materials have been studied numerically. The basic assumption of the latent heat option in Marc is that the latent heat is uniformly released in a temperature range between solidus and liquidus temperatures of the materials (see Figure 6-1). Marc uses a modified specific heat to model the latent heat effect. If the experimental data is sufficient and available, a direct input of the temperature-dependent specific heat data (see Figure 6-2) can be used. Results of both approaches are comparable if the temperature increments are relatively small.

Main Index

CHAPTER 6 231 Nonstructural Procedure Library

Specific Heat

Latent Heat Uniformly Release Between ST and LT

ST – Solidus Temperature LT – Liquidus Temperature

ST

LT

Temperature

Modeling Phase Changes with the Latent Heat Option

Specific Heat

Figure 6-1

Temperature

Figure 6-2

Modeling Phase Changes with the Specific Heat Option

Initial Conditions In a transient heat transfer analysis, Marc accepts nonuniform nodal temperature distribution as the initial condition. Enter the initial condition through the INITIAL TEMP model definition option or through the USINC user subroutine. Initial conditions are not required in steady-state heat transfer analysis, even though they can improve convergence when temperature-dependent properties are included.

Boundary Conditions There are two types of boundary conditions in transient/steady-state heat transfer analysis: prescribed nodal temperatures and nodal/element heat fluxes. These boundary conditions are entered directly through input or through user subroutines. Prescribe nodal temperatures using the FIXED TEMPERATURE model definition option. These prescribed temperatures are constant with time unless a time dependent table is referenced, the FORCDT user subroutine is invoked, or a TEMP CHANGE history definition option is encountered. The POINT FLUX model definition option allows you to enter concentrated (nodal) heat fluxes such as heat source and heat sink. These applied fluxes are constant with time unless a time dependent table is referenced, the FORCDT user subroutine or a POINT FLUX history definition option is encountered.

Main Index

232 Marc Volume A: Theory and User Information

The DIST FLUXES or QVECT model definition option allow the definition of distributed (surface or volumetric) heat flux. These applied fluxes may be spatially varying by an invoked spatial table or by the use of the FLUX or UQVECT user subroutine. These applied fluxes are constant with time unless a time dependent table is referenced, the FLUX or UQVECT user subroutine is invoked, or a DIST FLUXES history definition option is encountered. A special case is the volumetric heat generated by inelastic loads. This will be calculated by the program when the distributed flux type is 101. It may also be necessary to include the CONVERT option. For spatially varying fluxes associated with a welding heat source, it is more convenient to use the WELD FLUX model definition option. Specialized welding related options are discussed in the next section. Notes:

In heat transfer analysis, you must always specify total values; for example, total temperature boundary conditions or total fluxes. This specification is to be used consistently for the heat transfer portion of analysis on coupled thermal-mechanical (thermal-solid), fluid-thermal, and fluid-thermal-solid. The time variation used for thermal boundary conditions is a function of the stepping procedure that is used. If adaptive stepping (either TRANSIENT or AUTO STEP) is used, thermal boundary conditions are applied instantaneously. If fixed stepping (TRANSIENT NON AUTO) is used, the magnitudes of the thermal boundary conditions are applied in accordance with the tables used to define them.

Use the FILMS model definition option to input the constant film coefficient and the ambient temperature associated with the convective boundary conditions. Use the FILM user subroutine for time/temperaturedependent convective boundary conditions. When not using the table input option, the expression of the convective boundary condition is q = H ( Ts – T∞ )

(6-7)

where q , H , T s , and T ∞ are heat flux, film coefficient, unknown surface temperature, and ambient temperature, respectively. The radiative boundary condition can be expressed as 4 – T4 ) q = σε ( T sa ∞a

(6-8)

where q is the heat flux, σ is the Stefan-Boltzmann coefficient, ε is emissivity, and T s a and T ∞ a are unknown surface and ambient temperatures, respectively. The radiative boundary condition can be rewritten as 3 + T2 T 2 3 q = σε ( T sa sa ∞ a + T s a T ∞ a + T ∞ a ) ( T s – T ∞ )

= H ( σ, ε, T s, T ∞ ) ( T s – T ∞ )

Main Index

(6-9)

CHAPTER 6 233 Nonstructural Procedure Library

This shows that the radiative boundary condition is equivalent to a nonlinear convective boundary condition, in which the equivalent film coefficient H ( σ, ε, T s, T ∞ ) depends on the unknown surface temperature T s . When using the nontable driven input, this case requires the FILM user subroutine. When using the table driven input, the distributed thermal flux into an element may be defined as: α

4

4

q = H ( T s – T ∞ ) + H n v ( T s – T ∞ ) + e v f ⋅ εσ ( T s a – T ∞ a ) + f

(6-10)

where: H

is the conventional film coefficient

Ts

is the unknown surface temperature

T∞

is the sink temperature

T s a is the unknown surface temperature in absolute units T ∞ a is the sink temperature in absolute units H n v is the natural convection coefficient α

is the natural convection exponent

ev f

in the effective view factor to the environment; usually equal to 1.0

ε

is the emissivity

σ

is the Stefan Boltzman constant

f

is the distributed flux from other sources

The absolute temperature is the temperature in user units plus the offset, which is defined in the PARAMETERS model definition option.

A surface flux may be entered on the FILMS model definition option using the table driven input or the DIST FLUXES model definition option. If both convective behavior and other terms contributing to the flux are present it is computationally efficient to do it here. When using table driven input, all coefficients given above may be temperature dependent by referencing a table. If more complex physical boundary conditions exist, then the UFLIM user subroutine should be used. When using the table driven input, an alternative method is available for defining the sink temperature through the use of the SINK POINTS model definition option. This allows the user to interface to exterior fluid/thermal programs to input spatially varying environment temperatures. In Figure 6-3, temperatures may be known at the points marked with an X. Using the SINK POINTS model definition option when evaluating the flux into an element, the program will first determine the closest sink point to the surface integration point, and then use this sink point temperature in the calculation.

Main Index

234 Marc Volume A: Theory and User Information

x x

x

x

x

x

Figure 6-3

x

x

Temperature Points

If the heat flux defined in the FLUX or FORCDT user subroutine is temperature dependent, then the convergence behavior of the solution process of the set of nonlinear equations can be improved by defining not only the current flux value, but also the derivative of the flux with respect to temperature. Based on this derivative, Marc adapts the conductivity matrix K ( T ) as well as the heat flux vector Q . This is done by rewriting the heat flux using a Taylor series expansion. For a temperature dependent point flux on node i , the flux during iteration n is thus given by: i

dq i i i i q n = q n – 1 + ⎛ -------⎞ ( T – Tn – 1 ) ⎝ dT ⎠ n – 1 n

(6-11) i

Since all the terms in Equation (6-11) except for T n are known from iteration n – 1 , the corresponding entries in the conductivity matrix and heat vector are updated as: i

ii ii dq K n → K n – ⎛⎝ -------⎞⎠ dT n – 1

(6-12)

i

i i i dq Q n → Q n – ⎛ -------⎞ T ⎝ dT ⎠ n – 1 n – 1

(6-13)

The temperature dependent distributed fluxes are treated in a similar way and require the FILM user subroutine. If a film coefficient is temperature dependent, then, similar to temperature dependent fluxes, defining the derivative of the film coefficient with respect to temperature may speed up the convergence of the iterative process. This derivative should be defined in the FILM user subroutine. The QVECT option may be used to define a directed flux into the surface. The user specifies a magnitude q 0 and an orientation n . The magnitude of the flux applied is then Q = – q 0 ⋅ αA ⋅ n ⋅ n s where A is ˜ ˜ the area of the surface, α is the face absorptivity, and n s in the outward unit normal into the surface. The absorptivity is defined through the EMISSIVITY option. Note that when using heat transfer membranes or shell element, the normal is based upon the right-hand rule. For both the FILMS and QVECT option using table driven input, the coefficients used in the expressions may be temperature dependent or dependent upon other quantities. For FILMS, this lead to: q = H ( Te v a l ) ⋅ ( Ts – T∞ )

Main Index

CHAPTER 6 235 Nonstructural Procedure Library

and for QVECT, this leads to: q = q0 ( Te v a l ) ⋅ α ( Te v a l ) ⋅ A ( n ⋅ ns ) ˜ The user can specify that the evaluation temperature be either at the surface (TEMTYP=0), the average of the surface and environment temperature (TEMPTYP=10), or the environment temperature (TEMPTYP=20). Furthermore, for the FILMS option, one can specify that the environment temperature at a control node; in which case, q = H ( Te v a l ) ⋅ ( T s – T ∞ ( T c n t r l n d ) ) Control Systems Often in heat transfer, one desires that a boundary condition is dependent upon the temperature at another point. In HVAC systems, this is driven by the temperature at the thermostat (multiple thermostats). If multiple thermostats are involved, an effective temperature should be obtained by using a Servo Link. If a control node is specified, then the following boundary conditions are applied: Point Flux

q = Q ( Tc n t r l n d )

FLUXTYPE=6

q = Q ⋅ Tc n t r l n d

FLUXTYPE=4

Distributed Flux

q = qa ( Tc n t r l n d ) ⋅ A

FLUXTYPE=6

q = qa ⋅ Tc n t r l n d ⋅ A

FLUXTYPE=4

Film

q = H ( Te v a l ) ⋅ ( T s – T ∞ ( T c n t r l n d ) )

FLUXTYPE=6

q = H ⋅ ( Te v a l ) ⋅ Tc n t r l n d ⋅ ( Ts – T∞ )

FLUXTYPE=4

QVECT

q = qo ( Tc n t r l n d ) ⋅ α ( Te v a l ) ⋅ A ⋅ ( n – ns ) ˜ ˜ q = qo ⋅ Tc n t r l n d ⋅ α ( Te v a l ) ⋅ A ⋅ ( n – ns ) ˜ ˜

FLUXTYPE=6 FLUXTYPE=4

The FLUXTYPE is specified in the respective options. FLUXTYPE=4 is compatible with Nastran definition of control node.

Main Index

236 Marc Volume A: Theory and User Information

Velocity and Pressure Dependent Convection In many applications, the convective coefficients are dependent upon the external fluid boundary conditions. In such cases, one can express: q = H ( T e v a l ,V ,P ) ⋅ ( T s – T ∞ ) where P and V are the pressure and the velocity of the flow field. This simulation can be done by using the VELOCITY option to define the velocity and the FIXED PRESSURE option to define the pressure at the nodal points on the boundary. This data is then interpolated to the integration points where it is used to evaluate the function/table describing H. Furthermore, in a transient simulation where the velocity and pressure are a function of time, the VELOCITY and FIXED PRESSURE option may be used to define the temporal variation. In the most general case, one then has: q = H ( T e v a l ,V ( t ) ,P ( t ) ,t ) ⋅ ( T s – T ∞ ( t ) ) If spatial variation is also required, then the UFILM user subroutine is required.

Surface Energy The SURFACE ENERGY option calculates contributions to the thermal boundary conditions, including the recession due to thermochemical ablation at the surface of a material which is subjected to very high thermal fluxes. This includes the effects of convective heat flux with a possible blowing effect by mass injection, an enthalpy flux due to molecular diffusion, a thermochemical ablation due to heterogeneous chemical reactions with gases, a possible thermal internal decomposition, a thermochemical ablation and a mechanical erosion by liquid or solid particles impacts. Surface energy allows one to obtain the recession due to thermochemical ablation by gases or particles. The mechanical erosion must be calculated by use of a UFLUXMEC user subroutine, and added to the thermochemical ablation in order to obtain the total surface recession. Surface energy is coupled with the heat transfer into the material by the conductive heat flux, and possibly with the mass flow rate towards the surface due to water evaporation and/or thermal decomposition gases generated inside the material. The SURFACE ENERGY option may be used in any heat transfer analysis, but depending on the model, some terms could be null. When used in conjunction with the THERMO-PORE option for materials undergoing pyrolysis, most of the terms are nonzero. The PRINT,15 parameter allows the printing of each contribution to the surface energy.

Main Index

CHAPTER 6 237 Nonstructural Procedure Library

Thermochemical Ablation and Surface Energy Balance Physical Presentation convection

diffusion

radiative balance

blowing

particles impact

flow surface

wall

conduction

Figure 6-4

decomposition

ablation by gases

ablation by particles

Schema of the Surface Energy Balance

Surface Energy Balance The surface energy balance is summarized by this equation: Convection + Enthalpy flux due to external chemical species diffusion effects + Enthalpy flux due to thermochemical ablation by gases + Enthalpy flux due to internal thermal decomposition products flow – Enthalpy flux due to blowing of gaseous products + Enthalpy flux due to thermochemical ablation by impacting particles + Thermal effects of mechanical erosion by impacting particles – Enthalpy flux due to mechanical removal of liquid phases at the surface + Radiative heat transfer balance – Thermal conduction = 0

Mathematical Presentation The equation below is noted Φ c o n v ( x ,t ,T s ) + Φ d i ff ( x ,t ,T s ) + Φ s ,t h ,g ( x ,t ,T s ,m· s ,t h ) + Φ g ( x ,t ,T s ,m· g ,p ,m· g ,w ) – Φ b l o w ( x ,t ,T s ,m· g ,p ,m· g ,w ,m· s ,t h ) – Φ l i q ( x ,t ,T s ,m· l ,j ) + Φ s ,t h ,p ( x ,t ,T s ,m· p ,j ,… ) + Φ p a r t ,k i n ( x ,t ,T s ,m· p ,j ,… ) + Φ r a d ( x ,t ,T s ) – Φ c o n d ( x ,t ,T s ) = 0 It is homogeneous with a power per surface unit [ W.m – 2 ] . Details on Terms:

Main Index

Convection:

enthalpy flux at the surface due to processes of heat conduction in the boundary layer.

Diffusion:

enthalpy flux at the surface due to processes of chemical species diffusion in the boundary layer.

238 Marc Volume A: Theory and User Information

Thermochemical ablation by gases:

enthalpy flow associated to mass flow of thermochemically ablated material by gases.

Decomposition products flow:

enthalpy flow from inside of the material and ejected to the boundary layer without change of phase (generally pyrolysis gases and water).

Blowing:

enthalpy flux due to evacuation of gases freed both by thermochemical ablation (by both gaseous products and chemical effects of particle impacts) at the surface, and internal thermal decomposition (including possibly water evaporation).

Liquid phases removal:

enthalpy flow associated with the blowing of liquid phases possibly appearing at the surface, by external actions (flow, …)

Thermochemical ablation by external particles:

enthalpic flow associated with mass flow of thermochemically ablated material by surface impacting particles.

Thermal effects of mechanical erosion by impacts of particles:

enthalpy flow associated with energy given to the surface by impacting particles (fraction of conversed kinetic energy).

Radiative balance:

balance of radiative heat flux, resulting from absorption and emission.

Conduction:

apparent conductive flow within the material.

Each time that a upper-case H is used for an enthalpy, it means that is the total enthalpy, including both the formation enthalpy and the so-called sensible enthalpy. If we refer only to the sensible part, a lower-case h is used. In all cases, we refer to specific enthalpies J.kg – 1 . Equation of Each Term of the Energy Balance: Convection: α H ⎛ H r e c – H e ;T s⎞ ⎝ ⎠ with: α H = α H ( x ,t ,T s )

heat transfer coefficient (homogeneous with surface mass flow rate [ kg.m – 2 .s – 1 ] /specific enthalpy [ J.kg – 1 ] ). In some papers, α H is sometimes written as ρ e u e C H , with C H being the Stanton number for heat transfer, and ρ e u e the mass flow rate of the external flow parallel to the surface at the edge e of the boundary layer.

Main Index

CHAPTER 6 239 Nonstructural Procedure Library

H r e c = H r e c ( x ,t )

Ts Ts He ; = H e ; ( x ,t ,T s )

specific recovery enthalpy of the external flow ( [ J.kg – 1 ] ) . This quantity depends also implicitly on the external pressure. But this dependence is hidden behind the time dependence (because the pressure is itself a function of the time and the space variable). specific enthalpy of the external flow, calculated for the frozen chemical composition existing at the edge e of the boundary layer, but evaluated at the surface temperature T s . This term is calculated by neglecting the variation of the chemical composition of the external flow between the edge of the boundary layer and the wall, due to both chemical reactions in the gas phase, and molecular diffusion of chemical species in the boundary layer with possibly unequal mass diffusion coefficients for the species. Other diffusion effects of the second-order are neglected (Soret effect, Dufour effect). The non-neglected diffusion effects are taken into account in the diffusion term. This quantity depends also implicitly on the external pressure. But this dependence is hidden behind the time dependence (because the pressure is itself a function of the time and the space variable).

Often, a 'blowing correction' modifies the heat transfer coefficient. In fact, there are two possibilities: 1. the CFD software allows one to take into account the blowing in some manner, for instance by using a simplified subroutine representing the material behavior as a boundary condition. In that case, the coefficient α H ( x ,t ,T s ) is obtained directly. 2. the CFD software allows one to calculate only a heat transfer coefficient α H 0 for 'inert' wall (no blowing). So, this coefficient must be corrected in the thermal software. The usual correction is: 2κB' ; Ln ⎛ 1 + 2κB' ; ⎞ ⎝ CH αH v0 v⎠ ---------- = ---------- = --------------------------------------------- = ----------------------------------------CH αH 2κB' ; 0 0 exp ⎛ 2κB' ; – 1⎞ ⎝ ⎠ v v0 with: ( ρv ) w B' ; ≡ --------------v0 αH 0

( ρv ) w B' ; ≡ --------------αH v

κ is the ‘transpiration factor’. Usual values are κ = 0.5 for laminar flow and κ = 0.4 for turbulent flow. Marc has two options to enter the heat transfer coefficient: either directly α H or α H with the above 0

correction. For the latter, there is both the standard form above with κ as an entry in the data deck, and a UFAH user subroutine allowing one to enter another kind of correction.

Main Index

240 Marc Volume A: Theory and User Information

Ts Diffusion: α M ∑ ⎛ Z i ;* – Z i ;*⎞ H ⎝ e s⎠ i i

with: α M = α M ( x ,t ,T s )

mass transfer coefficient (homogeneous with surface mass flow rate [ kg.m – 2 .s – 1 ] /specific enthalpy [ J.kg – 1 ] ). In some papers, α M is sometimes written as ρ e u e C M ; C M being the Stanton number for mass transfer and ρ e u e the mass flow rate of the external flow parallel to the surface at the edge e of the boundary layer. Very often, C M (or α M ) is supposed to be correlated to C H (or α H ) by C M ≈ C H ( Le ) n , Le being the Lewis number for the frozen external flow. This Lewis number is often supposed to be equal to 1, so that C M ≈ C H and n is meaningless Otherwise, n depends on the configuration of the external flow, a value n = 2 ⁄ 3 is generally accepted. For the sake of generality, one can enter separate entry tables for α H and α M .

T

T

specific enthalpy of the chemical component i in the external flow, evaluated

H i s = H i s ( x ,t ,T s )

at the surface temperature T s ( [ J.kg – 1 ] ) .

Z i ;*e = Z i ;*e ( x ,t )

special fraction characterizing the component i in the chemical composition of the external flow at the edge e of the boundary layer. Z i ;*e has no dimension (no unit). It is a rather complicated algebraic combination of the mole fractions and the mass fractions of all the chemical species existing in the flow. These quantities depend also implicitly on the external pressure and on the temperature. But these dependencies are hidden behind the time dependence (because the pressure and the temperature of the flow are themselves functions of the time and the space variable). special fraction characterizing the component i in the chemical composition

Z i ;*s = Z i ;*s ( x ,t )

of the external flow near the surface s of the material. The difference between Z i ;*e and Z i ;*s characterizes the diffusion effects across the boundary layer. These quantities depend also implicitly on the external pressure and on the temperature. But these dependencies are hidden behind the time dependence (because the pressure and the temperature of the flow are themselves functions of the time and the space variable). The quantities

Ts

∑ Z i ;*e H i i

Main Index

( x ,t ,T s ) and

Ts

∑ Z i ;*s H i i

( x ,t ,T s ) are tabulated as a whole.

CHAPTER 6 241 Nonstructural Procedure Library

Thermochemical Ablation by External Gases: m· s ,t h ,g H s m· s ,t h ,g = m· s ,t h ,g ( x ,t ,m· g ,T s ) surface mass flow rate of thermochemically ablated surface material by the action of external gases ( [ kg.m – 2 .s – 1 ] ) . specific enthalpy of the solid material of the surface, evaluated at the H = H (T ) s

s

s

surface temperature T s ( [ J.kg – 1 ] ) .

A table gives H s as a function of T s , for each material possibly present at the surface. Decomposition Products Flow: m· g H g m· g = m· g ( x ,t )

Hg = Hg ( Ts )

surface mass flow rate of gaseous products produced internally by thermal decomposition (both pyrolysis and water evaporation, [ kg.m – 2 .s – 1 ] ). Note that if there is no pyrolysis in the model defined by the THERMO-PORE option, this term is zero. specific enthalpy of the gases taken into account in, evaluated at the surface temperature T s ( [ J.kg – 1 ] ) . This quantity is tabulated.

Blowing: ( ρv ) w H w with: ( ρv ) w = ( ρv ) w ( m· g ,m· s ,t h ,g m· s ,t h ,p )

H w = H w x ,t ,( T s, m· g m· s ,t h ,g m· s ,t h ,p )

surface mass flow rate of all gaseous products leaving the surface of the material (including gas coming from internal thermal decomposition [pyrolysis, water, …], thermochemical ablation by external gases, thermochemical ablation by impacting particles) [ kg.m – 2 .s – 1 ] . specific enthalpy of the mix of all gaseous products existing at the surface, including blowed gases and chemical species from the external flow, evaluated at the surface temperature T s ( [ J.kg – 1 ] ) .

For each point x and time t (discrete values), a table gives H w as a function of the mass flow rate of gaseous products coming from the inside (pyrolysis, water evaporation), the total mass flow rate coming from thermochemical ablation, and the surface temperature T s . Thermochemical Ablation by Impacting Particles: m· s ,t h ,p = f t h ,p ( T s ) ∑ G t h ,p ,j m· p ,j ΔH r ,p ,j with:

Main Index

242 Marc Volume A: Theory and User Information

m· p ,j m· p ,g ( x ,t ) G t h ,p ,j ΔH r ,p ,j

surface mass flow rate of particles for the j family

( [ kg.m – 2 .s – 1 ] ) . = G t h ,p ,j ( V p ,j ( x ,t ) ,D p ,j ,α p ,j ( x ,t ) ,… ) empiric law for thermochemical ablation by impacting particles (without unit) specific enthalpy of reaction for the interaction = ΔH r ,p ,j ( T s ,J ) between the surface material and the j family of particles ( [ J.kg – 1 ] ) .

f t h ,p = f t h ,p ( T s )

empiric correction for the effect of surface temperature (without unit)

The summation is based on families of particles. Each family j is characterized by an impacting mass flow rate, a velocity of impact V p ,j , an angle of impact α p ,j , and the mean diameter of the family D p ,j . The three first quantities are generally dependent on time, and on the location on the surface. The mass flow rate of the surface material ablated thermochemically by the family j is generally given by a correlation G t h ,p ,j ( V p ,j ,D p ,j ,α p ,j ) of these parameters (often called G-Law): m· s ,t h ,p ,j ( x ,t ) = G t h ,p ,j ( V p ,j ( x ,t ) ,D p ,j ,α p ,j ( x ,t ) )m· p ,j ( x ,t ) The correlation is established by experiments. The G-Law can be entered by a UGLAW user subroutine or a table.The total ablated mass flow rate m· s ,t h ,p is obtained by summing the above formula for the j families.For the sake of generality, all the families are not obliged to be composed by particles of the same chemical species. So it is more general to consider an enthalpy of reaction different for each family j : ΔH r ,p ,j . The enthalpy of reaction depends on the temperature of the surface T s This enthalpy of reaction is a property of both the surface material (which can be different depending on the location on the part to be calculated), and the family of particles p under consideration. It is attached to the material, and the family of particle j is considered as a parameter. This model does not take into account the effect of the temperature of the surface, as far as the ablated mass flow rate is concerned. An empiric correction has been proposed by several authors. The value given above (after summation on j ) must be corrected by multiplying it by a function of the surface temperature. Several functions have been proposed: Ts – T1 ⎧ ⎫ f 1 ( T s ) = ⎨ 0 if T s < T 1 ; ------------------- if T 1 < T s < T 2 ; 1 if T 2 < T s ⎬ – T T 2 1 ⎩ ⎭ Ts – T0 1 f 2 ( T s ) = --- tan h ⎛ -------------------⎞ + 1 ⎝ ΔT ⎠ 2

Main Index

CHAPTER 6 243 Nonstructural Procedure Library

1 with T 0 = --- ( T 1 + T 2 ) and ΔT = n ( T 2 – T 1 ) . 2 These two corrections are implemented in standard input, and an alternate UFTHP user subroutine allows one to enter other kinds of corrections. A last point is that m· p ,j ( x ,t ) generally comes from an aerothermal analysis (performed with a CFD software) at discrete times and are calculated on a mesh which does not match with the thermal mesh. The analysis provides as well other parameters such as V p ,j ( x ,t ) , D p ,j , α p ,j ( x ,t ) . For 3-D analysis, the proper angle α p ,j ( x ,t ) will be calculated within the CFD software (angle between the normal direction at the surface and the velocity vector, in the common plan defined by these two vectors). Thermal Effects of Particle Impacts: Φ p ,k with: φ p ,k = φ p ,k ( m· p ,j ( x ,t )V p ,j ( x ,t )D p ,j α p ,j ( x ,t ) ,… )

This term takes into account a possible energy deposit by the particles impacting the surface, besides the phenomena of thermochemical ablation and mechanical erosion. For instance, it could be due to a partial conversion into heat of the kinetic energy of the particles, during inelastic collisions. There does not seem to exist any general accepted law or formulation for this term. This effect is even neglected in many ablation models. So this term can only be introduced by a UTIMP user-subroutine.

Liquid Phases Removal: f t h ,p ∑ m· 1 H 1 · m 1 = m· 1 ( x ,t )

surface mass flow rate of liquid products formed at the surface of the material, and blowed out by the action of the external flow or other mechanisms ( [ kg.m – 2 .s – 1 ] ) .

H1 = H1 ( Ts )

specific enthalpy of the liquid phase 'l' taken into account in, evaluated at the surface temperature T s ( [ J.kg – 1 ] ) .

This term takes into account possible liquid phases appearing at the surface of the ablating material, by several mechanisms (phase change of a component of the material [silica, …], oxidation at the surface of gaseous products coming from the inside forming liquid phase [ SiO g → SiO 2 ] , for instance), and the blowing of these phases (gravity, shear stress, …). Moreover, this kind of phenomena would require a more complex modeling, for example with the explicit modeling of the liquid film running at the surface. Finally, there could exist a liquid film at the surface produced by other mechanisms such as impacts of many liquid particles. These quantities are tabulated, and a user-subroutine can be used to provide this flux as a whole.

Main Index

244 Marc Volume A: Theory and User Information

Radiative Balance: Φ r

ab

– Φr

em

This is defined through the FILMS or RAD-CAVITY option. Mass Conservation Equation: Mass flow blown (injected in the outflow) + mass flow of removed liquid phases = mass flow of internally produced gaseous products + mass flow of the gaseous products of thermochemical ablation reactions with external gases + mass flow of gaseous products of thermochemical ablation reactions with impacting particles. ( ρv ) w +

∑ m· 1

= m· s ,t h ,g + m· g + m· s ,t h ,p = m· s ,t h ,g + m· g + f t h ,g ∑ G t h ,p ,j m· p ,j

1

Velocity of Surface Recession Due to Thermochemical Ablation: The surface recession S· t h due to thermochemical ablation (and by extension due to other possible 'physical-chemical' mechanisms such as phase change or blowing of liquid phase) is only one part of the total surface recession S· . This part is calculated from the SEB. To obtain the total surface recession, it must be added the contribution of mechanical erosion S· m e c : S· = S· t h + S· m e c The contribution S· m e c must be calculated by other means. Velocity of surface thermochemical recession S· t h velocity of chemical thermochemical ablation by gases + velocity of thermochemical ablation by impacting particles (unit: m s-1) S· t h = [ m· s ,m e c ,p + m· s ,h ,p ] ⁄ ρˆ s with m· s ,t h ,p = f t h ,p ∑ G t h ,p ,j m· p ,j ρˆ s is the density of the solid, when pyrolysis is included through the THERMO-PORE option, this is the current density.

Mechanical Erosion The mechanical erosion is currently considered to be due both to impacts of particles, and to other external actions such as the shear stress of the flow, the vibrations of the part, … S· m e c = [ m· s ,m e c ,p + m· s ,m e c ,o t h ] ⁄ ρˆ s Mechanical Erosion by Particles The expression is similar to the one for thermochemical ablation by particles described above:

Main Index

CHAPTER 6 245 Nonstructural Procedure Library

m· s ,m e c ,p = f m e c ,p ∑ G m e c ,p ,j m· p ,j m· s ,m e c ,p

unit: kg m – 2 s – 1

f m e c ,p

without unit

G m e c ,p ,j

without unit

with here a mechanical 'G-Law' G m e c ,p ,j , and a similar temperature correction f m e c ,p . These two quantities may be defined through the UGMEC and UFMEC user subroutines, respectively. Alternatively, a UTIMP user-subroutine is provided for calculating m· s ,m e c ,p .

Mechanical Erosion by Other Actions There is no generally accepted expression for. And there are many possibilities depending on the kind of material and the environment. The UFLUXMEC user-subroutine is provided for calculating m· s ,m e c ,o t h .

Pyrolysis Pyrolysis involves the decomposition of materials due to thermal processes. There are two aspects of these simulations: the thermal-chemical decomposition of the material and the creation of gas and transport of this gas. The creation of the gas is based upon the conservation of mass. The material models used in these simulations have increasing levels of complexity. There are two models used to simulate the transport of the gas known as the streamline model and the D’Arcy fluid model. The choice of these two models is made on the PYROLYSIS parameter. In the streamline model, the gas moves along streamlines that are aligned with the mesh, as shown in Figure 6-5. This procedure is available for planar, axisymmetric and solid elements using either linear or quadratic interpolation functions. But, because the need for regular meshes, triangular and tetrahedral elements are not available. The user must identify which element contain streamlines. The streamline method introduces two new terms: streamlines and streamline integration points (SIP). For lower order elements, the SIP are at the intersection of the streamlines and the element edges. For higher order elements, an additional SIP exists midway between the two. The pyrolysis calculation occurs at the SIP. An extrapolation and interpolation procedure is used to move data from the SIP to conventional integration points (CIP). The pyrolysis gas m· g moves from SIPi to SIPi+1. If the temperature becomes hotter in the interior, such that flow of gases would reverse, an error would occur. When using the D’Arcy law model, any solid heat transfer element may be used. When this method is used, the pyrolysis calculation occurs at the CIP. The pyrolysis gas may move in any direction.

Main Index

246 Marc Volume A: Theory and User Information

SFIP node

SIPi+1

SIPi

CIP Regular Mesh SIP Streamline Integration Point CIP Conventional Integration Point SFIP Surface Integration Point Figure 6-5

Streamlines

Presentation of the Mass Equation The conservation of mass equation for the streamline model yields: ∂ρˆ s ,p * ∂ρˆ l ∂ρˆ s ,c ,c * ∇.m· g = – --------------- – -------- – ------------------∂t ∂t ∂t where the first term is the conventional generation (source) term due to a change in density of the solid, the second term represent the change in density of initial water vapor, and the final term is due to change in density due to coking.

Main Index

m· g

mass flow rate of the gases of decomposition = ρˆ g υ g .

ρˆ g

mass density of the pyrolysis gas.

ρˆ s ,p *

mass density of the solid undergoing pyrolysis.

ρˆ l

mass density of the liquid vapor.

ρˆ s ,c ,c *

mass density of the coked solid.

υg

velocity of the pyrolysis gas.

CHAPTER 6 247 Nonstructural Procedure Library

∂ρˆ s ,p * – --------------∂t

source term of decomposition.

∂ρˆ s ,c ,c * – ------------------∂t

source term of carbon deposit.

∂ρˆ l – -------∂t

source term of water drying.

The drying of the initial water vapor occurs before the pyrolysis occurs so: ∂ρˆ l ∇.m· g ,w = – -------∂t The global mass equation is defined as the sum of these. The global mass flow rate m· g is equal to m· g ,p + m· g ,w . Principle of Pyrolysis When pyrolysis occurs, the solid material is degraded due to the effect of the temperature. This degradation is done in steps (Figure 6-6), according to the temperature. We represent these steps on the drawing below. With each step a loss of density corresponds: Δρˆ s ,p ,j . ρˆ s ρˆ s ,p ,v Δρˆ s ,p ,1

Δρˆ s ,p ,3 ρˆ s ,p ,c

Temperature Figure 6-6

Degradation Steps

The density of material ρˆ s thus varies from ρˆ s ,p ,v , density of virgin material to ρˆ s ,p ,c , the density of charred (entirely pyrolyzed material). If coking occurs the density increases because carbon is redeposited in the solid

Main Index

248 Marc Volume A: Theory and User Information

We define a dimensionless variable ϕ j which varies from 1 to 0 during pyrolysis (it represents the advancement of pyrolysis). It is calculated by the law of Arrhenius: ∂ϕ j – T a ,j ψ -------- = – B j exp ⎛⎝ ------------⎞⎠ ϕ j j . ∂t Ts The coefficients B j , T a ,j , and ψ j are determined by thermogravimetry (TGA). The material properties associated with each phase (virgin, charred, coked, liquid, gas) are entered through the ISOTROPIC or ORTHOTROPIC options. The THERMO-PORE option is used to reference these phases and provide additional material data including the terms of the Arrhenius series. ∂ρˆ s ,p * This variable ϕ j facilitates the calculation of the variation in solid density due to pyrolysis, --------------- , ∂t which is the sum of the preceding ϕ j law of Arrhenius: ∂ρˆ s ,p * --------------- = ∂t

Nd

∑

∂ϕ j ( Δρˆ ) s ,p ,j -------- = – ∂t

j = 1

Nd

⎛

– T a ,j ⎞

ψ

- ϕ ∑ ( Δρˆ ) s ,p ,j B j exp ⎝ ----------Ts ⎠ j

j

j–1

or ∂ρˆ s ,p * --------------- = ∂t

Nd

∑ j = 1

∂ϕ j ( Δρˆ ) s ,p ,j -------- = – ∂t

Nd

∑ j = 1

– E a ,j ψ ( Δρˆ ) s ,p ,j B j exp ⎛ ------------⎞ ϕ j j ⎝ R*T⎠

where Nd

is the number of terms in the Arrhenius series.

T a ,j

is the temperature of activation of the reactions of decomposition

ψj

is the order of the reaction

ϕj

dimensionless variable of decomposition varying from 1 to 0 during pyrolysis

Bj

is a factor to the exponential

E a ,j

is the energy of activation of the reaction j of decomposition,

( Δρˆ ) s ,p ,j

represents the reduction of density (counted in positive quantity)

Ts

is the local temperature of the solid phase.

R

is the perfect gas constant.

It is assumed that at a point thermal equilibrium occurs and the temperature of the solid and the gas are the same.

Main Index

CHAPTER 6 249 Nonstructural Procedure Library

Alternative Formulation We see in the literature an alternative writing of the Arrhenius law know as the rho law: δρˆ s ,p ------------ = δt

Nd

∑ j = 1

ψ T a ,j ⎛ ρˆ s ,p ,j – ρˆ s, c ,j⎞ j – Γ j B' j exp ⎛ – ---------⎞ ρˆ s ,v ,j ⎜ --------------------------------⎟ ⎝ T ⎠ ρˆ ⎝ ⎠ s ,v ,j

where: ρˆ s ,v ,j

is the virgin j material density.

ρˆ s ,c ,j

is the charred j material density.

ρˆ s ,p ,j

is the current j material density.

The user can enter the input for Arrhenius law for the both laws. If he chooses the rho law, then he must give: Nd, Γ , B' , E ψ , ρˆ s ,v ,j, ρˆ s ,c ,j . If he chooses the ϕ law, then he must give: j

j

a ,j

j

j

Nd, Δρˆ s ,p ,j, B j, E a ,j, ψ j . One can define an alternate model for pyrolysis using the UPYROLSL user subroutine.

Coking The processes considered when the material is heated are very complex. For instance, we can consider the primary pyrolysis chemical reactions producing gases, and the subsequent secondary chemical reactions, between gases, between gases and solid, and between constituents in the solid phase. We focus here on one class of secondary chemical reactions, namely the heterogeneous reactions between gases and porous solid leading to a carbon deposit, known as coking phenomenon. The processes mentioned above are governed by complex sets of kinetically controlled chemical reactions, which are neither well known, nor the constants associated with them. One Term Arrehenius Model ˜ c g in the gaseous phase, In this model, we consider the total mass fraction of atomic element carbon K independently of the molecular configuration (chemical specie) in which it is present. The initial value ˜ c g 0 , corresponding to the gases generated by the initial primary pyrolysis chemical reactions, is data K that can be determined experimentally by calculating the difference in carbon content between the ˜ c g m· is the mass flow rate virgin material and the one of the char before coking. We should note that K g

of atomic element carbon independently of the molecular configuration. This model is inspired by a paper written by R.A. Rindal [Ref. 20].

Main Index

250 Marc Volume A: Theory and User Information

During the subsequent process of secondary gas/gas chemical reactions, this quantity does not change, because only the molecular configurations are changing in the gaseous phase, but not the content in any ˜ cg0 . ˜ cg = K atomic element: K It is known that the gaseous phase at lower temperature contains more carbon than it would contain in the case of chemical equilibrium. When the gases flow towards the heated surface, the temperature is rising; the rate of reactions is rising too, and the composition of gases approaches the one corresponding ˜ c g is to chemical equilibrium. It results in a deposit of solid carbon (coking), and then the quantity K changing in the zone where coking occurs. From the considerations above, it seems reasonable to assume that the potential of coking is driven by ˜ c g and the value of K ˜ c g E at chemical equilibrium, and that the the difference between the local value K rate with which chemical equilibrium is approached is of Arrhenius kind. Furthermore, the homogenous chemical reactions in the gaseous phase are generally not equimolar, so that a pressure dependence and an order of reaction different from the unity are assumed. So, the following kinetic equation for the ˜ c g is proposed: evolution of the quantity K ˜ cg –Ea c n n ∂K ˜ cg – K ˜ cgE) c ------------- = – k c exp ⎛⎝ ------------⎞⎠ ( P ) c ( K ∂t RT with: k c, E a c, n c :

kinetic coefficients for coking reactions.

˜ cg : K

total mass fraction of the atomic element carbon in the pyrolysis gas.

˜ cgE : K

total mass fraction of the atomic element carbon in the pyrolysis gas when chemical equilibrium is achieved.

˜ c g E can be calculated using standard thermochemical calculation software. The quantity K The streamline model does not give access to the value of the local pressure P . There are two assumptions that can be made: • either neglect the pressure dependence, by setting P equals to 1 • assume that P is equal to the external pressure. In the current implementation the pressure ( P ) = 1.0 When using the D’Arcy law model, the pressure to be considered will be the calculated pore pressure. Remarks ˜ c g will always be between K ˜ c g 0 and K ˜ c g E , and its variation rate will approach zero The quantity K ˜ c g becomes close to K ˜ cgE . when K

Main Index

CHAPTER 6 251 Nonstructural Procedure Library

Based upon the assumption made in this analysis that the coking only begins when the material is completely pyrolysed, we control the coking area by the advancement of the pyrolysis. Coking occurs if the advancement variable of pyrolysis at this location is bigger than a critical value, named “pyrmax”. It is usually just smaller than 1., which means that pyrolysis is over. This may be defined through the THERMO-PORE option; the default is 0.96. Beside this Arrhenius model to calculate the mass fraction of carbon in the pyrolysis gas, a linear model is proposed. Linear Model This model determines the mass fraction of carbon in the pyrolysis gas as a function of the temperature. The evolution is linear from a low temperature where the pyrolysis gas has an excess of carbon to a higher temperature where it is in equilibrium: ˜ c g( T ) . ˜ cg = K 1. For temperatures below the low temperature T , there is no coking: K l

l

2. For temperatures between the low temperature and the equilibrium one: ˜ c g is a linear function of temperature. ((2)) • If the temperature is increasing, K ˜ c g retains its last value. • If the temperature is decreasing, the coking is stopped and K This forbids the inverse coking reaction that would lead to an increase of carbon in the pyrolysis gas. For temperatures larger than the equilibrium temperature, there is no more chemical reaction: ˜ c g E . Figure 6-7 illustrates this: ˜ cg = K K The user can also specify a coking model through the UCOKSL user subroutine. Kcg ~ Kcg(Tl)= K cg 0

KcgE

Tlow Figure 6-7

Thigh=TE

Temperature

Calculation of Mass Fraction of Carbon in Pyrolysis Gas by Linear Function of Temperature

Water Drying Model The water drying model chosen for the streamline model is based upon the same principle than the pyrolysis one, namely an Arrhenius law.

Main Index

252 Marc Volume A: Theory and User Information

Written in function of the liquid mass density variable ρˆ l , the Arrhenius law for water drying is: ψ Ew ⎛ ρˆ l ⎞ w ∂ρˆ l -------- = – B w * exp ⎛⎝ – -----------⎞⎠ *ρˆ l ,0 ⎜ ---------⎟ ∂t R*T ⎝ ρˆ l ,0⎠

ρˆ l If we set ϕ w = 1 – --------- , we have: ρˆ l ,0 ∂ ( 1 – ϕw ) Ew ψ ρˆ l ,0 ------------------------- = – B* exp ⎛ – -----------⎞ *ρˆ l ,0 ( 1 – ϕ w ) w , ⎝ R*T⎠ ∂t So the temporal gradient of ϕ w is: ∂ϕ w Ew ψ ---------- = B w * exp ⎛⎝ – -----------⎞⎠ * ( 1 – ϕ w ) w ∂t R*T where: ϕw

ρˆ 1 is defined by ϕ w = 1 – ---------- , and represents the drying state. It varies from 0 to 1 ρˆ 1 ,0 during evaporation,

Bw

is a pre-exponential factor,

Ew

is the energy of activation of the reaction of water drying,

ψw

is the order of the reaction,

T

is the local temperature of the solid phase.

R

is the perfect gas constant.

Moreover, we have: ∂ϕ w ∂ρˆ l -------- = – ρˆ l ,0 * ---------∂t ∂t where ρˆ l ,0 is the mass density of liquid at the beginning of the analysis. ∂ρˆ l The user can define its own law to calculate the term -------- via a UWATERSL user subroutine. ∂t

Main Index

CHAPTER 6 253 Nonstructural Procedure Library

Presentation of the Energy Equation To take into account pyrolysis and coking and water evaporation in the calculation of the temperature, a convective and three enthalpic terms are added to the standard equation. The phenomena is included in: • the convective term by the mass flow rate m· g . The latter decreases during coking because of the mass loss of gaseous carbon to solid carbon. ∂ρˆ s ,p * • an enthalpic term --------------- ( H g ,p – H s ,p ,v c ) that represents the energy consumed by the ∂t pyrolysis reaction. ∂ρˆ s ,c ,c * • an enthalpic term – ------------------- ( H c * – H g ,p ) that represents the energy consumed by the ∂t coking reaction. ∂ρˆ l • an enthalpic term -------- ( H v – H l ) that represents the energy consumed by the evaporation of the ∂t water vapor. The equation becomes: ∂T ( ρˆ s ,i * c p i + ρˆ s ,p * c s ,p * + ρˆ s ,c ,c * c c * ) ------∂t ∂ρˆ s ,p * ∇. ( λ*∇T ) + --------------- ( H g ,p – H s ,p ,v c ) – ∂t

+ c p g ,p m· g .ΔT = ∂ρˆ s ,c ,c * ∂ρˆ l ------------------- ( H c * – H g ,p ) + -------- ( H v – H l ) ∂t ∂t

where: ( ρˆ c p ) e f f

is effective heat capacity of the material during the analysis.

c p ,g

is the effective specific heat of the gas (pyrolysis and vapor).

λ*

is the effective conductivity of the material during the analysis.

H g ,p

is the enthalpy of the gas, including only gas of decomposition.

H s ,p ,v c

is the enthalpy of the solid in course of pyrolysis (no liquid influence).

Hv

is the enthalpy of the water vapor.

Hl

is the enthalpy of the liquid water.

The effective specific heat c p ,g is based upon a mixture law between heat capacity of pyrolysis gas ( ρˆ g ,p c p ,g ,p ) and the one of vapor ρˆ g ,w c p ,g ,w : We have ρˆ g c p ,g = ρˆ g ,p c p ,g ,p + ρˆ g ,w c p ,g ,w

Main Index

254 Marc Volume A: Theory and User Information

m· g ,p c p ,g ,p + m· g ,w c p ,g ,w And so c p ,g = ----------------------------------------------------------m· g

To take into account the effect of water drying in the material properties, we use the drying state ϕ w ρˆ l defined above by ϕ w = 1 – --------- . ρˆ l ,0 The effective heat capacity is defined by: ( ρˆ c p ) e f f = ( 1 – ξ p ) ( ρˆ c p ) v + ξ p ( 1 – ξ c ) ( ρˆ c p ) c + ξ p ξ c ( ρˆ c p ) c d + ( 1 – ϕ w )ρˆ l ,0 c p ,l . The effective conductivity λ* = ( 1 – ξ p )λ v + ξ p ( 1 – ξ c )λ c + ξ p ξ c λ c d The heat capacity of the virgin material, charred material, deposit by coking effect and the liquid part ( ρˆ c ) , ( ρˆ c ) , ( ρˆ c ) , ( ρˆ c ) p v

p c

p cd

l ,0 p ,l

The conductivity of the virgin material, charred material, deposit by coking effect λ v, λ c, λ c d We can note that: • the vapor is not taking into account, which is consistent with the fact that we neglect also the effect of the pyrolysis gas, • the conductivity does not depend on the liquid water. Indeed, we can consider that the liquid belongs to small porosity, and that water evaporates before the beginning of the pyrolysis. We have, respectively: • the rate of pyrolysis, coking ξ p, ξ c • the drying state ϕ w ∂ξ c ∂ρˆ s ,c ,c * 1 -------- = ----------------------------------- ------------------∂t ρˆ c ,d * – ρˆ s ,p ,c * ∂t The enthalpy of material in the course of pyrolysis function of the densities and enthalpies of virgin and ρˆ s ,p ,v * H s ,p ,v * – ρˆ s ,p ,c * H s ,p ,c * charred material: H s ,p ,v c = --------------------------------------------------------------------------- . ρˆ s ,p ,v * – ρˆ s ,p ,c * The enthalpies, written in upper case, are the absolute enthalpies. They are equal to: H = ΔH f0 + h = ΔH f0 +

Main Index

T

∫T

0

c p dT .

CHAPTER 6 255 Nonstructural Procedure Library

ΔH f0

is the enthalpy of formation, is an input of the program.

T0

is the temperature of reference for enthalpy of formation, is an input of the program.

h

is the sensible enthalpy.

Ablation In many mechanical and thermal processes, there is the loss or removal of surface material by an erosive process such as melting or vaporization. Mechanical processes, such as particle impact or friction, may be involved as well. This process is particularly significant in high temperature applications, such as spacecraft reentry, where the intentional removal of material contributes to the thermodynamic cooling. For high temperature applications, special ablative materials have been created which may be defined using the THERMO-PORE option. In the current release, ablation has been designed to be used in thermal analyses only. The capability exists for 2-D, axisymmetric and 3-D solid elements, but the 3-D capability is in pre-release stage. There are seven aspects that control the receding surface calculation in Marc. 1. Specifying which surfaces are to undergo recession. The RECEDING SURFACE option is used to specify which surface is to be subjected to recession. For nodes that reside on elements edges (2-D) of faces (3-D) specified by the RECEDING SURFACE, the incremental displacement will be calculated during the recovery phase. 2. Specifying the magnitude of the recession rate. The recession rate is based upon either: a. Simple model, that is either a constant, or evaluated by a table. b. Based upon the data given in the SURFACE ENERGY model definition block. c. Specified in UABLATE user subroutine. 3. Specifying the direction of the movement of the nodes on the surface. The direction of the recession is based upon the normal evaluated at the node. If the ABLATION,1 parameter is used, then the normal is based upon applying a unit distributed load to all external surfaces. The magnitude of the equivalent force is the effective area, and the direction is the normal. This procedure is based upon lower order elements. The result is that at corners of the mesh the calculated normal is not perpendicular to either surface, but a weighted average (based upon the area of the edges). This procedure may lead to more physically reasonable results, as corners tend to be rounded off, but leads to more meshing problems. If the ABLATION,2 parameter is used, then the normal is based upon applying a unit distributed load to those element edges/faces specified by the ABLATION option. This results in the movement of the node lying at the corner to be perpendicular to the surface. If the ABLATION,3 parameter is used, then the direction of recession is based upon the direction of the streamline, assuming that the streamline method is specified on the PYROLYSIS parameter.

Main Index

256 Marc Volume A: Theory and User Information

If the ABLATION,4 parameter is used, then the direction of recession is based upon the direction of the streamline, assuming that the streamline method is specified on the PYROLYSIS parameter. The magnitude of the recession is adjusted based upon the difference between the true normal and this direction. 4. Specifying when remeshing is to occur. Remeshing is based upon three criteria specified via the ADAPT GLOBAL option. The tolerance values are relevant, but not critical unless the recession rate is very high, the time step is large, or the elements are small. The two key issues are: a. The element should not be so distorted at the beginning of the increment that the recession during the increment would lead to an inside-out element. This may lead to an Exit 1005. b. The ablation criteria should only find at most one element along each streamline that should be shaved off. This may lead to an Exit 1111. With this in mind, the following remeshing criteria have been developed: a. Element size reduction – two ratios are calculated. The first is the ratio of the current element edge length divided by the original element edge length. The second ratio is the ratio of the projected current element edge length with the surface normal divided by the projected original element edge length with the surface normal. For a 2-D quadrilateral mesh for each element on the receding surface, two edges are checked; while for 3-D hexahedral mesh, four edges are checked. If any edge satisfies the criteria, remeshing occurs. The recommended value of the tolerance is 0.4. b. Motion of a node. The magnitude of the displacement since the last remeshing is compared with the user-specified tolerance. This method is not recommended. c. The program also uses the previous displacements to predict if in the next increment the element will go inside out. As long as the next increment is similar to the previous increment this is a reasonable procedure. If may fail if the either the recession rate suddenly increases, or if the time step is increased. The user does not need to provide any tolerance value. While in theory, this method could be used exclusively, without the ones mentioned above, this is not recommended, because it leads to very thin elements. Two procedures are used to determine if an element has gone inside out. The first is based upon the Jacobian of the isoparametric shape functions. This method was determined not to be conservative. Hence additionally the area of four triangles (2-D) or volume of eight tetrahedrals is used. 5. Specifying the mesher used to create a new mesh Currently the user needs to specify whether the shaver mesher, relax mesher, or stretch mesher is to be used. These meshers may be used with quadrilateral and hexahedral elements. a. The shaver (type 9) is advantageous because rezoning is required in only a smaller region of the mesh. Elements are only modified if they have failed any of the criteria specified above, or they are adjacent to a modified element. The shaved mesher is also advantageous because the original biased mesh is retained during the process. The shaver mesher results in degenerated quadrilateral elements (triangles), or degenerated hexahedral elements (wedges), which may not be esthetically pleasing.

Main Index

CHAPTER 6 257 Nonstructural Procedure Library

b. The relax mesher modifies ever element in a body, as soon as any one of them fails the mesh criteria specified above. The relax mesher itself is simpler than the shaver mesher. The relax mesher also requires the use of the SPLINE option to identify edges that are to be fixed. c. The stretch mesher modifies ever element in a body, as soon as any one of them fails the mesh criteria specified above. The stretch mesher is similar to the relax mesher, but it only works in one direction, and it reasonably assures that all elements have a uniform thickness in this direction. 6. Which element type is being used and control of midside nodes Either mesher may be used with either lower order or higher order elements for both 2-D and 3-D problems. When using higher order elements, two considerations are made. a. During the recession itself the midside node on the surface is positioned such that the surface geometry is linear within and element, bi-linear for 3-D geometries. While this is not strictly consistent with the idea of higher order elements, it resulted in less distortion problems. Temperature fields are still quadratic. The midside nodes on the edges perpendicular to the surface that are in the interior of the element are adjusted such that they are mid-edge. This was done to make sure the quadratic shape functions did not break down. b. The remeshing process itself is based upon using lower order elements, and the midside nodes are then repositioned to the midpoints. 7. Region geometry. For the streamline model the element edges normal to the surface in theory should follow the streamline behavior; i.e., be normal to the surface. This is also advantageous from a surface recession perspective. When the recession, which by default is normal to the surface, is not aligned with the element edges, addition mesh distortion occurs. To overcome this problem a projection procedure can be requested. This is only available in conjunction with the shaver mesher, and is still not as good as creating a good mesh to begin with. It is highly advantageous to have initially a good mesh. Examples 1. Axisymmetric analysis with edges not perpendicular to surface). This is an example of a nonoptimal meshing technique because the element edges are not perpendicular to the surface.

Figure 6-8 Original Mesh – Note vertical edges are not normal to the surface

Main Index

258 Marc Volume A: Theory and User Information

Figure 6-9 Time=44.0 seconds

Figure 6-10 Close Up Showing Effect of Edges Not Aligned Perpendicular to Surface

2. Axisymmetric analysis of a nozzle using four node element and shaver mesher. Here the mesh is well aligned with the geometry, which leads to the ability to ablate further, and improves the remeshing.

Figure 6-11 Initial Mesh

Main Index

CHAPTER 6 259 Nonstructural Procedure Library

Figure 6-12 Time = 220. seconds

Figure 6-13 Close Up at Leading Edge

Figure 6-14 Final Temperatures

Main Index

260 Marc Volume A: Theory and User Information

3. Example of nozzle using 2-D quadratic elements tolerance = 0.2

Figure 6-15 Initial Mesh, Showing Nodes

Figure 6-16 Time = 220 Seconds

Figure 6-17 is a close-up showing nodes, including those shaved off. Note that outer edges remain straight, and that the midside nodes for the elements on the receding surface also remain at the midside of the edges. The element distortion is due to the fact that the element edges are not aligned perpendicular to the surface.

Main Index

CHAPTER 6 261 Nonstructural Procedure Library

Figure 6-17 Time = 220 Seconds

4. Example of 3-D nozzle.

Figure 6-18 Initial Mesh has 6480 Elements, 7657 8-node Bricks

Main Index

262 Marc Volume A: Theory and User Information

Figure 6-19 Time = 44.0 seconds

Figure 6-20 Close Up of Leading Edge

Main Index

CHAPTER 6 263 Nonstructural Procedure Library

5. Example using linear elements and relax mesher.

Figure 6-21 Final Configuration

Note that the number of elements using the relaxed mesher does not change so elements become thinner during the ablation process. 6. Example – 3-D – Linear hexahedral elements – Relax mesher – extruded nozzle.

Figure 6-22 Final Configuration - Linear 3-D Elements

Main Index

264 Marc Volume A: Theory and User Information

7. Example – 3-D – Quadratic hexahedral elements – Relax mesher – extruded nozzle.

Figure 6-23 Time = 44.0 Seconds

Note that in Figure 6-24, the outer edges remain straight and that the midside nodes for the elements on the receding surface also remain at the midside of the edges.

Figure 6-24 Close Up of Leading Edge – Showing nodes

Main Index

CHAPTER 6 265 Nonstructural Procedure Library

Welding Welding is a thermal process with specialized boundary conditions. These boundary conditions are specified through the WELD FLUX model definition option in conjunction with the WELD PATH and WELD FILL model definition options. Using these options, the welding heat input can be specified through two different techniques: • Modeling the heat input as a spatially varying distributed flux through the WELD FLUX model definition option applied to the base metal and filler elements. No temperatures are specified on the WELD FILL model definition option in this case. • Modeling the heat input as a spatially varying temperature boundary condition through the WELD FILL model definition option applied to the nodes of filler elements. No flux value (zero power) is specified on the WELD FLUX model definition option in this case. It is also possible to combine a nonzero flux applied to base metal elements through the WELD FLUX model definition option with a nonzero temperature applied to filler element nodes through the WELD FILL model definition option. In all these cases, the heat input path for the welding heat source or for the filler element deposition is defined by the WELD PATH model definition option. Weld Flux A disc shaped surface/edge heating source or a double ellipsoidal shaped volume heating source can be specified using the WELD FLUX model definition option. For more complex shapes, the heating source can be specified through the UWELDFLUX user subroutine. The associated weld path (defined through the WELD PATH model definition option) and the associated filler element set (defined through the WELD FILL model definition option) are also referred to through the WELD FLUX model definition option. Pavelic’s disc shaped weld heat source is expressed as [Ref. 16]. 3Q – 3x 2 ( – 3z 2 ) q ( x, y, z ) = -------- exp ⎛ ------------⎞ exp ---------------⎝ ⎠ 2 2 πr r r2

(6-14)

where q is the heat flux rate per unit area; Q = ηVI is the applied power with η = efficiency, V = Applied Voltage and I = Applied Current; r is the radius of the disc; z is the local coordinate along the weld path and x is the local coordinate along the tangent to the weld path. The disc shaped model can be used for specifying edge fluxes in 2-D and surface fluxes in 3-D. It is particularly useful for situations where the depth of weld penetration is not significant. Goldak’s double ellipsoidal shaped weld heat source can be used to specify volume fluxes in 2-D and 3-D [Ref. 16]: 6 3f f Q – 3x 2 – 3y 2 – 3z 2 q f ( x, y, z ) = ----------------------- exp ⎛ ------------⎞ exp ⎛ ------------⎞ exp ⎛ ------------⎞ ⎝ a2 ⎠ ⎝ b2 ⎠ ⎝ c2 ⎠ abc f π π 6 3f r Q – 3x 2 – 3y 2 – 3z 2 q r ( x, y, z ) = ----------------------- exp ⎛ ------------⎞ exp ⎛ ------------⎞ exp ⎛ ------------⎞ 2 2 ⎝ a ⎠ ⎝ b ⎠ ⎝ c2 ⎠ abc r π π

Main Index

(6-15)

266 Marc Volume A: Theory and User Information

where q f and q r are the weld flux rates per unit volume in the front and rear weld pools respectively; Q = ηVI is the applied power; a is the weld width along the tangent direction x; b is the weld penetration depth along the arc direction y; c f and c r are the forward and rear weld pool lengths in the weld path direction z; f f and f r are dimensionless factors given by 2 f f = ----------------------------( 1 + cr ⁄ cf )

(6-16)

2 f r = ----------------------------( 1 + cf ⁄ cr ) The double ellipsoidal source is also shown below in Figure 6-25.

cr

cf

z

a x

b

y Figure 6-25 Double Ellipsoidal Weld Flux showing the Local Coordinate Dimensions

The weld pool dimensions in Equations (6-14) and (6-15) are to be estimated and provided by the user. The width, depth, forward length and rear length are used for the volume weld flux. The surface radius is used for the edge or face weld flux. The dimensions are mandatory when the standard disc or ellipsoidal models are used and are optional when the UWELDFLUX user subroutine is used. The weld pool dimensions are used in three different ways by the program: – for defining the weld flux rate, – for defining a bounding box for filler element detection, and – for defining box dimensions when a box adaptive meshing criterion is used. The weld pool dimensions can be optionally varied with the help of tables. The tables can be functions of time or arc length. The arc length is measured along the associated weld path, from the first point of the path to the current position of the weld flux. The weld flux rate in Equations (6-14) and (6-15) can be further scaled by a factor. This scale factor can be automatically calculated by the program or optionally set by the user. For 3-D problems, the automated scale factor is set to 1. For 2-D problems (both planar and axisymmetric), the automated scale factor s is calculated by equating the integral of the flux rate over the entire x-y plane and the out-of plane thickness t to the applied power Q . s ∫ ∫ q ( x, y, 0 )tdxdy = Q

Main Index

CHAPTER 6 267 Nonstructural Procedure Library

For Equations (6-14) and (6-15), the scale factor can be shown to be s =

π r --- 3 t

s =

π --3

(6-17)

( cr + cf ) --------------------2t

It should be noted that the automated scale factor only ensures that the applied fluxes in the 2-D case matches the 3-D case. In general, the temperature solution comparisons between 2-D and 3-D also depend on the velocity of the weld source, the thermal properties, other thermal and mechanical boundary conditions, and heating effects before and after the heat source has crossed the 2-D plane. Weld Path The path followed by the welding heat source and the orientation of the weld arc are specified by the WELD PATH model definition option. This information is used to determine a local coordinate system

for the moving source, as shown in Figure 6-26. The weld path vector is taken as the local z axis. The arc orientation vector is taken as the local y axis. The tangent vector that is perpendicular to both y and z axes is taken as the local x axis. It is possible to specify the weld path and orientation information through the Marc Input, Text Input or the UWELDPATH user subroutine. Y

(weld path) z

X x (weld width) Z y (weld orientation) Figure 6-26 Local Coordinate System for Moving Source obtained by Translation and Rotation of Global Coordinate System

Marc Input Two options are available for specifying the weld path – Ordered List of Nodes or Point Coordinates of Polyline Curves. The weld path vector at point N is defined as the vector from point N to point N+1. For a closed weld path, the first and last node should be identical, or, the first and last point should have the same coordinates. An update path option is provided for the nodes option for a coupled analysis which allows the path to be updated based on the current displacements of the nodes along the path. This option is used in conjunction with the FOLLOWER FOR parameter. When the latter flag is used, all distributed fluxes are evaluated on the updated geometry and the path followed by the weld source is also updated in this case.

Main Index

268 Marc Volume A: Theory and User Information

A variety of options are available for specifying the arc orientation: Ordered List of Nodes, Point coordinates of Polyline Curves, Vector Components, or Euler Angles. When nodes or points are used, the arc vector at point N is defined as the vector from the weld path point at N to the arc orientation point at N. It is further possible to rotate the arc vector through an angle specified in degrees about the weld path axis. When vector components are used, they can be specified at distinct points and can be optionally interpolated as a function of arc length (length of the path from the first point) or of position coordinates along the path. When Euler angles are used, a unit vector in the global X direction is rotated through the global X-axis, Y-axis, and Z-axis by the specified angles to yield the arc orientation vector. The rotation angle, arc orientation vectors or Euler angles can be further varied along the weld path using tables as a function of arc length or point coordinates. For a point that is in between two given path points, Marc can automatically interpolate to find out the current arc orientation. Text Input In many industrial applications, weld paths for robots are specified via text files. A generic text file capability is provided in Marc in order to allow the specification of the weld path and the weld orientation. The weld path is specified through point coordinates in the columns 1-3 of the text file. The weld path vector at point N is defined as the vector from point N to point N+1. The arc orientation, defined in columns 4 - 6 of the text file for each point N, can be defined via point coordinates, vector components or Euler angles. 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. User Routine Input The weld path can also be defined using the UWELDPATH user subroutine. The final position of the associated weld flux, the weld vector at that point, and the orientation vector at that point have to be defined in the subroutine. Refer to Marc Volume D: User Subroutines and Special Routines for more details. In some cases, it is possible that the given/computed local y axis is not perpendicular to the local z axis. It is however important for purpose of weld flux computation to have a set of mutually perpendicular local axes. Since weld flux dimensions are typically provided in directions along and perpendicular to the weld path, the weld path vector (z axis) is taken as fixed and an equivalent set of perpendicular x and y axes are computed from the given information. The actual position of a weld heat source can be offset by a user specified amount from the associated weld path. The offsets are specified in the local x and y directions. This offset allows the same weld path to be used for multiple weld heat sources and is particularly useful for multi-pass welding where the weld heat source repeatedly moves in a similar pattern, but offset from the original path by a small amount. Weld Filler The dynamic creation of filler elements and the generation of associated boundary conditions is defined by the WELD FILL model definition option. Two methods are supported for the creation of filler elements: – the quiet element method and – the deactivated element method.

Main Index

CHAPTER 6 269 Nonstructural Procedure Library

In the quiet element method, filler elements are initially used with scaled down material properties. The scale factor is 10-5 by default. The coefficient of thermal expansion is set to zero and all other material properties (except yield stress, specific heat, and thermal mass density) are scaled down. The scaling is applied to reference temperature material properties and tables defining temperature dependent material properties are ignored. Weld fluxes and other point/distributed thermal loads on the quiet elements are ignored. When the filler elements are physically created by the moving heat source, the thermal properties are fully restored while the filler elements are still quiet on the mechanical side. If the thermal activation time is zero, the mechanical properties are also fully restored in the next increment. If the thermal activation time is nonzero, the filler elements remain mechanically quiet till the thermal activation time duration is passed. During this period, all stresses and strains in the elements are reset to zero. This disjoint thermal and mechanical treatment of the weld filler prevents the build up of mechanical strains and stresses during the temperature ramp up period. The quiet element method allows the elements to move with the model. This is particularly useful for accommodating large deformations during the welding process. However, the quiet element method is prone to ill-conditioning due to the large discrepancy in material stiffnesses. In the deactivated element method, filler elements are initially deactivated in the analysis and are not shown on the post file. When the elements are physically created by the moving heat source, they are activated in the model and appear on the post file. The filler elements are only thermally activated initially and remain inactive on the mechanical side. If the thermal activation time is zero, the filler elements are activated on the mechanical side in the next increment. If the thermal activation time is nonzero, the filler elements remain mechanically inactive until the thermal activation time is passed. This disjoint thermal and mechanical activation of the weld filler prevents the build up of mechanical strains and stresses during the temperature ramp up period. The deactivated element method does not suffer from any ill-conditioning problems, but the interior nodes of the deactivated elements do not move with the rest of the model. This can cause distorted filler elements when used in a large-deformation welding analysis. The initial temperatures for the deposited filler elements can be directly specified on the WELD FILL model definition option. Alternately, heat input from the weld torch can be modeled as distributed fluxes acting on for the base metal and deposited weld filler through the WELD FLUX model definition option. When the temperature option is used, special thermal boundary conditions are dynamically specified on the filler elements as they are created. These melting point temperatures are directly specified on the nodes of the created filler elements as long as the latter remain in the weld pool. Once the heat source moves on, the nodal temperature boundary conditions are removed and the filler elements are allowed to cool. By default, the melting point temperatures are applied instantaneously. This sudden boundary condition can cause convergence difficulties, especially with the AUTO STEP time stepping algorithm which bases the time step on the allowable temperature increase. A small ramp time (thermal activation time) can be optionally provided by the user to alleviate this problem. The temperature of the filler elements is increased from the current value to the melting point value over the ramp time specified by the user. If the ramp time is left at 0, the melting point temperature is applied instantaneously. The identification of the filler elements to be created in any particular increment is given by the following algorithm: Let X g i , Y g i , Z g i be the global position of the weld heat source origin at the beginning of the increment. Let X g f , Y g f , Z g f be the global position of the weld heat source origin at the end of the increment. The global coordinates of the final position and of the filler element nodal points are

Main Index

270 Marc Volume A: Theory and User Information

transformed to local coordinates using the local welding coordinate system based on the weld path and arc orientation. Let X l f , Y l f , Z l f be the local coordinates of the final source position and X l n , Y l n , Z l n be the local coordinates of the nth node of a filler element. A bounding box in the local coordinate system is then used to determine if the nodal point falls within the weld pool. Let the dimensions of the bounding box be defined as X b , Y b , Z b f and Z b r , where X b is the dimension in the weld width direction, Y b is the dimension in the weld depth direction, Z b f is the dimension in the forward weld path direction and Z b r is the dimension in the rear weld path direction. If not specified by the user, X b is taken as 1.5 times the weld pool width, Y b is taken as 2 times the weld pool width, Z b f is taken as the forward weld pool length and Z b r is taken as the rear weld pool length. Nodal point n is said to be inside the weld pool if the following relations are satisfied: X ln – X b < 0 Z ln + Z br < 0

Y ln – Y b < 0 Z ln – Z lf – Z bf < 0

(6-18)

If all nodes of a particular element are inside the weld pool, then the element is activated. It should be noted that in case the weld heat source moves across multiple segments of the weld path in a given increment, a number of sub-steps are used within the increment and the above algorithm is used for a linear segment in each substep. Filler elements can be set up as a homogeneous mesh with the base structure or as separate contact bodies. In the former case, thermal boundary conditions are automatically created at the filler-base interface. In the latter case, an appropriate contact heat transfer coefficient needs to be specified to ensure that the heat from the filler is transferred to the base structure. Additional items to facilitate welding analysis in Marc are: Time-Stepping and Convergence Checking Fixed stepping or adaptive stepping procedures can be used for welding problems. The fixed stepping scheme that should be used is TRANSIENT NON AUTO. The adaptive stepping scheme that should be used is AUTO STEP. For fixed stepping, the only temperature control that can be used is the temperature error in estimate. For adaptive stepping, the temperature controls that can be used include the temperature error in estimate and the allowable temperature change per increment. The default temperature change per increment is 20. Time-step cutback is used in the AUTO STEP algorithm if the temperature controls are not satisfied. The TRANSIENT time stepping scheme is obsolete and is not recommended for welding problems since time step cutback is not available with that scheme when the time step is reduced. When the time step is reduced, time step cutback is necessary to ensure that the weld motion, filler element activation, etc. work properly. Adaptive Meshing Two of the most useful adaptive meshing criteria for welding are: – Temperature Gradient Based criterion and – the Node in Box criterion.

Main Index

CHAPTER 6 271 Nonstructural Procedure Library

The general Box criterion requires the UADAPBOX user subroutine. However, for welding, the box definition has been automated in the program. The current location of the weld source and the weld pool dimensions are used to define the box. Nodes that fall in the box and the associated elements are adapted. An unrefine capability is also provided so that when the box moves away, the subdivided element mesh become coarse. It is important that the user provides weld pool dimensions through the WELD FLUX model definition option for the box criterion to work properly. It is also important to note that if the weld filler elements are identified as candidates for adaptive meshing, a suitable upper bound for the number of weld filler elements should be provided on the WELDING parameter. Material Properties Nonlinear temperature dependence for mechanical and thermal material properties is automatically taken into account by the program. Latent heat of solidification can be modeled by specifying the solidus/liquidus temperatures or by varying the specific heat as a highly nonlinear function of temperature. An appropriate temperature error in estimate control should be used to ensure that the material properties at the current temperatures are used. It should be noted that a general solid-solid phase transformation capability is not available in the current version of Marc. Parallel Computation The welding capability is fully supported in DDM. Each data file should contain the complete weld path. When nodes are used to define the weld path/weld orientation, this may require nodes belonging to other domains to be written out to the domain file. Also, if a weld flux belonging to domain A refers to a weld filler F, the elements of which are in domain B, then weld filler F with an empty set of elements needs to be available in domain A.

Radiation There are six approaches to solve radiation problems in Marc with different levels of sophistication. They include: 1. 2. 3. 4. 5. 6.

Viewfactor calculation by direct adaptive integral method. View factor calculation by Monte Carlo method. Viewfactor calculation by Pixel Based Modified Hemi-cube method. Radiation to Space using the FILMS model definition option. Radiation to Space using any of the CONTACT or THERMAL CONTACT options. Radiation into the body using the QVECT option.

There are several aspects in performing a radiation viewfactor calculation including: 1. Defining the edges or faces involved in the viewfactor calculation and determining if the region (cavity) is open or closed. 2. Calculation of the viewfactors. 3. If the region is open defining the environment temperature. This temperature may be constant or varying with time. 4. Definition of the surface emissivity and absorptivity, including temperature dependence and frequency dependence (spectral behavior). By default, the absorptivity is equal to the emissivity.

Main Index

272 Marc Volume A: Theory and User Information

5. Redefinition of the viewfactors due to large deformation or other phenomena. 6. Redefinition of the viewfactors due to either local or global adaptive meshing. 7. Radiation between surfaces results in increasing the size of the operator (stiffness) matrix, which results in greater memory requirements and increased computational times. All of these aspects are discussed in the following paragraphs. In the radiation calculations in Marc, there are several assumptions made: • Each surface is a diffuse emitter and reflector; i.e., the thermal behavior is independent of the orientation of the radiation. • Each surface is black; i.e., is a perfect absorber for all incident radiation. • The surfaces are isothermal. The third assumption requires either that an “adaptive” procedure is used to insure accuracy or that the finite elements are sufficiently small for each surface to be assumed to be isothermal. Using modern mesh generation techniques, there is a tendency to over-refine the finite element mesh, so the need for these adaptive techniques may be less significant. In theory, the viewfactors would form a symmetric matrix, the size of which is dependent upon the number of radiating surfaces. If one has a closed cavity, in theory, the summation of all viewfactors emitting from a surface should equal one. If desired, the numerically evaluated viewfactors can be scaled such that the sum is one. Computational Approaches There are several methods available for the viewfactor calculation in Marc, namely Direct Adaptive Integration, Monte Carlo, and Pixel Based Modified Hemi-Cube Method. The choice is made on the RADIATION parameter. While this is the historical order that they have been implemented, the HemiCube method runs fastest, gives the most accurate viewfactors, and is the most flexible, and hence, is discussed first. 1. Defining the Radiating Surfaces Depending upon which technique is used for calculating the viewfactors, this can be summarized as follows: a. Pixel Based Modified Hemi-Cube The CAVITY DEFINITION option is used to define the edges (2-D) or faces (3-D). Using Marc Mentat, this is in the MODELING TOOLS CAVITIES menu. Shells may be included in the model, in which case, one needs to indicate if it is the top or bottom or both surfaces. Symmetry surfaces may be defined. If physically there are multiple cavities in the problem, they should be placed in separate cavities to reduce the computational time. b. Monte Carlo The definition of the edges (2-D) or faces (3-D) is done via Marc Mentat or MD Patran; see BOUNDARY CONDITIONS>THERMAL>EDGE RADIATION OR FACE RADIATION menu. The

calculation of the viewfactors is also performed in Marc Mentat or MD Patran via the BOUNDARY CONDITIONS>THERMAL>COMPUTE RADIATION menu.

Main Index

CHAPTER 6 273 Nonstructural Procedure Library

c. Direct Integration In Marc, this is only available for axisymmetric solid elements. The geometry is defined using the RADIATING CAVITY option by specifying the node numbers around the cavity. It is not supported by Marc Mentat. 2. Radiation Viewfactors In many analyses, the radiative transfer of heat between surfaces plays a significant role. To properly model this effect, it is necessary to compute the proportion of one surface which is visible from a second surface known as the formfactor or viewfactor. The viewfactor, defined by a fourth order integral, presents many difficulties in its computation. Primary among these is the large amount of computing power needed, especially when shadowing effects are included. The radiative flow of hear from surface 1 to surface 2 is given by: 4

4

q 12 = σF 12 ( T 1 – T 2 )

(6-19)

in which, F 12 is the viewfactor and is calculated as: 1 F 12 = ------A1

∫ ∫ A

1

A

2

cos φ 1 cos φ 2 ----------------------------- dA 2 d A 1 2 πr

Pixel Based Modified Hemi-Cube Method The foundation of radiation is based upon radiation being received from multiple directions and/or being emitted in multiple directions. This leads to the concept of a hemisphere, where one considers an element being projected onto the hemisphere as shown in Figure 6-27. This geometric projection can be “easily” calculated for 2-D or axisymmetric, but is problematic in 3-D. To overcome this problem of exact projections, one can consider dividing the hemisphere into pixels as shown in Figure 6-28, and the simple “count” the pixels. This procedure is easier to implement in 3-D, though it is still expensive. As an alternative one can approximate the hemisphere with a Hemi-Cube as shown in Figure 6-29.

Figure 6-27 Element Projected onto Hemisphere

Main Index

274 Marc Volume A: Theory and User Information

Figure 6-28 Hemisphere Divided into Pixels

Figure 6-29 Hemisphere with Hemi-Cube

Using the Hemi-Cube method is less expensive, but is still difficult around the edges, and especially the corners in 3-D. One way to reduce this problem is to change the dimensions of the box, such that there is a smaller possibility that leakage out of the sides is important and then simply neglect this. This is shown in Figure 6-30, where a Hemi-Box now replaces the Hemi-Cube. To retain accuracy, one must select a good dimension of the box, and as the space is now biased, an equally spaced pixel grid will lead to inaccuracies. To overcome this problem, a Hemi-Plane will be used with non-equally spaced pixels, such that the weight of each pixel is the same. This is shown in Figure 6-31

Main Index

CHAPTER 6 275 Nonstructural Procedure Library

Figure 6-30 Hemisphere with Hemi-Box

Figure 6-31 Hemisphere with Hemi-Plane

The basic algorithm for the viewfactor program is as follows: a. b. c. d. e. f. g. h. i. j.

Main Index

Read in file created by the analysis program containing the geometry. For axisymmetric geometries, radiating faces are swept over a user controlled angle. In 3-D, subdivide quadrilateral faces into triangles. Create a map of nonuniform pixels and associate a weight with them. Convert coordinates to local system. Loop over receiving surface, lines in 2-D, triangles in 3-D. In 2-D, project line unto line; in 3-D, project triangle onto plane. Identify pixels (number and location). Sum the pixel weights. Output the view factor for this surface.

276 Marc Volume A: Theory and User Information

When symmetry planes are present, the receiving faces are doubled for each symmetry plane. For cyclic symmetry, the receiving faces are doubled n times. This method does not guarantee a symmetric Radiation Exchange Matrix ( A j ⋅ F i j ) because all F i j are calculated separately and independently based upon the above algorithm. There exists a possibility to make the radiation Exchange Matrix symmetric. For large models, this may be time consuming. The method is based upon an iterative averaging and column normalization, and for large problems, requires a large amount of memory or disk space. Monte Carlo Method In this method, the idea is to randomly emit rays from the surface in question. The percentage of these rays which hit another surface is the formfactor between the surfaces. The Monte Carlo method computes N formfactors at one time, providing linear scaling. In fact, the larger the number of surfaces, the faster the formfactors are computed compared to the Direct Adaptive Integration and Adaptive Contour Integration. Hence, this method is adopted for the viewfactor calculations. Once the viewfactors are calculated by Marc Mentat; the resulting output file containing the viewfactors can be read in with the inclusion of the RADIATION parameter and the VIEW FACTOR model definition option. Some of the features of the viewfactor calculation in Marc are: a. You are not required to specify blocking elements. This is embedded into the algorithm completely and, hence, done automatically. This is specially useful in three-dimensional analysis since, for complex geometries, it is impractical to predict what surfaces are blocking other surfaces. b. The cost of calculation is nearly linearly proportional to the number of elements which means that, for big problems, the cost does not increase significantly. c. The methodology in Marc guarantees that the sum of viewfactors is always 1.0. This is in contrast to the direct integration approach which has the requirement of normalization to avoid artificial heat gain and loss, because the sum of the viewfactors for any one surface is unlikely to add up to 1.0 due to errors in the computation of individual viewfactors. d. Shadowing effects (due to two surfaces being hidden from one another by other surfaces) can be modeled. For a surface to participate in the computations, it must participate in the following operations: a. Ray Emission: The surface should be able to randomly emit a ray from its surface. The origin of the ray should be randomly distributed over the area of the surface (see Figure 6-32). The direction of the ray should be distributed according to the cosine of the angle between the ray and the normal to the surface at the origin of the ray, thereby emitting more rays normal to the surface than tangent to it. b. Ray Intersection: Given an origin, direction, and length of a ray, the surface should be able to determine whether it is hit by that ray, and if hit, the length of the ray at the point of intersection. Determination of viewfactors involves consideration of several desired properties like speed, accuracy, shadowing, translucence, absorption, nonuniform emission, reciprocity, and efficiency. In light of the

Main Index

CHAPTER 6 277 Nonstructural Procedure Library

properties listed above, the Monte Carlo approach is adapted in conjunction with the ray tracing and boxing algorithms. Figure 6-33 depicts the formation of shadows which essentially involves the computation of incident light by tracing rays from the light source to the point of incidence of the eye rays. These rays do not reflect or refract. Shadows are formed when light source rays are obstructed, either partially or fully, from reaching an object. Refraction and reflection of light from light sources is not computed.

2

1 Figure 6-32 Random Ray Emission in Monte Carlo Method Point Light

Eye Ray Light Source Rays

Shadow

Figure 6-33 Shadowing Effects in Ray Tracing

Finally, to compute the viewfactors, it is not necessary to check the intersection of incident rays with all objects under consideration. Such a method would be prohibitively computationally expensive and preclude a large scale three dimensional analysis. An effective technique for fast calculation of intersections is employed. The method relies on sorting the objects before any intersections are computed. The information computed is used to eliminate most of the intersection computations. The technique requires that each object to be sorted have a bounding box which entirely encloses it. The sorting relies on creation of a binary tree of bounding boxes. Thus, a bounding box is computed for all objects. The objects are then sorted by the coordinate of the longest dimension of the bounding box. This list of objects is then divided into two sets, each having an equal number of objects. This process is

Main Index

278 Marc Volume A: Theory and User Information

repeated recursively until each set contains no more than a given maximum number of objects. This recursive sorting process is depicted in Figure 6-34.

1

2

3

4

5

6

7

8

9 Figure 6-34 Fast Intersection Technique for Sorting Objects

Ray intersections are performed by searching the binary bounding box tree which involves determining whether the ray hits the bounding box of all the objects. If the intersection with one bounding box is not found, then another bounding box is considered. In the event an intersection does exist, each object in the

Main Index

CHAPTER 6 279 Nonstructural Procedure Library

node is intersected with the ray if the intersection is a bottom node of the tree. Otherwise, the bounding boxes of both subtrees are intersected with the search in the closest subtree conducted first. The process continues until all rays are exhausted. Direct Adaptive Integration This approach computes viewfactors by directly computing a fourth order integral between every pair of surfaces. This means that there are N squared integrations to be performed, a quadratic scaling. Besides being quadratic, to achieve reasonable accuracy, this approach requires a huge number computations for surfaces which are close together; a situation which frequently occurs. Using the direct integration approach, Marc calculates the viewfactors automatically for you in each cavity of an axisymmetric body involving radiative heat transfer. This capability is only available for axisymmetric bodies. You must subdivide the radiative boundary in this heat transfer problem into one or more unconnected cavities. For each cavity, you define the outline of the cavity in terms of an ordered sequence of nodes. Usually, the nodes coincide with the nodes of the finite element mesh. You can add extra nodes, provided you also give the appropriate boundary conditions. The nodes must be given in counterclockwise order with respect to an axis orthogonal to the plane of the figure and pointing to the viewer (see Figure 6-35). If the cavity is not closed, the program adds the last side by connecting the last node with the first one. This side is treated as a black body as far as radiation is concerned; its temperature is taken as the average between the temperatures of the adjacent nodes. 7

8

6

9

5

10 R 11

Z

4 Visibility ϑV

1

3

2

Figure 6-35 Radiating Cavity (Approach II: Valid for Axisymmetric Capability Only)

Marc internally computes the viewfactor between every side of the cavity and all other sides. The matrix with the viewfactors can be stored into a file, and read in again during a subsequent analysis, thus avoiding a new computation. During a transient heat transfer analysis, for every time step, the program estimates the temperature reached at the end of the step. From the estimated temperature, the emissivity (temperature dependent) is computed. In addition, the radiating heat fluxes are computed. The temperatures at the end of the step are computed by solving the finite element equations.

Main Index

280 Marc Volume A: Theory and User Information

At every node, the difference between estimated and computed temperature is obtained. If the tolerance allowed by the CONTROL model definition option is exceeded, iterations within the time step take place. Otherwise, the computation of the step is concluded. The cavity is defined by its boundary defined by a list of nodes ordered counterclockwise. Insulated boundary condition (for example, symmetry boundaries) requires that the sum of the heat fluxes at a node be zero. This requirement is satisfied automatically. Therefore, no input is required for this type of boundary condition. As previously mentioned, in a heat transfer analysis of axisymmetric body involving radiative boundary conditions, Marc automatically calculates viewfactors for radiation. A description of the viewfactor calculation follows. The amount of radiation exchanged between two surfaces will depend upon what fraction of the radiation from each surface impinges the other surfaces. Referring to Figure 6-35, the radiation propagating from surface i to surface j will be: cos φ i cos φ j A j q i j = J i A i ⎛ ----------------------------------⎞ = J i A i F i j ⎝ ⎠ r2

(6-20)

It is noted that the viewfactor, F i j , is solely geometrical in nature. From the definition of F i j , we see that (6-21)

Aj Fj i = A i Fi j

We are now ready to derive the heat transfer radiation equation. Steady-state (equilibrium) energy conservation requires: qi = Ai ( Ji – Gi )

(6-22)

Two independent expressions for G i can be formed. a. The incoming radiation on a surface must equal the radiation emitted by all other surfaces which strike this surface, N

∑

Ai Gi =

N

Jj Aj F j i =

j = 1

∑

Jj Ai Fi j

j = 1

(6-23)

or N

Gi =

∑

Jj Fi j

j = 1

where N is the number of surfaces involved in the computations. b. The other expression for G i is Ji – εi En Ji – εi En i i G i = ----------------------- = ----------------------ρi 1 – εi

Main Index

(6-24)

CHAPTER 6 281 Nonstructural Procedure Library

where En

is the emissive power

ε

is the emissivity

ρ

is the reflectance.

Substituting Equation (6-24) into Equation (6-22) and rearranging it gives 1 – εi J i = E n – -------------- q i Ai εi i

(6-25)

This expression for J i can be inserted into Equation (6-23). After regrouping terms, you get the governing equation for gray body diffuse radiation problems A i δ i j – ( 1 – ε j )A i F i j ⎧ ⎫ ---------------------------------------------------- { q j } = [ A i δ i j – A i F i j ] ⎨ E n ⎬ A j εj ⎩ i⎭

(6-26)

For the problem of black bodies, that is, ε = 1, we have, ⎧ ⎫ { qj } = [ Ai δi j – A i Fi j ] ⎨ En ⎬ i ⎩ ⎭

(6-27)

This equation states the obvious; net radiation heat flow from a black surface is the difference between radiation given off and received; that is, there is no reflection.

Aj Ai

r

θj

θi

Figure 6-36 Viewfactor Definition

The heat flux radiating from A i to A j is computed as A j cos θ j q i j = J i ( A i cos θ i ) ⎛ --------------------⎞ ⎝ πr 2 ⎠

Main Index

(6-28)

282 Marc Volume A: Theory and User Information

where J i is the power radiating from A i , the first term within parentheses is the projection of A i normal to the connecting line, and the second term is the solid angle under which A j is seen from the center of A i defining the viewfactor: cos θ i cos θ j F i j = ---------------------------- A j 2 πr qi j = J i Ai Fi j

(6-29)

3. Environment Temperature If the sum of the viewfactors from an emitting face is not equal to one, then there is a radiation contribution to the environment. Hence, If the cavity is closed, there is no radiation to the environment and the environment temperature is not used. Including a PRINT-30 parameter, one will obtain the sum of the viewfactors from each emitting surface. For a closed, cavity, comparing this to one will be a measure of the accuracy of the viewfactor calculation. a. Pixel Based Modified Hemi-Cube The environment temperature may either be defined by creating an extra node and associating it with a cavity on the CAVITY DEFINITION model definition option. The temperature of the node is defined using FIXED TEMPERATURE model definition option. As an alternative one can specify the environment temperature on the RAD-CAVITY model definition option. b. Monte Carlo A constant environment temperature is defined in Marc Mentat or MD Patran. This information is passed into Marc in the vfs file. c. Direct Integration The cavity is assumed to be closed; there is no radiation to the environment. 4. Definition of the Surface Emissivity a. Pixel Based Modified Hemi-Cube The emissivity may be entered on an element edge or face. Hence, a particular element such as a brick could have different emissivities because of surface conditions. The emissivity could be temperature and frequency dependent. This is defined using the EMISSIVITY model definition option and the TABLE model definition option if required. Is is also possible to define the emissivity via the ISOTROPIC, ORTHOTROPIC, or other material options. The emissivity of materials as a function of wavelength is discontinuous in nature due to the discrete nature of particle physics. Frequency dependent emissivity (spectral) is defined by three types of bands: zero value, narrow, and wide. The evaluation is also dependent on whether the band is at low or high frequency as shown in Figure 6-37. The value of emissivity at the endpoints of each band may be a function of temperature. Based upon the table input procedure, it is possible to enter the emissivity as a function of temperature and wavelength. The emissivity is assumed to have a linear variation within each band.

Main Index

CHAPTER 6 283 Nonstructural Procedure Library

Figure 6-37 Band Frequency

Besides entering the emissivity, if wavelength dependent data is used then one also needs to enter Planck’s second constant and the speed of light. This is done via the PARAMETERS model definition option. The unit of wavelength used in the table should be consistent with the unit of length used to define the speed of light. Wavelength dependent emissivity is based upon: • Narrow bands - use average reciprocal wavelength • Wide bands at short wavelength - use exponential expansion • Wide band at long wavelength - use power series in reciprocal wavelength b. Monte Carlo or Direct Integration The emissivity is defined via the ISOTROPIC, ORTHOTROPIC, or other material options. Temperature dependent emissivity is entered through the TEMPERATURE EFFECTS or TABLE model definition options. 5. Redefinition of Viewfactors due to Large Deformation If the distance between the updated coordinates and the coordinates at which the last viewfactor calculation was performed is greater than user-specified value, then the viewfactors will be reevaluated. Note that the motion of nodes on the cavity is only an approximate measure of the inaccuracies of the previously generated viewfactors. The theoretically correct way would be to continuously re-evaluate the viewfactors, and then measure the difference between the two sets of viewfactors. This, of course, would defeat the objective of minimizing calculations. The critical distance to re-evaluate is specified on the RAD-CAVITY model definition option. This method is only available if the LARGE STRAIN parameter is used. It is also possible to specify that the viewfactors should be re-evaluated based upon increment numbers. Viewfactors are only recalculated if the Pixel Based Modified Hemi-Cube method is used. In the current release, this is only available if there is one cavity in the model.

Main Index

284 Marc Volume A: Theory and User Information

6. Redefinition of Viewfactors due to Adaptive Meshing If the geometry of the cavity has been defined using geometric entities (curves and surfaces) in the CAVITY DEFINITION model definition option, then when local adaptive meshing (2-D or 3D) or global adaptive meshing (2-D) occurs, the viewfactors will be re-evaluated. This is based upon that after remeshing the new edges or faces are automatically attached to the curves or surfaces. The program will determine the new list of element edges or faces in the cavity and recalculate the viewfactors. This capability is only available with the Pixel Based Modified Hemi-Cube method. 7. Computational Costs Regardless of the method used to calculate the viewfactors, there are two consequences: a. The number of viewfactors becomes large, growing quadratically with the number of radiating surfaces. b. The subsequent calculation in the analysis program is dependent upon the number of viewfactors calculated. The number of viewfactors is reduced because of shadowing effects, but depending upon the procedure used to calculate the viewfactors, this may lead to higher computational costs in calculating them. Because self-shadowing or third surface shadowing is likely, sparse storage techniques are beneficial in storing the view factors. As the data structures required for the view factor calculations are different than what is required for traditional finite element or finite difference calculations, the computation is often put into stand-alone programs. Using finite difference, contour integral, Gaussian integration or direct integration, the number of operations increases quadratically with the number of radiating surfaces. All of these procedures (combined with adaptive approaches or refined meshes) can produce accurate results, but at a clear computational cost. With the Monte Carlo method, the computational cost increases linearly with the number of radiating surfaces and increases linearly with the number of emitting rays. This clearly is beneficial for large models. The problem with the Monte Carlo method is that a large number of rays may be necessary to achieve accurate results (for example, if thin cavities exist). The advantage of the Pixel Based Modified Hemi-Cube method is that the computational costs are linearly dependent on the number of radiating surfaces and linearly dependent upon the number of pixels. The accuracy is dependent upon the number of pixels chosen, and the size/shape of the cube. A very large number of pixels has the ramification that the amount of memory required is increased and the amount of calculations is increased. The number of viewfactors increases the cost of the analysis calculation, because the viewfactor file is larger, and because the bandwidth of the system increases. There are two ways to control the computational costs: a. One can set a tolerance and any viewfactor less than this value will be ignored. This results in radiation being neglected.

Main Index

CHAPTER 6 285 Nonstructural and Coupled Procedure Library

6

Nonstru ctural and Coupled Procedu re Library

b. One can set a second tolerance and viewfactors below this number will be treated explicitly as opposed to implicitly. This means that the radiation contribution will be on the right-hand side and not in the operator matrix. This may result in more iterations, but lead to a significant reduction in the size of the operator matrix. This leads to a smaller bandwidth and a reduction in the computational costs to solve the system of equations. Graphical Visualization Using the Pixel Based Modified Hemi-Cube method, is possible to visualize the relative magnitude of the viewfactors associated with an emitting surface. This will create a post file, jid_cxx_vfs.t19, where xx is the cavity id. Each increment will represent the viewfactors from one surface. Creating a contour plot with Marc Mentat, one will observe a triangle (2-D) or pyramid (3-D) indicating which face is emitting and the values of the viewfactors to the other faces. Data, Data Flow, and Data Constraints a. Pixel Based Modified Hemi-Cube The geometric information is created in Marc and written to a file, jid_cxx_t18, where jid is the job id and xx is the cavity number. The stand-alone program then reads this file and calculates the view factors. This is then written to a file, jid_cxx.vfs. The analysis program then reads this file and performs the thermal analysis. If graphical visualization of the viewfactors is requested, this will be written to file, jid_cxx_vfs.t19.

b. Limitations A radiating cavity must be fully contained within one domain if DDM is used. There is currently a limitation of 99 cavities.

Conrad Gap For the thermal contact gap element, in the gap open condition, two surface temperatures T a and T b at the centroid of the surfaces of a thermal contact element are obtained by interpolation from the nodal temperatures. These two surface temperatures are used for the computation of an equivalent conductivity for the radiation/convection link. The expression of the equivalent thermal conductivity k 1 is: 2

2

k 1 = εσL ( T k a + T k b ) ( T k a + T k b ) + H L

(6-30)

where ε is the emissivity, σ is the Stefan-Boltzmann constant, L is the length of the element (distance between a and b), T k a , T k b are absolute temperatures at a and b converted from T a and T b ; and H is the film coefficient. The film coefficient can be a function of the temperature by referencing a table. The equivalent thermal conductivity k 1 for the thermal contact element is assumed to be in the gap direction. The thermal conductivities in other two local directions are all set to zero. A coordinate

Main Index

286 Marc Volume A: Theory and User Information

transformation from the local to the global coordinate system allows the generation of the thermal conductivity matrix of the thermal contact element in the global system for assembly. Similarly, in the gap closed condition, tying constraints are automatically generated by the program for thermal contact elements. The constraint equation for each pair of nodes can be expressed as: TI + TJ

if ( T g a p > T c l o se )

(6-31)

where 1 T g a p = --- ( T I + T J ) 2 T I, T J = nodal temperatures at nodes I and J T close = gap closure temperature.

Channel For the fluid channel element, the one-dimensional, steady-state, convective heat transfer in the fluid channel can be expressed as: ∂T f m· c -------- + Γh ( T f – T s ) = 0 ∂s Tf ( 0 ) = Ti n l e t

(6-32)

where m· is mass flow rate, c is specific heat, T f is fluid temperature, T s is solid temperature, s is streamline coordinate, Γ is circumference of channel, h is film coefficient, and T inlet is inlet temperature. The film coefficient may be a function of the temperature, and the inlet mass flow rate and temperature may be a function of time. Similarly, the conductive heat transfer in the solid region is governed by the following equation: · CT s + KT s = Q

(6-33)

subjected to given initial condition and fixed temperature and/or flux boundary conditions. At the interface between the fluid and solid, the heat flux estimated from convective heat transfer is q = h ( Ts – Tf )

(6-34)

In Equation (6-33), C is the heat capacity matrix, K is the conductivity matrix and Q is the heat flux vector. Equations (6-33) and (6-34) are coupled equations. The coupling is due to the unknown solid temperature T s appearing in Equation (6-32) and unknown fluid temperature T f in Equation (6-34) for the solution of Equation (6-33).

Main Index

CHAPTER 6 287 Nonstructural and Coupled Procedure Library

The solutions for Equations (6-32) and (6-33) are obtained from the introduction of a backward difference for the discretization of time variable in Equation (6-33) and of streamline distance in Equation (6-32). Let i i–1 · T s = [ T s – T s ] ⁄ ( Δt )

(6-35)

we obtain i i–1 1 1 ⎛ ---C + K⎞ T s = Q i + ----- CT s ⎝ Δt⎠ Δt

(6-36)

where Δt = time-step in transient analysis. Similarly, let dT f j–1 --------- = [ T f – T f ] ⁄ ( Δs ) ds

(6-37)

we obtain j

j–1

T f = [ Δsβ + T f

] ⁄ ( 1 + Δsα )

(6-38)

where Δs is the streamline increment, α = Γh ⁄ ( m· c ) ;

and

j–1

β = ΓhT s

⁄ ( m· c )

(6-39)

Output Marc prints out both the nodal temperatures and the temperatures at the element centroid when the CENTROID parameter is used, or at the integration points if the ALL POINTS parameter is invoked. You can also indicate on the HEAT parameter for the program to print out the temperature gradients and the resulting nodal fluxes. To create a file of element and nodal point temperatures, use the POST model definition option. This file can be used as temperature input for performing a thermal stress analysis. This file is processed using the CHANGE STATE option in the subsequent thermal stress analysis. This post file can also interface with Marc Mentat or MD Patran plot temperature as a function of time. Heat Transfer with Convection Marc has the capability to perform heat transfer with convection if the velocity field is known. The numerical solutions of the convection-diffusion equation have been developed in recent years. The streamline-upwind Petro-Galerkin (SUPG) method has been implemented into the Marc heat transfer capability. The elements which are available are described in Table 6-1.

Main Index

288 Marc Volume A: Theory and User Information

Table 6-1

Heat Transfer Convection Elements

Element Type

Description

36, 65

2-, 3-node link

37, 39, 41, 69, 131

3-, 4-, 6-, 8-node planar

38, 40, 42, 70, 87, 88, 122, 132 3-, 4-, 8-node axisymmetric 43, 44, 71, 123, 133

8-, 20-node hexahedral

135. 133

4-, 10-node tetrahedral

To activate the convection contribution, use the HEAT parameter and set the fifth field to 2. Due to the nonsymmetric nature of the convection term, the nonsymmetric solver is used automatically. Specify the nodal velocity vectors using the VELOCITY option. To change velocity, use VELOCITY CHANGE. If nonuniform velocity vectors are required, the UVELOC user subroutine is used. This capability can be used in conjunction with the Rigid-Plastic Flow section in Chapter 5 of this volume to perform a coupled analysis, in which the velocity fields are obtained. Technical Background The general convection-diffusion equation is: ∂T ρ * c ⎛ ------- + v ⋅ ∇T⎞ = ∇ ⋅ ( κ∇T ) + Q ⎝ ∂t ⎠

(6-40)

The perturbation weighting functions are introduced as: h h W = N + α ⎛ ---------- ( v ⋅ ∇N )⎞ + β ⎛ ---------- Δt ( v ⋅ ∇N )⎞ ⎝4 v ⎠ ⎝2 v ⎠ N is the standard interpolation function in Equation (6-1). The upwinding parameter, α , is the weighting used to eliminate artificial diffusion of the solution; while the beta term, β , is to avoid numerical dispersion. v is the magnitude of local velocity vectors. T is the temperature, κ is the diffusion tensor. Q is the source term and Δt is the time increment. The optimal choice for α and β are: α = coth ( Peclet ⁄ 2 ) – ( 2 ⁄ Peclet ) β = C ⁄ 3 – ( 2 ⁄ Peclet ) * ( α ⁄ C )

(6-41)

where Peclet is the local Peclet number in the local element and C is the local Courant number: Peclet =

density ∗ specific heat ∗ characteristic length ∗ magnitude of the fluid velocity/conductivity

Peclet =

ρ*c*h* v ⁄ k

and C = v * ( Δt ) ⁄ h where ( Δt ) is the time increment.

Main Index

CHAPTER 6 289 Nonstructural and Coupled Procedure Library

The characteristic length h is defined in [Ref. 11] where C ≤ 1 is required for numerical stability. When C > 1 , the β is set to be zero and a large time step is recommended to avoid numerical dispersion. Note:

The interpolation function N is not the time-space functions defined in [Ref. 6], so that most Marc heat transfer elements can be used. The convection contribution of heat transfer shell elements is limited due to the definitions of the perturbation weighting function and the interpolation function.

Diffusion Marc has a capability to perform diffusion analyses using two approaches. One is to use the capability using the PORE parameter which was developed for poro-elasticity/soil analysis, and the one described here which is activated using the DIFFUSION parameter. The basic equations governing the behavior is D’Arcys Law, which is complemented by a compressibility model for the fluid/gas. This will be described later. The capability is available for either steady-state or transient behavior. The capability is available for one-, two-, or three-dimensional, including shell analysis using the standard heat transfer elements. Marc computes and prints the following information at the element integration points: pressure, gradient or pressure, and the mass flow rate. The nodal point data consists of the pressure and the equivalent nodal mass flux. The material permeability should be entered on either the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition options. Dependency on the pressure, or the temperature should be defined by referencing a table. The porosity or the void ratio should be entered using the INITIAL POROSITY or INITIAL VOID RATIO model definition options. In a pure diffusion analysis, those values do not change with time. The fluid/gas data required is the fluid viscosity, the fluid mass density, and the fluid bulk modulus. This data is also entered in the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition options. It should be noted that for a purely incompressible fluid, the rate term is not significant, and a steady-state solution is immediately obtained. The boundary conditions associated with diffusion analysis consists of prescribed pressures defined with the FIXED PRESSURE model definition option. Unless shell elements are used, there is always only one degree of freedom per node. For transient analyses, initial pressure should also be defined using the INITIAL PRESSURE model definition option. Input nodal point mass flux using the POINT MASS model definition option. Specify distributed mass fluxes in the DIST MASS model definition option. Nonuniform or time dependent distributed mas fluxes may be defined by the FLUX user subroutine or referencing a table.

Technical Background The diffusion capability is based upon an implementation of a modified D’Arcys law for the calculation of the fluid/gas pressure in the solid. The results in an equation for the conservation of mass. D’Arcys

Main Index

290 Marc Volume A: Theory and User Information

law require that the Reynolds number governing the fluid velocity be small. Additionally the current formulation is appropriate for a single fluid. 1. D’Arcys Law The fundamental equation of D’Arcys law is expressed as: V D = – K ⁄ μ∇P where VD

is the D’Arcys velocity or the seepage velocity or filtration velocity.

K

is the absolute permeability

μ

is the dynamic viscosity

P

is the pressure

The D’Arcys velocity can be related to the real velocity V g by the porosity, φ . V D = φV g The porosity is a dimensionless quantity relating the volume of the pores to the total volume, which is bounded by 0 < φ < 1 , where a homogeneous material would have the value of zero. A related quantity is the void ratio, e , which is a dimensionless quantity that is the ratio of the volume of pore to the volume of solid, which is an unbounded number, 0 < e < ∞ . They are related by: φ = e ⁄ (1 + e) The next issue is the permeability, which in the literature is given the same word and symbol to mean different things. The permeability in D’Arcys law is the “absolute Permeability” and has units of l 2 . It is related to the D’Arcys coefficient of permeability, k , by: K = kμ ⁄ γ Note that the D’Arcys coefficient of permeability has units of l ⁄ t and γ is the specific weight, γ = ρg . The dynamic viscosity has the units of m ⁄ lt and is related to the kinematic viscosity v which has the units of l 2 ⁄ t by: v = μ⁄ρ where ρ is the real mass density (units of m ⁄ l 3 ). Note that in the literature the dynamic viscosity often is given the symbol of ν and the kinematic viscosity the symbol η . 2. Extension for Compressibility

Main Index

CHAPTER 6 291 Nonstructural and Coupled Procedure Library

D’Arcys law is extended by assuming that the fluid is slightly compressible, following the approach used in soil mechanics as: · · P = Kf ρf ⁄ ρf , where K f is the bulk modulus of the fluid, and ρ f is the density of the fluid. β f the inverse of the bulk modulus is often introduced as the fluid “compressibility”. βf = 1 ⁄ Kf The governing equation for the fluid flow becomes · ∇ ( K ⁄ μφ )∇P = φβ f P + ∇V . It is often more meaningful to give the mass flow rate across a boundary, so the complete expression is multiplied by the fluid density. 3. Initial Values To complement the initial values in the thermal problem, it is necessary to provide initial values for the pressure problem as well.

Hydrodynamic Bearing Marc has a hydrodynamic bearing analysis capability, which enables you to solve lubrication problems. This capability makes it possible to model a broad range of practical bearing geometries and to calculate various bearing characteristics such as load carrying capability, stiffness, and damping properties. It can also be used to analyze elasto-hydrodynamic problems. The lubricant flow in hydrodynamic bearing is governed by the Reynolds equation. The bearing analysis capability has been implemented into Marc to determine the pressure distribution and mass flow in bearing systems. Marc is capable of solving steady-state lubrication problems; the incremental procedure analyzes a sequence of different lubricant film profiles. Marc also can be used to solve coupled elastohydrodynamic problems. This analysis requires a step-by-step solution for both the lubrication and the stress problems using separate runs. Because the finite element meshes for each problem are different, the program does not contain an automated coupling feature. Only one-dimensional or two-dimensional lubricant flow needs to be modeled, since no pressure gradient exists across the film height. This modeling is done with the available heat transfer elements. The library elements listed in Table 6-2 can be used for this purpose.

Main Index

292 Marc Volume A: Theory and User Information

Table 6-2

Hydrodynamic Bearing Elements

Element

Description

36

2-node, three dimensional link

37

3-node, planar triangle

39

4-node, bilinear quadrilateral

41

8-node, planar biquadratic quadrilateral

65

3-node, three-dimensional link

69

8-node, biquadratic quadrilateral with reduced integration

121

4-node bilinear quadrilateral with reduced integration

131

6-node triangle

Marc computes and prints the following elemental quantities: lubricant thickness, pressure, pressure gradient components, and mass flux components. Each of these is printed at the element integration point. The nodal point data consists of pressures, equivalent nodal mass flux at fixed boundary points, or residuals at points where no boundary conditions are applied. In addition, the program automatically integrates the calculated pressure distribution over the entire region to obtain consistent equivalent nodal forces. This integration is only performed in regions where the pressure exceeds the cavitation pressure. The output includes the load carrying capacity (the total force on the bearing). This capacity is calculated by a vectorial summation of the nodal reaction forces. In addition, the bearing moment components with respect to the origin of the finite element mesh can be calculated and printed. To activate the bearing analysis option, use the BEARING parameter. If the analysis requires modeling of flow restrictors, also include the RESTRICTOR parameter. The values of the viscosity, mass density, and cavitation pressure must be defined in the ISOTROPIC option. Specify temperature-dependent viscosity values via TEMPERATURE EFFECTS or TABLE. If thermal effects are included, the STATE VARS parameter is also required. In hydrodynamic bearing analyses, temperature is the second state variable. Pressure is the first state variable. The fluid thickness field can be strongly position-dependent. A flexible specification of the film profile is allowed by using either the nodal thickness or elemental thickness option. Define nodal thickness values in the THICKNESS option. You may also redefine the specified values via the UTHICK user subroutine. Elemental values of lubricant thicknesses can be defined in the GEOMETRY option. Marc also enables the treatment of grooves. Constant groove depth magnitudes can be specified in the GEOMETRY option. If the groove depth is position-dependent, the contribution to the thickness field can be defined in the UGROOV user subroutine. The relative velocity of the moving surfaces is defined on a nodal basis in the VELOCITY option. In addition, you can redefine the specified nodal velocity components in the UVELOC user subroutine. Specify prescribed nodal pressure values in the FIXED PRESSURE option. Define restrictor type boundary conditions in the RESTRICTOR option. To specify nonuniform restrictor coefficients, use the URESTR user subroutine.

Main Index

CHAPTER 6 293 Nonstructural and Coupled Procedure Library

Input nodal point mass fluxes using the POINT MASS option. Specify distributed mass fluxes in the DIST MASS option. If nonuniform fluxes are necessary, apply this via the FLUX user subroutine. The TABLE option may also be used to define spatially varying boundary conditions. Define variations of the previously specified lubrication film thickness field through the THICKNS CHANGE option. The program adds this variation to the current thickness values and solves the lubrication problem. Activate the calculation of bearing characteristics (that is, damping and stiffness properties) through the DAMPING COMPONENTS or STIFFNS COMPONENTS options. Marc evaluates these properties based on the specified change in film thickness. This evaluation requires the formation of a new right-handside, together with a matrix back substitution. This is performed within so-called subincrements. The bearing force components calculated within these subincrements represent the bearing characteristics (that is, the change in load carrying capacity for the specified thickness change or thickness rate). The previously specified total thickness is not updated within subincrements. The calculated bearing characteristics are passed through to the UTHICK user subroutine. This allows you to define an incremental thickness change as a function of the previously calculated damping and/or stiffness properties. This procedure can be applied when analyzing the dynamic behavior of a bearing structure. Mechanical problems can often be represented by simple mass-damper-spring systems if the bearing structure is nondeformable. A thickness increment can be derived based on the current damping and stiffness properties by investigating the mechanical equilibrium at each point in time. The bearing analysis capability deals with only steady-state solution and does not include the analysis of transient lubrication phenomena. Note that the incrementation procedure is only meant to analyze a sequence of film profiles. No nonlinearities are involved; each increment is solved in a single step without iteration. To calculate the reaction forces that act on the bearing structure, Marc requires information about the spatial orientation of the lubricant. This information is not contained in the finite element model because of the planar representation of the lubricant. Therefore, it is necessary to define the direction cosines of the unit normal vector that is perpendicular to the lubricant on a nodal basis in the UBEAR user subroutine. The resulting nodal reaction forces are printed. Marc requires a step-by-step solution of both the lubrication problem and the stress problem in separate runs. The thickness changes need to be defined within the lubrication analysis based upon the displacements calculated in the stress analysis. The stress analysis post file and the UTHICK user subroutine can be used for this purpose. The tractions to be applied in the stress analysis can be read from the bearing analysis post file in the FORCDT user subroutine.

Technical Background The flow of a lubricant between two surfaces that move relative to each other is governed by the Reynolds equation ρh 3 ∂ ( ρh ) 1 ∇ ⋅ ⎛ ---------- ∇p⎞ – --------------- – --- ∇ ( ρhu ) + M = 0 ⎝ 12η ⎠ ∂t 2

Main Index

(6-42)

294 Marc Volume A: Theory and User Information

where: p

is lubricant pressure

ρ

is mass density

h

is film thickness

η

is viscosity

t

is time

u

is the relative velocity vector between moving surfaces

M

is the mass flux per unit area added to the lubricant

The following assumptions are involved in the derivation of this equation: • • • • • •

The lubricant is a Newtonian fluid; that is, the viscosity is constant. There is no pressure gradient across the film height. There is laminar flow. Inertial effects are negligible. The lubricant is incompressible; that is, mass density is constant. Thermal effects are absent.

By introducing the film constant ρh 3 λ = ---------12η

(6-43)

Equation (6-43) can be written as ∇ ⋅ ( λ∇p ) + M r = 0

(6-44)

r

where M is the reduced mass flux given by ∂ ( ρh ) 1 M r = M – --------------- – --- ∇ ( ρhu ) ∂t 2

(6-45)

In case of a stationary bearing, the transient term in Equation (6-45) vanishes. Three different kinds of boundary conditions can be distinguished for the lubrication problem: prescribed pressure on boundary, prescribed mass flux normal to the boundary, and mass flux proportional to pressure. Prescribed pressure on boundary is specified as p = p where p is the value of the prescribed pressure. Prescribed mass flux normal to the boundary has the form

Main Index

(6-46)

CHAPTER 6 295 Nonstructural and Coupled Procedure Library

∂p 1 – λ ------ = m n – --- ρhu n = m nr ∂n 2

(6-47)

where m nr is the reduced inward mass flux. Here, n refers to the inward normal on the boundary, and m n and u n are the inward components of total mass flux and relative velocity, respectively. If a restrictor is used (as in hydrostatic bearings), the total mass flux is a linear function of the pressure on the boundary. This condition is specified as ∂p 1 m n = – λ ------ + --- ρhu n = c ( p – p ) ∂n 2

(6-48)

or, written in a slightly different form ∂p – λ ------ = c ( p r – p ) ∂n

(6-49)

where c is the restriction coefficient and ρhu n p r = p – -----------2c

(6-50)

is the reduced pressure. The differential Equation (6-42), together with the boundary conditions (Equations (6-47), (6-48), and (6-50)) completely describe the lubrication problem. This is analogous to a heat conduction problem as shown in Table 6-3. Table 6-3

Comparison of Lubrication and Heat Conduction

Lubrication

Heat Conduction

Pressure

p

Temperature

T

Film constant

λ

Conductivity

k

Body heat flux

Q

Reduced body mass flux

M

r

Reduced boundary mass flux

mn

Boundary heat flux

qn

Restriction coefficient

c

Film coefficient

h

Reference temperature

Tr

Reduced reference pressure

p

r

Electrostatic Analysis Marc has the capability to perform electrostatic analysis. This allows the program to evaluate the electric fields in a body or media, where electrical charges are present. This can be solved for one-, two-, or threedimensional fields. Semi-infinite elements can be used to represent an infinite domain. The electrostatic problem is governed by the Poisson equation for a scalar potential. This analysis is purely linear and has

Main Index

296 Marc Volume A: Theory and User Information

been implemented in Marc analogously to the steady state heat transfer problem. The available elements are described in Table 6-4 below. Table 6-4

Element Types for Electrostatic Analysis

Element Type

Description

37, 39, 131, 41

3-, 4-, 6-, 8-node planar

69

8-node reduced integration planar

121

4-node reduced integration planar

101, 103

6-, 9-node semi-infinite planar

38, 40, 132, 42

3-, 4-, 6-, 8-node axisymmetric

70

8-node reduced integration axisymmetric

122

4-node reduced integration axisymmetric

43, 44

8-, 20-node 3-dimensional brick

71

20-node reduced integration brick

105, 106

12-, 27-node semi-infinite brick

123

8-node reduced integration brick

135, 133

4-, 10-node tetrahedral

50, 85, 86

3-, 4-, 8-node shell

87, 88

2-, 3-node axisymmetric shell

137, 203

6-, 15-node pentrahedral

Marc computes and prints the following quantities: electric potential field vector ( E ) and electric displacement vector ( D ) at the element integration points. The nodal point data consists of the potential φ and the charge Q . To activate the electrostatic option, use the ELECTRO parameter. The value of the isotropic permittivity constant is given in the ISOTROPIC option, orthotropic constants can be specified using the ORTHOTROPIC option. Optionally, the UEPS user subroutine can be used. Specify nodal constraints using the FIXED POTENTIAL option. Input nodal charges using the POINT CHARGE option. Specify distributed charges by using the DIST CHARGES option. If nonuniform charges are required, the FLUX user subroutine can be used for distributed charges and the FORCDT user subroutine for point charges. The TABLE option may also be used to define spatially varying boundary conditions. The electrostatic capability deals with linear, steady-state problems only. The STEADY STATE option is used to begin the analysis. The resultant quantities can be stored on the post file for processing with Marc Mentat.

Main Index

CHAPTER 6 297 Nonstructural and Coupled Procedure Library

Technical Background The Maxwell equations to govern electrostatics are written in terms of the electric displacement vector D and the electric field vector E such that ∇⋅D = ρ

(6-51)

and ∇×E = 0

(6-52)

where ρ is a given volume charge density. The constitutive law is typically given in a form as: D = εE

(6-53)

where ε is the dielectric constant. Introducing the scalar potential φ such that E = – ∇φ

(6-54)

which satisfied the constraint Equation (6-52) exactly. Denoting the virtual scalar potential by ψ , the variational formulation is

∫ ∇ψ ⋅ ( ε∇φ )dV

∫ ψρdV + ∫ ψ ⋅ ( ε∇φ – n )dA

=

V

(6-55)

Γ

V

The natural boundary condition is applied through the surface integral in terms of the normal electric displacement using: – ε∇φ ⋅ n = D ⋅ n = D n

(6-56)

Consider a material interface Γ 12 , separating two materials 1 and 2, and as φ is continuous over the material interface, the tangential electric field constraint is automatically satisfied. n × ( E1 – E2 ) = 0

on Γ 12

(6-57)

If charges are present on the interface, these are applied as distributed loads as follows: n ⋅ ( D1 – D2 ) = ρs

on Γ 12

(6-58)

Using the usual finite element interpolation functions N and their derivatives β , we obtain ψ = NΨ K =

∫ βTε V

Main Index

φ = NΦ βdV

(6-59)

298 Marc Volume A: Theory and User Information

F =

∫ N T ρNdV + ∫ N T ND n dA + ∫ V

Γ

Γ

N T Nρ s dA

(6-60)

12

and finally KΦ = F

(6-61)

Capacitance A capacitor is a device that can store electrostatic charge and hence electrostatic potential energy. This energy can be thought as the energy stored in the electric field created by the charge on the capacitor.Capacitance is always associated with conductors that can store charge. A problem can contain a number of conductors each of which will store charge. This gives rise to self and cross capacitance due to interaction between the conductors. This is expressed by the capacitance matrix. All conductors in the problem are assumed to be bodies and defined as a set of elements. This is done using the THERMAL CONTACT model definition option. No two conductors can touch each other or overlap. It is required to model the inside of the conductor bodies. A sub-set of the conductor bodies can be considered for capacitance computation. This subset is specified using the EMCAPAC history definition in the THERMAL CONTACT model definition option. Marc performs capacitance computation only if the above definitions are specified in the input file. The electrostatic analysis is used for computation of the capacitance matrix. The computation of the capacitance matrix results from the usual electrostatic analysis with some constraints on boundary conditions: • The boundary of the problem must satisfy far-field conditions and the electric potential on this boundary must be zero. • At problem boundaries where far field is not satisfied, the homogenous Neumann boundary condition must apply. • The electrostatic charge boundary condition must not be used on the problem boundary. • Any boundary condition applied on an individual conductor body is ignored. When dissimilar meshes are used to model the problem, then the conductors and dielectrics are distinct contact bodies. In this case it is best that the conductors are the contact bodies which are being touched and the dielectrics are the touching contact bodies. Technical Background Consider a single conducting body placed in an infinite homogenous dielectric medium. This conductor can be charged by putting a charge on it or applying an electric potential. The charge redistributes on the conductor such that the electric field inside the conductor is zero. This indicates that these charges reside on the outside surface of the conductor and there is no charge inside the conductor. A normal electric field is present on the surface of the conductor. The value of the normal electric field is equal to: σ E n = --ε where:

Main Index

(6-62)

CHAPTER 6 299 Nonstructural and Coupled Procedure Library

σ

is the surface charge density

ε

is the permittivity of the medium surrounding the conductor

The normal electric displacement is D n = εE n = σ

(6-63)

The total charge on the conductor is: Q =

°∫ °∫ σdS

(6-64)

S

where S defines the surface of the conductor. The capacitance C is then defined as: Q C = ---V

(6-65)

where V is the constant potential on the conductor. Capacitance Matrix For multiple conductors the capacitance computation is expressed as a capacitance matrix. For n multiple conductors, the capacitance matrix is: Q1 Q2 . . Qn

=

C 11 C 12 . . C 1 n

V1

C 21 C 22 . . C 2 n

V2

.

.

.

.

Cn 1 Cn 2

. . . · . . . . , Cn n

. , Vn

where Ci j

is the self capacitance of conductor i , if i = j

Ci j

is the mutual capacitance between conductor i and j , if i ≠ j

To find the values of C i j , the analysis has to be repeated n times. To find C i j for any column j and i = 1 ,2 ,…n , the procedure is as follows: 1. Specify V j = 1 volt and V 1 = V 2 = …… = V i ≠ j = … = V n = 0 .

Main Index

(6-66)

300 Marc Volume A: Theory and User Information

2. For this run the values of Q i ( i = 1 ,2…n ) are computed and the capacitance values of column j are calculated.

Magnetostatic Analysis Marc has the capability to perform magnetostatic analysis. This allows Marc to calculate the magnetic field in a media subjected to steady electrical currents. This can be solved for two- or three-dimensional fields. Semi-infinite elements can be used to represent an infinite domain. The magnetostatic analysis for two-dimensional analysis is solved using a scalar potential, while for three-dimensional problems, a full vector potential is used. The magnetic permeability can be a function of the magnetic field, hence, creating a nonlinear problem. Only steady-state analyses are performed. The available elements which are described in Table 6-5. Table 6-5

Elements Types for Magnetostatic Analysis

Element Type

Description

37, 39, 131, 41

3-, 4-, 6-, 8-node planar

69

8-node reduced integration planar

121

4-node reduced integration planar

101, 103

6-, 9-node semi-infinite planar

102, 104

6-, 9-node semi-infinite axisymmetric

38, 40, 132, 42

3-, 4-, 6-, 8-node axisymmetric

70

8-node reduced integration axisymmetric

122

4-node axisymmetric reduced integration

109

8-node brick

110

12-node semi-infinite brick

181

4-node tetrahedron

182

10-node tetrahedron

183

2-node 3-D link

204

6-node pentahedral

205

15-node pentahedral

206

20-node brick

Marc computes and prints magnetic induction ( B ), the magnetic field vector ( H ), and the vector potential at the element integration points. The nodal point data consist of the potential ( A ) and the current ( J ). To activate the magnetostatic option, use the MAGNETO parameter. The value of the isotropic permeability (μ) is given on the ISOTROPIC option; orthotropic constants can be specified using the

Main Index

CHAPTER 6 301 Nonstructural and Coupled Procedure Library

ORTHOTROPIC option. Optionally, the UEPS user subroutine can be used. Often, it is easier to specify

(1/μ), which is also available through these options. A nonlinear permeability can be defined using the B-H relation. Specify nodal constraints using the FIXED POTENTIAL option. Input nodal currents using the POINT CURRENT option. Specify distributed currents by using the DIST CURRENT option. Permanent magnets can be introduced by using the PERMANENT option for isotropic materials, or by entering a remanence vector via the B-H RELATION option for orthotropic materials. In addition, the FLUX user subroutine can be used for nonuniform distributed current and the FORCDT user subroutine for fixed nodal potentials or point current. For convenience line element 183 can be used to define an external loading. The current on this element will be converted to point currents on the nodes, pointing in the direction of this line element. The TABLE option may also be used to define spatially varying boundary conditions. The magnetostatic capability is linear unless a nonlinear B-H relation is defined. In such problems, convergence is reached when the residual current satisfies the tolerance defined in the CONTROL option. The STEADY STATE option is used to begin the analysis. The resultant quantities can be stored on the post file for processing with Marc Mentat.

Technical Background The Maxwell equations for magnetostatics are written in terms of the magnetic flux density vector B such that: ∇×H = J

(6-67)

and ∇⋅B = 0

(6-68)

where J is the current density vectors. For magnetic materials, the following relation between B , H , and M , the magnetization vector, holds: B = μ0 ( H + M )

(6-69)

with μ 0 being the permeability of vacuum. Denoting the magnetic susceptibility by χ m and the permanent magnet vector by M 0 , we have M = χm H + M0

(6-70)

which can be substituted into Equation (6-69) to yield: B = μ H + Br

(6-71)

in which μ is the permeability, given by: μ = μ0 ( 1 + χm )

Main Index

(6-72)

302 Marc Volume A: Theory and User Information

and Br is the remanence, given by: Br = μ0 M0

(6-73)

Notice that ( 1 + χ m ) is usually called the relative permeability μ r . B

Br

H Figure 6-38 Nonlinear B-H Relationship

For isotropic linear material, χ m and M 0 are scalar constants. If the material is orthotropic, χ m and M change into tensors. For real ferromagnetic material, χ m and μ are never constant. Instead, they depend on the strength of the magnetic field. Usually this type of material nonlinearity is characterized by a socalled magnetization curve or B-H relation specifying the magnitude of (a component of) B as a function of (a component of) H. In Marc, the magnetization curve can be entered via the B-H RELATION option. For isotropic material, only one set of data points, representing the magnitude of the magnetic induction, B , as a function of H , the magnitude H, needs to be given. For orthotropic material, multiple curves are needed with each curve relating a component of B to the corresponding component of H. When the table driven input is used, different ways of entering a magnetization curve are available. Then the ISOTROPIC or ORTHOTROPIC material option contains either the permeability, the inverse permeability, the H-B relation, or the B-H relation. For ORTHOTROPIC, this can be different for each component. For the H-B relation and the B-H relation, a table has to be given where for the H-B relation, B is the independent variable, and for the B-H relation, H is the independent variable. Permeability and inverse permeability can also be controlled by a table where the independent variable can be H, B, or any other variable. A table can be either a set of data points or a function. From Equations (6-71) and (6-73), it can be seen that for orthotropic materials, a permanent magnetization or remanence can be entered through the B-H RELATION option, by putting in a nonzero B value for H = 0. For isotropic material, this does not work since the direction of the remanence vector is still indeterminate. Therefore, in the isotropic case, the only possibility is to supply the magnetization vector through the PERMANENT option. Any offset of the B ( H ) -curve, implying B ≠ 0 at ( H

= 0 ) is disregarded in this case. For orthotropic material, it is not allowed to use the

PERMANENT option. In this case, the magnetization can exclusively be specified through the B-H RELATION option or using the table driven input.

Main Index

CHAPTER 6 303 Nonstructural and Coupled Procedure Library

It is emphasized that the magnetization curve specified in the B-H relation or H-B relation must be monotonic and uniquely defined. Introducing the vector potential A such that: ∇×A = B

(6-74)

which automatically satisfies the constraint, Equation (6-68), and we then have the final form: –1

∇ × μ–1 ( ∇ × A ) = J + μ Br

(6-75)

The vector potential ( A ) is not uniquely defined by Equation (6-74). In 2-D magnetostatic simulations, this indeterminacy is removed by the reduction of A to a scalar quantity. In 3-D situations, Marc uses the Coulomb gauge for this purpose: ∇•A = 0

(6-76)

Denote the virtual potential by W ; then, the variational formulation is:

∫μ

–1

( ∇ × W ) • ( ∇ × A )dV =

V

∫ W • JdV + ∫ W • ( ∇ × μ V

–1

B r )dV + ∫ W • ( H × n )dA Γ

V

(6-77)

where n is the outward normal to V at the boundary Γ . In the three-dimensional case, the Coulomb gauge, Equation (6-76), is enforced with a penalty formulation. The resulting term added to the variational formulation, Equation (6-77) reads:

∫μ

–1

( ∇ × W ) • ( ∇ × A )dV =

V

∫ W • JdV + ∫ W • ( ∇ × μ V

+

–1

B r )dV + ∫ W • ( H × n )dA

V

∫ r ( ∇ • W ) ( ∇ • A ) dV

Γ

(6-78)

V

The default value used for r is: r = 10

–4

μ

–1

(6-79)

Using the usual finite element interpolation functions N , the discrete curl operator G , and the weighting function W = N .

Main Index

G =

∂N ⁄ ∂y ∂N ⁄ ∂x

G =

∂N ⁄ ∂y – ∂N ⁄ ∂z ∂N ⁄ ∂z – ∂N ⁄ ∂x ∂N ⁄ ∂x – ∂N ⁄ ∂y

for two-dimensional problems (6-80)

for three-dimensional problems

304 Marc Volume A: Theory and User Information

Leads to the resulting system of algebraic equations Ku = F

(6-81)

where K =

∫G

T –1

μ G dV

(6-82)

V

F =

∫N

T

N ( J ) dV +

V

∫G

T

–1

T

M B r dV + ∫ N N ( H × n ) dA

V

(6-83)

Γ

The Coulomb gauge is based upon the principle of conservation of electric charge which in its steady state form reads: ∇•J = 0

(6-84)

In Marc, it is up to you to specify the current distribution. When doing so, it is recommended to ensure that this distribution satisfies Equation (6-83). Otherwise, condition Equation (6-76) could be violated. As a consequence, the results could become less reliable. From the third term on the right-hand side of Equation (6-83), it becomes clear that the natural boundary condition in this magnetostatic formulation is H × n , the tangential component of the magnetic field intensity. Consequently, if no other condition is specified by you, by default a zero tangential magnetic field intensity at the boundaries is assumed. Besides, when there are no currents present on a Γ 12 material interface separating two materials 1 and 2, the tangential magnetic field intensity is assumed to be continuous: n × ( H 1 – H 2 ) = 0 on Γ 12

(6-85)

With H 1 and H 2 , the magnetic field intensities in material 1 and 2, respectively. A discontinuous tangential magnetic field intensity can be modeled by assigning an appropriate distributed “shear” current density to the interface. This (surface) current density J is related to H 1 and H 2 by: n × ( H 1 – H 2 ) = J on Γ 12

(6-86)

Electromagnetic Analysis Marc has the capability to perform both transient (dynamic) and harmonic fully coupled electromagnetic analysis. This allows Marc to calculate the electrical and magnetic fields subjected to external excitation. This can be solved for both two- or three-dimensional fields. A vector potential for the magnetic field is augmented with a scalar potential for the electrical field. If a transient analysis is performed, the magnetic permeability can be a function of the magnetic field; hence, a nonlinear problem. The elements available for electromagnetic analysis are described in Table 6-6.

Main Index

CHAPTER 6 305 Nonstructural and Coupled Procedure Library

Table 6-6

Element Types for Electromagnetic Analysis

Element Type

Description

111

4-node planar

112

4-node axisymmetric

113

8-node brick

Marc prints the magnetic flux density ( B ), the magnetic field vector ( H ), electric flux density ( D ), and the electrical field intensity at the integration points. In a harmonic analysis, these have real and imaginary components. The nodal point data consists of the vector potential A , the scalar potential V , the charge Q , and current I . To activate the electromagnetic option, use the EL-MA parameter. The values of the isotropic permittivity ( ε ), permeability ( μ ), and conductivity ( σ ) are given in the ISOTROPIC option. Orthotropic constants can be specified using the ORTHOTROPIC option. Optionally, the UEPS, UMU, and USIGMA user subroutines can be used. A nonlinear permeability can be defined using the B-H relation. Specify nodal constraints using the FIXED POTENTIAL option. Input nodal currents and charge using the POINT CURRENT option. Specify distributed currents by using the DIST CURRENT option and distributed charges by using the DIST CHARGE option. Nonuniform distributed currents and charges can also be specified by the FORCEM user subroutine. The electromagnetic capability is linear, unless a nonlinear B-H relation is defined. In such problems, convergence is reached when the residual satisfies the tolerance defined in the CONTROL option. The transient capability is only available with a fixed time step; use the DYNAMIC CHANGE option to activate this option. The resultant quantities can be stored on the post file for processing with Marc Mentat. In electromagnetic analysis, you can enter the current and/or the charge. In a harmonic analysis, you can enter both the real and imaginary components or the magnitude and the phase if the table driven input format is used. Table 6-7

Input Options for Electromagnetic Analysis

Input Options Load Description

Main Index

Model Definition

History Definition

User Subroutine

Nodal Current Nodal Charge

POINT CURRENT POINT CHARGE

POINT CURRENT POINT CHARGE

FORCDT

Distributed Current

DIST CURRENT

DIST CURRENT

FORCEM

Distributed Charge

DIST CHARGE

DIST CHARGE

FORCEM

306 Marc Volume A: Theory and User Information

Technical Background Technical Formulation Electromagnetic analysis is based upon the well-known Maxwell’s equations. This has been implemented in Marc for both transient and harmonic analyses. Transient Formulation The Maxwell’s equations are: · ∇×E+B = 0

(6-87)

· ∇ × H – εE – σ E = 0

(6-88)

· ∇ ⋅ ( εE + σE ) = 0

(6-89)

∇⋅B = 0

(6-90)

where the constitutive relations are D = εE B = μ0 ( H + M ) J = σE and E

is the electric field intensity

D

is the electric flux density

H

is the magnetic field intensity

B

is the magnetic flux density

J

is the current density

M

is the magnetization

and ε

is the permittivity

μ

is the permeability

σ

is the conductivity

μ0

is the permeability of free space.

· Additionally, we have the conservation of charge: ρ + ∇ ⋅ J = 0 where ρ is the charge density. We assume that the magnetization vector is given by:

Main Index

CHAPTER 6 307 Nonstructural and Coupled Procedure Library

M = χH + M 0

(6-91)

where M 0 is the strength of the permanent magnet and χ is the susceptibility. The magnetic field can be defined as: B = μ H + Br

(6-92)

in which μ is the permeability, given by: μ = μ0 ( 1 + χm )

(6-93)

and B r is the remanence, given by: Br = μ0 M0

(6-94)

Notice that ( 1 + χ m ) is usually called the relative permeability μ r . A vector magnetic potential A and a scalar potential V are introduced, such that B = ∇×A

(6-95)

E = – ( ∇V + A· )

(6-96)

Note that since only the curl of A is required, an arbitrary specification of the divergence can be made. The Coulomb gauge is then introduced. ∇⋅A = 0

(6-97)

This is implemented using a penalty condition. It is important to note that E depends not only on the scalar potential, but also upon the vector potential. Hence, interpretation of V as the usual voltage can lead to erroneous results. Substituting into Maxwell’s equations results in: ∇ × [ μ – 1 ( ∇ × A – μ 0 M 0 ) ] + ε ( ∇V· + A·· ) + σ ( ∇V + A· ) = 0

(6-98)

– ∇ ⋅ [ ε ( ∇V· + A·· ) + σ ( ∇V + A· ) ] = 0

(6-99)

· It has been assumed that ε = 0 ; in that, the permittivity has a zero time derivative. Two time stepping schemes have been implemented in Marc for transient electromagnetics. The default scheme uses the Newmark-Beta algorithm. This discretizes the second-order hyperbolic equations given in Equations (6-98) and (6-99) and is preferred in mid-to-high frequency situations where the permittivity-based terms in these equations have a significant influence in the transient response. For low-frequency systems where the permittivity-based terms can be insignificant, the Newmark-Beta scheme is sometimes found to produce spurious oscillations in the solutions for the potential, E and D.

Main Index

308 Marc Volume A: Theory and User Information

6

In such situations, a second scheme that uses the Backward-Euler algorithm to discretize first-order equations obtained by dropping the permittivity-based terms in Equations (6-98) and (6-99) is preferred. For the Newmark-Beta scheme, the general form is given by:

Nonstru ctural and Coupled Procedu re Library

1 A n + 1 = A n + ΔtA· n + ⎛ --- – β⎞ Δt 2 A·· n + βΔt 2 A n + 1 ⎝2 ⎠

(6-100)

A· n + 1 = A· n + ( 1 – γ )ΔtA·· n + γΔtA·· n + 1

(6-101)

The particular form of the dynamic equations corresponding to the trapezoidal rule: 1 γ = --2

1 β = --4

(6-102)

results in a symmetric formulation, which is unconditionally stable for linear systems. For the Backward-Euler scheme, the governing equations are rewritten as ∇ × [ μ – 1 ( ∇ × A – μ 0 M 0 ) ] + σ ( ∇V + A· ) = 0

(6-103)

– ∇ ⋅ [ σ ( ∇V + A· ) ] = 0

(6-104)

The derivative term

A·

in Equations (6-103) and (6-104) is discretized as n

An + 1 – A A· n + 1 = ----------------------------Δt

(6-105)

In the current formulation, a fixed time step procedure must be used. The time step is defined through the DYNAMIC CHANGE option. Harmonic Formulation In harmonic analysis, it is assumed that the excitation is a sinusoidal function, and the resultant also has a sinusoidal behavior. This results in the solution of a complex system of equations. In this case, Maxwell’s equations become: ∇ × E + iωB = 0

(6-106)

∇ × H – iεωE – σE = 0

(6-107)

∇⋅D–ρ = 0

(6-108)

∇⋅B = 0

(6-109)

where ω is the excitation angular frequency and i =

–1 .

Additionally, we have the conservation of charge: iωρ + ∇ ⋅ J = 0

Main Index

(6-110)

CHAPTER 6 309 Nonstructural and Coupled Procedure Library

where all symbols are the same as in the discussion above regarding transient behavior. Again, a vector potential A and a scalar potential V are introduced. In this case, these are complex potentials. Substituting into the Maxwell’s equations results in: ∇ × [ μ – 1 ( ∇ × A – μ o M o ) ] + σ˜ ( ∇V + iωA ) = 0

(6-111)

– ∇ ⋅ [ σ˜ ( ∇V + iωA ) ] = 0

(6-112)

where σ˜ = σ + iωε With a little manipulation, a symmetric complex formulation may be obtained. The excitation frequency is prescribed using the HARMONIC option. Note that the capability to extract the natural frequencies of a complex system by modal analysis does not exist in Marc. The harmonic formulation is assumed to be linear; therefore, you should not include the B-H RELATION option.

Piezoelectric Analysis The piezoelectric effect is the coupling of stress and electric field in a material. An electric field in the material causes the material to strain and vice versa. Marc has a fully coupled implementation of piezoelectric analysis, thus simultaneously solving for the nodal displacements and electric potential. The elements available for piezoelectric analysis are described in Table 6-8. They can be used in static, transient dynamic, harmonic, and eigenvalue analysis. The analysis can be geometrically nonlinear but is materially linear. The piezoelectric elements have their equivalent heat transfer elements, so that they can also be used in a coupled thermal-piezoelectric analysis. Such a coupled analysis is weakly coupled, and solved using a staggered approach. When piezoelectric elements are used in a contact analysis with a node of the piezoelectric element touching a segment of another piezoelectric element, then a multipoint constraint relation is set up for the nodal displacements as well as for the electric potential. Table 6-8

Element Types for Piezoelectric Analysis

Element Type

Description

160

4-node plane stress

161

4-node plane strain

162

4-node axisymmetric

163

8-node brick

164

4-node tetrahedron

Marc prints the stresses ( σ ), the strains ( ε ), the electric displacement ( D ) and the electric field intensity ( E ) at the integration points. The nodal data points consists of the displacements u , forces f , the potential ϕ , and the charge Q .

Main Index

310 Marc Volume A: Theory and User Information

To perform a piezoelectric analysis, use the PIEZO parameter. The values of the isotropic, orthotropic and anisotropic mechanical properties are given in the ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC model definition option, respectively. The electric constants, and the constants defining the coupling between the mechanical and electric part can be specified with the PIEZOELECTRIC model definition option. Specify nodal constraints using the FIXED DISP option or FIXED POTENTIAL option. Input nodal loads using the POINT LOAD option or nodal charges using the POINT CHARGE option. Specify distributed loads with the DIST LOADS option and distributed charges with the DIST CHARGE option. Fixed nodal displacements and potentials, or nodal forces and charges can also be specified by the FORCDT user subroutine, nonuniform distributed loads can be specified by the FORCEM user subroutine, and nonuniform distributed charges can be specified by the FLUX user subroutine. The TABLE option may also be used to specify spatially and temporarily varying boundary conditions.

Technical Background The mechanical equilibrium equation for the piezoelectric effect is:

∫ σ:δε dV

=

V

∫ t ⋅ δu dA + ∫ f ⋅ δu dV

Γ

(6-113)

V

and the electrostatic equilibrium equation is (see also Equation (6-55):

∫ D ⋅ δE dV

=

V

∫ δϕD ⋅ n dA + ∫ ρ V δϕ dV

Γ

(6-114)

V

where σ

is the stress tensor

ε

is the strain tensor

t

is the traction at a point on the surface

u

is the displacement

f

is the body force per unit volume

D

is the electric displacement vector

E

is the electric field vector

ρ

is the volume charge density

δE = –

∂ δϕ ∂x

is the virtual electric field corresponding to the virtual potential δϕ .

The constitutive equations to govern piezoelectricity are written for the mechanical behavior as: E

σ = L :ε – e ⋅ E

Main Index

(6-115)

CHAPTER 6 311 Nonstructural and Coupled Procedure Library

and for the electrostatic behavior as: ε

T

D = e :ε + ξ ⋅ E

(6-116)

where L

is the elastic stiffness

e

is the piezoelectric matrix (stress based)

ξ

is the permittivity

The superscripts E and ε represent coefficients measured at constant electric field, and constant strain, respectively. The term with e gives the electro-mechanical coupling in the two consitutive Equations (6-115) and (6-116). We approximate the displacements and electrical potential within a finite element as u = NU and ϕ = NΦ where N contains the shape functions and U and Φ contain the nodal degrees of freedom. The body forces and charges, as well as the distributed loads and distributed charges, are interpolated in a similar manner. The strains and the electric field are given as: ε = Bu U

(6-117)

and E = Bφ Φ

(6-118)

where B u and B φ contain the gradients of N . Denoting the virtual displacement by δU and the virtual potential by δΦ the variational formulations can be obtained by substituting Equations (6-115) and (6-117) into Equation (6-113):

∫ δε

T

σ dV =

V

∫

∫ δU

T T B u σ dV

T T δU B u LB u U dV

V

+

∫

∫ tδU dA + ∫ fδU dV

T T δU B u eB ϕ Φ dV

V T

=

Γ

V

T

V

=

∫ tδU dA + ∫ fδU dV

Γ

V T

δU K u u U + δU K u ϕ Φ = δU F u

Main Index

(6-119)

312 Marc Volume A: Theory and User Information

and similarly by substituting Equations (6-116) and (6-118) into Equation (6-114):

∫ δE –∫

T

D dV =

∫ –δ Φ

V V T T δΦ B ϕ eB u U dV +

∫

V

T T B ϕ D dV

=

∫ δΦDn dA + ∫ ρ V δΦ dV

Γ

T T δΦ B ϕ ξB ϕ Φ dV

V

=

V T

∫ δΦDn dA + ∫ ρ V δΦ dV

Γ

T

(6-120)

V T

– δΦ K ϕ u U + δΦ K ϕ ϕ Φ = δΦ ρ ϕ The final set of equations in matrix form is then: Ku u Ku ϕ –Kϕ u Kϕ ϕ

u = Φ

Fu ρϕ

(6-121)

Strain Based Piezoelectric Coupling It is also possible to apply strain based coefficients for the piezoelectric coupling matrix. Then the consitutive equations are for the mechanical behavior: ε = C:σ + d ⋅ E

(6-122)

and for the electrostatic behavior: D = d:σ + ξ∗ ⋅ E

(6-123)

where C

is the elastic compliance

d

is the piezoelectric matrix (strain based)

ξ∗

is the permittivity (strain based)

When d and ξ∗ are given, Marc converts this into stress based properties, where e = L:d and T

ξ = ξ∗ – e ⋅ d .

Acoustic Analysis Marc has the capability to perform acoustic analysis in a rigid as well as a deformable cavity. This allows the program to calculate the fundamental frequencies of the cavity, as well as the pressure distribution in the cavity. This can be solved for two- or three-dimensional fields.

Rigid Cavity Acoustic Analysis The acoustic problem with rigid reflecting boundaries is a purely linear problem analogous to dynamic analysis, but using the heat transfer elements.

Main Index

CHAPTER 6 313 Nonstructural and Coupled Procedure Library

The elements which are available for acoustic analysis of a rigid cavity are described in Table 6-9. Marc computes and prints the following quantities: pressure and pressure gradient at the integration points. The nodal point data consists of the pressure and the source. Table 6-9

Element Types for Rigid Cavity Acoustic Analysis

Element Type

Description

37, 39, 131, 41

3-, 4-, 6-, 8-node planar

69

8-node reduced integration planar

121

4-node reduced integration planar

101, 103

6-, 9-node semi-infinite planar

38, 40, 132, 42

3-, 4-, 6-, 8-node axisymmetric

70

8-node reduced integration axisymmetric

122

4-node reduced integration axisymmetric

133

10-node tetrahedral

135

4-node tetrahedral

Technical Background The wave equation in an inviscid fluid can be expressed in terms of the pressure p as: 2

∂ p --------2- = c 2 ∇ 2 p ∂t

(6-124)

where c is the sonic velocity: c =

K⁄ρ

(6-125)

where K is the bulk modulus and ρ is the density. Equation (6-124) can be rewritten as: 2

2 ∂ p K∇ p – ρ --------- = 0 2 ∂t

(6-126)

Where the source terms are neglected, note that this is analogous to the dynamic equation of motion. The modeling of rigid reflecting boundaries can be done as follows. Mathematically, a reflecting boundary is described by: ∂p ------ = 0 ∂n

Main Index

(6-127)

314 Marc Volume A: Theory and User Information

∂p where ------ is the pressure gradient normal to the reflecting surface. ∂n This is analogous to an insulated boundary in heat transfer. Hence, a reflecting boundary can be modeled by a set of nodes at the outer surface of the area which are not connected to another part of the medium. A reflecting plate in the middle of an acoustic medium can be modeled by double nodes at the same location. Note:

Where there are no boundary conditions applied, there is a zero-valued eigenvalue, corresponding to a constant pressure mode. Hence, you need to have a nonzero initial shift point.

To activate the acoustic option, use the ACOUSTIC parameter. The number of modes to be extracted should also be included on this parameter. The bulk modulus and the density of the fluid are given in the ISOTROPIC option. Specify nodal constraints using the FIXED PRESSURE option. Input nodal sources using the POINT SOURCE option. Specify distributed sources using the DIST SOURCES option. If nonuniform sources are required, apply these via the FLUX user subroutine or use the TABLE option. To obtain the fundamental frequencies, use the MODAL SHAPE option after the END OPTION. The nodes can be used in a transient analysis by invoking the DYNAMIC CHANGE option. The point and distributed sources could be a function of time.

Fluid Mechanics Marc has the capability to perform fluid flow analysis. Marc solves the Navier-Stokes equations in the fluid under the restrictions that the fluid is considered to be nonreactive, incompressible, single phases, and laminar. The capabilities in Marc can be applied to four different problems listed below: Fluid behavior only Fluid-thermal coupled behavior Fluid-solid coupled behavior Fluid-thermal-solid coupled behavior Mass Conservation The principle of mass conservation for a single-phase fluid can be expressed in differential form as: Dρ -------- + ρ∇ ⋅ v = 0 Dt where ρ is the mass density, v is the Eulerian fluid velocity, and t is the time. Momentum Conservation The principle of conservation of linear momentum results in:

Main Index

(6-128)

CHAPTER 6 315 Nonstructural and Coupled Procedure Library

∂v ρ ⎛ ------ + v ⋅ ∇v⎞ = ρf + ∇ ⋅ σ ⎝ ∂t ⎠

(6-129)

where σ is the stress tensor and f is the body force per unit mass. In general, the stress tensor can be written as the sum of the hydrostatic stress and the deviatoric stress as. tr ( σ ) 1 ------------- = --- σ i j δ i j 3 3

(6-130)

1 tr ( σ ) σ d = σ i j – --- σ i j δ i j = σ i j – ------------- δ i j 3 3

(6-131)

In fluid mechanics, the fluid pressure is introduced as the negative hydrostatic pressure: trσ p = – -------3

(6-132)

Energy Conservation For incompressible fluids, the principle of conservation of thermal energy is expressed by: ∂q i ∂T ∂T ρC p ⎛ ------- + v i --------⎞ = – -------- + H ⎝ ∂t ∂x i⎠ ∂x i

(6-133)

where T is the temperature, C p is the specific heat at constant pressure, q i is the thermal flux, and H is the internal heat generated. Equation of State The equation of state for a homogeneous, single-phase gas is: mRT pV = ------------M

(6-134)

m is the mass of the fluid, M is the molecular weight of the gas, R is the universal gas constant, V is the volume that the gas occupies. The gas constant is often expressed as R = R ⁄ M for each substance. The equation of state is then written as: P ρ = -------RT

(6-135)

In Marc, it is assumed that the fluid is incompressible. In such cases, the density is constant ρ = ρ o Constitutive Relations The shear strain rate tensor is defined:

Main Index

316 Marc Volume A: Theory and User Information

1 ∂v i ∂v j ε i j = --- ⎛ -------- + --------⎞ 2 ⎝ ∂x j ∂x i⎠

(6-136)

For viscous incompressible fluids, it is assumed that there is an expression: d · · σ i j = 2με i j = μγ i j

(6-137)

where μ is the dynamic viscosity. If the viscosity is not a function of the strain rate, the material is considered Newtonian. Viscous fluid flow is usually characterized by the Reynolds number Re : ρLv Re = ---------μ

(6-138)

where v is a typical velocity and L is the characteristic length. Viscosity for common fluids like air and water is fairly constant over a broad range of temperatures. However, many materials have viscosity which is strongly dependent on the shear strain rate. These materials include glass, concrete, oil, paint, and food products. There are several non-Newtonian fluid models in Marc to describe the viscosity as described below. Piecewise Non-Newtonian Flow · · 2· · 1 ⁄ 2 ε is the equivalent strain rate = ε = ⎛ --- ε i j ε i j⎞ ⎝3 ⎠

(6-139)

· μ = μ ( ε ) , where μ is a piecewise linear function. Bingham Fluid A Bingham fluid behaves as a “rigid” fluid if the stress is below a certain level, labeled the yield stress, and behaves in a nonlinear manner at higher stress levels. · d · · σ i j = μ o γ i j + gγ i j ⁄ γ if σ ≥ g

(6-140)

· γ i j = 0 if σ < g

(6-141) 1 ---

· · 1· · 2 The effective viscosity is μ = μ o + g ⁄ γ and γ = ⎛ --- γ i j γ i j⎞ ⎝2 ⎠ The materials that can be simulated with this model are cement, slurries, and pastes. Power Law Fluid The fluid is represented as: · n – 1· d σi j = μo K ( γ ) γi j

Main Index

(6-142)

CHAPTER 6 317 Nonstructural and Coupled Procedure Library

where K is a nondimensional constant. This model is useful for simulating flow of rubber solutions, adhesives, and biological fluids. Carreau Model This model alleviates the difficulties associated with the power law model and accounts for the lower and upper limiting viscosities for an extreme value of the equivalent shear strain rate. 2 · 2 ( n – 1) ⁄ 2 μ = μ∞ + ( μo – μ∞ )( 1 + τ γ )

(6-143)

where μ o and μ ∞ are the viscosity at time equals zero and infinity, respectively. The thermal flux is governed by the Fourier law. ∂T q i = k i j -------∂x j

(6-144)

Finite Element Formulation In the procedures developed, the fluid-thermal coupling can be treated as weak or strong. In the weak formulation, the solution of the fluid and thermal equilibrium equations are solved in a staggered manner. In the strongly coupled approach, a simultaneous solution is obtained. This section cannot cover all of the details of the finite element formulation. It does discuss the final form of the linearized set of equations and some of the consequences. Beginning with degrees of freedom in a system – namely, v, p, and T for the mixed method – we utilize the traditional finite element interpolation functions to relate the values within the element to the nodal values. Because the pressure stabilizing Petrov-Galerkin (PSPG) method is employed in Marc, equal order interpolation functions can be used for the velocity and the pressure. The method of weighted residuals is used to solve the coupled Navier-Stokes equations. Based upon the conservation laws of momentum (mass and energy), we obtain first order differential equations in the form: Mv· + A ( v )v + K ( T, v )v – Cp + B ( T )T = F ( t ) T

(6-145)

C v = 0

(6-146)

NT· + D ( v )T + L ( T )T = Q ( v, t )

(6-147)

where the first equation is obtained from momentum, the second from mass, and the third from energy conservation, respectively. This is expressed in matrix form as: A + K B –C M 0 0 ⎧⎪ v· ⎫⎪ · + 0 D+L 0 ⎨ ⎬ 0 N 0 T ⎪ · ⎪ T 0 0 0 ⎩ p ⎭ –C 0 0 if the penalty method is employed

Main Index

⎧ v ⎫ ⎧ F ⎫ ⎪ ⎪ ⎪ ⎪ ⎨ T ⎬ = ⎨ Q ⎬ ⎪ ⎪ ⎪ ⎪ ⎩ p ⎭ ⎩ 0 ⎭

(6-148)

318 Marc Volume A: Theory and User Information

–1

T

p = χM P C v

(6-149)

resulting in –1 T M 0 ⎧ v· ⎫ + A + K + χCM P C ⎨ · ⎬ 0 N ⎩ T ⎭ 0

⎧ v ⎫ ⎧ F ⎫ ⎨ ⎬ = ⎨ ⎬ ⎩ Q ⎭ D+L ⎩ T ⎭ B

(6-150)

The introduction of the streamline upwinding technique (SUPG) developed by Brooks and Hughes is a major improvement for the stability of the fluid equations. This procedure controls the velocity oscillations induced by the advection terms. Effectively, this procedure adds artificial viscosity to the true viscosity. The second stabilization method, PSPG, allows equal order velocity and pressure interpolation functions to be used without inducing oscillations in the pressure field. The PSPG term is not included when using the penalty formulation. The details of these stabilization terms are not provided here, but note that the magnitude of the contributions are dependent upon the element size, viscosity, and the time step. Including these contributions, the semi-discrete set of equations takes the form: M + M δ 0 0 ⎧ v· ⎪ N 0 ⎨ T· Mε ⎪ 0 0 0 ⎩ p·

A + K + Kδ B –( C + Cδ ) ⎫ ⎪ D+L 0 Kε ⎬+ ⎪ T ⎭ –C 0 Cε

⎧ v ⎫ ⎧ F + Fδ ⎪ ⎪ ⎪ ⎨ T ⎬ = ⎨ Q + Qε ⎪ ⎪ ⎪ ⎩ p ⎭ ⎩ 0

⎫ ⎪ ⎬ ⎪ ⎭

(6-151)

The terms K d is included for SUPG and C e and G e for PSPG. The other terms are neglected, leading to: A + K + Kδ B –C M 0 0 ⎧⎪ v· ⎫⎪ 0 D+L 0 0 N 0 ⎨ T· ⎬ + ⎪ · ⎪ T 0 0 0 ⎩ p ⎭ –C 0 Cε

⎧ F ⎫ ⎧ v ⎫ ⎪ ⎪ ⎪ ⎪ ⎨ T ⎬ = ⎨ Q ⎬ ⎪ ⎪ ⎪ ⎪ ⎩ 0 ⎭ ⎩ p ⎭

These submatrices can be interpreted as follows:

Main Index

A

represents advection of momentum

D

represents advection of energy

K

represents diffusion of momentum or viscosity matrix

L

represents diffusion of energy or conductance matrix

M

represents mass

N

represents heat capacitance

B

represents buoyancy

Kδ

represents SPUG stabilization matrix

C

represents gradient matrix

(6-152)

CHAPTER 6 319 Nonstructural and Coupled Procedure Library

CT

represents divergence matrix

Ce

represents PSPG stabilization matrix

F

represents externally applied forces

Q

represents externally applied fluxes

Note that typically D , K , B , L , Q , and F are dependent upon the temperature. If a non-Newtonian fluid is used, A , K , D , and G are dependent upon the rate of strain. If the fluid is subjected to large motions, F can also depend on the total displacement. In terms of physical parameter, excluding geometry, observe: A = A ( ρo ) D = D ( ρ o, C p ) = D ( ρ o, C p, T ) K = K ( μ ) = K ( μ, T ) L = L ( K ) = L ( K, T ) M = M ( ρo ) N = N ( ρ o, C p ) B = B ( ρ 0, g, B ) where: ρo

is the initial density

Cp

is the specific heat

K

is the thermal conductivity

g

is the gravity

B

is the coefficient of thermal expansion

Penalty Method The penalty method is an alternative method to satisfy the incompressibility constraints. The objective is to add another term to the operator matrix (viscosity matrix) such that incompressibility is satisfied. Effectively, K is replaced with K c where:

Main Index

320 Marc Volume A: Theory and User Information

K c = K + χK p

(6-153)

where χ is a large number and K p the penalty matrix. K p can be written as: –1

K p = CM p C

T

(6-154)

where C and M p are functions of the geometry and shape functions only. The value of χ is typically between 10 5 to 10 9 . The penalty method should not be used for three-node planar elements, or four-node tetrahedral elements.

Steady State Analysis It is possible to simplify the equations governing fluid flow by assuming that the time derivatives of the velocity and temperature are zero. This is achieved by using the STEADY STATE option. For thermally coupled, non-Newtonian flows, you still have a highly nonlinear system and multiple iterations are required.

Transient Analysis The equations discussed above are still differential equations because of the presence of time derivatives of velocity and temperature. The conversion of the equations to fully discrete linear equations requires an assumption of the behavior during the increment. The approximations inevitably result in problems with accuracy, artificial damping, and/or stability problems. Marc uses the first order backward Euler procedure such that: v· n + 1 = ( v n + 1 – v n ) ⁄ Δt

(6-155)

This is substituted into the equations to yield: A + K + K δ + M ⁄ Δt 0 –C

T

–C ⎧ ⎫ ⎧ F – M ⁄ Δt ⋅ v n ⎪ v ⎪ ⎪ D + L + N ⁄ Δt 0 ⎨ T ⎬ = ⎨ Q + Q – N ⁄ Δt ⋅ T ε n ⎪ ⎪ ⎪ 0 Cε ⎩ p ⎭ ⎩ 0 B

⎫ ⎪ ⎬ ⎪ ⎭

(6-156)

Marc allows either fixed time step or adaptive time step procedure. The equations of fluid flow are highly nonlinear even for Newtonian behavior because of the inclusion of the advection terms. The Newton-Raphson and direct substitution procedures are available to solve these problems.

Solid Analysis Solid can be modeled in two ways:

Main Index

CHAPTER 6 321 Nonstructural and Coupled Procedure Library

• The first is to model them as a fluid with a very large viscosity. In such cases, an Eulerian procedure is used throughout the model. The constitutive laws are limited to the fluid relationships. • The second is to model them as true solids. In such cases, a Lagrangian or updated Lagrangian approach is used in the solid. The complete Marc constitutive routines are available for representing the solid behavior. An important consideration is the interface between the fluid and solid. Large structural deformation or fluid motion are not supported in the coupled Fluid-Solid capability. For small changes in the structural deformation, the nodes at the interface are updated. The pressure is transmitted between the fluid and the solid.

Solution of Coupled Problems in Fluids The coupled fluid-thermal problem can be solved using either a tightly coupled procedure as shown above or in a staggered manner. Problems such as free convection are inherently coupled and are best solved using the tightly coupled procedure. The fluid-solid interaction problem is solved in a weakly coupled manner. Every attempt has been made to maximize the computational efficiency. It should be noted that, while the staggered procedure can result in more global iterations, there are several motivating factors for solving the system in this manner. • In solving fluid problems, especially in three dimensions, very large systems of equations are obtained. Any procedure that reduces the number of equations (for example, excluding the solid) is potentially beneficial. • The fluid flow solution always requires the solution of a nonsymmetric system. In a weakly staggered analysis, the structural problem can still be solved with a symmetric solver. • When using an iterative solver, the solution of the strongly coupled system will result in an ill-conditioned system, which results in poor convergence. This is because the terms associated with the fluid, thermal, and structural operator are of several different orders of magnitude. The problem can be divided into two regions (fluid and solid) to accommodate these requirements. In each region, a different solver can be invoked; different nodal optimizers can be used; and a different memory allocation can be performed. Often, the fluid uses an out-of-core nonsymmetric solver while the structure uses an in-core symmetric solver.

Degrees of Freedom The degrees of freedom in a fluid analysis are the velocities or, for the mixed method, the velocity and the pressure. When the pressure is not included explicitly as a degree of freedom, the incompressibility constraint is imposed using a penalty approach. If a strongly coupled fluid-thermal problem is solved, the degrees of freedom are either the velocities and temperatures or the velocities, pressure, and temperature. For a three dimensional problem, the number of degrees of freedom could be 5. The degrees of freedom associated with the solid are the conventional displacements or the displacements and temperatures.

Main Index

322 Marc Volume A: Theory and User Information

Element Types The fluid region can be represented using the conventional displacement elements in Marc. When using the mixed method, the pressure has the same order and interpolation functions as the velocity. In a coupled fluid-thermal analysis, the temperature also has the same order as the velocity. Hence, the element types available are: Planar Type

3-node

linear

3

4-node

isoparametric bilinear

4-node

isoparametric bilinear reduced integration

115

6-node

isoparametric triangle

125

8-node

isoparametric biquadratic

27

8-node

isoparametric biquadratic reduced integration

54

11

Axisymmetric Type

3-node

linear

2

4-node

isoparametric bilinear

4-node

isoparametric bilinear reduced integration

116

6-node

isoparametric triangle

126

8-node

isoparametric biquadratic

28

8-node

isoparametric biquadratic reduced integration

55

10

Three Dimensional Type

4-node

tetrahedron

134

8-node

trilinear brick

8-node

trilinear brick with reduced integration

20-node

brick

21

20-node

brick with reduced integration

57

7 117

The three-node triangular elements or the four-node tetrahedral element give poor results when used with the penalty formulation. The shape functions used are identical to those used for structural analyses and can be found in any finite element textbook.

Main Index

CHAPTER 6 323 Nonstructural and Coupled Procedure Library

All of the mesh generation capabilities in Marc Mentat can be used to generate the fluid mesh. Furthermore, Marc Mentat can be used to visualize the results in a manner consistent with structural analyses. Marc’s implementation of the Navier-Stokes equations utilizes the natural boundary condition. At nodal points, you can prescribe the time dependent values of the velocity and temperature. This can be achieved by using the FIXED VELOCITY, FIXED TEMPERATURE, VELOCITY CHANGE, and/or TEMP CHANGE options. The FORCDT user subroutine can be used for time-dependent behavior or the TABLE option. Gravity and centrifugal loads can also be applied. For coupled fluid-solid interaction problems, the pressure of the fluid is automatically applied to the structure. The resultant deformation of the structure is applied to the fluid boundaries. In the current release, only small deformations of the solid are permitted. The viscosity, mass density, conductivity, and specific head are defined through the ISOTROPIC option. The STRAIN RATE or TABLE option is used to define non-Newtonian viscous behavior. The penalty parameter can be entered through the PARAMETERS option. Note:

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 the fluid and/or heat transfer portion of analysis in coupled fluid-solid, fluid-thermal, and fluid-thermal-solid.

Coupled Analyses The definition of coupled systems includes the multiple domains and independent or dependent variables describing different physical systems. In the situation with multiple domains, the solution for both domains is obtained simultaneously. Similarly, the dependent variables cannot be condensed out of the equilibrium equations explicitly. Coupled systems can be classified into two categories: 1. Interface variables coupling: In this class of problems, the coupling occurs through the interfaces of the domain. The domains can be physically different (for example, fluid-solid interaction) or physically the same but with different discretization (for example, mesh partition with explicit/implicit procedures in different domains).

Figure 6-39 Fluid-structure Interaction (Physically Different Domains)

Main Index

324 Marc Volume A: Theory and User Information

2. Field variables coupling: In this, the domain can be the same or different. The coupling occurs through the governing differential equations describing different physical phenomenon; for example, coupled thermo-mechanical problems.

Figure 6-40 Metal Extrusion with Plastic Flow Coupled with Thermal Field

Marc can solve the following types of coupled problems: fluid-solid, fluid-thermal, fluid-solid-thermal interaction, piezoelectric, electrostatic-structural, thermo-electrical (Joule heating), thermo-mechanical, electrical-thermal-mechanical (Joule Mechanical), fluid-soil (pore pressure), electromagnetic, and electromagnetic-thermal. The type of coupling is summarized in Table 6-10.

Main Index

CHAPTER 6 325 Nonstructural and Coupled Procedure Library

6 Nonstru ctural and Coupled Procedu re Library

Table 6-10

Summary of Coupled Procedures

Interaction

Category

Coupling

Thermal- Mechanical

Field

Weak

Fluid-Solid added mass approach general approach

Interface Interface

Weak Weak

Fluid-Thermal channel approach general approach

Interface Field

Weak Strong or Weak

Fluid-Thermal-Solid

Field/Interface

Strong or Weak/Weak

Piezoelectric

Field

Strong

Electrostatic-Structural

Field

Weak

Thermal-Electric (Joule)

Field

Weak

Electrical-Thermal- Mechanical

Field

Weak

Fluid-Pore

Field

Strong

Electromagnetic

Field

Strong

Electromagnetic-Thermal

Field

Weak

There are two approaches for solving fluid-solid interaction problems. In the first approach, the fluid is assumed to be inviscid and incompressible. The effect of the fluid is to augment the mass matrix of a structure. Modal shapes can be obtained for a fluid/solid system; the modal superposition procedure predicts the dynamic behavior of the coupled fluid/solid system. This prediction is based on extracted modal shapes. This method is discussed later. The general fluid-solid capability models nonlinear transient behavior and is discussed in the fluid mechanics section. There are two approaches for solving fluid-thermal interaction problems. The first is for a fluid constricted to move through thin areas and is implemented using the CHANNEL option. This is discussed earlier in this chapter. The second approach solves the coupled Navier-Stokes equations and is discussed in the fluid mechanics section. The fluid-thermal-mechanical capability is described in more detail in the fluid mechanics section. In the coupled thermo-electrical problem, the coupling takes place through the temperature-dependent electrical conductivity in the electrical problem and the internal heat generation caused by electrical flow in the thermal problem. The program solves for the voltage and temperature distribution. Similarly, the coupling between the thermal and mechanical problems takes place through the temperature-dependent material properties in the mechanical (stress) problem and the internal heat

Main Index

326 Marc Volume A: Theory and User Information

generation in the mechanical problem caused by plastic work, which serves as input for the heat transfer problem. The temperature distribution and displacements are obtained. In each of the coupled problems described above, two analyses are performed in each load/time increment. Iterations can also be carried out within each increment to improve the convergence of the coupled thermo-electrical and thermo-mechanical solutions. In the coupled fluid-soil model, the fluid is assumed to be inviscid and incompressible. The effect of the fluid is to augment the stress in the soil material to satisfy equilibrium, and to influence the soil’s material behavior. In the electromagnetic analysis, the fully coupled Maxwell’s equations are solved. In the latter two analyses, the equations (fluid flow/structural or electrical/magnetic) are solved simultaneously.

Thermal Mechanically Coupled Analysis Many operations performed in the metal forming industry (such as casting, extrusion, sheet rolling, and stamping) can require a coupled thermo-mechanical analysis. The observed physical phenomena must be modeled by a coupled analysis if the following conditions pertain: • The body undergoes large deformations such that there is a change in the boundary conditions associated with the heat transfer problem. • Deformation converts mechanical work into heat through an irreversible process which is large relative to other heat sources. In either case, a change in the temperature distribution contributes to the deformation of the body through thermal strains and influences the material properties. Marc has a capability that allows you to perform mechanically coupled analysis. This capability is available for all stress elements and for small displacement, total Lagrangian, updated Lagrangian, or rigid plastic analysis. The COUPLE parameter is used to invoke this option. When defining the mesh, if you specify the element as a stress type through the CONNECTIVITY option, Marc generates an associated heat transfer element, if possible. The region having an associated heat transfer element has coupled behavior. If you specify the element as a heat transfer type through the CONNECTIVITY option, that region is considered rigid. Only heat transfer is performed in that region. Marc uses a staggered solution procedure in coupled thermo-mechanical analysis. It first performs a heat transfer analysis, then a stress analysis. Use the CONTROL option to enter the control tolerances used in the analysis. Depending on the type of stress analysis performed, Marc can perform three different types of coupled analysis: • Quasi-static coupled analysis: This comprises of a transient heat transfer pass and a static mechanical pass. Fixed stepping can be specified using TRANSIENT NON AUTO and adaptive stepping can use TRANSIENT or AUTO STEP. AUTO STEP is preferred over the TRANSIENT option. • Creep coupled analysis: This comprises of a transient heat transfer pass and a creep mechanical

Main Index

CHAPTER 6 327 Nonstructural and Coupled Procedure Library

pass. Fixed stepping can be specified using CREEP INCREMENT and adaptive stepping can use AUTO CREEP or AUTO STEP • Dynamic coupled analysis: This comprises of a transient heat transfer pass and a dynamic mechanical pass. Fixed stepping can be specified using DYNAMIC CHANGE and adaptive stepping can use AUTO STEP. Load control and time step control can be specified in either of two ways: • A fixed time step/load size can be specified by using the TRANSIENT NON AUTO option, the CREEP INCREMENT option, or the DYNAMIC CHANGE option. In these cases, mechanical loads and deformations are incremental quantities that are applied to each step. Fluxes are total quantities. Time variations for the mechanical and thermal loads can be specified using appropriate s. • An adaptive time step/load size can be specified by using the AUTO CREEP option or the AUTO STEP option. In this case, mechanical loads and deformations are entered as the total quantities that are applied over the load set. Fluxes are total quantities. By default, mechanical loads are linearly increased while thermal loads are applied instantaneously. • Exercise caution when applying boundary conditions. Use the FIXED DISP, FIXED TEMPERATURE, DISP CHANGE, TEMP CHANGE, or TABLE options for mechanical or thermal boundary conditions, respectively. There are two primary causes of coupling. First, coupling occurs when deformations result in a change in the associated heat transfer problem. Such a change can be due to either large deformation or contact. Large deformation effects are coupled into the heat transfer problem only if the LARGE STRAIN or UPDATE parameter is invoked. The gap element in Marc (Type 12) has been modified so that if no contact occurs, the gap element acts as a perfect insulator. When contact does occur, the gap element acts as a perfect conductor. The second cause of coupling is heat generated due to inelastic deformation. The irreversibility of plastic flow causes an increase in the amount of entropy in the body. This can be expressed as: ·p TS· = fW

(6-157)

· p is the fraction of the rate of plastic work dissipated into heat. Farren and Taylor measure f where fW as approximately 0.9 for most metals. Using the mechanical equivalent of heat ( M ), the rate of specific volumetric flux is: ·p⁄ρ R = MfW

(6-158)

Use the CONVERT model definition option to define Mf . Of course, all mechanical and thermal material properties can be temperature dependent. The governing matrix equations can be expressed as:

Main Index

Mu·· + Du· + K ( T ,u ,t )u = F

(6-159)

C T ( T )T· + K T ( T )T = Q + Q I + Q F

(6-160)

328 Marc Volume A: Theory and User Information

I

F

In Equation (6-160), Q represents the amount of heat generated due to plastic work and Q represents the amount of heat generated due to friction. The specific heat matrix C T and conductivity matrix K T can be evaluated in the current configuration if the updated Lagrange option is used. Note:

All terms except M can be temperature dependent.

Coupled Acoustic-Structural Analysis In a coupled acoustic-structural analysis, both the acoustic medium and the structure are modeled. In this way, the effect of the acoustic medium on the dynamic response of the structure and of the structure on the dynamic response of the acoustic medium can be taken into account. Such a coupled analysis is especially important when the natural frequencies of the acoustic medium and the structure are in the same range. In Marc, only a harmonic coupled acoustic-structural analysis can be performed. Since the interface between the acoustic medium and the structure is determined automatically by Marc based on the CONTACT option, setting up the finite element model is relatively easy since the meshes do not need to be identical at the interface. The acoustic medium will be called the fluid, although it might also be a gas, and is considered to be inviscid and compressible. The equilibrium equation is given by: ∇p + ρ f u·· = 0

(6-161)

in which p is the pressure, ρ f is the fluid density, u is the displacement vector and a superposed dot indicates differentiation with respect to time. Using the bulk modulus of the fluid K f , the constitutive behavior can be written as: p = – K f ∇u

(6-162)

The Equations (6-161) and (6-162) can be combined to: 1 1 ------ p·· – ----- ∇2p = 0 Kf ρf

(6-163)

It is also possible to add a damping term ru· to Equation (6-161), with r the resistivity or fluid drag: ∇p + ru· + ρ f u·· = 0

(6-164)

Since we restrict the discussion to harmonic analyses, we can write u· = iωu , with ω the excitation frequency and i the imaginary unit, so that Equation (6-164) reduces to: 1 1 ------ p·· – ----- ∇2p = 0 Kf ρf in which the complex density ρ f is given by:

Main Index

(6-165)

CHAPTER 6 329 Nonstructural and Coupled Procedure Library

ir ρ f = ⎛ ρ f – ----⎞ ⎝ ω⎠

(6-166)

The weak form of Equation (6-165) is obtained in a standard way by introducing the variational field δp and integrating over the fluid volume V : ⎛ 1 ··

⎞

1

- p – ----- ∇2p⎠ dV ∫ δp ⎝ ----Kf ρ

(6-167)

= 0

f

V

Applying the Green’s divergence theorem to this expression yields: ∂p

- p + ----- ∇δp ∇p⎞⎠ dV + ∫ ----- δp ----- dA ∫ ⎛⎝ δp ----∂n Kf ρ ρ 1 ··

V

1

1

f

Γ f

= 0

(6-168)

in which Γ represents the boundary of the fluid with an inward normal n . Along the boundary, various conditions can occur: • The pressure p is prescribed on the boundary Γ p . • The normal acceleration is prescribed to be a n on the accelerating boundary Γ a . • The normal acceleration of the fluid equals the normal acceleration of the solid, u·· f n = u·· s n , on the fluid-structure interface Γ f s . • Nonreflecting or reactive boundary conditions are introduced using a spring-dashpot analogy on 1 ∂p Γ as --- ----- = p· ⁄ c + p·· ⁄ k . In this way, a spring and a dashpot are placed in series between fn

ρ ∂n

I

I

the acoustic medium and its boundary, with k I the spring and c I the dashpot parameter, both per unit area. Some classical conditions can be modeled by this expression: ∂p 1. Free surfaces waves in a gravity field: ----- = p·· ⁄ g , with g the gravity acceleration; ∂n ∂p 2. The plane wave radiation boundary condition: ----- = p· ⁄ c , with c the wave velocity; ∂n

3. Using the complex admittance 1 ⁄ z ( ω ) of the boundary, with z ( ω ) the impedance, the normal velocity can be related to the pressure by u· f n = p ⁄ z ( ω ) = ( 1 ⁄ c I + iω ⁄ k I )p , so that a given z ( ω ) can be modeled by setting 1 ⁄ c I and 1 ⁄ k I . Upon discretizing the fluid and the solid using finite elements, the fluid pressure and the displacements of the solid can be approximated in a standard way, so that Equation (6-168) yields: ⎧

∫ ⎨⎩ δp

V

T

p 1 pT T p 1 pT ⎫ N ------ N p·· + δp ( ∇N ) ----- ( ∇N )p ⎬dV – Kf ρf ⎭

+

∫

Γf n

Main Index

∫ δp

Γa

T

p

N a n dA –

T p 1 pT · p 1 p T ·· δp ⎛ N ---- N p + N ---- N p⎞ dA = 0 ⎝ cI ⎠ kI

∫

Γf s

T

p

δp N N

uT

Gu·· dA (6-169)

330 Marc Volume A: Theory and User Information

where p and u contain the pressure and displacement degrees of freedom, N contains the interpolation functions and G is a transformation matrix to relate the displacements in normal direction to the global displacement components. Since Equation (6-169) must be valid for arbitrary admissible values of δp , · ·· ·· 2 2 evaluating the various integrals and using p = iωp , p = – ω p and u = – ω u , results in: ⎧ ⎫ 2 2 ⎨ K f + iωC f – ω M f ⎬p + ω S f s u = F f ⎩ ⎭

(6-170)

In order to end up with a set of coupled equations, we need to consider the solid as well. The effect of the fluid on the solid originates from the fluid pressure at the fluid-solid interface. This can be easily included by evaluating the virtual work corresponding to the fluid pressure: δW

p

=

∫

Γ

– δ u n s p dA =

∫

Γ

fs

T

T

u

–δ u G N N

pT

T T

p dA = – δu S f s p

(6-171)

fs

Notice that the minus sign has been used to express that u ns is positive in the outward direction of the solid. Including Equation (6-171), the solid behavior for a harmonic analysis is governed by: ⎧ ⎫ T 2 ⎨ K s + iωC s – ω M s ⎬u + S f s p = F s ⎩ ⎭

(6-172)

with K s the stiffness matrix, which can include stress-stiffening, C s is the damping matrix, M s the mass matrix, and F s the external load vector, except for the fluid pressure. –2

Premultiplying Equation (6-170) by ω and combining the result with Equation (6-172) gives the desired coupled complex equation system: –2

ω Af T

Sf s

Sf s As

p u

–2

=

ω Ff Fs

(6-173)

in which A f = K f + iωC f and A s = K s + iωC s . The procedure to perform a coupled acoustic-structural is as follows. The acoustic medium and the structure are modeled separately; the acoustic structure using heat transfer elements with acoustic material properties and the structure using conventional stress elements. The elements representing the acoustic medium are assigned to an acoustic contact body and the elements representing the solid to a deformable contact body. If the acoustic medium is not surrounded completely by a deformable structure and one wants to, for example, model radiation boundary conditions along this part of the acoustic medium, then one can define rigid contact bodies in this area. Like deformable bodies, rigid bodies can be used to define the spring-dashpot analogy defined before. A harmonic analysis can be performed

Main Index

CHAPTER 6 331 Nonstructural and Coupled Procedure Library

based on initial contact, so using the undeformed configuration of the contact bodies, but also after a preload of the deformable contact bodies. In the latter case, it might be necessary to remesh the acoustic and/or deformable bodies before the harmonic analysis can be performed, since during the static loading of the deformable bodies the deformation of the acoustic bodies is not taken into account. The elements which are available for coupled-structural acoustic analysis are described in Table 6-11. Table 6-11

Element Types for Coupled-Structural Acoustic Analysis

Element Type

Description

37, 39

3-, 4-node planar

121

4-node reduced integration planar

38, 40

3-, 4-node axisymmetric

122

4-node reduced integration axisymmetric

135

4-node tetrahedral

Marc computes and prints the following quantities: pressure and pressure gradient at the integration points. The nodal point data consists of the pressure and the source. The ACOUSTIC parameter is used to indicate that a coupled acoustic-structural analysis is performed. In addition to the CONTACT option, the ACOUSTIC and REGION model definition options are used to define the material properties of the acoustic medium and to set which elements correspond to the solid and the fluid region. Typical boundary conditions for the acoustic medium can be entered using the FIXED PRESSURE model definition and PRESS CHANGE history definition option. The DIST SOURCES and POINT SOURCE model definition and DIST SOURCES and POINT SOURCE history definition options are used to define the load on the acoustic medium. The HARMONIC history definition option is used to define the excitation frequencies. Spatially and frequency dependent boundary conditions may be defined by referencing the TABLE option.

Fluid/Solid Interaction – Added Mass Approach The fluid/solid interaction procedure investigates structures that are either immersed in, or contain a fluid. Examples of problems that make use of this feature are vibration of dams, ship hulls, and tanks containing liquids. Marc is capable of predicting the dynamic behavior of a structural system that is subject to the pressure loading of fluid. The fluid is assumed to be inviscid and incompressible; for example, water. In Marc, the fluid is modeled with heat transfer elements (potential theory) and the structure is modeled with normal stress or displacement elements. The element choice must ensure that the interface between the structural and fluid models has compatible interpolation; that is, both solid and fluid elements are either first order or second order. The TYING option can be used to achieve compatibility if necessary. To identify the interfaces between the fluid and the structure, the FLUID SOLID model definition set is necessary.

Main Index

332 Marc Volume A: Theory and User Information

During increment zero, Marc calculates the stiffness matrix for the structure and the mass matrix for the structure augmented by the fluid effect. Marc then extracts the eigenvalues of the coupled system using the MODAL SHAPE option. The modal superposition procedure can then be used to predict the time response of the coupled system. DYNAMIC CHANGE can be used to perform modal superposition. To input properties of solids and the mass density of the fluid elements, use the ISOTROPIC model definition option. The calculation of the structural mass augmentation requires triangularization of the fluid potential matrix: this matrix is singular, unless the fluid pressure is fixed at least at one point with the FIXED DISP option. Technical Background In a fluid/solid interaction problem, the equations of motion can be expressed as 1 T M s a + Ku = ----- S p ρf

(6-174)

The pressure vector p can be calculated from: – Sa = Hp

(6-175)

The matrices in Equations (6-174) and (6-175) are defined as β

α

∫ Ni Ni

Ms =

ρ s dV

(6-176)

V

K =

β

α

∫ β i j D i j k l β k l dV

(6-177)

V

S =

A

H =

α

β

∫

R ρ f n i N i dA

∫ V

f

β

α

∂R ∂R ---------- ---------- dV ∂x i ∂x i

where

Main Index

(6-178)

T

ρ f and ρ s

are mass densities of the fluid and solid, respectively

a

is the acceleration vector

u

is the displacement vector

βi j

is the strain displacement relation

Di j k l

is the material constitutive relation

(6-179)

CHAPTER 6 333 Nonstructural and Coupled Procedure Library

Ni

is the displacement interpolation function

R

is the pressure interpolation function

ni

is the outward normal to the surface with fluid pressure p

A

T

is the surface on which the fluid pressure acts

In the present case, the fluid is assumed to be incompressible and inviscid. Only infinitesimal displacements are considered during the fluid vibration, so that the Eulerian and material coordinates coincide. Substituting Equation (6-175) into Equation (6-174), we obtain: ( M s + S T H – 1 S ⁄ ρ f )a + Ku = 0 or

(6-180)

Ma + Ku = 0 This equation now allows the modes and frequencies of the solid structure immersed in the fluid to be obtained by conventional eigenvalue methods.

Coupled Electrostatic-Structural Analysis In a coupled electrostatic-structural analysis, both the electrostatic field and the structure are modeled. In this analysis type, the Coulomb force (the force between charged bodies) links the electrostatic part to the structural part, and, in turn, the deformation influences the electrostatic field. This is different from a piezoelectric analysis where a change in the electrostatic field causes the deformation which causes a change in the electrostatic field (movement of charge), but Coulomb forces are not taken into account. The electrostatic-structural coupling is a weak coupling, where in the first pass the electrostatic field is computed, then the corresponding Coulomb forces are transferred to the structural pass, and finally the structural pass is evaluated. In a next cycle, the newly deformed state is used in the electrostatic field calculation. Since the electrostatic solution is a steady-state solution, a time dependent problem will be considered as quasi static for the electrostatic part. In general, in an electrostatic analysis, we can distinguish conductors and insulators. For example, in a capacitor, the plates carrying a charge are the conductors, and the dielectric or air between the plates is the insulator. When a potential difference is applied between the plates, the surfaces of these plates are charged. In Marc, the calculation of the charge on the different bodies is performed using the concept of contact bodies. In the case of the capacitor, the plates and the dielectric are separate contact bodies. The charge is then computed at the interface of two contact bodies. Note that it is necessary that the insulating contact body is touching the conducting contact body. In other words, the contact bodies on which a Coulomb force is acting are the ones being touched. Coulomb Force Two methods are available to compute the Coulomb force in a coupled electrostatic-structural analysis. The default method uses the following equation:

Main Index

334 Marc Volume A: Theory and User Information

qE F C o u l o m b = ------2

(6-181)

where q is the charge at the node where the Coulomb force is calculated, and E is the electric field at the insulator side of the interface. Note that in principle the Coulomb force gets half the contribution from both sides of the interface, but it is assumed that one side is the conductor where E ≈ 0 , so this contribution is neglected. This method works well if the charged bodies are relatively close to each other (within 20 to 40 element edge lengths) such as the capacitor shown in Figure 6-41. When the gradient in the electric field becomes too large, the computation of the Coulomb force becomes less accurate. This is especially true when two charged bodies are located far away from each other. In such cases, the contribution to the Coulomb force from other bodies is small relative to the self contribution. For this situation, the following equation is available to compute the Coulomb force n

Fi =

∑ j = 1, i ≠ j

1 QiQj ------------ ----------4πε 0 r 2

(6-182)

ij

where Q i and Q j are the charge on two nodes, r i j the distance between the two charged nodes, and ε 0 the permittivity of the medium between the two nodes. This means that for each node carrying a charge the interaction with all the other nodes carrying a charge is calculated. However, the relevant nodes carrying a charge are at the surface of contact bodies, which reduces the number of calculations. The total charge computed on the surface of a contact body will balance the external and reaction charge on other nodes in the contact body. This procedure is activated by the ELECTRO,2 parameter.

Figure 6-41 Capacitor with Two Closely Spaced Charged Bodies

Equation (6-182) is valid in a 3-D analysis. For an axisymmetric analysis, the charge carrying nodes are extended to circles. Equation (6-182) is used for a number of points on the circle. For a planar analysis, the nodal charge is a line charge and the following equation then holds for the Coulomb force: n

Fi =

∑ j = 1, i ≠ j

Main Index

1 QiQj ------------ -----------2πε 0 r i j

(6-183)

CHAPTER 6 335 Nonstructural and Coupled Procedure Library

Analysis Procedure The procedure to perform a coupled electrostatic-structural analysis is as follows. The different bodies (conductors and insulators) that can be distinguished must be selected as contact bodies. The way the contact bodies are touching is important for the computation of the Coulomb Force. The contact bodies on which a Coulomb force is acting are the ones being touched, so in general a conductor is being touched, and air or a dielectric is the touching contact body. Both electrostatic and structural element types are available. If an electrostatic element type is selected, then it is not active in the structural pass. This means that this body does not deform, unless remeshing is carried out. When a structural element is selected the corresponding electrostatic element will be automatically used in the electrostatic pass. The ELECTRO parameter together with the STRUCTURAL parameter is used to indicate the coupled electrostatic-structural analysis. In addition the to the CONTACT option, the ISOTROPIC or ORTHOTROPIC model definition option is used to define the material properties for both the electrostatic and structural pass. Specify nodal constraints using the FIXED DISP or FIXED POTENTIAL option. Input nodal loads using the POINT LOAD option or nodal charges using the POINT CHARGE option. Specify distributed loads with the DIST LOADS option and distributed charges with the DIST CHARGE option. Fixed nodal displacements and potentials, or nodal forces and charges can also be specified by the FORCDT user subroutine, nonuniform distributed loads can be specified by the FORCEM user subroutine, and nonuniform distributed charges can be specified by the FLUX user subroutine. For the history definition, the AUTO LOAD and AUTO STEP options can be used.

Coupled Thermal-Electrical Analysis (Joule Heating) The coupled thermal-electrical analysis procedure can be used to analyze electric heating problems. The coupling between the electrical problem and the thermal problem in a Joule heating analysis is due to the fact that the resistance in the electric problem is dependent on temperatures, and the internal heat generation in the thermal problem is a function of the electrical flow. Marc analyzes coupled thermo-electrical (Joule heating) problems. Use the JOULE parameter to initiate the coupled thermo-electrical analysis. This capability includes the analysis of the electrical problem, the associated thermal problem, and the coupling between these two problems. The electrical problem is a steady-state analysis and can involve current and/or voltage boundary conditions as well as temperature-dependent resistivity. The thermal analysis is generally a transient analysis with temperature-dependent thermal properties and time/temperature-dependent boundary conditions. Use the ISOTROPIC, ORTHOTROPIC, TEMPERATURE EFFECTS, ORTHO TEMP, or TABLE model definition options to input reference values of thermal conductivity, specific heat, mass density, and electrical resistivity, as well as their variations with temperatures. The mass density must remain constant throughout the analysis. Use the FIXED VOLTAGE model definition option for nodal voltage boundary conditions, and the POINT CURRENT and/or DIST CURRENT model definition options for current boundary conditions. No initial condition is required for the electrical problem, since a steady-state solution is obtained.

Main Index

336 Marc Volume A: Theory and User Information

In the thermal problem, you can use the INITIAL TEMP, FILMS, POINT FLUX, DIST FLUXES, and FIXED TEMPERATURE model definition options to prescribe the initial conditions and boundary conditions. Use the FILM and FLUX user subroutines or tables for complex convective and flux boundary conditions. To enter the unit conversion factor between the electrical and thermal problems, use the JOULE model definition option. Marc uses this conversion factor to compute heat flux generated from the current flow in the structure. Use the STEADY STATE, TRANSIENT, POINT CURRENT, DIST CURRENT, VOLTAGE CHANGE, POINT FLUX, DIST FLUXES, and TEMP CHANGE history definition options for the incrementation and change of boundary conditions. A weak coupling between the electrical and thermal problems is assumed in the coupled thermo-electrical analysis, such that the distributions of the voltages and the temperatures of the structure can be solved separately within a time increment. A steady-state solution of the electrical problem (in terms of nodal voltages) is calculated first within each time step. The heat generation due to electrical flow is included in the thermal analysis as an additional heat input The temperature distribution of the structure (obtained from the thermal analysis) is used to evaluate the temperature-dependent resistivity, which in turn is used for the electrical analysis in the next time increment. For output, voltage, current density, and heat generation are available as integration point values. Note that current density must not be confused with Ohmic current. Current density is the electric current per unit area of cross section, while Ohmic current is the current going through the total area. So the latter is a global quantity. Technical Background In the coupled thermo-electrical analysis, the matrix equation of the electrical problem can be expressed as; E

K ( T )V = I

(6-184)

and the governing equation of the thermal problem is: E C T ( T )T· + K T ( T )T = Q + Q

In Equations (6-184) and (6-185): K

Main Index

E

is the temperature-dependent electrical conductivity matrix

I

is the nodal current vector

V

is the nodal voltage vector

C T ( T ) and K T ( T )

are the temperature-dependent heat capacity and thermal conductivity matrices, respectively

T

is the nodal temperature vector

T·

is the time derivative of the temperature vector

(6-185)

CHAPTER 6 337 Nonstructural and Coupled Procedure Library

is the heat flux vector

Q Q

E

is the internal heat generation vector caused by the current flow. E

E

The coupling between the electrical and thermal problems is through terms K and Q in Equations (6-184) and (6-185). The selection of the backward difference scheme for the discretization of the time variable in Equation (6-185) yields the following expression: 1 1 ----- [ C T ( T ) ] + K T ( T )T n = Q n + Q nE + ----- C T ( T )T n – 1 Δt Δt

(6-186)

Equation (6-186) is used for the computation of nodal temperatures in each time increment Δt . The internal heat generation vector Q Q

E

=

∫B

E

is computed from:

T E

q dV

(6-187)

V

q

E

2

= i R

(6-188)

where i and R are the current and electrical resistance, respectively. The controls for the heat transfer option allow input of parameters that govern the convergence solution and accuracy of heat transfer analysis.

Coupled Electrical-Thermal-Mechanical Analysis Coupled electrical-thermal-mechanical analysis (Joule-mechanical) basically combines electricalthermal analysis (Joule heating) with thermal-mechanical analysis. Coupled electrical-thermalmechanical analysis is handled using a staggered solution procedure. Using this approach, the electrical problem is solved first for the nodal voltages. Next, the thermal problem is solved to obtain the nodal temperatures. The mechanical problem is solved last for the nodal displacements. Coupling between the electrical and thermal problems is mainly because of heat generation due to electrical flow Q E (Joule heating). The thermal and mechanical problems are coupled through thermal strain loads F T and heat generation due to inelastic deformation Q I and friction Q F . Additional coupling may be introduced in case of temperature-dependant electrical conductivity K E and mechanical stiffness K M . Nonlinearities may arise in the thermal problem due to convection, radiation, and temperature-dependant thermal conductivity and specific heat. The mechanical problem may involve geometric and material nonlinearities. Contact is another source of nonlinearity. If contact occurs between deformable bodies or deformable and rigid bodies in the mechanical problem, boundary conditions of the electrical and thermal problems are updated to reflect the new contact conditions.

Main Index

338 Marc Volume A: Theory and User Information

Electrical

Q K

E

Thermal

T

M

I

F

F ,K

E

Q,Q

Mechanical

The matrix equations governing the electrical, thermal and mechanical problems can be expressed as: K E ( T )V = I C T ( T )T· + K T ( T )T = Q + Q E + Q I + Q F Mu·· + Du· + K M ( T ,u ,t )u = F + F T where V

is the nodal voltage vector

T

is the nodal temperature vector

u

is the nodal displacement vector

KE(T )

is the temperature-dependent electrical conductivity matrix

I

is the nodal current vector

CT( T )

is the temperature-dependent heat capacity matrix

KT(T )

is the temperature-dependent thermal conductivity matrix

Q

is the heat flux vector

QE

is the heat generation due to electrical flow vector

QI

is the heat generation due to inelastic deformation vector

QF

is the heat generation due to friction vector

M

is the mass matrix

D

is the damping matrix

K M ( T ,u ,t )

is the temperature, deformation and time-dependent stiffness matrix

F

is the externally applied force vector

FT

is the force due to thermal strain vector

The JOULE and COUPLE parameters are needed to initiate the coupled electrical-thermal-mechanical analysis. When defining the mesh through the CONNECTIVITY model definition option, specify the elements as stress type. Marc internally switches to the associated heat transfer element in the electrical and thermal passes.

Main Index

CHAPTER 6 339 Nonstructural and Coupled Procedure Library

The FIXED VOLTAGE model definition option can be used for nodal voltage boundary conditions, and POINT CURRENT and/or DIST CURRENT model definition options for current boundary conditions. No initial condition is required for the electrical problem, since a steady-state solution is obtained. In the thermal problem, INITIAL TEMP, FILMS, POINT FLUX, DIST FLUXES, and FIXED TEMPERATURE model definition options can be used to prescribe the initial conditions and boundary conditions. The FILM and FLUX user subroutines can be used for complex convective and flux boundary conditions. To enter the unit conversion factor between the electrical and thermal problems, use the JOULE model definition option. Marc uses this conversion factor to compute heat flux generated from

the current flow in the structure. In the mechanical problem, the usual structural model definition options such as FIXED DISP, POINT LOAD, and DIST LOADS are used to prescribe the boundary conditions. The history definition options (VOLTAGE CHANGE, POINT CURRENT, DIST CURRENT, TEMP CHANGE, POINT FLUX, DIST FLUXES, DISP CHANGE, POINT LOAD, and DIST LOADS) for the incrementation and change of boundary conditions. JOULE and CONVERT model definition options are used to enter the conversion factor for the electrical-

thermal and the thermal-mechanical problems.

Main Index

340 Marc Volume A: Theory and User Information

Resistance A resistor is a device that can dissipate electric energy. For a pure resistor, this usually happens in the form of heat. This energy per unit time (or power) depends on the current in the resistor and its resistance. Resistance is always associated with all conductors allowing flow of electric current. A typical model can contain a number of conductors allowing flow of electric current, which gives rise to a resistance value for each conductor. All conductors in a model are assumed to be bodies and defined as a set of elements. This is done using the THERMAL CONTACT model definition option. Two conductors can touch each other cannot overlap. If two conductors touch, it implies flow of current between the two. A sub-set of the conductor bodies can be considered for a resistance computation. This subset is specified using the EMRESIS history definition option, which refers to the bodies defined on the THERMAL CONTACT model definition option. Marc performs a resistance computation only if the EMRESIS history definition option is specified in the input file. A Joule heating analysis is used to compute the resistance values. All insulators in the problem are neglected for modeling. The computation of the resistance values results from the usual joule heating analysis with some constraints on boundary conditions: there must be at least one electric potential boundary condition on any node. If no boundary condition is specified on a portion of the problem boundary, it is assumed to satisfy homogeneous Neumann condition. The resistivity of each material is specified as per the usual Joule heating analysis. If the resistivity of any material is much higher than those of other materials then that material is to be treated as an insulator and should not be included in the model. Technical Background Ohms law for conductors is: V R = ---I

(6-189)

V2 W E = I 2 R = ------- = VI R

(6-190)

where: I

is the current through the resistor

R

is the resistance

V

is the voltage across it

The conductance G is given by: 1 G = ---R

Main Index

(6-191)

CHAPTER 6 341 Nonstructural and Coupled Procedure Library

Consider a single conducting body placed in an infinite homogenous insulating medium. The insulating medium can be assumed to have negligible conductivity, in which case the current through it is negligible. All current flows in the conductor. The current density J is then defined as the normal current passing through a unit cross-sectional area. This means that: I =

∫ ∫ J ⋅ dS

(6-192)

S

where S is the cross-sectional surface of the conductor. Conduction current I is conserved; hence, I is same for any conductor cross section. The electric field E is related to current density J in the conductor by: (6-193)

J = E where σ is the conductivity of the conductor. The power W E in a conductor is also given by: 1 W E = --- ∫ 2

∫ ∫ J ⋅ E dv Vc

1 = --- ∫ 2

1

∫ ∫ --σ- J ⋅ J dv

(6-194)

Vc

where V c is the conductor domain. The electric potential drop V c across the conductor is obtained from the finite element analysis. The resistance is then calculated using Equation (6-190).

Coupled Electromagnetic-Thermal Analysis A coupled electromagnetic thermal analysis couples a harmonic electromagnetic analysis with a thermal analysis. With this analysis type, induction heating processes can be simulated. The implementation in Marc follows a staggered approach. First, a harmonic electromagnetic analysis is performed followed by a thermal analysis. The harmonic electromagnetic field generates induction currents in the model. These induced currents generate heat and a heat flux is computed which is then used in the thermal analysis. Temperature dependency for material data can also be taken into account, which is especially important for the permeability of metals. The relative permeability drops to one when the Curie temperature is reached, which can result in a significant change in the generated heat flux. The depth of the material induction currents generated is an important factor in the heating process. This so-called skin depth is defined as the depth at which the magnitude of the induced current density drops to e at the surface δ =

Main Index

1 ------------- , πfσμ

–1

of the magnitude

(6-195)

342 Marc Volume A: Theory and User Information

where f is the frequency, σ the electrical conductivity, and μ the permeability. Hence, the penetration depth depends on the frequency. Low frequencies are used for more uniform preheating, and higher frequencies are used for surface heating. The heat generated in induction heating analysis is similar to a Joule heating analysis, however now in the harmonic electromagnetic analysis the computed current density is a complex vector instead of a scalar. The local heat generation is (see [Ref. 17]) q

E

1 = --- J σ

2

1 = --- J ⋅ J∗ , σ

(6-196)

with σ the electric conductivity, and J the complex current density. To initiate a coupled electromagnetic thermal analysis, add the EL-MA and HEAT parameters. The electromagnetic pass is a harmonic pass; the thermal part can be either a steady state or a transient analysis. When defining the mesh, if you specify the element as an electromagnetic type through the CONNECTIVITY option, Marc generates an associated heat transfer element. The region having an associated heat transfer element has coupled behavior. If you specify the element as a heat transfer type through the CONNECTIVITY option, that region is only active in the thermal pass. Use the ISOTROPIC or ORTHOTROPIC model definition options to input values for the thermal conductivity, specific heat, mass density, and emissivity, as well as permeability, permittivity, and electric conductivity. Temperature dependency for these material properties can be added when the table driven input option is used. For the electromagnetic pass, boundary conditions can be applied. Use FIXED POTENTIAL to prescribe the magnetostatic or electrostatic potential on nodes, and POTENTIAL CHANGE in the history definition option. To apply nodal currents or nodal charges used POINT CURRENT and POINT CHARGE respectively. Distributed currents or distributed charges can be applied using DIST CURRENT or DIST CHARGE, respectively. The FORCDF and FORCEM user subroutines can be used to manually control the size and/or direction of the different vectors. For the thermal pass INITIAL TEMP, FIXED TEMPERATURE, TEMP CHANGE, DIST FLUXES, POINT FLUX, and FILMS can be used to prescribe the initial conditions and boundary conditions. The FILM and FLUX user subroutines can be used for complex convective and flux boundary conditions. The excitation frequency has to be given for the harmonic electromagnetic pass using the HARMONIC history definition option. The thermal pass can be STEADY STATE or time dependent using the TRANSIENT or AUTO STEP history definition options. If noncompatible units are used in the electromagnetic and thermal analysis, a unit conversion factor between the current density and the generated heat can be used. Use the CONVERT model definition option for this.

Main Index

CHAPTER 6 343 Nonstructural and Coupled Procedure Library

References 1. T. J. R. Hughes, L. P. France, and M. Becestra, “A New Finite Element Formulation for Computational Fluid Dynamics, V. Circumventing the Babuska-Brezzi Conduction, A S PetrovGalerkin Formulation of the Stokes Problem Accommodating Equal-Order Interpolations”, Comp. Meth. in Applied Mech. and Eng., p. 85-90, Vol. 59, 1986. 2. G. Hauke and T. J. R. Hughes, “A unified approach to compressible and incompressible flow”, Comput. Methods Appl. Mech. Eng., p. 389-395, 113, (1994). 3. T. E. Tezduyar, S. Mittal, S. E. Ray, and R. Shih, “Incompressible Flow computations with stabilized bilinear and linear equal order-interpolation velocity-pressure elements”, Comput. Methods. Appl. Mech. Eng., p. 221-242, 95, (1992). 4. B. Ramaswaymy, T. C. Jue, “Some Recent Trends and Developments in Finite Element Analysis for Incompressible Thermal Flows”, Int. J. Num. Meth. Eng., p. 671-707, 3, (1992). 5. A. N. Brooks and T. J. R. Hughes, “Streamline upwind/Petrov-Galerkin formulations for convection dominated flows with particular emphasis on the incompressible Navier-Stokes equations”, Comp. Meth. Appl. Eng., 30, (1982). 6. Codina, R. “Finite element formulation for the numerical solution of the convection-diffusion equation” 1993. 7. Cornfield, G. C., and Johnson, R. H. “Theoretical Predictions of Plastic Flow in Hot Rolling Including the Effect of Various Temperature Distributions.” Journal of Iron and Steel Institute 211, pp. 567-573, 1973. 8. Hsu, M. B. “Modeling of Coupled Thermo-Electrical Problems by the Finite Element Method.” Third International Symposium on Numerical Methods for Engineering, Paris, March, 1983. 9. Peeters, F. J. H. “Finite Element Analysis of Elasto-Hydrodynamic Lubrication Problems.” in Proceedings of the XIth Int. Finite Element Kongress, edited by IKOSS GmbH. Baden- Baden, Germany, Nov. 15-16, 1982. 10. Yu, C C. and Heinrich, J. C. “Petro-Galerkin methods for the time-dependent convective transport equation.” Int. J. Numer. Meth. Engrg., Vol. 23 (1986), 883-901. 11. Yu, C C. and Heinrich, J. C. “Petro-Galerkin methods for multidimensional time-dependent convective transport equation.” Int. J. Numer. Meth. Engrg., Vol. 24 (1987), 2201-2215. 12. Zienkiewicz, O. C. The Finite Element Method in Engineering Science. Third Ed. London: McGraw-Hill, 1978. 13. Zienkiewicz, O. C., and Godbole, P. N. “A Penalty Function Approach to Problems of Plastic Flow of Metals with Large Surface Deformations.” Journal of Strain Analysis 10, 180-183, 1975. 14. Zienkiewicz, O. C., and Godbole, P. N. “Flow of Plastic and viscoPlastic Solids with Special Reference to Extrusion and Forming Processes.” Int. Num. Methods in Eng. 8, 1974. 15. Zienkiewicz, O. C., Loehner, R., Morgan, K., and Nakazawa, S. Finite Elements in Fluid Mechanics – A Decade of Progress, John Wiley & Sons Limited, 1984. 16. J. Goldak, A. Chakravarti, and M. Bibby, “A New Finite Element Model for Welding Heat Sources”, Metallurgical Transactions B., Volume 15B, June 1984, pp. 299 - 305

Main Index

344 Marc Volume A: Theory and User Information

17. S. Clain, J. Rappaz, M. Swierkosz, and R. Touzani, “Numerical Modelling of Induction Heating for two-Dimensional Geometries”,Math. Models Methods Appl. Sci., Vol 3 no 6, 805-822, 1993 18. C. Chaboudez, S. Clain, R. Glardon, J. Rappaz, M Swierkosz, and R. Touzani, “Numerical Modelling of Induction Heating of Long Workpieces”, IEEE Trans. Magn.,Vol 30, 5026-5037, 1994 19. C. Chaboudez, S. Clain, R. Glardon, D.Mari, J. Rappaz, and M Swierkosz, “Numerical Modeling of Induction Heating of Axisymmetric Geometries”, IEEE Trans. Magn.,Vol 33, 739-745, 1997 20. R.A. Rindal, “An analysis of the coupled chemically reacting boundary layer and charring ablator, Part IV: An approach for characterizing charring ablator response with in-depth coking reactions.”, NASA CR-1065, June 1968.

Main Index

Chapter 7 Material Library

7

Main Index

Material Library

J

Linear Elastic Material

J

Composite Material

J

Gasket

J

Nonlinear Hypoelastic Material

J

Thermo-Mechanical Shape Memory Model

J

Mechanical Shape Memory Model

J

Elastomer

J

Time-independent Inelastic Behavior

J

Time-dependent Inelastic Behavior

J

Temperature Effects and Coefficient of Thermal Expansion

J

Time-Temperature-Transformation

J

Low Tension Material

J

Soil Model

J

Damage Models

J

Nonstructural Materials

J

References

346 348

378 383 404

413

419

485

487

514

499 512

429 453

482

479

346 Marc Volume A: Theory and User Information

This chapter describes the material models available in Marc. The models range from simple linear elastic materials to complex time- and temperature-dependent materials. This chapter provides basic information on the behavior of various types of engineering materials and specifies the data required by the program for each material. For example, to characterize the behavior of an isotropic linear elastic material at constant temperatures, you need only specify Young's modulus and Poisson's ratio. However, much more data is required to simulate the behavior of material that has either temperature or rate effects. References to more detailed information are cited in this chapter. Data for the materials is entered into Marc either directly through the input file or by user subroutines. Each section of this chapter discusses various options for organizing material data for input. Each section also discusses the constitutive (stress-strain) relation and graphic representation of the models and includes recommendations and cautions concerning the use of the models.

Linear Elastic Material Marc is capable of handling problems with either isotropic linear elastic material behavior or anisotropic linear elastic material behavior. The linear elastic model is the model most commonly used to represent engineering materials. This model, which has a linear relationship between stresses and strains, is represented by Hooke’s Law. Figure 7-1 shows that stress is proportional to strain in a uniaxial tension test. The ratio of stress to strain is the familiar definition of modulus of elasticity (Young’s modulus) of the material. (7-1)

Stress

E (modulus of elasticity) = (axial stress)/(axial strain)

E 1 Strain Figure 7-1

Uniaxial Stress-Strain Relation of Linear Elastic Material

Experiments show that axial elongation is always accompanied by lateral contraction of the bar. The ratio for a linear elastic material is: v = (lateral contraction)/(axial elongation)

(7-2)

This is known as Poisson’s ratio. Similarly, the shear modulus (modulus of rigidity) is defined as: G (shear modulus) = (shear stress)/(shear strain)

Main Index

(7-3)

CHAPTER 7 347 Material Library

It can be shown that for an isotropic material G = E ⁄ ( 2( 1 + v) )

(7-4)

The shear modulus G can be easily calculated if the modulus of elasticity E and Poisson’s ratio v are known. Most linear elastic materials are assumed to be isotropic (their elastic properties are the same in all directions). Anisotropic material exhibits different elastic properties in different directions. The significant directions of the material are labeled as preferred directions, and it is easiest to express the material behavior with respect to these directions. The stress-strain relationship for an isotropic linear elastic method is expressed as σ i j = λδ i j ε k k + 2Gε i j

(7-5)

where λ is the Lame constant and G (the shear modulus) is expressed as λ = νE ⁄ ( ( 1 + ν ) ( 1 – 2ν ) )

and

(7-6)

G = E ⁄ ( 2( 1 + ν) ) The material behavior can be completely defined by the two material constants E and v . Use the ISOTROPIC model definition option for the input of isotropic linear elastic material constants E (Young’s modulus) and v (Poisson’s ratio). The effects of these parameters on the design can be determined by using the DESIGN SENSITIVITY parameter. The optimal value of the elastic properties for linear elastic analysis can be determined using the DESIGN OPTIMIZATION parameter. The stress-strain relationship for an anisotropic linear elastic material can be expressed as σi j = Ci j k l εk l

(7-7)

The values of C i j k l (the stress-strain relation) and the preferred directions (if necessary) must be defined for an anisotropic material. For example, the orthotropic stress-strain relationship for a plane stress element is

1 C = ------------------------------( 1 – ν 12 ν 21 )

E1

ν 21 E 1

0

ν 12 E 2

E2

0

0

0

( 1 – ν 12 ν 21 )G

(7-8)

There are only four independent constants in Equation (7-8). To input anisotropic stress-strain relations, use the ORTHOTROPIC or ANISOTROPIC model definition option and the ANELAS or HOOKLW user subroutine. The ORTHOTROPIC option allows as many as 9 elastic constants to be defined. The ANISOTROPIC option allows as many as 21 elastic constants to be defined. If the anisotropic material has a preferred direction, use the ORIENTATION model definition

Main Index

348 Marc Volume A: Theory and User Information

option or the ORIENT user subroutine to input a transformation matrix. Refer to Marc Volume D: User Subroutines and Special Routines for information on user subroutines. A Poisson’s ratio of 0.5, which would be appropriate for an incompressible material, can be used for the following elements: Herrmann, plane stress, shell, truss, or beam. A Poisson’s ratio which is close (but not equal) to 0.5 can be used for constant dilation elements and reduced integration elements in situations which do not include other severe kinematic constraints. Using a Poisson’s ratio close to 0.5 for all other elements usually leads to behavior that is too stiff. A Poisson’s ratio of 0.5 can also be used with the updated Lagrangian formulation in the multiplicative decomposition framework using the standard displacement elements. In these elements, the treatment for incompressibility is transparent to you.

Composite Material Composite materials are composed of layers of different materials (or layers of the same anisotropic material) with various layer thicknesses and different orientations. The material in each layer may be either linear or nonlinear. Tightly bonded layers (layered materials) are often stacked in the thickness direction of beam, plate, shell structures, or solids. Figure 7-2 identifies the locations of integration points through the thickness of beam and shell elements with/without the COMPOSITE option. Note that when the COMPOSITE option is used, as shown on the left, the layer points are positioned midway through each layer. When the COMPOSITE option is not used, the layer points are equidistantly spaced between the top and bottom surfaces. Marc forms a stress-strain law by performing numerical integration through the thickness. If the COMPOSITE option is used, the trapezoidal method is employed; otherwise, Simpson’s rule is used.

* * * * Beams or Shells with Composite Option Figure 7-2

* * * * * Beams or Shells without Composite Option

Integration Points through the Thickness of Beam and Shell Elements

Figure 7-3 shows the location of integration points through the thickness of composite continuum elements. Marc forms the element stiffness matrix by performing numerical integration based on the standard isoparametric concept.

Main Index

CHAPTER 7 349 Material Library

* * * * Figure 7-3

* * * * Integration Points through the Thickness of Continuum Composite Elements

Layered Materials To model layered materials including plates, shells, beams, and solids 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, various constitutive laws can be used. 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 0o ply angle within each element is defined in the ORIENTATION option. The ply thickness and the ply angle can be used as design variables in a design sensitivity analysis. The optimal values can be determined using the design optimization capability for linear elastic analysis. The material identification number specified in the COMPOSITE option, is cross-referenced with the material identification number supplied in the ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, NLELAST, TEMPERATURE EFFECTS, ORTHO TEMP, WORK HARD, and STRAIN RATE options. The ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC model definition options allow you to input material constants such as Young’s modulus, Poisson’s ratio, shear modulus, etc. The TEMPERATURE EFFECTS and ORTHO TEMP options allow for input of temperature dependency of these material constants. Material constants for a typical layer are as follows:

Main Index

ti

thickness of the ith layer

Young’s moduli

E x x, E y y, E z z

Poisson’s ratios

v x y, v y z, v z x

Shear moduli

G x y, G y z, G z x

ρ

density

α x x, α y y

coefficients of thermal expansion

σy

yield stress

Mat

material identifier associated with temperature-dependent properties and workhardening data

350 Marc Volume A: Theory and User Information

The ANELAS, HOOKLW, ANEXP, and ANPLAS user subroutines can be used for the anisotropic behavior of elastic constants, coefficient of thermal expansion, and yield condition. In models where there is ply drop-off, it is possible to specify a user ply layer id to simplify postprocessing. In this way, the top, middle, and bottom layers may all have the same id even if the elements have a different number of layers. There are eight given classes of strain-stress relations. The class of a particular element depends on the number of direct (NDI) and shear (NSHEAR) components of stress. Table 7-1 lists the eight classes of elements. Table 7-1

Class 1

Classes of Stress-Strain Relations

NDI = 1,NSHEAR = 0 Beam Elements 5, 8, 13, 16, 23, 46, 47, 48, 52, 64, 77, 79 and Rebar Elements { ε } = [ 1 ⁄ Ex x }{ σ }

Class 2

NDI = 2,NSHEAR = 0 Axisymmetric Shells 15 and 17 ⎧ εx x ⎫ ⎨ ⎬ = ⎩ εy y ⎭

1 ⁄ Ex x –νx y ⁄ Ex x

–νy x ⁄ Ey y ⎧ σx x ⎫ ⎨ ⎬ 1. ⁄ E y y ⎩ σ y y ⎭

νy x = νx y Ey y ⁄ Ex x Class 3

NDI = 1,NSHEAR = 1 Beam Elements 14, 45, 76, 78 ⎧ε ⎫ ⎨ ⎬ = ⎩γ ⎭

Class 4

1 ⁄ Ex x

0

0

1 ⁄ Gx y

⎧σ ⎫ ⎨ ⎬ ⎩τ ⎭

NDI = 2,NSHEAR = 1 Plane Stress, Plates and Thin Shells 49 and 72 ⎧ εx x ⎪ ⎨ εy y ⎪ ⎩ γx y

⎫ ⎪ ⎬ = ⎪ ⎭

1 ⁄ Ex x

–νy x ⁄ Ey y

0

–ν x y ⁄ Ex x

1 ⁄ Ey y

0

0

0

1 ⁄ Gx y

νy x = νx y ( Ey y ⁄ Ex x )

Main Index

⎧ σx x ⎫ ⎪ ⎪ ⎨ σy y ⎬ ⎪ ⎪ ⎩ τx y ⎭

CHAPTER 7 351 Material Library

Table 7-1

Class 5

Classes of Stress-Strain Relations (continued)

NDI = 2,NSHEAR = 1 Thick Axisymmetric Shells 1 and 89 ⎧ εm m ⎫ ⎪ ⎪ ⎨ εθ θ ⎬ = ⎪ ⎪ ⎩ γT ⎭

Class 6

1 ⁄ Em m

–νθ m ⁄ Eθ θ

0

–νm θ ⁄ Em m

1 ⁄ Eθ θ

0

0

0

1 ⁄ Gm θ

⎧ σm m ⎫ ⎪ ⎪ ⎨ σθ θ ⎬ ⎪ ⎪ ⎩ τT ⎭

NDI = 3,NSHEAR = 1 Plane Strain, Axisymmetric with No Twist, Elements 151-154. ⎧ εx x ⎫ ⎪ ⎪ ⎪ εy y ⎪ ⎨ ⎬ = ⎪ εz z ⎪ ⎪ ⎪ ⎩ γx y ⎭

1 ⁄ Ex x –νx y ⁄ Ex x

1 ⁄ Ey y

0

0

–νz y ⁄ Ez z

0

1 ⁄ Ez z

0

0

1 ⁄ Gx y

–νx z ⁄ Ex x –νy z ⁄ Ey y

νy x = νx y Ey y ⁄ Ex x Class 7

–νy x ⁄ Ey y –νz x ⁄ Ez z

0

⎧ σx x ⎫ ⎪ ⎪ ⎪ σy y ⎪ ⎨ ⎬ ⎪ σz z ⎪ ⎪ ⎪ ⎩ τx y ⎭

νx z = νz x Ex x ⁄ Ez z

νz y = νy z Ez z ⁄ Ey y

NDI = 2,NSHEAR = 3 Thick Shell, Elements 22, 75, and 140 ⎧ εx x ⎫ ⎪ ⎪ ⎪ εy y ⎪ ⎪ ⎪ ⎨ γx y ⎬ = ⎪ ⎪ ⎪ γy z ⎪ ⎪ ⎪ ⎩ γz x ⎭

1 ⁄ Ex x

–νy x ⁄ Ey y

0

0

0

–νx y ⁄ Ex x

1 ⁄ Ey y

0

0

0

0

0

1 ⁄ Gx y

0

0

0

0

0

1 ⁄ Gyz

0

0

0

0

0

1 ⁄ Gz x

⎧ σx x ⎫ ⎪ ⎪ ⎪ σy y ⎪ ⎪ ⎪ ⎨ τx y ⎬ ⎪ ⎪ ⎪ τy z ⎪ ⎪ ⎪ ⎩ τz x ⎭

νy x = νx y Ey y ⁄ Ex x Class 8

NDI = 3,NSHEAR = 3 Three-Dimensional Brick Elements, Elements 149, 150 ⎧ εx x ⎫ ⎪ε ⎪ ⎪ yy ⎪ ⎪ ⎪ ⎪ εz z ⎪ ⎨ ⎬ = ⎪ γx y ⎪ ⎪ ⎪ ⎪ γy z ⎪ ⎪ ⎪ ⎩ γz x ⎭

Main Index

1 ⁄ Ex x –νx y ⁄ Ex x

–νy x ⁄ Ey y –νz x ⁄ Ez z 1 ⁄ Ey y

–νx z ⁄ Ex x –νy z ⁄ Ey y

0

0

0

–νz y ⁄ Ez z

0

0

0

1. ⁄ E z z

0

0

0

0

0

0

1 ⁄ Gx y

0

0

0

0

0

0

1 ⁄ Gyz

0

0

0

0

0

0

1 ⁄ Gz x

⎧ σx x ⎫ ⎪σ ⎪ ⎪ yy ⎪ ⎪ ⎪ ⎪ σz z ⎪ ⎨ ⎬ ⎪ τx y ⎪ ⎪ ⎪ ⎪ τy z ⎪ ⎪ ⎪ ⎩ τz x ⎭

352 Marc Volume A: Theory and User Information

Classical Lamination Theory for Multi-Layered Shells Basic CLT Theory The stress tensor at a point inside a shell element is defined as σ = G ( ε – zχ )

(7-9)

where G is the tangent matrix connecting stress and strain tensors; z is the coordinate of the point in the thickness direction; ε is the strain tensor on the middle surface of the shell and χ is the tensor of curvature. The membrane forces is given by f =

∫ σ dz

(7-10)

The bending moments is given by m =

∫ ( – z )σ dz

(7-11)

Substituting Equations (7-9) into Equations (7-10) and (7-11) and use the definitions hG 1 =

∫ G dz ∫ ( – z )G dz

h 2 G4 = IG 2 =

∫ z 2 G dz

(7-12) (7-13) (7-14)

we obtain ⎧ f ⎫ ⎨ ⎬ = ⎩ m ⎭

hG 1 h 2 G 4 ⎧ ε ⎫ ⎨ ⎬ h 2 G 4 IG 2 ⎩ χ ⎭

(7-15)

In Equations (7-12) though (7-15), h is the shell thickness and I = h 3 ⁄ 12 . In the case where the composite material remains linear elastic, it is possible to choose alternative computational procedures to improve computational time. This maybe activated using either the SHELL SECT parameter or the COMPOSITE option. The first procedure is for linear elastic composite materials where no temperature dependent materials are present and thermal strains occur. This substantially reduces the computational time and the memory requirements. The second procedure is for linear elastic composite material, but either temperature dependent materials or thermal strains are present. This substantially reduces the computational time. Progressive composite failure cannot occur with either of these models.

Main Index

CHAPTER 7 353 Material Library

PSHELL Option PSHELL option is based on the classical lamination theory (also known as equivalent stiffness method). This option allows you to define the membrane, bending, transverse shear, and coupling properties of the shell elements independently.

Shell made of homogeneous materials can be modeled with the PSHELL option by simply using the same material properties for stiffness calculation of membrane, bending, and transverse shear deformations, and using nothing for the coupling part if there is no offset of the 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 nonlinear material behavior. Shell structures with layered composite materials can be solved using a full integration technique or the PSHELL option. The full layer integration technique is very general. It can simulate material behavior

ranging from a simple linear material to a very complex material with nonlinearity and failure mechanism. The use of the PSHELL option is limited to linear-elastic behavior. By use of this option, composite layers are converted into one layer with equivalent stiffness behaviors. This way, only one integration point is needed across the thickness which makes PSHELL very useful for shell structures with layered composite materials. It is particularly attractive when the number of composite layers is large, because analysis of these smeared shell structures uses less computer time and storage space. The smeared material matrices G 1 , G 2 , and G 4 are defined in Equations (7-12), (7-13), and (7-14) representing membrane, bending and coupling stiffness, respectively. G 1 in Marc contains both membrane and transverse shear parts. Unless you want to adjust transverse shear stiffness, there is no need to define new types of materials. Generally G 1 , G 2 , and G 4 can be described by the ANISOTROPIC option.

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 non-isotropic materials (orthotropic, anisotropic, nlelast, or composite materials). With the ORIENTATION option, you specify the orientation of the material axes of symmetry (relationship between the element coordinate system and the global coordinate system, or the 0o 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. as specified by the ORIENT user subroutine. This is accomplished by the specification of an orientation type, an orientation angle, or one or two user-defined vectors, or 5. by referencing a coordinate system defined by the COORD SYSTEM option.

Main Index

354 Marc Volume A: Theory and User Information

For the first option (EDGE I-J orientation type), the intersecting plane is defined by the surface normal vector and a vector parallel to the vector pointing from element node I to element node J. The intersection of this plane with the surface tangent plane defines the 0o orientation axis. (See Figure 7-4.) The orientation angle is measured in the tangent plane positive about the surface normal. n = Normal to Surface Tangent Plane Node I Vector Parallel to Edge I-J Projected onto Surface Tangent Plane Integration Point Ω Node J

α

00 Ply Angle Direction 1 of preferred coordinate system (fiber direction in the ply)

Element Surface

Z

Y

α = Ply angle (if COMPOSITE)

X Figure 7-4

Ω = Orientation Angle (Positive Right-hand Rotation About n)

Edge I-J Orientation Type

For the second option (global plane orientation type), the intersecting plane is the chosen global coordinate plane. The intersection of this plane with the surface tangent plane defines the 0o orientation axis. (See Figure 7-5.) The third option (user-defined plane orientation type) makes use of one or two user-defined vectors to define the intersecting plane. Using a single vector, the intersecting plane is that plane which contains the user vector and the chosen coordinate axis. Using two user vectors, the intersecting plane is that plane which contains both of them. (See Figure 7-6.) Orientation type 3-D ANISO also makes use of two user-defined vectors, but in this case, the first vector defines the first (1) principal direction and the second vector defines the second (2) principal direction. (See Figure 7-7.) In the fourth option, the ORIENT user subroutine must be used for the definition of the orientation of the material axis of symmetry. In the fifth option, if continuum elements are used, the material orientation will be as defined by the COORD SYSTEM option. If shell elements are used, the local x-axis is projected on the shell as shown in Figure 7-8.

Main Index

CHAPTER 7 355 Material Library

n - Normal to Surface Tangent Plane Global ZX Plane

Surface Tangent Plane

α Direction 1 of preferred coordinate system

ce

Ω

El em

en

tS ur fa

In pr ters efe ec rre tion dp o Z lan f e Y

α = Ply angle (if COMPOSITE)

X

Figure 7-5

Ω = Orientation Angle (Positive Right-hand Rotation About n)

Global ZX Plane Orientation Type n = Normal to Surface Tangent Plane Tangent Plane u = user-defined vector

Surface Tangent Plane Ω global X

Intersection of Two Planes

Y

Figure 7-6

Main Index

Direction 1 of Preferred Coordinate System

Element Surface

Z

X

α

Ω = Orientation Angle (Positive Right-hand Rotation About n) α = Ply angle (if COMPOSITE) User Defined XU Plane Orientation Type

356 Marc Volume A: Theory and User Information

U2 = User Vector 2

U3 = U1 x U2

U1 = User Vector 1

Z

U1 = Direction 1 of Preferred Coordinate System

Y

U2 = Direction 2 of Preferred Coordinate System X Figure 7-7

3-D ANISO Orientation Type x MCID Coordinate System

z G2 y

G3 ymaterial

xmaterial

G4

G1 Figure 7-8

COORD SYSTEM when Shell Elements are used

Post codes 691 and 694 can be used to obtain the first and second orientation vectors of the material coordinate system. It should be noted that these vectors are element based quantities and only account for the zero degree ply orientation. For specific layer orientations, these vectors are further modified by the layer angle given through post code 697. Marc Mentat can be used to plot both the element orientations (zero degree ply angle) and the layer orientations. These postprocessing features can be used to verify if the initial orientations are setup correctly (especially for the ORIENT user subroutine or the COORD SYSTEM option) and to evaluate the evolution of the orientation vectors as the structure deforms. More details on these orientation vectors are given under the POST option in Marc Volume C: Program Input.

Main Index

CHAPTER 7 357 Material Library

Material Dependent Failure Criteria Calculations of user specified failure criteria on a layer by layer basis are available in Marc. The available criteria are: maximum stress (MX STRESS), maximum strain (MX STRAIN), TSAI-WU, HOFFMAN, HILL, HASHIN, HASHIN FABRIC, HASHIN TAPE, PUCK, and the UFAIL user subroutine. During each analysis, up to three failure criteria can be selected; failure indices and strength ratios are calculated and printed for every integration point. The FAIL DATA model definition option is used for the input of failure criteria data. When the table driven input format is used, the failure material parameters may reference a table to introduce temperature dependent behavior. A simple description of these failure criteria is given below: 1. Maximum Stress Criterion At each integration point, Marc calculates six failure indices FI and six strength ratios SR: The six failure indices are given by: ⎛ σ 1⎞ ⎜ -------⎟ ⎝ X t⎠

if

σ1 > 0

1.

2.

(7-16)

⎛ σ 1⎞ ⎜ – -------⎟ ⎝ X c⎠

if

σ1 < 0

⎛ σ 2⎞ ⎜ ------⎟ ⎝ Yt⎠

if

σ2 > 0 (7-17)

⎛ σ 2⎞ ⎜ – ------⎟ ⎝ Y c⎠

if

σ2 < 0

σ ⎛ -----3-⎞ ⎝ Zt ⎠

if

σ3 > 0 (7-18)

3. σ ⎛ – -----3-⎞ ⎝ Z c⎠

Main Index

if

σ3 < 0

4.

⎛ σ1 2 ⎞ ⎝ -------S 12 ⎠

(7-19)

5.

⎛ σ 23 ⎞ ⎝ ------S 23 ⎠

(7-20)

358 Marc Volume A: Theory and User Information

6.

⎛ σ 31 ⎞ ⎝ ------S 31 ⎠

(7-21)

where X t, X c

are the maximum allowable stresses in the 1-direction in tension and compression.

Y t, Y c

are maximum allowable stresses in the 2-direction in tension and compression.

Z t, Z c

are maximum allowed stresses in the 3-direction in tension and compression.

S 12

maximum allowable in-plane shear stress.

S 23

maximum allowable 23 shear stress.

S 31

maximum allowable 31 shear stress.

For the Maximum Stress Failure Criterion, the strength ratios SR are the reciprocals of the corresponding failure indices FI. 1.0 SR = --------FI For example, the sixth strength ratio for the Maximum Stress Failure Criterion is ( S 31 ⁄ σ 31 ) . Note that if the maximum allowable stresses are not defined or if the actual stresses are 0, then the strength ratio is set to 100. 2. Maximum Strain Failure Criterion At each integration point, Marc calculates six failure indices and six strength ratios. The six failure indices are given by: ε1 ⎛ -----⎞ ⎝ e 1-t⎠

if

ε1 > 0

1.

(7-22)

ε1 ⎛ – ------⎞ ⎝ e 1 c⎠

if

ε1 < 0

ε2 ⎛ -----⎞ ⎝ e 2-t⎠

if

ε2 > 0 (7-23)

2. ε2 ⎛ – ------⎞ ⎝ e 2 c⎠

Main Index

if

ε2 < 0

CHAPTER 7 359 Material Library

ε3 ⎛ ------⎞ ⎝ e 3 t⎠

if

ε3 > 0 (7-24)

3. ε3 ⎛ – ------⎞ ⎝ e 3 c⎠

if

ε3 < 0

4.

⎛ γ 12 ⎞ ⎝ ------g 12 ⎠

(7-25)

5.

⎛ γ2 3 ⎞ ⎝ ------g 23 ⎠

(7-26)

6.

⎛ γ 31 ⎞ ⎝ ------g 31 ⎠

(7-27)

where e 1 t, e 1 c

are the maximum allowable strains in the 1 direction in tension and compression.

e 2 t, e 2 c

are the maximum allowable strains in the 2 direction in tension and compression.

e 3 t, e 3 c

are the maximum allowable strains in the 3 direction in tension and compression.

g 12

is the maximum allowable shear strain in the 12 plane.

g 23

is the maximum allowable shear strain in the 23 plane.

g 31

is the maximum allowable shear strain in the 31 plane.

For the Maximum Strain Failure Criterion, the strength ratios at the integration points are the reciprocals of the corresponding failure indices. 1.0 SR = --------FI For example, the sixth strength ratio for the Maximum Strain Failure Criterion is ( g 31 ⁄ γ 31 ) . Note that if the maximum allowable strains are not defined or if the actual strains are 0, then the strength ratio is set to 100. 3. Hill Failure Criterion Assumptions: a. Orthotropic materials only b. Incompressibility during plastic deformation c. Tensile and compressive behavior are identical

Main Index

360 Marc Volume A: Theory and User Information

At each integration point, Marc calculates the failure index FI as follows: σ 12 σ 22 σ 32 1 1 1 1 1 1 ------2- + ------2- + -----2- – ⎛⎝ ------2- + ------2- – -----2-⎞⎠ σ 1 σ 2 – ⎛⎝ ------2- + -----2- – ------2-⎞⎠ σ 1 σ 3 X Y Z X Y Z Z Y X 2 2 2 σ 12 σ 13 σ 23 1 1 1 – ⎛ ------- + ------ – -------⎞ σ 2 σ 3 + --------- + --------- + --------2 2 2 2 2⎠ ⎝ 2 S 12 S 13 S 23 Z X Y

(7-28)

For plane stress condition, it becomes 2

2

2

⎛ σ 1 σ 1 σ 2 σ 2 σ 12 ⎞ - + ------2- + --------⎟ ⎜ ------2- – -----------2 X2 Y S 12 ⎝X ⎠

(7-29)

where X

is the maximum allowable stress in the 1 direction

Y

is the maximum allowable stress in the 2 direction

Z

is the maximum allowable stress in the 3 direction

S 12, S 23, S 31

are as before

F

failure index scale factor

For the Hill Criterion, the strength ratio at each integration point is given by: 1.0 SR = ---------FI Note that if the failure index is 0 (either because no allowable stresses are prescribed or because actual stresses are 0), the strength ratio is set to 100. 4. Hoffman Failure Criterion Note:

Hoffman criterion is essentially Hill criterion modified to allow unequal maximum allowable stresses in tension and compression.

At each integration point, Marc the failure index FI calculates: 2

2

2

[ C1 ( σ 2 – σ3 ) + C2 ( σ3 – σ 1 ) + C3 ( σ1 – σ 2 ) + C4 σ1 + C5 σ 2 2 + C σ2 + C σ2 ] + C 6 σ 3 + C 7 σ 23 8 13 9 12

with

Main Index

(7-30)

CHAPTER 7 361 Material Library

1 1 1 1 C 1 = --- ⎛ ----------- + ------------- – -------------⎞ 2 ⎝ Z t Z c Y t Y c X t X c⎠ 1 1 1 1 C 2 = --- ⎛ ------------- + ----------- – -------------⎞ 2 ⎝ X t X c Z t Z c Y t Y c⎠ 1 1 1 1 C 3 = --- ⎛⎝ ------------- + ------------- – -----------⎞⎠ 2 Xt Xc Yt Yc Zt Zc 1 1 C 4 = ----- – -----Xt Xc 1 1 C 5 = ----- – -----Yt Yc C6

(7-31)

1 1 = ----- – -----Zt Zc

1 C 7 = -------2 S 23 1 C 8 = -------2 S 13 1 C 9 = -------2 S 12 For plane stress condition, it becomes 2

2

2

σ2 σ 12 σ 1 σ 2 ⎫ σ1 ⎧⎛ 1 1 1 1 – ------⎞ σ 1 + ⎛ ----- – ------⎞ σ 2 + ------------- + ------------- + --------- – ------------- ⎬ ⎨ ⎝ ----⎠ ⎝ ⎠ 2 X Y X Y X X Y Y Xt Xc ⎭ S 12 c t c t c t c ⎩ t

(7-32)

where: X t, X c, Y t, Y c, Z t, Z c, S 12, S 23, S 31, F are as before.

Note:

σ1

For small ratios of, for example, ------ , the Hoffman criterion can become negative due Xt

to the presence of the linear terms.

For the Hoffman Failure Criterion, the strength ratio SR is obtained by taking the smaller of the absolute values of the two roots obtained by solving the quadratic equation: A ( SR ) 2 + B ( SR ) + C = 0

Main Index

362 Marc Volume A: Theory and User Information

where for the general 3-D case: 2 2 2 σ 22 σ 32 τ 12 τ 23 τ 13 σ 12 ------------- + ------------- + ----------- + ------+ ------+ -------+ 2F 12 σ 1 σ 2 + 2F 23 σ 2 σ 3 + 2F 13 σ 1 σ 3 2 2 Xt Xc Yt Yc Zt Zc S 2 , S 23 S 13 12 A = --------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------F

1 1 1 1 1 1 ⎛ ----– -⎞ σ 1 + ⎛ ----- – ------⎞ σ 2 + ⎛ ----- – ------⎞ σ 3 ⎝ X t ----⎝ Y t Y c⎠ ⎝ Z t Z c⎠ , and C = – 1.0 . X c⎠ B = --------------------------------------------------------------------------------------------------------------F Note that if the allowable stresses are not defined or if the actual stresses are 0, then the strength ratio is set to 100. 5. Tsai-Wu Failure Criterion Tsai-Wu is a tensor polynomial failure criterion. At each integration point, Marc calculates the failure index F1 as follows: σ 12 σ 22 σ 32 1 1 1 1 1 1 ⎛ ----– ------⎞ σ 1 + ⎛ ----- – ------⎞ σ 2 + ⎛ ----- – ------⎞ σ 3 + ------------- + ------------- + ----------⎝ X t X c⎠ ⎝ Y t Y c⎠ ⎝ Z t Z c⎠ Xt Xc Yt Yc Zt Zc 2 2 2 τ 12 τ 23 τ 13 + -------- + -------- + -------- + 2F 12 σ 1 σ 2 + 2F 23 σ 2 σ 3 + 2F 13 σ 1 σ 3 ] 2 2 2 S 12 S 23 S 13

(7-33)

where X t, X c, Y t, Y c, Z t, Z c, S 12, S 23, S 31, F are as before. F 12

Interactive strength constant for the 12 plane

F 23

Interactive strength constant for the 23 plane

F 13

Interactive strength constant for the 31 plane

For plane stress condition, it becomes 2

2

2

σ1 σ2 σ1 2 ⎧⎛ 1 ⎫ 1 1 1 ----- – ------⎞⎠ σ 1 + ⎛⎝ ------- – ------⎞⎠ σ 2 + ------------- + ------------- + --------- + 2F 12 σ 1 σ 2 ⎬ ⎨⎝X X Y Y X X Y Y S c 2 c t c t c 12 ⎩ t ⎭ Note:

(7-34)

In order for the Tsai-Wu failure surface to be closed, 1 1 2 < -----------F 12 - • ------------Xt Xc Yt Yc

1 1 1 1 2 < -----------2 < -----------F 23 - • ----------- F 31 - • ----------Yt Yc Zt Zc Xt Xc Zt Zc

See Wu, R.Y. and Stachurski, 2, “Evaluation of the Normal Stress Interaction Parameter in the Tensor Polynomial Strength Theory for Anisotropic Materials”, Journal of Composite Materials, Vol. 18, Sept. 1984, pp. 456-463.

Main Index

CHAPTER 7 363 Material Library

For the Tsai-Wu failure criterion, the strength ratio SR is obtained by taking the smaller of the absolute values of the two roots obtained by solving the quadratic equation: A ( SR ) 2 + B ( SR ) + C = 0 where for the general 3-D case: 2 2 2 σ 22 σ 32 τ 12 τ 23 τ 13 σ 12 + + + 2F 12 σ 1 σ 2 + 2F 23 σ 2 σ 3 + 2F 13 σ 1 σ 3 ------------- + ------------- + ----------- + -------------------2 2 Xt Xc Yt Yc Zt Zc S 2 S S 12 23 13 A = --------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------F

1 1 1 1 1 1 ⎛ ----– -⎞ σ 1 + ⎛ ----- – ------⎞ σ 2 + ⎛ ----- – ------⎞ σ 3 ⎝ X t ----⎝ Y t Y c⎠ ⎝ Z t Z c⎠ , and C = – 1.0 . X c⎠ B = --------------------------------------------------------------------------------------------------------------F Note that if the allowable stresses are not defined or if the actual stresses are 0, then the strength ratio is set to 100. 6. User-defined Failure Criteria Using the UFAIL user subroutine, you can evaluate your own failure criterion as a function of stresses and strains at each integration point. Two quantities can be returned by the routine: A user-defined failure index A user-defined strength ratio. 7. Hashin Failure Criterion The Hashin failure criterion distinguishes between fiber failure and matrix failure. At each integration point, Marc calculates the failure index FI for each mode as follows: Tension fiber mode, σ 11 2 1 ⎛ ------⎞ + ----2 ) = 1 or σ - ( σ 2 + σ 13 11 = X T ⎝ X t-⎠ S 2 12

(7-35)

Compressive fiber mode, σ 1 < 0 σ 11 ------------ = X c Xc

(7-36)

Tensile matrix mode, σ 2 + σ 3 > 0 1 1 1 2 – σ σ ) + ------2 ) ----- ( σ 2 + σ 3 ) 2 + -------- ( σ 23 - ( σ 2 + σ 13 2 3 2 Yt S 12 12 S 23 Compressive matrix mode, σ 2 + σ 3 < 0

Main Index

(7-37)

364 Marc Volume A: Theory and User Information

Yc 2 1 1 1 2 – σ σ ) ------ ⎛ ⎛ -----------⎞ – 1⎞ ( σ 2 + σ 3 ) + ------------ ( σ 2 + σ 3 ) 2 + -------- ( σ 23 2 3 ⎝ ⎝ ⎠ 2 2 Y c 2S 23⎠ S 23 4S 23

(7-38)

1 2 + σ2 ) + -------- ( σ 12 13 2 S 12 For the Hashin failure criterion, the strength ratio SR for each mode is calculated as follows: 1.0 Tension fiber mode: SR = ---------- where FI is the failure index for the tension fiber mode FI 1.0 Compressive fiber mode: SR = --------- where FI is the failure index for the compressive FI fiber mode 1.0 Tensile matrix mode: SR = ---------- where FI is the failure index for the tensile matrix mode FI Compressive matrix mode: A ( SR ) 2 + B ( SR ) + C = 0 where 1 1 1 2 2 2 A = ----------( σ 23 – σ 2 σ 3 ) + ------+ σ 13 ) - ( σ 2 + σ 3 ) 2 + -------- ( σ 12 2 2 2 4S 23 S 23 S 12 Yc 2 1 B = ------ ⎛ ⎛ -----------⎞ – 1⎞ ( σ 2 + σ 3 ) , and C = – 1.0 . ⎠ Y c ⎝ ⎝ 2S 23⎠ Note that if the allowable stresses are not defined or if the actual stresses are 0, then the strength ratio is set to 100. A sixth failure index is available for postprocessing. It is the maximum of the first five failure criteria. Similarly, the minimum strength ratio is available as the seventh strength ratio. 8. Hashin Fabric Failure Criterion The Hashin Fabric failure criterion is a variant of the Hashin criterion adapted for fabric type materials. The 1 direction is the first fiber direction, the 2 direction is the second fiber direction, and the 3 direction is through the thickness direction. At each integration point, Marc calculates the failure indices as follows: Tensile fiber 1 mode, σ 1 > 0 σ1 2 2 σ 13 2 σ 2 ⎛ -----1-⎞ + ⎛ -------⎞ + ⎛ ------⎞ ⎝ X t⎠ ⎝ S 12 ⎠ ⎝ S 13-⎠

(7-39)

Compressive fiber 1 mode, σ 1 < 0 σ 2 σ1 2 2 σ 13 2 ⎛ -----1-⎞ + ⎛ -------⎞ + ⎛ ------⎞ ⎝ X c⎠ ⎝ S 12-⎠ ⎝ S 13-⎠

Main Index

(7-40)

CHAPTER 7 365 Material Library

Tensile fiber 2 mode, σ 2 > 0 σ 2 σ1 2 2 σ 13 2 ⎛ -----2-⎞ + ⎛ --------⎞ + ⎛ --------⎞ ⎝ Y t⎠ ⎝ S 12 ⎠ ⎝ S 13⎠

(7-41)

Compressive fiber 2 mode, σ 2 < 0 σ1 2 2 σ 13 2 σ 2 ⎛ -----2-⎞ + ⎛ -------⎞ + ⎛ ------⎞ ⎝ Y c⎠ ⎝ S 12 ⎠ ⎝ S 23-⎠

(7-42)

Tensile matrix mode, σ 3 > 0 σ1 2 2 σ 13 2 σ 23 2 σ 2 ⎛ -----3-⎞ + ⎛ -------⎞ + ⎛ ------⎞ + ⎛ ------⎞ ⎝ Zt ⎠ ⎝ S 12 ⎠ ⎝ S 13⎠ ⎝ S 23-⎠

(7-43)

Compressive matrix mode, σ 3 < 0 σ 2 σ1 2 2 σ 13 2 σ 23 2 ⎛ -----3-⎞ + ⎛ -------⎞ + ⎛ ------⎞ + ⎛ ------⎞ ⎝ Z c⎠ ⎝ S 12 ⎠ ⎝ S 13⎠ ⎝ S 23-⎠

(7-44)

where: X t, X c, Y t, Y c, Z t, Z c, S 12, S 23, S 13 are as before. For the Hashin Fabric Failure Criterion, the strength ratio SR for each of the six modes is 1.0 calculated as: SR = --------FI where FI is the failure index for the corresponding mode. Note that if the maximum allowable stresses are not defined or if the actual stresses are 0, then the associated strength ratios are set to 100. 9. Hashin Tape Failure Criterion The Hashin Tape failure criterion is a variant of the Hashin criterion adapted for tape type of materials. The 1 direction is in the tape fiber direction, the 2 direction is perpendicular to the fiber direction in the plane of the tape, and the 3 direction is through the thickness direction. At each integration point, Marc calculates the failure indices as follows: Tensile fiber mode, σ 1 > 0 σ 2 σ1 2 2 σ 13 2 ⎛ -----1-⎞ + ⎛ --------⎞ + ⎛ --------⎞ ⎝ X t⎠ ⎝ S 12 ⎠ ⎝ S 13⎠

(7-45)

Compressive fiber mode, σ 1 < 0 σ1 2 2 σ 13 2 σ 2 ⎛ -----1-⎞ + ⎛ -------⎞ + ⎛ ------⎞ ⎝ X c⎠ ⎝ S 12 ⎠ ⎝ S 13-⎠

Main Index

(7-46)

366 Marc Volume A: Theory and User Information

Tensile matrix mode, σ 2 + σ 3 > 0 σ 13 2 σ 23 2 σ 2 + σ 3 2 σ 22 σ 33 σ1 2 2 ⎛ ------------------⎞ – ----------------- + ⎛ -------⎞ + ⎛ ------⎞ + ⎛ ------⎞ ⎝ Yt ⎠ ⎝ S 12 ⎠ ⎝ S 13⎠ ⎝ S 23-⎠ 2 S 23

(7-47)

Compressive matrix mode, σ 2 + σ 3 < 0 Yc 2 σ1 2 2 σ 13 2 σ 23 2 σ 2 σ2 + σ3 σ2 + σ3 2 σ2 σ3 ⎛ ⎛ ----------⎞ – 1⎞ ⎛ ------------------⎞ + ⎛ ------------------⎞ – ------------- + ⎛ -------⎞ + ⎛ ------⎞ + ⎛ ------⎞ + A ⎛ -----1-⎞ 1 ⎝ ⎝ 2S 23⎠ ⎠ ⎝ Y c ⎠ ⎝ 2S 23 ⎠ ⎝ S 12 ⎠ ⎝ S 13⎠ ⎝ S 23⎠ ⎝ S 1⎠ 2 S 23 (7-48) where: X t, X c, Y t, Y c, S 12, S 23, S 13 are as before. A 1 is equal to zero or one and is used to determine if the last term should be used. S 1 is the maximum fiber stress for matrix compression. For the Hashin Tape Failure Criterion, the strength ratio SR for the first three modes is calculated 1.0 as SR = ---------- where FI is the failure index for the corresponding mode. FI For the compressive matrix mode, the strength ratio is calculated as follows: A ( SR ) 2 + B ( SR ) + C = 0 where σ 12 2 σ2 + σ3 2 σ2 σ3 σ 13 2 σ 23 2 σ1 2 A = ⎛ -------------------⎞ – -----------= ⎛ --------⎞ + ⎛ --------⎞ + ⎛ --------⎞ + A 1 ⎛ ------⎞ , 2 ⎝ 2S 23 ⎠ ⎝ S 12⎠ ⎝ S 13⎠ ⎝ S 23⎠ ⎝ S 1⎠ S 23 Yc 2 1 B = ------ ⎛ ⎛ -----------⎞ – 1⎞ ( σ 2 + σ 3 ) , and C = – 1.0 . ⎠ Y c ⎝ ⎝ 2S 23⎠ Note that if the maximum allowable stresses are not defined or if the actual stresses are 0, then the associated strength ratios are set to 100. 10. Puck Failure Criterion The Puck failure criterion distinguishes just as Hashin between fiber failure and matrix failure. The main difference is in the matrix failure where the concept of a fracture failure angle is used. This angle is the angle at which the fracture due to matrix failure will occur. See Figure 7-9 for the definition on how it is defined with respect to the preferred coordinates system. Figure 7-9 Definition of the Fracture Failure Angle θ fp

Main Index

CHAPTER 7 367 Material Library

θfp

3

t

n

2 1

The Puck failure criterion uses the following input parameters as defined above: X t, X c, Y t, Y c, S 12 . In addition, four parameters are used for describing the slopes of the failure (–) , and p (+) envelope: p 12 c = p ⊥(–)|| , p 12 t = p ⊥(+)|| , p 23 c = p ⊥⊥ 23 t = p ⊥⊥ . The notation

p 12 c etc. is used in Marc Volume C: Program Input and in the Marc output while the other notation is from Puck [Ref. 25]. The following parameters are calculated from the input parameters and used in the following S 12 ⎛ Yc Yc ⎞ R A = ----------------------------- = -------------- ⎜ 1 + 2p 12 c -------- – 1⎟ 2 ( 1 + p 23 c ) 2p 12 c ⎝ S 12 ⎠

(7-49)

σ 21 c = S 12 1 + 2p 23 c

(7-50)

The first two failure indices are given by Tensile fiber mode, σ 1 > 0 σ1 -----Xt

(7-51)

Compressive fiber mode, σ 1 < 0 σ1 --------Xc

(7-52)

The fracture failure angle θ fp can be calculated analytically for the plane stress case provided that the following relation between two of the failure envelope slopes is enforced: RA p 23 c = p 12 c -------S 12

(7-53)

It is recommended that either p 12 c or p 23 c is specified in the input. The other is by default calculated using Equations (7-49) and (7-53). This default setting is also used for other cases than plane stress although then this relationship is not necessary.

Main Index

368 Marc Volume A: Theory and User Information

For the plane stress case, we have three failure indices, denoted modes A, B, and C: Mode A, σ 2 > 0 , θ fp = 0 σ 12 2 Y 2 σ 2 σ2 ⎛ ------⎞ + ⎛ 1 – p -------t-⎞ ⎛ -----2-⎞ + p ------12 t S ⎠ ⎝ Y ⎠ 12 t S ⎝ S 12⎠ ⎝ 12 t 12

(7-54)

σ RA Mode B, σ 2 < 0 and 0 ≤ -------2- ≤ ----------- , θ fp = 0 σ 21 c σ 12 1 2 + (p 2 -------- ( σ 12 12 c σ 2 ) + p 12 c σ 2 ) S 12

(7-55)

σ 21 c σ1 2 Mode C, σ 2 < 0 and 0 ≤ --------. - ≤ ---------RA σ2 2 σ 12 σ 2 Yc ⎛ ⎛ ------------------------------------⎞ + ⎛ -----2-⎞ ⎞ --------⎝ ⎝ 2 ( 1 + p 23c S 12 )⎠ ⎝ Y c⎠ ⎠ σ 2

(7-56)

For this plane stress case, the fracture failure angle is calculated from the following formula 2

cos2 θ

fp

⎛ σ 12 2 ⎛ R A ⎞ ⎞ 1 = ----------------------------- ⎜ ⎛ --------⎞ ⎜ --------⎟ + 1⎟ ⎝ ⎠ 2 ( 1 + p 23 c ) ⎝ σ 2 ⎝ S 12⎠ ⎠

(7-57)

It is available as the sixth failure index but only for postprocessing. For other than plane stress, the failure angle is not determined analytically. Instead, a numerical procedure is used as outlined below. The stresses in a failure plane defined by 1, n and t directions in Figure 7-9 are σ n = σ 2 cos2 θ + σ 3 sin2 θ + 2σ 23 sin θ cos θ

(7-58)

σ n t = ( σ 3 – σ 2 ) sin θ cos θ + σ 23 ( cos2 θ – sin2 θ )

(7-59)

σ n 1 = σ 31 sin θ + σ 12 cos θ

(7-60)

The failure index as a function of θ is now formulated as follows, σ n ≥ 0 : f( θ) =

σn t 2 σn 1 2 2 1 ⎛ ----– p 1⎞ σ n2 + ⎛ --------⎞ + ⎛ ---------⎞ + p 1 σ n ⎝ Yt ⎠ ⎝ R A⎠ ⎝ S 12 ⎠

and for σ n < 0

Main Index

(7-61)

CHAPTER 7 369 Material Library

f(θ ) =

σn 1 2 σn t 2 ⎛ ------⎞ + ⎛ -------⎞ + ( p σ )2 + p σ 2 n 2 n ⎝ R A⎠ ⎝ S 12-⎠

(7-62)

where p 23 t σ n2t p 12 t σ n21 p 1 = --------- ------------------------- + --------- ------------------------R A σ n2t + σ n21 S 12 σ n2t + σ n21

(7-63)

p 12 c σ n21 σ n2t p 23 c p 2 = ---------- ------------------------- + ---------- ------------------------S 12 σ 2 + σ 2 R A σ n2t + σ n21 nt n1

(7-64)

The critical failure angle θ fp and the corresponding failure index is obtained by evaluating equations (7-58) through (7-64) with a sufficient number of angles between -90 and 90 degrees. For positive normal stress, it is saved as the 3rd failure index and as the 4th failure index. The 5th failure index is not used in this case. The critical failure angle is stored as the 6th failure index for post processing just as for plane stress. For the Puck Failure Criterion, the strength ratios for each mode are the reciprocals of the 1.0 corresponding failure indices, SR = --------- . Note that if the maximum allowable stresses are not FI defined or if the actual stresses are 0, then the associated strength ratios are set to 100. A seventh failure criterion is available for postprocessing. It is the maximum of the first five failure criteria. Similarly, the minimum strength ratio is available as the seventh strength ratio.

Interlaminar Shear for Thick Shell, Beam, Solid Shell and 3D Composite Brick Elements Another addition made for composite analysis is the calculation of interlaminar shears. These interlaminar shears are printed in the local coordinate system above and below each layer selected for printing by PRINT CHOICE or PRINT ELEMENT. These values are also available for postprocessing. The TSHEAR parameter must be used for activating the parabolic shear distribution calculations. In Marc, the distribution of transverse shear strains through the thickness for thick shell and beam elements was assumed to be constant. From basic strength of materials and the equilibrium of a beam cross section, it is known that the actual distribution is more parabolic in nature. As an additional option, the formulations for elements 1, 22, 45, 75, 89, 140, 149, 150, and 185 (TSHEAR will be switched off for elements 185, 149 and 150 when the elements are stacked) have been modified to include a parabolic distribution of transverse shear strain. The formulation is exact for beam element 45, but is approximate for the other thick shell elements. Nevertheless, the approximation is expected to give improved results from the previous constant shear distribution. Furthermore, interlaminar shear stresses for composite beams and shells can now be easily calculated.

Main Index

370 Marc Volume A: Theory and User Information

The generalized stiffness matrix for the complete section excluding transverse shear terms is given by: F 11

ε 11

F 22

ε 22

M 11

X Y ⋅ ε 12 Y Z κ 11

M 22

κ 22

M 12

κ 12

F 12

=

(7-65)

where X, Y, and Z are 3 x 3 matrices F

= section forces

M = section moments ε

= strain at mid plane of section

κ

= curvature

1,2 are in-plane directions A unique X, Y direction in the plane of the section is defined by a rotation around the element normal which maximizes the value of X 11 in the above equation. We then assume that the stresses in the X and Y direction are uncoupled, this gives: ⎧ ⎪ Fx x ⎨ ⎪ Mx x ⎩

⎫ ⎪ ⎬ = ⎪ ⎭

Xx x Yx x Yx x Zx x

⎧ ⎪ ε ⋅ ⎨ xx ⎪ κx x ⎩

⎫ ⎧ ⎪ ⎪ Fy y ⎬ and ⎨ ⎪ ⎪ My y ⎭ ⎩

⎫ ⎪ ⎬ = ⎪ ⎭

Xy y Yy y Yy y Zy y

⎧ ⎪ ε ⋅ ⎨ yy ⎪ κy y ⎩

⎫ ⎪ ⎬ ⎪ ⎭

(7-66)

If we assume only bending and transverse shear in the section, all section forces are zero and inverting the above equation gives: ⎧ ⎪ εx x ⎨ ⎪ κx x ⎩

⎫ ⎪ ⎬ = ⎪ ⎭

H1 x M2 x

⎧ ⎪ ε ⋅ { M x x } and ⎨ y y ⎪ κy y ⎩

⎫ ⎪ ⎬ = ⎪ ⎭

H1 y M2 y

⋅ { My y }

(7-67)

For a point in the section, we can now define the stresses as: σ x x ( z ) = E ( z ) ⋅ ε x x ( z ) = E ( z ) ⋅ { ε x x + κ x x ⋅ z } = E ( z ) ⋅ { H 1 x + H 2 x ⋅ z }M x x

and (7-68)

σ y y ( z ) = E ( z ) ⋅ ε y y ( z ) = E ( z ) ⋅ { ε y y + κ y y ⋅ z } = E ( z ) ⋅ { H 1 y + H 2 y ⋅ z }M y y Since we assumed that all stresses in the X and Y direction are uncoupled, the equilibrium conditions through the thickness are given by:

Main Index

CHAPTER 7 371 Material Library

∂τ z x ∂σ x x ( z ) ∂τ z y ∂σ y y ( z ) ----------- + -------------------- = 0 and ----------- + -------------------- = 0 ∂x ∂y ∂z ∂z

(7-69)

where τ x x and τ y y are the transverse shear stresses. From beam theory, we have: ∂M x x ∂M y y V x + -------------- = 0 and V y + -------------- = 0 ∂x ∂y

(7-70)

where M is the bending moments and V is the shear forces. Combining the Equations (7-68), (7-69), and (7-70) gives: ∂τ z y ∂τ z x ----------- = E ( z ) ⋅ { H 1 x + H 2 x ⋅ z } ⋅ V x and ----------- = E ( z ) ⋅ { H 1 y + H 2 y ⋅ z } ⋅ V y ∂z ∂z

(7-71)

We can integrate this through the thickness giving: t⁄2

τz x ( z ) =

∫

y

E ( z ) { H 1 x + H 2 x ⋅ z }V x dz and τ z y ( z ) =

–t ⁄ 2

∫

E ( z ) { H 1 y + H 2 y ⋅ z }V y dz (7-72)

–t ⁄ 2

with the boundary conditions that the shear stresses at the top and the bottom of the shell are zero. We can now define the transverse shear stiffness by matching the shear strain energy over the section obtained with the transverse shear stresses given in (7-72). This yields the flexibility matrix S: ⎫ ⎧ Vx ⎫ 1⎧ 1 --- ⎨ V x V y ⎬[ S ] ⎨ ⎬ = --2⎩ 2 V ⎭ ⎩ y⎭

t⁄2

∫ –t ⁄ 2

⎧ ⎫ G x x ( z ) G x y ( z ) ⎧ τz x ( z ) ⎫ ⋅⎨ ⎨ τz x ( z ) τz y ( z ) ⎬ ⋅ ⎬ dz ⎩ ⎭ G y x ( z ) G y y ( z ) ⎩ τz y ( z ) ⎭

(7-73)

where G is the transverse shear flexibilities of the material through the thickness. Inversion of the flexibility matrix S gives the transverse shear stiffness of the section.

Interlaminar Stresses for Continuum Composite Elements In Marc, the interlaminar shear and normal stresses are calculated by averaging the stresses in the stacked two layers. The stresses are transformed into a component tangent to the interface and a component normal to the interface. The two components, considered as shear stress and normal stress, respectively, are printed out in the output file. By using POST code 501 or 511 (see Marc Volume C: Program Input) representing interlaminar normal and shear stresses respectively, the interlaminar normal or shear stress can be written into a post file in the form of a stress tensor defined in the global coordinate directions. Marc Mentat can be used to plot the principal directions of the stress tensor which show the magnitude and the direction of the stress, and the changes based on deformation.

Main Index

372 Marc Volume A: Theory and User Information

Progressive Composite Failure Marc supports progressive failure analysis for composites and other elastic materials. The material is assumed to be linear elastic up to the point of failure. Failure is indicated by the failure criteria described in the previous section. When failure occurs, the element stiffness is degraded. Marc offers three different methods for the material degradation as described below. This is flagged through the FAIL DATA model definition option. Failure occurs when any of the up to three different failure criteria is satisfied. The material will not heal; the damaged elements keep the degraded properties after unloading. Model 1 – Selective Gradual Degradation This model uses a selective degradation of the moduli depending on failure mode. The moduli are decreased gradually when failure occurs. Within an increment, it attempts to keep the highest failure index less than or equal to one. Whenever a failure index F larger than one occurs, stiffness reduction factors ri are calculated based upon the value of the failure indices. The incremental contribution to the total reduction factor is calculated as Δr i = – ( 1 – e 1 – F )

(7-74)

This is done differently for different failure criteria as described below. Six such reduction factors are stored and updated. They are then used for scaling the respective material modulus according to new

= r 1 E 11

new

= r 2 E 22

new

= r 3 E 33

new

= r 4 G 12

new

= r 5 G 23

new

= r 6 G 31

E 11 E 22 E 33

G 12 G 23 G 31

orig orig orig orig orig orig

The Poisson’s ratios are scaled in the same way as the corresponding shear modulus. For the maximum stress and maximum strain criteria the reduction factors are calculated separately from each separate failure index: r1 is calculated from the first failure index as given by Equation 7-16 above, r2 is calculated from the second failure index from Equation 7-17 etc. Thus, there is no coupling of the different failure modes for these criteria. For the failure criteria which only have one failure index: Tsai-Wu, Hoffman and Hill, all six reduction factors are decreased in the same way, using the smallest of the ri:s. For the criteria which distinguish between fiber and matrix failure (Hashin, Hashin-tape and Puck) there is a more complex coupling between the failure modes. There is a default behavior which can be influenced by a number of input parameters. The default is as follows.

Main Index

CHAPTER 7 373 Material Library

• r1 depends on fiber failure (first and second failure index) • r2 depends on matrix failure (third, fourth and fifth failure index) • r3 behaves the same as r1 ( r 3 = r 1 ) • r4 behaves the same as r2 ( r 4 = r 2 ) • r5 and r6 behave the same as r4 ( r 5 = r 6 = r 4 ) In the FAIL DATA option, there are five parameters available for controlling the way the moduli are reduced. With the exception of a1, they are only used for the Hashin variants and Puck. a1 – Residual stiffness factor: The stiffness is never reduced to less than this factor. The default is 0.01. a2 – Matrix compression factor. With this factor, r2 can reduce less due to failure in matrix compression. Experiments show that certain materials show less degradation of the matrix properties in compression than in tension. See for example [Ref. 27]. For the case that Fmc indicates failure in matrix compression, Equation 7-74 is modified into Δr 2 = – ( 1 – a 2 ) ( 1 – e

1–F

mc)

(7-75)

a2 defaults to 0; so the default is full reduction a3 – Shear stiffness factor. This factor is used for taking into account the effect that the shear stiffness G12 can reduce less than the matrix stiffness E2. See [Ref. 28] for experimental data on this subject. With Fm indicating a matrix failure we have Δr 4 = – ( 1 – a 3 ) ( 1 – e

1–F

m)

(7-76)

The combined effect of a2 and a3 on the shear stiffness reduction for the case of matrix compression failure is then Δr 4 = – ( 1 – a 2 ) ( 1 – a 3 ) ( 1 – e

1 – Fm c )

a4 – E33 reduction from fiber failure: This factor controls the reduction of E33 due to fiber and matrix failure. The default is as mentioned above that E33 reduces due to fiber failure. With this factor this can be changed to vary linearly with fiber and matrix failure. With Ff indicating a fiber failure and Fm a matrix failure we have Δr 3 = – ( 1 – a 4 ) ( 1 – e

1–F

f)

– a4 ( 1 – e

1–F

m)

(7-77)

a5 – Shear reduction from fiber failure: With this factor it is possible to control the reduction of the shear stiffness due to fiber failure. By default it only reduces due to matrix failure. With Ff and Fm as in the previous we have Δr 4 = – ( 1 – a 5 ) ( 1 – e

Main Index

1–F

m)

– a5 ( 1 – e

1–F

f)

(7-78)

374 Marc Volume A: Theory and User Information

The Hashin-fabric failure criterion reduces the first three reduction factors from the respective failure index. The three shear reduction factors are taken from the worst of the first three factors. The factors a2 through a5 are not used for this criterion. In addition, it is also possible to use the user subroutine uprogfail to explicitly define the reduction factors r1 through r6. Model 2 – Selective Immediate Degradation This model uses selective degradation just as Model 1, but the stiffness is abruptly decreased. As soon as failure is indicated, the stiffnesses are set to a1 – the residual stiffness factor. The same rules as in Model 1 for how the different factors are defined depending on the type of failure is applied here. Model 3 – Original Marc Method This is the original method in Marc. 1. Upon failure, the material moduli for orthotropic materials at the integration points are set to the smallest of the original moduli, and the smallest is set to 10% of the original. 2. Upon failure, for isotropic materials, the failed moduli are taken as 10% of the original moduli. 3. If there is only one modulus, such as in a beam or truss problem, the failed modulus is taken as 10% of the original one. The different options are flagged through the FAIL DATA model definition option.

Mixture Model The mixture models allow the user to define a composite material that consists of multiple components for all element types. Effective material properties are formed based upon the volume fraction of each material component. There are three variations of the mixture model which have consequences on the type of material that may be used in each component. The component material is defined using the conventional ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, MOONEY, etc. options. The mixture model acts as a continuum in the sense that debonding between the components is not considered in any of the models. Mixture Model 1 This model is applicable to linear elastic materials and heat transfer. An effective material property is formed as N

E

eff

∑

=

Vf ⋅ E

i

i

i = 1 i

where E is the value of the ith component, V f is the volume fraction of the ith component, and N is i

the number of components. The same summation is done for all properties. If an orthotropic component is used, it is done for all nine material properties.

Main Index

CHAPTER 7 375 Material Library

Note that for orthotropic or anisotropic properties, is assumed that all components have the same preferred directions. If the component has temperature dependent properties, then the temperature dependence is evaluated for each component which can be expressed as N

E

eff

(T) =

·

i

∑ Vfi ⋅ E ( T ) :

The stresses obtained are an effective stress associated with the mixture material and not the stress in each component. Mixture Model 2 This model is applicable to linear elastic materials and heat transfer. An effective material stress-strain relationship is formed as N

D

e ff

∑

=

Vf D

i

i

i = 1

where i

i

σ = Dε σ

eff

= D

eff

ε

For heat transfer, analogous equations are used: i

i

q = D ∇T q

eff

= D

eff

∇T

Again, temperature dependent properties are dealt with on a component basis, and orthotropic or anisotropic mixtures must have the same preferred orientations. Mixture Model 3 This model is applicable to nonlinear material behavior. This requires additional allocation of memory to store the associated state variables (plastic strain, shift tensors, etc.) for each component. It is similar to model 2 in that an effective material stress-strain relationship is formed as N

D

e ff

=

∑ i = 1

Main Index

Vf D i

i

376 Marc Volume A: Theory and User Information

i

but now, D includes material nonlinear effects. for the case of elastic-plastic materials, we now have two types of quantities which are not completely consistent with one another. On a component level: i

i

i

i

Δσ = D e l ( Δε – Δε t h – Δε p l ) where again the i indicates the component number which is the correct expression. We also calculate effective quantities. These quantities are accumulated in the usual manner. i

i

σ n + 1 = σ n + Δσ pl(i)

pl(i)

εn + 1 = εn

i

+ Δε

pl(i)

There are also effective quantities calculated as: N

σ

eff

∑

=

Vf σi i

i = 1 N

Δε

pl(eff)

∑

=

V f Δε

pl(i)

i

i = 1

Δε

pl(eff)

N

∑

=

V f Δε

pl(i)

i

i = 1

which are also accumulated. pl(eff)

= εn

pl(eff)

= εn

εn + 1 εn + 1

pl(eff)

+ Δε

pl(eff)

+ Δε

p l ( e ff )

p l ( e ff )

pl

where the ε is the equivalent plastic strain. Note that the effective plastic strain is not used in a subsequent calculation and is only provided for output. Given a mixture of two identical nonlinear materials at a 50%-50% mix, the output of the effective equivalent plastic strain will not be the same as for a solitary material. Mixture model 3 can be used with most nonlinear material behavior, but there are a few restrictions in this release which include: All damage models introduced via the DAMAGE option Gasket material Soils User-defined generalized stress-strain law.

Main Index

CHAPTER 7 377 Material Library

ORNL Rigid Plastic Viscoelasticity Cohesive Grain size effects Thermo-Pore Mass Density The effective mass density for all of the mixture models is calculated as N

ρ

eff

=

∑

Vf ρ

i

i

i = 1

Specific Heat The effective specific heat for all of the mixture models is calculated as N eff Cp

=

i

∑

Vf Cp i

i = 1

Coefficient of Thermal Expansion There are two ways to calculate the coefficient of thermal expansion; the first directly uses the rule of mixtures. N

α

eff

=

∑

α

i

i = 1

The second formulation: α

eff

∑E

i

i

⋅ Vf ⋅ α i = -----------------------------------i ∑ E ⋅ Vf i

where, again, if temperature dependent material properties are used, these are applied at the component level. i

α

eff

i

∑ E ( T ) ⋅ V fi ⋅ α ( T )

( τ ) = -----------------------------------------------------i ∑ E ( T ) ⋅ Vf i

Main Index

378 Marc Volume A: Theory and User Information

Mixtures and Composites It is possible to have a shell element or a composite brick element where the layer of a composite material may be a mixture model that consists of multiple components. Restrictions If the VOID CHANGE or POROSITY CHANGE is used to define a state variable, and the material properties are a function of the void ratio, then all components will use the same void ratio. A mixture material cannot have as a component another mixture material. Mixture materials should not be used with the PSHELL option. Mixture materials cannot be used with design sensitivity or design optimization where the design variable is an elastic property in the mixture material or one of the components.

Gasket Engine gaskets are used to seal the metal parts of the engine to prevent steam or gas from escaping. They are complex (often multi-layer) components, usually rather thin and typically made of several different materials of varying thickness. The gaskets are carefully designed to have a specific behavior in the thickness direction. This is to ensure that the joints remain sealed when the metal parts are loaded by thermal or mechanical loads. The through-thickness behavior, usually expressed as a relation between the pressure on the gasket and the closure distance of the gasket, is highly nonlinear, often involves large plastic deformations, and is difficult to capture with a standard material model. The alternative of modeling the gasket in detail by taking every individual material into account in the finite element model of the engine is not feasible. It requires a lot of elements which makes the model unacceptably large. Also, determining the material properties of the individual materials might be cumbersome. The gasket material model addresses these problems by allowing gaskets to be modeled with only one element through the thickness, while the experimentally or analytically determined complex pressureclosure relationship in that direction can be used directly as input for the material model. The material must be used together with the first-order solid composite element types 149 (three-dimensional solid element), 151 (two-dimensional plane strain element) or 152 (two-dimensional axisymmetric element). In that case, these elements consists of one layer and have only one integration point in the thickness direction of the element. Gaskets can be used in mechanical, thermal or thermo-mechanically coupled analyses. The usual staggered scheme of a heat transfer pass followed by a structural pass is used for coupled analyses. For the heat transfer part, the elements used to model the gaskets are type 175 (three-dimensional first-order solid element), type 177 (two-dimensional first-order planar element), or type 178 (two-dimensional first-order axisymmetric element).

Constitutive Model The behavior in the thickness direction, the transverse shear behavior, and the membrane behavior are fully uncoupled in the gasket material model. In subsequent sections, these three deformation modes are discussed.

Main Index

CHAPTER 7 379 Material Library

Local Coordinate System The material model is most conveniently described in terms of a local coordinate system in the integration points of the element (see Figure 7-10). For three-dimensional elements, the first and second directions of the coordinate system are tangential to the midsurface of the element at the integration point. The third direction is the thickness direction of the gasket and is perpendicular to the midsurface. For two-dimensional elements, the first direction of the coordinate system is the direction of the midsurface at the integration point, the second direction is the thickness direction of the gasket and is perpendicular to the midsurface, and the third direction coincides with the global 3 direction. 3

2

2

1 1

Midsurface Integration Point

Midsurface Integration Point

Figure 7-10 The Location of the Integration Points and the Local Coordinate Systems in Two- and Three-dimensional Gasket Elements

In a total Lagrange formulation, the orientation of the local coordinate system is determined in the undeformed configuration and is fixed. In an updated Lagrange formulation, the orientation is determined in the current configuration and is updated during the analysis. Thickness Direction - Compression In the thickness direction, the material exhibits the typical gasket behavior in compression, as depicted in Figure 7-11. After an initial nonlinear elastic response (section AB), the gasket starts to yield if the pressure p on the gasket exceeds the initial yield pressure py0. Upon further loading, plastic deformation increases, accompanied by (possibly nonlinear) hardening, until the gasket is fully compressed (section BD). Unloading occurs in this stage along nonlinear elastic paths (section FG, for example). When the gasket is fully compressed, loading and unloading occurs along a new nonlinear elastic path (section CDE), while retaining the permanent deformation built up during compression. No additional plastic deformation is developed once the gasket is fully compressed. The loading and unloading paths of the gasket are usually established experimentally by compressing the gasket, unloading it again, and repeating this cycle a number of times for increasing pressures. The resulting pressure-closure data can be used as input for the material model. If the pressure also varies with temperature, then pressure-closure data at different temperatures can be provided. The user must supply the loading path and may specify up to ten unloading paths. In addition, the initial yield pressure py0 must be given. The initial yield pressure can also be varied with temperature and spatial coordinates. The loading path should consist of both the elastic part of the loading path and the hardening part, if present. If no unloading paths are supplied or if the yield pressure is not reached by the loading path, the gasket is assumed to be elastic. In that case, loading and unloading occurs along the loading path.

Main Index

380 Marc Volume A: Theory and User Information

E loading path py1

D G

Gasket Pressure p

py B

py0

A cp0

unloading path

F cp

cy0

C cp1

cy

cy1

Gasket Closure Distance c

Figure 7-11 Pressure-closure Relation of a Gasket

The loading and unloading paths must be defined using the TABLE model definition option (see Marc Volume C: Program Input) and must relate the pressure on the gasket to the gasket closure. Optionally, at each closure value, the loading and unloading paths can also be defined as functions of temperature and spatial coordinates using multi-variate TABLEs. The unloading paths specify the elastic unloading of the gasket at different amounts of plastic deformation; the closure at zero pressure is taken as the plastic closure on the unloading path. If unloading occurs at an amount of plastic deformation for which no path has been specified, the unloading path is constructed automatically by linear interpolation between the two nearest user supplied paths. The unloading path, supplied by the user, with the largest amount of plastic deformation is taken as the elastic path at full compression of the gasket. For example, in Figure 7-11, the loading path is given by the sections AB (elastic part) and BD (hardening part) and the initial yield pressure is the pressure at point B. The (single) unloading path is curve CDE. The latter is also the elastic path at full compression of the gasket. The amount of plastic closure on the unloading path is cp1. The dashed curve FG is the unloading path at a certain plastic closure cp that is constructed by interpolation from the elastic part of the loading path (section AB) and the unloading path CD. The compressive behavior in the thickness direction is implemented by decomposing the incremental gasket closure into an elastic and a plastic part: Δc = Δc e + Δc p

(7-79)

Of these two parts, only the elastic part contributes to the pressure. The constitutive equation is given by the following equation:

Main Index

CHAPTER 7 381 Material Library

p

7

Δp = D c Δc e = D c ( Δc – Δc ) .

Material Library

Here, D c is the consistent tangent to the pressure-closure curve. Plastic defomation develops when the pressure p equals the current yield pressure p y . The latter is a function of the amount of plastic deformation developed so far and is given by the hardening part of the loading path (section BD in Figure 7-11). Initial Gap The thickness of a gasket can vary considerably throughout the sealing region. Since the gasket is modeled with only one element through the thickness, this can lead to meshing difficulties at the boundaries between thick regions and thin regions. The initial gap parameter can be used to solve this. The parameter basically shifts the loading and unloading curves in the positive closure direction. As long as the closure distance of the gasket elements is smaller than the initial gap, no pressure is built up in the gasket. The sealing region can thus be modeled as a flat sheet of uniform thickness and the initial gap parameter can be set for those regions where the gasket is actually thinner than the elements of the finite element mesh used to model it. The initial gap can optionally be varied as a function of spatial coordinates by using a table. Thickness Direction - Tension The tensile behavior of the gasket in the thickness direction is linear elastic and is governed by a tensile modulus D t . The latter is defined as a pressure per unit closure distance (that is, length). D t can optionally be varied as a function of temperature and spatial coordinates by using a multi-variate table. Transverse Shear and Membrane Behavior The transverse shear is defined in the 2-3 and 3-1 planes of the local coordinate system (for threedimensional elements) or the 1-2 plane (for two-dimensional elements). It is linear elastic and characterized by a transverse shear modulus G t . G t can optionally be varied as a function of temperature and spatial coordinates by using a multi-variate table. The membrane behavior is defined in the local 1-2 plane (for three-dimensional elements) or the local 31 plane (for two-dimensional elements) and is linear elastic and isotropic. Young’s modulus E m and Poisson’s ratio ν m that govern the membrane behavior are taken from an existing material that must be defined using the ISOTROPIC model definition option. Multiple gasket material can refer to the same isotropic material for their membrane properties (see also the GASKET model definition option in Marc Volume C: Program Input). Thermal Expansion The thermal expansion of the gasket material is isotropic and the thermal expansion coefficient is taken from the isotropic material that also describes the membrane behavior.

Main Index

382 Marc Volume A: Theory and User Information

Constitutive Equations As mentioned above, the behavior in the thickness direction of the gasket is formulated as a relation between the pressure p on the gasket and the gasket closure distance c. In order to formulate the constitutive equations of the gasket material, this relation (Equation (7-80)) must first be written in terms of stresses and strains. This depends heavily on the stress and strain tensor employed in the analysis. For small strain analyses, for example, the engineering stress and strain are used. In that case, the incremental gasket closure and the incremental pressure are related to the incremental strain and the incremental stress by Δc = – hΔε

and

Δp = – Δσ

(7-80)

in which h is the thickness of the gasket. The resulting constitutive equation for three-dimensional elements, expressed in the local coordinate system of the integration points, now reads

Δσ 11 Δσ 22 Δσ 33 Δσ 12

=

Δσ 23 Δσ 31

νm Em Em ------------------------------- 0 2 2 1 – νm 1 – νm

0

νm Em Em ---------------- ---------------- 0 2 2 1 – νm 1 – νm

0

0

0 Δε 11

0

0

Δε 22 p

Δε 33 – Δε 33

0

0

C

0 0 Em 0 -------------------------- 0 2 ( 1 + νm )

0

Δγ 12

0

0

0

Δγ 23

0

0

0

0

Gt 0

0

0

0

0

0 Gt

(7-81)

Δγ 31

in which C = hD c . For two-dimensional elements, the equation is given by νm Em Em ---------------- 0 ---------------- 0 2 2 1 – νm 1 – νm

Δσ 11 Δσ 22 Δσ 33 Δσ 12

=

0 C 0 0 νm Em Em ---------------- 0 ---------------- 0 2 2 1 – νm 1 – νm 0

0

0

Δε 11 p

Δε 22 – Δε 22

(7-82)

Δε 33 Δγ 12

Gt

For large deformations in a total Lagrange formulation, in which the Green-Lagrange strains and the second Piola-Kirchhoff stresses are employed, as well as in an updated Lagrange environment, in which the logarithmic strains and Cauchy stresses are being used, similar but more complex relations can be derived.

Main Index

CHAPTER 7 383 Material Library

Nonlinear Hypoelastic Material The hypoelastic model is able to represent a nonlinear elastic (reversible) material behavior. For this constitutive theory, Marc assumes that σ· i j = L i j k l ε· k l + g i j

(7-83)

where L is a function of the mechanical strain and g is a function of the temperature. The stress and strains are true stresses and logarithmic strains, respectively, when used in conjunction with the LARGE STRAIN. When used in conjunction with the LARGE DISP option only, Equation (7-83) is expressed as · · Si j = Li j k l Ek l + gi j

(7-84)

where E, S are the Green-Lagrangian strain and second Piola-Kirchhoff stress, respectively. A HYPOELASTIC or NLELAST model definition option is necessary to invoke this model. These models can be used with any stress element, including Herrmann formulation elements. The tensors L and g are defined by you in the HYPELA2 user subroutine or via the NLELAST model definition option. HYPELA2 User Subroutine In order to provide an accurate solution, L should be a tangent stiffness evaluated at the beginning of the iteration. In addition, the total stress should be defined as its exact value at the end of the increment. This allows the residual load correction to work effectively. In HYPELA2, additional information is available regarding the kinematics of deformation. In particular, the deformation gradient ( F ), rotation tensor ( R ), and the eigenvalues ( λ ) and eigenvectors ( N ) to form the stretch tensor ( U ) are also provided. This information is available only for the continuum elements namely: plane strain, generalized plane strain, plane stress, axisymmetric, axisymmetric with twist, and three-dimensional cases. For more information on the use of user subroutines, see Marc Volume D: User Subroutines and Special Routines. NLELAST Model Definition The NLELAST model definition in Marc supports the Nastran NLELAST capability and simplified nonlinear elasticity models. These models all have the form that a strain energy function does not exist but have been found to be useful in solving engineering simulations, where only a limited amount of test data is available. The theory and algorithms are adequate to trace the stress-strain curve accurately for the uniaxial loading cases. However, the theory is not based on the classical theory of finite elasticity. Consequently, some of the constitutive relations may be violated in the multiaxial stress state and, as a result, limit the use of this model to small strain.

Main Index

384 Marc Volume A: Theory and User Information

Six models are implemented in Marc to support nonlinear elasticity based upon the input of a uniaxial stress strain law. These models are summarized as: 1. Nastran like NLELAST model based upon MATS1 input option. 2. Hypoelastic strain invariant model. 3. Model based upon working in principal strain space which results in induced anisotropic behavior. 4. Linear elasticity with tension and/or compression cut-off. 5. Bi-modulus elasticity with tension and/or compression cut-off. 6. Nonlinear orthotropic elasticity based upon non-rotating preferred directions. The HYPELA2 user subroutine can be used if special material behavior is required. Basic assumptions and definitions A material model is called elastic if the stress is a function of the strain. This implies two important properties: the material is reversible and the stress at a point in the material depends only on some measure of strain at that point. Elastic materials implemented with this option are in the hypoelastic framework. This group of nonlinear elastic materials is therefore grouped in Mentat under Materials -> HYPOELASTIC. The nonlinearity in the material models introduced here results from the definition of the stress as a function of the strain path. The models are anticipated to behave correctly in the small strain region only (less than 5%). Input of uniaxial stress-strain data In the next sections the theory and input is described for each of the different material models. As a basis it is assumed that the user has a set of engineering stresses and engineering strains available. This means that in the uniaxial test: • The measured elongations are compared to the original length of the test specimen, resulting in: ε engineering = ΔL ⁄ L 0 • The measured forces are compared to the original cross-section of the test specimen, resulting in: σ engineering = F ⁄ A 0 For analysis without large incremental or total rotation or large incremental or total strains, the engineering values can be used as is. In some models, certain characteristics still have to be derived. This is described in the sections per material type.

Main Index

CHAPTER 7 385 Material Library

For analysis where the LARGE DISP, UPDATE, and FINITE, or PLASTICITY,3, or LARGE STRAIN parameters are used, the uniaxial test data cannot be used ‘as is’. Engineering strain and stress are measures that are invalid once the strain in the analysis model is no longer ‘small’ (approximately 5%). For these large strain simulations, the true stress and strain definition have been adopted in Marc. This nonlinear strain measure is dependent upon the final length of the model. Since the NLELAST material models are only valid in this small range it is not necessarily required to convert the engineering data. Converting engineering strain/stress to true strain/stress True strain is defined as: ε true =

∫ ΔL ⁄ L

By integration, it can be shown that this directly defines the true strain as: ε true = ln ( 1 + ε engineering )

(7-85)

Similarly, the uniaxial engineering stress data can be converted to true stress (also known as Cauchy stress) by means of: σ true = σ engineering ( 1 + ε engineering )

(7-86)

By using Equations (7-85) and (7-86), the uniaxial test data can quickly be transformed into true stress/strain data. Figure 7-12 shows the deviation of engineering stress/strain compared to the engineering definition. In the remainder of this section on nonlinear elasticity the engineering stresses and strains can be mutually exchanged with their true counterpart. The tables can be either engineering or true data depending on the options activated in the analysis. Comparison between engineering and true stress/strain 200

true or engineering stress

150 100

True Stress Engineering Stress

50 0 -0.05

-0.04

-0.03

-0.02

-0.01

0

0.01

0.02

0.03

0.04

0.05

-50 -100 -150 -200 true or engineering strain

Figure 7-12 Comparison Between Engineering and True Stress/Strain

Main Index

386 Marc Volume A: Theory and User Information

Type 1: Nastran like nonlinear elasticity model The stress curve is supplied in a table with independent variable mechanical strain (id=69). An additional independent variable in the table may be temperature (id=12). Note that a table with independent variable mechanical strain is a requirement for the analysis. It is optional to define Poisson’s ratio as a function of temperature. The initial Young’s modulus is the slope of the equivalent stress-strain curve is derived by Marc from the table at ε = 0. This imposes the continuous definition of the slope at ε = 0. Theoretical Basis The nonlinear elastic capability in Nastran was designed to satisfy the equivalence of the deformation work per unit volume in the simple tension to the strain energy per unit volume (conservation of energy), while the work done for deformation may be defined by a stress-strain curve in simple tension, i.e.,

∫ σ dε

=

∫ <σ> { dε }

It is further assumed that the effective strain ε may be defined by: 1 2 1 --- Eε = --- <ε> [ D e ] { dε } 2 2 From the total differential of the above equation, we obtain 1 dε = ------ <ε> [ D e ] { ε } Eε Substituting the latter in the first equation above, where stresses may be expressed in terms of total strains, i.e. σ { σ } = ------ [ D e ] { ε } Eε The tangential matrix for such material may be obtained by differentiating the latter equation, i.e. ∂{σ} σ α ∂σ σ [ D n e ] = ------------- = ------ [ D e ] + ------ ⎛ ------- – ---⎞ [ D e ] { ε }<ε> [ D e ] T ∂{ ε} Eε Eε ⎝ ∂ε ε ⎠ In the original Nastran, implementation α is set to 1. In the Marc implementation, testing proved that setting this value to 0.0 (default) improves convergence significantly. Solution Algorithm The user specifies the nonlinear stress-strain curve, σ ( ε ) in a TABLE parameter along with a NLELAST model definition. The NLELAST entry does require a table for Young’s modulus; whereas, strain dependency for Poisson’s ratio is optional.

Main Index

CHAPTER 7 387 Material Library

The NLELAST material interfaces with the element routines with the following data: • Input: { σ } old , { ε } o l d , { Δε } , E , ν • Output: { σ } new , { ε } new , [ D n e ] The computational procedure is described below: Step 1:

Upon entry the new strain state is computed by: { ε } new = { ε } old + { Δε }

Step 2:

The effective strain is computed based on { ε } new by 1 ε 2 = --- <ε> { σ e } E where { σe } = [ De ] { ε } D e is simply formed using the Hookean law.

Step 3:

The effective stress ( σ ) is determined by looking-up the user-specified stressstrain curve for . ε .

Step 4:

The new stress state is determined by scaling the stress-strain law: σ { σ } new = ------ { σ e } Eε

Step 5:

The tangential matrix is determined by σ α ∂σ σ [ D n e ] = ------ [ D e ] + --------- ⎛ ------- – ---⎞ { σ e } { σ e } T Eε Eε 2 ⎝ ∂ε ε ⎠

∂σ Furthermore ------- is the slope at the current strain. ∂ε The tables for NLELAST must be supplied in the new table format. Combining Uniaxial Tension and Compression Stress-strain Curves Some materials exhibit appreciably different behavior in compression from that in tension even in the small strain range. For uniaxial loading the magnitude of the strain in that direction becomes the effective strain, i.e., ε = ε x for uniaxial tension in x

Main Index

388 Marc Volume A: Theory and User Information

ε = – ε x for uniaxial compression in x In order to remain compatible with the Nastran implementation of this material model, the user has the option to ignore the uniaxial compression data, even if it is supplied on input. In case of this unsymmetric material behavior, we need to be able to distinguish between a state of compression and a state of tension. There are two known data points for one effective strain ε , namely the effective stress for uniaxial tension ( σ t ) and the effective stress for uniaxial compression ( σ c ) . Some method of interpolation or extrapolation is required to predict the effective stress for the general stress state using two known data points. The first stress invariant ( I 1 ) has been adopted for interpolation/extrapolation as follows, I1 = σx + σy + σz Considering that the pure shear is in the midway between simple tension and simple compression, it seems appropriate to use the first stress invariant. Hydrostatic tension and compression cases will impose lower- and upper-bounds for extrapolation, i.e., I 1 = σ x for uniaxial tension/compression I 1 = 0 for pure shear

I1 = 3 p for hydrostatic pressure ∂σ The instantaneous modulus ⎛ -------⎞ should be interpolated or extrapolated in the same manner. ⎝ ∂ε ⎠ Solution Algorithm for Bilateral Stress-strain Relations The new stress state is proportional in magnitude to the effective stress σ , which should be determined as follows: 1. Compute the effective stress ( σ e ) based on { σ e } ; i.e., { σe } = [ De ] { ε } σ =

1 2 2 2 --- [ ( σ x – σ y ) 2 + ( σ y – σ z ) 2 + ( σ z – σ x ) 2 ] + 3 ( τ x y + τ y z + τ z x ) for 3-D 2

σ =

σ x – σ x σ y + σ y + 3τ x y for plane stress

σ =

1 2 --- [ ( σ x – σ y ) 2 + ( σ y – σ z ) 2 + ( σ z – σ x ) 2 ] + 3τ x y for plane strain 2

2

2

2

2. Compute the first invariant of I = σ x + σ y + σ z :

Main Index

CHAPTER 7 389 Material Library

where σ z = 0 for plane stress 3. Determine the ratio ( r ) by normalizing I I by σ c , i.e., I1 r = -----σe where r signifies the relative distance from the midpoint of σ c and σ t at ε . It would be implausible to process a large value of r (such is the case with a hydrostatic load). Therefore, r , will be confined to a plausible range, – 1 ≤ r ≤ 1 . The value will be reset to the limit ( r = ± 1 ) if r lies outside the range. 4. Look up the user specified stress-strain curve in the TABLE entry and determine σ t and σ c ; i.e., σt = σ ( ε ) σc = σ ( ε ) 5. Determine based on σ t , σ c . and r ; i.e., σt + σc σt – σc σ = ------------------ + r -----------------2 2 ∂σ For the tangent matrix the instantaneous modulus ⎛ -------⎞ should be determined using the same ratio (r) ⎝ ∂ε ⎠ as follows: 1. Compute the instantaneous slope at ε for tension, i.e., yi + 1 – yi ⎛ ∂σ -⎞⎠ = ------------------------ for x i ≤ ε ≤ x i + 1 ⎝ -----xi + 1 – xi ∂ε t where ( x i, y i ) is the i-th data point in the TABLE entry 2. Compute the instantaneous slope at – ε for compression; i.e., yj + 1 – yj ⎛ ∂σ -⎞⎠ = ------------------------ for x i ≤ ε ≤ x i + 1 ⎝ -----xj + 1 – xj ∂ε c ∂σ ∂σ ∂σ 3. Determine ------- based on ⎛ -------⎞ , ⎛ -------⎞ and r , i.e., ⎝ ⎠ ⎝ ∂ε ∂ε t ∂ε ⎠ c r ∂σ ∂σ 1 ∂σ ∂σ ∂σ ------- = --- ⎛⎝ -------⎞⎠ + ⎛⎝ -------⎞⎠ + --- ⎛⎝ -------⎞⎠ – ⎛⎝ -------⎞⎠ 2 2 ∂ε t ∂ε ∂ε t ∂ε c ∂ε c Subsequently the values can now be used as in the tension-only algorithm.

Main Index

390 Marc Volume A: Theory and User Information

Type 2: Strain Invariant Model This model, like others in Marc is based upon the incremental theory where dσ = C e l dε e l And C e l is a Hooke’s law based upon the current values of the Young’s modulus and Poisson’s ratio. In this model these quantities are a function of the strain invariants I 1 , I 2 , I 3 . For this model, Marc computes the three strain invariants in each integration point of the element. The three strain invariants are independent variables in the Young’s modulus vs strain-invariant table that is supplied on input. In principle a table with all three strain invariants can be supplied if necessary, however, when converting the uniaxial data into Young vs strain-invariant tables it is usually sufficient to choose one. The choice may depend on the element type used and the need to model non-symmetric behavior in compression and tension. This is explained further below. Marc looks up Young’s modulus in the user-supplied table and forms a Hookean stress-strain law. In order to arrive at proper input, additional data conversion of the uni-axial data needs to be done. Starting from uniaxial (engineering or true) stress strain data, the elasticity modulus (Young) needs to be derived for a number of engineering or true strain data points. See Figure 7-13.

160 140 120 100 80 60 40 20 0

10000 8000 engineering strain Young's modulus

Young's modulus

Stress

Uniaxial stress & Young vs Strain

6000 4000 2000

0

0.01

0.02

0.03

0.04

0 0.05

Strain

Figure 7-13 Uniaxial Stress and Young vs Strain

The definition of these invariants in Marc is as follows: I 1 = trace [ ε ] = ε x x + ε y y + ε z z 2

2

2

2

I 2 = 1 ⁄ 2 { trace ( [ ε ] ⋅ [ ε ] – I 1 ) } = ε x y + ε y z + ε z x ( ε x x ε y y + ε y y ε z z + ε z z ε x x ) 2

2

2

I 3 = det [ ε ] = ε x x ε y y ε z z + 2ε x y ε y z ε z x – ε y y ε y z + ε y y ε z x + ε z z ε x y

Main Index

CHAPTER 7 391 Material Library

Because only two elastic moduli (Young’s modulus and Poisson ratio) which are functions of the invarients are defined, the material will behave isotropically in the simulation. In the input table, the three strain invariants are indicated by means of id’s 70, 71, and 72. For uniaxial and plane stress elements, a special treatment is followed in Marc. The out-of-plane strains are not computed internally. Therefore incompressibility (poisson = 0.5, see Figure 7-14) is assumed, such that I 1 = 0 : the first invariant is very closely related to the hydrostatic strain ( I 1 ⁄ 3 ) . The other invariants automatically follow from this assumption. Influence of incompressibility on first strain invariant 0.02

0.015

First strain invariant

First strain invariant (poisson = 0.3)

0.01

First strain invariant (poisson = 0.5)

0.005

0 -0.05

-0.04

-0.03

-0.02

-0.01

0

0.01

0.02

0.03

-0.005

-0.01

-0.015

-0.02

Engineering strain

Figure 7-14 Influence of Incompressibility on First Strain Invariant

For a uniaxial element: ε x y = ε y z = 0 and ε y y = ε z z 1 I 1 = 0 = >ε y y = ε z z = – --- ε x x 2 3 2 I 2 = --- ε x x 4 1 3 I 3 = --- ε x x 4 For a plane stress element: εy z = εz x = 0

Main Index

0.04

0.05

392 Marc Volume A: Theory and User Information

I 1 = 0 = >ε z z = – ( ε x x + ε y y ) 2

2

2

I2 = εx y + εx x + εy y + εx x εy y 2

I3 = ( εx x + εy y ) ( εx y – εx x εy y ) It is important to realize that the incompressibility assumption for different elements has a direct impact on the material data supplied in the input deck. For different element types, the input data derived from the uniaxial test data will be different. We compare the behavior of a plain stress element (e.g., element 3), a hexahedral element (e.g., element 7), a plane strain element (e.g., element 11) and a beam element (e.g., element 52). For the materials, we define a Poisson’s ratio of 0.3 and we prescribe a fixed displacement which brings us into the nonlinear part of the stress-strain curve. Note that Poisson’s ratio may also vary with the uniaxially measured strain, in this case this has to be accounted for in the 2-D and 3-D elements. 3-D Element – Three Direct Components of Strain For the hexahedral element, we may choose any of the invariants as independent variable. In order to get a corresponding behavior with the uniaxial test, we have to supply the first invariant in the following form: ε x x = ε engineering ε y y = ε z z = – υε engineering I 1 = ε x x + ε y y + ε z z = ( 1 – 2υ )ε engineering ( or: I 1 = ( 1 – 2ν )ε true ) 2-D Elements – Two Direct Components of Strain (= Plane Stress) Although the plane stress elements in Marc have a third strain component unequal to zero, Marc does not compute it. It has been chosen that the user input for the stress-strain data has to follow the incompressibility assumption ( I 1 = 0 ) . In this case, we may use the definition of the second invariant in order to define a dependency on strain, supposing a uniaxial loading: ε x x = ε engineering ε x y = ε y z = ε z x = 0 (uniaxiality) ε y y = – υε engineering from I 1 = 0 , we deduce (see above): 2

2

I2 = εx x + εy y + εx x εy y

Main Index

CHAPTER 7 393 Material Library

2

I 2 = ( υ 2 – υ + 1 )ε engineering 2-D Elements – Three Direct Components of Strain (= Plane Strain) For the plane strain elements, the third direct strain term is zero. In this case, incompressibility is not assumed and the strain invariants can be easily derived from the conditions: σ y y = 0 and ε x x = 0 under uniaxial loading: ε x x = ε engineering ε x y = ε y z = ε z x = ε z z = 0 (uniaxiality and plain strain) ε y y = υ ⁄ ( υ – 1 ) ε engineering I 1 = ε x x + ε y y + ε z z = { 1 + ν ⁄ ( ν1 ) }ε engineering I2 = εx x εy y 2

I 2 = υ ⁄ ( υ – 1 ) ε engineering 1-D Elements – One Direct Components of Strain For the beam and truss elements, we cannot use the first invariant as independent variable either, since I 1 = 0 . We may quickly derive that: 2

2

I 2 = 3 ⁄ 4ε engineering (or I 2 = 3 ⁄ 4ε true ) Loading Under Tension/Compression It must be noted that for both beam and plane stress elements a nonsymmetric behavior in compression cannot be described by means of the second invariant because I 2 ≥ 0 (see Figure 7-15). The third invariant can be used for this purpose; e.g., for the 1-D elements: 3 3 (or I 3 = 1 ⁄ 4ε true ) I 3 = 1 ⁄ 4ε engineering And finally for the 2-D plane stress elements: ε x x = ε engineering ε x y = ε y z = ε z x = 0 (uniaxiality) ε y y = – υε engineering

Main Index

394 Marc Volume A: Theory and User Information

Second strain invariant (> 0) 1.4000E-03

Second strain invariant

1.2000E-03

1.0000E-03

8.0000E-04

6.0000E-04

4.0000E-04

2.0000E-04

0.0000E+00 -0.05

-0.04

-0.03

-0.02

-0.01

0

0.01

0.02

0.03

0.04

0.05

Engineering strain

Figure 7-15 Second Strain Invariant (>0)

from I 1 = 0 , we deduce 2

I3 = ( εx x + εy y ) ( εx y – εx x εy y ) 3

I 3 ν ( υ – 1 )ε engineering Data Approximation Finally it is important to realize that the second and third invariants are nonlinear functions of the strain. As a result, even a linear stress-strain curve will form a polynomial of the second or third order for the second and third strain invariant respectively. It is, therefore, wise to apply the load in a sufficient number of increments, even though the actual behavior is only linear. This is shown in Figure 7-16. Type 3: Principal Strain Space Model In the principal strain space theory, the strain tensor’s principal values are now computed. The compliance matrix is formed using a total strain approach; i.e., the secant modulus is computed for each principal strain by looking up the stress in the user defined table. This results in three values for the modulus. These values are then used to form an orthotropic stress-strain law together with poisson’s ratio and a shear modulus, which are also user defined. The definition of the orthotropic stress-strain law is described in Volume C (chapter 3). It must be noted that the constants have to fulfill certain requirements in order to guarantee stability. These criteria are checked by Marc. However, if stability cannot be guaranteed, Marc will continue to solve the increment at hand, and moreover that it will continue if the increment converges. From this point on, the solution may not be trustworthy anymore and care should be taken.

Main Index

CHAPTER 7 395 Material Library

Influence of # of datapoints on third strain invariant 2.0000E-05

Third strain invariant

1.5000E-05 1.0000E-05 5.0000E-06 0.0000E+00 -0.05

-0.04

-0.03

-0.02

-0.01

0

0.01

0.02

0.03

0.04

0.05

-5.0000E-06 -1.0000E-05 -1.5000E-05 -2.0000E-05

Engineering strain

Figure 7-16 Influence of Number of Data Points on the Third Strain Invariant

Theoretical Background The Principal strain space theory can be defined as the incremental stress strain law which is based upon an orthotropic Hooke’s law expressed with respect to a set of axis aligned with the principal axes based upon the strain tensor. The moduli ( E , ν , G ) are evaluated at the current values of the principal strains. Consider E to be the reference material system of the element. For a continuum element, this is the global system, while for a shell element this is the ν 1 , ν 2 , ν 3 system. Now, consider the total strain at the beginning of the increment ε n . One can obtain the principal strains and the eigenvectors of this system. The principal strains are ε 1 , ε 2 , ε 3 and the eigenvectors are n 1 , n 2 , n 3 , The matrix that transforms the E system to the principal system is R . The state is then rotated into the principal, this includes the stresses, strains, thermal strains and creep strains. σ n + 1 = R T σR , etc. Based upon the principal strains, the material properties for the current value of the principal strains are determined. The evaluated material constants are tested to make sure stability is not violated, also positive definiteness of the compliance matrix is checked. Then the constitutive law is evaluated based upon the current Young’s moduli, Poisson ratios, and shear modulus.

Main Index

396 Marc Volume A: Theory and User Information

Based upon either the estimated or calculated incremental strain, the incremental stress in principal space is determined. Subsequently the total stress in principal space is calculated and the quantities are rotated back to the E system. p

σ n + 1 = Rσ n + 1 R T = R ( σ p + Δσ p )R T The constitutive law is also rotated back into the E system. C = RC p R T This is then used in the tangent stiffness matrix calculation. Type 4: (Bimodulus) Elasticity Model This is conventional Hooke’s law, where the Young’s modulus and Poisson ratio may be function of temperature or position, but not strain or stress. Further below, a description is given of the treatment regarding tension and compression limits.

Linear Elasticity

Bimodulus Elasticity

Type 5: (Bimodulus) Elasticity Model with Either No Tension, Limited Tension, No Compression, or Limited Compression Enhancements In this model, the hydrostatic strain will be calculated and if the value is positive, the tensile values of Young’s modulus and Poisson’s ratio will be used. If the hydrostatic strain is 0, as in the very beginning of the analysis, the tensile values will be used. For Model 4 Given total strains, the total stresses are calculated based upon tensile properties. This results in C and σn + 1 ,

Main Index

CHAPTER 7 397 Material Library

For Model 5 To distinguish a tension or compression stress state the hydrostatic strain is computed. If the hydrostatic strain is positive the total stresses are calculated based upon tensile properties. Resulting in C ten and σ n + 1 If the hydrostatic strain is negative, the total stresses are calculated based upon compressive properties. This results in C com and σ n + 1 ,

No Tension Material

No Compression Material

Bimodulus with both Tension and Compression Cut-off

For Either Model 4 or 5 The treatment of the cut-offs works as follows, if they are defined in the simulation. The principal stresses σ 1 , σ 2 , σ 3 and the eigenvectors are n 1 , n 2 , n 3 are obtained. If σ I > Tensile stress limit, then principal direction i will be reduced. If σ I < Compressive stress limit, then principal direction i will be reduced. The reduction implies that a new secant modulus is computed for the current reduced direction. The maximum secant modulus in one of the reduced directions is used to form a new stress-strain law. The transformation matrix: R e p is obtained between Element system E and Principal system P .

Main Index

398 Marc Volume A: Theory and User Information

A stiffness matrix is recreated using the secant modulus of the current limit stress vs strain state.This is also done to improve stability. Cz = RepCpRe pT Rotate stresses to principal system and maximize the stress to the limit in ith component, and then rotate back into element system: p

σn + 1 = R e p T σn + 1 R e p p–z

σ nz + 1 = R e p σ n + 1 R e p T Note that there is no need to form C p because C is from isotropic elasticity, and R is a proper orthogonal matrix. Therefore the stiffness matrix C can be formed in the global system with the limited secant modulus. Type 6: Nonlinear Orthotropic Elasticity Model This model is based upon orthotropic Hooke’s law, written with respect to a fixed preferred material orientation. The difference is that the nine constants, E 11 , E 22 , E 33 , ν 12 , ν 23 , ν 31 , G 12 , G 23 , G 31 may be a function of the spatial position, temperature, and the strain in the associated direction. This can be expressed as: E 11 = E 11 ( X ,T ,ε 11 ) , etc. ν 12 = ν 12 ( x ,T ,γ 12 ) , etc. G 12 = G 12 ( x ,T ,γ 12 ) , etc. The material properties are evaluated based upon the current value of the independent variables, and the Hooke’s law is used to create the current tangent modulus. The incremental stress follows from these moduli and the incremental strains. The evaluated material constants are evaluated to make sure stability is not violated, also it is determined if the compliance matrix is positive definite. As the material orientations do not change, the usual procedure for defining them is used. Type 7: Small Strain Nonlinear Elasticity Model This is the only NLELAST model which is actually based on a strain energy function. The derivation of this material model follows below. The user supplies the experimental stress-strain data and optionally the Poisson’s ratio vs strain data. Marc will derive the necessary data as described below. It is assumed that the strain energy is a nonlinear function of the following form: 2 1 W = --- C 1 ( ˆI 1 )Iˆ 1 + C 2 ( ˆI 2 )Iˆ 2 2

Main Index

CHAPTER 7 399 Material Library

where: ˆI 1 = ε = ε ν ii

(volumetric)

1 Iˆ 2 = --- e i j e i j 2

(deviatoric)

1 e i j = ε i j – --- ε ν δ i j 3

(where δ i j is the Kronecker delta)

As a result, W is decoupled in a purely volumetric part and a purely deviatoric part. The stress tensor is directly related to the strain energy function, as follows: ∂C 1⎞ ∂Iˆ ∂C 2 ⎞ ∂Iˆ 2 ⎛ ∂W 1⎛ σ i j = --------- = --- ⎜ 2C 1 + ----------⎟ ˆI 1 --------- + ⎜ C 2 + ---------- ˆI 2⎟ --------∂ε i j 2⎝ ∂Iˆ 1 ⎠ ∂ε i j ⎝ ∂Iˆ 2 ⎠ ∂ε i j ∂C 1⎞ ∂C 2 ⎞ ⎛ 1⎛ = --- ⎜ 2C 1 + ----------⎟ ˆI 1 δ i j + ⎜ C 2 + ---------- ˆI 2⎟ e i j 2⎝ ⎝ ∂Iˆ 1 ⎠ ∂Iˆ 2 ⎠ Thus: σ i j = K ( Iˆ 1 )Iˆ 1 δ i j + 2G ( ˆI 2 )e i j where K is a nonlinear bulk modulus: ∂C 1 ⎞ 1⎛ K ( ˆI 1 ) = --- ⎜ 2C 1 + ---------- ˆI 1⎟ 2⎝ ∂Iˆ 1 ⎠ where G is a nonlinear shear modulus: ∂C 2 ⎞ 1⎛ G ( ˆI 2 ) = --- ⎜ C 2 + ---------- ˆI 2⎟ 2⎝ ∂Iˆ 2 ⎠ This can be related to the uniaxial tension (or compression) test as follows. The stress-strain curve has been measured. See Figure 7-17. Optionally, the user supplies a table for Poisson’s ratio with a dependency on the measured uniaxial strain. For example, see Figure 7-19:

Main Index

400 Marc Volume A: Theory and User Information

140 120

Stress

100 80 60 40 20 0 0

0.02

0.04

0.06

Uniaxial Strain

Figure 7-17 Experimental Uniaxial Stress Strain Date

Young’s moduli vs strain can then easily derived. 4500

E (Young's modulus)

4000 3500 3000 2500 2000 1500 1000 500 0 0

0.02

0.04

Uniaxial Strain

Figure 7-18 Derived Young’s Modulus vs Strain

Main Index

0.06

CHAPTER 7 401 Material Library

0.35

0.3

Poisson

0.25

0.2

0.15

0.1

0.05

0 0

0.01

0.02

0.03

0.04

0.05

0.06

Uniaxial Strain

Figure 7-19 ExPERIMENTAL POISSON’S RATIO VS STRAIN

Relating the Energy Function to the Experiment From the uni-axial tensile test the strain is available. The following derivation shows how the test data can be related to the Bulk and Shear expressions derived above. The Bulk and Shear expressions are subsequently used in an expression for the stiffness matrix. First, we derive the strain components and first invariant as a function of the uniaxial strain: ε 11 = ε ;ε 22 = ε 33 = – ν ε ˆI 1 = ε – 1--- ( 1 – 2ν )ε 3

(first strain invariant)

1 2 e 11 = ε – --- ( 1 – 2ν )ε = --- ( 1 + ν )ε 3 3 1 1 e 22 = e 33 = – νε – --- ( 1 – 2ν )ε = – --- ( 1 + ν )ε 3 3 The differential of the strain energy function is now used to evaluate the stresses: 4 σ 11 = --- ( 1 + ν )G ( ˆI 2 )ε + ( 1 – 2ν )K ( Iˆ 1 )ε = 3 2 σ 22 = – --- ( 1 + ν )G ( Iˆ 2 )ε + ( 1 – 2ν )K ( Iˆ 1 )ε = 3

Main Index

4 --- ( 1 + ν )G ( ˆI 2 ) + ( 1 – 2ν )K ( ˆI 1 ) ε 3 2 ( 1 – 2ν )K ( ˆI 1 ) – --- ( 1 + ν )G ( Iˆ 2 ) ε = 0 3

402 Marc Volume A: Theory and User Information

Thus: 2(1 + ν ) K ( ˆI 1 ) = ------------------------- G ( ˆI 2 ) 3 ( 1 – 2ν ) Using the latter equation in the expression for σ 11 results in: σ 11 =

2 4 --- ( 1 + ν ) + --- ( 1 + ν ) G ( Iˆ 2 )ε = 2 ( 1 + ν )G ( ˆI 2 )ε = Eε 3 3

As a result: E K ( Iˆ 1 ) = ------------------------3 ( 1 – 2ν ) E G ( ˆI 2 ) = --------------------2(1 + ν) Furthermore, we derive the strain invariants as function of the experimental uniaxial strain: ˆI 1 = ε = ( 1 – 2ν )ε ii ˆI 2 = 1--- ⎛ 4--- ( 1 + ν ) 2 ε 2 + 2 1--- ( 1 + ν ) 2 ε 2⎞ = 1 --- ( 1 + ν ) 2 ε 2 ⎠ 3 2⎝9 9 Now the curves E ( ε ) and ν ( ε ) can be translated into G ( ˆI 2 ) and K ( ˆI 1 ) curves. Stiffness Tensor The stiffness tensor is derived as follows: ∂σ i j E i j k l = ---------∂ε k l Ei j k l =

∂e i j ∂K ∂G -------- + K ( ˆI 1 ) δ i j δ k l + 2G ( ˆI 2 ) ---------- + 2 -------- e i j e k l ∂ε k l ∂Iˆ 1 ∂Iˆ 2

In which: ∂e i j 1 1 --------- = --- [ δ i k δ j l + δ i k δ j l ] – --- δ i j δ k l ∂k l 2 3 We finally arrive at: ∂G ∂K 2 E i j k l = G ( ˆI 2 ) [ δ i k δ j l + δ i k δ j l ] + 2 -------- e i j e k l + K ( ˆI 1 ) + -------- ˆI 1 – --- G ( ˆI 2 ) δ i j δ k l 3 ∂Iˆ 2 ∂Iˆ 1

Main Index

CHAPTER 7 403 Material Library

So G ( Iˆ 2 ) and K ( Iˆ 1 ) tables can easily be generated from σ ( ε ) and ν ( ε ) tables which come from measurements. This generation is automatically done in Marc after the uni-axial stress-strain data has been read in. In order to properly handle compression and tension, it is required to have: ∂K -------- = 0 for ˆI 1 = 0 ∂Iˆ 1 Furthermore we assume symmetry of the K ( ˆI 1 ) curve about ˆI 1 = 0 , but we may destroy this symmetry: then compression and tension behavior will not be the same. The model is thought to be reasonably sound as long as the strains are small (< 5%). Stability of the Model The volumetric behavior is stable as long as: ∂p ∂K K f = -------- = K ( ˆI 1 ) + -------- ˆI 1 < 0 ˆ ∂I 1 ∂Iˆ 1

Volum etric behaviour 140

120

Pressure

100

80

60

40

20

0 0

0.01

0.02

0.03

0.04

F i r s t i nv ar i ant I1

Figure 7-20 Volumetric Behavior

p = K ( Iˆ1 ) Iˆ1

Main Index

0.05

0.06

404 Marc Volume A: Theory and User Information

140 120

Shear Stress

100 80 60 40 20 0 0

0.01

0.02

0.03

0.04

0.05

0.06

gamma

Figure 7-21 Deviatoric Behavior

τ = G ( ˆI 2 )γ Similarly for the deviatoric (simple shear) behavior, we find ˆI 2 = 1--- ( γ 2 ⇒ γ ) = 2

2Iˆ 2

1 ˆ ( γ )γ τ = G ( ˆI 2 ) 2Iˆ 2 = G ⎛ --- γ 2⎞ γ = G ⎝2 ⎠ ˆ ∂τ ∂G ˆ (γ) > 0 G f = ------ = ------- γ + G ∂γ ∂γ

Thermo-Mechanical Shape Memory Model NiTi alloys with near-equiatomic composition exhibit a reversible, thermoelastic transformation between a high-temperature, ordered cubic (B2) austenitic phase and a low-temperature, monoclinic (B19) martensitic phase. The density change and thus the volumetric are small and on the order of 0.003. The transformation strains are, thus mainly deviatoric, of the order of 0.07-0.085. However, these small dilational strains do not necessarily lead to a lack of pressure sensitivity in the phenomenology. The behavior of nitinol is different depending on whether the materials are subjected to hydrostatic tension or compression. Typical phenomenology is shown in Figure 7-22 taken from Miyazaki et al. (1981). The curves indicate that upon cooling, the material transformation from austenite to martensite begins once the M s temperature is reached. Upon further cooling, the volume fraction on martensite is a given function of temperature; the volume fraction becomes 100% martensite when the M f temperature is reached. Upon heating, transformation from martensite to austenite begins only after A s temperature is reached. This

Main Index

CHAPTER 7 405 Material Library

re-transformation is complete when the A f temperature is reached. Finally, note that the four transformation temperatures are stress dependent. The experimental data indicate the M s , M f , A s , and A f may be approximated from their stress-free values, M s0 , M f0 , A s0 , and A f0 by σe q M s = M s0 + -------- , Cm σe q M f = M f0 + -------- ; and Cm σe q A s = A s0 + -------- , Ca σe q A f = A f0 + -------- . Ca where σ e q is the von Mises equivalent stress. At a sufficiently high temperature, often called the M d temperature, transformation to martensite does not occur at any level of stress. The transformation characteristics such as the transformation temperatures depend sensitively on alloy composition and heat treatment. Mf

1.0

As Austenite to martensite & martensite to austentie decomposition

0.9 0.8

Note: After partial transformation, decomposition begins at As.

0.6 0.5

600 Tensile Stress (MPa)

Martensite Volume Fraction

Stress = 0 0.7

0.4

400

200

0.3 0

0.2

77 150

Ms 200 Af

250

300

Temperature (K)

0.1 0.0

Af

MS 0

10

20

30

40

50

60

70

80

90

100

Temperature

Figure 7-22 Austenite to Martensite and Martensite to Austenite Decomposition

Main Index

406 Marc Volume A: Theory and User Information

Transformation Induced Deformation For the discussion of the thermo-mechanical response of NiTi, the data of Miyazaki et al. (1981) is shown in Figure 7-23. Following this thermal history, it is observed that, when unstrained specimens with fully austenitic microstructures are cooled, the transformation to martensite begins at a temperature of 190K; the transformation is complete at 128K. This established the so-called martensite start ( M s0 ) and martensite finish ( M f0 ) temperatures at 190K and 128K, respectively. With the imposition of an applied uniaxial tensile stress, the low temperature martensite is favored and the M s0 and M f0 temperatures increase. Upon heating a specimen with fully martensitic microstructure, the reverse transformation is observed to begin at a temperature of 188K and to be complete at 221K. These define the austenite start ( A s0 ) and austenite finish ( A f0 ) temperatures, respectively. Uniaxial tension tests are carried out in temperature ranges where T < M s , M s < T < A f , and A f < T < T c where T c is defined as the temperature above which the yield strength of the austenitic phase is lower than the stress required to induce the austenite-to-martensite transformation. (a) 77K

(b) 153K

(c) 164K

300 200 100

Tensile Stress (MPa)

0 400

0 (d) 224K

0 (e) 232K

(f) 241K

300 200 100 0

0

0

600 (g) 263K

(h) 273K

(i) 276K

400

200

0

Ms = 190K AF = 221K 2

4 0 2 4 Strain (%)

0

2

4

Figure 7-23 Thermal History

In the temperature range where T < M f , the microstructures are all martensitic. The stress versus strain curves display a smooth parabolic type of behavior which is consistent with deformation caused by the movement of defects such as twin boundaries and the boundaries between variants. Note that unloading occurs nearly elastically and that the accumulated deformation, caused by the reorientation of the existing martensite and the transformation of any pre-existing austenite, remains after the specimen is completely

Main Index

CHAPTER 7 407 Material Library

unloaded. Note also that the accumulated deformation is entirely due to oriented martensite and this would be recoverable upon heating to temperatures above the ( A s – A f ) range. This would, then, display the shape memory effect. Pseudoelastic behavior is displayed in the temperature range A f < T < T c . In this range, the initial microstructures are essentially all austenitic, and stress induced martensite is formed, along with the associated deformation; upon unloading, however, the martensite is unstable and reverts to austenite thereby undoing the accumulated deformation. Note that, as expected, the stress levels rise with increasing temperature. In this range, the transformation induced deformation is nearly all reversible upon unloading. At temperatures where T > T c , plastic deformation appears to precede the formation of stress induced martensite. The unloading part of the stress versus strain behavior displays nonlinearity and the unloading is now associated with permanent (plastic) deformation. Permanent deformation, due to plastic deformation of the martensite, is non-recoverable and, if such deformation is large, shape memory behavior is lost.

Constitutive Theory The model formulated below is based on the kinematics of small strains, although the extension to large strain is straightforward. Accordingly, the incremental strain, Δε , is simply the sum of the following contributions: Δε = Δε e l + Δε t h + Δε p l + Δε p h

(7-87)

In Equation (7-87), Δε e l is the incremental elastic, or lattice, strain rate; Δε t h is the incremental thermal strain, Δε p l is the incremental visco-plastic strain, and Δε p h is the incremental strain associated with thermoelastic phase transformations. The incremental elastic strain is taken to be simply related to a set of elastic moduli, L , and the incremental Cauchy stress rate, Δσ , as Δσ = LΔε e l

(7-88)

To calculate the coefficient of thermal expansion of the composite, the rule of mixtures is used as α = ( 1 – f )α A + fα M . In the above equations, the superscripts A and M refer to the austenite and martensite values, and f is the volume fraction of martensite.

Phase Transformation Strains As noted earlier, the phase transformation induced strains are a result of the formation of oriented, stress induced, martensite and the reorientation of randomly oriented thermally induced martensite. To account for this, Δε P h is expressed as

Main Index

408 Marc Volume A: Theory and User Information

Δε P h = Δε T R I P + Δε T W I N where 3 σ' Δε T R I P = Δf ( + ) g ( σ e q )ε eTq --- -------- + Δf ( + ) ε νT I + Δf ( - ) ε P h . 2 σe q

(7-89)

and 3σ' Δε T W I N = fΔg ( σ e q )ε eTq ------------ { σ e q } { σ e q – σ egf f } . 2σ e q

(7-90)

1 x+ x where Δf = Δf ( + ) + Δf ( - ) and { } represents McCauley’s bracket where { x } = --- ⎛⎝ ----------------⎞⎠ , 2 x x ≠ o. In Equation (7-89), Δf ( + ) represents the rate at which martensite is formed, ε eTq is the magnitude of the deviatoric part of the transformation, and ε νT is the volumetric part of the transformation strain. The function g ( σ e q ) is schematically depicted in Figure 7-24, and is a measure of the extent to which the martensite transformation strains are aligned with the deviatoric stress. σ e q is the equivalent stress defined as: 3 d --- σ : σ d where σ d is the deviatoric stress. 2

σe q = 1.1

0.9

g

0.7

0.5

0.3

0.1

-1.0

0.0

0.5

1.0 stress/g0

Figure 7-24 Function g ( σ e q )

Main Index

1.5

2.0

CHAPTER 7 409 Material Library

The first two terms in Equation (7-89) describe the development of transformation induced strains due to the formation of stress induced (partially oriented) martensite. Δf ( - ) is the change of formation of austenite; for example, the rate at which the volume fraction of martensite decreases. The last term in Equation (7-89), therefore, represents the recovery of the accumulated phase transformation strain. Note that there is no dilatational contribution to Δε T W I N since f is fixed. Note that the twinning strain rate is zero when σ e q is less than σ egf f , or when the magnitude of the stress change is negative ( Δσ e q < 0 ). Hence, σ egf f can be considered as a stress below which no twinning is possible. The function g represents the extent to which the transformation strains are coaxial with the applied deviatoric stress. This function can be calibrated with the experimental data. Note for uniaxial stressstrain curves performed below the martensite finish temperature, the material starts as 100% martensite, and that other than elastic strains, the deformation is dominated by the “twinning” of the randomly oriented martensite. A functional form that leads to sufficient fit to most experimental data has been implemented in Marc. σe q g ( σ e q ) = 1 – exp g a ⎛ --------⎞ ⎝ g0 ⎠

g

b

σe q + g c ⎛ --------⎞ ⎝ g0 ⎠

g

d

σe q + g e ⎛ --------⎞ ⎝ g0 ⎠

g

f

In most cases, the first term is sufficient, and a value of g a < 0 and g b = 2 yields the best results. g 0 is a stress level used to non-dimensionalize the constants, and can be chosen such that g → 1 when the σ e q → g 0 . In some cases, it is necessary to include the higher powers of equivalent stress for better experimental fits. In these, cases suggested values for g d = 2.55 or 2.75 and g e = 3 . However, depending on the values of g c and g e , this could lead to maxima or minima values of g in the range of interest. Note that 0 ≤ g ≤ 1 and it should be a monotonically increasing function (an increase in the stress level should lead to an increase in the increment of the phase strains). Thus, cut off values of g are provided in Marc, such that when g reaches its maximum value g = g m a x at the stress level g σe q = σm a x g 0 , it is held constant at the value g m a x . For the proper selection of g 0 , see the

following section.

Experimental Data Fitting for Thermo-mechanical Shape Memory Alloy The properties and transformation/retransformation behavior of Nititol depend upon alloy chemistry, microstructure and the thermal processing applied to the specimens and eventually to the components built from them. Every time any of the above change, it might be necessary to redo the calibration. Calibration of Nitinol experimental data works best if, in fact, all specimens can be initially rendered as 100% austenite. The list of properties that require calibration is given as follows:

Main Index

410 Marc Volume A: Theory and User Information

• The “unstressed transformation temperatures”, M s0 ,M f0 ,A s0 ,A f0 . • The coefficients C M , and C A that provide the stress dependence of the transformation temperatures. • The elastic constants ( E M ,E A ,v M and v A ). • Coefficients of thermal expansion, α M ,α A . • The calibration of the detwinning function, g ( σ e q ) that provides the description of the degree to which martensite is co-axial with the deviatoric stress state. M and σ A ), and their strain • The yield stress of the pure martensite and austenite phase ( σ Y Y

hardening properties. • The calibration of the transformation strains, ε eTq and ε vT . Transformation Temperatures and Their Stress Dependence ( M s0 ,M f0 ,A s0 ,A f0 ,C M , and C A ) For almost any use of shape memory alloy, it is highly desirable that one knows the Transformation Temperatures (TTRs) of the alloy. The TTRs are those temperatures at which the alloy changes from the higher temperature austenite to the lower temperature martensite or vice versa. There are in common use with NiTi alloys to provide helpful data to product designers – Constant Load, DSC and Active A f . The detail procedures to obtain TTRs using the above methods are shown in website (www.sma-inc.com). It is recommended that combined dilatometry and DSC tests be performed on unstressed specimens of thermally processed material to establish both the unstressed transformation temperatures and the thermal expansion coefficients. Those tests would provide a baseline set of values for M s0 ,M f0 ,A s0 , and A f0 . Note that the TTRs are stress dependent parameters, but it is difficult, in practice, to prepare totally unstressed samples. In order to determine the TTRs at zero stress, experimental data must be obtained at two or more stress levels. The particular transformation point of interest can then be extrapolated to zero stress. The estimations of TTRs, C M , and C A are shown in Figure 7-25. The typical range of TTRs is – 200 to 100°C. So, it is difficult to recommend the default values. As references, there are examples for two different SMA materials below. SMA 1) M s0 : – 50°C , M f0 : – 100°C , A s0 : 5°C , A f0 : 20°C , C M : 6.0Mpa/°C , C A : 8.0Mpa/°C SMA 2) M s0 : 190K , M f0 : 128K , A s0 : 188K , A f0 : 221K , C M : 5.33Mpa/K , C A : 6.25Mpa/K

Main Index

Stress

CHAPTER 7 411 Material Library

CM

M f0

M s0

CA

A s0 A f0 Temperature

Figure 7-25 Typical Stress vs. Temperature Curve Showing the Stress Dependence of Martensite and Austenite Start and Finish Temperature

Elastic Constants ( E M ,E A ,v M , and v A ) Literature estimates for the elastic moduli of martensite and austenite are typically in the range of E M = 28000-41000 Mpa , E A = 60000-83000Mpa , v M = v A = 0.33 . However, most experimental data appears to be significantly different than these. It is, therefore, suggested that estimates of these moduli should be made using actual experimental data for the materials being calibrated. Initial loading from a state corresponding to 100% austenite produces a linear elastic response from which E A can be readily estimated as in Figure 7-26. The modulus of martensite ( E M ) is also estimated for the unloading line, again as illustrated in Figure 7-26. In this figure, the loading should be performed to produce 100% martensite and thus the unloading occurs with the elastic response of martensite. Typical pseudoelastic response T = T1°C

Stress

EA

EM

Strain

Figure 7-26 Typical Stress-strain Curves in the Pseudo-elastic Regime, Depicting the Elastic Moduli

Thermal expansion coefficients ( α M ,α A ) A recommended method for measuring thermal expansion coefficients is through the use of dilatometry whereby carefully controlled cycles of temperature can be made. An alternative to this type of precise

Main Index

412 Marc Volume A: Theory and User Information

calibration, is to use literature values that have been shown to be consistent with values measured on actual specimens. These values are given as follows (See for example, TiNi Smart Sheet) α M = 6.6 × 10 – 6 ⁄ °C = 3.67 × 10 – 6 ⁄ °F ; and α A = 11.0 × 10 – 6 ⁄ °C = 6.11 × 10 – 6 ⁄ °F Detwinning and the calibration of the g function g ( σ e q ) The phenomenology of the NiTi phase transformation is such that the alignment of the martensite varies with the prevailing deviatoric stress. This intensity is measured via the von Mises equivalent stress, σ e q . As shown in Equations 7-89 and 7-90, the scaling function that provides the description of the degree to which the martensite is aligned is g ( σ e q ) . The most direct path to calibrating this g function is to fit it to the uniaxial stress vs. strain curve for pure, randomly oriented martensite conducted at a temperature below the M f0 temperature. Such a curve is shown as Figure 7-27. The solid curve shown in Figure 7-27 is the actual measured record of uniaxial stress vs. total strain for a specimen of 100% martensite tested at a temperature sufficiently low to ensure it remains 100% martensite. The dot curve is simply a convenient fit to it. The parameter ε eTq is the “equivalent deviatoric transformation strain”. Note that the function g is defined as it relates to the development of deviatoric strain due to the alignment of martensite variants. As mentioned in the previous section, in general, the variables g a < 0 , g b = 2f = 2.0 , g c ≥ 0 , g d = 2.25 and 2.75 , g e ≤ 0 and g f = 3.0 yield a good match to many experimental results. It is often observed that there exists a threshold equivalent stress level below which detwinning does not occur; this stress is referred to as σ egf f . The value of g at this stress is g e f f = g ( σ fgf ) . Note that from Equation (7-90), twinning strain is zero when σ e q < σ egf f . In addition, it is also found, in practice, that the function g tends to approach unity at a finite equivalent stress level, g

g

called σ 0 . By definition, g ( σ 0 ) = 1 . Also, g a should be chosen to match the general shape of the function. Since the ratio σ e q ⁄ g 0 is less than one, the higher powers take effect later, and thus g c can be added to lower the middle slope of the curve and g e to fix the final slope of the curve. However, depending on the relative values of g a , g b and g c , this curve might reach a maximum in the range of interest, and therefore, it should be cut-off at its maximum value g m a x . The value of g m a x which is g reach at a stress value σ e q ⁄ g 0 = σ m a x are also supplied as an input to Marc. Usually g

g

g 0 = 2σ e f f ∼ 10σ e ff is a good approximation. But, the selection of g 0 depends on the experimental measurement.

Main Index

CHAPTER 7 413 Material Library

ε T W I N = g ( σ e q )ε eTq

Experimental Model

Stress

g0

g0 Strain

Figure 7-27 Typical Stress-Strain Curve of 100% Martensite Tested Below M f0 Temperature

Others M A. Yield stresses of the pure martensite and austenite phases for NiTi: σ Y and σ Y M σY = 70-140 Mpa A σY = 195 – 690 Mpa

The calibration of the transformation strains for NiTi: ε eTq

(deviatoric transformation strain): 0.05-0.085

ε vT

(volumetric transformation strain): 0 – 0.003.

σ egf f

(detwinning stress): 100-150 Mpa

g0

2σ e f f ∼ 10σ egf f

Note:

g

The current model uses a nonsymmetric Jacobian matrix. It is recommended that the nonsymmetric solver be used to improve convergence.

Mechanical Shape Memory Model Shape-memory alloys can undergo reversible changes in the crystallographic symmetry-point-group. Such changes can be interpreted as martensitic phase transformations, that is, as solid-solid diffusionless phase transformations between a crystallographically more-ordered phase (the austenite or parent phase) and a crystallographically less-ordered phase (the martensite). Typically, the austenite is stable at high temperatures and high values of the stress. For a stress-free state, we indicate with the temperature

Main Index

414 Marc Volume A: Theory and User Information

above which only the austenite is stable and with the temperature below which only the martensite is stable. The phase transformations between austenite and martensite are the key to explain the superelasticity effect. For the simple case of uniaxial tensile stress, a brief explanation follows (Figure 7-28). Consider a specimen in the austenitic state and at a temperature greater than A; accordingly, only the austenite is stable at zero stress. If the specimen is loaded, while keeping the temperature constant, the material presents a nonlinear behavior (ABC) due to stress-induced conversion of austenite into martensite. Upon unloading, while again keeping the temperature constant, a reverse transformation from martensite to austenite occurs (CDA) as a result of the instability of the martensite at zero stress. At the end of the loading/unloading process, no permanent strains are present and the stress-strain path is a closed hysteresis loop. C

σ B D A

ε

Figure 7-28 Superelasticity

At the crystallographic level, if there is no preferred direction for the occurrence of the transformation, the martensite takes advantage of the existence of different possible habit plates (the contact plane between the austenite and the martensite during a single-crystal transformation), forming a series of crystallographically equivalent variants. The product phase is then termed multiple-variant martensite and it is characterized by a twinned structure. However, if there is a preferred direction for the occurrence of the transformation (often associated with a state of stress), all the martensite crystals trend to be formed on the most favorable habit plane. The product is then termed single-variant martensite and is characterized by a detwinned structure. According to the existence of different types of single-variant martensite species, the conversion of each single-variant martensite into different single variants is possible. Such a process, known as a reorientation process, can be interpreted as a family of martensite phase transformations and is associated with changes in the parameters governing the single-variant martensite production (hence, it is often associated to nonproportional change of stress). In addition to the thermo-mechanical shape memory model, a superelastic shape memory alloy model is also implemented in Marc based on the work of Auricchio [Ref. 1] and [Ref. 2]. This work has been enhanced to allow different elastic properties for the Austenite and Martensite phases. The superelastic shape memory model has been implemented in Marc in the framework of multiplicative decomposition. We assume the deformation gradient, F as the control variable, and the martensite fraction, ξ S as the only scalar internal variable. We also introduce a multiplicative decomposition of F in the form: F = Fe Ft r where F e is the elastic part and F t r is the phase transition part.

Main Index

CHAPTER 7 415 Material Library

Assuming an isotropic elastic response, the Kirchhoff stress τ and the elastic left Cauchy-Green tensor b e , defined as: b e = F e F e T , share the same principal directions. Accordingly, the following spectral decompositions can be introduced: 3

τ =

∑

τA nA ⊗ nB

A = 1 3

d =

∑

d

σA n A ⊗ n B

A = 1 3

∑

be =

e )2nA ⊗ nB ( λA

A = 1 e the elastic principal stretches and σ d the deviatoric part, according to the relation: with λ A

τ = pI + σ d

(7-91)

where I is the second-order identity tensor, p is the pressure, defined as p = tr ( τ ) ⁄ 3 , and tr ( . ) is the trace operator. We can write Equation (7-91) with the following component form: d

τA = p + σ A

(7-92)

with d

e . p = Kθ e , σ A = 2Ge A

Phase Transformations and Activation Conditions We consider two phase transformations: the conversion of austenite into martensite (A→ S) and the conversion of martensite into austenite (S→ A). To model the possible phase-transformation pressuredependence, we introduce a Drucker-Prager-type loading function: F( τ) =

σ d + 3αp

(7-93)

where α is a material parameter and σd

3

=

∑

d 2

( σA )

.

indicates the Euclidean norm, such that:

1⁄2

.

A = 1

Indicating variants in time with a superposed dot, we assume the following linear forms for the evolution of ξ S :

Main Index

416 Marc Volume A: Theory and User Information

· · F ξ S = H A S ( 1 – ξ S ) --------------------F – R fA S

for (A→ S)

(7-94)

· · F S A ξ S = H ξ S --------------------F – R fS A

for (S→ A)

(7-95)

where 2 σ fAS ⎛ --- + α⎞ , R fS A = ⎝ 3 ⎠

R fA S =

2 σ fSA ⎛ --- + α⎞ ⎝ 3 ⎠

with σ sA S , σ fA S , σ sS A , and σ fS A material constants. The scalar quantities H AS and H

SA

embed the

plastic-transformation activation condition – hence, allowing a choice between Equations (7-94) and (7-95) – and they are defined by the relations: H AS = 1 , if R sA S < F < R fA S , or F· > 0 . Otherwise, H AS = 0 . H SA = 1 , if R fS A < F < R sS A , or F· < 0 . Otherwise, H SA = 0 . where 2 σ sAS ⎛ --- + α⎞ , R sS A = ⎝ 3 ⎠

R sA S =

2 σ sSA ⎛ --- + α⎞ . ⎝ 3 ⎠

Time-discrete Model The time-discrete model is obtained by integrating the time-continuous model over the time interval [ t n, t ]. In particular, we use a backward-Euler integration formula for the rate-equations evaluating all the nonrate equations at time t . Written in residual form and clearing fraction from Equations (7-94) and (7-95), the time-discrete evolutionary equations specialize to: R A S = ( F – R fAS )λ s – H A S ( 1 – ξ S ) ( F – F n ) = 0

(7-96)

R S A = ( F – R fSA )λ s – H S A ξ S ( F – F n ) = 0

(7-97)

where t

λS =

·

∫ ξ dt t

= ξ S – ξ S ,n

(7-98)

n

The quantity λ S in Equation (7-98) can be computed expressing F as a function of λ S and requiring the satisfaction of the discrete equation relative to the corresponding active phase transition.

Main Index

CHAPTER 7 417 Material Library

The detailed solution algorithm for stress update and consistent tangent modulus are given in the work of Auricchio [Ref. 2]. In the enhanced version of this model, the user enters different elastic constants for the two phases. In this case, the effective elastic moduli are taken as: A

M

E = E ( 1 – ξS ) + E ξS A

M

ν = ν ( 1 – ξS ) + ν ξS

Experimental Data Fitting for Mechanical Shape Memory Alloy The experiment for mechanical shape memory alloy is quite simple. 1. To determine the transformation stresses ( σ SA S ,σ fAS ,σ SS A ,σ fS A ): σ SA S

Initial Stress for Austenite to Martensite

σ fA S

Final Stress for Austenite to Martensite

σ SS A

Initial Stress for Martensite to Austenite

σ fS A

Initial Stress for Martensite to Austenite

Uniaxial tension test is performed at the same temperature at which the simulation is desired. Here is one example set for SMA materials. σ SA S = 500Mpa , σ fA S = 600Mpa , σ SA S = 300Mpa , σ fS A = 200Mpa 2. α :It is measured from the difference between the response in tension and compression. Case 1) if the behavior in tension and compression are the same, the value is set to 0. Case 2) if the behavior in tension and compression have a difference as in the classical case of SMA, the value is usually set to 0.1 if there is no compression data for the phase transformation. One value for the phase transformation in compression, say σ sA S– (sigAS_s_compression) is available, α is calculated as follows: α = sqrt ( 2 ⁄ 3 ) ( σ SA S, – – σ SAS ) ⁄ ( σ SA S, – + σ SA S ) 3. ε L : epsL is a scalar parameter representing the maximum deformation obtainable only by detwinning of the multiple-variant martensite (or maximum strain obtainable by variant orientation). Classical values for epsL are in the range 0.005 and 0.10. Marc sets the default value as 0.07.

Main Index

418 Marc Volume A: Theory and User Information

Note:

The mechanical shape memory model only supports ndi = 3 case (3-D, plane-strain and axisymmetric elements). It does not support either ndi = 1 or ndi = 2 cases (1-D and plane-stress elements).

Conversion from Thermo-Mechanical to Mechanical SMA Table 7-2

Conversion Table

Thermo-Mechanical SMA

E = 0.5 ( E A + E M )

E

A

ν = 0.5 ( ν A + ν M )

ν

M

E = 0.5 ( E A + E M )

E

M

ν = 0.5υ ( ν A + ν M )

ν

εe q

T

3 T ε L = sqrt ⎛ ---⎞ ε e q ⎝ 2⎠

3 T ε L = sqrt ⎛ ---⎞ ε e q ⎝ 2⎠

CM

CM

CM

CA

CA

CA

To

To

To

ν E ν

Prediction from Linear Algebra

The Relationship between Mechanical Model and Thermo-Mechanical Model AS

= ( T o – M s )C m

AS

= ( T o – M f )C m

σs σf

0

0

0

σ sS A = ( T o – A s )C a 0

σ fS A = ( T o – A f )C a

Main Index

Enhanced Mechanical SMA

A

E

Table 7-3

Mechanical SMA

A A

M M

CHAPTER 7 419 Material Library

σ

AS

σf

AS

σs

CA

SA

σs

SA

σf

CM Mf

Ms

As Af To

T

Elastomer An elastomer is a polymer which shows nonlinear elastic stress-strain behavior. The term elastomer is often used to refer to materials which show a rubber-like behavior, even though no rubbers exist which show a purely elastic behavior. Depending upon the type of rubber, elastomers show a more or less strongly pronounced viscoelastic behavior. Marc considers both the viscous effects and the elastic aspects of the materials behavior. These materials are characterized by their elastic strain energy function.

σ, Stress

Elastomeric materials are elastic in the classical sense. Upon unloading, the stress-strain curve is retraced and there is no permanent deformation. Elastomeric materials are initially isotropic. Figure 7-29 shows a typical stress-strain curve for an elastomeric material.

100% e, Strain Figure 7-29 A Typical Stress-Strain Curve for an Elastomeric Material

Calculations of stresses in an elastomeric material requires an existence of a strain energy function which is usually defined in terms of invariants or stretch ratios. Significance and calculation of these kinematic quantities is discussed next. In the rectangular block in Figure 7-30, λ 1 , λ 2 , and λ 3 are the principal stretch ratios along the edges of the block defined by

Main Index

420 Marc Volume A: Theory and User Information

λi = ( Li + ui ) ⁄ Li

(7-99)

L3

λ3L3

Undeformed λ2L2

λ1L1

Deformed

L2 L1

Figure 7-30 Rectangular Rubber Block

In practice, the material behavior is (approximately) incompressible, leading to the constraint equation λ1 λ2 λ3 = 1

(7-100)

the strain invariants are defined as 2 2 2 1 2 2 2 2 λ1 λ + λ λ 2 2 3 2 2 2 λ1 λ2 λ3

I1 = λ + λ2 + λ3 I2 = I3 =

2 2 3 1

+λ λ

(7-101)

Depending on the choice of configurations, for example, reference (at t = 0 ) or current ( t = n + 1 ), you obtain total or updated Lagrange formulations for elasticity. The kinematic measures for the two formulations are discussed next. A. Total Lagrangian Formulation The strain measure is the Green-Lagrange strain defined as: 1 E i j = --- ( C i j – δ i j ) 2

(7-102)

where C i j is the right Cauchy-Green deformation tensor defined as: Ci j = Fk i Fk j

(7-103)

in which F kj is the deformation gradient (a two-point tensor) written as: ∂x k F kj = --------∂X j

Main Index

(7-104)

CHAPTER 7 421 Material Library

7

The Jacobian J is defined as: J = λ 1 λ 2 λ 3 = ( det C i j )

Material Library

1 --2

(7-105)

Thus, the invariants can be written as: I1 = Ci i

(implied sum on i) 2

( Ci j Ci j – ( Ci i ) ) I 2 = -----------------------------------------2 1 I 3 = --- e i j k e p q r C i p C j q C k r = det ( C i j ) 6

(7-106)

in which e i j k is the permutation tensor. Also, using spectral decomposition theorem, 2

A

A

Ci j = λA Ni Nj

(7-107) 2

in which the stretches λ A are the eigenvalues of the right Cauchy-Green deformation tensor, C i j A

and the eigenvectors are N i . B. Updated Lagrange Formulation The strain measure is the true or logarithmic measure defined as: 1 ε i j = --- l n b i j 2

(7-108)

where the left Cauchy-Green or finger tensor b i j is defined as: bi j = F i k Fj k

(7-109)

Thus, using the spectral decomposition theorem, the true strains are written as: 3

εi j =

∑

A

A

ln ( λ A ) n i n j

(7-110)

A = 1 A n i is

where the eigenvectors in the current configuration. It is noted that the true strains can also be approximated using first Padé approximation, which is a rational expansion of the tensor, as: εi j = 2 ( V i j – δ i j ) ( Vi j + δi j )

–1

(7-111)

where a polar decomposition of the deformation gradient F i j is done into the left stretch tensor V i j and rotation tensor R i j as:

Main Index

422 Marc Volume A: Theory and User Information

Fi j = V i k Rk j

(7-112)

The Jacobian J is defined as: J = λ 1 λ 2 λ 3 = ( det b i j )

1 --2

(7-113)

and the invariants are now defined as: I1 = b i i

and

2 1 I 2 = --- ( b i j b i j – ( b i i ) ) 2 1 I 3 = --- e i j k e p q r b i p b j q b k r = det ( b i j ) 6

(7-114)

It is noted that either Equation (7-106) or Equation (7-114) gives the same strain energy since it is scalar and invariant. Also, to account for the incompressibility condition, in both formulations, the strain energy is split into deviatoric and volumetric parts as: (7-115)

W = W deviatoric + W volumetric

Thus, the generalized Mooney-Rivlin (gmr) and the Ogden models for nearly-incompressible elastomeric materials are written as: gmr Wd e v i a t o r i c

=

N

N

∑

∑

m

Cm n ( I 1 – 3 ) ( I2 – 3 )

n

(7-116)

m = 1 n = 1

where I 1 and I 2 are the first and second deviatoric invariants. A particular form of the generalized Mooney-Rivlin model, namely the third order deformation (tod) model, is implemented in Marc. tod

W devratoric = 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

(7-117)

where tod

W deviatoric

is the deviatoric third order deformation form strain energy function,

C 10, C 01, C 11, C 20, C 30

are material constants obtained from experimental data

Simpler and popular forms of the above strain energy function are obtained as: nh

W deviatoric = C 10 ( I 1 – 3 ) mr

W deviatoric = C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 )

Main Index

Neo-Hookean Mooney-Rivlin

(7-118)

CHAPTER 7 423 Material Library

Use the MOONEY model definition option to activate the elastomeric material option in Marc and enter the material constants C 10, C 01, C 11, C 20, C 30 . The TEMPERATURE EFFECTS model definition option can be used to input the temperature dependency of the constants C 10 and C 01 . The UMOONY user subroutine can be used to modify all five constants C 01 , C 10 , C 11 , C 20 , and C 30 . Using the table driven input, all material parameters can reference tables to define temperature dependent behavior. For viscoelastic, the additional VISCELMOON model definition option must be included. The form of strain energy for the Ogden model in Marc is, N ogden Wd e v i a t o r i c

=

∑ k = 1

α

where λ i

k

=

αk αk αk μk ------ ⎛⎝ λ 1 + λ 2 + λ 3 – 3⎞⎠ αk

αk – ------- α k 3 J λi

(7-119)

are the deviatoric stretch ratios while C m n , μ k , and α k are the

material constants obtained from the curve fitting of experimental data. This capability is available in Marc Mentat. If no bulk modulus is given, it is taken to be virtually incompressible. This model is different from the Mooney model in several respects. The Mooney material model is with respect to the invariants of the right or left Cauchy-Green strain tensor and implicitly assumes that the material is incompressible. The Ogden formulation is with respect to the eigenvalues of the right or left Cauchy-Green strain, and the presence of the bulk modulus implies some compressibility. Using a two-term series results in identical behavior as the Mooney mode if: μ 1 = 2C 10 and α 1 = 2 and μ 2 = – 2C 01 and α 2 = – 2 The material data is given through the OGDEN model definition option or the UOGDEN user subroutine. For viscoelastic behavior, the additional VISCELOGDEN model definition option must be included. In the Arruda-Boyce strain energy model, the underlying molecular structure of elastomer is represented by an eight-chain model to simulate the non-Gaussian behavior of individual chains in the network. The two parameters, nkΘ and N ( n is the chain density, k is the Boltzmann constant, Θ is the temperature, and N is the number of statistical links of length l in the chain between chemical crosslinks) representing initial modules and limiting chain extensibility and are related to the molecular chain orientation thus representing the physics of network deformation. As evident in most models describing rubber deformation, the strain energy function constructed by fitting experiment data obtained from one state of deformation to another fails to accurately describe that deformation mode. The Arruda-Boyce model ameliorates this defect and is unique since the standard tensile test data provides sufficient accuracy for multiple modes of deformation. The model is constructed using the eight chain network as follows [Ref. 3]:

Main Index

424 Marc Volume A: Theory and User Information

Consider a cube of dimension α 0 with an unstretched network including eight chains of length r0 =

Nl , where the fully extended chain has an approximate length of Nl. A chain vector from the

center of the cube to a corner can be expressed as: α0 α0 α0 C 1 = ------ λ 1 i + ------ λ 2 j + ------ λ 3 k 2 2 2

(7-120)

Using geometrical considerations, the chain vector length can be written as: 1⁄2 1 r chain = ------- Nl ( λ 12 + λ 22 + λ 32 ) 3

(7-121)

and r chain 1⁄2 1 λ chain = ------------ = ------- ( I 1 ) r0 3

(7-122)

j

λ2 α0

C1 i λ3 α0

k

λ1 α0

Figure 7-31 Eight Chain Network in Stretched Configuration

Using statistical mechanics considerations, the work of deformation is proportional to the entropy change on stretching the chains from the unstretched state and may be written in terms of the chain length as: r chain β W = nkΘN ⎛ ------------ β + ln -------------- ⎞ – ΘCˆ ⎝ Nl sinh β ⎠

(7-123)

where n is the chain density and Cˆ is a constant. β is an inverse Langevin function correctly accounts for the limiting chain extensibility and is defined as: r chain β = L – 1 ⎛ ------------⎞ ⎝ Nl ⎠

Main Index

(7-124)

CHAPTER 7 425 Material Library

where Langevin is defined as: 1 ℑ ( β ) = coth β – --β

(7-125)

With Equations (7-122) through (7-125), the Arruda-Boyce model can be written Arruda-Boyce

W dev

1 1 11 = nkΘ --- ( I 1 – 3 ) + ---------- ( I 12 – 9 ) + ------------------- ( I 13 – 27 ) 2 2 20N 1050N 19 519 + ------------------- ( I 14 – 81 ) + ------------------------- ( I 15 – 243 ) ] 3 4 7000N 673750N

(7-126)

Also, using the notion of limiting chain extensibility, Gent [Ref. 5] proposed the following constitutive relation: Gent

W dev

– EI m I 1* ⎞ ⎛ = ------------- log ⎜ 1 – ------⎟ I m⎠ 6 ⎝

(7-127)

where I 1* = I 1 – 3

(7-128)

The constant EI m is independent of molecular length and, hence, of degree of cross linking. The model is attractive due to its simplicity, but yet captures the main behavior of a network of extensible molecules over the entire range of possible strains. The Arruda-Boyce and Gent model can be invoked by using the ARRUDBOYCE and GENT model definition options, respectively. The volumetric part of the strain energy is for all the rubber models in Marc: 1

W volumetric

--⎞ 9K ⎛ 3 = ------- ⎜ J – 1⎟ 2 ⎝ ⎠

2

(7-129)

when K is the bulk modulus. It can be noted that the particular form of volumetric strain energy is chosen such that: 1. The constraint condition is satisfied for incompressible deformations only; for example: ⎧ ⎪ > 0 if I 3 > 0 ⎪ f ( I 3 ) ⎨ = 0 if I 3 = 1 ⎪ ⎪ < 0 if I 3 < 0 ⎩

Main Index

(7-130)

426 Marc Volume A: Theory and User Information

2. The constraint condition does not contribute to the dilatational stiffness. This yields the constraint function as: 1

⎛ --6⎞ f ( I 3 ) = 3 ⎜ I – 1⎟ 3 ⎝ ⎠

(7-131)

upon substitution of Equation (7-133) in Equation (7-129) and taking the first variation of the variational principle, you obtain the pressure variable as: 1

⎛ --3⎞ p = 3K ⎜ J – 1⎟ ⎝ ⎠

(7-132)

The equation has a physical significance in that for small deformations, the pressure is linearly related to the volumetric strains by the bulk modulus K . The discontinuous or continuous damage models discussed in the models section on damage can be included with the generalized Mooney-Rivlin, Ogden, Arruda-Boyce, and Gent models to simulate Mullins effect or fatigue of elastomers when using the updated Lagrangian approach. In the total Lagrangian framework however, this is available for the Ogden model only. The rubber foam model which is based on Ogden formulation has a strain energy form as follows: N

W =

∑ n = 1

μn α α α ------ ( λ 1 n + λ 2 n + λ 3 n – 3 ) + αn

N

∑ n = 1

βn μn ------ ⎛⎝ 1 – J ⎞⎠ βn

(7-133)

where μ n , α n , β n are material constants. The model reduces to incompressible Ogden model when β n equals zero. You can define any other invariant based models through the use of the UENERG user subroutine when using the MOONEY option in model definition for elasticity in total or Updated Lagrangian framework. A more general and easy-to-use the UELASTOMER user subroutine (uelastomer.f) can be used to define a general strain energy function in the Updated Lagrangian framework. Once the strain energy function is defined, the stresses and material tangent can be evaluated for the total and Updated Lagrangian formulations as: A. Total Lagrangian Formulation: The stress measure in the total Lagrangian formulation is the symmetric second Piola-Kirchhoff stress S i j , calculated as: ∂W ∂W S i j = ---------- = 2 ---------∂E i j ∂C i j

(7-134)

The material elasticity tangent is: 2

2

∂ W ∂ W D i j k l = ---------------------- = 4 ----------------------∂E i j ∂E k l ∂C i j ∂C k l

Main Index

(7-135)

CHAPTER 7 427 Material Library

B. Updated Lagrangian Formulation: The stress measure in the Updated Lagrangian formulation is the Cauchy or true stress calculated as: 2 ∂W σ i j = --- ---------- b k j J ∂b i k

(7-136)

The spatial elasticity tangent is: 2

4 ∂ W L i j k l = --- b i m ------------------------ b n l J ∂b m j ∂b k n

(7-137)

The material constants for the Mooney-Rivlin form can be obtained from experimental data. The Mooney-Rivlin form of the strain energy density function is mooney-rivlin

W deviatoric

= C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 )

(7-138)

For the Mooney-Rivlin model, the force and deformation for a uniaxial test specimen can be related as 1 P = 2A 0 ⎛ 1 – ------⎞ ( λ 1 C 10 + C 01 ) ⎝ 3⎠ λ1

(7-139)

which can be written in the form: C 01 P ------------------------------------ = C 10 + --------1 λ1 2A 0 ⎛ λ 1 – ------⎞ ⎝ 2⎠ λ1

(7-140)

where P is the force of the specimen, A 0 is the original area of the specimen, and λ 1 is the uniaxial stretch ratio. This equation provides a simple way to determine the Mooney-Rivlin constants. The 1 Mooney-Rivlin constitutive equation is applicable if the plot of P ⁄ 2A 0 ⎛ λ 1 – ------⎞ ⎝ 2⎠ λ1

1 versus ----λ1

1 should yield a straight line of slope C 01 and intercept ( C 01 + C 10 ) on the vertical axis ----- = 1 as λ1 shown in Figure 7-32.

Main Index

428 Marc Volume A: Theory and User Information

0.4 G

σ/2(λ-1/λ2) (N/mn2)

F 0.3 E D C A 0.2 B

0.1 0.5

0.6

0.8

0.7

0.9

1.0

1/λ

Figure 7-32 Plots for Various Rubbers in Simple Extension for Mooney-Rivlin Model

If only the Young’s modulus E is supplied, and full uniaxial data are not available then C 01 ≅ 0.25C 10

(7-141)

is a reasonable assumption. The constants then follow from the relation: 6 ( C 10 + C 01 ) ≅ E

(7-142)

The material coefficients for the models can be obtained from Marc Mentat. This allows you to select which model is most appropriate for your data.

Updated Lagrange Formulation for Nonlinear Elasticity The total Lagrange nonlinear elasticity models in Marc have been augmented with a formulation in an Updated Lagrange framework. Hence, Rezoning can be used for elastomeric materials based upon the current configuration. This is specially useful in large deformation analysis since typically excessive element distortion in elastomeric materials can lead to premature termination of analysis. The new formulation accommodates the generalized Mooney-Rivlin and Ogden material models preserving the same format and strain energy functions as the total Lagrange formulation. In addition, the Arruda-Boyce and the Gent models are only available in the updated Lagrange framework. The updated Lagrangian rubber elasticity capability can be used in conjunction with both continuous as well as discontinuous damage models. Thermal, as well as viscoelastic, effects can be modeled with the current formulation. Using the table driven input, all of the material properties can reference tables, which facilitates the use of temperature dependent material properties. The singularity ratio of the system is inversely proportional to the order of bulk modulus of the material due to the condensation procedure.

Main Index

CHAPTER 7 429 Material Library

A consistent linearization has been carried out to obtain the tangent modulus. The singularity for the case of two- or three-equal stretch ratios is analytically removed by application of L’Hospital’s rule. The current framework with an exact implementation of the finite strain kinematics along with the split of strain energy to handle compressible and nearly incompressible response is eminently suitable for implementation of any nonlinear elastic as well as inelastic material models. In fact, the finite e θ p

deformation plasticity model based on the multiplicative decomposition, F = F F F is implemented in the same framework. To simulate elastomeric materials, incompressible element(s) are used for plane strain, axisymmetric, and three-dimensional problems for elasticity in total Lagrangian framework. These elements can be used with each other or in combination with other elements in the library. For plane stress, beam, plate or shell analysis, conventional elements can be used. For updated Lagrangian elasticity, both conventional elements (as well as Herrmann elements) can be used for plane strain, axisymmetric, and three-dimensional problems.

Time-independent Inelastic Behavior In uniaxial tension tests of most metals (and many other materials), the following phenomena can be observed. If the stress in the specimen is below the yield stress of the material, the material behaves elastically and the stress in the specimen is proportional to the strain. If the stress in the specimen is greater than the yield stress, the material no longer exhibits elastic behavior, and the stress-strain relationship becomes nonlinear. Figure 7-33 shows a typical uniaxial stress-strain curve. Both the elastic and inelastic regions are indicated.

Stress

Inelastic Region

Yield Stress Strain Elastic Region Note: Stress and strain are total quantities. Figure 7-33 Typical Uniaxial Stress-Strain Curve (Uniaxial Test)

Within the elastic region, the stress-strain relationship is unique. As illustrated in Figure 7-34, if the stress in the specimen is increased (loading) from zero (point 0) to σ 1 (point 1), and then decreased (unloading) to zero, the strain in the specimen is also increased from zero to ε 1 , and then returned to zero. The elastic strain is completely recovered upon the release of stress in the specimen.

Main Index

430 Marc Volume A: Theory and User Information

The loading-unloading situation in the inelastic region is different from the elastic behavior. If the specimen is loaded beyond yield to point 2, where the stress in the specimen is σ 2 and the total strain is e 2

ε 2 , upon release of the stress in the specimen the elastic strain, ε , is completely recovered. However, p

the inelastic (plastic) strain, ε 2 , remains in the specimen. Figure 7-34 illustrates this relationship. Total Strain = Strain and Elastic Strain

Stress

σ3 σ2

3

p

Δε 3

2

Yield Stress σ y

σ1 0

1

ε1 ε

ε2 p 2

ε3

p 3

p

e

p

e

ε2 = ε2 + ε2

ε 2e ε

Strain

ε3 = ε3 + ε3 ε

e 3

Figure 7-34 Schematic of Simple Loading - Unloading (Uniaxial Test)

Similarly, if the specimen is loaded to point 3 and then unloaded to zero stress state, the plastic strain p

p 2

p 3

ε 3 remains in the specimen. It is obvious that ε is not equal to ε . We can conclude that in the inelastic region: • Plastic strain permanently remains in the specimen upon removal of stress. • The amount of plastic strain remaining in the specimen is dependent upon the stress level at which the unloading starts (path-dependent behavior). The uniaxial stress-strain curve is usually plotted for total quantities (total stress versus total strain). The total stress-strain curve shown in Figure 7-33 can be replotted as a total stress versus plastic strain curve, as shown in Figure 7-35. The slope of the total stress versus plastic strain curve is defined as the workhardening slope (H) of the material. The workhardening slope is a function of plastic strain.

Main Index

CHAPTER 7 431 Material Library

Total Stress σ

θ

Plastic Strain εp H = tan θ (Workhardening Slope) = dσ/dεp Figure 7-35 Definition of Workhardening Slope (Uniaxial Test)

The stress-strain curve shown in Figure 7-33 is directly plotted from experimental data. It can be simplified for the purpose of numerical modeling. A few simplifications are shown in Figure 7-36 and are listed below: 1. 2. 3. 4. 5.

Bilinear representation – constant workhardening slope Elastic perfectly-plastic material – no workhardening Perfectly-plastic material – no workhardening and no elastic response Piecewise linear representation – multiple constant workhardening slopes Strain-softening material – negative workhardening slope

In addition to elastic material constants (Young’s modulus and Poisson’s ratio), it is essential to include yield stress and workhardening slopes when dealing with inelastic (plastic) material behavior. These quantities can vary with parameters such as temperature and strain rate. Since the yield stress is generally measured from uniaxial tests, and the stresses in real structures are usually multiaxial, the yield condition of a multiaxial stress state must be considered. The conditions of subsequent yield (workhardening rules) must also be studied. σ

σ

ε

ε

(1) Bilinear Representation

(2) Elastic-Perfectly Plastic

σ

σ

ε

ε

(4) Piecewise Linear Representation

(3) Perfectly Plastic

σ

ε (5) Strain Softening

Figure 7-36 Simplified Stress-Strain Curves (Uniaxial Test)

Main Index

432 Marc Volume A: Theory and User Information

Yield Conditions The yield stress of a material is a measured stress level that separates the elastic and inelastic behavior of the material. The magnitude of the yield stress is generally obtained from a uniaxial test. However, the stresses in a structure are usually multiaxial. A measurement of yielding for the multiaxial state of stress is called the yield condition. Depending on how the multiaxial state of stress is represented, there can be many forms of yield conditions. For example, the yield condition can be dependent on all stress components, on shear components only, or on hydrostatic stress. A number of yield conditions are available in Marc, and are discussed in this section. von Mises Yield Condition Although many forms of yield conditions are available, the von Mises criterion is the most widely used. The success of the von Mises criterion is due to the continuous nature of the function that defines this criterion and its agreement with observed behavior for the commonly encountered ductile materials. The von Mises criterion states that yield occurs when the effective (or equivalent) stress (σ) equals the yield stress (σy) as measured in a uniaxial test. Figure 7-37 shows the von Mises yield surface in twodimensional and three-dimensional stress space. For an isotropic material: σ = [ ( σ1 – σ2 ) 2 + ( σ2 – σ3 ) 2 + ( σ3 – σ1 ) 2 ] 1 ⁄ 2 ⁄

(7-143)

2

where σ1, σ2, and σ3 are the principal Cauchy stresses. d

σ3

σ2 Yield Surface

Yield Surface Elastic Region

σ1 Elastic Region (a) Two-dimensional Stress Space

d

d

σ1

σ2 (b) p-Plane

Figure 7-37 von Mises Yield Surface

σ can also be expressed in terms of nonprincipal Cauchy stresses. ( σ = [ ( σ x – σ y ) 2 + ( σ y – σ z ) 2 + ( σ z – σ x ) 2 + 6 ( τ x2y + τ y2z + τ z2x ) ] 1 ⁄ 2 ) ⁄

2

(7-144)

The yield condition can also be expressed in terms of the deviatoric stresses as: σ =

Main Index

3 d d --- σ i j σ i j 2

(7-145)

CHAPTER 7 433 Material Library

d

where σ i j is the deviatoric Cauchy stress expressed as 1 d σ i j = σ i j – --- σ k k δ i j 3

(7-146)

For isotropic material, the von Mises yield condition is the default condition in Marc. The initial yield stress σ y is defined in the ISOTROPIC and ORTHOTROPIC options. A user-defined finite strain, isotropic plasticity material model can be implemented through the UFINITE user subroutine. In this case, the finite strain kinematics is taken care of in Marc. You have to do the small strain return mapping only. See Marc Volume D: User Subroutines and Special Routines for more details. Hill’s [1948] Yield Function The anisotropic yield function (of Hill) and stress potential are assumed as 2

σ = [ a 1 ( σ y – σ z ) 2 + a 2 ( σ z – σ x ) 2 + a 3 ( σ x – σ y ) 2 + 3a 4 τ z x + +

3a 5 τ y2z

+

2 1⁄2 3a 6 τ x y ]

⁄

(7-147)

2

where σ is the equivalent tensile yield stress for isotropic behavior. Ratios of actual to isotropic yield (in the preferred orientation) are defined in the array YRDIR for direct tension yielding, and in YRSHR for yield in a shear (the ratio of actual shear yield to σ ⁄ shear yield). Then the a 1 above are defined by:

Main Index

3 isotropic

1 1 1 a 1 = --------------------------------------- + --------------------------------------- – --------------------------------------YRDIR ( 2 )**2 YRDIR ( 3 )**2 YRDIR ( 1 )**2

(7-148)

1 1 1 a 2 = --------------------------------------- + --------------------------------------- – --------------------------------------YRDIR ( 3 )**2 YRDIR ( 1 )**2 YRDIR ( 2 )**2

(7-149)

1 1 1 a 3 = --------------------------------------- + -------------------------------------- – -------------------------------------YRDIR ( 1 )**2 YRDIR ( 2 )**2 YRDIR ( 3 )**2

(7-150)

2 a 4 = ---------------------------------------YRSHR ( 3 )**2

(7-151)

2 a 5 = --------------------------------------YRSHR ( 2 )**2

(7-152)

2 a 6 = ---------------------------------------YRSHR ( 1 )**2

(7-153)

434 Marc Volume A: Theory and User Information

For anisotropic material, use the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition options to indicate the anisotropy. Use the ORTHOTROPIC option or the ANPLAS user subroutine for the specification of anisotropic yield condition (constants a1 through a6, as defined above), and the ORIENTATION model definition option or the ORIENT user subroutine, if necessary, to specify preferred orientations. Hill’s (1948) Yield Criterion has been extensively used in sheet metal forming, especially for steel. The experimental data can be related to the Marc input for the Hill’s Yield Criterion for the shells or plane stress case as given below. N (Thickness Direction)

R (Rolling Direction)

θ

T (Transverse Direction)

Figure 7-38 Axes of Anisotropy

The sample of tensile coupon cut from a sheet in the three directions, θ = 0 (rolling), 45° and 90° (transverse) is tested to obtain σ = σ 0 , σ 45 , and σ 90 , respectively. Similarly, the anisotropy parameter defined as: ε width r = -------------------ε thickness

(7-154)

is obtained for the 0°, 45°, and 90° directions. The yield stress in the third (thickness) direction can be written as: r 90 ( 1 + r 0 ) r 0 ( 1 + r 90 ) σ N = σ 0 --------------------------- = σ 90 --------------------------r 0 + r 90 r 0 + r 90

(7-155)

The direct stress coefficients are now: σ0 YRDIR ( 1 ) = -------σa v

(7-156)

σ 90 YRDIR ( 2 ) = -------σa v

(7-157)

σN YRDIR ( 3 ) = -------σa v

Main Index

(7-158)

CHAPTER 7 435 Material Library

where σ a v is the initial yield stress on the stress-strain curve used. If the stress-strain curve is averaged σ 0 + 2σ 45 + σ 90 from all directions, σ a v is defined as σ a v = ----------------------------------------- in orthotropic plasticity. Similarly, the 4 shear coefficients can be evaluated at: 3 YRSHR ( 1 ) = YRDIR ( 3 ) -------------------2r 45 + 1

(7-159)

YRSHR ( 2 ) = YRSHR ( 3 ) = 1.0

(7-160)

It is noted that the transverse direction along the thickness is usually considered isotropic which is reasonable on physical grounds. Also, notice that for complete isotropy, σ 0 = σ 45 = σ 90 and r 0 = r 45 = r 90 = 1 , which yields the von Mises yield criterion. Barlat’s (1991) Yield Function Barlat et al. [Ref. 6] proposed a general criterion for planar anisotropy that is particularly suitable for aluminum alloy sheets. This criterion has been shown to be consistent with polycrystal-based yield surfaces which often exhibit small radii of curvature near uniaxial and balanced biaxial tension stress states. An advantage of this criterion is that its formulation is relatively simple as compared with the formulation for polycrystalline modeling and, therefore, it can be easily incorporated into finite element codes for the analysis of metal forming problems. For three dimensional deformation, the yield function f is defined as (Barlat et al. [Ref. 6]) f = S1 – S2 where S i

m

+ S2 – S3

= 1 , 2, 3

m

+ S3 – S1

m

= 2σ

m

(7-161)

are principal values of a symmetric matrix S i j defined with respect to the components

of the Cauchy stress as

S =

C 3 ( σ xx – σ yy ) – C 2 ( σ zz – σ xx ) -------------------------------------------------------------------------------3

C6 σ x y

C 5 σ zx

C 6 σ xy

C 1 ( σ y y – σ zz ) – C 3 ( σ x x – σ y y ) -------------------------------------------------------------------------------3

C 4 σ zy

C 5 σ zx

C4 σz y

C 2 ( σ z z – σ x x ) – C 2 ( σ y y – σ zz ) ------------------------------------------------------------------------------3

(7-162)

In Equation (7-162), the symmetry axes (x, y, z), which represent the mutually orthogonal axes of anisotropy, are aligned with the initial rolling, transverse, and normal directions of the sheet. During deformation, the anisotropic yield surface of each material element rotates so that the symmetry axes are all in different directions during deformation. Therefore, it is necessary to trace the rotation of the yield surface during deformation in order to calculate the plastic strain increment properly. The rotation of the anisotropy axes is carried out based on the polar decomposition method.

Main Index

436 Marc Volume A: Theory and User Information

The material coefficients, C i Ci

= 1∼6

= 1∼6

in Equation (7-162) represent anisotropic properties. When

= 1 , the material is isotropic and Equation (7-161) reduces to the Tresca yield condition for

m = 1 or ∞ , and the von Mises yield criterion for m = 2 or 4. The exponent “ m ” is mainly associated with the crystal structure of the material. A higher “ m ” value has the effect of decreasing the radius of curvature of rounded vertices near the uniaxial and balanced biaxial tension ranges of the yield surface, in agreement with polycrystal models. Values of m = 8 for FCC materials (like aluminum) and m = 6 for BCC materials (like steel) are recommended. The yield surface has been proven to be convex for m ≥ 1 . Figure 7-39 shows the yield surfaces obtained from von-Mises, Hill and Barlat yield functions for Aluminum 2008-T4 alloy. 1.5

Vyy

Mises

V 1.0 Hill (1948)

0.5

Barlat’s 6D Vxx V

0.0

-0.5

-1.0 -1.0

-0.5

0.0

0.5

1.0

1.5

Figure 7-39 Comparison of Yield Surfaces Obtained from von Mises, Hill and Barlat Yield Functions p

Utilizing the normality rule, the associated plastic strain increment Δε i j is obtained from the yield function f as ∂f Δε ipj = λ ---------∂σ i j

(7-163)

∂f where λ is a scalar function. The calculation of ---------- in Equation (7-163) is lengthy but straightforward. ∂σ i j ∂f p The stress integration to obtain Δε i j along with the calculation of ------------- are shown in the works by ∂σ α β Chung and Shah, [Ref. 7], and Yoon et al,.[Ref. 8].

Main Index

CHAPTER 7 437 Material Library

In order to obtain four unknown independent coefficients ( C 1, C 2, C 3, C 6 ) with the assumption of C 4 = C 5 = 1 (isotropic properties for transverse directions), it is necessary to use four stresses from the experimental data ( σ 0, σ 45, σ 90, σ b ) , where σ 0, σ 45, σ 90 are the tensile yield stresses at 0o, 45o, and 90o from the rolling direction, and σ b is the balanced biaxial yield stress measured from bulge test. A detailed procedure to calculate the coefficients of Barlat’s yield function are summarized in the work of Yoon at el., [Ref. 9]. In Marc, Barlat’s coefficients are automatically calculated from user inputs for σ 0, σ 45, σ 90, σ b in Marc Mentat. If biaxial data is not available, generally Marc assumes σ b = σ 0 . Barlat’s yield function can be accessed from ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition options and can be used in conjunction with the ORIENTATION option.

Mohr-Coulomb Material (Hydrostatic Stress Dependence) Marc includes options for elastic-plastic behavior based on a yield surface that exhibits hydrostatic stress dependence. Such behavior is observed in a wide class of soil and rock-like materials. These materials are generally classified as Mohr-Coulomb materials (generalized von Mises materials). Ice is also thought to be a Mohr-Coulomb material. The generalized Mohr-Coulomb model developed by Drucker and Prager is implemented in Marc. There are two types of Mohr-Coulomb materials: linear and parabolic. Each is discussed on the following pages. Linear Mohr-Coulomb Material The deviatoric yield function, as shown in Figure 7-40, is assumed to be a linear function of the hydrostatic stress.

Main Index

σ f = αJ 1 + J 21 ⁄ 2 – ------- = 0 3

(7-164)

where

(7-165)

J1 = σi i

(7-166)

1 d d J 2 = --- σ i j σ i j 2

(7-167)

438 Marc Volume A: Theory and User Information

τ Yield Envelope

R c

φ

σ

σx + σy ------------------2 Figure 7-40 Yield Envelope of Plane Strain (Linear Mohr-Coulomb Material)

Analysis of linear Mohr-Coulomb material based on the constitutive description above is available in Marc through the ISOTROPIC model definition option. Through the ISOTROPIC option, the values of σ and α are entered. Note that, throughout the program, the convention that the tensile direct stress is positive is maintained, contrary to its use in many soil mechanics texts. The constants α and σ can be related to c and φ by σ c = ---------------------------------------------- ; 1⁄2 [ 3 ( 1 – 12α 2 ) ]

3α --------------------------------- = sin φ ( 1 – 3α 2 ) 1 ⁄ 2

(7-168)

where c is the cohesion and φ is the angle of friction. Parabolic Mohr-Coulomb Material The hydrostatic dependence is generalized to give a yield envelope which is parabolic in the case of plane strain (see Figure 7-41). f = ( 3J 2 +

3βσJ 1 ) 1 ⁄ 2 – σ = 0

(7-169)

The parabolic yield surface is obtained in Marc through the ISOTROPIC model definition option. Enter the values σ and β through the ISOTROPIC model definition option. σ

2

2

2 α = 3 ⎛ c – ------⎞ ⎝ 3⎠

where c is the cohesion.

Main Index

α β = --------------------------------------------( 3 ( 3c 2 – α 2 ) ) 1 ⁄ 2

(7-170)

CHAPTER 7 439 Material Library

τ

c

R

σx + σy ------------------2

σ

c2 ----α

Figure 7-41 Resultant Yield Condition of Plane Strain (Parabolic Mohr-Coulomb Material)

Buyukozturk Criterion (Hydrostatic Stress Dependence) This yield criterion [Ref. 4], which originally has been proposed as a failure criterion, has the general form: 2

f = β 3σJ 1 + γJ 1 + 3J 2 – σ

2

(7-171)

Through the ISOTROPIC model definition option, the user has to define σ and the factor β , where γ has a fixed value of 0.2 . The Buyukozturk criterion reduces to the parabolic Mohr-Coulomb criterion if γ = 0.

Powder Material Some materials, during certain stages of manufacturing are granular in nature. In particular, powder metals are often used in certain forging operations and during hot isostatic pressing (HIP). These material properties are functions of both the temperature and the densification. It should be noted that the soil model discussed in this chapter also exhibits some of these characteristics. In the model incorporated into Marc, a unified viscoplastic approach is used. The yield function is 1 3 p2 1 ⁄ 2 F = --- ⎛ --- σ d σ d + ------⎞ – σy γ ⎝2 β 2⎠

(7-172)

where σ y is the uniaxial yield stress, σ d is the deviatoric stress tensor, and p is the hydrostatic pressure. γ , β are material parameters. σ y can be a function of temperature and relative density, γ , β are functions only of relative density.

Main Index

440 Marc Volume A: Theory and User Information

Typically, we allow: γ = ( q1 + q2 ρ

q

q 3) 4

β = ( b1 + b2 ρ

b

b 3) 4

(7-173)

where ρ is the relative density. As the powder becomes more dense, ρ approaches 1 and the classical von Mises model is recovered. It should be noted that the elastic properties are also functions of relative density. In particular, as the material becomes fully dense, the Poisson’s ratio approaches 0.5.

2

p ----------------2 2 2 β γ σy

As most processes involving powder materials are both pressure and thermally driven, it can be necessary to perform a coupled analysis. Marc also allows you to specify density effects for the thermal properties, conductivity and specific heat. The basic input data is entered through the POWDER option. In addition to the TEMPERATURE EFFECTS option, there is a DENSITY EFFECTS option. The initial relative density is entered through the RELATIVE DENSITY option.

σ d :σ d -----------------2 2 2 --- γ σ y 3 Figure 7-42 Yield Function of Shima Model

Oak Ridge National Laboratory Options In Marc, the ORNL options are based on the definitions of ORNL-TM-3602 [Ref. 10] for stainless steels and ORNL recommendations [Ref. 16] for 2 1/4 Cr-1 Mo steel. The initial yield stress should be used for the initial inelastic loading calculations for both the stainless steels and 2 1/4 Cr-1 Mo steel. The 10th-cycle yield stress should be used for the hardened material. The 100th-cycle yield stress must be used in the following circumstances: 1. To accommodate cyclic softening of 2 1/4 Cr-1 Mo steel after many load cycles 2. After a long period of high temperature exposure 3. After the occurrence of creep strain To enter initial and 10th-cycle yield stresses, use the ISOTROPIC or ORTHOTROPIC model definition option.

Main Index

CHAPTER 7 441 Material Library

7

Effects of Temperature and Strain Rates on Yield Stress - not using table driven input

Material Library

Marc allows you to input a temperature-dependent yield stress. To enter the yield stress at a reference temperature, use the ISOTROPIC or ORTHOTROPIC model definition option. To enter variations of yield stress with temperatures, use the TEMPERATURE EFFECTS and ORTHO TEMP model definition options. Repeat the TEMPERATURE EFFECTS and ORTHO TEMP model definition options for each material, as necessary. The effect of temperatures on yielding is discussed further in Constitutive Relations. Marc allows you to enter a strain rate dependent yield stress, for use in dynamic and flow (for example, extrusion) problems. To use the strain rate dependent yield stress in static analysis, enter a fictitious time using the TIME STEP option. The zero-strain-rate yield stress is given on the ISOTROPIC or ORTHOTROPIC options. Repeat the STRAIN RATE model definition option for each different material where strain rate data are necessary. Refer to Constitutive Relations for more information on the strainrate effect on yielding.

Work or Strain Hardening In a uniaxial test, the workhardening slope is defined as the slope of the stress-plastic strain curve. The workhardening slope relates the incremental stress to incremental plastic strain in the inelastic region and dictates the conditions of subsequent yielding. The yield stress and the workhardening data must be compatible with the procedure used in the analysis. For small strain analyses, the engineering stress and engineering strain are appropriate. If only the LARGE DISP parameter is used, the yield stress should be entered as the second Piola-Kirchhoff stress, and the workhard data be given with respect to plastic Green-Lagrange strains. If the LARGE STRAIN parameter is used, the yield stress must be defined as a true or Cauchy stress, and the workhardening data with respect to logarithmic plastic strains. Flow Stress Definition - using table driven input When using the table driven input format, the yield (flow) stress dependence on the temperature, equivalent plastic strain, and the strain rate is defined simultaneously through a single table. As this table may be either a piecewise linear description or a mathematical equation based upon these independent variables, it allows a very general definition. The value of the yield stress is obtained by evaluating the table, including the reference value given on the ISOTROPIC or ORTHOTROPIC option. The strain hardening slope is obtained when necessary by numerically differentiating the values given. Work Hardening Definition - not using table input The uniaxial stress-plastic strain curve can be represented by a piecewise linear function through the TABLE or WORK HARD option. As an alternative, you can specify workhardening through the WKSLP user subroutine. There are two methods to enter this information, using the WORK HARD option. In the first method, you must enter workhardening slopes for uniaxial stress data as a change in stress per unit of plastic strain (see Figure 7-43) and the plastic strain at which these slopes become effective (breakpoint).

Main Index

442 Marc Volume A: Theory and User Information

Stress Δσ3

Δσ2 Δσ1

σ E

E

E p

p

Δε1

p

Δε 2

Δε 3

E Strain

Figure 7-43 Workhardening Slopes

Slope

Breakpoint

Δσ 1 ---------pΔε1

0.0

Δσ 2 ---------pΔε 2

Δσ 3 ---------pΔε 3

p

Δε1 p

p

Δε1 + Δε 2

and so on. Note:

The slopes of the workhardening curves should be based on a plot of the stress versus plastic strain for a tensile test. The elastic strain components of the stress-strain curve should not be included. The first breakpoint of the workhardening curve should be 0.0.

In the second method, you enter a of yield stress, plastic strain points. This option is flagged by adding the word DATA to the work hard statement. Note:

Main Index

The data points should be based on a plot of the stress versus plastic strain for a tensile test. The elastic strain components should not be included. The first plastic strain should equal 0.0 and the first stress should agree with that given as the yield stress in the ISOTROPIC or ORTHOTROPIC options.

CHAPTER 7 443 Material Library

Work Hardening Rules A number of workhardening rules (isotropic, kinematic, and combined) are available in Marc. A description of these workhardening rules is given below. Isotropic Hardening The isotropic workhardening rule assumes that the center of the yield surface remains stationary in the stress space, but that the size (radius) of the yield surface expands, due to workhardening. The change of the von Mises yield surface is plotted in Figure 7-44b. A review of the load path of a uniaxial test that involves both the loading and unloading of a specimen will assist in describing the isotropic workhardening rule. The specimen is first loaded from stress free (point 0) to initial yield at point 1, as shown in Figure 7-44a. It is then continuously loaded to point 2. Then, unloading from 2 to 3 following the elastic slope E (Young’s modulus) and then elastic reloading from 3 to 2 takes place. Finally, the specimen is plastically loaded again from 2 to 4 and elastically unloaded from 4 to 5. Reverse plastic loading occurs between 5 and 6. It is obvious that the stress at 1 is equal to the initial yield stress σ y and stresses at points 2 and 4 are larger than σ y , due to workhardening. During unloading, the stress state can remain elastic (for example, point 3), or it can reach a subsequent (reversed) yield point (for example, point 5). The isotropic workhardening rule states that the reverse yield occurs at current stress level in the reversed direction. Let σ 4 be the stress level at point 4. Then, the reverse yield can only take place at a stress level of – σ 4 (point 5). The isotropic workhardening model (with a work slope of 0) is the default option in Marc. For many materials, the isotropic workhardening model is inaccurate if unloading occurs (as in cyclic loading problems). For these problems, the kinematic hardening model or the combined hardening model represents the material better. σ 2

1

σy

σ′ 3

4 E

E E 0

5 6

+σ4

3 3 −σ4

5 6 (a) Loading Path

4

21 σ′ 2

σ′1 (b) von Mises Yield Surface

Figure 7-44 Schematic of Isotropic Hardening Rule (Uniaxial Test)

Main Index

0

444 Marc Volume A: Theory and User Information

Kinematic Hardening Under the kinematic hardening rule, the von Mises yield surface does not change in size or shape, but the center of the yield surface can move in stress space. Figure 7-45b illustrates this condition. Prager’s law is used to define the translation of the yield surface in the stress space. The loading path of a uniaxial test is shown in Figure 7-45a. The specimen is loaded in the following order: from stress free (point 0) to initial yield (point 1), 2 (loading), 3 (unloading), 2 (reloading), 4 (loading), 5 and 6 (unloading). As in isotropic hardening, stress at 1 is equal to the initial yield stress σ y , and stresses at 2 and 4 are higher than σ y , due to workhardening. Point 3 is elastic, and reverse yield takes place at point 5. Under the kinematic hardening rule, the reverse yield occurs at the level of σ 5 = ( σ 4 – 2σ y ) , rather than at the stress level of – σ 4 . Similarly, if the specimen is loaded to a higher stress level σ 7 (point 7), and then unloaded to the subsequent yield point 8, the stress at point 8 is σ 8 = ( σ 7 – 2σ y ) . If the specimen is unloaded from a (tensile) stress state (such as point 4 and 7), the reverse yield can occur at a stress state in either the reverse (point 5) or the same (point 8) direction. To invoke the kinematic hardening in Marc, use the model definition options ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC . To input workhardening slope data, use the TABLE or WORK HARD option or the WKSLP user subroutine. For many materials, the kinematic hardening model gives a better representation of loading/unloading behavior than the isotropic hardening model. For cyclic loading, however, the kinematic hardening model can represent neither cyclic hardening nor cyclic softening. σ′3

σ 7 2

1

σy

3 0 6

4

σ4

2σy

σ7 2σy

8

σ8 ε

σ5

5

(a) Loading Path

σ′1

σ′2 (b) von Mises Yield Surface

Figure 7-45 Schematic of Kinematic Hardening Rule (Uniaxial Test)

Combined Hardening Figure 7-46 shows a material with highly nonlinear hardening. Here, the initial hardening is assumed to be almost entirely isotropic, but after some plastic straining, the elastic range attains an essentially constant value (that is, pure kinematic hardening). The basic assumption of the combined hardening model is that such behavior is reasonably approximated by a classical constant kinematic hardening

Main Index

CHAPTER 7 445 Material Library

constraint, with the superposition of initial isotropic hardening. The isotropic hardening rate eventually decays to zero as a function of the equivalent plastic strain measured by ·p

∫ε

εp =

dt =

⎛2

p p⎞ 1 ⁄ 2

∫ ⎝ --3- ε· i j ε· i j⎠

dt

(7-174)

This implies a constant shift of the center of the elastic domain, with a growth of elastic domain around this center until pure kinematic hardening is attained. In this model, there is a variable proportion between the isotropic and kinematic contributions that depends on the extent of plastic deformation (as p

measured by ε ). Use the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition option to activate the combined workhardening option in Marc. Use the TABLE or WORK HARD option or the WKSLP user subroutine to input workhardening slope data. There are two formulations in the Marc program. The older one occurs whenever PLASTICITY,4 is not included as a parameter. The workhardening data at small strains governs the isotropic behavior, and the data at large strains ( ε p > 1000 ) governs the kinematic hardening behavior. If the last workhardening slope is zero, the behavior is the same as the isotropic hardening model. σ Initial Elastic Range

Combined Hardening Range

Fully Hardened Pure Kinematic Range

Stress

Initial Yield One-half Current Elastic Range

3 2

Kinematic Slope, ---

dα --------p dε

ε

Strain

Figure 7-46 Basic Uniaxial Tension Behavior of the Combined Hardening Model

The newer formulation, which is invoked by including a PLASTICITY,4 parameter allows greater generality by introducing the fractional contribution ( f h ) to kinematic hardening as a user input. As shown in Figure 7-47, f is the value between 0 and 1 .

Main Index

446 Marc Volume A: Theory and User Information

Work Hardening Curve

σ

σα

σy

σy

εp

Kinematic Hardening

Isotropic Hardening

α

εp σα = σy + ( 1 – fh ) * ( σ – σy )

εp α = f ( σ – σy )

Figure 7-47 Schematic Explanation for Kinematic Hardening Fraction

Isotropic hardening

fh = 0

Kinematic hardening

fh = 1

Combined hardening

0 < fh < 1

(default f h = 0.5 )

Combined hardening model utilizing kinematic fraction factor is available for Hill and Barlat models in ISOTROPIC, ORTHOTROPIC, and ANISOTROPIC options.

Flow Rule Yield stress and workhardening rules are two experimentally related phenomena that characterize plastic material behavior. The flow rule is also essential in establishing the incremental stress-strain relations for p

plastic material. The flow rule describes the differential changes in the plastic strain components dε as a function of the current stress state. The Prandtl-Reuss representation of the flow rule is available in Marc. In conjunction with the von Mises yield function, this can be represented as: ∂σ p dε i j = dε p ---------∂σ i j

(7-175)

where dε p and σ are equivalent plastic strain increment and equivalent stress, respectively. The significance of this representation is illustrated in Figure 7-48. This figure illustrates the “stressspace” for the two-dimensional case. The solid curve gives the yield surface (locus of all stress states causing yield) as defined by the von Mises criterion. Equation (7-175) expresses the condition that the direction of inelastic straining is normal to the yield surface. This condition is called either the normality condition or the associated flow rule. If the von Mises yield surface is used, then the normal is equal to the deviatoric stress.

Main Index

CHAPTER 7 447 Material Library

σ2

dεp

p

dε2 dε1p

σ1

Yield Surface Figure 7-48 Yield Surface and Normality Criterion 2-D Stress Space

Constitutive Relations This section presents the constitutive relation that describes the incremental stress-strain relation for an elastic-plastic material. The material behavior is governed by the incremental theory of plasticity, the von Mises yield criterion, and the isotropic hardening rule. Let the workhardening coefficient H be expressed as: H = dσ ⁄ dε p

(7-176)

and the flow rule be expressed as: dε

p

∂σ = dε p : ∇σ where ∇σ = ---------∂σ i j

(7-177)

Consider the differential form of the familiar stress-strain law, with the plastic strains interpreted as initial strains dσ = C : dε – C : dε p

(7-178)

where C is the elasticity matrix defined by Hooke’s law and “:” denotes the tensor contraction. After substitution of Equation (7-177), this becomes dσ = C : dε – C : ∇σdε p

(7-179)

Contracting Equation (7-179) by ∇σ ∇σ : dσ = ∇σ : C : dε – ∇σ : C : ∇σdε p

(7-180)

and recognizing that dσ = ∇σ : dσ with use of Equation (7-176) in place of the left-hand side,

Main Index

(7-181)

448 Marc Volume A: Theory and User Information

Hdε p = ∇σ : C : dε – ∇σ : C : ∇σdε p

(7-182)

By rearrangement ∇σ : C : dε dε p = ------------------------------------------H + ∇σ : C : ∇σ

(7-183)

Finally, by substitution of this expression into Equation (7-179), we obtain dσ = L e p :dε

(7-184)

where L e p is the elasto-plastic, small strain tangent moduli expressed as: L

ep

( C : ∇σ ) ⊗ ( C : ∇σ ) = C – -----------------------------------------------------H + ∇σ : C : ∇σ

(7-185)

The case of perfect plasticity, where H = 0 , causes no difficulty. Temperature Effects This section discusses the effects of temperature-dependent plasticity on the constitutive relation. The following constitutive relations for thermo-plasticity were developed by Naghdi. Temperature effects are discussed using the isotropic hardening model and the von Mises yield condition. The stress rate can be expressed in the form · · σ i j = L i j k l ε k l + h i j T·

(7-186)

For elastic-plastic behavior, the moduli L i j k l are ∂σ ∂σ L i j k l = C i j k l – ⎛ C i j m n ------------- ------------ C p q k l⎞ ⁄ D ⎝ ⎠ ∂σ m n ∂σ p q

(7-187)

and for purely elastic response Li j k l = Ci j k l

(7-188)

The term that relates the stress increment to the increment of temperature for elastic-plastic behavior is ∂σ 2 ∂σ h i j = X i j – C i j k l α k l – ⎛ C i j k l ----------- ⎛ σ p q X p q – --- σ -------⎞ ⎞ ⁄ D ⎝ ∂σ k l ⎝ 3 ∂T⎠ ⎠

(7-189)

and for purely elastic response Hi j = Xi j – Ci j k l αk l where

Main Index

(7-190)

CHAPTER 7 449 Material Library

4 ∂σ ∂σ ∂σ D = --- σ 2 -------- + ---------- C i j k l ----------9 ∂σ k l ∂ε p ∂σ i j

(7-191)

and ∂C i j k l e X i j = --------------- ε ∂T k l

(7-192)

and α k l are the coefficients of thermal expansion. Strain Rate Effects This section discusses the influence of strain rate on the elastic-plastic constitutive relation. Strain rate effects cause the structural response of a body to change because they influence the material properties of the body. These material changes lead to an instantaneous change in the strength of the material. Strain rate effects become more pronounced for temperatures greater than half the melting temperature ( T m ). The following discussion explains the effect of strain rate on the size of the yield surface. Using the von Mises yield condition and normality rule, we obtain an expression for the stress rate of the form ·· · · σi j = Li j k l εk l + ri j ε

p

(7-193)

For elastic-plastic response ∂σ ∂σ L i j k l = C i j k l – ⎛ C i j m n ------------- ------------ C p q k l⎞ ⁄ D ⎝ ⎠ ∂σ m n ∂σ p q

(7-194)

and ∂σ 2 ∂σ r i j = C i j m n ------------- --- σ -------- ⁄ D ·p ∂σ m n 3 ∂ε

(7-195)

where ∂σ 4 ∂σ ∂σ D = --- σ 2 -------- + ---------- C i j k l ----------9 ∂σ k l ∂ε p ∂σ i j

(7-196)

Time-independent Cyclic Plasticity The cyclic plasticity model is based on the work of Chaboche [Ref. 23]. The current version of Marc consists only of the basic model and plastic-strain-range memorization. The associated time-dependent model is described on Time-dependent Cyclic Plasticity. The model combines the isotropic hardening rule, to describe the cyclic hardening (Figure 7-49a) or softening, and the nonlinear kinematic hardening to capture the proper characteristic of cyclic plasticity

Main Index

450 Marc Volume A: Theory and User Information

like Bauschinger (Figure 7-49b), ratchetting (Figure 7-49c), and mean-stress relaxation (Figure 7-49d) effect. The influence of the plastic strain range on the stabilized cyclic response is taken into account by introducing the plastic-strain-range memorization variable (Figure 7-49e). The von Mises yield function is now defined as follows: f = σ – (R + k) 1 ---

3S i j S i j 2 1 where σ = ⎛ -----------------⎞ , s i j = σ' i j – --- δ i j σ' k k and σ' = σ – X ⎝ 2 ⎠ 3 X is the back stress tensor representing the center of the yield surface in stress space. σ

σ

σ –ε

ε ε

ε

(a) Cyclic Hardening under Multiple Cyclic Loading

(b) Bauschinger Effect

(c) Ratchetting

σ σ –ε

ε

ε

(d) Mean Stress Relaxation

(e) Cyclic Hardening

Figure 7-49 Typical Behavior of Material that can be Simulated with Cyclic Plasticity Model

Main Index

CHAPTER 7 451 Material Library

Isotropic Hardening/Softening The isotropic hardening/softening determines the size of the elastic region during the plastic loading. In this model, it is controlled by parameter R and k . The initial conditions of cyclic hardening are given as k = σ y and R = 0 , while a cyclic softening is initially described by k = σ y – R 0 and R = R 0 . The evolution equation for the variable R is described as follows: · · R = b ( R ∞ – R )λ where b and R ∞ are material constants. R ∞ represents the limit of the isotropic hardening/softening. In case of hardening, then R = R ∞ ⎛ 1 – e ⎝

–b e

p s⎞

⎠

.

Nonlinear Kinematic Hardening The nonlinear kinematic hardening is defined from the linear-Ziegler rule by adding the recall term as shown in the evolution of the back stress tensor below: · X =

· C -------------- ( σ – X ) – γX λ R+k

where C and γ are two material constants. γ = 0 stands for linear-kinematic rule. Plastic-strain-range Memorization Several experimental observations show that the asymptotic stress value of cyclic hardening can depend on the prior history. The influence of plastic-strain range on the stabilized cyclic response is evident from the comparison between the different histories of loading used to obtained the cyclic curve. Therefore, an introduction of new internal variables that memorize the prior maximum plastic range is introduced by defining a “memory” surface in the plastic strain space as follows: 2 F = --- ε e ( ε p – ζ ) – ρ 3 The evolution of the state variables are as follows * · · ρ = ηH ( F ) 〈 n ⋅ n 〉 λ

· ζ =

* *· 3 ⁄ 2 ( 1 – η )H ( F ) 〈 n ⋅ n 〉 n λ *

where n and n are the unit normal to the yield surface f = 0 and to the memory surface F = 0 defined as follows: n =

Main Index

2 --3

εp * ---·- and n = λ

2 ε p– ζ --- -----------3 ρ

452 Marc Volume A: Theory and User Information

The coefficient η is introduced in order to induce a progressive memory. For η = 0.5 then, the memorization is instantaneous and stabilization occurs after one cycle. A progressive memory is given by η < 0.5 . The dependency between cyclic plastic flow and the plastic strain range is introduced by considering an asymptotic isotropic state as follows: R ∞ = Q M + ( Q 0 – Q M )e

–2 μ ρ

where Q M , Q 0 and μ are material constants. Plastic Evolution Process and Elasto-plastic “Classical” Modular Matrix · The plastic evolution process must conform to the consistency condition, f = 0 . From this condition the plastic “rate” multiplier can be derived as follows: T

a L · · λ = --------------------------------------------------------------------------------------------------------------------ε T T C T a La + -------------- a ( σ – X ) – γa X + b ( R ∞ – R ) R+k

(7-197)

∂f 3 s where a = ------ = --- -------------- . ∂σ 2R + k Since the process involves nonlinear equation, iteration process using predictor-corrector technique is used. The predictor is calculated using the “trial” elastic stresses as follows: σ B = σ A + L Δσ and then calculate f B based on σ B and hardening parameter on A. Using the Taylor expansion at B, then fB δλ = --------------------------------------------------------------------------------------------------------------------C a T La + -------------- a T ( σ – X ) – γa T X + b ( R ∞ – R ) R+k Having the global plasticity iteration converged, then the iteration to satisfy the plastic strain memorization is started. If both iterations are converged, then the total plasticity iteration is considered completed. Inserting Equation (7-199) into Equation (7-198) and using Equation (7-197), the elasto-plastic “classical” tangent modular matrix can be derived as follows:

L

Main Index

EP

⎛ ⎞ T aa L = L ⎜ I – --------------------------------------------------------------------------------------------------------------------⎟ ⎜ ⎟ T T C T a La + -------------- a ( σ – X ) – γa X + b ( R ∞ – R )⎠ ⎝ R+k

(7-198)

CHAPTER 7 453 Material Library

Time-dependent Inelastic Behavior Force-displacement relationships vary in different material models. A perfectly elastic material and a perfectly viscous material can be represented by a spring and a dashpot, respectively (as shown in Figure 7-50). In a perfectly elastic material, the deformation is proportional to the applied load. In a perfectly viscous material, the rate of change of the deformation over time is proportional to the load. In the class of viscoelastic and creeping materials, the application of a constant load is followed by a deformation, which can be made up of an instantaneous deformation (elastic effect) followed by a continual deformation with time (viscous effect). Eventually, it can become pure viscous flow. Continued deformation under constant load is termed creep (see Figure 7-51). SPRING

f = ku f = force u = Displacement k = Spring Stiffness

DASHPOT

f = ηu f = Force u = Velocity (Time Rate of Change of Displacement η = Viscosity of the Dashpot

Figure 7-50 Perfectly Elastic (Spring) and Viscous (Dashpot) Materials ε (Strain)

C

B A t (Time)

0 OA – Instantaneous Elastic Effect AB – Delayed Elastic Effect BC – Viscous Flow Figure 7-51 The Creep Curve

A viscoelastic material can be subjected to sudden application of a constant deformation. This results in an instantaneous proportional load (elastic effect), followed by a gradual reduction of the required load

Main Index

454 Marc Volume A: Theory and User Information

with time, until a limiting value of the load is attained. The decreasing of load for a constant deformation, is termed relaxation (see Figure 7-52). Viscoelastic and creeping materials can be represented by models consisting of both springs and dashpots because the material displays both elastic effects and viscous effects. This implies that the material either continues to flow for a given stress, or the stress decreases with time for a given strain. The measured relation between stress and strain is generally very complex. σ (Stress)

0 Figure 7-52 The Relaxation Curve

t (Time)

Two models that are commonly used to relate stress and strain are the Maxwell and Kelvin (Voigt or Kelvin-Voigt) models. A description of these models is given below. The mathematical relation which holds for the Maxwell solid is · · ε = ασ + βσ

(7-199)

In the one-dimensional case for normal stress 1 α = --E

(7-200)

1 β = --η

This relation can be depicted as a spring and dashpot in series, as shown in Figure 7-53. The integration of Equation (7-199) yields σ σ ε = --- + ∫ --- dt η E σ

(7-201) σ

Figure 7-53 Maxwell Solid

The strain and stress responses of the Maxwell Solid model are shown in Figure 7-54 and Figure 7-55, respectively.

Main Index

CHAPTER 7 455 Material Library

σ

ε

σ0 -----E t

t Response to Constant Stress

Constant Stress Applied

Figure 7-54 Strain Response to Applied Constant Stress (Maxwell Solid) ε

σ

ε

t Constant Strain Applied

t τ Response to Constant Strain

Figure 7-55 Stress Response to Applied Constant Strain (Maxwell Solid)

The mathematical relation which holds for the Kelvin (Voigt or Kelvin-Voigt) solid is · σ = αε + βε

(7-202)

This equation is depicted as a spring and dashpot in parallel. (See Figure 7-56). When β = 0 (no dashpot), the system is a linearly elastic system in which α = E , the elastic modulus. When E = 0 (no spring), the “solid” obeys Newton’s equation for a viscous fluid and β = η , the viscous coefficient. Thus, we can rewrite Equation (7-202) in the form · σ = Eε + ηε

(7-203)

In the above relation, we have considered one-dimensional normal stress and strain. The relation holds equally well for shear stress τ and shear strain γ in which α = G , the shear modulus, and β = η , the viscous coefficient. Equation (7-202) can be rewritten as · τ = Gγ + ηγ

(7-204) E

σ

σ

η

Main Index

456 Marc Volume A: Theory and User Information

Figure 7-56 Kelvin (Voigt or Kelvin-Voigt) Solid

The strain responses of the Kelvin Solid model are depicted in Figure 7-57. For multiaxial situations, these equations can be generalized to tensor quantities. To invoke the Maxwell model, use the CREEP parameter. The creep strain can be specified as either deviatoric creep strain (conventional creep) or dilatational creep strain (swelling). To invoke the Kelvin model, also use the CREEP parameter and CRPVIS user subroutine. σ

σ0

t

t1 (a) Stress Pulse ε

σ0 -----E

t

t (b) Strain Response to Stress of Infinite Domain ε

t1

t

(c) Strain Response to Stress Pulse of Finite Length Figure 7-57 Strain Response to Applied Stress (Kelvin Solid)

Creep (Maxwell Model) Creep is an important factor in elevated-temperature stress analysis. In Marc, creep is represented by a Maxwell model. Creep is a time-dependent, inelastic behavior, and can occur at any stress level (that is, either below or above the yield stress of a material). In many cases, creep is accompanied by plasticity which occurs above the yield stress of the material. The creep behavior can be characterized as primary, secondary, and tertiary creep, as shown in Figure 7-58. Engineering analysis is often limited to the primary and secondary creep regions. Tertiary creep in a uniaxial specimen is usually associated with geometric instabilities, such as necking. The major difference between the primary and secondary creep is that the creep strain rate is much larger in the primary creep region than it is in the secondary creep

Main Index

CHAPTER 7 457 Material Library

region. The creep strain rate is the slope of the creep strain-time curve. The creep strain rate is generally dependent on stress, temperature, and time. The creep data can be specified in either an exponent form or in a piecewise linear curve. To specify creep data, use the CREEP model definition option. The CRPLAW user subroutine allows alternative forms of creep behavior to be programmed directly. ·c dε c ε = -------dt

(7-205)

Creep Strain εC Tertiary Creep Secondary Creep Primary Creep

Time (t)

Note: Primary Creep:

Fast decrease in creep strain rate Secondary Creep: Slow decrease in creep strain rate Tertiary Creep: Fast increase in creep strain rate

Figure 7-58 Creep Strain Versus Time (Uniaxial Test at Constant Stress and Temperature)

Marc offers two schemes for modeling creep in conjunction with plasticity: (a) treating creep strains and plastic strains separately; and (b) modeling creep strains and plastic strains in a unified fashion (viscoplasticity). Both schemes can be treated using two different procedures: explicit and implicit. Creep (Explicit Formulation) There are six possible modes of input for creep constitutive data. 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

Main Index

(7-206)

458 Marc Volume A: Theory and User Information

·c c where A is a constant; ε is equivalent creep strain rate; and σ , ε , T , and t are equivalent stress, equivalent creep strain, temperature and time, respectively. The functions f , g , h , and k are piecewise linear and entered in the form as either slope-break point data or function-variable data. This representation is shown in Figure 7-59. Enter functions f , g , h , and k through the CREEP model definition option. (Any of the functions f , g , h , or k can be set to unity by setting

the number of piecewise linear slopes for that relation to zero on the input data.) 1. The dependence of equivalent creep strain rate on any independent parameter can be given directly in power law form by the appropriate exponent. The equivalent creep strain rate is · n ε c = Aσ m ⋅ ( ε c ) ⋅ T p ⋅ ( qt q – 1 ) Enter the constants A , m , n , p , and q directly through the CREEP model definition option. This is often adequate for engineering metals at constant temperature where Norton’s rule is a good approximation. ·c ε = A σn

(7-207)

2. input procedure, one can define a table such that ·c ε = A ⋅ f ( v 1 ,v 2 ,v 3 ,v 4 )

(7-208)

where v 1 ,v 2 ,v 3 ,v 4 are four variables that could include equivalent stress, temperature, time, strain, position, or one of 30 variables. In this case, the function is piecewise linear. 3. Using the table driven input procedure, one can define the strain rate such that · cr ε = A ⋅ equation ( v 1 ,v 2 ,v 3 ,v 4 )

(7-209)

For example, one could enter the equation Aσ n e – Q R ⁄ T

(7-210)

The equation can take form as long as there is no conditional logic required. If this is not the case, the CRPLAW user subroutine should be used. 4. Define the equivalent creep strain rate directly with the CRPLAW user subroutine. 5. Use the ISOTROPIC option to activate the ORNL (Oak Ridge National Laboratory rules) capability of the program. Isotropic creep behavior is based on a von Mises creep potential described by the equivalent creep law · ε = f ( σ , ε c , T, t )

(7-211)

The material creep behavior is described by · · c ⎧ ∂σ ⎫ ε icj = ε ⎨ ---------- ⎬ ⎩ ∂σ i j ⎭

Main Index

(7-212)

CHAPTER 7 459 Material Library

During creep, the creep strain rate usually decreases. This effect is called creep hardening and can be a function of time or creep strain. The following section discusses the difference between these two types of hardening. Consider a simple power law that illustrates the difference between time and strain-hardening rules for the calculation of the creep strain rate. ε

c

= βt n

(7-213) F4 F3 S3

Function F (X) [for example, t ( σ ) ,

F2

S2

c

g ( ε ) , h (T), k (t)] S1 F1

X1

X2

X4

X3 Variable X (Such as σ, εC, T, t)

(1) Slope-Break Point Data Slope

Break Point

S1 S2 S3

X1 X2 X3 (2) Function-Variable Data

Function F1 F2 F3 F4 Figure 7-59 Piecewise Linear Representation of Creep Data

Main Index

Variable X1 X2 X3 X4

460 Marc Volume A: Theory and User Information

c

where ε is the creep strain, β and n are values obtained from experiments and t is time. The creep rate c

can be obtained by taking the derivative ε with respect to time c

dε ·c ε = -------- = nβt n – 1 dt

(7-214)

However, t being greater than 0, we can compute the time t as c 1/n

ε t = ⎛ -----⎞ ⎝ β⎠

(7-215)

Substituting Equation (7-210) into Equation (7-209) we have c (n – 1) ⁄ n ·c ) ε = nβt n – 1 = n ( β 1 ⁄ n ( ε )

(7-216)

Equation (7-210) shows that the creep strain rate is a function of time (time hardening). Equation (7-216) indicates that the creep strain rate is dependent on the creep strain (strain hardening). The creep strain rates calculated from these two hardening rules generally are different. The selection of a hardening rule in creep analysis must be based on data obtained from experimental results. Figure 7-60 and Figure 7-61 show time and strain hardening rules in a variable state of stress. It is assumed that the stress in a structure varies from σ 1 to σ 2 to σ 3 ; depending upon the model chosen, different creep strain rates are calculated accordingly at points 1, 2, 3, and 4. Obviously, creep strain rates obtained from the time hardening rule are quite different from those obtained by the strain hardening rule. εc

σ1 σ2

3

σ3

1 4 2 0

t

Figure 7-60 Time Hardening

Main Index

CHAPTER 7 461 Material Library

7

εc σ1 σ2

3 1 2

σ3 4

0 t

Figure 7-61 Strain Hardening

Oak Ridge National Laboratory Laws Material Library

Oak Ridge National Laboratory (ORNL) has performed a large number of creep tests on stainless and other alloy steels. It has also set certain rules that characterize creep behavior for application in nuclear structures. A summary of the ORNL rules on creep is given below. The references listed at the end of this section offer a more detailed discussion of the ORNL rules. 1. Auxiliary Rules for Applying Strain-Hardening to Situations Involving Stress Reversals The Blackburn Creep Law is required as the CRPLAW user subroutine. The parameter EQCP (first parameter in CRPLAW) is defined as 2 c c 1/2 ε c = ⎛ --- ΣΔε i j ΣΔε i j ⎞ ⎝3 ⎠

(7-217)

when the ORNL constitutive option is flagged through use of the ISOTROPIC option. In all other cases, the definition c 1/2 2 ε c = Σ ⎛ --- Δε icj Δε i j ⎞ ⎝3 ⎠

(7-218)

is retained. The equivalent primary creep strain passes into CRPLAW in EQCPNC, the second parameter. The second parameter must be redefined in that routine as the equivalent (total) creep strain increment. The first parameter (EQCP) must be redefined as the equivalent primary creep strain increment when the ORNL constitutive option is flagged. During analysis with the ORNL option, equivalent creep strain stores the distance between the two shifted origins in creep strain space ( ε in ORNL-TM-3602). The sign on this value indicates which origin is currently active, so that a negative sign indicates use of the “negative” origin ( – ε i j ).

Main Index

462 Marc Volume A: Theory and User Information

2. Plasticity Effect on Creep The effect of plastic strains on creep must be accommodated for the time-dependent creep behavior of 2 1/4 Cr -1 Mo Steel. Since plastic strains in one direction reduce the prior creep strain hardening accumulated in the reverse direction, ORNL recommends that the softening influence due to plastic strains be treated much the same as when reversed creep strain occurs. The following quantities are defined: +

+ + N i j = ( ε iIj – ε i j ) ⁄ G –

N i j = ( ε iIj – ε i–j ) ⁄ G

(7-219) –

(7-220)

where ε iIj is instantaneous creep strain components ε i+j ;ε i–j = positive and negative strain origins

(7-221)

and G

+

G–

= G ( ε iIj – ε i+j ) = [ 2 ⁄ 3 ( ε iIj – ε i+j ) ( ε iIj – ε i+j ) ] 1 ⁄ 2 = G ( ε iIj – ε i–j ) = [ 2 ⁄ 3 ( ε iIj – ε i–j ) ε iIj – ε i–j ] 1 ⁄ 2

(7-222) (7-223)

Swelling Marc allows pure swelling (dilatational creep) effect in a creep analysis. To use the swelling option, perform a regular creep analysis as discussed earlier. Use the VSWELL user subroutine to define the ΔV increment of volumetric swelling ⎛ --------⎞ . The increment of volumetric swelling is generally a function ⎝ V⎠ of neutron flux, time, and temperatures. For example, radiation-induced swelling strain model for 20% C. W. Stainless Steel 316 can be expressed as: R 1 + exp ( α ( τ – φt ) ) ΔV -------- = Rφt + ---- ln ------------------------------------------------α 1 + expτ V

(7-224)

where R , t , and α are functions of temperature, φ is neutron flux, and t is time. Creep (Implicit Formulation) This formulation, as opposed to that described in the previous section, is fully implicit. A fully implicit formulation is unconditionally stable for any choice of time step size; hence, allowing a larger time step than permissible using the explicit method. Additionally, this method is more accurate than the explicit method. The disadvantage is that each increment may be more computationally expensive. This model is activated using the CREEP parameter. There are two methods for defining the inelastic strain rate. The

Main Index

CHAPTER 7 463 Material Library

CREEP model definition option can be used to define a Maxwell creep model. The back stress must be specified through the field normally reserved for the yield stress in the ISOTROPIC or ORTHOTROPIC

options. The yield stress must be specified through the field normally reserved for the 10th cycle yield stress in the ISOTROPIC option. There is no plastic strain when the stress is less than the yield stress and there is no creep strain when the stress is less than the back stress. The equivalent creep strain increment is expressed as · ε c = Aσ m ⋅ ( ε c ) n ⋅ T p ⋅ ( qt q – 1 )

(7-225)

Enter the constants A , m , n , p , and q directly through the CREEP model definition option. A more general expression for the equivalent creep strain rate is given by: ·c dk ( t ) ε = A ⋅ σ m ⋅ g ( ε c ) ⋅ h ( T ) ⋅ ------------dt

(7-226)

Enter the terms A and m and the functions g , h , and k through the UCRPLW user subroutine. The creep strain components are given by: d

3 σi j Δε i j = --- Δε ------2 σ d

where σ i j is the deviatoric stress at the end of the increment. A is a function of temperature, time, etc. An algorithmic tangent is used to form the stiffness matrix. Based on a parameter defined in the CREEP parameter, one of three tangent matrices is formed. The first is using an elastic tangent, which requires more iterations, but can be computationally efficient because re-assembly might not be required. The second is an algorithmic tangent that provides the best behavior for small strain power law creep. The third is a secant (approximate) tangent that gives the best behavior for general viscoplastic models. When creep is specified in conjunction with plasticity, the elastic tangent option is not available.

Viscoplasticity (Explicit Formulation) The creep (Maxwell) model can be modified to include a plastic element (as shown in Figure 7-62). This plastic element is inactive when the stress ( σ ) is less than the yield stress ( σ y ) of the material. The modified model is an elasto-viscoplasticity model and is capable of producing some observed effects of creep and plasticity. In addition, the viscoplastic model can be used to generate time-independent plasticity solutions when stationary conditions are reached. At the other extreme, the viscoplastic model can reproduce standard creep phenomena. The model allows the treatment of nonassociated flow rules and strain softening which present difficulties in conventional (tangent modulus) plasticity analyses. The viscoplasticity option can be used to implement very general constitutive relations with the aid of the following user subroutines: ZERO, YIEL, NASSOC, and CRPLAW. See Nonlinear Analysis in Chapter 5 for details on how to use these procedures.

Main Index

464 Marc Volume A: Theory and User Information

σ

εe εvp

ε

p

= ε

vp

Plastic Element Inactive if σ < σy

Figure 7-62 Uniaxial Representation of Viscoplastic Material

Viscoplasticity (Implicit Formulation) To allow for the implementation of general unified creep-plasticity or viscoplastic models, the UVSCPL user subroutine is available. This routine requires you to define only the inelastic strain rate. The program automatically calculates a tangent stiffness matrix (only elastic tangent or secant tangent can be used). This option is activated by indicating that the material is VISCO PLAS in the ISOTROPIC or ORTHOTROPIC option.

Time-dependent Cyclic Plasticity The time-dependent effect of the model described in “Time-independent Cyclic Plasticity” on page 449 is modeled using the unified viscoplastic framework. The viscoplastic potential is based on “overstress” quantity as follows: f n+1 K Ω = ------------- 〈 ----〉 n+1 K The viscoplastic strain rate is defined as follows: 3· ∂Ω 3 · σ' – X' · = --- λ ----------------- = --- λ ∇f εv p = 2 ∂σ 2 σ˜ e

(7-227)

where f n · λ = 〈 ----〉 K

(7-228) 1 ---

In this case, the viscoplastic stress is σ v p

·n = Kλ .

The hardening rules are chosen to be identical to the time-independent case.

Main Index

CHAPTER 7 465 Material Library

Viscoplastic Evolution Process and Visco-plastic “Classical” Modular Matrix The iteration procedure, starting from the trial elastic stress as the predictor, is based on the implicit integration of Equation (7-228) that can be expressed as follows: Δλ f n r λ = – ------ + 〈 ---- 〉 Δt K

(7-229)

Using Newton iteration scheme, the iterative value of Δλ (that is, δλ ) can be expressed as follows: i

Δt r n δλ = --------------------------------------------------------------------------------------------------------------------------------------T n f n – 1⎛ T 2 T 1 + ---- 〈 ----〉 a La + --- Ca a – γa X + b ( R ∞ – R )⎞ ⎝ ⎠ K K 3 i

where r λ is the i-th iteration of the residual of Equation (7-229). The tangent modular matrix is based on the assumption that δr λ = 0 . Therefore the classical viscoplastic modular matrix can be expressed as follows:

L

vp

⎛ ⎞ ⎜ ⎟ T ⎜ ⎟ aa L = L ⎜ I – ------------------------------------------------------------------------------------------------------------------------------------⎟ T T 2 T 1 ⎜ a La + --- Ca a – γa X + b ( R ∞ – R ) + --------------------------------⎟ ⎜ 3 n f n–1 ⎟ Δt ⎠ ---- 〈 ---- 〉 ⎝ K K

This matrix is in line with the consistent model derived in [Ref. 20].

Viscoelastic Material Marc has two models that represent viscoelastic materials. The first can be defined as a Kelvin-Voigt model. The latter is a general hereditary integral approach. Kelvin-Voigt Model The Kelvin model allows the rate of change of the inelastic strain to be a function of the total stress and previous strain. To activate the Kelvin model in Marc, use the CREEP parameter. k ij

The Kelvin material behavior (viscoelasticity) is modeled by assuming an additional creep strain ε , governed by d k d ----- ε i j = A i j k l σ k l – B i j k l ε kkl dt

(7-230)

where A and B are defined in the CRPVIS user subroutine and the total strain is ε i j = ε iej + ε ipj + ε icj + ε ikj + εti hj

Main Index

(7-231)

466 Marc Volume A: Theory and User Information

εti hj = thermal strain components

(7-232)

ε iej = elastic strain components (instantaneous response)

(7-233)

ε ipj = plastic strain components

(7-234)

ε icj = creep strains defined via the CRPLAW and VSWELL user subroutines

(7-235)

ε ikj = Kelvin model strain components as defined above

(7-236)

The CRPVIS user subroutine is called at each integration point of each element when the Kelvin model is used. Use the AUTO CREEP option to define the time step and to set the tolerance control for the maximum strain in any increment. The CREEP option allows Maxwell models to be included in series with the Kelvin model. Hereditary Integral Model The stress-strain equations in viscoelasticity are not only dependent on the current stress and strain state (as represented in the Kelvin model), but also on the entire history of development of these states. This constitutive behavior is most readily expressed in terms of hereditary or Duhamel integrals. These integrals are formed by considering the stress or strain build-up at successive times. Two equivalent integral forms exist: the stress relaxation form and the creep function form. In Marc, the stress relaxation form is used. The viscoelasticity option in Marc can be used for both the small strain and large strain Mooney or Ogden material stress-relaxation problems for total Lagrange formulation. It can also be used with all hyperelastic models; i.e., Mooney, Ogden, Gent, Arruda-Boyce, Foam and generalized hyperelastic materials if the Updated Lagragian formulation is used. A description of these models is as follows: Small Strain Viscoelasticity In the stress relaxation form, the constitutive relation can be written as a hereditary integral formulation t

σi j ( t ) =

dε k l ( τ )

- dτ + G i j k l ( t )ε k l ( 0 ) ∫ G i j k l ( t – τ ) ----------------dτ

(7-237)

0

The functions G i j k l are called stress relaxation functions. They represent the response to a unit applied strain and have characteristic relaxation times associated with them. The relaxation functions for materials with a fading memory can be expressed in terms of Prony or exponential series. ∞

Gi j k l ( t ) = Gi j k l +

N

∑ n = 1

Main Index

n

n

G i j k l exp ( – t ⁄ λ )

(7-238)

CHAPTER 7 467 Material Library

n

n

in which G i j k l is a tensor of amplitudes and λ is a positive time constant (relaxation time). In the ∞

current implementation, it is assumed that the time constant is isotropic. In Equation (7-238), G i j k l represents the long term modulus of the material. The short term moduli (describing the instantaneous elastic effect) are then given by N

∞

0

∑

Gi j k l = Gi j k l ( 0 ) = Gi j k l +

n

Gi j k l

(7-239)

n = 1

The stress can now be considered as the summation of the stresses in a generalized Maxwell model (Figure 7-63) ∞ σi j ( t )

σi j ( t ) =

N

+

n

∑

σi j ( t )

(7-240)

n = 1

where ∞

∞

σi j = Gi j k l εk l ( t )

(7-241)

t n σi j

=

n

∫ G i j kl exp [ – ( t – τ ) ⁄ λ

n

dε k l ( τ ) ] ------------------ dτ dτ

(7-242)

0

E

∞

E η

1

1

E η

2

2

E η

3

3

E η

N

N

i

i

τ = η ⁄E

i

Figure 7-63 The Generalized Maxwell or Stress Relaxation Form

For integration of the constitutive equation, the total time interval is subdivided into a number of subintervals ( t m – 1, t m ) with time-step Δt = t m – t m – 1 . A recursive relation can now be derived expressing the stress increment in terms of the values of the internal stresses σ inj at the start of the interval. With the assumption that the strain varies linearly during the time interval Δt , we obtain the increment stress-strain relation as

Main Index

468 Marc Volume A: Theory and User Information

N

∞

Δσ i j ( t m ) =

N n

n

∑

Gi j k l +

β ( Δt )G i j k l Δε k l –

n = 1

∑

n

n

α ( Δt )σ i j ( t m – Δt )

(7-243)

n = 1

where n

α n ( Δt ) = 1 – exp ( – ( Δt ) ⁄ λ )

(7-244)

and n

n

n

β ( Δt ) = α ( Δt )λ ⁄ ( Δt )

(7-245)

In Marc, the incremental equation for the total stress is expressed in terms of the short term moduli (See Equation (7-239)). N

Δσ i j ( t m ) =

0 Gi j k l

–

∑

N

{1 – β

n

n ( Δt ) }G i j k l

n = 1

Δε k l ( t m ) –

∑

n

n

α ( Δt )σ i j ( t m – Δt )

(7-246)

n = 1

In this way, the instantaneous elastic moduli can be specified through the ISOTROPIC or ORTHOTROPIC options. Moreover, since the TEMPERATURE EFFECTS or TABLE option acts on the instantaneous elastic moduli, it is more straightforward to use the short term values instead of the long term ones. Note that the set of equations given by Equation 7-246 can directly be used for both anisotropic and isotropic materials. Isotropic Viscoelastic Material For an isotropic viscoelastic material, Marc assumes that the deviatoric and volumetric behavior are fully decoupled and that the behavior can be described by a time dependent shear and bulk modules. The bulk moduli is generally assumed to be time independent; however, this is an unnecessary restriction of the general theory. Both the shear and bulk moduli can be expressed in a Prony series N

∞

G(t) = G +

∑

n

n

n

n

G exp ( – t ⁄ λ d )

(7-247)

n = 1 ∞

N

K(t) = K +

∑

K exp ( – t ⁄ λ v )

(7-248)

n = 1

with short term values given by N

G0

=

G∞

+

∑ n = 1

Main Index

Gn

(7-249)

CHAPTER 7 469 Material Library

N

K0

=

K∞

∑

+

Kn

(7-250)

n = 1

Let the deviatoric and volumetric component matrices π d and π v be given by 4 ⁄ 3 –2 ⁄ 3 –2 ⁄ 3 –2 ⁄ 3 πd =

πv =

0

0

0

0

0

0

4⁄3

0

0

0

4 ⁄ 3 –2 ⁄ 3

–2 ⁄ 3 –2 ⁄ 3 0

0

0

1

0

0

0

0

0

0

1

0

0

0

0

0

0

1

1 1 1 0 0 0

1 1 1 0 0 0

1 1 1 0 0 0

0 0 0 0 0 0

0 0 0 0 0 0

(7-251)

0 0 0 0 0 0

The increment set of equations is then given by ⎧ ⎪ 0 Δσ ( t m ) = ⎨ G – ⎪ ⎩ ⎧ ⎪ 0 ⎨K – ⎪ ⎩

⎫

Nd

∑

[1 –

n⎪ n β d ( Δt ) ]G ⎬π d Δε ( t m )

⎪ ⎭

n = 1 N

⎫

v

∑

[1 –

⎪ ⎭

n = 1

Nd

–

∑

(7-252)

n⎪ n β v ( Δt ) ]K ⎬π v Δε ( t m ) Nv

n n α d ( Δt )σ d ( t m

– Δt ) –

n = 1

∑

n

n

α v ( Δt )σ v ( t m – Δt )

n = 1

and n

n

n

n

n

n

n

n

n

n

Δσ d ( t m ) = β d ( Δt )G π d Δε ( t m ) – α d ( Δt )σ d ( t m – Δt ) Δσ v ( t m ) = β v ( Δt )K π v Δε ( t m ) – α v ( Δt )σ v ( t m – Δt ) Note that the deviatoric and volumetric response are fully decoupled.

Main Index

(7-253)

470 Marc Volume A: Theory and User Information

The instantaneous moduli need to be given in the ISOTROPIC option. Time dependent values (shear n

n

n

moduli G n and time constants λ d ; bulk moduli K and time constants λ v ) need to be entered in the VISCELPROP option.

Time-stepping is performed using the TIME STEP or AUTO STEP option in the history definition block. Note that the algorithm is exact for linear variations of the strain during the increment. The algorithm is implicit; hence, for each change in time-step, a new assembly of the stiffness matrix is required. Anisotropic Viscoelastic Material Equation 7-243 can be used for the analysis of anisotropic viscoelastic materials. The tensor of n

0

amplitudes G i j k l must be entered through the ORTHOTROPIC option. However, both the G i j k l and the n

λ must be entered using the VISCELORTH option. Alternatively, a complete set of moduli (21 components) can be specified in the HOOKVI user subroutine. The ORIENTATION option or ORIENT user subroutine can be used to define a preferred orientation both n

0

for the short time moduli G i j k l and the amplitude functions G i j kl . Incompressible Isotropic Viscoelastic Materials Incompressible elements in Marc allow the analysis of incompressible and nearly incompressible materials in plane strain, axisymmetric and three-dimensional problems. The incompressibility of the element is simulated through the use of an perturbed Lagrangian variational principle based on the Herrmann formulation. The constitutive equation for a material with no time dependence in the volumetric behavior can be expressed as ⎧ ⎪ 0 Δσ i j ( t m ) = 2 ⎨ G i j kl – ⎪ ⎩

⎫

N

∑ n = 1

[1 – β

n

n ⎪ ( Δt ) ]G i j k l ⎬

1 Δε k l ( t m ) – --- Δε p p ( t m )δ k l 3 ⎪ ⎭

(7-254)

N

–

∑

n n 1 α ( Δt ) ( σ′i j ) ( t m ) + --- σ k k δ i j 3

n = 1 0

Δσ p p ( t m ) = 3K Δε p p ( t m )

(7-255)

The hydrostatic pressure term is used as an independent variable in the variational principle. The Herrmann pressure variable is now defined in the same way as in the formulation for time independent elastic materials.

Main Index

CHAPTER 7 471 Material Library

σp p H = -------------------------------2G 0 ( 1 + ν 0 )

(7-256)

The constitutive Equations (7-254) and (7-255) can then be rewritten N e

Δσ i j ( t m ) = 2G ( Δε i j + ν∗ Hδ i j ) –

∑

n

d n

α ( Δt ) ( σ i j ) ( t m – Δt )

(7-257)

n = 1

where N

Ge

=

G0

–

∑

[ 1 – β n ( Δt )G n ]

(7-258)

n = 1 0

0

e

0

G ( 1 + ν ) – G ( 1 – 2ν ) ν∗ = ------------------------------------------------------------------e 3G

(7-259)

Thermo-Rheologically Simple Behavior The rate processes in many viscoelastic materials are known to be highly sensitive to temperature changes. Such temperature-dependent properties cannot be neglected in the presence of any appreciable temperature variation. For example, there is a large class of polymers which are adequately represented by linear viscoelastic laws at uniform temperature. These polymers exhibit an approximate translational shift of all the characteristic response functions with a change of temperature, along a logarithmic time axis. This shift occurs without a change of shape. These temperature-sensitive viscoelastic materials are characterized as Thermo-Rheologically Simple. A “reduced” or “pseudo” time can be defined for the materials of this type and for a given temperature field. This new parameter is a function of both time and space variables. The viscoelastic law has the same form as one at constant temperature in real time. If the shifted time is used, however, the transformed viscoelastic equilibrium and compatibility equations are not equivalent to the corresponding elastic equations. In the case where the temperature varies with time, the extended constitutive law implies a nonlinear dependence of the instantaneous stress state at each material point of the body upon the entire local temperature history. In other words, the functionals are linear in the strains but nonlinear in the temperature. The time scale of experimental data is extended for Thermo-Rheologically Simple materials. All characteristic functions of the material must obey the same property. The shift function is a basic property of the material and must be determined experimentally. As a consequence of the shifting of the mechanical properties data parallel to the time axis (see Figure 7-64), the values of the zero and infinite frequency complex moduli do not change due to shifting. Hence, elastic materials with temperature-dependent characteristics neither belong to nor are consistent with the above hypothesis for the class of Thermo-Rheologically Simple viscoelastic solids.

Main Index

472 Marc Volume A: Theory and User Information

T0 f(T1) T2

GT

T1

f(T2)

ln t

Figure 7-64 Relaxation Modulus vs. Time at Different Temperatures

Let E ( ln t ) be the relaxation modulus as a function of ln t at uniform temperature, T . Then E T ( ln t ) = E T [ ln t+f ( T ) ]* ( ρT ⁄ ρ 0 T 0 ) 0

(7-260)

where f ( T ) is measured relative to some arbitrary temperature T . The modulus curve shifts towards shorter times with an increase of temperature; f ( T ) is a positive increasing function for T > T 0 . If G T ( t ) denotes the relaxation modulus as a function of time at uniform temperature T , so that, G T ( t ) = E T ( ln t )

(7-261)

then GT ( t ) = GT ( ξ ) 0

(7-262)

The relaxation modulus (and the other characteristic functions) at an arbitrary uniform temperature is thus expressed by the base temperature behavior related to a new time scale that depends on that temperature. There is some mapping of the time coordinate for nonuniform, nonconstant temperature, T ( x, t ) , which depends on the position For a nonuniform, nonconstant temperature, the shift function is a ( T ( x, t ) ) and the rate of change of reduced time can be written as: dξ = a T [ T ( x ,t ) ]dt Marc offers two explicit forms for entering the shift function. The first is based on the familiar WilliamsLandel-Ferry (WLF) equation. Rewriting the above expression for reduced time as t

ξ ( x, t ) =

dt′

∫ α------------------------------T [ T ( x, t′ ) ]

0

then the WLF form state that

Main Index

(7-263)

CHAPTER 7 473 Material Library

– C 1 ( T – T0 ) log 10aT ( T ) = ------------------------------------ = – h ( T ) C2 + ( T – T 0 )

(7-264)

and t

ξ( t) =

∫ 10

h[T(t′)]

dt′

(7-265)

0

Typically, the glassy transition point is taken as the reference temperature in the above relation. The logarithmic shift can also be expressed in a polynomial expansion about the arbitrary reference point as m

∑

log 10 A T ( T ) =

αi ( T – T 0 )

i

(7-266)

i = 0

Enter the shift function parameters associated with Thermo-Rheologically Simple behavior through the SHIFT FUNCTION model definition option. As an alternative to the WLF function, Marc allows use of series expansion or specification via the TRSFAC user subroutine.

In addition to the Thermo-Rheologically Simple material behavior variations of initial stress-strain 0

moduli G i j k l , the temperature of the other mechanical properties (coefficient of thermal expansion, etc.) due to changes in temperature can be specified via the TEMPERATURE EFFECTS option. Note, however, that only the instantaneous moduli are effected by the TEMPERATURE EFFECTS option. Hence, the long term moduli given by ∞ Gi j k l

N

=

0 Gi j k l ( t )

–

n

∑

(7-267)

Gi j k l

n = 1

can easily become negative if the temperature effects are not defined properly. Large Strain Viscoelasticity For an elastomeric time independent material, the constitutive equation is expressed in terms of an energy function W . For a large strain viscoelastic material, Simo generalized the small strain viscoelasticity material behavior to a large strain viscoelastic material. The energy functional then becomes N n ψ ( Ei j Qi j )

0

= ψ ( Ei j ) –

∑ n = 1

N n Qi j Ei j

+

∑

n

n

ψI ( Qi j )

(7-268)

n = 1 n

0

where E i j are the components of the Green-Lagrange strain tensor, Q i j internal variables and ψ the elastic strain energy density for instantaneous deformations. In Marc, it is assumed that ψ

Main Index

0

= W,

474 Marc Volume A: Theory and User Information

meaning that the energy density for instantaneous deformations is given by the third order James-GreenSimpson form or the Ogden form. When used with Updated Lagrange, one can also use the ArrudaBoyce or Gent model. The components of the second Piola-Kirchhoff stress then follow from

Si j

∂ψ ∂ψ 0 = ---------- = ---------- – ∂E i j ∂E i j

N n

∑

(7-269)

Qi j

n = 1

The energy function can also be written in terms of the long term moduli resulting in a different set of n

internal variables T i j N n ψ ( E i j, T i j )

ψ∞(E

=

ij)

+

∑

n

Ti j Ei j

(7-270)

n = 1 ∞

where ψ is the elastic strain energy for long term deformations. Using this energy definition, the stresses are obtained from

Si j

∂ψ ∞ ( E ) = -------------------- + ∂E i j

N

∑

n

Ti j

(7-271)

n = 1

Let the total strain energy be expressed as a Prony series expansion N

ψ = ψ∞ +

∑

ψ n exp ( – t ⁄ λ n )

(7-272)

n = 1

If, in the energy function, each term in the series expansion has a similar form, Equation (7-272) can be rewritten as N ∞

∑

ψ = ψ +

δ n ψ 0 exp ( – t ⁄ λ n )

(7-273)

n = 1 n

where δ is a scalar multiplier for the energy function based on the short term values. The stress-strain relation is now given by

Si j =

∞ Si j

N

+

∑ n = 1

Main Index

n

Ti j

(7-274)

CHAPTER 7 475 Material Library

⎛ ∞ ∂ψ ∞ S i j = ----------- = ⎜ 1 – ⎜ ∂E i j ⎝

⎞ ∂ψ 0 n⎟ --------δ ∑ ⎟ ∂E i-j n = 1 ⎠ N

(7-275)

Observing the similarity with the equations for small strain viscoelasticity, the internal variables can be obtained from a convolution expression t

n

Ti j =

n ·0 n δ ∫ S i j ( τ )exp [ – ( t – τ ) ⁄ λ ]dτ

(7-276)

0

Analogue to the derivation for small strain viscoelasticity, a recursive relation can be derived expressing the stress increment in terms of values of the internal stresses at the start of the increment. In Marc, the instantaneous values of the energy function are always given on the MOONEY, OGDEN, or FOAM option, the equations are reformulated in terms of the short time values of the energy function N ⎛ ⎞ 0 0 ⎜ ΔS i j ( t m ) = 1 – ∑ [ 1 – β n ( Δt ) ] δ n⎟ { S i j ( t m ) – S i j t m – Δt } ⎜ ⎟ ⎝ n=1 ⎠ N

–

∑

(7-277)

n

α n ( Δt )T i j ( t m – Δt )

n = 1 n

0

0

n

ΔT i j ( t m ) = β n ( Δt )δ n [ S i j ( t m ) – S i j ( t m – Δt ) ] – α n ( Δt )T i j ( t m – Δt )

(7-278)

It is assumed that the viscoelastic behavior in Marc acts only on the deviatoric behavior. The incompressible behavior is taken into account using special Herrmann elements. Large strain viscoelasticity is invoked by use of the VISCELMOON, VISCELOGDEN, or VISCELFOAM n

option in the constitutive option of the model definition block. The time dependent multipliers δ and n

associated relaxation times λ as defined by Equation 7-265 are given in the VISCELMOON, VISCELOGDEN, or VISCELFOAM option. For the Ogden model, both deviatoric and dilatational relaxation behavior is allowed. Viscoelasticity can be modeled with Arruda-Boyce and Gent models using VISCELMOON option. Time-stepping can be performed using the TIME STEP with AUTO LOAD or AUTO STEP option of the history definition block. The free energy function versus time data being used for large strain viscoelasticity can be generated by fitting the experimental data in Marc Mentat or MD Patran provided the following two tests are done: 1. Standard quasi-static tests (tensile, planar-shear, simple-shear, equi-biaxial tension, volumertic) 0 to determine the elastomer free energy W constants. 2. Standard relaxation tests to obtain stress versus time.

Main Index

476 Marc Volume A: Theory and User Information

Narayanaswamy Model The annealing of flat glass requires that the residual stresses be of an acceptable magnitude, while the specification for optical glass components usually includes a homogenous refractive index. The design of heat treated processes (for example, annealing) can be accomplished using the Narayanaswamy model. This allows you to study the time dependence of physical properties (for example, volumes) of glass subjected to a change in temperature. The glass transition is a region of temperature in which molecular rearrangements occur on a scale of minutes or hours, so that the properties of a liquid change at a rate that is easily observed. Below the glass transition temperature T g , the material is extremely viscous and a solidus state exists. Above T g , the equilibrium structure is arrived at easily and the material is in liquidus state. Hence, the glass transition is revealed by a change in the temperature dependence of some property of a liquid during cooling. If a mechanical stress is applied to a liquid in the transition region, a time-dependent change in dimensions results due to the phenomenon of visco-elasticity. If a liquid in the transition region is subjected to a sudden change in temperature, a time-dependent change in volume occurs as shown in Figure 7-65. The latter process is called structural relaxation. Hence, structural relaxation governs the time-dependent response of a liquid to a change of temperature. T1 T(t)

T2

t0 t (a) Step Input for Temperature

V(0,T1)

αg(T2-T1) αl(T2-T1)

V(0,T2)

V(∞,T2)

t0

t

(b) Volume Change as Function of Temperature

Figure 7-65 Structural Relaxation Phenomenon

Suppose a glass is equilibrated at temperature T 1 , and suddenly cooled to T 2 at t 0 . The instantaneous change in volume is α g ( T 2 – T 1 ) , followed by relaxation towards the equilibrium value V ( ∞, T 2 ) . The total change in volume due to the temperature change is α 1 ( T 2 – T 1 ) as shown in Figure 7-65b. The rate of volume change depends on a characteristic time called the relaxation time.

Main Index

CHAPTER 7 477 Material Library

The slope of dV ⁄ dT changes from the high value characteristic of the fluid α 1 to the low characteristic of the glass α g as shown in Figure 7-66. The glass transition temperature T g is a point in the center of the transition region. The low-temperature slope α g represents the change in volume V caused by vibration of the atoms in their potential wells. In the (glassy) temperature range, the atoms are frozen into a particular configuration. As the temperature T increases, the atoms acquire enough energy to break bonds and rearrange into new structures. That allows the volume to increase more rapidly, so α 1 > α g . The difference α = α 1 – α g represents the structural contribution to the volume. V(T)

αl

V(T0)

Liquid State

V(T1) αg

Transition Range Solidus State T0 T2

Tf (T1): Fictive Temperature

T1 Tg Tf(T1)

Figure 7-66 Property (Volume) – Temperature Plot

When a liquid is cooled and reheated, a hysteresis is observed as shown in Figure 7-67. V Equilibrium

Nonequilibrium

Tg

T

Figure 7-67 Volume Change During Cyclic Temperature History

Unfortunately, the notion of a glass transition temperature is insufficient as real glassy materials generally exhibit a temperature regime, called a transition range, across which their bulk properties gradually change from being solid-like to liquid-like in nature. As discussed earlier, properties have a time dependence in the transition range. An explanation for the strong time dependence lies in that the material resides at a nonequilibrium temperature which lags behind the applied temperature during the heating-cooling cycle. The nonequilibrium temperature is

Main Index

478 Marc Volume A: Theory and User Information

called the fictive temperature, T f , as shown in Figure 7-66. The fictive temperature at T 1, T f ( T 1 ) is found by extrapolating a line from V ( T 1 ) with slope α g to intersect a line extrapolated from V ( T 0 ) with slope α 1 (see Figure 7-66). For T ≤ T 2 (well below the glass transition), T f reaches a limiting value that is called T g . If the material were equilibrated at T f ( T 1 ) , then instantaneously cooled to T 1 , it would change along the line with slope α g because no structural rearrangement could occur. Therefore, it would have the same volume as the continuously cooled sample. The response of the volume change can be described by: V ( T 2 ,t ) = V ( T 1 ,∞ ) + α g ( T 2 – T 1 ) + ( α l – α g ) ( T f ( t ) – T 2 )

(7-279)

where T f ( t ) is the current value of the fictive temperature. The response function, M v , which dictates the value of the fictive temperature is assumed to be linear in its argument and governs both the value of the fictive temperature as well as the material property of interest. Tf ( t ) – T ( ∞ ) V(t ) – V( ∞) --------------------------------- = M v ( ξ ( t ) ) = --------------------------------V(0 ) – V( ∞) T(0 ) – T( ∞)

(7-280)

By virtue of its linearity, Boltzmann’s superposition principle can be invoked to calculate the fictive temperature at any time: t

Tf ( t ) = T ( t ) –

∫ –∞

d M v ( ξ ( t ) – ξ ( t′ ) ) -------(T ( t′ )) ( dt' ) dt′

(7-281)

The concept of reduced time, ξ ( t ) , is introduced in the spirit of Thermo-Rheologically Simple materials to capture the disparate nonlinear response curves on a single master curve. The reduced time used in Marc is given by the following expression: t

ξ( t) =

∫ –∞

τ re f --------------------- dt′ τ ( T ( t′ ) )

(7-282)

Here τ ref is the reference relaxation time of the material evaluated at a suitable reference temperature, T ref . The relaxation time τ at the given time and temperature can be represented as: H 1 x (1 – x) τ = τ re f ⋅ exp ⎛ – ---- ---------- – --- – ------------------ ⎞ ⎝ R Tr e f T ⎠ Tf The parameter x allows you to dictate how much of the fictive temperature participates in the prescription of the relaxation time, and must, therefore, range between 0 and 1.

Main Index

(7-283)

CHAPTER 7 479 Material Library

H is the activation energy for the particular process and R is the gas constant. A typical response function is: ξ M v ( ξ ) = exp ⎛ – --⎞ ⎝ τ⎠

(7-284)

Multiple structural relaxation times can exist. The response function has, therefore, been implemented as: n

Mv ( ξ ) =

∑ i = 1

ξ ( W g ) i ⋅ exp ⎛ – ----⎞ ⎝ τ i⎠

For a complete description of the model, it is necessary to prescribe the following: 1. The weight ( W g ) i for each term in the series (usually

∑ ( W g ) i ≈ 1 ).

2. The reference relaxation times τ i, ref . 3. The fraction parameter x and the activation energy-gas constant ratio. 4. The solid and liquid coefficients of thermal of expansion, α g and α 1 through the VISCEL EXP option.

A stable algorithm is employed to calculate the convolution integrals. For improved accuracy it is recommended that the time steps used during the simulation be sufficiently small.

Volume

In Figure 7-68, the volume of cube of material, which is allowed to contract freely and is experiencing a 100oC quench, is displayed. ΔT=100 αgΔT αlΔT

Temperature Tim

e

Figure 7-68 Volume-Temperature-Time Plot

Temperature Effects and Coefficient of Thermal Expansion Experimental results indicate that a large number of material properties vary with temperatures. In Marc, almost all material parameters may be a function of temperatures when using the table driven input procedure. A subset of which are shown in Table 7-4 for different types of analysis.

Main Index

480 Marc Volume A: Theory and User Information

7

Material Library

Table 7-4

Temperature-Dependent Material Properties

Analysis Type Stress Analysis

Material Properties Modulus of elasticity (Young’s Modulus) E ( T ) Poisson’s Ratio

ν(T)

Yield Stress

σy ( T )

Workhardening Slope h ( T ) Coefficient of Thermal Expansion α ( T ) Mooney Constants

C 01 ( T ), C 10 ( T ) C 11 ( T ), C 20 ( T ) C 30 ( T )

Heat Transfer Analysis

Thermal Conductivity K ( T ) Specific Heat

C(T)

Emissivity

ε(T)

Couples Thermo-Electrical (Joule Heating Analysis)

Electric Resistivity

π(T)

Hydrodynamic Heating

Viscosity

μ( T)

Please note that T is temperature in the above expressions. With the exception of heat transfer, Joule heating, or coupled thermal-mechanical analysis, the temperature is a state variable.

Piecewise Linear Representation In Marc, the temperature variation of a material constant F ( T ) may be entered as a piecewise linear function of temperature as shown in Figure 7-69 or as an equation. The base value or reference value is entered in the ISOTROPIC, ORTHOTROPIC, ANISOTROPIC, MOONEY, OGDEN, etc. model definition options. Using the nontable input format, these should be at the lowest temperatures. The variation with temperature is entered on the TEMPERATURE EFFECTS and ORTHO TEMP or TABLE model definition options.

Main Index

CHAPTER 7 481 Material Library

Temperature Dependent Property

F(T)

F4

F3 S3 F2

F1

S2

S1

Base Value F1

T4 T1

T2

T3

Temperature (T)

(1) Slope-Break Point Data Slope

Break Point

S1 = (F2 - F1)/(T2 - T1) S2 = (F3 - F2)/(T3 - T2) S3 = (F4 - F3)/(T4 - T3) (2) Function-Variable Data Function F1 F2 F3 F4

T1 T2 T3 Variable T1 T2 T3 T4

Figure 7-69 Piecewise Linear Representation of Temperature-Dependent Material Properties

Temperature-Dependent Creep In Marc, the temperature dependency of creep strain can be entered in two ways. The creep strain rate · may be entered as a piecewise linear function. If the creep strain ε c can be expressed in the form of a power law ·c ε = AT m

(7-285)

where A and m are two experimental constants, input the experimental constants through the CREEP model definition option.

Main Index

482 Marc Volume A: Theory and User Information

For other temperature dependency, you may use an equation or use the CRPLAW user subroutine for explicit creep and UCRPLW user subroutine for implicit creep to input the variation of creep strain with temperature.

Coefficient of Thermal Expansion Marc always uses an instantaneous thermal expansion coefficient definition th

dε i j = α i j dT

in general

(7-286)

or th

dε i j = α dT δ i j

for the isotropic case

(7-287)

In many cases, the thermal expansion data is given with respect to a reference temperature εth = α( T – T0 )

(7-288)

where a is a function of temperature: α = α(T)

(7-289)

Clearly, in this case dε t h =

dα α + ------- ( T – T 0 ) dT dT

(7-290)

so the necessary conversion procedure is: 1. Compute and plot Equation (7-288) in the form Equation (7-290) dα α = α + ------- ( T – T 0 ) dT

(7-291)

as a function of temperature. 2. Model Equation (7-291) in the ANEXP user subroutine, or with piecewise linear slopes and breakpoints in the TEMPERATURE EFFECTS or TABLE option. The anisotropic coefficient of thermal expansion can be input through either the ORTHOTROPIC model definition option or the ANEXP user subroutine.

Time-Temperature-Transformation Certain materials, such as carbon steel, exhibit a change in mechanical or thermal properties when quenched or air cooled from a sufficiently high temperature. At any stage during the cooling process, these properties are dependent on both the current temperature and the previous thermal history. The properties are influenced by the internal microstructure of the material, which in turn depends on the rate at which the temperature changes. Only in instances where the temperature is changed very gradually does the material respond in equilibrium, where properties are simply a function of the current

Main Index

CHAPTER 7 483 Material Library

temperature. In addition, during the cooling process certain solid-solid phase transformations can occur. These transformations represent another form of change in the material microstructure which can influence the mechanical or thermal properties. These transformations can be accompanied by changes in volume. The occurrence of phase change is also dependent on the rate of cooling of the material. This relationship is shown in a typical cooling diagram (see Figure 7-70). The curves A, B, and C in Figure 7-70 represent the temperature history of a structure that has been subjected to a different cooling rate. It is obvious that the structural material experiences phase changes at different times and temperatures, depending on the rate of cooling. Under cooling rate A, the material changes from phase 1 to phase 4 directly. The material undergoes three phase changes (phase 1 to phase 2 to phase 3 to phase 4) for both cooling rates B and C. However, the phase changes take place at different times and temperatures. The Time-Temperature-Transformation (TIME-TEMP) option allows you to account for the time-temperature-transformation interrelationships of certain materials during quenching or casting analyses. Use the T-T-T parameter to invoke the time-temperature-transformation. Input all the numerical data required for this option through the TIME-TEMP model definition option. In a transient heat transfer analysis, the thermal properties which can be defined as a function of time and temperature are the thermal conductivity and the specific heat per unit reference mass. Here, the effects of latent heat or phase transformation can be included through the definition of the specific heat. In a thermal stress analysis, the mechanical properties which can be defined as a function of time and temperature are the Young’s modulus, Poisson’s ratio, yield stress, workhardening slope, and coefficient of thermal expansion. The effects of volumetric change due to phase transformation can be included through the definition of the coefficient of thermal expansion. A

T1

T1 B

C

Temperature (T)

T4

Line of Phase Change – Change in Volume

T5

T3

T3

T2 t1

T2 t2

Time (t)

Figure 7-70 Simplified Cooling Transformation Diagram

Main Index

484 Marc Volume A: Theory and User Information

Test data must be available in a tabular form for each property of each material group. For a given cooling rate, the value of a property must be known at discrete points over a range of temperatures. There can be several sets of these discrete points corresponding to measurements at several different cooling rates. The cooling tests must be of a specific type known as Newton Cooling; that is, the temperature change in the material is controlled such that T ( t ) = A exp ( – at ) + B

(7-292)

In addition, a minimum and a maximum temperature that bracket the range over which the TIME-TEMP option is meant to apply must also be given. For the simulation of the cooling rate effect in finite element analysis, material properties of a structure can be assumed as a function of two variables: time and temperature. Two-dimensional interpolation schemes are used for the interpolation of properties. Interpolation is based on making the time variable discrete. Stress analysis is carried out incrementally at discrete time stations and material properties are assumed to vary piecewise linearly with temperature at any given time. These temperature-dependent material properties are updated at each increment in the analysis. For illustration, at time t 1 , the material is characterized by the phase 1 and phase 4 behaviors at temperature ranges T 1 to T 3 , and T 3 to T 2 , respectively (see Figure 7-71). Similarly, at time t 2 , the material behavior must be characterized by all four phases, each in a different temperature range (that is, phase 1, T 1 to T 4 ; phase 2, T 4 to T 5 ; phase 3, T 5 to T 3 ; phase 4, T 3 to T 2 ). The selection of an interpolation scheme is generally dependent on the form of the experimental data. A linear interpolation procedure can be effectively used where the properties are expressed as a tabulated function of time and temperature. During time-temperature-transformation, the change in volume in a stress analysis is assumed to take place in a temperature range ΔT . The change in volume is also assumed to be uniform in space, such that the effect of the volume change can be represented by a modification of the coefficient of thermal expansion. For a triangular distribution of α ( T ) in the temperature range ΔT , the value of the modified coefficient of thermal expansion is 2 α m = ------- [ 3 1 + φ – 1 ] ΔT where φ is the change in volume. A schematic of the modified α ( T ) is shown in Figure 7-71.

Main Index

(7-293)

CHAPTER 7 485 Material Library

Coefficient of thermal Expansion (α)

ΔT

Temperature (T)

αm

Figure 7-71 Modified Coefficient of Thermal Expansion for Short-Time Change in Volume

Low Tension Material Marc can handle concrete and other low tension material. The CRACK DATA option assists in predicting crack initiation and in simulating tension softening, plastic yielding and crushing. This option can be used for the following: • Elements with a one-dimensional stress-strain relation (beam and truss elements) • Elements with a two-dimensional stress-strain relation (plane stress, plane strain, axisymmetric, and shell elements) • Three-dimensional elements (bricks) Analytical procedures that accurately determine stress and deformation states in concrete structures are complicated by several factors. Two such factors are the following: • The low strength of concrete in tension that results in progressive cracking under increasing loads • The nonlinear load-deformation response of concrete under multiaxial compression Because concrete is mostly used in conjunction with steel reinforcement, an accurate analysis requires consideration of the components forming the composite structure. Steel reinforcement bars are introduced as rebar elements. Each rebar element must be input with a separate element number. The REBAR model definition option or REBAR user subroutine is used to define the orientation of the reinforcement rods.

Uniaxial Cracking Data The cracking option is accessed through the ISOTROPIC option. Uniaxial cracking data can be specified using the CRACK DATA option or the UCRACK user subroutine. When the CRACK DATA option is used to specify uniaxial cracking data, the following must be specified: the critical cracking stress, the modulus of the linear strain softening behavior, and the strain at which crushing occurs. Material properties, such as Young’s modulus and Poisson’s ratio, are entered using the ISOTROPIC option and

Main Index

486 Marc Volume A: Theory and User Information

the WORK HARD option. This model is for a material which is initially isotropic; if the model is initially orthotropic, see FAIL DATA for an alternative cracking model. A typical uniaxial stress-strain diagram is shown in Figure 7-72.

σcr Es

εcrush

ε

E

σy Workhardening

E Es σy σcr εcrush

Young’s Modulus Tension-Softening Modulus Yield Stress Critical Cracking Stress Crushing Strain

Figure 7-72 Uniaxial Stress-Strain Diagram

Low Tension Cracking A crack develops in a material perpendicular to the direction of the maximum principal stress if the maximum principal stress in the material exceeds a certain value (see Figure 7-73). After an initial crack has formed at a material point, a second crack can form perpendicular to the first. Likewise, a third crack can form perpendicular to the first two. The material loses all load-carrying capacity across the crack unless tension softening is included.

Tension Softening If tension softening is included, the stress in the direction of maximum stress does not go immediately to zero; instead the material softens until there is no stress across the crack. At this point, no load-carrying capacity exists in tension (see Figure 7-73). The softening behavior is characterized by a descending branch in the tensile stress-strain diagram, and it may be dependent upon the element size.

Main Index

CHAPTER 7 487 Material Library

σ2

y

σ1

θ x

σ1

σ2

Figure 7-73 Crack Development

Crack Closure After a crack forms, the loading can be reversed; therefore, the opening distance of a crack must be considered. In this case, the crack can close again, and partial mending occurs. When mending occurs, it is assumed that the crack has full compressive stress-carrying capability and that shear stresses are transmitted over the crack surface, but with a reduced shear modulus.

Crushing As the compressive stress level increases, the material eventually loses its integrity, and all load-carrying capability is lost; this is referred to as crushing. Crushing behavior is best described in a multiaxial stress state by a crushing surface having the same shape as the yield surface. The failure criterion can be used for a two-dimensional stress state with reasonable accuracy. For many materials, experiments indicate that the crushing surface is roughly three times larger than the initial yield surface.

Analysis The evolution of cracks in a structure results in the reduction of the load carrying capacity. The internal stresses need to be redistributed through regions that have not failed. This is a highly nonlinear problem and can result in the ultimate failure of the structure. The AUTO INCREMENT or AUTO STEP option should be used to control the applied load on the structure.

Soil Model Soil material modeling is considerably more difficult than conventional metals, because of the nonhomogeneous characteristics of soil materials. Soil material usually consists of a large amount of random particles. Soils show unique properties when tested. The bulk modulus of soil increases upon pressing. Also, when the preconsolidation stress is exceeded, the stiffness reduces dramatically while the stiffness increases upon unloading. At failure, there is no resistance to shear, and stiff clays or dense sands are dilatant. Over the years, many formulations have been used, including linear elastic, nonlinear elastic, Drucker-Prager or Mohr Coulomb, and Cam-Clay and variations thereof. In Marc, the material models for available soil modeling are linear elasticity, nonlinear elasticity, and the Cam-Clay model.

Main Index

488 Marc Volume A: Theory and User Information

Elastic Models Linear elasticity is defined in the conventional manner, defining the Young’s moduli and the Poisson’s ratio in the SOIL option. The nonlinear elasticity model is implemented through the NLELAST option or the HYPELA2 user subroutine. Some of the simplest models include the bilinear elasticity, where a different moduli is used during the loading and unloading path, or to represent total failure when a critical stress is obtained. A more sophisticated elastic law is the hyperbolic model, where six constants are used. In this model, the tangent moduli are E =

R f ( 1 – sin φ ) ( σ 1 – σ 3 ) 1 – --------------------------------------------------------2c cos φ + 2σ 3 sin φ

2

σ n ⎛ -----3-⎞ ⎝ pa⎠

(7-294)

Two of the elastic models are the E-ν and K-G variable elastic models. In the E-ν model, Poisson’s ratio is considered constant and E = E0 + α E p + βE τ

(7-295)

while, in the K-G model K = K0 + αK p

(7-296)

G = G0 + αG p + βG τ

(7-297)

The key difficulty with the elastic models is that dilatancy cannot be represented.

Cam-Clay Model The Cam-Clay model was originally developed by Roscoe, and then evolved into the modified Cam-Clay model of Roscoe and Burland. This model, which is also called the critical state model, is implemented in Marc. The yield surface is an ellipse in the p,τ plane as shown in Figure 7-74, and is defined by τ2 F = ---------- – 2pp c + p 2 = 0 M c2s

(7-298)

where p c is the preconsolidation pressure, and M c s is the slope of the critical state line. The Cam-Clay model has the following no properties. At the intersection of the critical state line and the ellipse, the normal to the ellipse is vertical. Because an associated flow rule is used, all plastic strain at failure is distortional; the soil deforms at constant volume (Figure 7-74). The strain hardening and softening behavior are shown in Figure 7-75. Also, if the preconsolidation pressure is large, the soil remains elastic for large stresses. The evolution of the preconsolidation pressure is · p· c = – θp c tr ( ε p l )

Main Index

(7-299)

CHAPTER 7 489 Material Library

where 1+e θ = ------------λ–κ

(7-300)

where e

is the void ratio

λ

is the virgin compression index (see Figure 7-76)

κ

is the recompression index (see Figure 7-76)

τ (εq)

Critical State Line Strain Softening Ceases

Strain Hardening Ceases 2

1 3 Region originally elastic

4

( ε v )p

PC O

Figure 7-74 Modified Cam-Clay Yield Surface q

q 2

3

1 q2

4 q4 εq

Figure 7-75 Strain Hardening and Softening Behavior

Main Index

εq

490 Marc Volume A: Theory and User Information

e

1

κ

1

λ

ln ( – p )

Figure 7-76 Response of Idealized Soil to Hydrostatic Pressure

The void ratio and the porosity are related by the expression e φ = -----------1+e

(7-301)

In the modified Cam-Clay model, it is also assumed that the behavior is nonlinear elastic with a constant Poisson’s ratio, the bulk modulus behave as: 1+e K = – ------------ p κ

(7-302)

Note that this implies that at zero hydrostatic stress, the bulk modulus is also zero. To avoid computational difficulties, a cutoff pressure of one percent of the preconsolidation pressure is used. This constitutive law is implemented in Marc using a radial return procedure. It is available for either small or large strain analysis.When large displacements are anticipated, you should use the LARGE STRAIN parameter. The necessary parameters for the Cam-Clay soil model can be obtained by the following experiments: 1. Hydrostatic test: determines volumetric elastic bulk modulus, yield stress, and the virgin and recompression ratio of soils. 2. Shear-box test: determines the slope of critical state line and shear modulus of the soil. However, the tests have to be calibrated with numerical simulations to get the necessary constants. 3. Triaxial shear test: the most comprehensive experimental information and obviates the need for the first two tests and obtains all the necessary constants listed above.

Evaluation of Soil Parameters for the Critical State Soil Model To illustrate how to extract soil parameters, namely M , κ , and λ , a hypothetical data set for a normally consolidated clay in presented in Figures 7-77 to 7-83. Now we shall use these data to show the procedure of determination of parameters for the critical state model. The data presented here pertain to conventional triaxial conditions. Figures 7-77 and 7-78 show the stress-strain relations for constant pressure tests under different initial conditions p0=10 (69), 20 (139), and 30 (207) psi (kPa), respectively. Here the mean effective pressure

Main Index

CHAPTER 7 491 Material Library

of the soil sample is kept constant throughout the test. The last data point shown on the deviatoric stress (q) versus axial strain (ε1) plot for any test is considered as the ultimate condition for that test. The void ratio values at the beginning and the end of each test are given in Table 7-5. Figures 7-80 to 7-82 show stress-strain relation plots for three fully drained tests performed at initial pressures 10, 20, and 30 psi. Here, there is no pore pressure development, and the effective mean pressure increases during the test. The void ratio values at the beginning and end of each test are given in Table 7-5. Figures 7-83 to 7-85 show stress-strain behavior under undrained conditions. Here there is no change in volume of the sample. However, fluid pore pressure are developed during the test, thereby reducing the effective stresses until the ultimate (failure) state is reached. Figure 7-86 shows the variation of void ratio with mean pressure which is obtained from a hydrostatic compression (HC) test with three load reversals (that is, unloading-reloading cycles). In this figure, void ratio is plotted to a linear scale while the hydrostatic stress is plotted to a logarithmic (base 10) scale. In fact, this is the usual way of presenting one-dimensional consolidation or hydrostatic test results in geotechnical engineering practices. Determination of parameter, M: The parameter M is the slope of the critical state line on a p-q plot. To determine its value, the values of p and q at ultimate conditions for each test are plotted as shown in Figure 7-87; the ultimate condition for each test is assumed to be the last point plotted in Figures 7-77 to 7-85. At the ultimate conditions, the sample undergoes excessive deformations under constant deviatoric stress, and hence it could be taken as the asymptotic stress to the curve. The slope of the critical state line (Figure 7-87) is calculated as 1.0 for the soil above. That is, M = 1.0 . Table 7-5

Main Index

Test Values for Cam Clay Model

Test

Initial Pressure, p0 (effective) (psi)

Initial void Ratio, e0

Final Pressure, pf (effective) (psi)

Final Void Ratio, e1

p-constant

10

1.080

10

0.980

p-constant

20

0.959

20

0.860

p-constant

30

0.889

30

0.787

Drained

10

1.080

15

0.908

Drained

20

0.959

30

0.787

Drained

30

0.889

45

0.716

Undrained

10

1.080

05.55

1.080

Undrained

20

0.959

11.09

0.959

Undrained

30

0.889

16.64

0.889

Deviatoric stress,q = σ 1 – σ 3 (psi)

492 Marc Volume A: Theory and User Information

10 8 6 4 2 0

0.10 Axial strain, ε1 0.10

0.20 0.20

Volumetric strain, ε ν

0.01 0.02 0.03 0.04 0.05

Volumetric strain, εv

Deviatoric stress,q = σ 1 – σ 3(psi)

Figure 7-77 Constant Pressure Test: p0 = 10 psi

25 20 15 10 5 0

0.10 Axial strain, ε1 0.10

0.01 0.02 0.03 0.04 0.05

Figure 7-78 Constant Pressure Test: p0 = 20 psi

Main Index

0.20 0.20

Deviatoric stress, q = σ 1 – σ 3 (psi)

CHAPTER 7 493 Material Library

30 25 20 15 10

5 0.10 Axial strain, ε1 0.10

0.20 0.20

Volumetric strain,

εν

0.01 0.02 0.03 0.04 0.05

16 14 12 10 8 6 4 2 0.10 Axial strain, ε1 0.10

Volumetric strain, ε

ν

Deviatoric stress, q = σ 1 – σ 3 (psi)

Figure 7-79 Constant Pressure Test: p0 = 30 psi

0.02 0.04 0.06 0.08 0.10

Figure 7-80 Drained Test: p0 = 10 psi

Main Index

0.20 0.20

Deviatoric stress, q = σ – σ (psi) 1 3

494 Marc Volume A: Theory and User Information

30

25 20 15

Volumetric strain,

εν

10 5 0.10 Axial strain, ε1 0.10

0.20 0.20

0.02 0.04 0.06 0.08 0.10

Deviatoric stress, q = σ 1 – σ 3(psi)

Figure 7-81 Drained Test: p0 = 20 psi

50

40 30 20 10 0.10 Axial strain, ε1 0.10

Volumetric strain,

εν

0.02 0.04 0.06 0.08 0.10

Figure 7-82 Drained Test: p0 = 30 psi

Main Index

0.20 0.20

Pore pressure, u (psi)

Deviatoric stress, q = σ 1 – σ 3 (psi)

CHAPTER 7 495 Material Library

6 5 4 3 2 1 0.01

0.02 0.03 Axial strain, ε1

0.04

0.01

0.03 0.02 Axial strain, ε1

0.04

6 5 4 3 2 1

Pore pressure, u (psi)

Deviatoric stress, q = σ 1 – σ 3 (psi)

Figure 7-83 Undrained Test: p0 = 10 psi

12 10 8 6 4

2 0.01

0.02 0.03 Axial strain, ε1

0.04

0.01

0.03 0.02 Axial strain, ε1

0.04

10 8 6 4 2

Figure 7-84 Undrained Test: p0 = 20 psi

Main Index

Deviatoric stress, q = σ – σ (psi) 1 3

496 Marc Volume A: Theory and User Information

16 14 12 10 8 6 4 2 0

0.01

0.03 0.02 Axial strain, ε1

0.04

0.01

0.02 0.03 Axial strain, ε1

0.04

Pore pressure, u (psi)

16 14 12 10

8 6 4 2

Figure 7-85 Undrained Test: p0 = 30 psi

1.2

Void ratio, e

1.1

A

1.0

Cc

0.9

0.8

C

B Cs

0.7 10

20 30 40 50 Pressure, p (psi) (logarithmic scale with base 10)

Figure 7-86 Hydrostatic Compression Test: Cc = 0.04, Cs = 0.06

Main Index

CHAPTER 7 497 Material Library

Deviatoric stress, q (psi)

45 40

30 Drained Constant pressure Undrained

20

Slope = M = 1.0

10

0

M 10

20

30

40

50

Mean Pressure, p (psi)

Figure 7-87 Critical State Line in q-p (psi)

Determination of parameters λ and κ: The values of gamma and kappa can be related to the commonly known quantities such as compression index ( C c ) and swelling index ( C s ). The compression index, C c , is defined as the slope of virgin loading line on e-log10p plot while the swelling index, C s , is defined as the unloading-reloading curves on the same plot. Usually, the compression index and swelling index are defined with respect to a one-dimensional consolidation test. However, it can be shown that the e-ln(p) curve for any constant stress ratio test, that is, for constant q/p ratio, is parallel to that obtained from a hydrostatic test, (Figure 7-88). 1.2

e0 vs. p0 ef vs. pf

Void ratio, e

1.1

1.0 Hydrostatic loading 0.9

0.8

At critical state

0.7 20 40 50 30 Pressure (psi) (logarithmic scale with base 10)

60

70

80 90

Figure 7-88 Isotropic Consolidation (Data from 5-8)

In fact, one-dimensional hydrostatic test is parallel to that obtained under critical state conditions. The values of gamma and kappa can be related to C c and C s as follows. The virgin compression line can be expressed as

Main Index

498 Marc Volume A: Theory and User Information

p e – e 0 = C c log 10 ⎛ -----⎞ ⎝ p 0⎠

(7-303)

or p e – e 0 = λ ln ⎛ -----⎞ ⎝ p 0⎠

(7-304)

and the swelling line (unloading-reloading) can be expressed as p e – e 0 = C s log 10 ⎛ -----⎞ ⎝ p 0⎠

(7-305)

or p e – e 0 = κ ln ⎛⎝ -----⎞⎠ p0

(7-306)

Therefore, comparing Equations (7-303) and (7-304), we have Cc Cc λ = ------------- = ------------ln 10 2.303

(7-307)

and comparing Equations (7-305) and (7-306) yields Cs Cs κ = ------------- = ------------ln 10 2.303

(7-308)

The value of C c can be computed by considering two points, A and B, in Figure 7-86 as eA – eB C c = -------------------------------------log p B – log p A 1.08 – 0.08 = ------------------------------------log 50 – log 10 = 0.40

(7-309)

Here the subscript denotes the value at that point. The swelling index, C s , can be computed by considering points B and C of the same figures eC – eB C s = -------------------------------------log p B – log p C 0.842 – 0.80 = ------------------------------------log 50 – log 10 = 0.06

Main Index

(7-310)

CHAPTER 7 499 Material Library

Hence, the values of gamma and kappa can be computed from Equations (7-307) and (7-308) as 0.40 λ = ------------- = 0.174 2.303

(7-311)

Damage Models In many structural applications, the finite element method is used to predict failure. This is often performed by comparing the calculated solution to some failure criteria, or by using classical fracture mechanics. Previously, we discussed two models where the actual material model changed due to some failure, see “Progressive Composite Failure” on page 372 and the previous section on “Low Tension Material” on page 485. In this section, the damage models appropriate for ductile metals and elastomeric materials will be discussed.

Ductile Metals In ductile materials given the appropriate loading conditions, voids will form in the material, grow, then coalesce, leading to crack formation and potentially, failure. Experimental studies have shown that these processes are strongly influenced by hydrostatic stress. Gurson studied microscopic voids in materials and derived a set of modified constitutive equations for elastic-plastic materials. Tvergaard and Needleman modified the model with respect to the behavior for small void volume fractions and for void coalescence. In the modified Gurson model, the amount of damage is indicated with a scalar parameter called the void volume fraction f. The yield criterion for the macroscopic assembly of voids and matrix material is given by: ⎛ q 2 σ k k⎞ σ 2 F = ⎛ ------⎞ + 2q 1 f∗ cosh ⎜ ---------------⎟ – [ 1 + ( q 1 f∗ ) 2 ] = 0 ⎝ σ y⎠ ⎝ 2σ y ⎠ as seen in Figure 7-89. σe ⁄ σM 1.0

· f* = 0 · f* ⁄ f u* = 0.01

0.5 0.1 0.6

0.3

0.9 0 0

1

2

3

4

σ k k ⁄ 3σ M

Figure 7-89 Plot of Yield Surfaces in Gurson Model

Main Index

(7-312)

500 Marc Volume A: Theory and User Information

7

The parameter q 1 was introduced by Tvergaard to improve the Gurson model at small values of the void volume fraction. For solids with periodically spaced voids, numerical studies [Ref. 10] showed that the values of q 1 = 1.5 and q 2 = 1 were quite accurate.

Material Library

The evolution of damage as measured by the void volume fraction is due to void nucleation and growth. Void nucleation occurs by debonding of second phase particles. The strain for nucleation depends on the particle sizes. Assuming a normal distribution of particle sizes, the nucleation of voids is itself modeled as a normal distribution in the strains, if nucleation is strain controlled. If void nucleation is assumed to be stress controlled in the matrix, a normal distribution is assumed in the stresses. The original Gurson model predicts that ultimate failure occurs when the void volume fraction f, reaches unity. This is too high a value and, hence, the void volume fraction f is replaced by the modified void volume fraction f∗ in the yield function. The parameter f∗ is introduced to model the rapid decrease in load carrying capacity if void coalescence occurs. f∗ = f ⎛ f u* – f c⎞ f∗ = f c + ⎜ ----------------⎟ ( f – f c ) ⎝ f F – f c⎠

if f ≤ fc (7-313)

if f > fc

where f c is the critical void volume fraction, and f F is the void volume at failure, and f u* = 1 ⁄ q 1 . A safe choice for f F would be a value greater than ( 1 ⁄ q 1 ) namely, f F = 1.1 ⁄ q 1 . Hence, you can control the void volume fraction, f F , at which the solid loses all stress carrying capability. Numerical studies show that plasticity starts to localize between voids at void volume fractions as low as 0.1 to 0.2. You can control the void volume fraction f c , beyond which void-void interaction is modeled by Marc. Based on the classical studies, a value of f c = 0.2 can be chosen. The existing value of the void volume fraction changes due to the growth of existing voids and due to the nucleation of new voids. · · · f = f g r o wt h + f n u c l e a t i o n

(7-314)

The growth of voids can be determined based upon compressibility of the matrix material surrounding the void. ·p · f g r o w t h = ( 1 – f )ε k k

(7-315)

As mentioned earlier, the nucleation of new voids can be defined as either strain or stress controlled. Both follow a normal distribution about a mean value.

Main Index

CHAPTER 7 501 Material Library

In the case of strain controlled nucleation, this is given by fN · f n u c l e a t i o n = -------------S 2π

p 2 1 εm – εn ·p exp – --- ⎛ -------------------⎞ ε m 2⎝ S ⎠

(7-316)

where f N is the volume fraction of void forming particles, ε n the mean strain for void nucleation and S the standard deviation. In the case of stress controlled nucleation, the rate of nucleation is given by: fN 1 Σ – σn 2 · f n u c l e a t i o n = -------------- Σ exp – --- ⎛ ----------------⎞ 2⎝ S ⎠ S 2π

(7-317)

1 where Σ = σ + --- σ k k . 3 If the second phase particle sizes in the solid are widely varied in size, the standard deviation would be larger than in the case when the particle sizes are more uniform. The Marc user can also input the volume fraction of the nucleating second phase void nucleating particles in the input deck, as the variable f N . A typical set of values for an engineering alloy is given by Tvergaard for strain controlled nucleation as ε n = 0.30 ; f N = 0.04 ; S = 0.01 .

(7-318)

It must be remarked that the determination of the three above constants from experiments is extremely difficult. The modeling of the debonding process must itself be studied including the effect of differing particle sizes in a matrix. It is safe to say that such an experimental study is not possible. The above three constants must necessarily be obtained by intuition keeping in mind the meaning of the terms. When the material reaches 90 percent of f F , the material is considered to be failed. At this point, the stiffness and the stress at this element are reduced to zero.

Elastomers Under repeated application of loads, elastomers undergo damage by mechanisms involving chain breakage, multi-chain damage, micro-void formation, and micro-structural degradation due to detachment of filler particles from the network entanglement. Two types of phenomenological models namely, discontinuous and continuous, exists to simulate the phenomenon of damage. 1. Discontinuous Damage: The discontinuous damage model simulates the “Mullins’ effect” as shown in Figure 7-90.

Main Index

502 Marc Volume A: Theory and User Information

Figure 7-90 Discontinuous Damage

This involves a loss of stiffness below the previously attained maximum strain. The higher the maximum attained strain, the larger is the loss of stiffness. Upon reloading, the uniaxial stressstrain curve remains insensitive to prior behavior at strains above the previously attained maximum in a cyclic test. Hence, there is a progressive stiffness loss with increasing maximum strain amplitude. Also, most of the stiffness loss takes place in the few earliest cycles provided the maximum strain level is not increased. This phenomenon is found in both filled as well as natural rubber although the higher levels of carbon black particles increase the hysteresis and the loss of stiffness. The free energy, W , can be written as: W = K ( α, β )W

0

(7-319)

0

where W is the nominal strain energy function, and 0

α = max ( W )

(7-320)

determines the evolution of the discontinuous damage. The reduced form of Clausius-Duhem dissipation inequality yields the stress as: 0

∂W S = 2K ( α ,β ) ----------∂C

(7-321)

where C is the deformation tensor. Mathematically, the discontinuous damage model has a structure very similar to that of strain space plasticity. Hence, if a damage surface is defined as: Φ = W–α≤0

(7-322)

The loading condition for damage can be expressed in terms of the Kuhn-Tucker conditions: Φ≤0

Main Index

· α≥0

· αΦ = 0

(7-323)

CHAPTER 7 503 Material Library

The consistent tangent can be derived as: 2

0

0

0

∂ W ∂K ∂W ∂W D = 4 K --------------- + ----------- ----------- ⊗ ----------∂C∂C ∂W 0 ∂C ∂C

(7-324)

2. Continuous Damage: The continuous damage model can simulate the damage accumulation for strain cycles for which the values of effective energy is below the maximum attained value of the past history as shown in Figure 7-91. This model can be used to simulate fatigue behavior. More realistic modeling of fatigue would require a departure from the phenomenological approach to damage. The evolution of continuous damage parameter is governed by the arc length, s , of the effective strain energy as: t

β =

∫ 0

∂ 0 ----- W ( s ) ds ∂s

(7-325)

Hence, β accumulates continuously within the deformation process.

Figure 7-91 Continuous Damage

The Kachanov factor K ( α, β ) is implemented in Marc through both an additive as well as a multiplicative decomposition of these two effects as: 2 ∞

K ( α, β ) = d +

∑ n = 1 2

∞

K ( α, β ) = d +

∑ n = 1

Main Index

α dn

α exp ⎛ – ------⎞ + ⎝ η n⎠

2

∑ n = 1

α + δn β d n exp ⎛ – --------------------⎞ ⎝ ηn ⎠

β β d n exp ⎛ – -----⎞ ⎝ λ n⎠

(7-326)

(7-327)

504 Marc Volume A: Theory and User Information

α

β

∞

You specify the phenomenological parameters d n , d n , η n, λ n, d n, δ n and d . If d

∞

is not

defined, it is automatically determined such that, at zero values of α and β , the Kachanov factor K = 1 . If, according to Equation (7-325) or Equation (7-326) the value of K exceeds 1, K is set back to 1. The above damage model is available for deviatoric behavior and is flagged by means of the OGDEN and DAMAGE model definition options. If, in addition, viscoelastic behavior is desired, the VISCELOGDEN option can be included. Finally, the UELDAM user subroutine can be used to define damage functions different from Equations (7-323) to (7-326). The parameters required for the continuous or discontinuous damage model can be obtained using the experimental data fitting option in Marc Mentat and MD Patran.

Cohesive Zone Modeling Marc has a library of so-called interface elements (186, 187, 188, 189, 190, 191, 192,and 193), which can be used to simulate the onset and progress of delamination. The constitutive behavior of these elements is expressed in terms of tractions versus relative displacements between the top and bottom edge/surface of the elements (see Figure 7-92). 8 4

v1 ˜

top face 7

v3 ˜ v2 ˜

5 1

3 bottom face

6 2 Figure 7-92 3-D Linear Interface Element

Considering a 3-D interface element, the relative displacement components are given by one normal and two shear components, expressed with respect to the local element system (see Marc Volume B: Element Library for the definition of the local element systems): top

vn = u1

top

vs = u2

t op

vt = u3

bottom

– u1

bottom

– u2

(7-328)

bottom

– u3

Based on the relative displacement components, the effective opening displacement is defined as: v =

2

2

2

vn + vs + vt

Later on, some modifications of this definition will be discussed.

Main Index

(7-329)

CHAPTER 7 505 Material Library

The effective traction t is introduced as a function of the effective opening displacement and is characterized by an initial reversible response followed by an irreversible response as soon as a critical effective opening displacement v c has been reached. The irreversible part is characterized by increasing damage ranging from 0 (onset of delamination) to 1 (full delamination). Three standard functions are currently available; namely, a bilinear, an exponential, and a linearexponential function (see Figure 7-93): 2G c v t = ---------- ----vm vc

if

0 ≤ v ≤ vc

2G c ⎛ v m – v ⎞ if t = ---------- ⎜ -------------------⎟ v m ⎝ v m – v c⎠

vc < v ≤ vm

t = 0

v > vm

if

v –v ⁄ vc t = G c ----- e 2 vc 2qG c v t = ------------------------ ----vc ( q + 2 ) vc

if

2qG c q ( 1 – v ⁄ v c ) if t = ------------------------ e vc ( q + 2 )

Bilinear

(7-330)

Exponential

(7-331)

Linear-exponential

(7-332)

0 < v ≤ vc

v > vc

in which G c is the energy release rate (cohesive energy), v m is the maximum effective opening displacement (which is only used by the bilinear model), and q is the exponential decay factor (which is only used by the linear-exponential model). t

t

vc

vm

v

t

vc

v vc

Figure 7-93 Bilinear (left), Exponential (middle), and Linear-exponential (right)

Main Index

v

506 Marc Volume A: Theory and User Information

Cohesive Material Model

It can easily be verified that the maximum effective traction t c , corresponding to the critical effective opening displacement v c is given by: 2G c t c = ---------vm

Bilinear

(7-333)

Gc t c = -------ev c

Exponential

(7-334)

2qG c t c = -----------------------vc ( q + 2 )

Linear-exponential

(7-335)

So if the maximum effective traction is known, the critical or maximum effective opening displacement can be determined by: 2G c v m = ---------tc

Bilinear

(7-336)

Gc v c = ------et c

Exponential

(7-337)

2qG c v c = ---------------------tc ( q + 2 )

Linear-exponential

(7-338)

Note that for the bilinear model, the critical effective opening displacement does neither affect the cohesive energy nor the maximum effective traction. Until now, the behavior in the normal and shear direction is treated similarly. However, sometimes the behavior of an interface material may be different in tension and shear. The first method to include such differences is incorporated by the shear-normal stress ratio β 1 , which defines the ratio of the maximum stress in shear and the maximum stress in tension [Ref. 26]. This ratio is used to redefine the effective opening displacement according to: v =

2

2 2

2 2

vn + β1 vs + β1 vt

The effect of β 1 = 0.5 is depicted in Figure 7-94 for the bilinear model.

Main Index

CHAPTER 7 507 Material Library

t

t tension only

shear

only

Gc

vm

vc

Gc

vm

vc

v

v

Figure 7-94 Response in Tension and Shear for a Shear-normal Stress Ratio β 1 = 0.5 (Bilinear Model)

Although the use of the shear-normal stress ratio offers some flexibility, it assumes that the cohesive energy in tension and shear is the same. If one wants to define a different value of the cohesive energy in shear than in tension, the shear-normal energy ratio β 2 can be used. In a general state of deformation, when β 2 ≠ 1 , the curve defining the effective traction versus the effective opening displacement is defined as a linear combination of the response in pure tension and pure shear. Using β 1 = 0.5 and β 2 = 0.75 , Figure 7-95 shows the response in tension and shear for the bilinear model. t

t tension only

shear only

Gc

vc

vm

0.75G c

v

vc

vm

v

Figure 7-95 Response in Tension and Shear for a Shear-normal Stress Ratio β 1 = 0.5 and a Shear-normal Energy Ratio β 2 = 0.75 (Bilinear Model)

In order to avoid convergence problems in a finite element simulation of delamination, one may activate so-called viscous energy dissipation. The basic idea of the dissipation model is that when delamination starts, the rate of deformation may suddenly increase. This increase is used to augment the constitutive behavior with a viscous contribution being equivalent to this rate of deformation: ζt c v· t v i s = ---------v· r

Main Index

(7-339)

508 Marc Volume A: Theory and User Information

in which ζ is the viscous energy factor, v· is effective opening displacement rate and v· 0 is the reference value of the effective opening displacement rate. This reference value can either be user-defined or calculated by the program. In the latter case, the reference value is given by the maximum effective opening displacement rate in any interface element, as long as the response in all the interface elements is reversible. The viscous energy dissipation model does not directly have a physical background, but is basically numerical in nature. In the equations discussed above, no distinction has been made between tensile and compressive loading in the normal direction. Assuming that in compression the behavior will remain reversible, Equation (7-340) will be adapted as: v =

2

2

2

[ max ( v n, 0 ) ] + v s + v t

(7-340)

Since, irrespective of the damage level, the interface elements should be able to sustain ongoing loading in compression (so that inter-penetration is prohibited), it is possible to make the stiffness in compression a function of the corresponding (negative) opening displacement. By default, the stiffness in compression is constant and given by the slope of the traction versus opening displacement curve at the origin. If a non-default value of the stiffening factor in compression F is given, the stiffness at v = – v c is given by: ∂t n -------∂v n

– vc

∂t n = F -------∂v n

0

So far, the constitutive behavior has been discussed in terms of an effective traction versus an effective opening displacement. The traction components follow from the effective traction according to: ∂v ∂v t n = t --------- ; t s ,t = t ----------∂v n ∂v s ,t

(7-341)

As an alternative to the above mentioned standard models, the UCOHESIVE user subroutine can be used to enter a user-defined material behavior. 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. 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

Main Index

CHAPTER 7 509 Material Library

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 dD = ------------------------------------------- dε p , 2E ⋅ S ⋅ ( 1 – D ) 2

0≤D≤1

where the triaxiality function f ( η ) contains information about the state of stresses and is defined as follows: 2 f ( η ) = --- ( 1 + v ) + 3 ( 1 – 2v )η 2 3

σm η = ------σ

σ is the von Mises stress, E the Young’s modulus, v the Poisson’s ratio, σ m the mean normal stress, D the current integrated value of the absolute damage at that material point and dε 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). 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 1 c --------------------------(1 – D) 2 (σ f(η ))

1 ≥ Dc ≥ 0

D 1 c 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 : D c = 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 r e l (reflected in the postprocessing):

Main Index

510 Marc Volume A: Theory and User Information

D D r e l = -----Dc

0 ≤ Dr e l ≤ 1

When D r e l 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 – df )

If model 10 is used, then: p ·p σ y = σ y ( ε , ε , T )* ( 1.0 – df )

and

E = E ( T )* ( 1.0 – df )

The normal data for a specific material are defined with the ISOTROPIC, WORK HARD, and OGDEN options. Cross-reference to this material is made with the material number. 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. σm a x ·

- ε dt ≥ C ∫ -----------σ · where σ m a x is the maximum principal stress, σ is the effective von Mises stress and ε is the effective plastic strain rate. C is material constant threshold for damage. Principal-tension Damage Indicator This damage indicator does not affect the yield stress. σm a x

- dt ≥ C ∫ -----------σ where σ m a x is the maximum principal stress and σ is the effective von Mises stress. C is material constant threshold for damage. Figure 7-96 shows the application of the Cockroft-Latham damage criterion used to predict cracks known as Chevron cracks in the drawing process.

Main Index

CHAPTER 7 511 Material Library

Oyane Damage Indicator σm

- + B⎞⎠ ε dt ≥ C ∫ ⎛⎝ -----σ ·

Similar to Cockraft-Latham, Oyane damage indicates a possible damage area where σ m is the mean or average stress, B and C are both material constants. The UDAMAGE_INDICATOR user subroutine can be used to define unsupported damage criteria. The UACTIVE user subroutine can be used for element removal. Figure 7-97 show the application of the Oyane damage criterion used to predict cracks known as Chevron cracks in the extrusion process.

Figure 7-96 Chevron Crack Prediction with Cockroft-Latham Damage Criterion

Figure 7-97 Chevron Crack Prediction with Oyane Damage Criterion

Main Index

512 Marc Volume A: Theory and User Information

Nonstructural Materials In addition to stress analysis, Marc can be used for heat transfer, coupled thermo-electrical heating (Joule heating), coupled electrical-thermal-mechanical analysis (Joule-mechanical), hydrodynamic bearing, fluid/solid interaction, electrostatic, magnetostatic, electromagnetic, piezoelectric, acoustic, and fluid problems. Material properties associated with these analyses and Marc options that control these analyses are described below.

Heat Transfer Analysis In heat transfer analysis, use the ISOTROPIC, ORTHOTROPIC, or ANISOTROPIC model definition options to input values of thermal conductivity, specific heat, and mass density. If the latent heat effect is to be included in the analysis, the value of latent heat and associated solidus and liquidus temperatures must be entered through the LATENT HEAT or TEMPERATURE EFFECTS model definition option. Both the thermal conductivity and specific heat can be dependent on temperatures. The mass density must be constant throughout conventional heat transfer analysis. In addition, the ANKOND user subroutine can be used for the input of anisotropic thermal conductivity. For radiation analysis, you must enter the Stefan-Boltzmann constant in the RADIATION parameter and the emissivity through the EMISSIVITY or ISOTROPIC option. The emissivity can be temperature dependent. For high temperature analysis where pyrolysis occurs, the THERMO-PORE option is used to define the advanced material behavior.

Piezoelectric Analysis In a piezoelectric analysis, the material properties contain a mechanical part, an electrostatic part, and a part connecting these two. The material properties for the mechanical part are the same as for an elastic stress analysis. The material properties for the electrostatic part, the permittivity, and the material properties for the piezoelectric coupling can be defined through the PIEZOELECTRIC option. The coefficients for the piezoelectric coupling can be either stress based or strain based.

Thermo-Electrical Analysis In addition to thermal conductivity, specific heat and mass density, the value of electric resistivity must be entered using the ISOTROPIC and ORTHOTROPIC model definition options in a coupled thermoelectrical analysis. Input the variation of electric resistivity with temperature through the TEMPERATURE EFFECTS option.

Coupled Electrical-Thermal-Mechanical Analysis Material properties for coupled electrical-thermal-mechanical analysis are the same for stress analysis in addition to those of Joule heating analysis (thermal conductivity, specific heat and mass density and electric resistivity).

Main Index

CHAPTER 7 513 Material Library

Hydrodynamic Bearing Analysis In a hydrodynamic bearing analysis, the ISOTROPIC and ORTHOTROPIC model definition options can be used for entering both the viscosity and specific mass. Define the temperature dependency of viscosity through the TEMPERATURE EFFECTS option.

Fluid/Solid Interaction Analysis – Added Mass Approach In a fluid/solid analysis, the density of a fluid is given in the first field of the ISOTROPIC option. The fluid is assumed to be nonviscous and incompressible.

Electrostatic Analysis In an electrostatic analysis, the permittivity can be defined through either the ISOTROPIC or ORTHOTROPIC options. In addition, the UEPS user subroutine can be used for the input of anisotropic permittivity.

Magnetostatic Analysis In a magnetostatic analysis, the permeability can be defined through either the ISOTROPIC or ORTHOTROPIC options. A nonlinear relationship can be entered via the B-H RELATION option. The UMU user subroutine can be used for the input of isotropic permeability.

Electromagnetic Analysis In an electromagnetic analysis, the permittivity, permeability and conductivity can be defined using either the ISOTROPIC or ORTHOTROPIC options. An assumption made is that the permittivity is a constant (does not vary with time) in the analysis. A nonlinear permeability can be entered via the B-H RELATION option. The UEPS, UMU, and USIGMA user subroutines can be used for the input of anisotropic permittivity, permeability, and conductivity, respectively. Both the dependent and harmonic analysis can be performed.

Coupled Electrostatic-Structural Material properties for a coupled electrostatic-structural are the same as for a stress analysis in addition to those for an electrostatic analysis (permittivity).

Acoustic Analysis In an acoustic analysis of a cavity with rigid boundaries, the bulk modulus and the relative density of the medium can be entered through the ISOTROPIC option. The ACOUSTIC parameter is used to indicate that a coupled acoustic-structural analysis is performed. In addition to the CONTACT option, the ACOUSTIC and REGION model definition options are used to define the material properties of the acoustic medium and to set which elements correspond to the solid and the fluid region.

Main Index

514 Marc Volume A: Theory and User Information

Fluid Analysis In the fluid analysis, viscosity and density can be defined using the ISOTROPIC option. In addition, conductivity and specific heat are defined for coupled fluid-thermal analysis. Non-Newtonian fluid behavior can be defined using the STRAIN RATE option. The TEMPERATURE EFFECTS option can be used to define the temperature dependence of the properties above.

References 1. Auricchio, F. and Taylor, R.L., “Shape-memory alloy: modeling and numerical simulations of the finite-strain superelastic behavior”, Comput. Methods Appl. Mech. Engrg., Vol. 143, pp.175-194 (1997). 2. Auricchio, F., “A robust integration-algorithm for a finite-strain shape-memory-alloy superelastic model”, Int. J. Plasticity, Vol.17, pp.971-990 (2001). 3. Arruda, E. M. and Boyce, M. C. “A three-dimensional constitutive model for the large stretch behaviour of rubber elastic materials”, J. Mech. Phys. Solids, Vol.41, No. 2, 1993. 4. Buyukozturk, O., “Nonlinear Analysis of Reinforced Concrete Structures”, Computers and Structures, 7, 149-156 (1977). 5. Gent, A. N., “A new constitutive relation for rubber”, Rubber Chem. Tech., 69, 1996. 6. Barlat, F., Lege, D.J. and Brem, J.C., “A six-component yield function for anisotropic metals”, Int. J. Plasticity, 7, 693-712 (1991). 7. Chung, K. and Shah, K., “Finite element simulation of sheet metal forming for planar anisotropic metals”, Int. J. Plasticity, 8, 453-476 (1992). 8. Yoon, J.W., Yang, D.Y. and Chung, K. and Barlat. F., “A general elasto-plastic finite element formulation based on incremental deformation theory for planar anisotropy and its application to sheet metal forming”, Int. J. Plasticity, 15, 35-67 (1999). 9. Yoon, J.W., Barlat, F., Chung, K., Pourboghrat, F. and Yang, D.Y., “Earing predictions based on asymmetric nonquadratic yield function”, Int. J. Plasticity, 16, 1075-1104 (2000). 10. “Current Recommended Constitutive Equations for Inelastic Design Analysis of FFTF Components.” ORLN-TM-360Z, October 1971. 11. “Finite Element Calculation of Stresses in Glass Parts Undergoing Viscous Relaxation”, J.Am.Ceram.Soc. Vol. 70[2], pp. 90-95, 1987. 12. Mooney, M. J. Appl Phys., Vol. II, p. 582, 1940. 13. Naghdi, P. M. “Stress-Strain Relations in Plasticity and Thermoplasticity.” In Plasticity, Proceedings of the Second Symposium on Naval Structural Mechanics, edited by E. H. Lee and P. S. Symonds. Pergamon Press, 1960. 14. Narayanaswamy, O.S., “A Model of Structural Relaxation in Glass”, J.Am.Ceram.Soc., Vol. 54[10], pp. 491-498, 1971. 15. Prager, W. Introduction to Mechanics to Continua. New York: Dover Press, 1961. 16. “Proposed Modification to RDT Standard F9-5T Inelastic Analysis Guidelines.” ORNL, October 1978.

Main Index

CHAPTER 7 515 Material Library

17. Rivlin, R. S. Phil Trans Roy Soc (A), Vol. 240, 459, 1948. 18. Rivlin, R. S. Phil Trans Roy Soc (A), Vol. 241, 3-79, 1948. 19. Timoshenko, S. P., and J. N. Goodier. Theory of Elasticity. Third Ed. New York: McGraw-Hill, 1970. 20. Simo, J. C. “On a Fully Three-dimensional Finite Strain Viscoelastic Damage Model: Formulation and Computational Aspects,” Computer Methods in Applied Mechanics and Engineering, Vol. 60, 1987, pp. 153-173. 21. Tvergaard, V., “Influence of Voids on Shear Band Instabilities under Plane Strain Conditions”, Int. J. Fracture, Vol. 17, pp. 389-407, 1981. 22. Tvergaard, V., “Material Failure by Void Coalescence in Localized Shear Bands”, in Int. J. Solids Struct., Vol. 18, No. 8, pp. 652-672, 1982. 23. Chaboche, J. L., “Constitutive Equations for Cyclic Plasticity and Cyclic Viscoplasticity”, International Journal of Plasticity, Vol. 5, pp. 247-302, 1989 24. van den Boogard, A.H., “Implicit integration of the Perzyna viscoplastic material model”, TNO Building and Construction Research, The Netherlands, TNO-report, 95-NM-R711, 1995 25. Puck, A. and Schürmann, H., “Failure Analysis of FRP Laminates by Means of Physically Based Phenomenological Models”; Composite Science and Technology, 58, pp. 1045-1067, 1998. 26. Camacho, G.T. and Ortiz, M., “Computational modelling of impact damage in brittle materials”, Int. J. Solids Struct., Vol. 33, pp 2899-2938, 1996. 27. Greve, L. and Picket, A. K., “Modelling Damage and Failure in Carbon/Epoxy Non-crimp Fabric Composites Including Effects of Fabric Pre-shear”, Composites: Part A, Vol. 37, pp. 1983-2001, 2006. 28. Knops, M. and Bögle, C. “Gradual Failure in Fibre/Polymer Laminates”, Composites Science and Technology, Vol. 66, pp. 616-625, 2006.

Main Index

516 Marc Volume A: Theory and User Information

Main Index

Chapter 8 Contact

8

Main Index

Contact

J

Definition of Contact Bodies

J

Numbering of Contact Bodies

J

Motion of Bodies

J

Detection of Contact

J

Implementation of Constraints

J

Friction Modeling

J

Separation

J

Coupled Analysis

J

Thermal Contact

J

Element Considerations

J

Dynamic Impact

J

Global Adaptive Meshing and Rezoning

J

Adaptive Meshing

554

J

Result Evaluation

555

J

Tolerance Values

556

J

Numerical and Mathematical Aspects of Contact

J

References

518 521

524 526 530

532

544

568

545 548 550

553 554

557

518 Marc Volume A: Theory and User Information

The simulation of many physical problems requires the ability to model the contact phenomena. This includes analysis of interference fits, rubber seals, tires, crash, and manufacturing processes among others. The analysis of contact behavior is complex because of the requirement to accurately track the motion of multiple geometric bodies, and the motion due to the interaction of these bodies after contact occurs. This includes representing the friction between surfaces and heat transfer between the bodies if required. The numerical objective is to detect the motion of the bodies, apply a constraint to avoid penetration, and apply appropriate boundary conditions to simulate the frictional behavior and heat transfer. Several procedures have been developed to treat these problems including the use of Perturbed or Augmented Lagrangian methods, penalty methods, and direct constraints. Furthermore, contact simulation has often required the use of special contact or gap elements. Marc allows contact analysis to be performed automatically without the use of special contact elements. A robust numerical procedure to simulate these complex physical problems has been implemented in Marc.

Definition of Contact Bodies There are two types of contact bodies in Marc – deformable and rigid. Deformable bodies are simply a collection of finite elements as shown below.

Figure 8-1

Deformable Body

This body has three key aspects to it: 1. The elements which make up the body. 2. The nodes on the external surfaces which might contact another body or itself. These nodes are treated as potential contact nodes. 3. The edges (2-D) or faces (3-D) which describe the outer surface which a node on another body (or the same body) might contact. These edges/faces are treated as potential contact segments. Note that a body can be multiply connected (have holes in itself). It is also possible for a body to be composed of both triangular elements and quadrilateral elements in 2-D or tetrahedral elements and brick elements in 3-D. Beam elements and shells are also available for contact. Both lower-order (linear) and higher-order (quadratic) elements may be used. One should not mix continuum elements, shells, and/or beams in the same contact body. Each node and element should be in, at most, one body. The elements in a body are defined using the CONTACT option. It is not necessary to identify the nodes on the exterior surfaces as this is done automatically. The algorithm used is based on the fact that nodes on the boundary are on element edges or faces that belong to only one element. Each node on the exterior surface is treated as a potential contact node. In many problems, it is known that certain nodes never come into contact; in such cases, the

Main Index

CHAPTER 8 519 Contact

CONTACT NODE option can be used to identify the relevant nodes. As all nodes on free surfaces are considered contact nodes, if there is an error in the mesh generation such that internal holes or slits exist, undesirable results can occur.

Note:

These problems can be visualized by using Marc Mentat to create an outline plot and fixed by using the sweep command in Marc Mentat.

The potential segments composed of edges or faces are treated in potentially two ways. The default is that they are considered as piece-wise linear (PWL). As an alternative, a cubic spline (2-D) or a Coons surface (3-D) can be placed through them. The SPLINE option is used to activate this procedure. This improves the accuracy of the calculation of the normal to the surface. Rigid bodies are composed of curves (2-D) or surfaces (3-D) or meshes with only thermal elements in coupled problems. The most significant aspect of rigid bodies is that they do not deform. Deformable bodies can contact rigid bodies, but contact between rigid bodies is not considered. They can be created either in CAD systems and transferred through Marc Mentat into Marc, created within Marc Mentat, or created directly through the Marc input. There are several different types of curves and surfaces that can be entered including: Table 8-1

Geometrical Entities Used in Modeling Contact

2-D

3-D

line

4-node patch

circular arc

ruled surface

spline

surface of revolution

NURBS

Bezier poly-surface cylinder sphere NURBS trimmed NURBS

Within the Marc Mentat GUI, all curves or surfaces are mathematically treated as NURBS curves or surfaces. This allows the greatest level of generality. Within the analysis, these rigid curves or surfaces can be treated in two ways – discrete piecewise linear lines (2-D) or patches (3-D), or as analytical NURBS curves or surfaces. When the discrete approach is used, all geometric primitives are subdivided into straight line segments or bilinear patches. You have control over the density of these subdivisions to approximate a curved line or surface within a desired degree of accuracy. This subdivision is also relevant when the corner conditions (see “Detection of Contact” on page 526) are determined. Too few subdivisions might lead to a very bad surface description and too many subdivisions might lead to a more expensive analysis due to more complex contact checking. When using the analytical description, the

Main Index

520 Marc Volume A: Theory and User Information

number of subdivisions given is less relevant. It should be large enough to roughly visualize the shape of the NURBS. In 3-D, a too large number is automatically reduced so that the analysis cost is not influenced too much. The treatment of the rigid bodies as NURBS surfaces is advantageous because it leads to greater accuracy in the representation of the geometry and a more accurate calculation of the surface normal. Additionally, the variation of the surface normal is continuous over the body which leads to a better calculation of the friction behavior and better convergence. To create a rigid body, you can either read in the curve and surface geometry created from a CAD system or create the geometry in Marc Mentat or directly enter it in Marc. You then use the CONTACT option to select which geometric entities are to be a part of the rigid body. An important consideration for a rigid body is the definition of the interior side and the exterior side. For two-dimensional analysis, the interior side is formed by the right-hand rule when moving along the body. This is easily visualized with Marc Mentat by activating ID CONTACT. Deformable

top/front

Rigid

top/front/inside bottom/back/outside

Y Z

Y X 1

Figure 8-2

Z

X 1

Orientation of Rigid Body Segments

For three-dimensional analysis, the interior side is formed by the right-hand rule along a patch. The interior side is visualized in Marc Mentat as the front surface (pink); whereas, the exterior side is visualized in Marc Mentat as the back surface (gold). It is not necessary for rigid bodies to define the complete body. Only the bounding surface needs to be specified. You should take care, however, that the deforming body cannot slide out of the boundary curve in 2-D (Figure 8-3). This means that it must always be possible to decompose the displacement increment into a component normal and a component tangential to the rigid surface.

Incorrect Figure 8-3

Main Index

Correct

Deformable Surface Sliding Out of Rigid Surface

CHAPTER 8 521 Contact

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. Note:

For problems involving adaptive meshing or automated remeshing, care must be taken to satisfy this rule before as well as after the mesh change.

If one has defined a body numbering which violates the general rule, or if the rule is violated upon remeshing, then a CONTACT TABLE model or history definition option can be used to modify the order in which contact is established. This order can be directly user-defined or decided by the program. In the latter case, the order is based on the rule that if two deformable bodies might come into contact, searching is done such that the contacting nodes are on the body having the smallest element edge length and the contacted segments are on the body having the coarser mesh. It should be noted that this implies single-sided contact for this body combination, as opposed to the default double-sided contact. For deformable-deformable contact, the CONTACT option offers the following three global contact search controls: • SINGLE-SIDED • DOUBLE_SIDED • OPTIMIZE CONTACT CONSTRAINT EQUATIONS If flexible region A comes into contact with flexible region B, the following rules will be satisfied by the program to determine the constraint equations: 1. Region A and region B belong to the same contact body: a. If OPTIMIZE CONTACT CONSTRAINT EQUATIONS is active, the finer meshed region contacts the coarser meshed region. b. If OPTIMIZE CONTACT CONSTRAINT EQUATIONS is not active, the region containing the lower node number coming into contact contacts the other region. 2. Region A and region B do not belong to the same contact body: a. If SINGLE-SIDED contact is active, the region belonging to the lower contact body number contacts the region belonging to the higher contact body number. b. If DOUBLE_SIDED contact is active, the region containing the lower node number coming into contact contacts the other region. Because of the search order for contact is from lower body numbers to higher body numbers, this often leads to the same solution as mentioned above. c. If OPTIMIZE CONTACT CONSTRAINT EQUATIONS is active, the region with the softer material contacts the region with the harder material, or the region with the finer mesh contacts the region with the coarser mesh (soft-hard criterion has priority over mesh-density criterion).

Main Index

522 Marc Volume A: Theory and User Information

d. All the above settings can be overruled by the CONTACT TABLE model or history definition option where you can specify that a certain body AA should contact body BB and not viceverse, or that the body with the smallest element edge should contact the other body. As an example, two identical bodies shown in Figure 8-4, but created using two different approaches so that the node numbering order is different. Each U-Section is one contact body. In particular, for the model on the left, the left leg of the U-section has lower node ids that the right leg; while for the model on the right, the opposite is true.

Figure 8-4 Node Numbers on Models

A uniform distributed load is placed on the right leg, such that self-contact occurs. Without using optimized contact, the behavior is shown in Figure 8-5.

Figure 8-5 Contact Based upon Original Model.

The dark squares indicate nodes that are in contact based upon the Contact Status. Observe that the model on the left gives good behavior, while that on the right does not. This is because the lower node numbers on the left leg detect contact with the right leg before the corner node on

Main Index

CHAPTER 8 523 Contact

the right leg (which has a higher id) detects contact with the left leg. Then, activate the Optimized Contact Constraint option, and the results are shown in Figure 8-6. The node number IDs are no longer controlling the solution.

Figure 8-6 Contact using Optimized Contact Constraints

Each model is then subdivided into two contact bodies as shown in Figure 8-7, the contact table option is not used and the optimized procedure is not used.

Figure 8-7 Contact Based upon Contact Body Numbering

Observe now that in the left model, the left leg is a lower body number, so the nodes on this body try to contact the segments on the right leg. In the model on the right then, the right leg has the lower body number, and so the nodes on this leg contact (successfully) with the segments on the left leg. When either the Optimized Contact Constraint Procedure or a well-selected Contact Table utilizing Single-Sided Contact, the consistent results may be obtained for either model as shown in Figure 8-8

Main Index

524 Marc Volume A: Theory and User Information

Figure 8-8 Contact Using either Optimized Contact Constraint or Contact Table.

Motion of Bodies The motion of deformable bodies is prescribed using the conventional methods of applying displacements, forces, or distributed loads to the bodies. It is advantageous to not apply displacements or point loads to nodes which might come into contact with other rigid bodies. If a prescribed displacement is to be imposed, it is better to introduce another rigid body and apply the motion to the rigid body. Symmetry surfaces are treated as a special type of bodies which have the property of being frictionless and where the nodes are not allowed to separate. If a distributed load is applied to an edge or face, it is possible for this load to be deactivated if all nodes on the edge or face are in contact with another body. There are four ways to prescribe the motion of rigid surfaces: Prescribed velocity Prescribed position Prescribed load Prescribed scaling Associated with the rigid body is a point labeled the centroid. When the first two methods are chosen, you define the translational motion of this point, and the angular motion about an axis through this point. The direction of the axis can be defined for three-dimensional problems. For two-dimensional problems, it is a line normal to the plane. For complex time-dependent behavior, the MOTION user subroutine can be used to prescribe the motion as an alternative to the input. The motion during a time increment is considered to be linear. The position is determined by an explicit, forward integration of the velocities based upon the current time step. A time increment must always be defined even if a static, rateindependent analysis is performed. When load controlled rigid bodies are used, two additional nodes, called the control nodes, are associated with each rigid body. In 2-D problems, the first node has two translational degrees of freedom (corresponding to the global x- and y-direction) and the second node has one rotational degree of freedom (corresponding to the global z-direction). In 3-D problems, the first node has three translational degrees of freedom (corresponding to global x-, y-, and z-direction) and the second node has three rotational degrees of freedom (corresponding to the global x-, y-, and z-direction). In this way, both forces and moments can be applied to a body by using the POINT LOAD option for the control nodes. Alternatively, one may prescribe one or more degrees of freedom of the control nodes by using the FIXED DISP or DISP

Main Index

CHAPTER 8 525 Contact

CHANGE options. Generally speaking, load-controlled bodies can be considered as rigid bodies with three (in 2-D) or six (in 3-D) degrees of freedom. These degrees of freedom may be in a user-defined system of either the TRANSFORMATION or COORD SYSTEM option is used. The prescribed position and prescribed velocity methods (see Figure 8-9) have less computational costs than the prescribed load method (see Figure 8-10). 2 Centroid

3

1

V

ω

2 1 Figure 8-9

Velocity Controlled Rigid Surface Fy Mz

Extra Node

Fx

Figure 8-10 Load Controlled Rigid Surface

If the second control node is not specified, the rotation of the body is prescribed to be zero. It should be noted that the nodal coordinates of the first control node define the center of rotation for the body. The nodal coordinates of the second control node are arbitrary. It is also possible to either expand or contract the size of the rigid body through the use of specified scale factors multiplied by a table to make the scaling time dependent. Alternately, the UGROWRIGID user subroutine may be used to provide scale factors. The scale factors must be initialized to 1.0 but can change afterwards. Abrupt or discontinuous changes in the scale factors should be avoided while the rigid surface is in contact with other bodies. If no rotations are applied, the scale factors can be different in the x-, y-, and z-directions.

Main Index

526 Marc Volume A: Theory and User Information

Initial Conditions At the beginning of the analysis, bodies should either be separated from one another or in contact. Bodies should not penetrate one another unless the objective is to perform an interference fit calculation. Rigid body profiles are often complex, making it difficult for you to determine exactly where the first contact is located. Before the analysis begins (increment zero), if a rigid body has a nonzero motion associated with it, the initialization procedure brings it into first contact with a deformable body. No motion or distortion occurs in the deformable bodies during this process. In a coupled thermal mechanical analysis, no heat transfer occurs during this process. If more than one rigid body exists in the analysis, each one with a nonzero initial velocity is moved until it comes into contact. Because increment zero is used to bring the rigid bodies into contact only, you should not prescribe any loads (distributed or point) or prescribed displacements initially. For multistage contact analysis (often needed to simulate manufacturing processes), the APPROACH and SYNCHRONIZED options in conjunction with the CONTACT TABLE and MOTION CHANGE options allow you to model contact bodies so that they just come into contact with the workpiece. In assembly analysis, it is possible that multiple bodies are initially in contact. Because of mesh discretization, it is possible that the contact is not perfect, which would result in inducing stresses due to overclosure. The CONTACT TABLE option may be used to specify that the initial contact should be stress free. In such cases, the coordinates of the nodes are relocated on the surface so that initial stresses do not occur.

Detection of Contact During the incremental procedure, each potential contact node is first checked to see whether it is near a contact segment. The contact segments are either edges of other 2-D deformable bodies, faces of 3-D deformable bodies, or segments from rigid bodies. By default, each node could contact any other segment including segments on the body that it belongs to. This allows a body to contact itself. To simplify the computation, it is possible to use the CONTACT TABLE option to indicate that a particular body will or will not contact another body. This is often used to indicate that a body will not contact itself. During the iteration process, the motion of the node is checked to see whether it has penetrated a surface by determining whether it has crossed a segment. Because there can be a large number of nodes and segments, efficient algorithms have been developed to expedite this process. A bounding box algorithm is used so that it is quickly determined whether a node is near a segment. If the node falls within the bounding box, more sophisticated techniques are used to determine the exact status of the node. During the contact process, it is unlikely that a node exactly contacts the surface. For this reason, a contact tolerance (Figure 8-11) is associated with each surface.

Main Index

CHAPTER 8 527 Contact

rance 2 x Tole

Figure 8-11 Contact Tolerance

If a node is within the contact tolerance, it is considered to be in contact with the segment. The contact tolerance is calculated by the program as the smaller of 5% of the smallest element side or 25% of the smallest (beam or shell) element thickness. It is also possible for you to define the contact tolerance through the input. (t)

( t+ Δ )

( t+ Δ )

During an increment, if node A moves from A to A , where A is beyond the contact tolerance, the node is considered to have penetrated (Figure 8-12). In such a case, a special procedure is invoked to avoid this penetration. More details are discussed in Numerical and Mathematical Aspects of Contact in this chapter. A(t)

A(t + δt) Figure 8-12 Trial Displacement with Penetration

The size of the contact tolerance has a significant impact on the computational costs and the accuracy of the solution. If the contact tolerance is too small, detection of contact and penetration is difficult which leads to higher costs. Penetration of a node happens in a shorter time period leading to more recycles due to iterative penetration checking or to more increment splitting and increases the computational costs. If the contact tolerance is too large, nodes are considered in contact prematurely, resulting in a loss of accuracy or more recycling due to separation. Furthermore, the accepted solution might have nodes that “penetrate” the surface less than the error tolerance, but more than desired by the user. The default error tolerance is recommended.

Main Index

528 Marc Volume A: Theory and User Information

Many times, areas exist in the model where nodes are almost touching a surface (for example, in rolling analysis close to the entry and exit of the rolls). In such cases, the use of a biased tolerance area with a smaller distance on the outside and a larger distance on the inside is advised. This avoids the close nodes from coming into contact and separating again and is accomplished by entering a bias factor. The bias factor should be given a value between 0.0 and 0.99. The default is 0.0 or no bias. Also, in analyses involving frictional contact, a bias factor for the contact tolerance is recommended. The outside contact area is (1. - bias) times the contact tolerance on the inside contact area (1. + bias) times the contact tolerance (Figure 8-13). The bias factor recommended value is 0.95. In some instances, you might wish to influence the decision regarding the deformable segment a node contacts (or does not contact). This can be done using the EXCLUDE option.

(1 - Bias)∗ tolerance

(1 + Bias)∗ tolerance

Figure 8-13 Biased Contact Tolerance

Shell Contact A node on a shell makes contact when the position of the node plus or minus half the thickness projected with the normal comes into contact with another segment (Figure 8-14). In 2-D, this can be shown as: x1 = A + n t ⁄ 2 x2 = A – n t ⁄ 2

S

Shell Midsurface 1

2

anc e x toler

x

2 A

x Figure 8-14 Default Shell Contact

Main Index

t

CHAPTER 8 529 Contact

If point x or y falls within the contact tolerance distance of segment S, node A is considered in contact with the segment S. Here x 1 and x 2 are the position vectors of a point on the surfaces 1 and 2 on the shell, A is the position vector of a point (node in a discretized model) on the midsurface of the shell, n is the normal to the midsurface, and t is the shell thickness. As the shell has finite thickness, the node (depending on the direction of motion) can physically contact either the top surface, bottom surface, or mathematically contact can be based upon the midsurface. You can control whether detection occurs with either both surfaces, the top surface, the bottom surface, or the middle surface. In such cases, either two or one segment will be created at the appropriate physical location. Note that these segments will be dependent, not only on the motion of the shell, but also the current shell thickness (Figure 8-15). Note:

Shell elements should be oriented consistently. Also, a shell segment cannot be in contact simultaneously on both the Top and Bottom sides. If simultaneous contact is required, use the solid shell element.

S1 2

n

S1

n

S2

2

1 1 Include Both Segments n

Top Segment Only 2 S1

S2

1

2 1

Bottom Segments Only

Ignore Shell Thickness

Figure 8-15 Selective Shell Contact

S 1, S 2 are segments associated with shell consisting of node 1 and 2.

Neighbor Relations When a node is in contact with a rigid surface, it tends to slide from one segment to another. In 2-D, the segments are always continuous and so are the segment numbers. Hence, a node in contact with segment n slides to segment n – 1 or to segment n + 1 (Figure 8-16). This simplifies the implementation of contact.

Main Index

530 Marc Volume A: Theory and User Information

n-1 n+1

n

Figure 8-16 Neighbor Relationship (2-D)

In 3-D, the segments are often discontinuous (Figure 8-17). This can be due to the subdivision of matching surfaces or, more likely, the CAD definition of the under lying surface geometry.

Hole Physically Discontinuous

Nonmatching Segments Continuous Surface Segments

Discontinuous Surface Geometry

Figure 8-17 Neighbor Relationship (3-D)

Continuous surface geometry is highly advantageous as a node can slide from one segment to the next with no interference (assuming the corner conditions are satisfied). Discontinuous surface geometry results in additional operations when a node slides off a patch and cannot find an adjacent segment. Hence, it is advantageous to use geometry clean-up tools to eliminate small sliver surfaces and make the surfaces both physically continuous and topologically contiguous.

Implementation of Constraints For contact between a deformable body and a rigid surface, the constraint associated with no penetration is implemented by transforming the degrees of freedom of the contact node and applying a boundary condition to the normal displacement. This can be considered solving the problem: K aˆ aˆ K aˆ b ⎧ u aˆ ⎫ ⎧ f aˆ ⎫ ⎨ ⎬ = ⎨ ⎬ K b aˆ K b b ⎩ u b ⎭ ⎩ fb ⎭ where aˆ represents the nodes in contact which have a local transformation, and b represents the nodes not in contact and, hence, not transformed. Of the nodes transformed, the displacement in the normal direction is then constrained such that δu aˆ n is equal to the incremental normal displacement of the rigid body at the contact point.

Main Index

CHAPTER 8 531 Contact

t P

n Figure 8-18 Transformed System (2-D)

As a rigid body can be represented as either a piecewise linear or as an analytical (NURBS) surface, two procedures are used. For piecewise linear representations, the normal is constant until node P comes to the corner of two segments as shown in Figure 8-19. During the iteration process, one of three circumstances occur. If the angle α is small ( – α smooth < α < α smooth ) , the node P slides to the next segment. In such a case, the normal is updated based upon the new segment. If the angle α is large ( α > α smooth or α < – α smooth ) the node separates from the surface if it is a convex corner, or sticks if it is a concave corner. The value of α smooth is important in controlling the computational costs. A larger value of α smooth reduces the computational costs, but might lead to inaccuracies. The default values are 8.625° for 2-D and 20° for 3-D. These can be reset using the PARAMETERS option in the model definition or history definition section.

Π

α

α

Convex Corner Figure 8-19 Corner Conditions (2-D)

Concave Corner

In 3-D, these corner conditions are more complex. A node (P) on patch A slides freely until it reaches the intersection between the segments. If it is concave, the node first tries to slide along the line of intersection before moving to segment B. This is the natural (lower energy state) of motion. These corner conditions also exist for deformable-to-deformable contact analysis. Because the bodies are continuously changing in shape, the corner conditions (sharp convex, smooth or sharp concave) are continuously being re-evaluated. When a rigid body is represented as an analytical surface, the normal is recalculated at each iteration based upon the current position. This leads to a more accurate solution, but can be more costly because of the NURBS evaluation.

Main Index

532 Marc Volume A: Theory and User Information

A B P P

Figure 8-20 Corner Conditions (3-D)

When a node of a deformable body contacts a deformable body, a multipoint constraint (called tying) is automatically imposed. Recalling that the exterior edges (2-D) or faces (3-D) of the other deformable bodies are known, a constraint expression is formed. For 2-D analysis using lower-order elements, the number of retained nodes is three – two from the edge and the contacting node itself. For 3-D analysis, the number of retained nodes is five – four from the patch and the contacting node itself. When using higher-order elements and true quadratic contact, the number of retained nodes for 2-D becomes four, for 3-D, (hexahedrals) nine, and for 3-D (tetrahedrals) seven. The constraint equation is such that the contacting node should be able to slide on the contacted segment, subject to the current friction conditions. This leads to a nonhomogeneous, nonlinear constraint equation. In this way, a contacting node is forced to be on the contacted segment. This might introduce undesired stress changes, since a small gap or overlap between the node and the contacted segment will be closed (note that using the Single Step Houbolt or generalized alpha/HHT operator in dynamics, forcing a node to be on the contacted segment is switched off by default, but can be activated via the PARAMETERS option). During initial detection of contact (increment 0), the stress-free projection option avoids those stress changes for deformable contact by adapting the coordinates of the contacting nodes such that they are positioned on the contacted segment. This stress-free projection can be activated using CONTACT TABLE. A similar option exists for glued contact; however, in this case, overlap will not be removed. During the iteration procedure, a node can slide from one segment to another, changing the retained nodes associated with the constraint. A recalculation of the bandwidth is automatically made. Because the bandwidth can radically change, the bandwidth optimization is also automatically performed. A node is considered sliding off a contacted segment if is passes the end of the segment over a distance more than the contact tolerance. As mentioned earlier, the node separates from the contacted body if this happens at a convex corner. For deformable contact, this tangential tolerance at convex corners can be enlarged by using the delayed sliding off option activated via CONTACT TABLE.

Friction Modeling Friction is a complex physical phenomenon that involves the characteristics of the surface such as surface roughness, temperature, normal stress, and relative velocity. An example of this complexity is that quite often in contact problems neutral lines develop. This means that along a contact surface, the material flows in one direction in part of the surface and in the opposite direction in another part of the surface. Such neutral lines are, in general, not known a priori.

Main Index

CHAPTER 8 533 Contact

The actual physics of friction and its numerical representation continue to be topics of research. Currently, in Marc the modeling of friction has basically been simplified to two idealistic models. The most popular friction model is the Coulomb friction model. This model is used for most applications with the exception of bulk forming as encountered in e.g. forging processes. For such applications the shear friction model is more appropriate.

Coulomb Friction The Coulomb model can be characterized by: σ t < μσ n (stick) and σ t = – μ σ n ⋅ t (slip) where σt

is the tangential (friction) stress

σ n is the normal stress μ

is the friction coefficient

t

is the tangential vector in the direction of the relative velocity: vr t = ----------- , in which v r is the relative sliding velocity. vr

Similarly, the Coulomb model can also be written in terms of nodal forces instead of stresses: f t < μf n (stick) and f t = – μ f n ⋅ t (slip) where ft

is the tangential (friction) force

fn

is the normal force

When Coulomb friction is used with the stress-based model, the integration point stresses are first extrapolated to the nodal points and then transformed, so that a direct component is normal to the contacted surface. Given this normal stress and the relative sliding velocity, the tangential stress is then evaluated and a consistent nodal force is calculated. For shell elements, the nodal force based Coulomb model must be used, since a reduced stress state is assumed with σ n = 0 . For continuum elements, both the stress-based and force-based Coulomb model can be used. For a given normal stress or normal force, the friction stress or force has a step function behavior based upon the value of the relative sliding velocity v r or the tangential relative incremental displacement Δu t , as outlined in Figure 8-21 for a 2-D case, where the relative velocity and incremental displacement are scalar values.

Main Index

534 Marc Volume A: Theory and User Information

σ t or f t

Stick

v r or Δu t

Slip Figure 8-21 Coulomb Friction Model

Since this discontinuity in the friction value may easily cause numerical difficulties, different approximations of the step function have been implemented. They are graphically represented in Figure 8-22 and they will be successively discussed. σ t or f t

ft

Δu t

vr

arctangent model

ft

stick-slip (modified step function) model

Δu t

bilinear model

Figure 8-22 Different Approximations for the Coulomb Friction Model

Arctangent Model The first procedure is based on a continuously differentiable function in terms of the relative sliding velocity: vr 2 σ t = – μ σ n --- arctan ⎛ -------------------------⎞ ⋅ t ⎝ RVCNST⎠ π for the friction stress, and: vr 2 f t = – μ f n --- arctan ⎛ -------------------------⎞ ⋅ t ⎝ RVCNST⎠ π for the friction force.

Main Index

CHAPTER 8 535 Contact

Physically, the value of RVCNST can be seen as the value of the relative velocity below which sticking occurs. The value of RVCNST is important in determining how closely the mathematical model represents the step function, as shown in Figure 8-23. A very large value of RVCNST results in a reduced value of the effective friction. A very small value may result in poor convergence. It is recommended that the value of RVCNST be 1% to 10% of a typical relative sliding velocity, v r . The friction implementation not only affects the external force vector, but also the stiffness matrix of the final set of equations to be solved on a global level. This stiffness matrix contribution follows from: ∂f t ∂v r i k K i j = – ---------- ------------∂v r ∂Δu t k

j

This later contribution, if fully implemented, would lead to a non-symmetric system. Because of the additional computational costs, both in terms of memory and CPU costs, the contribution to the stiffness matrix is symmetrized. ft μf n

vr – 10

10 RVCNST = 10

RVCNST = 1 –μ fn

RVCNST = 0.1

Figure 8-23 Step Function Approximation for Different Values of RVCNST (-10
During iteration ( i ) of the Newton-Raphson process, the change of the friction force δf t

is related to

(i)

the change of the relative sliding velocity δv r . Since the latter can be written as: (i) δv r

(i)

(i – 1)

(i)

Δu t – Δu t δu t = ----------------------------------------- = -----------Δt Δt

the resulting equation can still be expressed in displacement degrees of freedom. During the very first iteration of an increment, it turns out that the convergence can be significantly improved by using:

Main Index

536 Marc Volume A: Theory and User Information

(1) δv r

(1)

( previous increment )

(1)

Δu t δu t Δu t ( previous increment ) = -------------- – ------------------------------------------------ = ------------- – v r ( previous increment ) Δt Δt Δt ( previous increment )

where v r

results in a contribution to the right hand side of the global set of equations.

As a result of the smoothing procedure, a node in contact always has some slipping. Besides the numerical reasons, this ‘ever slipping node’ model has a physical basis. Oden and Pires pointed out that for metals, there is an elasto-plastic deformation of asperities at the microscopic level (termed as ‘cold weld’) which leads to a nonlocal and nonlinear frictional contact behavior. The arctangent representation of the friction model is a mathematical idealization of this nonlinear friction behavior. A complicating aspect of the arctangent model is that it may be difficult to estimate a priori the typical relative sliding velocity. This is particularly true in quasi-static deformable contact analyses (where the velocity is not an input quantity) and in cases where the sliding velocity varies strongly during the analysis. Stick-slip (Modified Step Function) Model The second procedure is based on a slightly modified step function and can be used to simulate true stickslip behavior. In this procedure, each node in contact gets a friction status, being either stick or slip. Depending on this status, different constraints are applied and after each iteration in the iterative solution process, the correctness of the friction status is checked and if necessary adapted. The typical parameters used (see also Figure 8-24) are the friction coefficient multiplier α , the slip to stick transition region β and the friction force tolerance e . The multiplier α (with a default value of 1.05 ) can be seen as an overshoot parameter used to simulate the difference between static and dynamic friction. –6

The slip-to-stick transition region β (with a default value of 1 ×10 ) can be seen as a tolerance on the friction solution. If a node is in slipping mode and moves in the direction of the friction force (which is physically incorrect), but the corresponding relative displacement magnitude is within the slip-to-stick transition region, then this will not cause the increment to be restarted with modified friction conditions. –6

Related to the parameter β , a reduction factor ε = 1.0 ×10

is used. This fixed factor causes the

product of ε and β to be very small, so that it can be used as a criterion to estimate if a node is initially in slipping or sticking mode. This initial assumption serves as the starting point of the above mentioned process of checking and adapting the friction status, which, for a 2-D analysis, is given in Figure 8-25 (note that Δu t ≈ 0 implies Δu t < εβ ).

Main Index

CHAPTER 8 537 Contact

8

α : friction coefficient multiplier

ft

β : slip to stick transition region αμf n

ε : reduction factor ( 1 ×10

β

μf n

εβ

–6

)

Δu t

Figure 8-24 Stick-slip or Modified Step Function Friction Parameters Contact

Initial Contact

No

Δu t ≈ 0

Assume Slipping Mode

Yes

Assume Sticking Mode

Determine Solution of Next Iteration

Remain in Slipping Mode if:

Remain in Sticking Mode if:

f t • Δu t < 0 and Δu t > β

f t ≤ αμf n

Change to Sticking Mode if: f t • Δu t > 0 and Δu t > β

Change to Slipping Mode if:

or if Δu t ≈ 0

f t > αμf n

Figure 8-25 Flow Diagram for the Stick-slip or Modified Step Function Friction Model

When a node is in slipping mode, the contribution to the stiffness matrix is: Ki j

∂f t i = – ------------∂Δu t j

Main Index

538 Marc Volume A: Theory and User Information

while in sticking mode constraints are applied which exactly enforce a zero relative tangential displacement. It should be noted that in slipping mode the current friction force is not only a function of the current normal force and relative displacement, but also of the friction force during the previous iteration. This generally improves the stability of the nonlinear solution process. As opposed to the procedure based on the arctangent model, this procedure requires additional frictionbased testing. Changes in the friction status as well as too large changes in the friction forces compared to the previous iteration may cause the program to perform an additional iteration. In 2-D, the latter implies that the friction force should fulfil1: ft 1 – e ≤ ----p- ≤ 1 + e ft where f p is the friction force of the previous iteration and e is the above mentioned friction force t tolerance, with a default value of 0.05. In 3-D, in addition to this requirement on the magnitude of the friction force, a check is performed on the change in direction of the friction force vector: 1 – e ≤ cos ( ϕ f ) ≤ 1 + e in which ϕ f is the angle between the friction vector in the current and the previous iteration. In order to limit the amount of friction-related iterations, the above mentioned requirements will not cause extra iterations if the number of nodes not fulfilling the friction requirements compared to the total number of nodes in contact is small. This can be expressed in the friction force tolerance as: number of nodes which do not fulfil friction tolerances ----------------------------------------------------------------------------------------------------------------------------------- < e total number of nodes in contact and must be true for all contact bodies in the model. If the maximum number of iterations as defined on the CONTROL model definition option has been reached, additional friction iterations will not be enforced and the analysis will continue with the next increment. The stick-slip model is always based on nodal forces. This model is not recommended for quadratic elements in 3-D, because of the varying magnitude and sign of nodal forces of such elements. When using the PRINT parameter to get extra contact-related information in the output file, the program will echo the contact status, the ratio of the magnitude of the current and previous friction force vector (and in 3-D also the cosine of the angle between the current and previous friction force vector), as well as the total number of nodes with a friction contribution and the number of nodes with a friction contribution which do not fulfil the friction tolerance criteria.

Main Index

CHAPTER 8 539 Contact

Bilinear Model The third procedure is called the bilinear model. Similar to the modified step function model, it is based on relative tangential displacements. Instead of defining special constraints to enforce sticking conditions, the bilinear model assumes that the stick and slip conditions correspond to reversible (elastic) and permanent (plastic) relative displacements, respectively. The clear resemblance with the theory of elasto-plasticity will be used to derive the governing equations. First, Coulomb’s law for friction is expressed by a slip surface φ : φ =

f t – μf n

The stick or elastic domain is given by φ < 0 , while φ > 0 is physically impossible. Next, the rate of the relative tangential displacement vector is split into an elastic (stick) and a plastic (slip) contribution according to: p e u· t = u· t + u· t

(8-1)

and the rate of change of friction force vector is related to the elastic tangential displacement by: e f·t = Du· t

(8-2)

in which matrix D is given by:

D =

μf n -------δ

0

0

μf n -------δ

with δ the slip threshold or relative sliding displacement below which sticking is simulated (see Figure 8-26). The value of δ is by default determined by the program as 0.0025 times the average edge length of the finite elements defining the deformable contact bodies. Now attention is paid to the case that, given a tangential displacement vector, the evolution of f t would result in a physically impossible situation, so φ > 0 . This implies that the plastic or slip contribution must be determined. Equations (8-1) and (8-2) yield: · · ·p ft = D ( ut – ut )

Main Index

540 Marc Volume A: Theory and User Information

ft

μf n

δ

Δu t

δ slip threshold

Figure 8-26 Bilinear Model

It is assumed that the direction of the slip displacement rate is given by the normal to the slip flow potential ψ , given by: ψ =

ft

So that, by indicating the slip displacement rate magnitude as

· λ:

·p · ∂ψ u t = λ ------∂f t with the slip surface, φ , different from the slip flow potential, ψ an analogy to nonassociative plasticity can be observed. Since a ‘force point’ can never be outside the slip surface, it is required that: ∂φ T · · φ = ⎛ ------⎞ f t = 0 ⎝ ∂f t⎠ In this way, the magnitude of the slip rate can be determined. To this end, the equations above can be combined to: ∂φ ⎞ T ⎛ · · ∂ψ ⎛ ----D u t – λ -------⎞ = 0 ⎝ ∂f-t⎠ ⎝ ∂f t ⎠ or: ∂φ ⎞ T · ⎛ ----Du t ⎝ ∂f-t⎠ · λ = ---------------------------∂φ ⎞ T ∂ψ ⎛ ----D ------⎝ ∂f-t⎠ ∂f t

Main Index

CHAPTER 8 541 Contact

Utilizing this result, the final set of rate equations reads: ∂ψ ∂φ T ⎞ ⎛ D ------- ⎛ ------⎞ D⎟ ⎜ ∂f t ⎝ ∂f t⎠ · · * · f t = ⎜ D – ---------------------------------⎟ u t = ( D – D )u t T ⎜ ⎟ ∂φ⎞ ∂ψ ⎛ ----⎜ - ⎟ ⎝ ∂f-t⎠ D -----∂f t ⎠ ⎝ *

Similar to non-associative plasticity, matrix D will generally be non-symmetric. In Marc, a special procedure has been used which results in a symmetric matrix, while maintaining sufficient numerical stability and rate of convergence. The bilinear model also uses an additional check on the convergence of the friction forces, which has been achieved if the following equation is fulfilled: p

Ft – Ft --------------------------------- ≤ e Ft p

where F t is the current total friction force vector (the collection of all nodal contributions), F t is the total friction force vector of the previous iteration and e is the friction force tolerance, which has a default value of 0.05. In the output file one can find, per deformable contact body, information about the current total friction force, the current total normal force and the total friction force change, compared to the previous iteration. If a node comes into contact and the structure is still stress-free, then the friction stiffness matrix according to the derivation above will still be zero. This could result in an ill-conditioned system during the next solution of the global set of equations. To avoid this problem, the initial friction stiffness will be based on the average contact body stiffness (following from the trace of the matrix defining the material behavior), which is determined during increment 0 of the analysis. Alternatively, the user can define this initial friction stiffness via the PARAMETERS model definition or history definition option. Limitations of the Coulomb Model When the normal force or stress becomes large, the Coulomb friction model may not correlate well with experimental observations. This is caused by the fact that the Coulomb model predicts that the frictional shear stresses increase to a level that can exceed the flow stress or the failure stress of the material. As this is not physically possible, a different friction calculation should be applied. The choices are either to have a nonlinear coefficient of friction, or to introduce the friction stress limit in the bilinear model or to use the shear based friction model.

Main Index

542 Marc Volume A: Theory and User Information

σt

Linear Coulomb Model μ

Observed Behavior

σn Figure 8-27 Linear Coulomb Model versus Observed Behavior

A nonlinear friction coefficient can be defined via UFRIC user subroutine or via table driven input. limit

The friction stress limit for the bilinear model ( σ t

) can be entered via the CONTACT TABLE option

and is used to bound the maximum friction stress, based on the assumption that the extrapolated and averaged shear (friction) stress in a node is proportional to the applied shear (friction) force (see Figure 8-28). If the shear stress reaches the limit value, then the applied friction force is reduced, so that limit

the maximum shear stress is given by min ( μσ n, σ t

).

Finally, instead of using an adapted Coulomb friction model, one may use the shear friction model, which is the second idealistic friction model in Marc. σt Friction Stress Limit

μ

σn Figure 8-28 Friction Stress Limit used by Bilinear Model

Shear Friction The shear based model states that the frictional stress is a fraction of the equivalent stress σ in the material: σ σ σ t < m ------- (stick) and σ t = – m ------- ⋅ t (slip) 3 3 where m is the friction factor. Given the similarity with the Coulomb model, this shear model is implemented using two approximations of the theoretical step function. First, the arctangent function to smooth out the step function is applied:

Main Index

CHAPTER 8 543 Contact

vr σ 2 σ t = – m ------- --- arctan ⎛ -------------------------⎞ ⋅ t ⎝ ⎠ π RVCNST 3 This model is available for all elements using the distributed load approach. Second, the bilinear model has been adapted based on the assumption that the shear (friction) stress in a node is proportional to the applied shear (friction) force. Similar to the friction stress limit, the shear stress due to friction is limited by: σ σ t = min ⎛ mσ n, m -------⎞ ⎝ 3⎠ Friction Coefficient When a node contacts a rigid body, the coefficient of friction associated with the rigid body is used. When a node contacts a deformable body, the average of the coefficients for the two bodies are used. The CONTACT TABLE option can be used if complex situations occur. Recalling that friction is a complex physical phenomenon, due to variations in surface conditions, lubricant distribution, and lubricant behavior, relative sliding, temperature, geometry, and so on, it was decided to implement the above two friction models (Coulomb and shear), and to allow you to extend them, if necessary, by means of the UFRIC user subroutine or by referencing a table. In such a routine, you provide the friction coefficient or the friction factor as μ = μ ( x, f n, T, v r, σ ) or m = m ( x, f n, T, v r, σ ) where x

is the position of the point at which friction is being calculated

fn

is the normal force at the point at which friction is being calculated

T

is the temperature at the point at which friction is being calculated

vr

is the relative sliding velocity between point at which friction is being calculated and surface

σy

is the equivalent stress at the point at which friction is being calculated

Glue Model A special type of friction model is the glue option, which imposes that there is no relative tangential motion. The glue motion is activated through the CONTACT TABLE option.

Main Index

544 Marc Volume A: Theory and User Information

A novel application of contact is to join two dissimilar meshes. In such a case, by specifying that the glue motion is activated, the constraint equations are automatically written between the two meshes. Unless a flag has been set, nodes in contact via the glue option are not allowed to separate. When a node of a shell or beam element is glued to a load controlled rigid body or to the face of a shell or solid element, the rotation of the shell or beam can be suppressed. This allows a true moment carrying glued connection. For the case that a connection is made to the face of a solid element, the rotations of the touching node are connected to the translations of the nodes of the contacted patch by a constraint relation based upon the large rotation RBE3 theory. The moment carrying feature is optional and is activated through the CONTACT TABLE option.

Deact Glue Another option related to the glue option id DEACT GLUE. Suppose two bodies are glued together and a part of the interface should have standard contact (in order to model, for example, a crack), the nodes in the region that should have standard contact are then identified with DEACT GLUE. Without this option, one would have to split up the contact bodies in order to model this case.

Breaking Glue There is an option to break up the glued connection using a stress criterion. When the following criterion is fulfilled at a node, the glued contact is released: σ m σ n ⎛ -----n-⎞ + ⎛ -----t⎞ > 1 ⎝ S n⎠ ⎝ S t⎠

(8-3)

Here σ n is the contact normal stress, σ t the contact tangential stress, and S n , S t , m, and n are user-defined parameters. When a node is released due to breaking glued, it changes status from being glued to standard contact permitting separation and friction. The contact stresses are calculated using extrapolated stresses for solid elements and as contact force divided by equivalent area for shell elements. Nodal post codes are available for postprocessing the separate terms in Equation (8-3) as well as the sum. A nodal post code for the deact glue status is also available.

Separation After a node comes into contact with a surface, it is possible for it to separate in a subsequent iteration or increment. Mathematically, a node should separate when the reaction force between the node and surface becomes tensile or positive. Physically, you could consider that a node should separate when the tensile force or normal stress exceeds the surface tension. Rather than use an exact mathematical definition, you can enter the force or stress required to cause separation. Separation can be based upon either the nodal forces or the nodal stresses. The use of the nodal stress method is recommended as the influence of element size is eliminated.

Main Index

CHAPTER 8 545 Contact

When using higher-order elements and true quadratic contact, the separation criteria must be based upon the stresses as the equivalent nodal forces oscillate between the corner and midside nodes. In many analysis, contact occurs but the contact forces are small; for example, laying a piece of paper on a desk. Because of the finite element procedure, this could result in numerical chattering. Marc has some additional contact control parameters that can be used to minimize this problem. As separation results in additional iterations (which leads to higher costs), the appropriate choice of parameters can be very beneficial. When contact occurs, a reaction force associated with the node in contact balances the internal stress of the elements adjacent to this node. When separation occurs, this reaction force behaves as a residual force (as the force on a free node should be zero). This requires that the internal stresses in the deformable body be redistributed. Depending on the magnitude of the force, this might require several iterations. You should note that in static analysis, if a deformable body is constrained only by other bodies (no explicit boundary conditions) and the body subsequently separates from all other bodies, it would then have rigid body motion. For static analysis, this would result in a singular or nonpositive definite system. This problem can be avoided by appropriate boundary conditions. When the direct solvers are used, the AUTOSPC parameter may also be used to suppress singular modes.

Release A special case of separation is the intentional release of all nodes from a rigid body. This is often used in manufacturing analysis to simulate the removal of the workpiece from the tools. After the release occurs in such an analysis, there might be a large redistribution of the loads. It is possible to gradually reduce the residual force to zero, which improves the stability, and reduces the number of iterations required. The RELEASE history definition option allows the release (separation) of all the nodes in contact with a particular surface at the beginning of the increment. The rigid body should be moved away using the MOTION CHANGE option or deactivated using the CONTACT TABLE option to ensure that the nodes do not inadvertently recontact the surface they were released from.

Coupled Analysis Contact analysis has several consequences on performing a coupled analysis. When performing a coupled contact analysis between multiple deformable bodies, each body deforms due to mechanical and thermal loads and undergoes heat conduction. When the bodies come into contact, there is heat flux across the surfaces. You need to provide a coefficient of heat transfer between the surfaces. This is often quite significant as a hot workpiece might come into contact with a cold tool set. Additionally, if friction is present, heat is generated based upon: q = ff r ⋅ v r ⋅ Me q where M e q is the mechanical equivalent of heat. Half of the heat generated due to friction is contributed to each body. If the model allows a body to be rigid, two options are available. In the first case, the rigid body is considered to have a constant temperature (heat source or heat sink). Heat flux is exchanged between the rigid body and the deformable body. In the second case, it is required to perform a heat transfer analysis in the rigid body. In this case, the rigid body must be constructed of finite elements, but

Main Index

546 Marc Volume A: Theory and User Information

they are chosen as heat transfer types. Deformation does not occur in this body, but a heat transfer analysis is performed. This is computationally more efficient than performing a coupled analyses where all bodies are deformable. Symmetry bodies have different characteristics as they are frictionless (hence, no heat generated) and because there is no heat flux across a symmetry plane. Heat fluxes (FILMS) are automatically created on all the boundaries of the deformable-bodies. Three types of heat fluxes can be distinguished, where each flux has its own physical characteristic. The type of flux Marc uses, depends on the distance between the contacting bodies (see Figure 8-29). We define the distance, d c o n t a c t , as the distance below which the two bodies are touching each other. For a distance smaller than d c o n t a c t , the first flux type is used. The second flux type is used when the distance is between d c o n t a c t and d n e a r , where d n e a r is called the near contact distance. This distance represents a small gap between the contact bodies, and should not be chosen larger than the smallest element size. If this distance is not set, this type of flux is disregarded. The third flux type is used when the distance is larger then d n e a r . T1 d T2 Figure 8-29 Contact Distance

If d < d c o n t a c t , the bodies touch and conduction takes place between the two contacting bodies. The heat flux is written as: q = HT C ( T2 – T1 ) where T1

is the surface temperature,

HT C

is the film coefficient between the two surfaces,

T2

is the temperature of the same contact location, as obtained from interpolation of nodal temperatures of the body being contacted.

If d c o n t a c t < d < d n e a r , a small gap between the bodies exists. The heat flux that exists through this gap can be decomposed in the following physical processes: convection, natural convection, radiation, and a distance dependent term. This flux is given by:

Main Index

CHAPTER 8 547 Contact

q = HC V ( T2 – T1 ) + HN C ( T2 – T1 )

B

NC

4

4

+ σεf ( T A 2 – T A 1 )

⎧ d ⎫ d + ⎨ H C T ⎛ 1 – -------------⎞ + H B L ------------- ⎬( T 2 – T 1 ) ⎝ ⎠ d d near near ⎭ ⎩ where HC V

is the convection coefficient for near field behavior.

HN C

is the natural convection coefficient for near field behavior.

BC N

is the exponent associated with natural convection.

σ, ε, and f

are the coefficients for radiation, the Stefan-Boltzman coefficient, the emissivity, and the viewfactor, respectively. The Stefan-Boltzman constant is given via the PARAMETERS option.

HB L

is the separation distance dependent heat transfer coefficient.

TA 2

T 2 + T A B S R E F is the temperature in absolute scale. The offset between the user temperature and the absolute temperature is given in the PARAMETERS option.

If d > d n e a r , or d n e a r has not been defined and d > d c o n t a c t , the bodies are not touching and a heat flux to the environment exists in the following form, 4

4

q = H C T VE ( T 2 – T S I NK ) + σεf ( T A 2 – T A 1 ) where HC T V E

is the heat transfer coefficient to the environment

T S I NK

is the environment sink temperature

When a deformable-body contacts a rigid-body, the coefficients associated with the rigid-body are used. When two deformable bodies are in contact, the average value of the film coefficient specified for the bodies is used. This only works for the coefficients discussed in the first and third heat flux type. A better way to prescribe the coefficients is to use the CONTACT TABLE option. With this option, all the previously discussed coefficients can be set for each interface separately. For the second heat flux type, this is the only way to specify the coefficients. As with all other coupled problems, heat generated by plastic deformation can be calculated and applied as a volumetric flux. The heat generated by friction is also calculated and applied as a surface flux. Three user subroutines are available to facilitate the creation of more sophisticated boundary flux definitions (such as radiation and convections with variations in space, temperature, pressure, etc.). UHTCON allows you to specify a film coefficient while the surface is in contact ( d < d c o n t a c t ),

Main Index

548 Marc Volume A: Theory and User Information

UHTNRC allows you to specify a film coefficient while the surface is almost in contact

( d c o n t a c t < d < d n e a r ), and UHTCOE allows you to specify a film coefficient while the surface is free ( d > d n e a r ).

Thermal Contact A thermal contact analysis is performed when no structural pass is present, this results in a computationally more efficient analysis. Possible analyses types are Heat Transfer, Coupled ThermalElectrical, Magnetostatics and Electrostatics. For Heat Transfer and Coupled Thermal-Electrical the analysis is comparable to a coupled analysis. The two types of rigid bodies that are described in the coupled analysis are allowed. So one is a rigid which is considered to have a constant temperature (heat source or heat sink), and the other is a finite element body with thermal properties. The three types of heat fluxes as described in Coupled Analysis can also be used here. The coefficients are prescribed in the same way as in a Coupled Analysis where it is advised to use the CONTACT TABLE option. The three user subroutines UHTCON, UHTNRC, and UHTCOE as previously discussed in Coupled Analysis can also be used in a Heat Transfer and Coupled Thermal-Electrical analysis.

Joule Heating In a Joule heating analysis similar conditions as thermal contact apply regarding the flow of current between contacting bodies. If d < d c o n t a c t , the bodies touch and electrical conduction takes place between the two contacting bodies. The current is written as: i = H E C ( V 2 – V 1 ) or H E C ( V b o d y – V 1 ) where V1

is the surface voltage,

HE C

is the electrical contact conductivity,

V2

is the voltage of the same contact location, as obtained from interpolation of nodal voltages of the body being contacted.

VB o d y

is the voltage of the rigid body being touched.

If d c o n t a c t < d < d n e a r , a small gap between the bodies exists. The current that exists through this gap can be decomposed into: ⎧ d ⎫ d i = H NE ( V 2 – V 1 ) + ⎨ H E C ⎛ 1 – -------------⎞ + H B L E ------------- ⎬( V 2 – V 1 ) ⎝ ⎠ dn e a r ⎭ dn e a r ⎩

Main Index

CHAPTER 8 549 Contact

where HN E

is the coefficient for near field behavior.

HB L E

is the separation distance dependent conductivity coefficient.

If d > d n e a r , or d n e a r has not been defined and d > d c o n t a c t , the bodies are not touching and a current leakage to the environment exists in the following form, q = H V E ( V SI N K – V 1 ) where HV E

is the coefficient to the environment

VS I N K

is the environment sink voltage

Electrical contact between bodies does contribute a term to the heat generation. Note that near electrical contact for Joule heating does not represent electrical arcing between bodies, which is a much more complex phenomena. In a Joule heating analysis the THERMAL CONTACT option is also used to identify elements which are in a conducting body to perform a resistance calculation using EMRESIS. Three user subroutines are available to facilitate the creation of more sophisticated boundary definitions. UVTCON allows you to specify a film coefficient while the surface is in contact ( d < d c o n t a c t ), UVTNRC allows you to specify a film coefficient while the surface is almost in contact

( d c o n t a c t < d < d n e a r ), and UVTCOE allows you to specify a film coefficient while the surface is free ( d > d n e a r ).

Contact in an Electrostatic or Piezoelectric Analysis In an electrostatic analysis if two bodies are in contact, the scalar potential is tied between the bodies composed of elements. For an electrostatic analysis the THERMAL CONTACT option is used. When a node is in contact with a symmetry surface it will be treated as a free surface, that is no current transmitted through the symmetry surface. The THERMAL CONTACT option is also used to identify the elements which are in a conducting body to perform a capacitance calculation using EMCAPAC. In such cases, the conducting bodies should not be in contact. Cyclic symmetry may not be used in a pure electrostatic analysis in this release.

Main Index

550 Marc Volume A: Theory and User Information

Contact in Magnetostatic Analysis For Magnetostatics all the degrees of freedom of the magnetic vector potential are tied for nodes in contact. When a node is in contact with a symmetry surface a constraint is imposed such that only the normal component of the potential is zero. For a magnetostatic analysis the THERMAL CONTACT option is used. Cyclic symmetry may not be used in a pure magnetostatic analysis in this release.

Contact in Electromagnetic Analysis Contact is not currently supported in harmonic or transient electromagnetic analysis.

Contact in Soil Analysis When two deformable bodies are in contact the displacements are treated in the conventional manner. The pressure degree of freedom associated with the fluid hydrostatic pressure is tied. If a node contacts a rigid body, nothing is done with the pressure degree of freedom.

Contact in an Acoustic Analysis In an acoustic analysis with flexible and/or rigid walls composed of finite elements and/or rigid bodies, a coupling interface between the acoustic medium and the walls is created to connect the fluid pressure to the wall movement taking into account accelerations and reactive boundary conditions.

Element Considerations Marc allows contact with almost all of the available elements, but the use of certain elements has a consequence on the analysis procedure. Contact analysis can be performed with all of the structural continuum elements, either lower order or higher order, including those of the Herrmann (incompressible) formulation, except axisymmetric elements with twist. Friction modeling is available in all of these elements except the semi-infinite elements. Higher-order isoparametric elements use shape functions which, when the elements are loaded by a (for example) uniform pressure, lead to equivalent nodal loads that oscillate between the corner and midside nodes. This has a detrimental effect on determining contact separation and two procedures have been implemented to eliminate this problem: 1. Linearized Contact: The midside nodes on the exterior surface are automatically tied to the corner nodes in this case. This effectively results in a linear variation of both the geometry and the displacement on the exterior element edges. Hence, the elements with edges on the exterior do not behave as full bi-quadratic (2-D) or tri-quadratic (3-D) elements. All elements in the interior of the body behave in the conventional higher-order manner, but the constraints on the exterior easily cause the behavior of the complete structure to be too stiff; while in the area of contact, the stress distribution might be irregular.

Main Index

CHAPTER 8 551 Contact

2. True Quadratic Contact: No special constraints introduced on the exterior surface other than coming from contact in this case. Both the midside and the corner nodes may come into contact and when contact is established with another deformable body consisting of quadratic elements, a constraint equation corresponding to the complete quadratic shape function is automatically incorporated. Since the above mentioned oscillating nodal loads cannot be used for separation, the decision whether or not a node should separate is based on the contact normal stress rather than the contact normal force. In many manufacturing and rubber analyses, the lower-order elements behave better than the higher-order elements because of their ability to represent the large distortion; hence, these lower-order elements are recommended. The constraints imposed on the nodal degrees of freedom are dependent upon the type of element. 1. When a node of a continuum element comes into contact, the translational degrees of freedom are constrained. 2. When a node of a shell element comes into contact, the translational degrees of freedom are constrained and no constraint is places on the rotational degrees of freedom. The exception to this is when a shell contacts a symmetry surface. In this case, the rotation about the element edge is also constrained. Additionally, beams and shells contact is governed by the rules outlined below.

2-D Beams All nodes on beams are potential contact nodes. Beam elements can be used in contact in two modes. 1. The two-dimensional beams can come into contact with rigid bodies composed of curves in the same x-y plane. The normal is based upon the normal of the rigid surface. 2. The two-dimensional beams can come into contact with deformable bodies either of continuum elements or other beam elements. As the beams are in two dimensions, they do not intersect one another.

3-D Beams Three-dimensional beam elements can be used in contact in three methods. 1. The nodes of the beams can come into contact with rigid bodies composed of surfaces. The normal is based upon the normal of the rigid surface. 2. The nodes of the beam and truss elements can also come into contact with the faces of threedimensional continuum elements or shell elements. The normal is based upon the normal of the element face. 3. The three-dimensional beam and truss elements can also come into contact with other beam or truss elements (beam-to-beam contact). The first two methods are activated by default if contact bodies consisting of beam or truss elements are defined using the CONTACT option. The third method must be activated explicitly by additionally switching on the beam-to-beam contact flag on the CONTACT option.

Main Index

552 Marc Volume A: Theory and User Information

In the beam-to-beam contact model, a beam or truss element is viewed as a conical surface with a circular cross-section. The radius of the cross-section can vary linearly between the start and end node of a beam element. For each beam or truss element of a contact body, a contact radius must be entered via the GEOMETRY option. The contact radius at a node follows from the average contact radius of the elements sharing that node. Hence, the start and end node of an element may have different contact radii. Contact is detected between two beam or truss elements if the associated conical surfaces touch each other; that is, if the distance d between the closest points on the conical surfaces is smaller than the distance below which bodies are considered touching each other. This is outlined in Figure 8-30, where beam elements and their contact body representation are given. It should be emphasized that the contacting points are points on the conical surfaces and not nodes of the finite element model.

d

Y X

Z

Figure 8-30 Beam-to-Beam Contact: Finite Element Model (top) and Contact Body Representation (bottom)

If two beam or truss elements are in contact, a multipoint constraint equation (tying) is automatically imposed to ensure that the conical surfaces will not interpenetrate. This constraint equation involves the displacements of the begin and end nodes of both elements. The tied node in that equation is automatically selected, taking into account the location of the contacting points with respect to the elements, any boundary conditions applied to the nodes and any contact between the nodes and rigid surfaces or faces of continuum or shell elements. During the iteration procedure, the contacting points of two beam or truss elements can change if the elements slide with respect to each other. In addition, the points in contact can move from one element to another. In that case, the nodes involved in the multipoint constraint equations are automatically updated. During sliding, friction may be taken into account. Since for beam or truss elements the normal

Main Index

CHAPTER 8 553 Contact

stress in the contact points is not available, only Coulomb friction based on nodal forces (either the arctangent or the bilinear model) is supported for beam-to-beam contact. The glue model, which imposes that there is no relative tangential motion, is also available. A limitation of the beam-to-beam contact model is that a contact body cannot contain branches, that is, every element in the contact body must have a unique successor and predecessor.

Shell Elements All nodes on shell elements are potential contact nodes. As the midside nodes of shell elements are automatically tied, the high-order shell element (type 22) has no benefit. Shell elements can contact either rigid bodies, continuum elements, or other shell elements. Shell-shell contact involves a more complex analysis because it is necessary to determine which side of the shell contact occurs. By default, the top and bottom face of a shell element (which follow from the mid face by using the thickness offset vector) are separately taken into account. This implies that a node may be found to be in contact based on the top or the bottom face of an element. However, due to the nature of the shell formulation, it is not possible to simultaneously use contact conditions following from the top and the bottom face. Touching a shell element may also occur at its top or bottom face. The user has the option to set per pair of contact bodies on the CONTACT TABLE option how the geometry of the shell elements should be handled. This means that both for the contacting and the contacted body it can be defined that the contact description will be based on one of the following options: both top and bottom (default), top only (with or without the thickness offset vector) or bottom only (with or without the thickness update vector). For glued contact it is possible to use the top and bottom face, but without the thickness update vector. The beam-to-beam contact model discussed above can also be used to model shell edge-to-edge contact. This requires switching on the beam-to-beam contact flag on the CONTACT option and, for a shell contact body combination, the edge-to-edge contact flag on the CONTACT TABLE option. For edge-toedge contact, half of the thickness of the shell is used to set the contact radius.

Dynamic Impact The capability is available for both implicit time integration via the Newmark-beta or Houbolt operators, and the explicit time integration via the (fast) central difference operator. The Newmark-beta, Single Step Houbolt and Generalized Alpha procedure have the capability to allow variable time steps and, when using the user-defined fixed time step procedure, the time step is split by the algorithm to satisfy the contact conditions. Since the central difference operator is constrained to small time steps by the stability requirement, time splitting is not used by the contact algorithm. For most dynamic impact problems, the Single Step Houbolt method is recommended, as this procedure possesses high-frequency dissipation. This is often necessary to avoid numerical problems by contactinduced high-frequency oscillations. If the other dynamic operators are used, it is recommended that numerical damping is used during the analysis, or, when using the Generalized Alpha method, that a small spectral radius is defined. Note that for a zero spectral radius, the Generalized Alpha method is identical to the Single Step Houbolt method with default parameters ( γ

Main Index

1

= 1.5 , γ = – 0.5 ).

554 Marc Volume A: Theory and User Information

In dynamic analysis, the requirement of energy conservation is supplemented with the requirement of momentum conservation. In addition to the constraints placed upon the displacements, additional constraints are placed on the velocity and acceleration of the nodal points in contact, except for the Single Step Houbolt and Generalized Alpha method. When a node contacts a rigid surface, it is given the velocity and acceleration of the rigid surface in the normal direction. The rigid surfaces are treated as if they have infinite mass, hence, infinite momentum.

Global Adaptive Meshing and Rezoning In manufacturing simulations the objective is to deform the workpiece from some initial (simple) shape to a final, often complex shape. This deformation of the material, results in mesh distortion. For this reason, it is often required to perform a rezoning/remeshing step. At this point, a new mesh is created; the current state of deformation, strains, stresses, etc. is transferred to the new mesh, and the analysis is continued. This has several consequences for contact analysis. 1. When manual rezoning is used, it is necessary to redefine the elements associated with the deformable body that is being rezoned. This is done through the CONTACT CHANGE option. 2. If a contact tolerance was not defined by you, a new contact tolerance is calculated based upon the new mesh. This distance can be smaller than the previously calculated tolerance, leading to more iterations. 3. After the new mesh is created, the program redetermines the potential contact nodes. The memory is automatically allocated to accommodate the contact data in the new mesh. 4. At the first increment after remeshing, Marc determines which nodes are in contact. If the new mesh does not reflect the exterior surface of the old model, it is possible that a region that was previously in contact is no longer in contact. This is usually not so serious; as most likely, the node subsequently comes into contact. A more significant problem is if a node in the new mesh is created which, in fact, has penetrated another body. If the newly created node is beyond another body’s surface by more than the contact tolerance, it is possible that a poor contact analysis results. With automatic global remeshing, steps are taken to made sure contact conditions are preserved and incorrect penetrations are removed in the new mesh. This is achieved by correcting the nodal position after a new mesh is created. If rezoning occurs, rigid surfaces must be kept the same and cannot be changed. Marc auto-rezoning feature, activated by the parameter REZONING,1 for 2-D problems and REZONING,2 for 3-D problems, automatically creates new meshes and performs rezoning to resolve mesh distortion problems. In such cases, points (1) and (4) are treated automatically.

Adaptive Meshing Contact between a deformable-body and a rigid body is insured such that the nodes do not penetrate the rigid surface. It is possible that an edge of an element penetrates a rigid surface, especially where high curvature is present because of the finite element discretization. The use of the adaptive mesh generation procedure can be used to reduce these problems.

Main Index

CHAPTER 8 555 Contact

In addition to the traditional error criteria such as Zienkiewicz-Zhu or maximum stress, etc., you can request that the mesh be adaptively refined due to contact. In such a case, when a node comes into contact, the elements associated with that node are refined. This results in a greater number of elements and nodes on the exterior region where contact occurs. This can lead to a substantial improvement in the accuracy of the solution.

Penetration of Element Edge due to Mesh Discretization

Result of Adaptive Meshing

Figure 8-31 Contact Closure Condition

The adaptive meshing procedure has consequences to the contact procedure similar to the rezoning procedure. If a contact tolerance was not defined by you, a new contact tolerance is calculated based upon the new mesh. This distance can be smaller than the previously calculated tolerance, leading to more iterations.

Result Evaluation The Marc post file contains the results for both the deformable bodies and the rigid bodies. In performing a contact analysis, you can obtain three types of results. The first is the conventional results from the deformable body. This includes the deformation, strains, stresses, and measures of inelastic behavior such as plastic and creep strains. In addition to reaction forces at conventional boundary conditions, you can obtain the contact forces and friction forces imparted on the body by rigid or other deformable bodies. By examining the location of these forces, you can observe where contact has occurred, but Marc also allows you to select the contact status as a post file variable: A value of 0 means that a node is not in contact. A value of 0.5 means the node is in near thermal contact. A value of 1 means that a node is in contact. A value of 2 means the node is on a cyclic symmetry boundary. It is also possible to obtain the resultant force following from contact on the deformable bodies and the resultant force and moment on the rigid bodies. The moment is taken about the user-defined centroid of the rigid body. The time history of these resultant forces are of significant issues in many engineering analysis. Of course, if there is no resultant force on a rigid body, it implies that body is not in contact with any deformable body.

Main Index

556 Marc Volume A: Theory and User Information

Finally, if the additional print is requested via the PRINT parameter, the output file reflects information on when a node comes into contact, what rigid body/segment is contacted, when separation occurs, when a node contacts a sharp corner, the displacement in the local coordinate system, and the contact force in the local coordinate system. For large problems, this can result in a significant amount of output. The motion of the rigid bodies can be displayed as well as the deformable bodies. Rigid bodies which are modeled using the piecewise linear approach are displayed as line segments for flat patches. When the rigid surfaces are modeled as analytical surfaces, the visualization appears as piecewise linear in older versions (pre-K7/Mentat 3.1) or as trimmed NURBS in subsequent versions.

Tolerance Values On the third data block for contact, five tolerances can be set for determination of the contact behavior. Not entering any values here means that Marc calculates values based on the problem specification. Relative Sliding Velocity Between Surfaces Below Which Friction Forces Drop As discussed in the Friction Modeling section, the equations of friction are smoothed internally in the program to avoid numerical instabilities. The equations are inequalities whenever two contacting surfaces stick to each other and equalities whenever the surfaces slide (or slip). Thus, the character of contact constraints change depending on whether there is sticking or slipping. The smoothing procedure consist of modifying it in such a way, that there is always slip; the amount is a function of the relative velocity and a constant RVCNST. The value of this constant must be specified here. It actually means, that if we specify a small value in comparison to the relative velocity, the jump behavior is better approximated, but numerical instabilities can be expected. A large value means, that we need a large relative velocity before we get the force at which the slip occurs. It is suggested to use values between 0.1 and 0.01 times a typical surface velocity. Distance Below Which a Node is Considered Touching a Surface In each step, it is checked whether a (new) node is in contact with other surfaces. This is determined by the distance between the nodes and the surfaces. Since the distance is a calculated number, there are always roundoff errors involved. Therefore, a contact tolerance is provided such that if the distance calculated is below this tolerance, a node is considered in contact. A too large value means that a high number of body nodes are considered to be in contact with the surface and are consequently all moved to the surface, which can be unrealistic in some applications. A too small value of this number means that the applied deformation increment is split into a high number of increments, thus increasing the cost of computation. The tolerance must be provided by the analyst or can be calculated by Marc. In general, the contact tolerance should be a small number compared to the geometrical features of the configuration being analyzed. The value calculated by Marc is determined as 1/20 of the smallest element size for solid elements or 1/4 of the thickness of shell elements. If both shell and continuum elements are present, the default is based upon the smaller of the two values.

Main Index

CHAPTER 8 557 Contact

Tolerance on Nodal Reaction Force or Nodal Stress Before Separation Occurs If a tensile force occurs at a node which is in contact with a surface, the node should separate from the surface. Rather than using any positive value, a threshold value can be specified. This number should theoretically be zero. However, because a small positive reaction might be due only to errors in equilibrium, this threshold value avoids unnecessary separations. A too small value of this force results in alternating separation and contact between the node and the surface. A too large value, of course, results in unrealistic contact behavior. Marc calculates this value as the maximum residual force in the structure. Note that the maximum residual force can be specified in the CONTROL option. Default for this value, a 10 percent of the maximum reaction force is used. Consequently, if locally high reaction forces at a particular point are present, the separation force is large as well. In most cases, however, the default value is a good measure. If you indicate that separation is to be based upon stresses, a value of the separation stress should be entered. The default value is the maximum residual force at a node divided by the contact area of node n.

Numerical and Mathematical Aspects of Contact Lagrange Multipliers In performing contact analysis, you are solving a constrained minimization problem where the constraint is the ‘no penetration’ constraint. The Lagrange multiplier technique is the most elegant procedure to apply mathematical constraints to a system. Using this procedure, if the constraints are properly written, overclosure or penetration does not occur. Unfortunately, Lagrange multipliers lead to numerical difficulties with the computational procedure as their inclusion results in a nonpositive definite mathematical system. This requires additional operations to insure an accurate, stable solution which leads to high computational costs. Another problem with this method is that there is no mass associated with the Lagrange multiplier degree of freedom. This results in a global mass matrix which cannot be inverted. This precludes the used of Lagrange multiplier techniques in explicit dynamic calculations which are often used in crash simulations. The Lagrange multiplier technique has often been implemented in contact procedures using special interface elements such as the Marc gap element (type 12). This facilitates the correct numerical procedure, but puts a restriction on the amount of relative motion that can occur between bodies. The use of interface elements requires an apriori knowledge of where contact occurs. This is unachievable in many physical problems such as crash analysis or manufacturing simulation.

Penalty Methods The penalty method or its extension, the Augmented Lagrangian method, is an alternative procedure to numerically implement the contact constraints. Effectively, the penalty procedure constrains the motion by applying a penalty to the amount of penetration that occurs. The penalty approach can be considered as analogous to a nonlinear spring between the two bodies. Using the penalty approach, some penetration occurs with the amount being determined by the penalty constant or function. The choice of the penalty value can also have a detrimental effect on the numerical stability of the global solution procedure. The penalty method is relatively easy to implement and has been extensively used in explicit dynamic

Main Index

558 Marc Volume A: Theory and User Information

analysis although it can result in an overly stiff system for deformable-to-deformable contact since the contact pressure is assumed to be proportional to the pointwise penetration. The pressure distribution is generally oscillatory.

Hybrid and Mixed Methods In the hybrid method, the contact element is derived from a complementary energy principle by introducing the continuity on the contact surface as a constraint and treating the contact forces as additional elements. Mixed methods, based on perturbed Lagrange formulation, usually consist of pressure distribution interpolation which is an order less than the displacement field, have also been used to alleviate the difficulties associated with the pure Lagrange method.

Direct Constraints Another method for the solution of contact problems is the direct constraint method. In this procedure, the motion of the bodies is tracked, and when contact occurs, direct constraints are placed on the motion using boundary conditions – both kinematic constraints on transformed degrees of freedom and nodal forces. This procedure can be very accurate if the program can predict when contact occurs. This is the procedure that is implemented in Marc through the CONTACT option. No special interference elements are required in this procedure and complex changing contact conditions can be simulated since no apriori knowledge of where contact occurs is necessary. The details of the implementation are presented later. Contact can be defined as finding the displacement of points A and B such that ( u A – u B ) ⋅ n < TOL where A is on one body and B is on another body, n is the direction cosine of a vector between the two points, and TOL is the closure distance.

A

B n

Figure 8-32 Normal Gap Between Potentially Contacting Bodies

Lagrange Multiplier Procedure In the Lagrange Multiplier Procedure, the variational procedure is augmented by the constraint. The virtual work principle leads to the traditional systems equation: Ku = f The constraint conditions can be expressed as Cu = 0

Main Index

CHAPTER 8 559 Contact

Through the minimization of the augmented functional T T 1 T Ψ = --- u Ku – u f + λ Cu 2

you obtain T K C ⎧⎨ u ⎫⎬ = ⎧⎨ f ⎫⎬ ⎩0 ⎭ C 0 ⎩λ ⎭

This equation can be solved simultaneously for both the displacement ( u ) and the Lagrange multiplier ( λ ). Note that the introduction of Lagrange multipliers results in a zero on the diagonal. Hence, even well posed physical problems no longer have positive definite systems. This often results in numerical difficulties and restricts the type of linear equation solver that can be used.

Direct Constraint Procedure Marc divides contact problems into two domains; the first is when a deformable body makes contact with a rigid surface and the second is when a deformable body makes contact with another deformable body or itself. Two-dimensional or three-dimensional bodies are treated conceptually in the same manner. Deformable-Rigid Contact In such a problem, a target node on the deformable body has no constraint while contact does not occur. Once contact is detected, the degrees of freedom are transformed to a local system and a constraint is imposed such that Δu n o r m a l = v ⋅ n where v is the prescribed velocity of the rigid surface. This local transformation is continuously updated to reflect sliding of point A along the rigid surface. If the glue option is activated, an additional displacement constraint is formed as Δu tangential = v ⋅ t The determination of when contact occurs and the calculation of the normal vector are critical to the numerical simulation. Historically in Marc, three procedures are used for detecting penetration and imposing contact, but now two of them are preferred and are discussed here. The first (and most general one) is the Iterative Penetration Checking Procedure. The second one (Time Step Reduction Procedure) is recommended only for a transient dynamic analysis with automatic time stepping. In Figure 8-34, node A is not in contact with the rigid body at the beginning of an iteration. After time step Δt , node A penetrates rigid surface if no constraint is imposed during the iteration which is not an acceptable solution.

Main Index

560 Marc Volume A: Theory and User Information

A

B

B A

Before Contact

y

t

n After Contact

x z

Figure 8-33 Contact Coordinate System

A

Start of Iteration, No Contact

A

End of Iteration, If No Constraint

Figure 8-34 Contact Constraint Requirement

The Iterative Penetration Checking Procedure checks for every iteration in the Newton-Raphson process if the displacement solution found would cause nodes to penetrate. If this is the case, the iterative displacement solution is scaled such that at the start of the subsequent iteration, new contact will be established. Some mathematical details can be found at the end of this chapter. When in a transient dynamic analysis, the adaptive time stepping procedure AUTO STEP is used, Marc reduces the time step of the current increment such that nodes, which would penetrate based on the original time step, will just come into contact. In the current increment, no contact constraints are applied to these nodes. In the next increment, the nodes are given the appropriate contact constraints and a new time step is determined based upon the convergence criteria.

Main Index

CHAPTER 8 561 Contact

8

Analytical Contact

Contact

Utilizing the analytical representation of rigid surfaces influences the numerical procedure in several ways: 1. The rigid surface is represented by a nonuniform rational B-spline surface (NURBS) which provides a precise mathematical form capable of representing the common analytical shapes – circle, conic curve, free-form curves, surfaces of revolution, and sculptured surfaces. The surface can be expressed in simple mathematical form to model complex multiple surfaces with advantage of continuity in first and second derivative. Those analytical forms are expressed in four-dimensional homogeneous coordinate space by: n+1

m+1

∑

∑

B i, j h i, j N i, k ( u )M j, l ( v )

j = 1 = 1 P ( u, v ) = i---------------------------------------------------------------------------------------n+1 m+1

∑

∑

i = 1

j = 1

h i, j N i, k ( u )M j, l ( v )

For curves, it simplifies to: n+1

∑

B i h i N i, k ( u )

= 1 P ( u ) = i----------------------------------------n+1

∑

h i N i, k ( u )

i = 1

where the B are 4-D homogeneous defining polygon vertices, N i, k and M j, l are nonrational B-spline basis functions, hi,j is homogeneous coordinates. For given parameters u and v in local system, the location (x, y, z) in three-dimensional space, first derivative and second derivative (if required), are calculated. Given a point with x, y and z Cartesian coordinates, there is no explicit mathematical form to find out the parameters u and v in the local space, so they are obtained using an iterative procedure. 2. The location of the closest point on the contact surface corresponding to node A needs to be determined. This process, determined analytically when using flat patches, requires an iterative approach for rigid bodies modeled with NURBS. A P

Figure 8-35 Closest Point Projection Algorithm

Main Index

562 Marc Volume A: Theory and User Information

3. Once the point P is known, the normal is calculated based upon the NURBS. This normal is used in a manner consistent with the PWL procedure. 4. Because the normal can change from iteration to iteration, the imposition of the kinematic boundary conditions is continuously changing. In the PWL approach: ( Δu n )

0

= v⋅n

i

( δu n ) = 0 In the analytical approach: ( Δu n )

0

= v ⋅ n0

i

( δu n ) = v ⋅ n 1 – v ⋅ n 0 where the subscripts represent the iteration number. 5. In the PWL approach, when a node slides from one segment to another, the corner condition logic is activated. The advantages of analytical surfaces is that this logic is not necessary until you come to the end of the spline. This reduces the amount of iterations required. 6. The friction calculation is dependent upon the surface normal and tangent. When using the analytical approach, the friction calculation includes the effect of changes in the direction of the normal vector from iteration to iteration. This improves the accuracy and convergence behavior. 7. Because the normal is continuous, the calculation of nodal forces is more accurate. This allows for the determination of nodal separation to occur beginning with the second iteration as opposed to when equilibrium convergence has been achieved using the PWL approach. Solution Strategy for Rigid Contact Step 1: At the start of an increment, all boundary nodes are checked for contact with surfaces and flagged if so. If the Iterative Penetration Checking Procedure has detected potential penetration, this is repeated at the start of an iteration. Step 2: Next, transformations and imposed displacements are determined for each touching node. With the knowledge of the time increment and surface velocity, the configuration of the surface at the end of the increment is found. Then, the distance from the node starting position to the current surface segment is determined and is the probable normal displacement to be imposed. If there is a previous solution for displacement increments, these are used to estimate the tangential displacement increment (Figure 8-36). If this estimate still puts the node at the end of the increment in the same surface segment, then this one is used to determine the transformation matrix between local and global coordinates, and the normal displacement is accepted. Otherwise, the procedure is repeated for the adjacent segment. If a concave corner is hit, the boundary node is fixed to such corner. If the node goes out of a sharp convex corner, it is immediately released from the surface.

Main Index

CHAPTER 8 563 Contact

SEGB

SEGB - Die segment at beginning of increment SEGE - Die segment at end of increment

P

Δu

Δu Δun

Δun

Δutest - Estimate of tangential displacement β - Angle used in transformation matrix

SEGE Δutest

β

- Displacement increment of previous increment - Imposed normal displacement

Figure 8-36 Node P Already In Contact (2-D)

Step 3: One increment of the problem is solved iteratively. During each iteration, the Iterative Penetration Checking Procedure checks if the current iterative displacement solution must be scaled to avoid penetration (Figure 8-37). If needed, Step 1 is repeated to establish new contact constraints. Step 2 is repeated at each iteration for possible changes in surface segment. SEGB A

SEGE B

SEGB - Die segment at beginning of iteration SEGE - Die segment at end of iteration

Δu P

Δu

- Iterative Displacement calculated

PB -------PA

- Factor to scale iteration

Figure 8-37 New Node in Contact P

Step 4: Once convergence is obtained, nodal forces are checked. Whenever a positive normal force (or stress) is detected which is larger than the tolerance, a node is released from the surface segment at which such force (or stress) corresponds and Step 3: is repeated. This tolerance can be modified using the SEPFOR or SEPSTR user subroutine. Step 5: Go to next increment (Step 1:).

Main Index

564 Marc Volume A: Theory and User Information

PATB P

Δu Δun

PATE

Δutest 3 2

1

PATB - Patch at beginning of increment PATE - Patch at end of increment Δu Δun

- Previous displacement increment of Node P - Imposed normal displacement increment (local direction 3) Δutest - Estimated tangential displacement Figure 8-38 Node P Already in Contact (3-D)

Deformable-Deformable Contact When a node contacts a deformable body, a tying relation is formed between the contacting nodes and the nodes of the contacted segment on the other body. This constraint relationship uses information regarding the normal vector to the segment and the closest point projection of the contacting node on the contacted segment. For lower-order elements, the normal vector and the projection are calculated based upon the piecewise linear representation of the element. This has the consequence that the constraint relation may not be accurate because the normal vector is constant over the complete segment, whereas the actual structure may be curved with a varying normal vector. When a node slides from one segment to another, there may be a discontinuity of the normal vector, which leads to potential numerical difficulties or an inaccurate solution. This is especially important for contact analyses where the deformations are small. When higher-order elements are used, the normal vector and projection are created based upon the true quadratic element description. Provided that the midside nodes are defined to be on the actual curved geometry, this improves the accuracy, but does not necessarily result in continuity of the normal vector at nodes shared by multiple segments.

Main Index

CHAPTER 8 565 Contact

Actual Geometry

Finite Element Approximation

Cubic Spline Representation

: Nodes with a normal vector discontinuity Figure 8-39 2-D Deformable Contact; Piece wise Linear FE Description and Cubic Spline Representation

Both for lower- and higher-order elements, you can fit a smooth curve (2-D) or surface (3-D) through the finite element segments. For 2-D, a cubic spline is used (see Figure 8-39). This spline is calculated based upon the tangent and position vectors of the nodes on the segment. For lower-order elements, each segment is internally replaced by one cubic spline; where for higher-order elements, each segment is replaced by two cubic splines. This gives a more accurate representation of the actual physical geometry and a more accurate calculation of the normal vector. You must identify where actual discontinuities exist. This is done by defining nodes where the normal vector is discontinuous or by activating the option that the program will determine such nodes based on the angle spanned by the normal vectors to adjacent segments. You can use the SPLINE option to define deformable bodies in 2-D or 3-D where the smoothness is required. For 3-D problems, the concept of a cubic spline can be expanded to generate a Coons surface to improve the geometric representation of a segment (see Figure 8-40). When calculating the closest point projection, it is advantageous to replace the Coons surface description by a cubic serendipity surface. For 2-D problems, you have to define nodes where the actual normal vector has a discontinuity; for 3-D problems, you have to specify edges where the normal vector is discontinuous. The SPLINE option allows you to enter a list of nodes (where each edge is defined by its start and end node) or to activate the option that the program will determine such edges based on the angle spanned by the normal vectors to adjacent segments. At edges with a discontinuous normal vector, the smooth surface description of adjacent segments can be set up independently of each other, which usually results in C0-discontinuity. Alternatively, the smooth surface description of adjacent segments can be forced to include information from the interface they have in common, which results in C0-continuity. You can force C0-continuity in 3-D also on the SPLINE option. If the SPLINE option is used for curved contact bodies defined by higher-order elements, the coordinates of the midside nodes can be recalculated based on the cubic splines defined by the position and tangent vectors of the corner nodes. This can be advantageous if the structure to be modeled is available only based on lower-order elements, so that a change from lower- to higher-order elements yields midside nodes which are not on the curved boundary, but on the straight edges between the corner nodes.

Main Index

566 Marc Volume A: Theory and User Information

C0-discontinuous Coons Surface Representation

Actual Geometry

Finite Element Approximation

C0-continuous Coons Surface Representation Figure 8-40 3D Deformable Contact; Piece wise Linear FE Description and Coons Surface Representations

Solution Strategy for Deformable Contact 1. Upon initiation, the program determines the boundary nodes on each body. For 2-D, these nodes are ordered in sequence in order to describe the boundary in a counterclockwise manner. Linear geometrical entities are then created out of subsequent pairs of nodes, to define a surface profile as in a rigid surface. If higher-order elements are used in full quadratic mode, quadratic entities are created from the three nodes. For 3-D using lower-order elements, 4-node patches are created. For 3-D higher-order hexahedral elements, a quadratic surface is created. 2. Once contact between a node and a deformable surface is detected, a tie is activated. The tying matrix is such that the contacting node follows the shape of the surface (Figures 8-41 and 8-42); it can slide along it or be stuck according to the general contact conditions. 3. Contact occurs between all deformable bodies unless the CONTACT TABLE option is used. In deformable contact, there is no master or slave body; each body is checked against every other body, except single-sided contact or the CONTACT TABLE option is used. 4. During the iteration process of finding an incremental solution, a node can slide from one segment to another, changing the retained nodes of its tie. A recalculation of the bandwidth is, therefore, made every iteration. From increment (or subincrement) to increment, the number of nodes in contact can change. In such cases, an optimization of the bandwidth is automatically available to cope with the possible drastic changes in bandwidth that a new tie produces. When the glue option is used between two deformable bodies, a simpler tying relationship is formed, such that no relative motion occurs.

Main Index

CHAPTER 8 567 Contact

C Tied Node A Retained Nodes A B C

A

segt B ΔUB

ΔUA

ΔUC

segt+Δt Figure 8-41 Tyings in Deformable Contact (2-D) using Lower-order Elements R2 R3

T/R1

t

R5

Tied Node T Retained Nodes T, R2, R3,R4,R5

R4

t+ Δt

Figure 8-42 Tying in Deformable Contact (3-D) using Lower-order Elements

Iterative Penetration Checking Except for a transient dynamic analysis with automatic time stepping where the Time Step Reduction Procedure is used, the commonly used method to prevent penetration in a contact analysis is the Iterative Penetration Checking Procedure. Using this procedure, the iteration process is done simultaneously to satisfy both the contact constraints and global equilibrium using the Newton-Raphson procedure. This procedure is accurate and stable. This procedure is automatically activated when the AUTO STEP procedure is used in static analysis or when beam-beam contact is present. In a conventional iteration process, the finite element system calculates for each iteration: K T δu i = R i – 1 where K T is the tangent stiffness matrix and R i – 1 are the residuals based on displacements from the previous iteration.

Main Index

568 Marc Volume A: Theory and User Information

Using the iterative penetration method K T is now based upon the contact status at this iteration, both from a constraint and friction perspective. Furthermore, after the solution for δu i is obtained, the contact procedure is used to determine if new penetration will occur. If, at least, one node penetrates a contact surface, a scale factor is applied to the change in displacements such that the penetrating nodes are moved back to the contact surface. This procedure can be considered a type of line search. Given that s is the fraction of δu i such that no new penetration occurs, the displacement increment then becomes ΔU i = ΔU i – 1 + sδu i and the total displacement is U n = ΔU n – 1 + ΔU i The strains, stresses, and residuals are based upon these quantities. Separation is based upon these values. When global equilibrium is achieved, based upon the user’s criteria, the solution proceeds to the next increment. Because the procedure can reduce the change in displacements, it may require more iterations to complete an increment. It is important to ensure that the maximum allowable number of iterations to complete an increment is set to a sufficiently large value.

Instabilities In some analyses, because of instabilities such as buckling or a loss of contact, large displacements increments may occur. In such cases, it is possible to specify a maximum δu i allowed in this case if: sδu i > δu a l l o we d for any node if it is scaled down. Finally, if the solution is still not able to converge and the cutback feature is activated, the time step is reduced in magnitude and the increment is repeated.

References 1. Oden, J. T. and Pires, E. B. “Nonlocal and Nonlinear Friction Laws and Variational Principles for Contact Problems in Elasticity,” J. of Applied Mechanics, V. 50, 1983. 2. Ju, J. W. and Taylor, R. L. “A perturbed Lagrangian formulation for the finite element solution of nonlinear frictional contact problems,” J. De Mechanique Theorique et Appliquee, Special issue, Supplement, 7, 1988. 3. Simo, J. C. and Laursen, T. A. “An Augmented Lagranian treatment of contact problems involving friction,” Computers and Structures, 42, 1992. 4. Peric, D. J. and Owen, D. R. J. “Computational Model for 3-D contact problems with friction based on the Penalty Method,” Int. J. of Meth. Engg., V. 35, 1992. 5. Taylor, R. L., Carpenter, N. J., and Katona, M. G. “Lagrange constraints for transient finite element surface contact,” Int. J. Num. Meth. Engg., 32, 1991. 6. Wertheimer, T. B., “Numerical Simulation Metal Sheet Forming Processes,” VDI BERICHET, Zurich, Switzerland, 1991.

Main Index

Chapter 9 Boundary Conditions

9

Main Index

Boundary Conditions

J

Loading

J

Kinematic Constraints

J

Mesh Independent Connection Methods

571 599 637

570 Marc Volume A: Theory and User Information

Marc is based on the stiffness method and deals primarily with force-displacement relations. In a linear elastic system, force and displacement are related through the constant stiffness of the system; the governing equation of such a system can be expressed as (9-1)

Ku = F

where K is the stiffness matrix and u and F are nodal displacement and nodal force vectors, respectively. Equation (9-1) can be solved either for unknown displacements subjected to prescribed forces or for unknown forces (reactions) subjected to prescribed displacements. In general, the system is subjected to mixed (prescribed displacement and force) boundary conditions, and Marc computes both the unknown displacements and reactions. Obviously, at any nodal point, the nodal forces and nodal displacements cannot be simultaneously prescribed as boundary conditions for the same degree of freedom. Note:

You must prescribe at least a minimum number of boundary conditions to insure that rigid body motion does not occur.

The prescribed force boundary conditions are often referred to as loads and the prescribed displacement boundary conditions as boundary conditions. Note:

Boundary conditions can be prescribed in either the global or a local coordinate system. A nodal transformation between the global and the local coordinate systems must be carried out if the boundary condition is prescribed in a local system.

In a nonlinear stress analysis problem, Marc carries out the analysis incrementally and expresses the governing equation in terms of the incremental displacement vector δu and the incremental force vector δF . Kδu = δf

(9-2)

Consequently, you must also define both the loads and the prescribed nodal displacements incrementally. In addition to the prescribed displacement boundary conditions, constraint relations can exist among the nodal displacements. For example, the first degree of freedom of node i is equal to that of node j at all times. The expression of this constraint relation is ui = uj

(9-3)

Generally, a homogenous linear constraint equation can be expressed as ut = a 1 u1 + a 2 u2 + … + an un

(9-4)

where u represents the degrees of freedom to be constrained, u 1, …, u n are other retained degrees of freedom in the structure, and a 1, …, a n are constants.

Main Index

CHAPTER 9 571 Boundary Conditions

You can enter constraints through either the TYING, SERVO LINK, RBE2, or RBE3 options. You can use linear/nonlinear springs and foundations to provide special support to the structure and the gap and friction element (or CONTACT option) to simulate the contact problem.

Loading Different types of analyses require different kinds of loading. For example, the loads in stress analysis are forces; those in heat transfer analysis are heat fluxes. Force is a vector quantity defined by magnitude and direction; heat flux is a scalar quantity defined by magnitude only. Loading can be time invariant (constant value) or time dependent.

Loading Types You can categorize a particular type of load as either a point (concentrated) load or surface/volumetric (distributed) load, depending on application conditions. The spatial distribution of the load can be uniform or nonuniform. Special loading types also exist in various analyses. For example, centrifugal loading exists in stress analysis, and convection and radiation exist in heat transfer analysis. You can add point loads directly to the nodal force vector, but equivalent nodal forces first must be calculated by Marc from distributed loads and then added to the nodal force vector. These distinguishing features are described below. A point (or nodal) load of either a vector (force, moment) or a scalar (heat flux) quantity is a concentrated load that is applied directly to a nodal point (see Figure 9-1). Mechanical point loads can be defined as fixed direction forces or as follower forces. In a global or local coordinate system, a force vector must be defined in terms of its vector components (see Figure 9-2). If the force vector is defined in a local coordinate system, then a global-to-local coordinate transformation matrix must be defined for the nodal point (see Figure 9-3 and Figure 9-4). For axisymmetric elements, the magnitude of the point load must correspond to the ring load integrated around the circumferences. F

Q y

y

x Point (a) Heat Flux Q (Scalar) Figure 9-1

Main Index

x Point (b) Force F (Vector)

Schematic of a Point Load

572 Marc Volume A: Theory and User Information

y’ F

Fy

Fx

y

Fx’

y

x’

x

x

Figure 9-2

F

Fy’

Force Components y”

x” Fy” = 0

y

x Figure 9-3

F = Fx”

Special Selection of Local (x”, y”) Coordinate System Force Components: F

y'' = 0

Surface/volumetric loads, such as pressure, distributed heat flux, and body force, are distributed loads that are applied to the surface (volume) of various elements (see Figure 9-4). A surface/volumetric load is characterized by the distribution (uniform/nonuniform) and the magnitude of the load, as well as the surface to which the load is applied (surface/volume identification). The total load applied to the surface (volume) is, therefore, dependent on the area (interior) of the surface (volume). Equivalent nodal forces first must be calculated from surface/volumetric loads and then added to the nodal force vector. Marc carries out this computation through numerical integration. (See Marc Volume B: Element Library for the numbers and locations of these integration points for different elements). The calculated equivalent nodal forces for lower-order elements are the same as those obtained by equally lumping the uniformly distributed loads onto the nodes. However, for high-order elements, the lumping is no longer simple (see Figure 9-5). As a result, the surface/volumetric loads should not be lumped arbitrarily.

Main Index

CHAPTER 9 573 Boundary Conditions

P1

P1

P2 4

3

P2 4

3

Px

1

y

Q

Py

2

1

y

P

x (a) Distributed Mechanical Load

2 q

x (b) Distributed Heat Flux

Surface 2-3: Uniform Normal Pressure p

Uniform Heat flux q

Surface 3-4: Nonuniform Normal Pressure p1 - p2

Nonuniform Heat flux q1 = q2

Whole Volume: Volumetric Loads Px’Py

Volumetric Heat Flux Q

Figure 9-4

Schematic of Surface/Volumetric Load

1/2 1/4

1/2

1/4

1/4 1/4 1/4 1/4

1/4 -1/12

1/4 1/3

1/3

-1/12

1/6

2/3

1/6 1/3 -1/12

-1/12 1/3 -1/12

1/3

1/3 -1/12

1/3

Figure 9-5

-1/12

-1/12

1/3

Allocation of a Uniform Body Force to Nodes for a Rectangular Element Family

Using the table driven input format, boundary conditions may be applied to finite element entities, nodes, elements, edges or faces, or geometric entities such as points, curves, and surfaces. The latter is advantageous because it improves compatibility with CAD and because it facilitates adaptive meshing. The application of boundary conditions on geometric entities is only effective if finite elements have been associated with these geometric entities using the ATTACH NODE, ATTACH EDGE, and

Main Index

574 Marc Volume A: Theory and User Information

ATTACH FACE model definition options. As shown in Figure 9-6, Marc Mentat shows a 2-D model

consisting of four curves around the perimeter and a curve where the circle is. The mesh was created using the automatic mesh generator which automatically attaches the edges to the curves. Those nodes which are attached to points are shown using the circle symbol as opposed to the square symbol. Now, if a boundary condition, such as an internal pressure, is applied on a curve during the analysis, it will automatically be applied to those edges attached to the curve as shown in Figures 9-8 and 9-9. In a similar manner, if a displacement is applied to a point, then it will be applied to the node. For 3-D, the analogous situation exists; namely, a distributed load applied to a surface will be applied to those elements attached to this face as shown in Figure 9-10. And nodal boundary conditions will be attached to nodes attached to face.

Main Index

Figure 9-6

Geometric Representation with Five Curves

Figure 9-7

Original Mesh, Red Edges Indicate that they are Attached to Curve

CHAPTER 9 575 Boundary Conditions

Main Index

Figure 9-8

Boundary Conditions Applied to Curves

Figure 9-9

Boundary Conditions Applied to Attached Element Edges

576 Marc Volume A: Theory and User Information

Figure 9-10 Distributed Load Applied to Surfaces. In Marc Mentat, Faces Attached to Surfaces are Indicated by a Darker Color (usually Blue and Midnight Blue)

Now, if global or local adaptive meshing is used, then, as shown in Figures 9-11 and 9-12, the load automatically is applied to the new element edges which are attached to the curve. If a point load of prescribed displacement is applied to a geometric point, the mesh generator will make sure that a point/node is in this exact location after remeshing occurs. This allows all boundary conditions to be used in conjunction with global or local adaptive meshing in 2-D. In 3-D, one can apply boundary conditions to geometric entities as well, but they are not updated with global adaptive meshing in this release. For the case of shells, this is complicated because, for certain types of load, there is a difference between application to the top and bottom surfaces. In mechanical analysis, a positive pressure on the top surface is equivalent to a negative pressure applied to the bottom surface. This is because the degrees of freedom of a mechanical shell are considered to be at the neutral surface. For thermal analysis, distributed fluxes, convective boundary conditions and radiation, there is a difference between application of thermal boundary conditions on the top or bottom surfaces. This is particularly relevant for radiation, as the choice of surfaces will strongly influence the viewfactor calculation. Figure 9-13, shows a surface, with the top (yellow) and bottom (blue) surfaces identified. To select either the top or bottom surface, use the FILTER command. A boundary condition applied to the “top” and “bottom” surface is shown in Figures 9-14 and 9-15, respectively. If the shell mesh is automatically generated from the surface, the top face of the element is associated with the top surface of the shell. It is also possible to display the shell elements to indicate the thickness as shown in Figure 9-16, in which case, one can easily select the top or bottom faces for which the boundary condition is to be applied.

Main Index

CHAPTER 9 577 Boundary Conditions

Figure 9-11 Distributed Load on Top Surface after Global Adaptive Remeshing

Figure 9-12 Distributed Load to Top Surface after Local Adaptive Remeshing

Figure 9-13 Identification of Top and Bottom Surface of a Shell

Main Index

578 Marc Volume A: Theory and User Information

Figure 9-14 Boundary Condition on Top Surface

Figure 9-15 Boundary Condition on Bottom Surface

Figure 9-16 Shell Elements shown in Expanded Mode

Figure 9-17 is an example of what can go wrong if either geometric entities or elements are not consistently defined. Two curves are used to represent an axisymmetric shell, but as shown by the orientation vector, they are not continuous in direction.

Main Index

CHAPTER 9 579 Boundary Conditions

Figure 9-17 Oriented Curves

Figure 9-18 shows the finite element mesh obtained from the convert option, which does not indicate any potential problem. If one displays the shell in expanded mode and identifies backfaces, then one will see an inconsistency between the top (blue) and the bottom (brown) surfaces as shown in Figure 9-19.

Figure 9-18 Finite Element Mesh

Figure 9-20 shows the boundary condition applied to the “top” curve, which is not what is desired. To get a consistent applied boundary condition, one needs to flip both the curves and elements of one of the sections.

Figure 9-19 Shell Elements Expanded showing Top (Blue) and Bottom (Brown) Surfaces

Main Index

580 Marc Volume A: Theory and User Information

Figure 9-20 Incorrect Boundary Condition on Top Surface

Face ID for Distributed Loads, Fluxes, Charge, Current, Source, Films, and Foundations When using the table driven input procedure, there are three ways to identify the type of load and which edge or face it is applied to. In the first method. an IBODY, as defined for each element type defined in Marc Volume B: Element Library, is associated with each distributed load list. This IBODY effectively defines the type (normal pressure, shear, gravity, pressure, centrifugal, Coriolis) and the edge or face to which the load is applied. For the second method, one needs to enter the type of load and the location separately, but the location of the load is consistent for all element types of the same class. This is called the face ID and is shown in the following figures. It should be noted that when input files are created using Marc Mentat, the convention is to use the same ID as used in the Marc convention minus 1. 1-D 2-Node Elements y

FACE ID

NODES

1

1–2

2 1

x

1-D 3-Node Elements 3 2 1

Main Index

FACE ID

NODES

1

1–2–3

CHAPTER 9 581 Boundary Conditions

2-D 4-Node Quadrilateral Elements 4

3

1

FACE ID

NODES

1 2 3 4

1–2 2–3 3–4 4–1

2

Load shown on FACE ID 1

2-D 8-Node Quadrilateral Elements 4

7

3

8

6

1

FACE ID

NODES

1 2 3 4

1–5–2 2–6–3 3–7–4 4–8–1

FACE ID

NODES

1 2 3

1–2 2–3 3–1

FACE ID

NODES

1 2 3

1–4–2 2–5–3 3–6–1

2

5

2-D 3-Node Triangle 3

1

2

2-D 6-Node Triangle 3

6

1

Main Index

5

4

2

582 Marc Volume A: Theory and User Information

3-D 3-Node Shell z

3

FACE ID

NODES

1 2

1–2–3 1–3–2

(top) (bottom)

1 y x

2

3-D 4-Node Shell/Membrane 4

FACE ID 1

P

2

3

NODES 1–2–3–4 1–4–3–2

(top) (bottom)

1 2

3-D 6-Node Shell 3

P

6

FACE ID

NODES

1 2

1–2–3–4–5–6 1–3–2–6–5–4

5

1

4

(top) (bottom)

2

3-D 8-Node Shell 4

7

3

8

FACE ID

NODES

1 2

1–2–3–4–5–6–7–8 1–4–3–2–8–7–6–5

6

1

5

2

3-D 4-Node Tetrahedral 4 3

1 2

Main Index

FACE ID

NODES

1 2 3 4

1–2–4 2–3–4 3–1–4 1–2–3

(top) (bottom)

CHAPTER 9 583 Boundary Conditions

3-D 6-Node Pentahedral 6 4 5

FACE ID

NODES

1 2 3 4 5

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

3 1 2

3-D 15-Node Pentahedral 3 15 6

8

9

FACE ID

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

5

10

4

3-D 8-Node Brick 8 7

5 6 4 1

3 2

Main Index

FACE ID

NODES

1 2 3 4 5 6

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

584 Marc Volume A: Theory and User Information

3-D 10-Node Tetrahedral 4

10

8

3

9 7 6

FACE ID

NODES

1 2 3 4

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

1 5 2

3-D 20-Node Brick 8 16

15 7

5

20

13

14

6 17

19

4

12

11

FACE ID

NODES

1 2 3 4 5 6

1 – 2 – 6 – 5 – 9 – 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 – 9 – 10 – 11 – 12 6 – 5 – 8 – 7 – 13 – 16 – 15 – 14

18 1

3 9

10 2

For the third method, the element edges or faces are attached to a curve or surface, respectively. In this case, one only needs to give the type of load as the location is inferred from the ATTACH EDGE and ATTACH FACE data.

Mechanical Loads Marc allows you to enter mechanical loads in various forms for stress analysis. These loads can be concentrated forces and moments, uniformly and nonuniformly distributed pressures, body forces, gravity or centrifugal loads. Table 9-1 lists input options for mechanical loads.

Main Index

CHAPTER 9 585 Boundary Conditions

Table 9-1

Input Options for Mechanical Loads

Input Options Load Description

Model Definition

History Definition

User Subroutine

Point Load: Concentrated Force/Moment

POINT LOAD

POINT LOAD

FORCDT

Surface Load Pressure Shearing Forces, and Distributed Moment (Uniform/Nonuniform Distribution)

DIST LOADS

DIST LOADS

FORCEM

Volumetric Load Body DIST LOADS Forces and Acceleration Forces

DIST LOADS

FORCEM

Centrifugal Loading

DIST LOADS ROTATION A

DIST LOADS

Coriolis Loading

DIST LOADS ROTATION A

DIST LOADS

Fluid Loading

DIST LOADS FLUID DRAG

Application of centrifugal and Coriolis loadings require the ROTATION A model definition option, which defines the data corresponding to the axis of rotation. If multiple parts are rotating, then different rotation axes may be defined. The actual load can be invoked by specifying an IBODY load types 100, 103,104, or 105 for centrifugal and Coriolis loadings, respectively. For load types 100 or 103, the square 2

of rotation speed, ω , is entered in radians per time, for the magnitude of the distributed load. For load types 104 or 105, the angular velocity is entered as cycles per time. The mass density must also be defined in the ISOTROPIC, ORTHOTROPIC, or other material options. Application of gravity load (load per unit mass) is achieved by using IBODY load type 102. The mass density must be defined in the ISOTROPIC, ORTHOTROPIC, or other material options. The acceleration can be given independently in the x, y, and z direction through the DIST LOADS option. Volumetric loads (load per unit volume) may be entered by using IBODY type 106 or 107. The FOLLOW FOR parameter is used when the direction of Distributed and/or Point Loads are not fixed and need to follow the geometry. FOLLOW FOR automatically invokes the LOAD COR parameter, so stresses should be stored at all integration points. Separate flags under this parameter are used to control follower forces for distributed loads and point loads respectively. When the FOLLOW FOR parameter is flagged for distributed loads, equivalent nodal loads due to pressures are calculated based on the current geometry. Any change of surface area or orientation results in a change of load. You can also specify that

Main Index

586 Marc Volume A: Theory and User Information

the follower force stiffness matrix due to distributed loads can be included. The FOLLOW FOR parameter for distributed loads is typically used when a shell structure, which can undergo large deformation and rotations, is subjected to a pressure load. A separate flag on the FOLLOW FOR parameter allows follower forces to be specified for point loads. When this parameter option is flagged, the user still has the choice of specifying individual point loads as fixed direction load vectors or as follower forces. Fixed direction load vectors are specified by the usual vector components. When defined as a follower force, there are two techniques available for specifying the load: • The first technique is similar to the option available in Nastran. The scalar magnitudes of the load and/or moment are specified instead of the vector components. The direction of the force is then specified through 2 or 4 independent nodes in a manner similar to the FORCE1/MOMENT1 or FORCE2/MOMENT2 options in Nastran. In the former, two nodes A and B are to be specified by the user and the direction of the load follows the vector directed from node A to node B, as shown in Figure 9-21(a). In the latter, four nodes A, B and C, D are specified by the user. The direction of the load follows the cross product of the vector directed from node A to node B and the vector directed from node C to node D, as shown in Figure 9-21(b).

P (Load Magnitude) P (Load Magnitude)

A Load Direction

Load Direction B

(a) FORCE1 Style

D

A,C

B (b) FORCE2 Style

Figure 9-21 Nastran Style Follower Force Definition for Point Load

• The second technique offers an automated way of defining the follower force. The load/moment is specified through vector components as usual. The initial orientation of the load with respect to an optimal mesh location is noted. Then, as the structure deforms, the load direction is updated such that the relative orientation of the load with respect to the mesh is maintained, as shown in Figure 9-22. Optimal nodes in the mesh are automatically chosen for calculating and maintaining the relative orientation. One or two optimal nodes can be used. The optimal nodes are chosen based on the following criteria: The nodes should belong to the same element as the loaded node. If the initial vector from the loaded node to any node matches the initial load direction, then that node is chosen as the optimal node. Else, the closest node to the loaded node is chosen. For 3-D shells and solids, two optimal nodes are chosen if the cross product of the vectors of the loaded node to these two nodes matches the load direction.

Main Index

CHAPTER 9 587 Boundary Conditions

Initial Load Direction α α

Optimal Node

Updated Load Direction

Figure 9-22 Geometry Based Automated Follower Force Definition for Point Load

The second technique is quite convenient and can be generally applied to 2-D and 3-D beams, shells and solids. In situations where the loaded node does not belong to an element (for example, load controlled rigid dies, etc.), the first technique should be used. It should be noted that a follower force stiffness matrix is not currently available for the point loads. Also, the follower force capability is not supported for a point load specified through the FORCDT user subroutine. A number of history definition options are available for input of multiple load increments. For example, the AUTO LOAD option generates a specified number of increments, all having the same load increment, and is useful for nonlinear analysis with proportional loads; the PROPORTIONAL INCREMENT option allows the previous load increment to be scaled up or down for use in the current load increment. The AUTO INCREMENT option allows automatic load stepping in a quasi-static analysis and is useful for both geometrically and materially nonlinear problems.

Fluid Drag and Wave Loads Marc provides a fluid drag and wave load capabilities that can be applied on beam type structures that are partially or fully submerged in fluid (see Figure 9-23). Morison’s equation is used to evaluate the fluid drag loads that are associated with steady currents. Only distributed drag and buoyancy effects are considered. Marc employs Airy wave theory to evaluate wave velocities that can be invoked for dynamic analysis option. Fluid drag and wave loads are invoked using the DIST LOADS model definition with an IBODY load type of 11. These loads also require the FLUID DRAG model definition to input the relevant information regarding the fluid elevation and its flow. Table 9-2 lists input options for fluid drag and wave loads. Table 9-2

Input Options for Fluid Drag and Wave Loads

Input Options Load Description

Main Index

Model Definition

History Definition

Fluid Drag Load

DIST LOADS FLUID DRAG

DIST LOADS

Wave Load

DIST LOADS FLUID DRAG

DIST LOADS

User Subroutine

588 Marc Volume A: Theory and User Information

Steady Velocity

Wave Load

Pipe

Flow Velocity Distribution Buoyancy Force Velocity Gradient

Outside Fluid Fluid Drag Force Inside Fluid

Sea Bed Figure 9-23 Fluid Drag and Wave Loads

Cavity Pressure Loading Marc allows the modeling of structures enclosing cavities by updating the cavity internal pressure as the cavity volume change. For ideal gas-filled cavities, the equation of state relating the cavity pressure and volume can be written as: pV = nR o T

(9-5)

where p is the cavity total pressure, V is the cavity volume, n is the number of molecules of the gas, R o is the Universal Gas Constant ( R o = 8.31447 J/(mol°K) = 1545.35 ft.lbf/(mol°R) ), and T is the absolute gas temperature. The gas mass, M , is related to the number of molecules of the gas by: μ = M⁄n

(9-6)

where μ is the molar mass of the gas. Substituting by n from Equation (9-6) into Equation (9-5) gives: pV = MRT

(9-7)

where R = R 0 ⁄ μ is the Specific Gas Constant. With the gas density, ρ , defined as: ρ = M⁄V

Main Index

(9-8)

CHAPTER 9 589 Boundary Conditions

the equation of state of an ideal gas can be finally written as: p = ρRT

(9-9)

The Specific Gas Constant is calculated from: R = pr ⁄ ρr Tr

(9-10)

where p r is the gas reference pressure, T r is the gas reference temperature, and ρ r is the gas reference density. The user must ensure that the values entered for the gas reference pressure, temperature and density are consistent. The cavity total pressure is given by: p = pa + pg

(9-11)

where p a is the ambient pressure and p g is the cavity gage pressure. Only the cavity gage pressure is applied to the structure forming the cavity. The following loading scenarios are available for cavities: Closed Cavity If the cavity is closed, the mass of the gas is preserved M = Mo

(9-12)

where M o is the cavity mass from the previous increment. The gas is assumed to undergo a general polytropic process represented by: pV

γ

= constant

(9-13)

where γ is the polytropic exponent. The gas pressure can thus be updated using Vo γ p ----- = ⎛⎝ -------⎞⎠ po V

(9-14)

where p o and V o are the cavity pressure and volume from the previous increment, respectively. Using Equation (9-7) and Equation (9-14), the gas temperature can be updated using Vo γ – 1 T ------ = ⎛⎝ -------⎞⎠ To V

(9-15)

where T o is the cavity temperature from the previous increment. The gas density is calculated from: ρ = M⁄V Closed cavity processes can be set to occur: • at constant pressure, isobaric, using γ = 0 .

Main Index

(9-16)

590 Marc Volume A: Theory and User Information

• at constant temperature, isothermal, using γ = 1 . • with no heat transfer to the surroundings, adiabatic, using γ = k , where k is the adiabatic exponent. For ideal gases, k is a constant that depends only on the number of atoms in the gas molecule (monoatomic gases: k = 1.67 , diatomic gases: k = 1.4 , triatomic gases: k = 1.33 ). Applied Pressure In this case the new cavity pressure is updated using p = p o + Δp

(9-17)

The gas temperature is assumed to be constant T = To

(9-18)

The gas density is updated using ρ = p ⁄ RT

(9-19)

and the gas mass is recalculated as M = ρV

(9-20)

Applied Mass In this case, the new cavity mass is updated using M = M o + ΔM

(9-21)

If ΔM ≠ 0 , gas is pumped in or out of the cavity. The gas density is first updated as ρ = M⁄V

(9-22)

the gas temperature is assumed to be constant T = To

(9-23)

and the cavity pressure is calculated as p = ρRT

(9-24)

If ΔM = 0 , the cavity is assumed to be closed and Equations 9-12 to 9-16 apply with γ = 1 . User Defined Loading The UCAV user routine allows the user to define and control the cavity pressure for loading scenarios other than the ones specified above.

Main Index

CHAPTER 9 591 Boundary Conditions

Cavity Modeling The CAVITY parameter is used to enter the number of cavities in the model (maximum 1000), an upper bound to the number of segments in each cavity and an upper bound to the number of nodes per segment of cavity boundary. The CAVITY model definition option is used to enter the ambient pressure, the polytropic process exponent, and the reference pressure, temperature and density for each cavity. The applied pressure or mass is entered through the DIST LOADS model definition and history definition options. The distributed load type, entered on the DIST LOADS option of the elements forming the cavity, is modified for cavity loading according to the following relation ibody_cavity = icavity * 10000 + icavity_type * 1000 + ibody

(9-25)

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: 1: 2: 9:

ibody

cavity is closed. cavity is loaded with an applied pressure. cavity is loaded with an applied mass. cavity load is defined by the UCAV user subroutine

is the original value for the distributed load type (see library element description in Marc Volume B: Element Library.)

In the first increment of the analysis, increment zero, the cavity temperature is calculated by averaging the temperatures of the elements forming the cavity. If there are no nodal temperatures defined, the cavity temperature is taken equal to the cavity reference temperature. For AXITO3D (or PRE STATE) analysis, the cavity pressure, mass, and temperature for increment zero are read from the post file of the corresponding axisymmetric problem. If the cavity is closed in increment zero, the cavity is assumed to be initially at ambient conditions. In this case, the initial gage pressure is equal to zero and the initial mass is based on the ambient pressure and initial volume. Moreover, if the ambient pressure is equal to zero, the cavity is assumed to be initially unloaded. Tables 9-3 and 9-4 summarize the cavity functioning for the different cavity load types and incremental load values during the initial and subsequent load increments, respectively. Table 9-3

Cavity Functioning for Increment Zero

Cavity Load Type Incremental Load Value Function 0 Ignored Cavity is initially at ambient conditions 1 Cavity is initially empty Δp = 0.0

Main Index

1

Δp ≠ 0.0

Cavity is initially at the applied pressure

2

ΔM = 0.0

Cavity is initially empty

2 9

ΔM ≠ 0.0 Passed to UCAV

Cavity initially contains the applied mass Call UCAV

592 Marc Volume A: Theory and User Information

Table 9-4

Cavity Functioning for Subsequent Increments

Cavity Load Type

Incremental Load Value

Function

0

Ignored

Cavity is closed, constant mass, polytropic process

1

Δp = 0.0

Cavity is open, constant pressure and temperature

1

Δp ≠ 0.0

Cavity is open, pressure is applied, constant temperature

2

ΔM = 0.0

Cavity is closed, constant mass, isothermal process

2

ΔM ≠ 0.0

Cavity is open, mass is applied, constant temperature

9

Passed to UCAV

Call UCAV

In general, standard structural elements are used to define the boundaries of cavities and no extra elements are required. However, to model the boundaries of cavities in regions where standard finite elements are not present (for example, along rigid boundaries) cavity surface elements (elements 171174) can be used. These elements can also be glued to moving rigid surfaces. They are for volume calculation purposes only and do not contribute to the stiffness equations of the model. For 2-D problems, the volume of the cavity is calculated as the sum of the areas of all the triangles formed by the cavity segments as bases and the coordinate system origin as the apex multiplied by the cavity thickness. Elements forming the cavity are assumed to be of equal thickness. For 3-D problems, the volume of the cavity is calculated as the sum of the volumes of all the tetrahedrons formed by the cavity patches as bases and the coordinate system origin as the apex. For axisymmetric problems, the volume of the cavity is calculated as the sum of the volumes of all the cone frustums formed by the cavity segment as the cone slant height and two parallel base circles and with an axis along the axis of symmetry of the problem. In the axisymmetric case, it is not necessary to use cavity surface elements along lines that are perpendicular to the axis of symmetry to close cavities. In coupled thermo-mechanical analysis, heat transfer between the gas inside the cavity and the surrounding structure is not supported. Cavities are not allowed to split or to join due to deformation or self-contact. If self-contact occurs within a cavity, the resulting cavities are still treated as a single cavity. If the cavity is formed out of membrane and/or shell elements, the user must ensure that all elements defining the cavity are aligned; that is, the cavity surface is defined by either all top or all bottom element faces.

Main Index

CHAPTER 9 593 Boundary Conditions

Cyclic Loading Application of cyclic loading is important when investigating fatigue issues in a structure. There are two ways of easily doing this in Marc. In the first method, one associates a table that is time dependent with each boundary condition. This table can be either a sawtooth function or a sinusoidal function. The boundary condition will be repeated for as long as one has a time period assigned. note that the AUTO STEP option can either exactly reach the peaks or not be constrained to reach the peaks. The alternative is to use the BEGIN SEQUENCE and END SEQUENCE options. All history definition options placed between these two options will be repeated as often as requested. One should make sure that the value of the boundary conditions at the beginning of the sequence is the same as the value at the end of the sequence. Multiple loadcases may be repeated.

Thermal Loads Element integration point temperatures are used in a thermal stress analysis to generate thermal load. The AUTO THERM history definition option allows automatic application of temperature increments based on a set of temperatures defined throughout the mesh as a function of time. The CHANGE STATE option presents the temperatures to Marc which then creates its own set of temperature steps based on a temperature change tolerance provided through this option. Table 9-5 lists input options for thermal loads. You can input either the incremental temperature or the total temperatures as thermal loads. Table 9-5

Input Options for Thermal Loads

Input Options Load Description

Parameter

Model Definition

History Definition

User Subroutine

Incremental Temperatures*

THERMAL

THERMAL LOADS** THERMAL LOADS** CREDE

Total Temperatures*

THERMAL

CHANGE STATE

Initial Temperature*

INITIAL STATE

Total Nodal Temperatures

POINT TEMP

Initial Nodal Temperature

INITIAL TEMP

CHANGE STATE

NEWSV

INITSV POINT TEMP USINC

* Temperatures must be specified at each integration point (or at the centroid if the CENTROID parameter is used) of each element in the mesh. ** The THERMAL LOADS option and CREDE user subroutine should not be used with the table driven input procedure.

The thermal strain increment is defined as Δε

Main Index

th

=

∫ αΔT

(9-26)

594 Marc Volume A: Theory and User Information

th

where Δε is thermal strain increment, α is the coefficient of thermal expansion, and ΔT is the temperature increment. Equivalent nodal forces are calculated from the thermal strain increment and then added to the nodal force vector for the solution of the problem. You can input the coefficient of thermal expansion through the ISOTROPIC, ORTHOTROPIC, or other material options and the temperature increment through various options.

Initial Stress and Initial Plastic Strain Marc allows you to enter a set of initial stresses that simulate the stress state in the structure at the beginning of an analysis. A typical example is prestress in a tensioned fabric roof. The set of initial stresses must be self-equilibrating and should not exceed the yield stress of the material. Table 9-6 shows the input options for initial stress. Table 9-6

Input Options for Initial Stress and Initial Plastic Strain

Input Options Load Description Initial Stress Prestress Initial Plastic Strain

Main Index

Parameter ISTRESS

Model Definition

User Subroutine

INIT STRESS

UINSTR

INITIAL PLASTIC STRAIN

INITPL

CHAPTER 9 595 Boundary Conditions

9

Marc also provides various ways of initializing the equivalent plastic strain throughout the model. This is useful in metal forming analysis in which the previous amount of equivalent plastic strain is often required. 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. The input option is shown in Table 9-6.

Boundar y Conditio ns

Heat Fluxes In a heat transfer analysis, you can enter heat fluxes in various forms. Heat transfer analysis requires entering the total values of flux. Table 9-7 lists the input options for heat fluxes. Table 9-7

Input Options for Heat Fluxes

Input Options Load Description

Model Definition

History Definition

User Subroutine

Point Heat Flux (Sink or Source)

POINT FLUX

POINT FLUX

FORCDT

Surface Heat Flux, Convection, Radiation

DIST FLUXES QVECT FILMS SURFACE ENERGY

DIST FLUXES QVECT FILMS

FLUX* UQVECT FILM*

Volumetric Flux Load Body Flux

DIST FLUXES

DIST FLUXES FILMS

FLUX*

* Can be used for complicated flux loadings, convection, and radiation, allowing the input of nonuniform temperature- and time-dependent boundary conditions.

There are three special heat flux conditions representing insulation, convection, and radiation as discussed in Chapter 6: Nonstructural and Coupled Procedure Library in the Boundary Conditions section. 1. Insulation q = 0

(9-27)

No input is required for the insulated case. 2. Convection Nondirected: q = H ( Ts – T )

(9-28)

You must enter the film coefficient H and ambient temperature T through the FILMS model definition option or the FILM user subroutine. You can also directly input the heat flux q using the FLUX user subroutine.

Main Index

596 Marc Volume A: Theory and User Information

Directed q = –q0 ⋅ α ⋅ n ⋅ ns (9-29) ˜ where n is the orientation defined in the QVECT option and n s is the outward unit normal. ˜ 3. Radiation 4

4

q = σ ⋅ ε ( Ts – T∞ )

(9-30)

You must enter either the heat flux q using the FLUX user subroutine or the temperature dependent film coefficient H ( T s, T, σ, ε ) and ambient temperature T using the FILM user subroutine. These relationships are shown in Equation (9-31). Using the table driven input format, you can directly specify radiation to the environment through the FILMS model definition option. The use of the FILM user subroutine is recommended to ensure a stable solution. 4

4

q = σε ( T s – T ∞ ) 3

2

2

(9-31)

3

= σ ⋅ ε ( Ts + Ts T∞ + Ts T∞ + T∞ ) ( Ts – T∞ ) = H ( T s, T ∞ ) ( T s – T ∞ )

where σ is the Stefan-Boltzmann constant, ε is emissivity, T s and T ∞ are unknown surface and ambient temperatures, respectively. As an alternative for radiation between surfaces, Marc will calculate the viewfactors using the CAVITY DEFINITION and RAD-CAVITY model definition options or the VIEW FACTOR model definition option can be used to read in viewfactors calculated by Marc Mentat. The RADIATION parameter is also required.

Mass Fluxes and Restrictors In a hydrodynamic bearing analysis, you can enter mass fluxes, restrictors, and pump pressures as loads. Table 9-8 lists input options for these quantities. Table 9-8

Input Options for Mass Fluxes and Restrictors

Input Options Load Description

Parameter

Model Definition

History Definition

Nodal Mass Fluxes

BEARING

POINT MASS

POINT MASS

FORCDT

Distributed Mass Fluxes

BEARING

DIST MASS

DIST MASS

FLUX*

Restrictors

BEARING RESTRICTOR

RESTRICTOR

* Can be used for nonuniform mass fluxes ** Can be used for nonuniform restrictions or pump pressures.

Main Index

User Subroutine

URESTR**

CHAPTER 9 597 Boundary Conditions

Electrical Currents In coupled thermo-electrical (Joule heating) analysis and coupled electrical-thermal-mechanical analysis (Joule-mechanical), you can prescribe electrical currents as loads for the calculation of unknown nodal voltages. In magnetostatic analysis, you can also define the current. In such cases, as a steady state analysis is performed, there is no time variation of the currents. Table 9-9 lists input options for electrical currents. Table 9-9

Input Options for Electrical Currents

Input Options Load Description

Model Definition

History Definition

User Subroutine

Nodal Current

POINT CURRENT

POINT CURRENT

FORCDT

Surface and Body Currents

DIST CURRENT

DIST CURRENT

FLUX

Electrostatic Charges In an electrostatic analysis, the charge can be entered, noting that a steady state analysis is performed so there is no time variation of charge. In a coupled electrostatic structural analysis there can be a variation of charge in time, but this variation is considered to be quasi-static. Table 9-10 summarized the input options. Table 9-10

Input Options for Electrostatic Charge

Input Options Load Description

Model Definition History Definition User Subroutine

Nodal Charge

POINT CHARGE

POINT CHARGE

FORCDT

Distributed and Body Charges

DIST CHARGES

DIST CHARGE

FLUX

Acoustic Sources In acoustic analysis, you can enter a source pressure if a transient analysis by modal superposition is being performed. Table 9-11 summarized the input options. Table 9-11

Input Options for Acoustic Sources

Input Options Load Description

Main Index

Model Definition

History Definition

User Subroutine

Nodal Source

POINT SOURCE

POINT SOURCE

FORCDT

Distributed Source

DIST SOURCES

DIST SOURCES

FLUX

Nodal Source

FIXED PRESSURE

PRESS CHANGE

FORCDT

598 Marc Volume A: Theory and User Information

Piezoelectric Loads In a piezoelectric analysis, both mechanical loads and electrostatic charges can be entered. These values can have time variation if a transient analysis is performed or a harmonic excitation can be applied. Table 9-1 gives a summery of the mechanical input options, and Table 9-10 gives a summary of the electrostatic input options.

Electrostatic-Structural Loads In a coupled electrostatic-structural analysis, both mechanical loads and electrostatic charges can be entered. Table 9-1 gives a summery of the mechanical input options, and Table 9-10 gives a summary of the electrostatic input options.

Magnetostatic Currents In a magnetostatic analysis, the current can be entered, noting that a steady state analysis is performed so there is no time variation of current. Table 9-12 summarizes the input options. Table 9-12

Input Options for Magnetostatic Current

Input Options Load Description

Model Definition

History Definition

User Subroutine

Nodal Current

POINT CURRENT

POINT CURRENT

FORCDT

Distributed and Body Current 2-D

DIST CURRENT

DIST CURRENT

FLUX

Distributed and Body Current 3-D

DIST CURRENT

DIST CURRENT

FORCEM

Electromagnetic Currents and Charges In an electromagnetic analysis, the current can be entered. These values can have time variation if a transient analysis is performed or a harmonic excitation can be applied. Table 9-13 summarizes the input options. Table 9-13

Input Options for Currents and Charges

Input Options Load Description

Main Index

Model Definition

History Definition

User Subroutine

Nodal Current

POINT CURRENT

POINT CURRENT

FORCDT

Distributed and Body Current

DIST CURRENT

DIST CURRENT

FLUX

Nodal Charge

POINT CURRENT POINT CHARGE

POINT CURRENT

FORCDT

Distributed and Body Charge

DIST CHARGE

DIST CHARGE

CHAPTER 9 599 Boundary Conditions

Kinematic Constraints Marc allows you to input kinematic constraints through various options that include • • • • • • • • • • • • • •

Boundary Conditions (prescribed nodal values) Transformation of Degree of Freedom Shell Transformation Tying Constraint Rigid Link Constraint Shell-to-Solid Tying Insert AUTOMSET Support Conditions Bushings Cyclic Symmetry Nastran RBE2 and RBE3 Beam - Shell Offsets Pin Code for Beam Elements

Boundary Conditions Marc allows you to specify the nodal value for a particular degree of freedom. If you do not give a nodal value when you specify the boundary condition, Marc sets the fixed nodal value to zero. An option allows boundary conditions to be specified at the time of two-dimensional mesh generation with MESH2D. You can apply a different set of boundary conditions for each load increment. Table 9-14 gives the nodal values for the various analyses, and Table 9-15 lists the input options for boundary conditions in different analyses. Table 9-14

Analyses with Corresponding Nodal Values

Analysis

Main Index

Nodal Values

Acoustics

Pressure

Coupled Fluid Thermal

Velocity, Pressure, and Temperature

Coupled Thermo-electrical

Voltage and Temperature

Coupled Thermo-mechanical

Displacement and Temperature

Coupled Electrical-thermo-mechanical

Voltage, Temperature, and Displacement

Electrostatic

Potential

Piezoelectric

Displacement and Potential

Fluid

Velocity and Pressure

Heat transfer

Temperature

600 Marc Volume A: Theory and User Information

Table 9-14

Analyses with Corresponding Nodal Values (continued)

Analysis

Nodal Values

Hydrodynamic Bearing

Pressure

Magnetostatic

Potential

Rigid Plastic Flow

Velocity

Stress

Displacements

Table 9-15

Input Options for Boundary Conditions

Input Options Load Description

Model Definition

History Definition

User Subroutine

Displacement

FIXED DISP

DISP CHANGE

FORCDT

Temperature

FIXED TEMPERATURE

TEMP CHANGE

FORCDT

Voltage

FIXED VOLTAGE

VOLTAGE CHANGE

FORCDT

Pressure

FIXED PRESSURE

PRESS CHANGE

FORCDT

Potential (Electrostatic)

FIXED EL-POT FIXED POTENTIAL

Potential (Magnetostatics)

FIXED MG-POT FIXED POTENTIAL

Velocity

FIXED VELOCITY

FORCDT

VELOCITY CHANGE

FORCDT

Transformation of Degree of Freedom Marc allows transformation of individual nodal degrees of freedom from the global direction to a local direction through an orthogonal transformation that facilitates the application of boundary conditions and the tying together of shell and solid elements. Transformations are assumed to be orthogonal. Once you invoke a transformation on a node, you must input all loads and kinematic conditions for the node in the transformed system.Nodal output is in the transformed system. This option is invoked using the TRANSFORMATION option. The UTRANFORM option allows transformations to be entered via the UTRANS user subroutine. This allows you to transform the degrees of freedom at an individual node from global directions to a local direction through an orthogonal transformation. UTRANFORM allows you to change the transformation with each increment. When you invoke this option, the nodal output is in both the local and the global system.

Main Index

CHAPTER 9 601 Boundary Conditions

Shell Transformation The SHELL TRANSFORMATION option allows you to transform the global degree of freedom of doubly curved shells to shell degrees of freedom in order to facilitate application of forces in the shell directions, edge moments, and clamped or simply supported boundary conditions. There are four types of shell transformations. The SHELL TRANSFORMATION model definition option specifies information on the shell transformation. For Types 1 and 3, only the node number has to be specified. For Types 2 and 4, a boundary direction (the direction cosine of t as shown in Figure 9-24) also has to be specified in the θ 1, θ 2 surface. θ2 1

θ1 Figure 9-24 Boundary Directions in Shell Transformation

After transformation, the following definitions apply. Type 1: Transformation for two-dimensional beams and shell nodes (Element Types 15, 16, and 17). The transformation defines the degrees of freedom with respect to a local coordinate system (s, n) (see Figure 9-32). The four degrees of freedom after transformation are: 1 = us

tangential displacement

2 = u n normal displacement

Main Index

3= φ

rotation

4= ε

Meridional stretch

602 Marc Volume A: Theory and User Information

x2 n

s

Positive Direction

x1 Figure 9-25 Type 1: Shell Transformation

Type 2: Transformations for doubly curved shell nodes with nine degrees of freedom (Element Type 4 corner nodes of Element Type 24). The transformation defines a local coordinate system ( t, s, n ). (See Figure 9-26). The nine degrees of freedom after transformation are: 1 = ut

displacement in specified (boundary) direction

2 = us

displacement normal to (boundary) direction but tangential to shell surface

3 = un

displacement normal to shell surface

4 = φt

rotation of shell around boundary

5 = φs

rotation of shell around normal to boundary tangential to the shell surface

6 = φn

rotation of boundary around normal to shell surface

7 = εt

stretch tangential to specified (boundary) direction

8 = εs

stretch normal to specified (boundary) direction

9 = γt s

shear stretch in t-s direction

s

n

θ2

t θ1

x3 x2

x1 Figure 9-26 Types 2 and 4: Shell Transformations

Main Index

CHAPTER 9 603 Boundary Conditions

Type 3: Transformations at midside nodes for doubly curved shell nodes with three degrees of freedom (Element Type 24). The transformation defines a local coordinate system ( t, s, n ), (see Figure 9-27). The degrees of freedom after transformation are: 1 = ∂u t ⁄ ∂s

rotation of normal to boundary around normal to shell

2 = ∂u s ⁄ ∂s

stretch normal to boundary

3 = ∂u n ⁄ ∂s

rotation around boundary

n x3

t

s

x2

x1 Figure 9-27 Type 3: Shell Transformation

Type 4: Transformation for doubly curved nodes with 12 degrees of freedom (Element Type 4). The transformation defines a local coordinate system ( t, s, n ). The first 9 degrees of freedom after transformation are the same as 1 through 9 in Type 2 (Figure 9-26), and the remaining three are: 2

10 = ∂ u t ⁄ ∂Θ 1 ∂Θ 2 2

11 = ∂ u s ⁄ ∂Θ 1 ∂Θ 2 2

12 = ∂ u n ⁄ ∂Θ 1 ∂Θ 2

variation of g along the boundary

(9-32)

variation of e along the boundary

(9-33)

variation of f along the boundary

(9-34)

When using the SHELL TRANSFORMATION option, the displacement increments and reaction forces are output in the local directions immediately after solution of the equations. At the end of the increment, you can print out the global displacement increments and total displacements in the global coordinate directions. If you invoke the FOLLOW FOR parameter, the SHELL TRANSFORMATION option defines a local coordinate system in the current (updated) geometry of the structure. This additional feature is especially useful with the LARGE STRAIN parameter, because you can then specify edge moments and/or large edge rotations of shells and beams. Caution: If you apply a shell transformation to a node, do not apply a standard transformation or shell tying type to that node.

Main Index

604 Marc Volume A: Theory and User Information

Tying Constraint Marc contains a generalized tying (constraint) condition option. Any constraint involving linear dependence of nodal degrees of freedom can be included in the stiffness equations. A tying constraint involves one tied node and one or more retained nodes, and a tying (constraint) condition between the tied and retained nodes. The degrees of freedom (for example, displacements, temperatures) of the tied node are dependent on the degrees of freedom of the retained nodes through the tying condition. In some special tying conditions, the tied node can also be a retained node. The tying condition can be represented by a tying (constraint) matrix. Note that if the tying constraint involves only one retained node, the choice of which node is to be tied to retained is arbitrary. As a simple example, impose the constraint that the first degree of freedom of node I be equal to that of node J at all times (see Figure 9-28). As a second example, the simulation of a sliding boundary condition requires the input of both the boundary conditions and the tying constraints (see Figure 9-29). UI

I

Constraint Equation: UI = UJ 2,V

J 1,U

UJ

Tied node I, retained node J, or Tied node J, retained node I

Figure 9-28 Simple Tying Constraint

Local axes i

Y (v)

j

X

Y

k l X (u) Figure 9-29 Tying Constraint Illustration (Sliding Boundary Conditions)

The example illustrated in Figure 9-29 enforces rigid sliding on the boundary in the local coordinates defined above.

Main Index

vi = vj = vk = v1 = 0

(9-35)

ui = uj = uk = u1

(9-36)

CHAPTER 9 605 Boundary Conditions

The first equation is a set of fixed boundary conditions. The second equation is a constraint equation and can be rewritten as three constraint equations: ui = uj

(9-37)

uk = uj

(9-38)

u1 = uj

(9-39)

These equations express all the u displacements in terms of u j . In this example, node j is chosen to be the retained node; nodes i, k, and l are tied nodes. You can use the TYING option to enter this information. Marc has a number of standard tying constraints that can be used for mesh refinement, shell-to-shell, shell-to-beam, beam-to-beam, and shell-to-solid intersections. Tables 9-16 through 9-19 describe these options. Tables Table 9-21 through Table 9-23 show the tying constraints for pipe elements, shell stiffeners, and nodal degrees of freedom. Table 9-24 summarizes the rigid link constraint. The SERVO LINK option uses the homogeneous linear constraint capability (tying) to input simple constraints of the form ut = a1 ur 1 + a2 ur 2 + …

(9-40)

where u t is a degree of freedom to be constrained; u r 1, u r 2, … are the other retained degrees of freedom in this structure; and a 1, a 2, … are constants provided in this option. You can use the TYING or SERVO LINK model definition option to enter standard tying constraint information, and the TYING CHANGE option to change tying constraints during load incrementation. The UFORMSN user subroutine is a powerful method to specify a user-defined constraint equation. This constraint can be nonlinear; for example, it can be dependent on time or previous deformation.

Main Index

606 Marc Volume A: Theory and User Information

Table 9-16

Tying Constraints for Mesh Refinement

Tying Code

Number of Retained Nodes

31

Purpose

Remarks

2

Refine mesh of first order (linear displacement) elements in two dimensions

Tie interior nodes on refined side to corner nodes in coarse side (see Figure 9-30)

32

3

Refine mesh of second order (quadratic displacement in two dimensions

Tie interior nodes on refined side to edge of element of coarse side (see Figure 9-31)

33

4

Refine mesh of 8-node bricks

Tie interior node on refined side to four corner nodes of an element face on coarse side (see Figure 9-32)

34

8

Refine mesh of 20-node bricks

Tie interior nodes on refined side to eight (four corner, four midside) nodes of element face on coarse side (see Figure 9-33)

R

T – Tied Node R – Retained Node

T

R Figure 9-30 Mesh Refinement for 4-Node Quad R T T T – Tied Node R – Retained Node

R T T R Figure 9-31 Mesh Refinement for 8-Node Quad

Main Index

CHAPTER 9 607 Boundary Conditions

R T R

R Figure 9-32 Mesh Refinement for 8-Node Brick R T R T R T R T R Figure 9-33 Mesh Refinement for 20-Node Brick Table 9-17

Tying Constraints for Shell-to-Shell Intersection

Tying Code

Number of Retained Nodes

22

2

Join intersecting shells, Element Type 4, 8, or 24; fully momentcarrying joint

Tied node is also the second retained node*

18

2

Join intersecting shells, Element Type 4, 8, or 24; fully momentcarrying joint

Tied node is also the second retained node

28

2

Join intersecting shells, Element Type 4, 8, or 24; pinned point

Tied node is also the second retained node

24**

2

Join intersecting shells or beams, Element Types 15-17

Tied node is also the second retained node

Purpose

Remarks

* Thickness vector must be specified at tied nodes and retained nodes. ** See Figure 9-34.

Main Index

608 Marc Volume A: Theory and User Information

2

B

A

S

S

1 Figure 9-34 Standard Tying Type 24, Tie Shell-to-Shell or Beam-to-Beam; Moment-Carrying Table 9-18

Tying Constraints for Beam-to-Beam Intersection

Tying Code 13

Number of Retained Nodes 2

52

1

53

1

Table 9-19

Purpose Join Two Elements Type 13 under an arbitrary angle; full momentcarrying joint Pin joint for Beam Type 14, 25, 52, 76-79, 98 Full moment-carrying joint for Beam Types 14, 25, 52, 76-79, 98

Remarks Tied node also the second retained node

Tie interior node on refined side to four corner nodes of an element face on coarse side (see Figure 9-32)

Tying Constraints for Shell-to-Solid Intersections

Tying Code

Number of Retained Nodes

23

1

Tie axisymmetric solid node to axisymmetric shell (Element Type 1 or 89) node

25

2

Join solid mesh to beam (Type 16) Tied node also second retained Join solid mesh to axisymmetric node. (see Figure 9-36)

Purpose

Remarks Tied and retained nodes must be transformed to local system and TRANSFORMATION option invoked (see Figure 9-35).

shell (Type 15) 26

Main Index

2

Tie axisymmetric solid node to axisymmetric shell (Element Type 1 or 89) node

Similar to tying type 23 but no transformation is required. Tied node also second retained node. (see Figure 9-36)

CHAPTER 9 609 Boundary Conditions

T1 y’

R T2 x’

Figure 9-35 Standard Tying Type 23, Tie Solid-to-Shell (Element Type 1 or 89) T1 T2 ε B A

α

R

T3 T4

Figure 9-36 Standard Tying Type 25, Tie Solid-to-Beam (Element Type 16) Standard Tying Type 25, Tie Solid-to-Axisymmetric Shell (Element Type 15) Standard Tying Type 26, Tie Solid-to-Axisymmetric Shell (Element Type 1 or 89)

Main Index

610 Marc Volume A: Theory and User Information

Table 9-20

Tying Code 44

Tying Constraints for Beams to Element Edge or Face or Axisymmetric Shell to Element Edge

Number of Retained Nodes

Purpose

Remarks

2 is 2-D or axisymmetric lower-order element edge

Rigidly tie a node with displacements and rotations to a surface patch. This is internally used for CWELD and CFAST option.

The number of retained nodes is required. This tying type fully supports large deformation/rotations. No transformations are required. See Figure 9-37.

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

Main Index

CHAPTER 9 611 Boundary Conditions

R R T

T

R R R

2-D Application Lower-order

2-D Application Higher-order

R

R R

R

R

R

T

T

R R

R R

3-D Application Lower-order Quadrilateral Face

3-D Application Higher-order Triangular Face

Figure 9-37 Beam to Edge Moment Carrying Constraints

Main Index

612 Marc Volume A: Theory and User Information

Table 9-21

Tying Constraints for Pipe Bend Element (Elements 14 and 17)

Tying Code

Number of Retained Nodes

15

One less than the number of shell Special tying types for pipe bend Element 17 to nodes in the z-r plane of the section remove rigid body modes

16

Number of shell nodes in the z-r plane of the section

17

Table 9-22

Main Index

Purpose

2

Special tying types for pipe bend Element 17 to remove rigid body modes Special tying types for pipe bend Element 17 to couple bend section into pipe bend

Tying Constraints for Shell Stiffener (Element 13 as a Stiffener on Shell Elements 4 or 8)

Tying Code

Number of Retained Nodes

19

2

Use beam Element 13 as a stiffener on Tied node also second retained node 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 Type 8 Always used after tying Element tied to the interpolated shell Type 21 displacements 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 Must be followed by tying interpolated shell node not a vertex of Type 20 an element (Element Type 8 only) must be followed by Type 20 to tie interpolated shell node into shell mesh

Purpose

Remarks

CHAPTER 9 613 Boundary Conditions

Table 9-23

Tying Code

Tying Constraints for Nodal Degrees of Freedom

Number of Retained Nodes

Purpose

Remarks

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

>100

1

Generate several tyings of type ≤NDEG

Tying code is first degree of freedom multiplied by 100 added to last degree of freedom (209 means tie second through ninth degree of freedom at tied node to respective second through ninth degree of freedom at retained node)

User-defined

User-generated tying type through the UFORMSN user subroutine

<0 (negative integer)

NDEG = number of degrees of freedom per node

Rigid Link Constraint Tying type 80 can be used to define a rigid link between nodes. This capability can be used for both small deformation and large deformation, large rotation problems. In small deformations, a linear constraint equation is used. In addition to the end points of the link, a second retained node must be given. This node is used to calculate and store the rigid body rotations. For two-dimensional problems, this represents a rotation about the Z-axis and this is stored as the first degree of freedom for the node. In 3D, it should be noted that the rotations/moments about the x, y, and z axes for the second retained node are stored and output as its first, second, and third degrees of freedom, respectively. A complete rigid region can be modeled by using multiple tying type 80’s. In this case, the same two nodes are used for the retained nodes in all of the constraints. Transformations can be applied to the retained nodes so that any kinematic or force boundary conditions can be defined in a local coordinate system. It is not necessary that the same transformations should be applied to both retained nodes. It is also optional to transform the tied nodes to the same or a different local coordinate system. The rigid links can be used with all elements except types 4, 8, 24, 15, 16, and 17. In addition, it should not be used in rigid plastic analysis.

Main Index

614 Marc Volume A: Theory and User Information

To reduce linearization errors in large deformation, large rotation problems using tying type 80, an optional recycling feature is offered through the CONTROL model and history definition options. Recycling occurs if the maximum change over the retained nodes of rigid link 80 exceed a rotation tolerance (default is 0.001 radians). This check can be circumvented by setting the rigid link rotation tolerance to zero (in conjunction with the FEATURE,5701 parameter) or a negative number. Table 9-24

Rigid Link Constraint

Tying Code

Number of Retained Nodes

80

2

Purpose

Remarks

Define a rigid link between nodes The second retained node is an unattached node which contains the rotation

Shell-to-Solid Tying In many problems, a region exists that is modeled with both brick elements and shell elements. A particular case of this is shown is Figure 9-38 and Figure 9-39.

Figure 9-38 4-Node Shell-to-Solid Automatic Constraint

Figure 9-39 8-Node Shell-to-Solid Automatic Constraint

In the first case, an 8-node brick which has been reduced to a triangular prism is connected to a 4-node shell. In the second case, a 20-node brick is connected to an 8-node shell. An automatic constraint equation is developed between the elements. Note that the thickness of the shell must be entered as the brick thickness.

Main Index

CHAPTER 9 615 Boundary Conditions

Rigid Tying to a Surface Patch Tying type 44 rigidly ties a node with its translation and rotation degrees of freedom to a surface patch. There are four different tying types for 3-D analyses tying the displacements and rotations of a node (assuming it has 6 degrees of freedom) to the motion of a 3- or 6-node triangular patch or a 4- or 8-node quadrilateral patch. There are two different tying types for 2-D analyses, tying the displacements and rotation of a node (assuming it has three degrees of freedom) to the motion of a 2- or 3-node line patch. The tied node can be a node of a beam or a shell element and will generally have translation and rotation degrees of freedom. The retained nodes are the nodes of the patch and the only retained degrees of freedom involved in the tying are the patch node translations. The exact tying type is determined from the tying type number (44) and the number of retained nodes and, therefore, the latter is required in the input. The location where the tied node pierces the patch is computed in terms of the local parametric coordinates that define locations inside a patch using the usual shape functions for such a patch. The translations of this piercing point are computed from the nodal displacements of the patch, again using the usual shape functions of the patch and these define the translations of the tied node. The rotations can be computed by constructing a local triad to the patch at the piercing point. The translations of the patch nodes define the change in orientation of the triad. The orientation change of the triad defines the rotations of the tied node. The tied node must have a proper projection on the patch inside its boundary. When it does not lie exactly on the patch, the distance will be treated as an offset. The patch does not necessarily have to coincide with a shell or brick element face in a 3-D model or a beam or quad element edge in a 2-D model, but the nodes constituting a patch must adhere to the conventions that are generally required for the particular patch. The patch also does not have to be a flat surface in 3-D or a straight line in 2-D, but it is recommended to avoid overly distorted patches. A patch is considered overly distorted when the patch normals at two of its nodes make an angle larger than 10 degrees. In case of a heat transfer or a thermo-mechanically coupled analysis the temperatures may be tied as well. The temperature constraints are similar to the mechanical displacement constraints, but only one degree of freedom is involved. When the retained nodes are shell nodes, the temperature is always tied to the first degree of freedom of the shell nodes (i.e., the top surface of the shell), regardless of the orientation in space. When the tied node is a shell node, its first degree of freedom is tied. In other analysis procedures, tying type 44 is not supported. When no geometric nonlinearities are flagged in the model (i.e., neither the LARGE DISP nor the LARGE STRAIN parameter is activated), Marc uses the small displacement method to apply the constraints. In all other cases, the large displacement method is used fully accounting for finite rotations. The small displacement method linearizes the constraint equations w.r.t. the reference configuration. The large displacement method takes account of all geometric nonlinearities caused by finite displacements and rotations.

Main Index

616 Marc Volume A: Theory and User Information

e3 η GA

e2 e1 ξ

Patch at end of increment

Patch at start of increment Figure 9-40 Motion of a Patch From Start to End of an Increment

The large displacement method (Figure 9-40) can be summarized as follows. The point GA is the node of, for example, a beam and it pierces the patch at some point for which the parametric coordinates ξ G A , η G A have been computed. A local triad is fixed to the beam cross section and another triad to the piercing point on the patch. For simplicity, it is assumed that both triads have the same orientation in the initial configuration. The tying constraints are that the displacements of the beam node and the displacements of the piercing point on the patch are equal and that the rotations of the triad connected to the beam cross-section and the triad connected to the patch are equal. The rotations of the triad fixed to the beam cross-section are expressed in terms of the rotational degrees of freedom of the beam node. The rotations of the triad fixed to the patch are expressed in terms of the displacement degrees of freedom of the patch nodes. In this way, the nonlinear relations are established between the beam rotations and the patch displacements. The relations between the displacements of the beam node and the displacements of the patch nodes are linear when the beam node lies exactly on the patch. In case of an offset, nonlinear contributions due to the rotations are added to the constraints. The tied node generally has translation and rotation degrees of freedom, but this is not a requirement. In case it has only translation and rotation degrees of freedom, the displacements are tied to the patch, possibly accounting for an offset. No constraints are applied for rotations; hence, adequate constraints must be applied to prevent a singular system. The connectivity conventions for the patches are shown in Figure 9-41 for 2-D and 3-D models:

Main Index

CHAPTER 9 617 Boundary Conditions

Line2 1

2-D Model

2

Line3 1

2

3

(a) Line Patch in 2-D Analysis 4

3

1

2

Quad4

3-D Model 4 Quad8

3

7

8

6

1

2

5

(b) Quadrilateral Patch in 3-D Analysis 3 Tria3 1

2

3-D Model 3 Tria6

6 1

5 4

2

(c) Triangular Patch in 3-D Analysis

Figure 9-41 Patch Connectivity Convention

Overclosure Tying In various engineering applications, it is necessary to define a pre-stress in, for example, bolts or rivets before applying any other structural loading. Although such a pre-stressed state is often simulated using a temperature loading, it is rather difficult to arrive at a desired net force in the bolt or rivet. An easier way is to use overclosure tyings (type 69). These tyings create overlaps or gaps between two parts of a model. If the motion of these parts is somehow constrained in the direction in which the gap or overlap is being created, then an overlap will introduce an tensile (pre-) stress in each of the parts and a gap will result in a compressive stress. Overclosure tyings have one tied node and two retained nodes. The tied node and the first retained node are usually nodes on the boundaries of the respective parts (see Figure 9-42). The second retained node is very often a free node and is usually shared by all overclosure tyings which connect the parts. This node is also called the control node of the tying, since it can be used to apply load or control the size of the gap or overlap between the parts.

Main Index

618 Marc Volume A: Theory and User Information

top part top nodes (first retained)

top part mesh split overclosure tyings

Fcontrol

F1,bot

F2,bot

u1,bot

u2,bot ucontrol

u1,top

u2,top

F1,top

F2,top

(overlap) ucontrol

control node (second retained) bottom nodes (tied) bottom part

bottom part

undeformed

deformed

Figure 9-42 Pre-stressing a Structure by Creating an Overlap Between the top and the Bottom Part Using Overclosure Tyings

An overclosure tying imposes the following constraint on the model: u tied = u retained + u control ,

(9-41)

in which u tied , u retained and u control are the displacement and rotation degrees of freedom (if any) of, respectively, the tied node, the first retained node, and the control node of the tying. It immediately follows from this equation that u control is the displacement difference of the tied and the retained node of the tying and is equal to the size of the overlap or gap between the parts. Hence, by prescribing this displacement using the FIXED DISP and DISP CHANGE options, gaps or overlaps of a particular size can be created. Instead of prescribing the size, gaps or overlaps can also be created by prescribing the total force in the model. This follows immediately from the fact that the work done by a constraint equation is zero. To demonstrate this, consider the model displayed in Figure 9-42. The model is split into two disjoint parts: the top part and the bottom part. At the split, corresponding nodes of the respective parts are connected by overclosure tyings, in which the nodes of the bottom part are the tied nodes and the nodes of the top part are the first retained nodes of the tyings. Both tyings share a common (free) control node. If u 1, bot and u 2, bot are the displacements of the bottom nodes and u 1, top and u 2, top are the displacements of the top nodes, then the two overclosure tyings impose the following two constraints on this model: u 1, bot = u 1, top + u control ,

(9-42)

u 2, bot = u 2, top + u control .

(9-43)

Introducing the vectors, u =

Main Index

u 1, bot u 2, bot u 1, top u 2, top

T

and uˆ =

u 1, top u 2, top u control

T

,

CHAPTER 9 619 Boundary Conditions

and the constraint matrix

T =

I 0 I 0 0 I 0 I I I 0 0

T

,

in which I and 0 are the unit and null matrices, Equations (9-42) and (9-43) can be summarized into the matrix equation: u = Tuˆ .

(9-44)

Let F =

F 1, bot F 2, bot F 1, top F 2, top

T

and

Fˆ =

Fˆ 1, top Fˆ 2, top Fˆ control

T

be the force vectors which are work conjugate to the displacements u and uˆ , respectively. Then the zerowork principle states that T

T F u = Fˆ uˆ .

(9-45)

Substitution of Equation (9-44) into Equation (9-45) and requiring that the result is valid for all uˆ , it T follows that T F = Fˆ , or

F 1, bot + F 1, top = Fˆ 1, top ,

(9-46)

F 2, bot + F 2, top = Fˆ 2, top ,

(9-47)

F 1, bot + F 2, bot = Fˆ control .

(9-48)

Equations (9-46) and (9-47) express the equilibrium of forces across the split, in which Fˆ 1, top and Fˆ 2, top can be viewed as externally applied forces. While Equation (9-48) enables overclosure tyings to pre-stress a model with a certain total force. It states that if the constraints described by Equations (9-42) and (9-43) are applied, the force on the control node is the sum of the forces on the tied nodes of all overclosure constraints which share that control node. Hence, the total force on the bottom part of the model is prescribed by applying a force to the control node using the POINT LOAD option. Obviously (by the equilibrium Equations (9-46) and (9-47)) if no external force is applied to the nodes on the split, the total force on the top part is equal but opposite is sign to the force on the control node.

Main Index

620 Marc Volume A: Theory and User Information

Notes:

Both methods to control the size of overlaps or gaps can be combined in one analysis. For example, in the first part of an analysis, a pre-stress can be defined by prescribing the net force in the structure using the POINT LOAD option on the control node of the overclosure tyings. Then in the second part, the size of the gap or the amount of overlap which is the result of this load, can be fixed by suppressing the displacement changes of the control node using the DISP CHANGE option. If similar arguments are applied to tying 100 (which yields Equation (9-41) without the dependence on the control node), then only the equilibrium Equations (9-46) and (9-47) are obtained. Equation (9-48) is solely due to the dependence of Equation (9-41) on the control node.

The control node of an overclosure tying has the same displacement and rotation degrees of freedom as the tied and the first retained node as given by Equation (9-41). This allows creation of overlaps or gaps in any particular direction or combination of directions. Local coordinate systems can be defined at any of the nodes of an overclosure tying using the TRANSFORMATION option. Since the constraint Equation (9-42) is always applied in the global coordinate system, a local coordinate system at the control node can be used to pre-stress the model in directions other than the global coordinate directions. Sufficient boundary conditions must be applied on the control node to suppress any rigid body modes, if the two parts of the structure are not constrained otherwise. Total forces on the split are available for postprocessing as reaction forces on the control node for all suppressed or prescribed displacements and rotations. Overclosure tyings can be used in combination with the CONTACT option, that is, the tied and the first retained node may be nodes on the boundary of a contact body. In non-mechanical passes of a coupled analysis, the overclosure tying reduces to tying type 100 between the tied node and the first retained node. There is no dependence on the control node in that case. This guarantees continuity of the primary field variable (for example, temperature) across the split. Table 9-25

Main Index

Overclosure Tying

Tying Code

Number of Retained Nodes

69

2

Purpose

Remarks

Create 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 nonmechanical passes, the tying reduces to tying type 100 between the tied and the first retained node.

CHAPTER 9 621 Boundary Conditions

9

Insert

Boundar y Conditio ns

Marc provides an INSERT model definition option which 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. The INSERT model definition option can be used to place reinforcing cords or rods, such as 2-D rebar membrane elements, into solid elements. The INSERT model definition 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. If a node to be inserted is also a node of a host body element, no tying is applied to the node. Transformation must not be used at any nodes of host body elements and at inserted nodes, unless the same set of local coordinate system is used for all nodes involved.

AUTOMSET This parameter automatically re-writes the constraint equations such that a tied degree of freedom is not used as a retained degree of freedom in another constraint equation. It also modifies constraint equations where a constrained degree of freedom is used in a prescribed boundary condition. Because of chaining of constraint equations, this is not always possible, in which case the analysis will terminate. The constraint equations that are considered are those obtained from user-specified options: TYING SERVO LINK RBE2 RBE3 RROD CONRAD GAP

Constraint equations internally generated are not considered from the following options: CONTACT INERTIA RELIEF INSERT

If both the MPC-CHECK and AUTOMSET parameters are included in the model, the MPC-CHECK parameter is ignored.

Support Conditions Marc provides linear and nonlinear springs and foundations for the modeling of support conditions. For dynamic analysis, a dashpot can also be included. Table 9-26 lists input options for linear and nonlinear springs and elastic foundations.

Main Index

622 Marc Volume A: Theory and User Information

Table 9-26

Input Options for Springs and Elastic Foundations

Input Options Load Description

Model Definition

Springs

SPRINGS

Elastic Foundation

FOUNDATION

History Definition

User Subroutine USPRNG

FOUNDATION

USPRNG

The force in the spring is F = K ( u2 – u1 ) + D ( v2 – v1 )

(9-49)

where K is the spring stiffness, u 2 is the displacement of the degree of freedom at the second end of the spring, and u 1 is the displacement of the degree of freedom at the first end of the spring. In a dynamic analysis, D is the damping factor and v 2 and v 1 are the velocities of the nodes. You can specify the elements in Marc to be supported on a frictionless, elastic foundation. The foundation supports the structure with a force per unit area (force per unit length, for beams) given by p n = Ku n

(9-50)

where K is the equivalent spring stiffness of the foundation, and u n is the normal displacement of the surface at a point in the same direction as p n . The same conventions apply to the elastic foundation specification as for pressure specification, in terms of the face of the element that is used. The force is applied whether the displacement is tensile or compressive. Nonlinear spring stiffness for mechanical, thermal, and electrical analyses can be specified through tables using the parameter and model definition option. For more details, refer to Chapters 2 and 3 in Marc Volume C: Program Input. The USPRNG user subroutine allows you to supply or further modify a nonlinear spring stiffness or specify a nonlinear foundation stiffness as a function of prior displacement and force.

Bushings A generalized spring-damper capability is provided in Marc to model bushings between various components. They are modeled using element types 194 and 195 for 2-D and 3-D applications, respectively. The connectivity of these elements is generally comprised of two nodes which are specified through the CONNECTIVITY model definition option. Grounded bushing elements can be defined by providing only the first end-node for connectivity. The properties of these bushing elements are specified through the PBUSH or PFAST model definition option. These elements may be automatically generated using the CFAST option.

Main Index

CHAPTER 9 623 Boundary Conditions

Bushing Coordinate System A unique coordinate system is used to specify the bushing properties. A number of options are available to define this coordinate system: • local element coordinate system along the bushing element • global cartesian coordinate system, or • a user-specified coordinate system specified through the COORD SYSTEM option. The bushing coordinate system defined through global cartesian coordinates or through the user-specified COORD SYSTEM option are maintained constant and are not updated for large displacement analysis. The local element coordinate system can only be used for 2-node bushing elements. In this case, the local X axis is along the element length and forms a perpendicular triad with the local Y and Z axes. In 2-D, the local Z axis is always taken as (0,0,1) and the local Y axis is then perpendicular to the local X axis in the global x-y plane. In 3-D, the local Y-Z axes are located by using an extra node or an orientation vector. If both are specified, the extra node takes precedence. The local Y axis is first estimated by using the orientation vector or using the vector from the first bushing node to the extra node. The local Z axis is then formed by taking the cross product of the local X and estimated local Y axis. The final local Y axis is obtained by taking the cross product of the local Z and local X axes. For large displacement analysis, the local element coordinate system is updated continuously. Mid-increment direction cosines are used to calculate the strains while end-increment direction cosines are used to calculate the stiffnesses and internal bushing forces. Nodal Offsets for Bushing Elements The exact position of the bushing element can be modified by specifying nodal offsets. This offset point is generally defined from the first end-node of the bushing element. It serves two purposes: It allows convenient modeling of the bushing at a location away from the actual physical location. Also, it allows coupling between translational and rotational stiffnesses. The offset point can be located along the bushing element axis, in the global cartesian coordinate system, or in a user-defined coordinate system. In the first case, the offset point is located along the line joining the two end nodes of the bushing element. The distance of the offset point from the first node S is specified by the user. In the second case, the offset vector to the bushing location from the first end-node is specified. The treatment of offsets for bushing elements closely follows the treatment of offsets for beam elements (described later in Beam - Shell Offsets). Once the offset point location is specified, the offset vector from each node is determined. The equations governing the treatment and update of the offsets are given by Equations (9-62) to (9-65). Bushing properties are used to define the stiffness/damping/mass matrix at the offset position and are then transformed to the geometrical position.

Main Index

624 Marc Volume A: Theory and User Information

zelem Bush Location

zelem

1

yelem CID

xelem (S1,S2,S3) OCID

v yelem

S.l

2

(1-S) . l Bush Location

1 2

xelem Figure 9-43 Offset location Specification for Bushing Element

Bushing Properties Five sets of properties can be provided for bushing elements depending on the analysis type. All properties are provided through the PBUSH or PFAST model definition option: • • • • •

mechanical stiffness - for static/dynamic/harmonic analysis mechanical dashpot - for dynamic/harmonic analysis mass - for dynamic/harmonic analysis thermal conduction coefficient - for heat transfer/coupled analysis involving a thermal pass electrical resistance coefficient - for electrical/coupled analysis involving a joule pass

Mechanical stiffness for bushing elements can be specified either directly in coefficient form or through force-displacement curves. Note that 2-D bushing elements have two translational and one rotational degree of freedom and separate stiffnesses can be specified for the X, Y and RZ degrees of freedom. Three-dimensional bushing elements have three translational and three rotational degrees of freedom and separate stiffnesses can be specified for X, Y, Z and RX, RY, RZ degrees of freedom. For nonlinear bushing elements, these stiffnesses can be varied through tables. These tables can be a function of time, increment number, position coordinates, frequency (only for harmonic analysis), temperature, displacement (this variable is mandatory when stiffness is specified via forces). Up to four independent variables can be used in the tables. Based on the current stiffness value and the change in displacement between the end-nodes, the bushing forces are updated in the specified bushing coordinate system. Two forms of damping can be specified for the bushing elements: Nominal damping B i for the ith degree of freedom of the bushing elements where the damping is specified either directly in coefficient form or through force-velocity curves. For nonlinear dampers, the nominal damping can be varied through tables as a function of time, increment number, position coordinates, frequency (only for harmonic analysis), temperature or velocity (this variable is mandatory when nominal damping is specified via forces). The second form of damping is structural damping Si for the ith degree of freedom of the bushing elements.

Main Index

CHAPTER 9 625 Boundary Conditions

The damping is specified in coefficient form only in this case and can be varied through tables with similar independent variables as the nominal damping case. A composite damping coefficient is formed for the bushing element as follows: G 1 C i = B i + -------- K i + -------- S i K i W3 W4 where C i is the total damping coefficient; G, W3, and W4 are structural coefficients that are specified through the COEFFICIENT model definition option; B i is the nominal damping coefficient; S i is the structural damping coefficient; and K i is the current stiffness coefficient. For a linear bushing element, the total force is given by Equation (9-49). Note that for bushing elements defined in the local element coordinate system, the force is positive if the bushing element is in tension and negative if it is in compression. For bushing elements defined via the global coordinate or user-coordinate systems, the force along a particular degree of freedom is positive if the displacements of end-node 2 along the specified degree of freedom is greater than the displacement of end-node 1 along the specified degree of freedom. Note that if tables are used to define the bushing properties, care should be taken to include both positive and negative values of independent variables like displacements/velocities since these would influence the calculated stiffnesses. For dynamic and harmonic analyses, lumped translational and rotational masses can be provided at the end-nodes of the cbush elements. Uniform masses apply to translational and rotational degrees of freedom at the end-nodes and are maintained constant through the analysis. Stresses in the bushing elements can be related to the associated forces through recovery coefficients. Similarly, strains in the bushing elements can be related to the associated deformations through recovery coefficients. Separate coefficients are allowed for the translational components and the rotational components through the PBUSH option. If set to 1.0, the stresses are equal to the forces and the strains are equal to the difference in displacements between the end-nodes. The bushing elements can also be used for thermal or electrical field analyses. The coefficients of thermal conduction and electrical resistance are specified via the PBUSH option. The bushing element behaves like a general link in this case and dashpot properties are not considered. Tables can be used to vary the properties as a function of temperature (for thermal conduction), voltage (for electrical resistance), time, increment number, coordinates.

Cyclic Symmetry A special set of tying constraints for continuum elements can be automatically generated by the Marc program to effectively analyze structures with a geometry and a loading varying periodically about a symmetry axis. Figure 9-44 shows an example where, on the left-hand side, the complete structure is given and, on the right-hand side, a sector to be modeled.

Main Index

626 Marc Volume A: Theory and User Information

Y

Y y’

B

x’

α X

A

X

Figure 9-44 Cyclic Symmetric Structure: Complete Model (Left) and Modeled Sector (Right)

Looking at points A and B on this segment, the displacement vectors should fulfil: (9-51)

u' B = u A which can also be written as:

(9-52)

u B = Ru A where the transformation matrix R depends on the symmetry axis (which, in the example above,

coincides with the global Z-axis) and the sector angle α (see Figure 9-44). In Marc, the input for the CYCLIC SYMMETRY option consists of the direction vector of the symmetry axis, a point on the symmetry axis and the sector angle α . The following items should be noted: 1. The meshes do not need to line up on both sides of a sector (for example, see Figure 9-45).

Figure 9-45

Finite Element Mesh for Cyclic Symmetric Structure with Different Mesh Densities on the Sector Sides

2. Any shape of the sector sides is allowed provided that upon rotating the sector 360 ⁄ α times about the symmetry axis over the sector angle α will result in the complete model. 3. The CYCLIC SYMMETRY option can be combined with the CONTACT option. In this case, both sides of the cyclic symmetry sector must belong to a contact body and corresponding parts of the sector sides must belong to the same body (see Figure 9-46). Note that the contact bodies do not need to span between the sector sides.

Main Index

CHAPTER 9 627 Boundary Conditions

Figure 9-46

Cyclic Symmetry and Contact Bodies; upper left: one body (correct); upper right: two bodies (correct); lower left: two bodies (right); lower right: two bodies (wrong; corresponding parts of the sector sides are not in the same body).

4. The CYCLIC SYMMETRY option can be combined with global remeshing. 5. In a coupled thermo-mechanical analysis, the temperature is forced to be cyclic symmetric ( T A = T B as in Figure 9-44). 6. A nodal point on the symmetry axis is automatically constrained in the plane perpendicular to the symmetry axis. 7. The possible rigid body motion about the symmetry axis can be automatically suppressed. 8. Cyclic Symmetry is valid for: a. 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 is 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. nonlinear static analysis including remeshing as well as coupled analysis. c. valid for all analysis involving contact. d. 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 the following paragraphs. 9. Cyclic Symmetry is invalid for pure heat transfer. 10. In order to check which nodes get tying constraints due to cyclic symmetry, nodal post code 38 (contact status) can be used; its value will be 2.

Main Index

628 Marc Volume A: Theory and User Information

To prevent confusion, it must be emphasized that the cyclic symmetry feature described above is different than linear cyclic symmetry commonly used in modal analysis where physical quantities such as, x n , displacements, forces, stresses and temperature in the n-th segment are expanded in a Fourier series with k

terms of the cyclic components, u , in the fundamental region, like: K

xn

1 0 = ---- u + N

2 ---N

∑

[u

k, c

cos ( n – 1 )kα + u

k = 1

k, s

N n – 1 ----

2 ( –1 ) sin ( n – 1 ) kα ] + ---------------------- u N

(9-53)

where k is the harmonic order; N is the total number of sectors; α is the fundamental inter-sector phase shift defined as 2π ⁄ N ; and K is defined as: N–1 ⎧ ------------⎪ 2 K = ⎨ N–2 ⎪ ------------⎩ 2

if N is odd (9-54) if N is even

There are considerable savings in both computing time and data storage associated with the use of the linear cyclic symmetry concept. Assuming a finite element model with a sector size of m degrees of freedom, a real-valued cyclic symmetry approach leads, in the worst case, to one eigenvalue problem of size m and ( N – 1 ) ⁄ 2 eigenvalue problems of size 2m ; a complex approach leads to N eigenvalue problems of size m; while the full analysis leads to a single, but very costly, eigenvalue problem of size Nm . Although linear cyclic symmetry can reduce the problem size greatly, it is restricted to linear analysis, and the sector must have its surface mesh on the symmetry planes to be identical on each side of the sector. The nonlinear cyclic symmetry implemented in Marc can be used for nonlinear problems, such as contact, and the nodes do not need to line up on both symmetry planes of the sector (for example, see Figure 9-45).

Nastran RBE2 and RBE3 The basic formulation of the Nastran rigid body elements RBE2 and RBE3 is similar to tying type 80, which is also known as a rigid link. However, they offer additional flexibility because the degrees of freedom may be partly unconstrained and a list of tied/retained nodes can be entered with RBE2 and RBE3. RBE2 The nonlinear relation of an RBE2 can be expressed as follows: xt = R ( θr ) ( xt – xr )

Main Index

(9-55)

CHAPTER 9 629 Boundary Conditions

where x t is the coordinate of the tied node, x r is the coordinate of the reference node, and R ( θ r ) is the rotation matrix of the retained node. The linearized relation between the incremental displacement of a tied node to a retained node and its correction term is expressed as follows: i

i

Δu t = SΔu r + C n o n

(9-56)

where the tying matrix S is derived from the linearized rigid body relation. For linear analysis, C n o n is i

zero. For large displacement analysis, SΔu r may not match the nonlinear constraint exactly. Therefore, an error vector, C n o n , is required to meet the constraint. It is defined as the difference between the expected coordinates ( x t e ), using the rigid body kinematics, and the current coordinates ( x t ) of the tied node. n+i

xt e

n

n+i

= xr + R ( θr

n+i

Cn o n = xt e

0

0

) ( xt – xr )

(9-57)

n+i

– xt

where n is increment number, i is iteration number, and zero is the original value. In order to reduce linearization errors, an optional recycling feature is offered through the CONTROL model and history definition options. Recycling occurs if the maximum iterative rotation change over the retained nodes of the RBE2 exceeds a rotation tolerance (default is 0.001 radians). This check can be bypassed by setting the rigid link rotation to zero (in conjunction with the FEATURE,5701 parameter) or a negative number. When the rotation is finite, then the coordinate system attached to the tied node will be co-rotated according to the rotation of the retained node. The degrees of freedom of the tied node will be assigned with this co-rotated system. As an illustration, consider a slider link shown in Figure 9-47. In this case, a local transformation must be defined for the tied node in which the x-direction is coincident with the line connecting the tied and the retained node. Then, an RBE2 is defined where y-translational degree of freedom is tied but not the x-translational and any of the rotation degrees of freedom. .

y

x y

Y

RB

X Figure 9-47

E2

(a) Increment i

2 RBE

x

(b) Increment i + 1

Co-rotated Coordinate System at the Tied Node

As another example of the use of RBE2 options, consider Figure 9-48 where a cylindrical tube is shown. The tube is clamped at one end and loaded by a torque at the other end.

Main Index

630 Marc Volume A: Theory and User Information

If it is assumed that the loaded end remains circular with a constant radius, then a single RBE2 option can be easily used instead of a number of tyings of type 80. With the RBE2 option, node 1 is defined as the retained or reference node and nodes 2 to 13 are defined as the tied nodes, with all the degrees of freedom constrained. However, if the tube is allowed to expand in radial direction, then tying type 80 cannot be used. However, RBE2 option can still be used, but now the radial displacement is not included in the list of degrees of

freedom to be constrained. 2 13 12

3

θ

11 Mz

Z

1

10

4 5

R

6

9

Clamped end

7 8 Figure 9-48 RBE2 Example: Cylindrical Tube loaded in Torsion

RBE3 The RBE3 option is a powerful tool to distribute applied loads and massed in a finite element model. Forces and moments applied to reference or tied node are distributed to a set of independent degrees of freedom based on the RBE3 geometry and local weight factors. The way in which the forces are distributed is analogous to the classical bolt pattern analysis. Consider the bolt pattern shown in Figure 9-49 with a force F A and moment M A acting at reference point A. The force and moment can be transferred directly to the weighted center of gravity along with the moment produced by the force offset e . FA

FA Reference point A MA

CG e

MCG = MA + FAe

Figure 9-49 Transfer of Force and Moment on a Reference Point to the Weighted Center of Gravity (CG)

The force is distributed on the bolts proportional to their weighting factors. The moment is distributed as forces proportional to the product of their distance from the center of gravity with corresponding weighting factors, as shown in Figure 9-50. The total force acting on the bolts is equal to the sum of the two forces. These results apply to both in-plane and out-of-plane loadings.

Main Index

CHAPTER 9 631 Boundary Conditions

Fi

Force Distribution: ⎛ ωi ⎞ F i = F A ⎜ -------------⎟ ⎝ ∑ ω k⎠

Moment Distribution:

Fi ri

⎛ M C G ω i r i⎞ F i = ⎜ -----------------------⎟ ⎝ ∑ ω k r 2k ⎠ where

F i = force at DOF i ω i = weighting factor for DOF i r i = radius from the weighted center of gravity to point i

Figure 9-50 RBE3 Force and Moment Distribution

As an example, consider the cantilever plate model with a single quadrilateral shell element shown in Figure 9-51. The plate is subjected to nonuniform pressure represented by a resultant force acting at a distance of 10 mm from the center of gravity. The easiest way to apply the pressure is to use an RBE3 option, with a reference node 5, to distribute the resultant load to each of the four corner points. Setting the weighting factors to be equal for all nodes, results in a force distribution based exclusively on the spatial location of the connected nodes. In this way, nodes 3 and 4 will get 3N each and nodes 1 and 2 will get 2N each. 10N 2 m

3 100 m

5

1 4

50 mm

40 mm 100 m m

Figure 9-51 Using the RBE3 Option to Represent a Nonuniform Pressure Load

The formulation of the RBE3 is based on the idea that the motion at a reference node is the weighted average of the so-called error terms of the generalized displacements at a set of connected nodes. The error terms x e l , and θ e l are defined as follows:

Main Index

632 Marc Volume A: Theory and User Information

xl = R ( θt ) ( xl – xt ) + xe l

(9-58)

θl = θt + θe l

where x l and θ l are the coordinates and rotations of the l-th retained node, respectively; x t and θ t are the coordinates and rotations of the reference node, respectively; R is a rotation matrix of the reference node. The error measure for translational and rotation degrees of freedom are weighted with weighting factors, W l . N

et r a n =

T

∑

xe l Wl xe l

l = 1 N

e ro t =

(9-59) T

∑

θe l Wl θ e l

l = 1

The final nonlinear constraint relation is derived by minimizing the error terms with regard to the reference node coordinates and rotations using least square fit. The linearized relation between the reference node and the connected nodes and its correction term can be expressed as: i

i

Δu t = SΔu r + C n o n

(9-60)

with C n o n being zero for linear analyses. For large rotation analysis, the error vector, C n o n , is required rot

to meet the constraint. The rotational error, C n o n , is assumed to be zero. In other words, the expected incremental rotation of the reference node is the same with the current value. t ra n

The translational error, C n o n , is derived by evaluating the difference between the expected coordinate ( x t e ) of the reference node with the current one ( x t ). The expected coordinates are calculated by introducing the coordinates of the connected nodes at the previous increment and the incremental rotation of the reference node into the nonlinear constraint equations.

xt e

⎛ N ⎞ = ⎜ ∑ W l⎟ ⎜ ⎟ ⎝l = 1 ⎠

–1 N

∑

W l ( x l + R l ( Δθ t ) )

l = 1

(9-61)

tran

C n o n = xt e – xt

Beam - Shell Offsets In many problems, it is convenient and sometimes necessary to model beam and shell elements at a geometric location that does not match the actual physical location. Such cases are common when flanges or surfaces for shell and beam elements with varying cross-section properties have to be aligned. Another

Main Index

CHAPTER 9 633 Boundary Conditions

common instance is when beams are used as stiffeners for shells. It is most convenient to model the beam elements by sharing the shell nodes at the midsurface of the shell, as shown in part (a) of Figure 9-52. The fact that the beam is actually offset by half the plate thickness and half the height of the beam section will have to be achieved by providing a suitable beam offset as shown in part (b) of Figure 9-52.

(a) Geometric model with the beam element sharing the nodes of the shell elements.

(b) Physical model with the beam offset by half-shell thickness + half-beam height.

Figure 9-52 Beam-stiffened Shell Structure

There are two methods by which beam/shell offsets can be modeled: The first method is to place the beams and shells at the actual offset position and then tie the nodes of these elements back to the original position through manually defined RBE2 links. While this method is accurate, it is difficult to used for large models. Furthermore, it is not possible for the offset elements to contact other bodies since the nodes of the offset elements are already tied. The second method involves the beam/shell offset capability in Marc. The elements are specified at the original position in the model and the offset vectors at the nodes of the element are specified in a variety of ways through the GEOMETRY option. The current nodal offset is applied to each node of the offset element to calculate the offset element position. 0

n+i

x o f f se t = x + voff

n+i

(9-62) n+i

where n is the increment number, i is the iteration number, x o f f se t is the current coordinate 0

vector of the node at the offset position, x is the original user-specified coordinate vector of the node at the original position, and voff

n+i

is the current offset vector. For small displacement 0

analysis, the initial user-specified offset vector, voff , is maintained through the analysis. For large displacement analysis, the offset vector is rotated based upon the rotations at the node. voff

n+i

= R(θ n+i

n+i

)voff

0

(9-63) n+i

where R ( θ is the current rotation vector ) is the current rotation matrix at the node and θ at the node. The tying relationship between the offset nodal position and the original nodal position is then established. The basic formulation for this tying relationship is similar to the RBE2 link described in the previous section.The relation between the incremental displacement of the node

Main Index

634 Marc Volume A: Theory and User Information

in the offset position to the corresponding displacement at the original position is expressed as follows: Δu oi f f se t = SΔu oi r i g i n a l + C n o n

(9-64)

where the tying matrix S is based on a linearized rigid body relation and its terms are derived from offset vector components. For linear analysis, C n o n is zero. For large displacement i

analysis, SΔu r may not match the nonlinear constraint exactly. Therefore, an error vector, C n o n , is required to meet the constraint. It is defined in a manner similar to Equation (9-57). In order to reduce linearization errors, an optional recycling feature is offered through the CONTROL model and history definition options. Recycling occurs if the maximum iterative

rotation change over the offsets nodes exceeds a rotation tolerance (default is 0.0001 radians). This check can be by passed by setting the rigid link rotation tolerance to zero (in conjunction with the FEATURE,5701 parameter) or a negative number. The element stiffness matrix is formed on the offset element geometry. It is then converted to the original element geometry through a suitable tying relationship. T

Ko r i g i n a l = S Ko f f s e t S

(9-65)

All distributed loads on the offset element are also treated in the same way. Note that point load vectors are not offset and are always calculated at the original nodal positions. The nodal displacements at the original positions are calculated during the solution phase. Finally, during the recovery phase, the displacements at the offset position are calculated from Equation (9-64) and element strains, stresses are calculated on the offset element geometry. Additional details for beam/shell offsets in Marc are provided below: Offset Vector Specification For beams, offset nodal vectors can be specified in four different ways: 1. Offset nodal vector specified in the global coordinate system. 2. Offset nodal vector specified in the local beam coordinate system: For 2-D beams (element types 5, 45), the x-axis is along the beam axis, the z-axis is (0,0,1) and the y axis is perpendicular to both. For 3-D beams, the z-axis is along the beam, the x-axis is user-specified and the y-axis is perpendicular to both. This option is not available for heat transfer links. 3. Offset nodal vector along the associated shell normal: This option is particularly useful when beams are used as stiffeners for shells. In the case, only the offset magnitude is provided by the user. The associated shell normal vector at the node is automatically calculated and is used for defining the offset vector. This option is not available for 2-D beams. 4. Offset nodal vector specified in the local coordinate system at the node:

Main Index

CHAPTER 9 635 Boundary Conditions

The local coordinates at the node can be specified using the TRANSFORMATION, CYLINDRICAL, or similar options. For shells, the offset magnitude is provided by the user and the element normal calculated at the centroid of the shell element is used to define the nodal offset vector. Supported Elements Beam/Shell offset support is provided for all standard beam and shell elements with global translational and rotational degrees of freedom at the corner nodes. Supported mechanical beam elements include element types 5, 14, 25, 45, 52, 76, 77, 78, 79, 98. Heat transfer links, element type 36, 65, 99, and 100 are also supported (see section on field analysis below). Non-standard beam elements that are not supported include element types 13, 16, 51. Supported mechanical shell elements include element types 1, 22, 75, 89, 138, 139, 140. Heat transfer shell elements, element types 50, 85, 86, 87, 88 are also supported (see section on field analysis below). Nonstandard shell elements that are not supported include elements types 4, 8, 15, 24, 49, 72. For higher order beam/shell elements (element types 45, 22, 89), there is a choice to use interpolated values of the corner node offset vectors at the midside nodes. If this is not chosen, the offset is taken as 0 at the mid-side nodes. For beam elements 76, 77, where the midside node degree of freedom is not compatible with the corner node degree of freedom, only the nodal position is updated for the offset and no other tying is undertaken at the midside node. Post File All nodal vectors on the post file are calculated and depicted at the original nodal positions. This allows visual compatibility when elements with offsets and elements without offsets are in the model. Element quantities like strains and stresses on the post file are calculated based on the offset element geometries. Adaptive Meshing There is no support for global remeshing with beam/shell offsets. Local adaptive meshing is supported. Nodal offsets are automatically interpolated and transferred over to the new nodes created during the adaptive meshing process. Field Analysis Beam/shell offsets are predominantly supported for mechanical analysis. Since offset elements can also be used in thermo-mechanical analysis and other field analyses, offset support is extended for field analyses other than purely mechanical analysis. In this case, only the coordinates of the element are adjusted for the offsets, as per Equation (9-62). No other tying of the field variables or element matrices is undertaken. Contact The average nodal offset vector is calculated at every node of all beam/shell contact bodies. All touching nodes and touched patches are then updated using the average nodal offset vectors.

Main Index

636 Marc Volume A: Theory and User Information

Dynamics The stiffness matrix, mass matrix and damping matrix for the offset element are all calculated in a manner similar to Equation (9-65). Implicit in this calculation is the assumption that the displacements as well as velocities and accelerations between the original and offset positions are tied in a manner similar to Equation (9-64).

Pin Code for Beam Elements Pin code is used to remove connections between the node and selected degrees of freedom of the beam. It can only be applied on the nodes at the ends of the beam. It is not allowed to use it for the middle node of 3-noded beams. The degrees of freedom are defined in the element’s coordinate system (see Marc Volume B: Element Library for more detail description how the local coordinate system of beam element is set up), and the pin code is applied at the offset ends of the beam. Marc manipulates the pin code in two different ways. The first one, by default, is done by internally generating a new node which is tied to the flagged node. The tied degrees of freedom are the negation of the pinned ones. The tying process is carried out at element level. The element stiffness matrix and internal forces of the element are calculated using a standard procedure. During the assembly process they are “expanded” to include the degrees of freedom of the new internally generated node. This procedure works fine both for quasi static and dynamics analysis. The second one, using FEATURE, 6901, is done by using the so-called static condensation technique. In this way, no internal node is generated. The pinned degrees of freedoms are condensed out from the element stiffness and internal forces before they are assembled into the global system. This feature is added to allow Marc pin code fully compatible with Nastran implementation. For quasi-static analysis, both ways give exactly the same behavior. For dynamics analysis, the coefficients used to condensed out the element stiffness matrix is reused for mass matrix. This is an approximation to the correct procedure where the static condensation has to be done on the element operator matrix before being assembled into global system. The pin code is activated using PIN CODE or the GEOMETRY option. For postprocessing purposes, the element connectivity is always presented with the original nodes. For example, in a stress-free large displacement analysis for a beam element with pin code that simulate slider, the beam length will become shorter or longer although the element is stress free (see Figure 9-53; node 4 is generated internally. If FEATURE, 6901 is activated, node 4 is not generated). The pin code is defined on element 10 at node 2. The axial-displacement and out-of-plane rotation degrees of freedom are flagged. 2 2 10

4

20 10 1

1 3

Figure 9-53 Slider Connection using Pin Code

Main Index

20 3

CHAPTER 9 637 Boundary Conditions

Mesh Independent Connection Methods In Marc, there are various ways to model connections between structural components in a finite element model. These connections may represent spot welds, seam welds, bolts, screws, rivets, and so on. Depending on the modeling goals, they can be modeled using line elements (like trusses and beams), linear or nonlinear springs, rigid body connections (RBE2, RBE3), and tyings or servo links (MPC constraints). In this way, general connections can be made between parts, but they often require a lot of modeling effort in defining the connections or in assuring that meshes of the parts involved are congruent so that they match in those points where connections are desired. Data and input preparation for these connections can be a formidable task in real-world applications. Often, it is desired to model certain stiffness characteristics in the connections. An easy way to establish this is by making point-to-point connections between the parts and using beam elements or springs as the connector elements. Apart from the high meshing effort, this modeling technique may also produce poor results. Increasing mesh refinement can introduce stiffness errors; point-to-point connections in which the effective crosssectional areas are larger than 20% of the characteristic element face areas can often lead to significant underestimation of connector stiffness. Point-to-point connections can also cause numerical problems in finite element shell models. The stiffness of the rotations normal to the shell plane may not exist or may be represented by a penalty stiffness to suppress the associated singularity, but in the point-to-point connections, such rotations may be excited. If the surface of one of the parts is defined by the faces of continuum elements, there are no rotational degrees of freedom for the nodes of these elements and point-to-point connections may introduce undesired singularities. The CWELD and CFAST connection methods that are available in Nastran have also been implemented in Marc to address and solve the aforementioned modeling issues. Connections can now be established with ease between points, elements, patches, or any of their combinations and load transfer between the parts can be established over multiple nodes on each side of a connection providing a more accurate stiffness representation of the connection. The following connections between two parts can be made: patch-to-patch, point-to-patch and point-to-point as illustrated in Figure 9-54. n

Patch-to-patch Connection For noncongruent meshes, area wise connection

Point-to-patch Connection For noncongruent meshes, point to area wise connection

Point-to-point Connection For nearly congruent meshes, point wise connection

Figure 9-54 Supported Connections Between Different Parts

Each connection involves the two end nodes of a connector element and two surfaces that are to be connected at a certain location. The connector element can be any Marc beam element, a truss element or a cbush element. The surfaces can be defined by shell elements, the faces of continuum elements or by nodal points. These surface element faces are referred to as patches, can be triangular or quadrilateral, and may be linear or quadratic. On each side of the connection, either a patch connection or a point

Main Index

638 Marc Volume A: Theory and User Information

connection is made thus giving the three connections shown in Figure 9-54. A patch-to-patch connection can be shell-to-shell, shell-to-solid, or solid-to-solid. A point-to-patch connection can be point-to-shell or point-to-solid. A point connection is the simplest connection since the end node of the connector element is directly connected to a node of the surface; the connector element and the surface share a common node and no additional constraints are required to establish the connection. A patch connection connects the end node of a connector element to one or more element faces and is more general as it eliminates the need of congruent meshes. The location where the end node pierces the surface is automatically determined. The element face being pierced is called the master patch. Internal constraints are generated to assure a rigid (i.e., a force and moment carrying) connection of the connector end node to the surface. Two types of patch connections can be made: Direct Patch Connection which connects the connector end node directly to the nodes of the master patch with tying type 44; the constraints involved in this tying are also known as Kirchhoff constraints, (see Rigid Tying to a Surface Patch in this chapter) or the Indirect Patch Connection which connects the connector end node indirectly to the nodes of the surface by constructing a four-node auxiliary patch at the end node normal to the connector. The size of this auxiliary patch is determined from the diameter or area of the connector. The end node of the connector makes a rigid (tying type 44) connection to this auxiliary patch. The four nodes of this auxiliary patch (the auxiliary nodes) are connected to the surface by additional constraints. The location where each auxiliary node pierces the surface is automatically determined. The patch being pierced is called the secondary patch. By default, RBE3 constraints are generated between each auxiliary node and the nodes of the secondary patch it pierces, but other constraints may be chosen as well. Note that, depending on the mesh density, two or more auxiliary nodes may connect to the same secondary patch. All piercing points are determined by normal projections to the surface to which the connection is made. The two patch connection types are illustrated in Figure 9-55 which displays a top view of one side of the connection involving regular four-node quadrilateral element faces. Other element face types and element faces with collapsed edges may be present as well. All constraints are applied internally as tying constraints and they are automatically generated when processing the input.

master patch auxiliary patch master patch secondary patch

Direct Patch Connection

Indirect Patch Connection

Figure 9-55 Patch Connection Types

The direct patch connection is the simpler type, but may lead to asymmetrical load transfer between the surfaces when the projections are near the element face boundaries and the element faces are not nicely facing each other. It may also lead to a very localized load transfer in case of fine meshes, resulting again

Main Index

CHAPTER 9 639 Boundary Conditions

in a poor stiffness representation of the connection. The indirect patch connection improves the load transfer by incorporating more element faces, and thus more nodes, in the connection, but this will also lead to more constraint equations. In general, a connection between two surfaces can be defined by entering a point that identifies the approximate location of the connection and the two surfaces that are to be connected. This point can be entered by referencing a node or by entering its coordinates when defining the connection and it is referred to as the GS-node or GS-point. These GS reference points determine the spacing of the connections and they can be defined beforehand, independently of the surface meshes. The surfaces can be identified by entering the element faces to which the connection will be made or by entering element or face sets from which the element faces to connect to will be sought. For indirect patch connections, only the master patches need to be entered. The secondary patches are automatically found in the vicinity of the master patches. If the surfaces are entered as sets, the master patches and the secondary patches are searched from these sets. The connection between the two surfaces is established as follows. The GS-node is projected to the first (side A) and second (side B) surface by a normal projection. These two projections determine the end nodes of the connector and therefore its final position and are referred to as the GA-node for side A and the GB-node for side B. The nodes on side A and B of the master patches are referred to as GAi and GBi respectively, where i ranges from one to the number of nodes in the patch. The auxiliary nodes are referred to as GAHi and GBHi respectively, where i always ranges from one to four. The nodes of a secondary patch are referred to as GAij and GBij respectively, where j ranges from one to the number of nodes in the patch and i refers to the ith auxiliary node. The definitions of the connection are made on the CWELD or CFAST model definition options. The properties of the connector elements are defined on the PWELD or PFAST model definition options. These properties are material and geometric properties in case of CWELD connections and stiffness properties in case of CFAST connections. A number of control parameters can be entered on the SWLDPRM option to enhance the search and projection process and to control its output.

CWELD patch-to-patch connections There are several methods to define CWELD patch-to-patch connections. The methods available are ELEMID, GRIDID, ELPAT, and PARTPAT. In each of these methods, the surfaces on both sides have to be defined together with the GS reference point of the connection. The ELEMID and GRIDID methods make the simpler direct patch connections and the ELPAT and PARTPAT methods make the more advanced indirect patch connections. All methods can be used to connect noncongruent meshes of any type and they are recommended when the cross-sectional area of the connector is larger than 20% of the characteristic element face area. The connector element can be any Marc beam element. The default type used is 98 which is a straight beam in space that includes transverse shear effects. By default, it assumes elastic behavior and a solid circular cross-section. It is always required to include the ELEMENTS parameter for each element type used as a connector, even when it does not appear in the CONNECTIVITY input. The data for each connection are defined on the CWELD model definition input. Some data inputs are always required, because no defaults exist for them. Other data inputs are optional and if not defined, Marc assumes appropriate default values for them. These optional data inputs concern the connector element type, the way the projections are carried out, the type of constraints and the orientations of specific CWELD connections.

Main Index

640 Marc Volume A: Theory and User Information

Direct Patch-to-patch Connections The ELEMID and GRIDID methods define the connection directly between two master patches. For ELEMID the patches are entered as shell elements or the faces of continuum elements (SHIDA and SHIDB). For GRIDID, the patches are entered as nodes (GAi and GBi) following the same connectivity conventions as for corresponding shell patches. The two methods are illustrated in Figure 9-56. The GS-node is projected to both patches and, in case it is already positioned between the two patches, these projections determine the connector end node locations. But it is not a requirement to position the GS-node between the two patches, and if it is not, the projection is done in two steps as illustrated in Figure 9-57. First, a normal projection to patch A and patch B is made resulting in the points GA’ and GB’. Then the midpoint GC’ between these two points is projected to both patches and this determines the connector end point locations GA and GB. The nodal coordinates of the connector element are updated after this projection. The GS-node must have a proper projection to the patch within its boundaries. The PROJTOL parameter can be defined to accept projections outside but near patch boundaries. GS

GS SHIDA

GA4

GB3

SHIDA GA3

GA1

GA2

SHIDB GB1 GRIDID

ELEMID Figure 9-56 ELEMID and GRIDID Connection Methods GS

GS PIDB

Shel lB

GB′

GB SHIDB

L

GB

PIDA

D

SHIDA

A Shell

Figure 9-57 Determination of the Connector End Node Locations GA and GB

Main Index

GC

GC′

GA

GA

GA′

GB2

CHAPTER 9 641 Boundary Conditions

The data needed to define a connection with ELEMID are: 1. The reference node GS or its coordinates (XS,YS,ZS). 2. The patches SHIDA and SHIDB on both sides, where for shell elements these are the element numbers and for continuum elements these are element and face number pairs. 3. A PWID, which is the identification number of a corresponding PWELD property entry. The data needed to define a connection with GRIDID are: 1. The reference node GS or its coordinates (XS,YS,ZS). 2. The patch nodes GAi and GBi on both sides. The number of nodes determines the patch type, which can be quad4, quad8, tria3 or tria6. No mixed patches with partly linear and partly quadratic edges are supported. 3. A PWID, which is the identification number of a corresponding PWELD property entry. Indirect Patch-to-patch Connections The ELPAT and PARTPAT methods make the connection of the connector end nodes to the surfaces involved in two phases, as illustrated in Figure 9-58 and Figure 9-59. First the reference GS-node is projected to a master patch. For the ELPAT method, the master patches are specified in the input. For the PARTPAT method, the master patches are searched from sets that have been specified in the input. Around each projection point, a square four-node auxiliary patch is constructed. This auxiliary patch is normal to the line connecting the two projection points. The dimensions of this auxiliary patch follow from the diameter or the area of the connector as displayed in the right part of Figure 9-58. For the four auxiliary nodes, new projections are computed on the master patches or on patches in their vicinity. The patches to which these new projections are found are called secondary patches and each auxiliary node is connected by default with RBE3 constraints to the nodes of its respective secondary patch.

GBH4

GBi GBH3

GB

D/2

D/2

Shell B

GAH3

GAH4

GBH1 GBH2

a GA

a =

GAH4

a GAH1

GAH3

GA

GAH1 GAH2 Shell A

Figure 9-58 ELPAT or PARTPAT Connections

Main Index

GAi a

a

GAH2

D π ---4

642 Marc Volume A: Theory and User Information

The master patches and the secondary patches do not have to be distinct as can be seen from Figure 9-58 and Figure 9-59. For a coarse mesh, they may even be one and the same patch but for fine meshes they may all be distinct. The requirement is that the secondary patches do not span a larger area of the mesh than a 3 x 3 area as shown in the right part of Figure 9-59 otherwise a number of nodes not involved in the constraints defining the connection is present under the area covered by the auxiliary patch. If the NREDIA parameter is set and the secondary patches violate the 3 x 3 requirement, the auxiliary patch size is reduced a number of times in an attempt to fulfill this requirement. GAij

GAH4

GAH3

GAij

GAH3

GAH4

GA

GAH1

Coarse Mesh

GAH2

GAH2

GAH1 Fine Mesh

Figure 9-59 Connections in Coarse and Fine Meshes for the ELPAT and PARTPAT Methods

The main purpose of the ELPAT and PARTPAT methods is to improve the load transfer between the two surfaces. These methods allow for a more symmetrical load transfer than the simpler ELEMID or GRIDID methods as illustrated in Figure 9-60. On side A in the left part of the figure, the shaded patch is the master patch and the constraints are only applied between the connector node and the nodes of this patch. On side A in the right part of the figure the neighboring patches also become involved in the connection and the load at the connector node is transferred through the four auxiliary nodes to all the nodes of the secondary patches in the surface, leading to a better load transfer. It also avoids a too localized load transfer as may be clear from the right part in Figure 9-59. If this connection were of the ELEMID type, the only patch involved in the load transfer would be the one entirely covered by the shaded area leading to a much more localized load transfer. The PARTPAT method defines a connection between two sets. In case the part is meshed with shell elements, the set can be an element set identifying the elements that make up the surface. In case the part is meshed with continuum elements, the set must be a face set identifying the faces that make up the surface. A shell surface can also be identified by a face set, but the face information is not essential and therefore element sets can be used as well. The ELPAT method is similar to the PARTPAT method. The only difference is that the ELPAT method defines the master patches, whereas the PARTPAT method searches them from a set of elements. A further difference is that for shell meshes the ELPAT method searches its secondary patches from the whole mesh, whereas the PARTPAT method searches them from the same sets from which the master patches were found, but sets may be used to limit the search regions. Sets are only required for the ELPAT method if the surfaces contain faces of continuum elements.

Main Index

CHAPTER 9 643 Boundary Conditions

SHIDB

SHIDB

SHIDA

SHIDA Connected Elements for ELEMID Format

Connected Elements for ELPAT Format

Figure 9-60 Comparison of Load Transfer in the ELEMID and the ELPAT Methods

The data needed to define a connection with PARTPAT are: 1. The reference node GS or its coordinates (XS,YS,ZS). 2. The sets SetA and SetB for both sides, where, for shell elements, these sets may be element sets, and for continuum elements, they must be face sets containing element and face number pairs. The two sets SetA and SetB do not have to be disjoint, but the search procedure is facilitated if they are. 3. A PWID, which is the identification number of a corresponding PWELD property entry. The data needed to define a connection with ELPAT are: 1. The reference node GS or its coordinates (XS,YS,ZS). 2. The patches SHIDA and SHIDB on both sides, where for shell elements these are the element numbers and for continuum elements these are element and face number pairs. 3. The sets SetA and SetB for both sides, where, for shell elements, these sets may be element sets and for continuum elements they must be face sets containing element and face number pairs. The two sets SetA and SetB do not have to be disjoint. For surfaces defined by shell elements, these sets are optional, but for surfaces defined by faces of continuum elements, they must be specified. 4. A PWID, which is the identification number of a corresponding PWELD property entry.

Parameters for the Projection Process When searching master or secondary patches, it may happen that no projection is found at all to any of the candidates because the surface is not flat and the GS-node or an auxiliary node only has a projection outside two neighboring patches as illustrated in the left part of Figure 9-61 or because one or more of the auxiliary nodes lie outside a free edge as illustrated in the right part of Figure 9-61.

Main Index

644 Marc Volume A: Theory and User Information

GS

Free Edge

Figure 9-61 Exceptional Cases needing Special Consideration

In the first case, a projection is accepted to the common edge of the two patches and the nearest patch is selected as the master or secondary patch. In the second case, two parameters may be used to improve the situation. The GSMOVE parameter allows the GS-node to be moved in the direction of the auxiliary nodes that have found successful projections. The NREDIA parameter allows the area of the auxiliary patch to be reduced without moving the GS-node. Both parameters may be used simultaneously. In that case, it is first tried to move the GS-node a number of times and if that is not successful the area is reduced a number of times. If that still fails, it is once more tried to move the GS-node a number of times, now using the reduced area for the auxiliary patch. Successful projections of the auxiliary nodes are counted in pairs. A successful pair means that the two corresponding auxiliary nodes on both sides of the connection have found a successful projection. So in the situation in the right part of Figure 9-61, two pairs of auxiliary nodes are successful and two pairs have failed, because their projections fall over a free edge of one or both of the surfaces. In addition, the PROJTOL parameter may be used to accept projections outside but near patch boundaries. If GSMOVE is nonzero, the new GS location is determined from the successfully projected GAHi and GBHi pairs as follows: • If one pair of GAHi and GBHi finds a successful projection, GS is moved to the middle position between that pair and the original GS. • If two pairs of GAHi and GBHi find a successful projection, GS is moved to the middle position between those two pairs and the original GS. • If three pairs of GAHi and GBHi find a successful projection, GS is moved closer to the second pair found. The move is one quarter of the distance from GS to the second pair. • If no pairs are found at all, moving GS is abandoned. If the number of moves has been exhausted and NREDIA is nonzero, the characteristic diameter of the CWELD connector is halved a number of times reducing the auxiliary patch size, thus bringing its nodes

closer to each other. If one or more pairs still fail after this diameter reduction, a last attempt is made to move the GS node while maintaining the reduced sized of the auxiliary patch. The size of this movement is twice that of the movement before the size reduction which, in general, is still a small movement, because of the reduced auxiliary patch size. This second attempt to move the GS-node is only carried out when NREDIA is nonzero.

Main Index

CHAPTER 9 645 Boundary Conditions

In some occasions, it may happen that a proper projection is found far away from the GS point (e.g., when the surface is curved and the situation displayed in the left part of Figure 9-61 occurs for patches near to the GS point. In that case, the GSTOL parameter may be used to reject projections that are further away than specified by the parameter, so projections will only be accepted that are relatively near to the GS point. It is assumed that the two surfaces that are being connected are reasonably parallel. The GSPROJ parameter may be used to check this explicitly as illustrated in Figure 9-62. If the master patch normal vectors on both sides make an angle larger than specified by the parameter, the projection is rejected. It is also assumed that master patches and associated secondary patches are reasonably parallel. It is not desirable that elements almost normal to the master patch are selected as secondary patches. The GSCURV parameter may be used to reject secondary patches that make a large angle with the master patches as illustrated in Figure 9-62. This may occur in sharp corners of the surface which in practice may represent edges of the structure. The parameters discussed in this section are defined on the SWLDPRM option. GSCURV

nB

GSPROJ GSCURV

nA

nA H 1 nA GAH1

GA

GAH2

Figure 9-62 Angle Parameter GSPROJ and GSCURV to Control the Patch Selection Process

Internal Constraints to Connect Two Surfaces Each connector end node, that is not making a point connection, makes a rigid connection to its master or auxiliary patch by means of a Kirchhoff constraint (tying type 44). This constraint rigidly constrains the displacements and rotations of the end node to the motion of the patch it connects to. The possible patches to which such a connection can be made are linear and quadratic quadrilateral and linear and quadratic triangular patches. With the ELPAT and PARTPAT methods, the auxiliary patch nodes are connected to their partnering secondary patches by additional constraints. By default, these will be RBE3 constraints, but alternatively Kirchhoff constraints may be used or a combination of RBE2 and RBE3 constraints. The RBE2/RBE3 combination makes a RBE2 constraint between the auxiliary patch node and its projection point on the secondary patch and RBE3 constraints between this projection point and the nodes of this patch. When a surface is curved, the auxiliary patch nodes will in general not lie on the surface. A special parameter may be set in the CWELD input to force a repositioning of these nodes onto the surface. This slightly alters the orientation of the auxiliary patch and in some cases this might allow the connector to follow the curvature of the surface somewhat better. By default, this repositioning is not done.

Main Index

646 Marc Volume A: Theory and User Information

For the RBE3 constraints involved in the CWELD connection, a weighting other than uniform weighting can be used by specifying a distance weighting exponent. The weight factor for each retained node in the RBE3 is: 1 f i = -----ndi where f i is the weighting factor for retained node i, d i is the distance from the tied node to retained node i and n is the weighting exponent. Negative values for n are not recommended, since they will result in heavier weighting for nodes further away. The default results in uniform weighting ( f i = 1 ) . The RBE2/RBE3 combination is only useful when the auxiliary nodes are not lying on the secondary patches and when a nonuniform distance weighting is used. It also comes with a cost penalty because it involves more constraint equations in each connection. If the CONNECTIVITY input contains no elements with nodes having displacements and rotations as degrees of freedom, it is necessary to set the RBE parameter.

Multiple Surface Connections The patch-to-patch connection can be used to connect more than two layers of shell elements by using the same GS-node in multiple CWELD definitions. For example, if three layers need to be connected, a second CWELD definition is made, that refers to the same GS-node as the first CWELD definition. Surface B on the first CWELD definition is repeated as surface A in the second CWELD definition. If the surfaces are not curved, the locations of the connector end nodes connecting from the top and bottom side to the surface in the middle automatically coincide, but for curved surfaces, this is not guaranteed. For all connection types except PARTPAT, there is no real difference between repeating the GS-node or defining it a multiple number of times. When the PARTPAT method is used and a set pair is repeated in a number of connections that use the same GS-node (e.g., the same set is used for side A and side B for each of these connections), this repeated usage of the GS-node results in searching through a stack of patches that can be found from the two sets, in order to connect multiple plate surfaces. However, when the set pairs are different, i.e., at least one side in a new connection refers to a set with a name different from the name referred to by this side in a previous connection using the same GS-node, the effect is as in all other connection types. The definition for a search through a stack of surfaces can only be made by repeated usage of a GS-node (i.e., a repetition of its node ID, not just a repetition of its coordinates XS, YS, and ZS) in combination with the same sets for side A and side B for all the connections that must be present in the stack. It only applies to the PARTPAT connection type and in that case the sets necessarily have an overlap, i.e., they are not disjoint. The stack is limited to 10 connections, i.e., 11 plate surfaces.

Coupled Thermo-mechanical Analysis Cweld connections are be used in a coupled thermo-mechanical analysis. In the heat transfer pass of an increment, the Kirchhoff constraints will tie the temperature of the tied node to the temperature of the projection point on its corresponding patch. For RBE3 constraints, the temperature of the tied node will

Main Index

CHAPTER 9 647 Boundary Conditions

be the least squared weighted average of the temperatures of its retained nodes. The same weighting factors apply as in the mechanical pass. If the retained nodes are the nodes of a shell element, all temperature degrees of freedom of the shell node are used in the weighting process. For RBE2 constraints, the temperature of the tied node is set equal to the temperature of its corresponding retained node, so the constraint in the heat pass is identical to typing type 1.

Rules for usage of the GS-node or the GA-, GB-node Pair in the Projection Process In most cases, the GS-node will be used to find the projections determining the end nodes of the connector element. The GS-node and its XS,YS,ZS-coordinates are ignored on a CWELD definition if both the GA and the GB end nodes of the connector are specified. In that case, GA and GB should, at least, be approximately in the right locations and GA is projected to side A and GB is projected to side B of the connection. If GS and GA are not specified, but GB is, then GB is used as GS and 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 XS,YS,ZS coordinates must be specified. If GS is specified and maximally one of the GA or GB, then GS is used for the projections on both sides and the GA or GB is 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 will be made to the GS-node and the GS-node will be projected onto the opposite side to determine the location of the other connector node. If the opposite side also makes a point connection, the node for that side must have been specified. CWELD Point-to-patch Connections It is possible to connect one end of the connector element to the surface by a point connection as is shown in Figure 9-63. This may even be a free node to which certain boundary conditions may be applied. In such cases the surface information that identifies the master patch for the particular side is omitted. This means that for the ELEMID and ELPAT method, the input for SHIDA or SHIDB is omitted, for the GRIDID method, the nodes GAi or GBi are omitted, and for the PARTPAT method, the set SetA or SetB is omitted. The GS-node is projected to the surface on the other side according to the specifications made in the input.

Main Index

648 Marc Volume A: Theory and User Information

n

GS

GA3

GA4 GA

GA1

GA2 Figure 9-63 Point-to-Patch Connection on Side A using GRIDID

CWELD Point-to-point Connections All methods may be used to define point-to-point connections by omitting the surface information that identifies the master patches and by specifying the connector end nodes on the CWELD input. These must be existing nodes in the structure, because they can no longer be generated internally. Using any of the patch connection methods would lead to cumbersome definitions of such point-to-point connections and the ALIGN method was designed to simplify their definition. It is shown in Figure 9-64. The GS-node is no longer required, because the connector end nodes in general will be nodes belonging to the two surfaces. Point-to-point connections are only recommended for nearly congruent mesh, so the connector element will be approximately normal to the surfaces. However, they are not recommended when the connector cross sectional area exceeds 20% of the characteristic element face area. n GA

Upper Shell Midsurface

n GB

Figure 9-64 Point-to-point Connection using ALIGN

Main Index

Lower Shell Midsurface

CHAPTER 9 649 Boundary Conditions

CWELD Properties PWELD Property Definition The properties for the connector element can be entered on the PWELD model definition option. The material properties are defined by entering the material identification number of a valid material for the element. The default cross section is a solid circular section for which the diameter can be entered on the PWELD input. If other geometric properties than those of a circular section are required, a complete set of geometric input data can be entered here as well. In that case, the diameter is only used to determine the size of the auxiliary patches. If no diameter is entered but a set of geometric data is, an attempt is made to estimate the auxiliary patch size from the geometric data. The geometric data input also specifies the local directions of the cross section. If their corresponding data values are all zero, the local directions are determined by the procedure outlined in the Connector Orientation section in this chapter, otherwise the local directions are determined from the geometric data input according to the usual Marc convention. The default length of the connector is given by the distance between the two end points GA and GB. Two control values on this length can be entered to prevent overly stiff or overly flexible behavior of the connector element. Additionally, a spot weld connection type can be selected as an alternative to the default general weld connection type. In both cases, the effective stiffness of the element is changed by making certain length modifications. Their details are discussed later in the Connector Length Modifications and Spot Connections section. Connector Orientation The connector element is positioned between the two projections GA and GB and these points determine the end nodes of the element and thus its direction. The section forces for the default beam type are displayed in Figure 9-65 and the local section directions are determined as follows. The element z-axis points from GA to GB. The first procedure outlined in this section is used when the 4th, 5th, and 6th fields of the appropriate data blocks in the PWELD or GEOMETRY options are all zero and no coordinate system (MCID) is specified in the CWELD option. This procedure is as follows: xB – xA e 3 = ------------------------- is the local z-axis xB – xA In case of zero length, the average normal of the two surfaces is taken. Find the index j of smallest component of e 3 . j

i

e 3 = min { e 3 }

Main Index

i = 1, 2, 3

650 Marc Volume A: Theory and User Information

In case of two equal components, the smaller index i is taken. Define the corresponding base vector as follows: δ1 j bj =

δ 2 j , where δ k j = 1 when k = j and 0 otherwise, e.g. for j = 3 , b 3 = δ3 j

0 0 1

mz fz ze GB

my B fy fx mx B

mx A

plane 2

fx GA

ye plane 1

fy

fz

axial force

fx

shear force plane 1

fy

shear force plane 2

mz

torque

m x A bending moment end A, plane 2 m x B bending moment end B, plane 2 m y B bending moment end A, plane 1 m y A bending moment end B, plane 1

xe

my A fz

mz Figure 9-65 Connector Orientation, Local Cross-section Directions and Forces

It provides a good directional choice for e 1 . In addition, the vector e 1 must be orthogonal to e 3 . e˜ 1 e˜ 1 = b j – ( e 3 ⋅ b j )e 3 and e˜ 1 = ----------- is the local x-axis e˜ 1 The cross product of local z and local x provides the local y-axis e2 = e3 × e1 The second procedure outlined in this section is used when the 4th, 5th, and 6th fields of the appropriate data blocks in the PWELD or GEOMETRY options are all zero, but a coordinate system (MCID) is specified in the CWELD option. In that case the local directions are determined by a procedure that uses a coordinate system defined in the COORD SYSTEM option. This procedure is as follows:

Main Index

CHAPTER 9 651 Boundary Conditions

xB – xA e 3 = ------------------------- is again the local z-axis. xB – xA In case of zero length, the average normal of the two surfaces is taken. The 2nd direction (T2) defined by MCID is used to define the orientation vector v of the connector element. The local y-axis is then defined as e3 × v e 2 = --------------------e3 × v The cross product of local y and local z provides the local x-axis e1 = e2 × e3 If any of the 4th, 5th, or 6th fields of the appropriate data blocks in the PWELD or GEOMETRY options is nonzero, the conventional Marc procedure is used to determine the local element directions, irrespective of the presence of a MCID input in the CWELD option. A coordinate system may be associated with the first beam node (GA), but offsets are not possible and are ignored. An angle α may be specified for each connector element, which rotates the local axes about the line connecting the two end points. This rotation takes effect after the orientation has been found by either one of the procedures outlined above or by the geometric specifications made in the PWELD or GEOMETRY options. Connector Length Modifications and Spot Connections In the default general connection, the distance between the points GA and GB determines the length of the connector element. To prevent the connector element from overly stiff or overly flexible behavior two tolerance values, LDMIN and LDMAX can be entered on the PWELD input. LDMIN and LDMAX are the minimum and maximum length to diameter ratio of the connection. If the length to diameter ratio is less than LDMIN, the behavior of the connection may become overly stiff and if it is more than LDMAX, it may become overly flexible. In either case, a length modification of the CWELD is made such that its behavior remains within the two limits. There are three methods available to account for this length modification. The first method is stiffness scaling. For linear elastic material behavior, the length modification could be accounted for by scaling the Young’s modulus such that the axial, shear, and torsional stiffness of the beam with its actual length (i.e., the length determined by the distance between its end nodes) is identical to the axial, shear, and torsional stiffness of a beam with the modified length using the original Young’s modulus. This scaling can only be done when the beam material behavior is linear elastic and the crosssection properties are not entered through the BEAM SECT parameter. Internally, the cross-section geometric properties of the beam are scaled and not the Young’s modulus. The second method is repositioning of the end nodes of the beam. Each beam node is moved in a direction normal to its patch such that the beam obtains the desired length. The distance to the patch is treated as an offset in the Kirchhoff constraints. If there is a point connection on one side, then that node is not repositioned.

Main Index

652 Marc Volume A: Theory and User Information

The third method is repositioning of the end nodes and the auxiliary nodes. For methods ELPAT and PARTPAT, the auxiliary nodes can be repositioned together with the beam nodes such that the beam obtains the desired length. This requires updating the projections of the auxiliary nodes which may fail if these nodes become located far away from their respective surfaces and these surfaces are curved. In that case, they may no longer have a projection inside any of the element face boundaries. If the element and its material behavior allow it, the default method is the first method, stiffness scaling, otherwise, no length modification is made. The length modification method can be activated by defining the CWSPOT parameter on the SWLDPRM option. If a CWELD has a point connection on both sides (like in ALIGN) or the distance between the two end nodes of the beam is zero, no length modification will be made. Alternatively, a spot weld connection can be defined. In this case, the length of the connecting beam is modified to be 0.5∗ ( t A + t B ) where t A is the patch shell thickness on side A and t B is the patch shell thickness on side B. If the surface on one side is defined by the faces of a solid element, its thickness contribution is zero. If both sides are faces of solid elements, the connection type is automatically reset to a general connection. The type of connection, general connection or spot connection, can be selected on the PWELD input. Spot connections are only possible when one of the methods ELEMID, ELPAT, or PARTPAT is used. If the distance between the connector end nodes GA and GB is zero, the two nodes will be connected rigidly using tying type 100 and no beam element is activate in the connection. If stiffness scaling is requested as the length modification method and the material is nonlinear or the cross section properties are entered through the BEAM SECT parameter, the scaling is not done and a warning message is written to the output.

CWELD Input Styles For CWELD connections, two different input styles can be used to define the connections and these styles may be mixed in one model. The first style is the most natural style, where only the GS-node and the two surfaces are defined in the CWELD input. This style was used in the foregoing discussion. The beam connector elements and its nodes are generated internally and are not present in the CONNECTIVITY and COORDINATES inputs. All necessary geometric properties of the connection are defined in the PWELD input and its material properties are defined by entering a valid material identification number in the PWELD input. With the second style, the connector elements are entered explicitly in the CONNECTIVITY option and their nodes in the COORDINATES option. The connector nodes do not have to be in the right location as long as the GS-node is in the approximate location. The material properties of the connectors may then be entered through the usual material options and their cross-section properties through the GEOMETRY option. All these properties are assigned to the elements directly. The CWELD option still defines the connection, but only refers to the connector elements and a PWELD input is generally no longer required. The second style requires that the CWELD input is made before the CONNECTIVITY input of the element. However, it is not required to rigidly adhere to the input styles mentioned above. A connector element with its ID, type, and nodes may be defined entirely on the CWELD option. If no element ID is specified,

Main Index

CHAPTER 9 653 Boundary Conditions

Marc generates it internally. If no node IDs are specified, Marc generates them internally. It no type is specified, type 98 is chosen for a 3-D analysis and type 5 for a 2-D analysis. If the CONNECTIVITY for an element is entered after its CWELD input, the CONNECTIVITY input determines the element type and the nodes of the element. If the CWELD input for an element is entered after its CONNECTIVITY input, the CWELD input determines the element type and nodes of the element. If the CWELD input specifies the element ID, a CONNECTIVITY input for the element is not required. It is optional and can be used to redefine the nodes if these were left undefined in the CWELD input. If the connector element is only defined through the CWELD input, it is necessary to enter an ELEMENTS parameter for the type of the connector element as it is necessary to enter an ELEMENTS parameter for each element type that is used in the CONNECTIVITY input. If a side of a connection makes a point connection, the node to which this connection is made cannot be an automatically generated node. It must be a node defined by the user in the input. The user has no control over automatically generated nodes; i.e., how their ID’s are assigned to them. Therefore, it is not possible to load or constrain such nodes or to connect them to other parts of the model.

CWELD Error and Warning Messages A number of error and warning messages can be written to the output file for any of the connector end nodes or the auxiliary nodes. Error messages obtain a positive code and terminate the job with exit number 13. Warning messages obtain a negative code and allow the job to continue. The possible messages are listed in Table 9-27. Table 9-27

Value

Description

1

Projection algorithm did not converge within desired tolerance.

2

Projection converged, but not inside the patch boundary.

-2

Projection converged, but near the patch boundary (inside: 0.01, outside: PROJTOL).

3

The patch is severely distorted or inside out (normal vectors in different locations make larger than 90° angles).

-3 4 -4 5 -5

6

Main Index

Codes for CWELD Error and Warning Messages

The patch is OK, but still has much distortion (normals in different locations make larger than 10° angles). The angle of an element/face normal to its auxiliary or master patch normal is too large; the patches are almost normal to each other. The angle of an element/face normal to its auxiliary or master patch normal is rather large. GS projects OK, but is located too far away from the projection. GS or an auxiliary node projects OK, but is located far away from the projection. For GS nodes we use GSTOL as the tolerance. For auxiliary nodes, we use XDIM (characteristic cweld dimension) as the tolerance. XDIM = 1 ⁄ 4πD , where D is characteristic cweld diameter. The element we want to project to is unknown (i.e., useless, because element type = 0).

654 Marc Volume A: Theory and User Information

Table 9-27

Value -6

Codes for CWELD Error and Warning Messages (continued)

Description A projecting is being made to a deactivated element, but accepted anyway.

7

The beam is almost parallel to the patch. (its angle with the patch is less than GSPROJ)

-7

The beam is not very normal to the patch (it makes an angle larger than 2*GSPROJ to the patch normal).

8

The patches to which the auxiliary nodes tie are more than 3 x 3.

9

The patch nodes have invalid degrees of freedom.

10

The patch has an invalid number of retained nodes.

11

A search over a group of patches resulted in no success at all; no projection has been even attempted to any of the patches.

12

A search over a group of patches resulted in no success at all; although projections were tried, they were all unsuccessful.

13

The projection is outside the patch boundary and there are no neighbors; so, there is no positioning to a common edge or a common corner.

-14/14

Warning/Error: Position the cweld node to corner 1 of patch.

-15/15

Warning/Error: Position the cweld node to corner 2 of patch.

-16/16

Warning/Error: Position the cweld node to corner 3 of patch.

-17/17

Warning/Error: Position the cweld node to corner 4 of patch.

-18/18

Warning/Error: Position the cweld node to edge 1-2 of patch.

-19/19

Warning/Error: Position the cweld node to edge 2-3 of patch.

-20/20

Warning/Error: Position the cweld node to edge 3-4 (quad) or 3-1 (tria) of patch.

-21/21

Warning/Error: Position the cweld node to edge 4-1 of patch.

22

No face id was specified for the continuum element.

24

No viable patches in the set (PARTPAT, ELPAT).

26

No viable elements in the whole model (PARTPAT, ELPAT).

-27 28

To account for a length modification, the beam node on this side of the patch has been offset with regard to the patch it is connecting with. The beam node is shared with other elements, while not making a point connection. Or the GS-node is shared with elements on the side that makes a point connection.

-28

Main Index

The GS-node is shared with other elements.

29

The face ID identifying a patch is missing for a continuum element.

30

The connector node cannot connect to this element because it is not a valid connection type.

32

In 3-D, a connection to a line type of element was attempted; this is not possible.

CHAPTER 9 655 Boundary Conditions

Table 9-27

Codes for CWELD Error and Warning Messages (continued)

Value -33/33

Description The connector node made a point connection but is not connected to any other element than the connector element. If this node is an automatically generated node, the result is an error; otherwise, a warning.

34

The projection is to an element/face sharing the point connection node.

35

An element/face of another connection lies between the current element/face pair.

CWELD Output A CWELD connection defines a beam element as the connector element and generates internal tyings to define the connector constraints. Output to the .t16 or .t19 post file can be requested for the beam elements by using the standard element post codes available for them. Tying forces can be requested by using the standard nodal post codes available for them. The displacements of all nodes involved in the connection will by default be on the post file. Four sets are automatically generated and available on the post file when the CWSETS parameter on the SWLDPRM option is set to one. The first set contains all the beam elements used in the connections. The second and third sets contain all patches defining side A and side B of all connections, respectively. The fourth set contains all elements that have caused warnings. An error set is not available because, upon encountering an error, no attempt is made to complete a connection. This means that, in case of an error, the information at best is incomplete, but because of its intermediate character it may often be misleading and often it is not yet available at all. The sets are called: Set 1: fastener_all_beams_inc0000 Set 2: fastener_all_faces_sidea_inc0000 Set 3: fastener_all_faces_sideb_inc0000 Set 4: fastener_all_warnings_inc0000 Set definitions defining sets with any of these names should not be made in the input. The PRTSW parameter in the SWLDPRM input can be used to control the amount of output of each CWELD connection. If PRTSW = 0 or is left undefined, no diagnostic messages are printed to the output file. If PRTSW = 1, only errors are printed. If PRTSW = 2, errors and warnings are printed. if PRTSW = 3, all projection diagnostics are printed for each CWELD connection. If PRTSW = 4, all projection diagnostics and all specifics of the tying constraints involved in each connection are printed.

Two Dimensional Models The previous sections described the CWELD connections for three dimensional models. However, CWELD connections can also be made in two dimensional models. In that case, the patches consist of beams, trusses, or edges of continuum elements. The same connection methods that are available for three dimensional models can be used in two dimensional models. The connector element must be a two dimensional beam or an axisymmetric shell depending on the type of two dimensional analysis. The number of auxiliary nodes is two instead of four; one to the left and one to right of the projection point

Main Index

656 Marc Volume A: Theory and User Information

on the master patch. Two patch types are available: linear (with two nodes) and quadratic (with three nodes) patches. The 3 x 3 requirement only applies in one direction now, so a connection on one side can not span more than three patches of the surface.

CFAST Connections CFAST connections can only be defined using indirect patch-to-patch connections. Two methods, ELEM or PROP, are available to create them. They are equivalent with the CWELD ELPAT and PARTPAT

methods, respectively (see Figures 9-57 and 9-58). In each of these methods, the surfaces on both sides have to be defined together with the GS reference point of the connection. Both methods can be used to connect noncongruent meshes of any type. The constraints between the connector nodes and the auxiliary patches are applied through Kirchhoff constraints (typing type 44) and the constraints between the auxiliary nodes and the secondary patches are applied through RBE3 constraints. The connector element is a cbush element. In a two dimensional model, it is element type 194 and in a three dimensional model, it is element type 195. For more details about the cbush elements, refer to Marc Volume B: Element Library. It is always required to include the ELEMENTS parameter for each element type used as a connector even when it does not appear in the CONNECTIVITY input. The data for each connection is defined on the CFAST model definition input. Some data inputs are always required because no defaults exist for them. Other data inputs are optional and if not defined, Marc assumes appropriate defaults values for them. These optional data inputs concern the connector element type, the way the projections are carried out, the type of constraints, and the orientations of the specific CFAST connections. For a more detailed description of the CFAST option, refer to Marc Volume C: Program Input.

CFAST Properties PFAST Property Definition The properties of the CFAST connection are defined using the PFAST model definition option. It contains the diameter of the fastener, the stiffness matrix, damping coefficient, and mass. The diameter data is only used to compute the locations of the auxiliary nodes involved in the CFAST connection. It will not affect the element stiffness as the latter has to be explicitly entered. For a more detailed description of the PFAST option, refer to Marc Volume C: Program Input. CFAST Element Coordinate System The stiffness and damping values are given is a specified coordinate system ( e 1 ,e 2 ,e 3 ) . This coordinate system is used as the element coordinate system. The output of CFAST is given in this system. There are two options to define it: 1. Using the connector element orientation. The x-axis points from GA to GB. xB – xA e 1 = ------------------------xB – xA In case of zero length, the normal of the first patch is taken. Find the index of j of smallest component of e 1

Main Index

CHAPTER 9 657 Boundary Conditions

j

i

e 1 = min { e 1 } i = 1 ,2 ,3

In case of two equal components, the smaller index i is taken. Define an auxiliary vector: σ1 j b =

σ 2 j , where σ k j = 1 when k = j and 0 otherwise (for example, for j = 3 , σ3 j

b =

0 0 ) e 3 is created by the normalized cross product of e 1 and b . And, finally, e 2 is the 1

normalized cross product of e 3 and e 1 . For geometrically nonlinear analysis, this coordinate system co-rotates with the element. u

u

u

2. Using a global or user-defined coordinate system ( e 1 ,e 2 ,e 3 ) . For this option, you may choose between a relative and an absolute orientation. a. the absolute orientation: u

u

u

( e 1 ,e 2 ,e 3 ) = ( e 1 ,e 2 ,e 3 ) For a geometrically non-linear analysis, this coordinate system is fixed in time. b. The relative orientation: the x-axis points from GA to GB. xB – xA e 1 = ------------------------xB – xA In case of zero length, the normal of the first patch is taken. e 3 is defined by the normalized u

cross product of e 1 and e 2 . e 2 is defined by the normalized cross product of e 3 and e 1 . For a geometrically nonlinear analysis, this coordinate system co-rotates with the element.

SWLDPRM, Special CWELD/CFAST Parameters A number of global parameters that control the behavior of CWELD and CFAST connections and their output to the jobid.out file can be entered through the SWLDPRM model definition option. These parameters and their descriptions are summarized in Table 7-28. Table 7-28

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.

658 Marc Volume A: Theory and User Information

Table 7-28

Name

SWLDPRM Parameter Names and Descriptions (continued)

Default

Description

NREDIA

0 < Integer < 4

Type

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.

PRTSW

0 < Integer < 4

0

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).

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)

Main Index

CHAPTER 9 659 Boundary Conditions

Table 7-28

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

660 Marc Volume A: Theory and User Information

Table 7-28

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.

CHAPTER 9 661 Boundary Conditions

Table 7-28

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 1 involved in a CWELD/CFAST connection is: f i = ----n di where fi

is the weighting factor for retained node i.

d i 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

662 Marc Volume A: Theory and User Information

Table 7-28

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

Chapter 10 Element Library

10

Main Index

Element Library

J

Truss Elements

J

Membrane Elements

666

J

Continuum Elements

666

J

Beam Elements

J

Plate Elements

668

J

Shell Elements

668

J

Heat Transfer Elements

J

Electromagnetic Analysis

J

Soil Analysis

J

Fluid Analysis

J

Piezoelectric Analysis

J

Special Elements

J

Incompressible Elements

666

667

668 670

670 670 670

671 672

664 Marc Volume A: Theory and User Information

Marc includes an extensive element library. The element library allows you to model various types of one-, two-, and three-dimensional structures, such as plane stress and plane strain structures, axisymmetric structures, full three-dimensional solid structures, and shell-type structures. (See Marc Volume B: Element Library for a detailed description of each element, a reference to the use of each element, and recommendations concerning the selection of element types for analysis). After you select an element type or a combination of several element types for your analysis with the ELEMENTS or SIZING parameter, you must prepare the necessary input data for the element(s). In general, the data consist of element connectivity, thickness for two-dimensional beam, plate and shell elements, cross section for three-dimensional beam elements, coordinates of nodal points, and face identifications for distributed loadings. You can choose different element types to represent various parts of the structure in an analysis. If there is an incompatibility between the nodal degrees of freedom of the elements, you have to provide appropriate tying constraints to ensure the compatibility of the displacement field in the structure. Marc assists you by providing many standard tying constraint options, but you are responsible for the consistency of your analysis. You can use almost all of the Marc elements for both linear and nonlinear analyses, with the following exceptions. • No plasticity or cracking is allowed in the elastic beams, the shear-panel, and the Fourier elements. • The updated Lagrange and finite strain plasticity features are not available for all elements. • Plasticity is available for the Herrmann elements when using the FeFp formulation only. • Only heat links and two-dimensional heat transfer elements can be used for hydrodynamic bearing analysis. • Fourier analysis can be carried out only for a limited number of axisymmetric elements. Marc defines all continuum elements in the global coordinate system. Truss, beam, plate, and shell elements are defined in a local coordinate system and the resulting output must be interpreted accordingly. You should give special attention to the use of these elements if the material properties have preferred orientations. The ORIENTATION option is available to define the preferred directions. All Marc elements are numerically integrated. Element quantities, such as stresses, strains, and temperatures, are calculated at each integration point of the element if you use the ALL POINTS parameter. This is the default in Marc. These quantities are computed only at the centroid of the element, if the CENTROID parameter is used. Distributed loads can be applied along element edges, over element surfaces, or in the volume of the element. Marc automatically evaluates consistent nodal forces through numerical integration. (See Marc Volume B: Element Library for details on this process). Concentrated forces must be applied at the nodal points. All plate and shell elements can be used in a composite analysis. You can have a variable thickness shell, and control the thickness and material property and orientation for each layer. For the thick shell elements (types 22, 45, 75, or 140), the interlaminar shear can also be calculated.

Main Index

CHAPTER 10 665 Element Library

Five concepts differentiate the various elements types. These concepts are listed invalid for pure heat transfer. below. 1. The type of geometric domain that the element is modeling. These geometric domains are: Truss Membrane Beam Plate Shell Plane stress Plane strain Generalized plane strain Axisymmetric Three-dimensional solid Special 2. The type of interpolation (shape) functions used in the element. These functions are: Linear Quadratic Cubic Hermitian Special The interpolation function is used to describe the displacement at an arbitrary point in the body. u i ( x ) = N i ( x )u i

(10-1)

where u ( x ) is the displacement at x, N are the interpolation (shape) functions, and u are the generalized nodal displacements. Engineering strain is ∂u i ( x ) ∂u j ( x ) ε i j ( x ) = 1 ⁄ 2 ⎛ ---------------- + ----------------⎞ ⎝ ∂x j ∂x i ⎠

(10-2)

Therefore, the computational evaluation is ∂N i u i ∂N j u j ε i j ( x ) = 1 ⁄ 2 ⎛ -------------- + --------------⎞ = β i j u i ⎝ ∂x j ∂x i ⎠

(10-3)

Hence, ∂N i β i j = --------∂x j

(10-4)

3. The number of nodes in a particular element. 4. The number of degrees of freedom associated with each node, and the type of degrees of freedom. 5. The integration method used to evaluate the stiffness matrix. Marc contains elements which use full integration and reduced integration.

Main Index

666 Marc Volume A: Theory and User Information

Truss Elements Marc contains 2- and 3-node isoparametric truss elements that can be used in three dimensions. These elements have only displacement degrees of freedom. Since truss elements have no shear resistance, you must ensure that there are no rigid body modes in the system.

Membrane Elements Marc contains 3-, 4-, 6-, and 8-node isoparametric membrane elements that can be used in three dimensions. These elements have only displacement degrees of freedom. Since membrane elements have no bending resistance, you must ensure that there are no rigid body modes in the system. Membrane elements are often used in conjunction with beam or truss elements.

Continuum Elements Marc contains continuum elements that can be used to model plane stress, plane strain, generalized plane strain, axisymmetric and three-dimensional solids. These elements have only displacement degrees of freedom. As a result, solid elements are not efficient for modeling thin structures dominated by bending. Either beam or shell elements should be used in these cases. The solid elements that are available in Marc have either linear or quadratic interpolation functions. They include • • • • • • • •

3-, 4-, 6-, and 8-node plane stress elements 3-, 4-, 6-, and 8-node plane strain elements 6 (4 plus 2)- and 10 (8 plus 2)-node generalized plane strain elements 3-, 4-, 6-, and 8-node axisymmetric ring elements 8-, 10-, and 20-node brick elements 4- and 10-node tetrahedron 6-node and 15-node pentahedral 12- and 27-node semi-infinite brick elements

In general, the elements in Marc use a full-integration procedure. Some elements use reduced integration. The lower-order reduced integration elements include an hourglass stabilization procedure to eliminate the singular modes. Continuum elements are widely used for thermal stress analysis. For each of these elements, there is a corresponding element available for heat transfer analysis in Marc. As a result, you can use the same mesh for the heat transfer and thermal stress analyses. Marc has no singular element for fracture mechanics analysis. However, the simulation of stress singularities can be accomplished by moving the midside nodes of 8-node quadrilateral and 20-node brick elements to quarter-point locations near the crack tip. Many fracture mechanics analyses have used this quarter-point technique successfully.

Main Index

CHAPTER 10 667 Element Library

The 4- and 8-node quadrilateral elements can be degenerated into triangles, and the 8-and 20-node solid brick elements can be degenerated into wedges and tetrahedra by collapsing the appropriate corner and midside nodes. The number of nodes per element is not reduced for degenerated elements. The same node number is used repeatedly for collapsed sides or faces. When degenerating incompressible elements, exercise caution to ensure that a proper number of Lagrange multipliers remain. You are advised to use the higher-order triangular or tetrahedron elements wherever possible, as opposed to using collapsed quadrilaterals and hexahedra.

Beam Elements Marc’s beam elements are 2- and 3-node, two- and three-dimensional elements that can model straight and curved-beam structures and framed structures and can serve as stiffeners in plate and shell structures. A straight beam of a circular cross section can be used for modeling the straight portion of piping systems. Translational and rotational degrees of freedom are included in beam elements. The cross section of the beam can be solid or thin-walled. The solid sections can be standard elliptical, rectangular, trapezoidal, or hexagonal sections or arbitrary solid sections. The thin-walled sections can be standard closed circular sections or arbitrary closed or open sections. The BEAM SECT parameter is used to define all solid sections and to define arbitrary thin-walled open or closed sections. The beam elements are numerically integrated along their axial direction using Gaussian integration. The stress strain law is integrated through thin-walled sections using a Simpson rule and through solid sections using a Simpson, Newton-Cotes, or Gauss rule depending on the input specifications. Stresses and strains are evaluated at each integration point through the thickness. This allows an accurate calculation if nonlinear material behavior is present. In elastic beam elements, only the total axial force and moments are computed at the integration points. If element 52 or 98 is used with numerical section integration, six stiffness factors may be used to modify its stiffness behavior in axial tension, bending, torsion and shear. The modified internal virtual work of beam element type 98 when using any of the stiffness factors is given as: L

δW i n t =

∫ ( f 1 N z δε z + f2 M z δκ z + f 3 M y δκ y + f 4 D x δγ x + f 5 D y δγ y + f 6 T z δκ z ) dz 0

For element type 52 the transverse shear terms are absent. In this expression, f 1 is the normal stiffness factor, f 2 and f 3 are the bending stiffness factors, f 4 and f 5 are the transverse shear stiffness factors and f 6 is the torsional stiffness factor. All stiffness factors have a default value of 1 and must be positive. If stiffness factors with other values than 1 are used, the stress output must be interpreted as follows: Generalized stresses will be scaled with their respective stiffness factors (i.e., f 1 N z , f 2 M x , etc. will be written to the output or post file) Layer stresses are not scaled with their respective stiffness factors, meaning that their section integration will result in the unscaled generalized stresses (i.e., N z , M x , etc.)

Main Index

668 Marc Volume A: Theory and User Information

If the section is used as a pre-integrated section all stiffness factors can have arbitrary positive values, but if the section is used with numerical integration throughout the analysis the stiffness contributions resulting from the direct stresses must use identical positive stiffness factors (i.e., f 1 = f 2 = f 3 ) and the stiffness contributions resulting from the shear stresses must use identical positive stiffness factors (i.e. f 4 = f 5 = f 6 ) in order to guarantee symmetry of the stiffness matrix. If these conditions are not met, f 2 and f 3 will silently be set to f 1 and f 4 and f 5 will silently be set to f 6 .

Plate Elements The linear shell elements (Types 49, 72, 75, 138, 139, or 140) or the quadratic element (Type 22) can be used effectively to model plates and have the advantage that tying is unnecessary. For element type 49, you can indicate on the GEOMETRY option that the flat plate formulation is to be used. This reduces computational costs. To further reduce computational costs for linear elastic plate analysis, the number of points through the thickness can be reduced to one by use of the SHELL SECT parameter.

Shell Elements Marc contains three isoparametric, doubly curved, thin shell elements: 3-, 4-, and 8-node elements (Types 4, 8, and 24, respectively) based on Koiter-Sanders shell theory. These elements are C1 continuous and exactly represent rigid-body modes. The program defines a mesh of these elements with respect to a surface curvilinear coordinate system. You can use the FXORD model definition option to generate the nodal coordinates. Tying constraints must be used at shell intersections. Thin shell analysis can be performed using either the 3-node discrete Kirchhoff theory (DKT) based element (Type 138), the 4-node bilinear DKT element (Type 139), the 6-node bilinear semi-loof element (Type 49), or the 8-node bilinear semi-loof element (Type 72). Thick shell analysis can be performed using the 4-node bilinear Mindlin element (Type 75), the 4-node reduced integration with hourglass Mindlin element (Type 140), or the 8-node quadratic Mindlin element (Type 22). The thick shell elements have been developed so that there is no locking when used for thin shell applications. The global coordinate system defines the nodal degrees of freedom of these elements. These elements are convenient for modeling intersecting shell structures since tying constraints at the shell intersections are not needed. Marc contains three axisymmetric shell elements: 2-node straight, 2-node curved, and 3-node curved. You can use these elements to model axisymmetric shells; combined with axisymmetric ring elements, they can be used to simulate the thin and thick portions of the structure. The program provides standard tying constraints for the transition between shell and axisymmetric ring elements.

Heat Transfer Elements The heat transfer elements in Marc consist of the following: • 2- and 3-node three-dimensional links • 3-, 4-, 6-, and 8-node planar and axisymmetric elements • 6- and 9-node planar and axisymmetric semi-infinite elements

Main Index

CHAPTER 10 669 Element Library

• • • • • •

8-, 10-, and 20-node solid elements 4- and 10-node tetrahedral 6-, 15-node pentahedral 12- and 27-node semi-infinite brick elements 2-, 3-, 4-, 6-, and 8-node shell elements. 3-, 4-, 5-, and 8-node 3-D membrane elements

For each heat transfer element, there is at least one corresponding stress element, enabling you to use the same mesh for both the heat transfer and thermal stress analyses. Heat transfer elements are also employed to analyze coupled thermo-electrical (Joule heating) problems. In heat transfer continuum elements or link elements, temperature is the only nodal degree of freedom. The heat transfer shell elements can be used in two modes. In the first mode, the number of degrees of freedom is two or three for linear or quadratic temperature distribution across the complete thickness. In the second mode, the number of degrees of freedom are M + 1 or 2 * M + 1 for linear or quadratic temperature distribution for each M layer. This is defined through the HEAT parameter. The heat transfer membrane elements have only one degree of freedom per node, so there is no thermal gradient through the thickness. In Joule heating, the voltage and temperature are the nodal degrees of freedom. Shell elements are not available for Joule heating.

Acoustic Analysis Heat transfer elements are also used to model the compressible media in acoustic analysis. In this case, the pressure is the single nodal degree of freedom.

Electrostatic Analysis Heat transfer elements are also used for electrostatic analysis. The scalar potential is the degree of freedom.

Coupled Electrostatic-Structural Stress elements are used for a coupled electrostatic-structural analysis. For each of these elements, there is a corresponding heat transfer element available for the electrostatic pass. When a medium has no stiffness, like air, heat transfer elements can be chosen for this region. Then this region will be inactive in the stress pass.

Fluid/Solid Interaction Heat transfer elements are used to model the inviscid, incompressible fluid/solid interaction problems. The hydrostatic pressure is the degree of freedom.

Main Index

670 Marc Volume A: Theory and User Information

Hydrodynamic Bearing Analysis The three-dimensional heat transfer links and planar elements are used to model the lubricant film. As no variation occurs through the thickness of the film, two-dimensional problems are reduced to onedimensional, and three-dimensional problems are reduced to two-dimensional. The pressure is the degree of freedom.

Magnetostatic Analysis For two-dimensional problems, a scalar potential can be used; hence, the heat transfer planar and axisymmetric elements are employed. The single degree of freedom is the potential. For threedimensional analyses, magnetostatic elements are available. In such cases, there are three degrees of freedom to represent the vector potential.

Electromagnetic Analysis In electromagnetic problems, a vector potential, augmented with a scalar potential, is used. There are lower-order elements available for these analyses.

Soil Analysis There are three types of soil/pore pressure analysis. If a pore pressure analysis only is performed, “heat transfer” elements (41, 42, or 44) are used. If an uncoupled soil analysis is performed, the standard elements (21, 27, or 28) are used. If a coupled analysis is performed, the Herrmann elements (32, 33, or 35) are used. In this case, the last degree of freedom is the pore pressure.

Fluid Analysis When performing fluid analysis, any planar, axisymmetric or solid continuum element can be used. These elements either used a mixed formulation or a penalty formulation based upon the value of the FLUID parameter. For the mixed formulation, each node of lower- or higher-order continuum element has velocities as well as pressure degrees of freedom. The penalty method yields elements with only the velocities as the nodal variables.

Piezoelectric Analysis In a piezoelectric analysis, a strong coupling exist between stress and electric field. There are lower-order elements available for this analysis. The first two or three degrees of freedom (in resp. 2-D or 3-D) are available for displacement components, and the last (3rd or 4th) degree of freedom is available for the electric potential.

Main Index

CHAPTER 10 671 Element Library

Special Elements Marc contains unique features in the program.

Gap-and-Friction Elements The gap-and-friction elements (12, 97) are based on the imposition of gap closure constraint and frictional-stick or frictional-slip through Lagrange multipliers. These elements provide frictional and gapping connection between any two nodes of a structure; they can be used in several variations, depending on the application. In the default formulation, the elements simulate a gap in a fixed direction, such that a body does not penetrate a given flat surface. Using the optional formulation, you can constrain the true distance between two end-points of the gap to be greater than some arbitrary distance. This ability is useful for an analysis in which a body does not penetrate a given two-dimensional circular or three-dimensional spherical surface. Finally, you can update the gap direction and closure distance during analysis for the modeling of sliding along a curved surface.

Pipe-bend Element The pipe-bend (3-node elbow) element 17 is designed for linear and nonlinear analysis of piping systems. It is a modified axisymmetric shell element for modeling the bends in a piping system. The element has a beam mode superposed on the axisymmetric shell modes so that ovalization of the crosssection is admitted. The twisting of a pipe-bend section is ignored because the beam has no flexibility in torsion. Built-in tying constraints are used extensively for coupling the pipe-bend sections to each other and to straight beam elements.

Curved-pipe Element The curved-pipe (2-node) element 31 is designed for linear analysis only. The stiffness matrix is based upon the analytic elastic solution of a curved pipe.

Shear Panel Element The shear panel (4-node) element 68 is an elastic element of arbitrary shape. It is an idealized model of an elastic sheet. This element only provides shearing resistance. It must be used with beam stiffeners to ensure any normal or bending resistance. The shear-panel element is restricted to linear material and small displacement analysis.

Cable Element The cable element (51) is an element which exactly represents the catenary behavior of a cable. It is an elastic element only.

Main Index

672 Marc Volume A: Theory and User Information

Rebar Elements The rebar elements (23, 46, 47, 48, 142, 143, 144, 145, 146, 147, 148, 165, 166, 167, 168, 169, and 170) are hollow elements in which you can place single-direction strain members (reinforcing cords or rods). The rebar elements are used in conjunction with other solid elements (filler) to represent a reinforced material such as reinforced concrete. The reinforcing members and the filler are accurately represented by embedding rebar elements into solid elements. The rebar elements can be used for small as well as large strain behavior of the reinforcing cords. Also, any kind of material behavior can be simulated by the rebar elements in Marc.

Interface Elements Elements 186 through 193 are special elements which are used to model the delamination in composite structures where each ply is modeled with solid elements. The material behavior of these elements is defined with the COHESIVE model definition option.

Incompressible Elements Incompressible and nearly incompressible materials can be modeled by using a special group of elements in the program. These elements, based on modified Herrmann variational principles, are capable of handling large deformation effects as well as creep and thermal strains. The incompressibility constraint is imposed by using Lagrange multipliers. Generally, the low (linear) order elements have a single additional node which contains the Lagrange multiplier, while the high-order (quadratic) elements have Lagrange multipliers at each corner node. Elements 155 (plane strain triangle), 156 (axisymmetric triangle), and 157 (3-D tetrahedron) are loworder elements and are exceptions within the incompressible element group. They have an additional node located at the center of the elements and have Lagrange multipliers at each corner node. The shape function of the center node is a bubble function. See Figure 10-1 for an element 155 case. The degrees of freedom of the center node is condensed out on the element level before the assembly of the global matrix. 3

Nodes with both displacements and pressure as degrees of freedom

x Center node with only displacement degrees of

4

x

freedom. The shape function for this node is a bubble function. 2

1

Figure 10-1 Element 155

Large Strain Elasticity The incompressible elements based on Herrmann formulations can be used for large strain analysis of rubber-like materials, using either total Lagrangian formulation or updated Lagrangian formulation.

Main Index

CHAPTER 10 673 Element Library

Large Strain Plasticity Elemen The incompressible elements can be used for large strain analysis of elasto-plastic materials using updated Lagrangian formulation, based on multiplicative decomposition of deformation gradient. t Library Incomp ressibl e Elemen ts

Rigid-Plastic Flow In rigid-plastic flow analysis, with effectively no elasticity, incompressible elements must be used. For such analyses, you have a choice of using either the elements with Lagrange multipliers discussed above, or standard displacement continuum elements. In the latter case, a penalty function is used to satisfy the incompressibility constraint.

Constant Dilatation Elements You can choose an integration scheme option, which makes the dilatational strain constant throughout the element. This can be accomplished by setting the second field of the GEOMETRY option to one. Constant dilatational elements are recommended for use in approximately incompressible, inelastic analysis, such as large strain plasticity, because conventional elements can produce volumetric locking due to overconstraints for nearly incompressible behavior. This option is only available for elements of lower order (Types 7, 10, 11, 19, and 20). For the lower-order reduced integration elements (114 to 117) with hourglass control, as only one integration point is used, these elements do not lock, and effectively, a constant dilatation formulation is used. (The constant dilatation approach has also been referred to mean dilatation and B-bar approach in the literature.)

Reduced Integration Elements Marc uses a reduced integration scheme to evaluate the stiffness matrix or the thermal conductivity matrix for a number of isoparametric elements. The mass matrix and the specific heat matrix of the element are always fully integrated. For lower-order, 4-node quadrilateral elements, the number of numerical integration points is reduced from 4 to 1; in 8-node solid elements, the number of numerical integration points is reduced from 8 to 1. For 8-node quadrilateral elements, the number of numerical integration points is reduced from 9 to 4; for 20-node solid elements, the number of numerical integration points is reduced from 27 to 8. The energy due to the higher-order deformation mode(s) associated with high-order elements is not included in the analysis. Reduced integration elements and fully integrated elements can be used together in an analysis. Reduced integration elements are more economical than fully integrated elements and they can improve analysis accuracy. However, with near singularities and in regions of high-strain gradients, the use of reduced integration elements can lead to oscillations in the displacements and produce inaccurate results. Using reduced integration elements results in zero-energy modes, or breathing nodes. In the lower-order elements, an additional stabilization stiffness is added which eliminates these so-called “hourglass” modes.

Main Index

674 Marc Volume A: Theory and User Information

Continuum Composite Elements There is a group of isoparametric elements in Marc which can be used to model composite materials. Different material properties can be used for different layers within these elements. The number of continuum layers within an element, the thickness of each layer, and the material identification number for each layer are input via the COMPOSITE option. A maximum number of 1020 layers can be used in one 2-D continuum composite element. A 3-D continuum composite element only allows a maximum of 510 layers within the element. These structural elements are available as both lower- and higher-order and can be used for plane strain (element types 151 and 153), axisymmetric (element types 152 and 154) or 3-D solid analysis (element types 149 and 150). Corresponding heat transfer elements are available for lower- and higher-order and can be used for planar (element types 177 and 179), axisymmetric (element types 178 and 180) or 3-D solid analysis (element types 175 and 176).

Fourier Elements A special class of elements exists which allows the analysis of axisymmetric structures with nonaxisymmetric loads. The geometry and material properties of these structures do not change in the circumferential direction, and the displacement can be represented by a Fourier series. This representation allows a three-dimensional problem to be decoupled into a series of two-dimensional problems. Both solid and shell Fourier elements exist in Marc. These elements can only be used for linear elastic analyses.

Semi-infinite Elements This group of elements can be used to model unbounded domains. In the semi-infinite direction, the interpolation functions are exponential, such that the function (displacement) is zero at the far domain. The rate of decay of the function is dependent upon the location of the midside nodes. The interpolation function in the non semi-infinite directions are either linear or quadratic. These elements can be used for static plane strain, axisymmetric, or 3-D solid analysis. They can also be used for heat transfer, electrostatic, and magnetostatic analyses.

Cavity Surface Elements This group of elements can be used to define the boundaries of cavities where standard finite elements are not used; for example, along rigid boundaries. These elements are for volume calculation purposes only and do not contribute to the stiffness equations of the model. They can be used for plane strain, plane stress, axisymmetric, and 3-D analyses. No material properties are needed for these elements. They do not undergo any deformation except if they are attached or glued to other elements or surfaces.

Main Index

CHAPTER 10 675 Element Library

Assumed Strain Formulation Conventional isoparametric four-node plane stress and plane strain, and eight-node brick elements behave poorly in bending. The reason is that these elements do not capture a linear variation in shear strain which is present in bending when a single element is used in the bending direction. For the six elements (3, 7, 11, 160, 161, and 163), the interpolation functions have been modified such that shear strain variation can be better represented. For the lower-order reduced integration elements (114 to 123), an assumed strain formulation written with respect to the natural coordinates is used. For elastic isotropic bending problems, this allows the exact displacements to be obtained with only a single element through the thickness. This is invoked by using the ASSUMED STRAIN parameter or by setting the third field of the GEOMETRY option to one.

Follow Force Stiffness Contribution When activating the FOLLOW FOR parameter, the distributed loads are calculated based upon the current deformed configuration. It is possible to activate an additional contribution which goes into the stiffness matrix. This improves the convergence. This capability is available for element types 3, 7, 10, 11, 18, 72, 75, 80, 81, 82, 83, 84, 114, 115, 116, 117, 118, 119, 120, 139, 140, 149, 151, 152, 160, 161, 162, or 163. Inclusion of the follower force stiffness can result in nonsymmetric stiffness for nonenclosed volumes, thereby, resulting in increased computational times. You can flag the nonsymmetric solver in the SOLVER option.

Explicit Dynamics The explicit dynamics formulation IDYN=5 model is restricted to the following elements: 1, 2, 3, 5, 6, 7, 9, 10, 11, 18, 19, 20, 52, 64, 75, 89, 98, 114, 115, 116, 117, 118, 119, 120, 130, 139, and 140. When using this formulation, the mass matrix is defined semi-analytically; for example, no numerical integration is performed. In addition, a quick method is used to calculate the Courant stability limit associated with each element. For these reasons, this capability is limited to the elements mentioned above.

Adaptive Mesh Refinement Marc has a capability to perform local adaptive mesh refinement to improve the accuracy of the solution. This capability is invoked by using the ADAPTIVE parameter and model definition option. The adaptive meshing is available for the following 2-D and 3-D elements: 2, 3, 6, 7, 10, 11, 18, 19, 20, 37, 38, 39, 40, 43, 75, 80, 81, 82, 83, 84, 111, 112, 113, 114, 115, 116, 117, 118, 119, 120, 121, 122, 123, 138, 139, 140, 155, 156, 157, 160, 161, 162, 163, 164, 196, 198, and 201.

Main Index

676 Marc Volume A: Theory and User Information

Main Index

Chapter 11 Solution Procedures for Nonlinear Systems

11

Main Index

Solution Procedures for Nonlinear Systems J

Considerations for Nonlinear Analysis

J

Full Newton-Raphson Algorithm

J

Modified Newton-Raphson Algorithm

J

Direct Substitution

J

Arc-length Methods

J

Convergence Controls

J

Singularity Ratio

J

Solution of Linear Equations

J

Flow Diagram

J

Remarks

J

References

692

695 695 702

705

711

712 713

678

706

693

678 Marc Volume A: Theory and User Information

This chapter discusses the solution schemes in Marc for nonlinear problems. Issues of convergence controls, singularity ratio, and available solvers for linearized system of equations are also discussed. In a nonlinear problem, a set of equations must be solved incrementally. The governing equation of the linearized system can be expressed, in an incremental form, as Kδu = r

(11-1)

where δu and r are the correction to the incremental displacements and residual force vectors, respectively. There are several solution procedures available in Marc for the solution of nonlinear equations: • • • •

Full Newton-Raphson Algorithm Modified Newton-Raphson Algorithm Direct Substitution Arc-length Methods

Considerations for Nonlinear Analysis Nonlinear analysis is usually more complex and expensive than linear analysis. Also, a nonlinear problem can never be formulated as a set of linear equations. In general, the solutions of nonlinear problems always require incremental solution schemes and sometimes require iterations (or recycles) within each load/time increment to ensure that equilibrium is satisfied at the end of each step. Superposition cannot be applied in nonlinear problems. The iterative procedures supported in Marc are: Newton-Raphson, Modified Newton-Raphson, Newton-Raphson with strain correction, and direct substitution. If the R-P flow contribution model is chosen, a direction substitution is used. A nonlinear problem does not always have a unique solution. Sometimes a nonlinear problem does not have any solution, although the problem can seem to be defined correctly. Nonlinear analysis requires good judgment and uses considerable computing time. Several runs are often required. The first run should extract the maximum information with the minimum amount of computing time. Some design considerations for a preliminary analysis are: • Minimize degrees of freedom whenever possible. • Halve the number of load increments by doubling the size of each load increment. • Impose a coarse tolerance on convergence to reduce the number of iterations. A coarse run determines the area of most rapid change where additional load increments might be required. Plan the increment size in the final run by the following rule of thumb: there should be as many load increments as required to fit the nonlinear results by the same number of straight lines. Marc solves nonlinear static problems according to one of the following two methods: tangent modulus or initial strain. Examples of the tangent modulus method are elastic-plastic analysis, nonlinear springs, nonlinear foundations, large displacement analysis and gaps. This method requires at least the following three controls: • A tolerance on convergence • A limit to the maximum allowable number of recycles • Specification of a minimum number of recycles

Main Index

CHAPTER 11 679 Solution Procedures for Nonlinear Systems

An example of the initial strain method is creep or viscoelastic analysis. Creep analysis requires the following tolerance controls: • Maximum relative creep strain increment control • Maximum relative stress change control • A limit to the maximum allowable number of recycles To input control tolerances, use the model definition option CONTROL for all simulations. These values can be reset upon restart or through the CONTROL history definition option. For creep simulations, addition controls are provided in the AUTO CREEP or AUTO STEP options. See Convergence Controls in this chapter for further discussion on tolerance controls.

Behavior of Nonlinear Materials Nonlinear behavior can be time- (rate-) independent, or time- (rate-) dependent. For example, plasticity is time-independent and creep is time-dependent. Both viscoelastic and viscoplastic materials are also time-dependent. Nonlinear constitutive relations must be modeled correctly to analyze nonlinear material problems. A comprehensive discussion of constitutive relations is given in Chapter 7.

Scaling the Elastic Solution The SCALE parameter causes scaling of the linear-elastic solution to reach the yield stress in the highest stressed element. Scaling takes place for small displacement elastic-plastic analysis, where element properties do not depend on temperature. The SCALE parameter causes all aspects of the initial solution to be scaled, including displacements, strains, stresses, temperature changes, and loads. Subsequent incrementation is then based on the scaled solution.

Load Incrementation Several history definition options are available in Marc to input mechanical and thermal load increments (see Table 11-1). The choice is between a fixed and an automatic load stepping scheme. Table 11-1

History Definition Options for Load Incrementation

Load Type

Fixed

Adaptive

Mechanical

AUTO LOAD DYNAMIC CHANGE CREEP INCREMENT

AUTO STEP AUTO INCREMENT AUTO THERM AUTO CREEP AUTO THERM CREEP*

Thermal

TRANSIENT NON AUTO

AUTO STEP TRANSIENT*

*The option is obsolete; use AUTO STEP instead.

For a fixed scheme, the load step size remains constant during a load case. The fixed schemes are AUTO LOAD for static mechanical, CREEP INCREMENT for creep, DYNAMIC CHANGE for dynamic mechanical, and TRANSIENT NON AUTO for thermal/thermo-mechanically coupled.

Main Index

680 Marc Volume A: Theory and User Information

In many nonlinear analyses, it is useful to have Marc automatically determine the appropriate load step size. For an adaptive scheme, the load step size changes from one increment to the other and also within an increment depending on convergence criteria and/or user-defined physical criteria. The adaptive schemes are AUTO STEP and AUTO INCREMENT for static mechanical, AUTO STEP and AUTO CREEP for creep, AUTO STEP, AUTO THERM, and AUTO THERM CREEP for thermally driven mechanical problems, and AUTO STEP for dynamic mechanical, and AUTO STEP and TRANSIENT for thermal/thermo-mechanically coupled. The adaptive stepping scheme of choice is AUTO STEP. AUTO STEP has been designed as a unified load stepping scheme and many of the capabilities of the other stepping schemes can now be handled by AUTO STEP. AUTO STEP can be used for mechanical (static, creep, dynamic), thermal, and thermomechanically coupled analysis problems. • In the AUTO STEP scheme, either a recycle based convergence criterion is used to automatically determine the time step based upon a comparison of the actual number of recycles needed in an increment to a user-specified desired number of recycles or a damping energy procedure is used. In addition to this, user-defined or program-determined physical criteria based upon strain, stress, displacement, or temperature increments can be used to control the time step. Reductions in the time step through cut-backs are used to satisfy both convergence criteria and physical criteria. More details on the AUTO STEP option are provided in the next section. • Post buckling or snap-through analyses require the so-called arclength method which is available through the AUTO INCREMENT option. This option can only be used in static mechanical analyses and the applied load is automatically increased or decreased in order to maintain a certain arclength. Note:

AUTO INCREMENT can also be used for general situations without instabilities, but, in general, the AUTO STEP option is preferred for these situations.

• For creep analysis, the available adaptive options are AUTO CREEP and AUTO STEP. The AUTO CREEP option determines the time step in an explicit creep analysis based on the creep strain change and the stress change (see Volume C: Program Input, Chapter 3). These checks are not available by default in AUTO STEP. These may however be incorporated by using an absolute or relative creep strain increment criterion and an absolute or relative stress increment criterion as additional user-defined physical criteria in combination with the default convergence criterion. Addition of these user-defined criteria for AUTO STEP is quite simple. If an appropriate input flag is set, two physical criteria are automatically added by the program at run-time for explicit creep problems: creep strain increment/elastic strain = 0.5, and stress increment/stress at beginning of increment = 0.5. It should also be noted that AUTO STEP is usually more reliable in cases involving creep and contact. • For the case of automatic load stepping for a thermally loaded elastic-creep/elastic-plastic-creep stress analysis, the available adaptive schemes are AUTO THERM CREEP and AUTO STEP. Allowable increments for normalized creep strain, normalized stress and state variables can be optionally prescribed for AUTO STEP either through user-defined criteria or program determined

Main Index

CHAPTER 11 681 Solution Procedures for Nonlinear Systems

automatic physical criteria. • For thermally driven mechanical problems, the available options are AUTO THERM and AUTO STEP. The thermal loads derived from a thermal analysis are applied using the CHANGE STATE option in a mechanical analysis. In the AUTO THERM scheme, the load step of the mechanical analysis is automatically adjusted based upon user-specified (allowed) changes in temperature from the thermal analysis per increment. For example, if there is a change of 50° in the thermal analysis in one increment but only a change of 10° per increment is allowed in the mechanical analysis, AUTO THERM splits up the thermal increment into five mechanical increments. Allowable state variable increments can be optionally prescribed for AUTO STEP either through a user-defined criterion or program determined automatic physical criterion. If these criteria are violated in an increment, AUTO STEP cuts the time-step back and repeats the increment with a smaller time step.

Selecting Load Increment Size Selecting a proper load step increment is an important aspect of a nonlinear solution scheme. Large steps often lead to many recycles per increment and, if the step is too large, it can lead to inaccuracies and nonconvergence. On the other hand, using too small steps is inefficient.

Fixed Load Incrementation When a fixed load stepping scheme is used, it is important to select an appropriate load step size that captures the loading history and allows for convergence within a reasonable number of recycles. For complex load histories, it is necessary to prescribe the loading through time tables while setting up the run. For fixed stepping, there is an option to have the load step automatically cut back in case of failure to obtain convergence. When an increment diverges, the intermediate deformations after each recycle can show large fluctuations and the final cause of program exit can be any of the following: maximum number of recycles reached (exit 3002), elements going inside out (exit 1005 or 1009) or, in a contact analysis, nodes sliding off a rigid contact body (exit 2400), and nodes not being projected properly onto 3-D NURBS (exit 2401). These deformations are normally not visible as post results (there is a feature to allow for the intermediate results to be available on the post file, see the POST option). If the cutback feature is activated and one of these problems occur, the state of the analysis at the end of the previous increment is restored and the increment is subdivided into a number of subincrements. The step size is halved until convergence is obtained or the user-specified number of cutbacks has been performed. Once a subincrement is converged, the analysis continues to complete the remainder of the original increment. No results are written to the post file during subincrementation. When the original increment is finished, the calculation continues to the next increment with the original increment count and time step maintained. If the global remeshing option is activated in conjunction with the cutback feature, then, for exit 1005 or 1009, the chosen contact body is remeshed and the analysis is repeated with the original time step before the first cutback.

Main Index

682 Marc Volume A: Theory and User Information

Arc Length Method The arc-length procedures assume that the control of the nonlinear behavior and possible instabilities is due to mechanical loads, and that the objective is to obtain an equilibrium position at the end of the loadcase. Hence, while the program may increase or decrease the load, the load can always be considered to be F = F b + λ ( F e – F b ) , where F b and F e are the loads at the beginning and end of the loadcase. The scale factor does not necessarily vary linearly from 0 to 1 over the increments, and may, in fact, become negative. This would result in negative time steps as well; hence, the AUTO INCREMENT history definition option cannot be used with dynamics and should not be used with table driven input where the load is a function of time. Mechanical loads, as shown above, are applied in a proportional manner and thermal loads are applied instantaneously. This means that any automatic load incrementation method is limited to mechanical input histories that only have linear variations in load or displacement and thermal input histories that have immediate change in temperature. For example, one may not use a rigid body with a linearly changing velocity, since the resulting displacement of the rigid body would give parabolically changing displacements. In this case, one would need to use a constant velocity for the arc length method to work properly. For the arc length method, care must be taken to appropriately define the loading history in each loadcase. The load case should be defined between appropriate break points in the load history curve. For example, in Figure 11-1, correct results would be obtained upon defining three distinct loadcases between times 0 – t 1 , t 1 – t 2 , and t 2 – t 3 during the model preparation. However, if only one load case is defined for the entire load history between 0 – t 3 , the total applied load for the loadcase is zero. This is also true when the AUTO STEP history definition option is used when the table driven input is not used. P2 P (Load)

P (Load)

P2

P1

t1 0

t2

t (Time) a. Three Defined Loadcases

Figure 11-1

P1

t3

t3 0

t (Time) b. One Defined Loadcase

Defining Loadcases for Automatic Load Incrementation

When the table driven input method is used with the AUTO INCREMENT history definition option and behavior as shown in Figure 11-1 is desired, the independent variable should be the load case number and not time. A quasi-static total mechanical load can, hence, be given which is both a function of position and the load case number.

Main Index

CHAPTER 11 683 Solution Procedures for Nonlinear Systems

AUTO STEP The scheme appropriate for most applications is AUTO STEP. The primary control of the load step is based upon the number of recycles needed to obtain convergence. There are a number of optional userspecified physical criteria that can be used to additionally control the load step. The user inputs needed to define the AUTO STEP scheme are described in Marc Volume C: Program Input. Recycling Criterion The default recycle based criterion works as follows: The user specifies a desired number of recycles. For most problems, it is sufficient to provide a value in the range of three to five. For problems with severe nonlinearities or for problems with very small convergence tolerances, it may be necessary to increase this number. This number is used as a target value for the load stepping scheme. If the number of recycles required in the current increment is less than the desired number, the load step for the next increment is increased. The time step increase is based on a factor, S u , that can also be specified by the user. Typical values for S u are in the range of 1.2 to 1.5. While the time step increase is obviously more aggressive with larger scale factors, it should be noted that there may be excessive recycling and cutbacks if sudden nonlinearities are encountered. In order to avoid this, Marc uses the following logic for higher scale factors. If the actual number of recycles in an increment is greater than 60 % of the desired number of recycles (i.e., the current increment did not converge easily), the increase scale factor for the next increment is limited to 1.25 for scale factor values between 1.25 and 1.5625, and to 80 % of the value for scale factors above 1.5625. See Damping Energy for alternative approach. Time Step Cutback Scheme The load step is never increased during an increment. If the number of recycles needed to obtain convergence exceeds the desired number, the load step size is scaled back, the recycling cutback number N r is incremented by 1 and the increment is performed again with the new load step. The scaleback factor for the N r th cutback is taken as s s = [ Ts ⁄ Tm ]

2 ⁄ ( Nr m ( Nr m + 1 ) )

Nr

, where the factor s is calculated from the expression

; where N r m is the maximum number of recycling related cutbacks

for the increment and is calculated from N r m = log 10 ( 10 5 * T s ⁄ T m ) , T s is the time increment before any recycling related cutbacks occur for the increment and T m is the minimum possible time step for the increment. T m is equal to the value set by the user ( 10 – 5 by default) if there is no quasi-static inertial damping and is equal to 10 – 3 times the value set by the user ( 10 – 8 by default) if there is quasi-static inertial damping. The scaleback factor for any cutback is the smaller of ( s

Nr

, 1 ⁄ S u ). This scheme

guarantees that no matter what the starting time step for an increment, the minimum time step is reached in a reasonable number of cutbacks if the increment consistently fails to converge. For special cutbacks such as maximum number of recycles reached (exit 3002), elements going inside out (exit 1005 or 1009) or, in a contact analysis, nodes sliding off a rigid contact body (exit 2400) nodes not being projected

Main Index

684 Marc Volume A: Theory and User Information

Nr

properly onto a 3-D NURB (exit 2401), the scaleback factor is the smaller of ( s , 0.5). If the minimum time step is reached and the analysis still fails to converge, it is terminated with exit 3015. If the ‘proceed when not converged’ option is used, then the analysis proceeds to the next increment if and when the maximum number of recycles are reached. Exceptions There are some exceptions to the basic scheme outlined above. If an increment is consistently converging with the current load step and the number of recycles exceeds the desired number, the number of recycles is allowed to go beyond the desired number until convergence or up to the user specified maximum number. The time step is then decreased for the next increment by 1 ⁄ S u . An increment is determined to be converging if the convergence ratio was decreasing in three previous recycles. Special rules also apply in a contact analysis. For quasi-static problems, the AUTO STEP option is designed to only use the automated penetration check option (see CONTACT option, 7th field of 2nd data block; option 3 is always used). During the recycles, the contact status can keep changing (new nodes come in contact, nodes slide to new segments, separate etc.). Whenever the contact status changes during an increment, a new set of contact constraints are incorporated into the equilibrium equations and more recycles are necessary in order to find equilibrium. These extra recycles, due to contact changes, are not counted when the recycle number is checked against the desired number for determining if the load step needs to be decreased within the increment. Thus, only true Newton-Raphson iterations are taken into account. For the load step of the next increment, the accumulated number of recycles during the previous increment is used. This ensures that the time step is not increased when there are many changes in contact during the previous increment. Thermal Analysis For the most part, the recycling criterion works in a similar fashion for thermal analysis (heat transfer analysis, or thermal part of a coupled thermo-mechanical analysis). The recycling criterion is used to satisfy the tolerance value provided for the temperature error in estimate on the CONTROL option; that is, the analysis cuts back and starts the increment over if the temperature error in estimate is not consistently converging within the desired number of recycles. If the temperature estimate consistently converges in three previous recycles, the analysis continues recycling. Once the temperature estimate tolerance is satisfied, the actual incremental temperature change ΔT a is calculated and checked against the corresponding tolerance ΔT m provided on the CONTROL option. It should be noted that if a user criterion on temperature is also provided, the latter parameters over-ride the one provided on the CONTROL option. More details on how user criteria are handled are described in the next section. If the incremental temperature change is not satisfied, the time step is scaled-back using a factor = 0.8 ( ΔT m ⁄ ΔT a ) . In this case, the thermal pass is simply continued with the smaller time step without a cut-back because if there was a cutback, the analysis would have redo the temperature error in estimate convergence from scratch. However, if the maximum number of allowed recycles is reached before thermal convergence is achieved, a cutback with a scale-back factor of min( s increment is repeated.

Main Index

Nr

, 0.5) is made and the

CHAPTER 11 685 Solution Procedures for Nonlinear Systems

User-defined Physical Criteria In addition to allowing Marc to use the number of recycles for automatically controlling the step size for AUTO STEP, user-specified physical criteria can optionally be used for controlling the step size. The user-specified physical criteria work as follows. The user can specify the maximum allowed incremental change within certain ranges for specific quantities during an increment. The quantities available are displacements, rotations, stresses, strains, strain energy, temperature (in thermal or thermomechanically coupled analyses), and state variables (in mechanical or thermomechanically coupled analysis). These criteria can be utilized in one of two ways. By default, they are used as limits, which means that the load step is immediately decreased if a criterion is violated during any iteration of the current increment, but they do not influence the decision to change the load step for the next increment; that is, only the actual number of recycles versus desired number of recycles controls the load step for the next increment. The criteria can also be used as targets; in which case, they are used to control the time step for the current and next increments. If the calculated values of the criteria are higher than the user-specified values in any iteration, the time step is scaled down and the current increment is repeated. If the calculated values of the criteria for the current increment are consistently smaller than the user-specified values prior to convergence, the time step for the next increment is scaled up. The scale factor used for reduction or increase is the ratio between the actual value and the target value and this factor is limited by user-specified minimum and maximum factors (defaults to 0.1 and 10 respectively). If this type of load step control is used together with the recycle based control, the time step can be reduced in the current increment due to whichever criterion that is violated. The decision to increase the step size for the next increment is solely based upon the physical criteria. Specification of user-defined physical criteria can be further simplified by setting a special flag in the AUTO STEP option that allows for physical criteria to be automatically added by the solver at run-time. These automatic criteria serve as upper-bound controls to prevent run-away Newton-Raphson iterations that ultimately cause the program to abort. Currently, four mechanical criteria are automatically added depending on the kind of analysis that is being run: a total strain criterion is added for any large displacement analysis and the maximum allowable equivalent total strain increment at any point in the model is set to 50%; a plastic strain criterion is added for any large displacement, finite strain analysis and the maximum allowable equivalent plastic strain increment at any point in the model is set to10%; a relative creep strain criterion and a relative stress change criterion are added for any explicit creep analysis wherein the maximum allowable creep strain change/elastic strain and the maximum allowable equivalent stress change/equivalent stress are each set to 0.5; a state variable criterion is added for any large displacement analysis wherein the maximum allowable temperature increment is such that the equivalent stress increment associated with the change in thermal properties of the materials does not exceed 50% of the total equivalent stress. These criteria are only added in the analysis if there are no competing explicitly defined user-criteria found. It should also be noted that these automatic criteria are only used as limits; i.e. they are used to control the time step within an increment but not for the next increment. Failure to satisfy user-defined physical criteria can occur due to two reasons — the maximum number of cutbacks allowed by the user can be exceeded, or the minimum time step can be reached. In this case, the analysis terminates with exit 3002 and exit 3015, respectively. These premature terminations can be avoided by using the option to continue the analysis even if physical criteria are not satisfied. If this flag

Main Index

686 Marc Volume A: Theory and User Information

is set on the AUTO STEP option, and either the maximum number of user-allowed cutbacks or the minimum time step is reached, a mechanical analysis moves on to the next increment if it is otherwise converged (see Convergence Controls in this chapter) or continues to recycle and scales back based solely on the recycling criterion. Setting this flag for a thermal analysis simply allows it to move on to the next increment. User Programmed Time Steps Selection In addition to controlling the time step through the recycle based criterion and the physical criteria, direct control of the time step is possible through the use of the UTIMESTEP user subroutine. In this case, the new time step that is determined by the auto step algorithm enters the program as input and the modified time step by the user is returned as output. More details are provided in Marc Volume D: User Subroutines and Special Routines, Chapter 2. Post Files Output In many analyses it is convenient to obtain post file results at specified time intervals. This is naturally obtained with a fixed load stepping scheme but not with an automatic scheme. Traditionally, the post output frequency is given as every nth increment. With the AUTO STEP history definition option, you can request post output to be obtained at equally spaced time intervals. In this case, the time step is temporarily modified to exactly reach the time for output. The time step is then restored in the following increment. Table Considerations When tables are used in the new input format to specify loads with complex time variations, in most cases, it is important that the exact peaks and valleys of the loading history are not missed due to the adaptive time stepping. By default, AUTO STEP adjusts the time step temporarily so that the peaks and valleys of the loading history are reached exactly. The time step is then restored in the following increment. In analyses where the boundary conditions are obtained from experimental data containing many points, it is often useful to turn this behavior off, in which case large time steps will be achieved and the load will be smoothed out. Quasi-Static Damping Scheme The AUTO STEP option also has an optional artificial damping feature available for mechanical statics analyses. Damping Energy A comparison between the incremental strain energy and the estimated damping energy is used as a criteria for time step control when either a 4 or 5 is given on the 10th field of the 2nd data block (idampit flag).The criteria based upon the number of cycles is bypassed. Decisions to decrease and increase the time step are based on the damping energy rate of the system. Furthermore, if a 4 is entered, then artificial damping is added to the system. The details of the time stepping procedure and the damping procedure are as follows:

Main Index

CHAPTER 11 687 Solution Procedures for Nonlinear Systems

A damping factor, F d , is introduced, which at the start of the loadcase, is set to 0. The time step for the first increment is set equal to the user given initial time step. During the first cycle of the loadcase, a “small” strain energy value ΔE s m a l l is calculated as ΔE s m a l l =

∫ 0.5D ( 1, 1 )ε ( 1 ) 2 dV V

where D ( 1, 1 ) is the first component of the stress-strain relation at the integration point and E ( 1 ) is 10-6. This small energy value is used later to distinguish between real deformations of the structure and zero-energy modes. During the assembly of the stiffness matrix K and the right-hand side vector F , the following contributions are added to K and F , respectively. K d a m p = F d M ⁄ timinc F da m p = F d Mdu ⁄ timinc where M is the lumped mass matrix, du is the incremental displacement and timinc is the time increment. Note that when F d = 0 , there is no change to the equations. During the recovery phase, the incremental damping energy for the nth iteration is calculated as n

ΔE d a m p = du T Mdu ⁄ timic when F d = 0 and as n

ΔE d a m p = F d Mdu ⁄ timinc when F d is not 0 . The check to determine if the time-step should be reduced through a cut-back is made as follows: If F d = 0 , perform a cutback if 1

n

ΔE > ΔE sm a l l and ΔE d m a p > 4ΔE d a m p where ΔE is the incremental strain energy. The time step reduction factor in this case is given by fr e d u c =

1

(n)

ΔE d a m p ⁄ ΔE d a m p

Such a cutback is triggered in the first increment of the loadcase in the case of severe non-linearities, as expressed by the fact that the damping energy for the nth iteration deviates considerably from that of the first iteration.

Main Index

688 Marc Volume A: Theory and User Information

If F d is not 0 , perform a cutback if n

n

ΔE d a m p > 4ΔE p r e d i c t e d and ΔE d a m p > ΔE m a x and tol > 2 where ΔE p r e d i c t e d is the predicted damping energy for the current increment, ΔE m a x is the maximum damping energy in any previously converged increment and tol is the global user-defined convergence tolerance. The reduction factor in this case is set to 0.5. This cut-back is triggered in the case where the solution is clearly diverging and avoids unnecessary recycles. The same reduction factor (0.5) is also used for cases when the maximum number of iterations are reached or when user criteria are violated. For the first increment of the loadcase, the calculation of F d and predicted energy is as follows: • Estimated strain energy for the loadcase E e s t i m a t e d = ΔE timinc 2 • E m a x = max ( E e st i m a t e d ,E ) , where E = total strain energy in system . n

• Estimated damping energy for the loadcase E d a m p _ e s t i m a t e d = ΔE d a m p totinc ⁄ timinc , where totinc = total time period . • F d = δE m a x ⁄ E d a m p _ e st i m a t e d where δ is a user-defined factor. Recommended default value is 10-4. • Predicted damping energy for next increment n

ΔE p r e d i c t e d = F d ΔE d a m p timincnew ⁄ timincold where timincnew is the time step for the next increment and timincold is the time increment for the previous increment. n

n

• Set ΔE p r e v = F d ΔE d a m p ⁄ timinc and ΔE m a x = F d ΔE d a m p For subsequent increments of the loadcase, the modification of F d and the time step is as follows: • If the total strain energy E is larger than twice the estimated strain energy E e s t i m a t e d , then Fd = Fd E ⁄ Ee s t i m a t e d . n

• If ΔE d a m p ⁄ timinc < 1.1ΔE p r e v , then increase the time step by a factor of 1.5. Avoiding Exit 3015 When the minimum time step t m i n is reached, Marc normally exits with 3015. If the quasi-static damping schemes (10th field, 2nd data block) is a 0 or 1, a quasi-static damping option is triggered in an attempt to avoid this premature exit: When exit 3015 is encountered for the first time, the increment is repeated with a new time step given by t n e w = fclrg t m i n , where fclrg is the maximum ratio between steps (4th field of the 2nd data block of the AUTO STEP option = 10 by default). The increment is further

Main Index

CHAPTER 11 689 Solution Procedures for Nonlinear Systems

stabilized by added the factored lumped mass matrix to the stiffness matrix and modifying the force vector consistently. The damping factor associated with the lumped mass matrix is again based on the ratio of the estimated strain energy to the estimated damping energy in a manner similar to the idampit = 4 scheme. If exit 3015 is again encountered, a second attempt is made with t n e w = fclrg2 t m i n and again stabilizing the incremental solution by adding the quasi-static damping in the solution. It should be noted that this procedure is not available for the first increment of the auto step loadcase since the damping factor is only calculated after the first increment is completed. It should also be noted that once exit 3015 is encountered and damping is turned on, it remains on for the rest of the loadcase. Auto Step for Transient Dynamics The AUTO STEP algorithm is further modified for transient dynamics problems: • When penetration is detected in dynamic contact problems, instead of using the default iterative penetration procedure, a time cutback is made and the increment is repeated with a smaller time step that avoids the penetration. This scheme allows for momentum conservation without spurious penetration induced oscillations in the response. If no other cutbacks are made, the time step is restored in the following increment. • Additional, optimal checks are available in transient dynamic problems to control the time step since larger time steps that may have been assessed based on the recycle based criterion or physical criteria can give rise to unacceptable time integration errors. The time integration error check is only turned on if the 13th field of the 3rd data block of the AUTO STEP option is set to 1. If this field is not present or set to 0, the time integration error check is skipped and the time stepping algorithm for dynamic problems is then similar to that of static problems. If the check is turned on, an additional check is made at the end of each increment to see if the time step needs to be reduced for the following increment. This check is only made for the Newmark-Beta (NB) and the Single Step Houbold (SSH) methods. The scheme that is followed is a modified version of the scheme outlined by Bergan and Mollestad [Ref. 1]. The time step for increment n + 1 should satisfy the inequality Δu nT MΔu n ( Δt ) n + 1 ≤ 2πα --------------------------------Δu nT K T Δu n where Δu n is the incremental displacement vector at increment n ; M is the mass matrix; K T is the tangent stiffness matrix, and α is a user-customizable scaling factor. The default value of α is as follows: for the SSH operator α = 0.375 * fcsml . and for the NB operator α = 0.75 * fcsml , where fcsml is the smallest ratio between time steps (3rd field of the 2nd data block of the AUTO STEP option = 0.1 by default). The smaller default value of α = 0.0375 for SSH

problems compared to α = 0.075 for NB problems is to better control the artificial damping inherent in the SSH method. The user can control the accuracy of the solution by changing

Main Index

690 Marc Volume A: Theory and User Information

fcsml . The time step is only reduced if the value predicted by the above equation is less than 67% of the current time step. The check is bypassed if t n + 1 is already at t m i n , if the strain energy is negligible (for example, rigid body motion). When there are multiple loadcases in a transient dynamic run and the time integration error check is flagged for all of them, the initial time step of a loadcase that follows a transient dynamic loadcase is also adjusted if it is too high compared to the time step predicted by the error check. This avoids accuracy problems associated with using an initial user-prescribed time step that is too large. The defaults of the AUTO STEP option are carefully chosen to be adequate in a wide variety of applications. There are cases, however, when the settings may need to be modified. Assume that the default settings are used, which means that the recycle based control is active with an initial load of one per cent of the total. If the structure is weakly nonlinear, convergence is obtained in just a few recycles and the time steps for successive increments get progressively larger. This can lead to problems if the initially weakly nonlinear structure suddenly exhibits stronger nonlinearities; for instance, occurrence of plasticity or parts coming into contact. Possible remedies to this problem include: a. b. c. d.

decrease the time step scale factor to a smaller number so the step size does not grow so rapidly; use a physical criterion like maximum increment of displacements to limit the load step; use the maximum time step to limit large steps; decrease the desired and maximum number of recycles to decrease the load step if more recycles are needed.

Another situation is if the structure is highly nonlinear and convergence is slow. In this case, it may be necessary to increase the desired number and maximum number of recycles. In general, there is a close connection between the convergence tolerances used and the desired number and maximum number of recycles. In many cases, it may be beneficial to use one or more physical criteria; for example, the increment of plastic strain as targets for controlling the load step. This can easily be achieved by allowing the program to add automatic physical criteria where appropriate. This is especially a good idea if the ‘proceed if not converged’ option is used or if the ‘non-positive definite flag’ is set since the added physical criteria then serve as controls to limit the time step and produce a realistic numerical solution in each increment rather than letting the solution proceed unchecked with unrealistic results.

Residual Load Correction The residual load is applied as a correcting force to ensure that equilibrium is maintained and, hence, that an accurate solution is obtained for nonlinear problems. The residual load correction enforces global equilibrium at the start of each new increment. This prevents the accumulation of out-of-equilibrium forces from increment to increment and makes the solution less sensitive to the step size. Figure 11-2 shows how stiffness is based on the state at the start of a step. The variables are defined below for increments i = 1,2,3: • F i applied forces for i = 1,2,3 • u i calculated displacements for i = 1,2,3 • R i residual loads for i = 1,2,3

Main Index

CHAPTER 11 691 Solution Procedures for Nonlinear Systems

F3 F2 F1

R3 R2

R1

U1

U2

U3

Figure 11-2 Stiffness Based on State at Start of Step

The residual load correction is the difference between the internal forces and the externally applied loads. The residual load correction is expressed as R = P – ∫ β T σdV

(11-2)

where β is the differential operator which transforms displacements to strains, σ is the current generalized stresses, P is the total applied load vector, and R is the residual load correction. In order to evaluate the residual load correction accurately, evaluate the integral by summing the contributions from all integration points. The residual load correction feature requires that stresses be stored at all the integration points. Data storage at all integration points is the default in Marc, but can be overridden in linear analysis by use of the CENTROID parameter. Residual load correction should always be used unless the ELASTIC parameter is invoked; this is the default.

Restarting the Analysis The RESTART model definition option creates a restart file for the current analysis which can be used in subsequent analyses. It can also be used to read in a previously generated file to continue the analysis. The RESTART option is very important for any multi-increment analysis because it allows you to continue the analysis at a later time. The default situation writes the restart information to unit 8 and reads a previously generated file from unit 9. For post processing, the RESTART option can be used to plot or combine load cases (see CASE COMBIN). Upon restart, you can use the model definition REAUTO option to redefine parameters associated with an automatic load sequence. To save storage space, it is not necessary to store each increment of analysis. The frequency can be set using the RESTART option, and subsequently modified using the RESTART INCREMENT option. It is also possible to store only the last converged solution by using the RESTART LAST option. This should not be used with elastic analysis because the stiffness matrix is not stored.

Main Index

692 Marc Volume A: Theory and User Information

Full Newton-Raphson Algorithm The basis of the Newton-Raphson method in structural analysis is the requirement that equilibrium must be satisfied. Consider the following set of equations: K ( u )δu = F – R ( u )

(11-3)

where u is the nodal-displacement vector, F is the external nodal-load vector, R is the internal nodalload vector (following from the internal stresses), and K is the tangent-stiffness matrix. The internal nodal-load vector is obtained from the internal stresses as R =

∑ ∫β

T

σ dv

(11-4)

elem V

In this set of equations, both R and K are functions of u . In many cases, F is also a function of u (for example, if F follows from pressure loads, the nodal load vector is a function of the orientation of the structure). The equations suggest that use of the full Newton-Raphson method is appropriate. i

Suppose that the last obtained approximate solution is termed δu , where number. Equation (11-3) can then be written as i–1

i

indicates the iteration

i–1

K ( u n + 1 )δu = F – R ( u n + 1 )

(11-5)

i

This equation is solved for δu and the next appropriate solution is obtained by i

Δu = Δu

i–1

i

i

+ δu and u n + 1 = u n + Δu

i

Solution of this equation completes one iteration, and the process can be repeated. The subscript

(11-6) n

denotes the increment number representing the state t = n . Unless stated otherwise, the subscript n + 1 is dropped with all quantities referring to the current state. The full Newton-Raphson method is the default in Marc (see Figure 11-3). The full Newton-Raphson method provides good results for most nonlinear problems, but is expensive for large, three-dimensional problems, when the direct solver is used. The computational problem is less significant when the iterative solvers are used.

Main Index

CHAPTER 11 693 Solution Procedures for Nonlinear Systems

r1 Fn + 1

Fn

Force δu1

Solution Converged

Δu1 Δu2 Δu3 Incremental Displacements

0

Figure 11-3 Full Newton-Raphson

Modified Newton-Raphson Algorithm The modified Newton-Raphson method is similar to the full Newton-Raphson method, but does not reassemble the stiffness matrix in each iteration. 0

i

K ( u )δu = F – R ( u

i–1

)

(11-7)

Fn + 1 r1 Fn

Force

δu1 Solution Converged

0

Δu1 Δu2 Δu5 Incremental Displacements

Figure 11-4 Modified Newton-Raphson

The process is computationally inexpensive because the tangent stiffness matrix is formed and decomposed once. From then on, each iteration requires only forming the right-hand side and a backward substitution in the solution process. However, the convergence is only linear, and the potential for a very large number of iterations, or even nonconvergence, is quite high. If contact or sudden material nonlinearities occur, reassembly cannot be avoided. The modified NewtonRaphson method is effective for large-scale, only mildly nonlinear problems. When the iterative solver is employed, simple back substitution is not possible, making this process ineffective. In such cases, the full Newton-Raphson method should be used instead.

Main Index

694 Marc Volume A: Theory and User Information

If the load is applied incrementally, Marc recalculates the stiffness matrix at the start of each increment or at selected increments, as specified.

Strain Correction Method The strain correction method is a variant of the full Newton method. This method uses a linearized strain calculation, with the nonlinear portion of the strain increment applied as an initial strain increment in subsequent iterations and recycles. This method is appropriate for shell and beam problems in which rotations are large, but membrane stresses are small. In such cases, rotation increments are usually much larger than the strain increments, and, hence, the i+1

nonlinear terms can dominate the linear terms. After each displacement update, the new strains E α β i

i

are calculated from u and δu ( = δ u ) which yield i+1

Eα β

i i 1 = E α β + --- ( δ u α, β + δu β, α ) + u κ, α δu κ, β + δu κ, α u κi β + δu κ, α δu κ, α 2

(11-8)

This expression is linear except for the last term. Since the iteration procedures start with a fully linearized calculation of the displacement increments, the nonlinear contributions yield strain increments inconsistent with the calculated displacement increments in the first iteration. These errors give rise to either incorrect plasticity calculations (when using small strain plasticity method), or, in the case of elastic material behavior, yields erroneous stresses. These stresses, in their turn, have a dominant effect on the stiffness matrix for subsequent iterations or increments, which then causes the relatively poor performance. The remedy to this problem is simple and effective. The linear and nonlinear part of the strain increments are calculated separately and only the linear part of i i i l 1 ( E αβ ) = E α β + --- ( δu α, β + δu β, α ) + u κ, α δu κ, β + δu κ, α u κ β 2

(11-9)

is used for calculation of the stresses. The nonlinear part nl

( E αβ )

i+1

1 = --- δu κ, α δu κ, β 2

(11-10)

is used as an “initial strain” in the next iteration or increment, which contributes to the residual load vector defined by R

C

=

∫

δ κ, β X κ, α L

αβ γ δ

nl

ΔE γ δ dV

(11-11)

V0

This “strain correction” term is defined by i

i

K ( u n + 1 )δu = F – R ( u n + 1 ) – R

Main Index

C

(11-12)

CHAPTER 11 695 Solution Procedures for Nonlinear Systems

Since the displacement and strain increments are now calculated in a consistent way, the plasticity and/or equilibrium errors are greatly reduced. The performance of the strain correction method is not as good if the displacement increments are (almost) completely prescribed, which is not usually the case. Finally, note that the strain correction method can be considered as a Newton method in which a different stiffness matrix is used.

Direct Substitution In the Eulerian formulation (R-P FLOW parameter), the governing equation of the system can be expressed as (11-13)

Kv = F where v is a velocity vector, and F is a force vector.

This equation is very nonlinear because K is a nonlinear function of v . By default, a direct substitution i

method is used to solve the problem. If v is the velocity at iteration i , the result of iteration i + 1 is i

K( v ) v

i+1

(11-14)

= F

If this method does not converge in 10 iterations, it is possible to switch into a full Newton-Raphson method.

Arc-length Methods The solution methods described above involve an iterative process to achieve equilibrium for a fixed increment of load. Besides, none of them have the ability to deal with problems involving snap-through and snap-back behavior. An equilibrium path as shown in Figure 11-5 displays the features possibly involved.

2

6

F

3

Force 4 5 u Displacements Figure 11-5 Snap-through Behavior

Main Index

696 Marc Volume A: Theory and User Information

The issue at hand is the existence of multiple displacement vectors, u , for a given applied force vector, F . The arc-length methods provide the means to ensure that the correct displacement vector is found by Marc. If you have a load controlled problem, the solution tends to jump from point 2 to 6 whenever the load increment after 2 is applied. If you have a displacement controlled problem, the solution tends to jump from 3 to 5 whenever the displacement increment after 3 is applied. Note that these problems appear essentially in quasi-static analyses. In dynamic analyses, the inertia forces help determine equilibrium in a snap-through problem. Thus, in a quasi-static analysis sometimes it is impossible to find a converged solution for a particular load (or displacement increment): λ n + 1 F – λ n F = ΔλF This is illustrated in Figure 11-5 where both the phenomenon of snap-through (going from point 2 to 3) and snap-back (going from point 3 to 4) require a solution procedure which can handle these problems without going back along the same equilibrium curve. As shown in Figure 11-6, assume that the solution is known at point A for load level λ n F . For arriving at point B on the equilibrium curve, you either reduce the step size or adapt the load level in the iteration process. To achieve this end, the equilibrium equations are augmented with a constraint equation expressed typically as the norm of incremental displacements. Hence, this allows the load level to change from iteration to iteration until equilibrium is found. g

λn + 1 F

B λn F

A r

F

u Figure 11-6 Intersection of Equilibrium Curve with Constraining Surface

The augmented equation, c ( u, λ ) , describes the intersection of the equilibrium curve with an auxiliary surface g for a particular size of the path parameter η : r ( u, λ ) = λF – R ( u ) = 0 (11-15) c ( u, λ ) = g ( u, λ ) – Δη = 0 Variations of the parameter η moves the surface whose intersection with the equilibrium curve r generates a sequence of points along the curve. The distance between two intersection points, denoted with η 0 and η , denoted by l is the so-called arc-length.

Main Index

CHAPTER 11 697 Solution Procedures for Nonlinear Systems

Linearization of Equation (11-15) around point A in Figure 11-6 yields: K P ⎧ δu ⎫ ⎧ –r ⎫ ⎨ ⎬ = ⎨ –r ⎬ T n n 0 ⎩ δλ ⎭ ⎩ 0⎭

(11-16)

where: ∂r ∂r K = ------ : P = -----∂u ∂λ n

(11-17)

∂c ∂c = ------ : n 0 = -----∂u ∂λ

T

(11-18)

r = λF – R

(11-19)

r 0 = g ( u, λ ) – Δη

(11-20)

It can be noted that a standard Newton-Raphson solution procedure is obtained if the constraint condition is not imposed. The use of the constraint equation causes a loss of the banded system of equations which would have been obtained if only the K matrix was used. Instead of solving the N + 1 set of equations iteratively, the block elimination process is applied. Consider the residual at iteration i to which the fraction of load level λ i

r (λ

i–1

) = λ

i–1

i

F – R (u

i–1

)

i–1

corresponds (11-21)

i

The residual for some variation of load level, δλ , becomes i

r (λ

i–1

i

i

i

+ δλ ) = δλ F + r ( λ

i–1

)

(11-22)

which can be written as: i

δu ( λ

i–1

i

where δu ( λ and

i

i

+ δλ ) = δu ( λ i–1

i–1

i

i

) + δλ δu *

i –1

) = (K ) r

(11-24)

i –1

i

(11-23)

δu * = ( K ) F

(11-25)

i

Notice that δu * does not depend on the load level. The equation above essentially establishes the i

influence of a change in the load level δλ during one iteration on the change in displacement increment for that iteration. After one iteration is solved, this equation is used to determine the change in the load level such that the constraint is followed. There are several arc-length methods corresponding to different constraints.

Main Index

698 Marc Volume A: Theory and User Information

11

Among them, the most well-known arc-length method is one proposed by Crisfield, in which the iterative solution in displacement space follows a spherical path centered around the beginning of the increment. This requirement is translated in the formula:

Solution Procedu res for Nonlinea r Systems

c = l

2

i

= Δu Δu

i

(11-26)

where l is the arc length. The above equation with the help of Equations (11-25) and (11-26) is applied as: i T

i 2

i

i–1

+ δu ( λ

i–1

+ δu ( λ

[ ( δu * ) δu * ] ( δλ ) + [ 2 ( Δu [ ( Δu

i–1

i

+ δu ( λ

i–1

T

) ) ( Δu

i

i–1

i

i–1

T

i

i

) ) δu * ] ( δλ ) +

(11-27)

2

)) – l ] = 0

The equation above is interpreted with i = 1 and δu

1

= 0 in the prediction phase while retaining the

full form of Equation (11-27) in the correction phase. Two solutions for δλ are available. There are several methods to determine which root to select. By default, we choose the one that maintains a positive angle of the displacement increment from one iteration to the next. i

i

The two roots of this scalar equation are ( δλ ) 1 and ( δλ ) 2 . To avoid going back on the original loaddeflection curve, the angle between the incremental displacement vectors, Δu

i–1

i

and Δu (before and i

after the current iteration, respectively) should be positive. Two alternative values of Δu (namely, i

i

i

i

( Δu ) 1 and ( Δu ) 2 corresponding to ( δλ ) 1 and ( δλ ) 2 are obtained and the cosine of two corresponding angles ( φ 1 and φ 2 ) are given by T

i

cos φ 1

i–1

[ ( Δu n + 1 ) 1 ] Δu n + 1 = ---------------------------------------------------l T

i

and cos φ 2

(11-28)

i–1

[ ( Δu n + 1 ) 2 ] Δu n + 1 = ---------------------------------------------------l

(11-29) 0

Once again, the prediction phase is interpreted with i = 1 and Δu n + 1 = Δu n , while Equations (11-28) and (11-29) retain their full form in the correction phase. i

i

As mentioned earlier, the appropriate root, ( δλ ) 1 or ( δλ ) 2 is that which gives a positive cos φ . In case both the angles are positive, the appropriate root is the one closest to the linear solution given as: i–1

i

i–1

i

2

i ( Δu + δu ) ( Δu + δu ) – l δλ = -------------------------------------------------------------------------------------i i–1 i + δu )δu * 2 ( Δu

(11-30)

Crisfield’s solution procedure, generalized to an automatic load incrementation process, has been implemented in Marc as one of the options under the AUTO INCREMENT history definition option. Various components of this process are shown in Figure 11-7.

Main Index

CHAPTER 11 699 Solution Procedures for Nonlinear Systems

F

–1 2 2 1 δu ( λ ) = K 2 f Force

r1

1 1 0 λ ( Δu * ) ( Δu * )

Incremental Displacement

2

( δu * ) Figure 11-7 Crisfield’s Constant Arc Length

The constraints in Equations (11-26) and (11-27) are imposed at every iteration. Disadvantage of the quadratic equation suggested by Crisfield is the introduction of an equation with two roots and thus the need for an extra equation to solve the system for the calculated roots if two real roots exists. This 1

1

situation arises when the contribution Δu (or δu ) is very large in comparison to the arc-length. This can be avoided in most cases by setting sufficiently small values of the error tolerance on the residual force. In case the above situation still persists despite the reduction of error tolerance, Marc has two options to proceed: a. To attempt to continue the analysis with the load increment used in the initial step of auto increment process. b. Use the increment resulting from the linear constraint for the load. There are two alternate methods using the Crisfield method for selecting the roots: • Singularity ratio method; where if the system of equations is positive definite, the largest root is used; while if the system was negative, the smallest root is used. • Falzon’s method described in Reference 7 is applicable for problems which have multiple nearly equal buckling modes. This is circumvented in Ramm’s procedure due to the linearization. Another approach to impose the constraint is due to Ramm, who also makes use of a quadratic equation to impose the constraint giving rise to the Riks-Ramm method. The difference is that while Crisfield imposes the constraint as a quadratic equation, Ramm linearized the constraint. Geometrically, the difference between the two methods is that the Crisfield method enforces the correction on the curve of the augmented equation introducing no residual for the augmented equation. Ramm takes the intersection between the linearizations of the curves which gives a residual of the augmented equation for the next step. Both methods converge to the same solution, the intersection of the two curves, unless approximations are made.

Main Index

700 Marc Volume A: Theory and User Information

The Riks-Ramm constraint is linear, in that: c = l

2

= Δu n Δu n + 1

which results in a linear equation for δλ : T

i

i

Δu n ( δu + δλ δu * ) = l

2

Thus, the load parameter predictor is calculated as: 1 δλ n + 1

T

i –1 i

Δu n l – ( Δu n ) [ ( K ) r ] = ---------------------------------------------------------------------1 T Δu n ( δu * )

(11-31)

while during the corrector phase it is: i

i δλ n + 1

T

i –1 i

( Δu n + 1 ) [ ( K ) r ] = – ---------------------------------------------------i T i ( Δu n + 1 ) ( δu * )

(11-32)

It is noted that in the definition of the constraint, the normalized displacement of the previous step is used ∂c for the normal to the auxiliary surface ------ = n . Thus, problems can arise if the step size is too big. In ∂u situations with sharp curvatures in the solution path, the normal to the prediction may not find intersections with the equilibrium curve. Note that the norm of the displacement increment during the iterations is not constant in Riks-Ramm method. In contact problems, sudden changes of the stiffness can be present (due to two bodies which are initially not in contact suddenly make contact). Hence, a potential problem exists in the Riks-Ramm method if i

the inner-product of the displacement due to the load vector δu * and the displacement increment Δu n is small. This could result in a very large value of the load increment for which convergence in the subsequent iterations is difficult to achieve. Therefore, a modified predictor can be used resulting in a modified Riks-Ramm procedure as: 1

Δλ

1

1 T

1

l n – 1 δu – [ αδu * ] δu * = ----------------------------------------------------------------1 1 [ αδΔu * ]Δu *

(11-33)

where T

i

Δu n δu * α = ------------------------T i Δu n δu *

(11-34)

This method effectively scales the load increment to be applied in the prediction and is found to be effective for contact problems.

Main Index

CHAPTER 11 701 Solution Procedures for Nonlinear Systems

Refinements and Controls The success of the methods depend on the suitable choice of the arc-length: C = l

2

The initial value of the arc-length is calculated from the initial fraction β of the load specified by you in the following fashion: Kδu = βF – R 2

li n i =

Δu

(11-35) (11-36)

In subsequent steps the arc-length can be reduced or increased at the start of a new load step depending on the number of iterations I 0 in the previous step. This number of iterations in compared with the desired number of iterations I d which is typically set to 3 or 5. The new arc-length is then given by: rt = I d ⁄ I o

(11-37) 2

2

l new = rt ⋅ l p r e v Often, this results in too large of an arc-length growth, especially initially when the system is nearly linear and I o is small (often one). In this case, one can gradually grow the value as: l n e w = sf ⋅ l p re v sf = .1

if rt ≤ .1

sf = 1

if .1 < rt < 1

sf = 1.25

if 1 < rt ≤ 3

sf = 1.5

if 3 ≤ rt

Two control parameters exist to limit the maximum enlargement or the minimum reduction in the arc-length. 2

l min < ------- < max 2 l ini

(11-38)

The min and max defined here are the 7th and 5th field of the 2nd data block. It is also possible that the maximum fraction of the load allowed can vary during the loadcase. This is often useful if one knows that one is approaching the limit load.

Main Index

702 Marc Volume A: Theory and User Information

In addition, the maximum fraction of the total load may be defined. In general, control on the limiting values with respect to the arc-length multiplier is preferred in comparison with the maximum fraction of the load to be applied in the iteration since a solution is sought for a particular value of the arc-length. Also, attention must be paid to the following: 1. In order to tract snap-through problems, the method of allowing solution if the stiffness matrix becomes nonpositive needs to be set. 2. The maximum number of iterations must be set larger than the desired number of iterations.

Convergence Controls The default procedure for convergence criterion in Marc is based on the magnitude of the maximum residual load compared to the maximum reaction force. This method is appropriate since the residuals measure the out-of-equilibrium force, which should be minimized. This technique is also appropriate for Newton methods, where zero-load iterations reduce the residual load. The method has the additional benefit that convergence can be satisfied without iteration. The basic procedures are outlined below. 1. RESIDUAL CHECKING F r e si d u a l ∞ ------------------------------< TOL 1 F re a c t i o n ∞

(11-39)

F r e si d u a l ∞ M r e si d u a l ∞ ------------------------------< TOL 1 and --------------------------------- < TOL 2 F re a c t i o n ∞ M re a c t i o n ∞

(11-40)

F r e si d u a l

∞

< TOL 1

F r e si d u a l

∞

< TOL 1 and M r e si d u a l

(11-41) ∞

< TOL 2

(11-42)

Where F is the force vector, and M is the moment vector. TOL 1 and TOL 2 are control tolerances. F

∞

indicates the component of F with the highest absolute value. Residual

checking has two drawbacks. First, if the CENTROID parameter is used, the residuals and reactions are not calculated accurately. Second, in some special problems, such as free thermal expansion, there are no reaction forces. The program uses displacement checking in either of these cases. 2. DISPLACEMENT CHECKING

Main Index

δu ∞ --------------- < TOL 1 Δu ∞

(11-43)

δu ∞ δφ ∞ --------------- < TOL 1 and --------------- < TOL 2 Δu ∞ Δφ ∞

(11-44)

CHAPTER 11 703 Solution Procedures for Nonlinear Systems

δu

∞

δu

< TOL 1 ∞

(11-45)

< TOL 1 and δφ

∞

< TOL 2

(11-46)

where Δu is the displacement increment vector, δu is the correction to incremental displacement vector, Δφ is the correction to incremental rotation vector, and δφ is the rotation iteration vector. With this method, convergence is satisfied if the maximum displacement of the last iteration is small compared to the actual displacement change of the increment. A disadvantage of this approach is that it results in at least one iteration, regardless of the accuracy of the solution. Correction to incremental displacements of ith iteration

δi

Displacements at increment n

un

F

δ0

i

δ ---------------- ≤ Tolerance

δ1 δk

0 un + 1

u

k+1 n+1

i

∑

δj

j = 0

u

Figure 11-8 Displacement Control

3. STRAIN ENERGY CHECKING This is similar to displacement testing where a comparison is made between the strain energy of the latest iteration and the strain energy of the increment. With this method, the entire model is checked. δE ------- < TOL 1 ΔE

(11-47)

where ΔE is the strain energy of the increment and δE is the correction to incremental strain energy of the iteration. These energies are the total energies, integrated over the whole volume. A disadvantage of this approach is that it results in at least one iteration, regardless of the accuracy of the solution. The advantage of this method is that it evaluates the global accuracy as opposed to the local accuracy associated with a single node. Different problems require different schemes to detect the convergence efficiently and accurately. To do this, the following combinations of residual checking and displacement checking are also available. 4. RESIDUAL OR DISPLACEMENT CHECKING This procedure does convergence checking on both residuals (Procedure 1) and displacements (Procedure 2). Convergence is obtained if one converges. 5. RESIDUAL AND DISPLACEMENT CHECKING This procedure does a convergence check on both residuals and displacements (Procedure 4). Convergence is achieved if both criteria converge simultaneously.

Main Index

704 Marc Volume A: Theory and User Information

In several types of analyses, maximum reactions or displacements are extremely small (even close to the round-off errors of computers). In such circumstances, not all types of relative convergence criteria may work properly. For example, in a problem with stress-free motion, the convergence check based on relative displacement increments works correctly but not the convergence check based on relative residual or strain energy. In this situation, it is necessary to check the convergence with absolute values of reactions or strain energy; otherwise, the analysis may terminate prematurely. Similarly, this kind of situation may happen for problems with springback and free thermal expansion or constraint thermal expansion. The details for the cases where convergence checking with relative values may encounter difficulties are listed in Table 11-2. The AUTO SWITCH option is designed for Marc to switch to the proper convergence check scheme automatically if any of the situations mentioned above occur during the analysis. The AUTO SWITCH option allows Marc to automatically switch the convergence check scheme to check as required on either residuals or displacements if small reactions or displacements are detected, or to use the absolute strain energy checking if necessary. Table 11-2

Effectiveness of various Relative Tolerance Convergence Testing Criterion

Convergence Variable Displacement/ Rotation

Residual Force/Torque

Strain Energy

Stress-free motion

Yes

No

No

Springback

No

Yes

No

Free Thermal Expansion

Yes

No

No

Constraint Thermal Expansion

No

Yes

Yes

Analysis Type

Yes – relative tolerance testing works. No – relative tolerance testing does not work.

If AUTO SWITCH is turned on, it: 1. Switches on the relative residual checking if the relative displacement criterion is used (which fails when the maximum incremental displacement becomes very small Max._incremental_displacement/Smallest_element_size<1.0e-6)

2. Switches on the relative displacement checking if the relative residual force (moment) criterion is used (which fails when the maximum reaction force becomes very small <1.0e-8) 3. To switch on the absolute energy checking if the structure is free of stress and deformation (strain energy density < 1.0e-15). Notes: 1. If any criterion with absolute value testing is being used as convergence checking, this feature is deactivated. 2. If the combined convergence check scheme with relative displacements or residuals is chosen as convergence criterion, it is not necessary to turn the AUTO SWITCH on. 3. Once the extreme cases disappear in the analysis, Marc recovers to use the convergence criteria given by user.

Main Index

CHAPTER 11 705 Solution Procedures for Nonlinear Systems

Singularity Ratio The singularity ratio, R , is a measure of the conditioning of the system of linear equations. R is related to the conditioning number, C , which is defined as the ratio between the highest and lowest eigenvalues in the system. The singularity ratio is an upper bound for the inverse of the matrix conditioning number. 1⁄R≤C

(11-48)

C and R establish the growth of errors in the solution process. If the errors on the right-hand side of the equation are less than E prior to the solution, the errors in the solution will be less than δ , with δ ≤ CE

(11-49)

The singularity ratio is a measure that is computed during the Crout elimination process of Marc using the direct solver. In this process, a recursive algorithm redefines the diagonal terms (k) Kk k

=

(k – 1) Kk k

k–1

∑

–

1 ≤i≤k–1

Km k Km k

(11-50)

m = i

where i is a function of the matrix profile. K k k is a diagonal of the kth degree of freedom. The singularity ratio is defined as (k)

(k – 1)

R = min K k k ⁄ K k k (k)

(k – 1)

If all K k k and K k k

(11-51)

are positive, the singularity ratio indicates loss of accuracy during the Crout

elimination process. This loss of accuracy occurs for all positive definite matrices. The number of digits lost during the elimination process is approximately equal to n l o s t = – log 10 R

(11-52)

The singularity ratio also indicates the presence of rigid body modes in the structure. In that case, the (k)

elimination process produces zeros on the diagonal K k k ≅ 0 . Exact zeros never appear because of numerical error; therefore, the singularity ratio is of the order R = O ⎛ 10 ⎝

– nd i g i t

⎞ ⎠

(11-53)

where n digit is the accuracy of floating-point numbers used in the calculation. For most versions of Marc, (k)

n digit > 12 . If rigid body modes are present, K k k is very small or negative. If either a zero or a negative diagonal is encountered, execution of Marc is terminated because the matrix is diagnosed as being singular.

Main Index

706 Marc Volume A: Theory and User Information

You can force the solution of a nonpositive definite or singular matrix. In this case, Marc does not stop (k)

when it encounters a negative or small term K k k on the diagonal. If you use Lagrangian multiplier elements, the matrix becomes nonpositive definite and Marc automatically disables the test on the sign (k)

of K k k . However, it still tests on singular behavior. Note:

The correctness of a solution obtained for a linearized set of equations in a nonpositive definite system is not guaranteed.

AutoSPC The autospc capability, which can be activated either on the AUTOSPC parameter or on the SOLVER option, attempts to eliminate rigid body motion by constraining degrees of freedom. This procedure occurs if the singularity ratio is smaller than 1.e-11. This option is only available with the direct solution procedure. This is different than setting the non-positive definite flag, which puts a small number into the stiffness matrix.

Solution of Linear Equations The finite element formulation leads to a set of linear equations. The solution is obtained through numerically inverting the system. Because of the wide range of problems encountered with Marc, there are several solution procedures available. Most analyses result in a system which is real, symmetric, and positive definite. While this is true for linear structural problems, assuming adequate boundary conditions, it is not true for all analyses. Marc has two main modes of solvers – direct and iterative. Each of these modes has two families of solvers, based upon the storage procedure. While all of these solvers can be used if there is adequate memory, only a subset uses spill logic for an out-of-core solution. Finally, there are classifications based upon nonsymmetric and complex systems. This is summarized below:

Main Index

CHAPTER 11 707 Solution Procedures for Nonlinear Systems

Direct Profile

Iterative Sparse

Direct Sparse

Vendor Provided Sparse*

Multifrontal Sparse

CASI Iterative

Mixed Direct Iterative

0

2

4

6

8

9

10

Real Symmetric

Yes

Yes

Yes

Yes

Yes

Yes

Yes

Real Nonsymmetric

Yes

No

No

No

Yes

No

No

Complex Symmetric

Yes

No

No

SUN only

Yes

No

No

Complex nonsymmetric

No

Yes

No

No

Yes

No

No

Out-of-core

Yes

Yes

Yes

SGI only

Yes

Yes

No

Possible problem with poorly conditioned systems

No

Yes

No

No

No

No

No

Solver Option

*Available for SGI, HP, and SUN platforms only.

The choice of the solution procedure is made through the SOLVER option.

Direct Methods Traditionally, the solution of a system of linear equations was accomplished using direct solution procedures, such as Cholesky decomposition and the Crout reduction method. These methods are usually reliable, in that they give accurate results for virtually all problems at a predictable cost. For positive definite systems, there are no computational difficulties. For poorly conditioned systems, however, the results can degenerate but the cost remains the same. The problem with these direct methods is that a large amount of memory (or disk space) is required, and the computational costs become very large.

Iterative Methods Marc offers iterative solvers as a viable alternative for the solution of large systems. These iterative methods are based on preconditioned conjugate gradient methods. The single biggest advantage of these iterative methods is that they allow the solution of very large systems at a reduced computational cost. This is true regardless of the hardware configuration. The disadvantage of these methods is that the solution time is dependent not only upon the size of the problem, but also the numerical conditioning of the system. A poorly conditioned system leads to slow convergence – hence increased computation costs. When discussing iterative solvers, two related concepts are introduced: fractal dimension, and conditioning number. Both are mathematical concepts, although the fractal dimension is a simpler physical concept. The fractal dimension, the range of which is between 1 and 3, is a measure of the “chunkiness” of the system. For instance, a beam has a fractal dimension of 1, while a cube has a fractal dimension of 3.

Main Index

708 Marc Volume A: Theory and User Information

The conditioning number is related to the ratio of the lowest to the highest eigenvalues of the system. This number is also related to the singularity ratio, which has been traditionally reported in the Marc output when using a direct solution procedure. In problems involving beams or shells, the conditioning number is typically small, because of the large differences between the membrane and bending stiffnesses.

Mixed Direct-Iterative Solver The mixed direct iterative solver attempts to combine the advantages of both solution methods. In the first iteration of an increment, the Multifrontal Sparse Solver (type 8) is used to obtain a solution while simultaneously creating the Cholesky pre-conditioner. In subsequent iterations, the sparse iterative solver is used with the previously calculated preconditioner. If solver convergence is not being obtained at a fast enough rate, the program switches back to the direct solver. This procedure has been shown to be effective for contact problems where small deformation or inelastic problems occur.

Preconditioners The choice of preconditioner can substantially improve the conditioning of the system, which in turn reduces the number of iterations required. While all positive definite systems with N degrees of freedom converges in N iterations, a well conditioned system typically converges in less than the square root of N iterations. The available preconditioners in the sparse iterative solver are diagonal, scaled diagonal, and incomplete Cholesky. The available preconditioners in the CASI sparse iterative solver are: CASI Primal and CASI Standard. The iterative solvers require an error criteria to determine when convergence occurs. The default is to use an error criteria based upon the ratio between the residuals in the solution and the reaction force. After c

obtaining the solution of the linear equations u evaluate: Ku

C

= F

C

(11-54)

The residual from the solution procedure is: A

Res = F – F

C

A

= F – Ku

C

(11-55)

If the system is linear ( K does not change) and exact numerics are preformed, then Res = 0 . Because this is an iterative method the residual is nonzero, but reduces in size with further iterations. Convergence is obtained when Res ⁄ Reac < TOL The tolerance is specified through the SOLVER option.

Main Index

(11-56)

CHAPTER 11 709 Solution Procedures for Nonlinear Systems

Storage Methods In general, a system of linear equations with N unknowns is represented by a matrix of size N by N , or 2

N variables. Fortunately, in finite element or finite difference analyses, the system is “banded” and not all of the entries need to be stored. This substantially reduces the memory (storage) requirements as well as the computational costs. In the finite element method, additional zeroes often exist in the system, which results in a partially full bandwidth. This profile storage method is used in Marc to store the stiffness matrix when solver type 0 is chosen. When many zeroes exist within the bandwidth, the sparse storage methods can be quite advantageous. Such techniques do not store the zeroes, but require additional memory to store the locations of the nonzero values. You can determine the “sparsity” of the system (before decomposition) by examining the statements: “Number of nodal entries excluding fill in” x “Number of nodal entries including fill in” y If the ratio ( x ⁄ y ) is large, then the sparse matrix storage procedure is advantageous.

Nonsymmetric Systems The following analyses types result in nonsymmetric systems of equations: Inclusion of convective terms in heat transfer analysis Coriolis effects in transient dynamic analysis Fluid mechanics Steady state rolling Soil analysis Follower force stiffness Frictional contact The first four always result in a nonsymmetric system. The last three can be solved either fully using the nonsymmetric solver, or (approximately) using a symmetric solver. The nonsymmetric problem uses twice as much memory for storing the stiffness matrix.

Complex Systems Marc utilizes a complex operator matrix for dynamic harmonic analyses when the damping matrix is present or for harmonic electromagnetic, acoustic, or piezoelectric analyses. The matrix is always symmetric.

Iterative Solvers In Marc, an iterative sparse solver is available using a sparse matrix technique. This method is advantageous for different classes of problems. There exist certain types of analyses for which the sparse iterative solver, CASI iterative or Mixed direct-iterative solvers are not appropriate. These types include: elastic analysis

Main Index

710 Marc Volume A: Theory and User Information

explicit creep analysis complex harmonic analysis substructures central difference techniques eigenvalue analysis use of gap elements auto increment loadcases Elastic or explicit creep analysis involves repeated solutions using different load vectors. When a direct solver is used, this is performed very efficiently using back substitution. However, when an iterative solver is used, the stiffness matrix is never inverted, and the solution associated with a new load vector requires a complete re-solution. The sparse iterative solver can exhibit poor convergence when shell elements or Herrmann incompressible elements are present. The CASI iterative solver should not be used with higher order Herrmann elements which includes element types 155, 156, and 157. If the mixed direct-iterative solver is used and convergence is poor, Marc switches to the multifrontal sparse direct solver.

Basic Theory A linear finite element system is expressed as: Ku = F

(11-57)

And a nonlinear system is expressed as: T

K Δu = F – R = r

(11-58)

where K is the elastic stiffness matrix, K

T

is the tangent stiffness matrix in a nonlinear system, Δu is

the displacement vector, F is the applied load vector, and r is the residual. The linearized system is converted to a minimization problem expressed as: T

T

ψ ( u ) = 1 ⁄ 2u Ku – u F

(11-59)

For linear structural problems, this process can be considered as the minimization of the potential energy. The minimum is achieved when –1

u = K F

(11-60)

The function ψ decreases most rapidly in the direction of the negative gradient. ∇ψ ( u ) = F – Ku = r

(11-61)

The objective of the iterative techniques is to minimize function, ψ , without inverting the stiffness matrix. In the simplest methods,

Main Index

CHAPTER 11 711 Solution Procedures for Nonlinear Systems

uk + 1 = uk + α k rk

(11-62)

where T

T

α k = r k r k ⁄ r k Kr k

(11-63)

The problem is that the gradient directions are too close, which results in poor convergence. An improved method led to the conjugate gradient method, in which uk + 1 = uk + α k Pk T

T

α k = P k r k – 1 ⁄ P k KP k

(11-64) (11-65)

The trick is to choose P k to be K conjugate to P 1, P 2, …, P k – 1 . Hence, the name “conjugate gradient methods. Note the elegance of these methods is that the solution may be obtained through a series of matrix multiplications and the stiffness matrix never needs to be inverted. Certain problems which are ill-conditioned can lead to poor convergence. The introduction of a preconditioner has been shown to improve convergence. The next key step is to choose an appropriate preconditioner which is both effective as well as computationally efficient. The easiest is to use the diagonal of the stiffness matrix. The incomplete Cholesky method has been shown to be very effective in reducing the number of required iterations.

Flow Diagram Figure 11-9 is a diagram showing the flow sequence of Marc. This diagram shows the input phase, equivalent nodal load vector calculation, matrix assembly, matrix solution, stress recovery, and output phase. It also indicates load incrementation and iteration within a load increment.

Main Index

712 Marc Volume A: Theory and User Information

Input Phase: Read Input Data Space Allocation Data Check Incremental Loads Equivalent Nodal Load Vector

Iteration Loop

Time Step Loop

Matrix Assembly

Matrix Solution

Stress Recovery

No

Convergence Yes Output Phase

Adapt Mesh

Yes

Next Increment No Stop

Figure 11-9 Marc Flow Diagram

Remarks Which solution method to use depends very much on the problem. In some cases, one method can be advantageous over another; in other cases, the converse might be true. Whether a solution is obtainable or not with a given method, usually depends on the character of the system of equations being solved, especially on the kind on nonlinearities that are involved. As an example in problems which are linear until buckling occurs, due to a sudden development of nonlinearity, it is necessary for you to guide the arc-length algorithm by making sure that the arc length remains sufficiently small prior to the occurrence of buckling. Even if a solution is obtainable, there is always the issue of efficiency. The pros and cons of each solution procedure, in terms of matrix operations and storage requirements have been discussed in the previous sections. A very important variable regarding overall efficiency is the size of the problem. The time required to assemble a stiffness matrix, as well as the time required to recover stresses after a solution,

Main Index

CHAPTER 11 713 Solution Procedures for Nonlinear Systems

vary roughly linearly with the number of degrees of freedom of the problem. On the other hand, the time required to go through the direct solver varies roughly quadratically with the bandwidth, as well as linearly with the number of degrees of freedom. In small problems, where the time spent in the solver is negligible, you can easily wipe out any solver gains, or even of assembly gains, with solution procedures such as a line search which requires a double stress recovery. Also, for problems with strong material or contact nonlinearities, gains obtained in assembly in modified Newton-Raphson can be nullified by increased number of iterations or nonconvergence. The development of new solution procedures is still an active field of research in the academic community.

References 1. Bergan, P. G. and E. Mollestad, “An Automatic Time-Stepping Algorithm for Dynamic Problems”, Computer Methods in Applied Mechanics and Engineering, 49, (1985), pp. 299 - 318 2. Bathe, K. J. Finite Element Procedures, Prentice Hall, Englewood Cliffs, NJ, 1996. 3. Riks, E. “An incremental approach to the solution of solution and buckling problems”, Int. J. of Solids and Structures, V. 15, 1979. 4. Riks, E. “Some Computational Aspects of the Stability Analysis of Nonlinear Structures”, Comp. Methods in Appl. Mech. and Eng., 47, 1984. 5. Crisfield, M. A. “A fast incremental iterative procedure that handles snapthrough”, Comput. & Structures, V. 13, 1981. 6. Ramm, E. “Strategies for tracing the nonlinear response near limit points,” in K. J. Bathe et al (eds), Europe-US Workshop on Nonlinear Finite Element Analysis in Structural Mechanics, Ruhr University Bochum, Germany, Springer-Verlag, Berlin, pp/ 63-89. Berlin, 1985. 7. Cerini, M. and Falzon, B. G., “Use of Arc-Length Method for Capturing Mode Jumping in Postbuckling Aerostructures”, AIAA Journal, V43,3,(2005), pp 681-689.

Main Index

714 Marc Volume A: Theory and User Information

Main Index

Chapter 12 Output Results

12

Main Index

Output Results

J

Workspace Information

J

Increment Information

J

Selective Printout

J

Restart

J

Element Information

J

Nodal Information

J

Post File

J

Forming Limit Parameter (FLP)

J

Program Messages

J

Marc HyperMesh Results Interface

J

Marc SDRC I-DEAS Results Interface

J

Marc - ADAMS Results Interface

J

Status File

716 720

721

723 723 728

731

738

731

734 735

736

735

716 Marc Volume A: Theory and User Information

This chapter summarizes the information that Marc provides in the output. In addition to reviewing your input, Marc provides information about the procedures the program uses and the workspace allocation. All calculated results are automatically written to the output file unless the user specifically requests otherwise.

Workspace Information Marc reports several aspects of workspace information, specifically, the allocation of memory workspace and the size of the work files. For the general memory, Marc first gives the workspace needed for the input and stiffness assembly. This number tells how much memory is needed to store the user-supplied data, the program-calculated data, and two-element stiffness matrices. Each set of data comprises three parts: overhead, element information, and nodal information. Element information consists of properties, geometries, strains, and stresses, and nodal information consists of coordinates, displacements, and applied forces. Next, Marc specifies the internal core allocation parameters. These values are useful in user subroutines and are often provided to the user subroutines. The values provided here are: • • • • • •

number of degrees of freedom per node (ndeg) maximum number of coordinates per node maximum number of invariants per integration point (neqst) maximum number of nodes per element (nnodmx) maximum number of stress components per integration point (nstrmx) number of strain components per integration point (ngens)

Note the following: • The number of degrees of freedom per node indicates the number of boundary conditions necessary to eliminate rigid body modes. • The number of stresses per integration point is the number of stresses per layer multiplied by the number of layers. • The number of invariants per integration point is the number of layers for either shell or beam elements. The ELSTO parameter stores element information on an auxiliary storage device, rather than in main memory. You can invoke this option, or Marc invokes it automatically. In this option, Marc: • • • •

sets a flag for element storage (IELSTO) specifies how many words are used per element (NELSTO) specifies the number of elements per buffer (MXELS) specifies the total amount of space needed to store this information

The number of elements per buffer should be at least two, and you can change the buffer size in the ELSTO parameter option to increase the number of elements which will be in the buffer. Marc reports the memory for different parts as it is allocated.

Main Index

CHAPTER 12 717 Output Results

For contact bodies: allocated workspace of

4567 words of memory for body

1

For incremental backup: space needed for incremental backup:

555313

For boundary conditions: allocated 600 words of memory due to kinematic boundary conditions We also get printouts like total workspace needed with in-core matrix storage =

893281

This printout refers to the memory in general memory (see Marc Workspace Requirements in Chapter 2 in this volume) and is not the total memory used. The solution of the equations of equilibrium result in the formation of the operator matrix and the decomposition/inversion of the matrix. In an mechanical analysis, this is the global stiffness matrix. For some solvers, there is an intermediate stage where the matrix is restructured from a sparse format to a more optimal format for numerical calculations. The allocation of this memory is reported in the memory summary (see below) either under solver:first part or under the allocated separately: category. This is summarized as follows: Solver 0 -Profile direct 2 - Sparse Iterative 4 - Sparse Direct 6 - Hardware Provided 8 - Multi-front Direct Sparse 13 - Mixed Direct Iterative

Operator Matrix first part first part first part first part first part first part

Restructured Matrix first part N/A first part allocated separately N/A N/A

Decomposition or Inverted Matrix first part N/A first part allocated separately allocated separately allocated separately

For solvers 0, 2, and 4, all the memory for the matrix solution is allocated within the general memory. For solver 6 and 8, the workspace for the restructuring stage (solver 6 only) and decomposition part is allocated separately outside of the general memory. Solvers 0, 4, and 8 have an out-of-core option for both storing the operator matrix and for inverting the matrix. Solver 6 (SGI) has an out-of-core option for inverting the matrix only. For this solver, there must be enough memory to assemble the operator matrix in-core. When using solver 0, if the out-of-core solver is invoked, one observes: total workspace needed with in-core matrix storage = 89686633 out-of-core matrix storage will be used core allocation based on 50498 nodal entries per assembly buffer. ...file 14-- maximum record length= 40960 approximate no. of words on file= 3686400 ...file 11-- maximum record length= 44622892

Main Index

718 Marc Volume A: Theory and User Information

approximate no. of ...file 12-- maximum record length= approximate no. of ...file 13-- maximum record length= approximate no. of

words on file= 44622892 words on file= 712 words on file=

99316916 89245784 712

If solver 4 were used, one would observe: total workspace needed with sparse in-core matrix storage = 34288801 out-of-core matrix storage will be used core allocation based on 50498 nodal entries per assembly buffer. ...file 14-- maximum record length= 40960 approximate no. of words on file= 3686400 core allocation based on 160473 nodal entries per assembly buffer. ...file 2-- maximum record length= 40960 approximate no. of words on file= 23429120

Note that until 14 contains the true sparse matrix, and, as the same problem is used, the I/O is the same for both solvers 0 and 4. For solver 0, this matrix gets expanded on unit 11 using a row blocking system, and decomposed to unit 12. For solver 4, it gets expanded and decomposed using unit 2. Solver 4 uses substantially less I/O than solver 0. For solver 8, we observe solver workspace needed for out-of-core matrix storage 6389794 solver workspace needed for in-core matrix storage 31339042 matrix solution will be out-of-core approximate disk space for out-of-core matrix storage 62678084

= =

=

At the end of the run, Marc prints out a summary of the memory used. This typically looks something like memory usage: of total

mbyte

words

within general memory: element stiffness matrices:

0

64982

solver: first part

4

963934

overallocation initial allocation

49

12957302

other:

0

0.2 3.6 48.1 0.1 allocated separately:

Main Index

15713

%

CHAPTER 12 719 Output Results

incremental backup:

5

1253317

10

2581002

nodal vectors:

1

349427

contact:

1

261625

tyings:

0

13362

transformations:

0

25182

kinematic boundary conditions:

0

4200

element storage:

5

1324844

4.7 solver 8 9.6 1.3 1.0 0.0 0.1 0.0 4.9 executable and common blocks:

27

7000000

26.0 miscellaneous 0 121763 0.5 --------------------------------------------------------------total: 103 26936653 general memory allocated: general memory used: peak memory usage:

53 4

14001931 1044629

110

28936653

In a parallel analysis, Marc also prints out the memory usage summed over the domains. The memory printout, during the execution, can also be obtained by means of the control file. Suppose the job defined in the input file jobname.dat is running. The memory summary printout is obtained by creating a file called jobname.cnt with a single line containing the word “memory”. The information is output at the beginning of the next increment. If the ALLOCATE parameter is to be used for initial memory allocation, the value to look for is the one for the line general memory used:

4

1044629

In this example, one would choose a value of 5 for ALLOCATE to insure that no dynamic reallocation of memory is performed. The top part defines the memory in general memory. The “overallocation initial memory” specifies the amount of general memory specified with the ALLOCATE option that is not used. The above example is very small and there is a large overallocation due to the default used (although the total amount is small). For larger problems, this part should be small. The line “other” specifies the part of the general memory that is not categorized.

Main Index

720 Marc Volume A: Theory and User Information

Further down are the parts that are allocated separately from the general memory, listed for each category. Similar to “other” above, “miscellaneous” specifies memory not categorized. The two lines for general memory is for highlighting the memory allocated and the memory actually used. The difference between the two is reflected in the “overallocation” line in the table. “executable and common blocks” is an estimate of the memory needed for loading the executable and storing values in common blocks. This is added so the total better agrees with the amount of memory the operative system reports for the program. Finally, the peak memory denotes the maximum amount of memory allocated at any instant during the job. In some cases, memory is allocated and then released. The “total:” in the summary table may then show a smaller value than the maximum during the run.

Increment Information A variety of information is given for each increment, and often for each iteration, of the analysis. This information is useful in determining the accuracy and the stability of the analysis.

Summary of Loads The printout entitled “Load Increments Associated with Each Degree of Freedom” allows you to check the load input quickly. It represents the sum, over all nodes in the mesh, of the point loads and the equivalent forces obtained after distributed loads (pressures, body forces) are applied. For example, you can easily check a pressure because the total force in a global coordinate direction would be the projected area normal to that direction of the surface upon which the pressure is applied, multiplied by the pressure magnitude.

Timing Information The amount of CPU necessary to reach the given location in the analysis is indicated by the following output: • • • • •

start of increment start of assembly start of matrix solution end of matrix solution end of increment

As an example, subtract the time associated with the start of the matrix solution from the time associated with the end of the matrix solution to determine how much time was spent in the equation solver.

Singularity Ratio The singularity ratio is a measure of the conditioning of the matrix (see Chapter 11 Solution Procedures for Nonlinear Systems for further details). This ratio is printed each time there is a solution of the matrix equations. You can measure the influence of the nonlinearities in the structure by examining the change in singularity ratios between increments.

Main Index

CHAPTER 12 721 Output Results

Convergence Several messages are printed that concern the convergence of the solution. These messages indicate the displacement, velocity, or residual error and are very important because they provide information concerning the accuracy of the solution procedure. These messages also indicate the ratio of the error and its relative quantity. This ratio must be less than that given in the CONTROL option for convergence to occur. See Appendix A for details on convergence testing. When the iterative solver is used, additional messages are printed regarding the convergence of the solution procedures.

Selective Printout Marc gives you several options and user subroutines for the control of the Marc output.

Options PRINT CHOICE allows you to select how much of the element and nodal information is to be printed. The possible selections are

• • • • •

group of elements group of nodes which layers (form beam and shell elements) which integration points increment frequency between printouts

The data entered through this option remain in control until you insert a subsequent PRINT CHOICE set. You can include such a set with either the model definition or with the history definition set. To obtain the default printout after a previous PRINT CHOICE, invoke PRINT CHOICE using blank entries. Note:

The PRINT CHOICE option has no effect on the restart or post file.

You can use the PRINT ELEMENT capability as a replacement for, or in conjunction with, the PRINT CHOICE option. The enhancements this option offers over the PRINT CHOICE option are the following: 1. You have a choice of integration and layer points for each element to be printed, which is especially useful when several different element types are used in one analysis. 2. You have a choice of the type of quantity to be printed, for instance, stresses could be printed for all elements, but strains for only a few. 3. The types of output quantities that can be selected are stresses, strains, creep strain, thermal strain, cracking strain, Cauchy stress, state variables, strain energy, or all nonzero quantities. 4. The output can be placed in a file other than the standard output file. 5. The PRINT NODE option can be used to obtain element quantities such as stresses and strains at the nodal points of each element. These are obtained by extrapolating the integration point values to the nodes.

Main Index

722 Marc Volume A: Theory and User Information

The PRINT NODE option is an alternative to the PRINT CHOICE option for controlling the output of nodal quantities. The additional capabilities of this option compared to the PRINT CHOICE are as follows: 1. You can choose which of the following nodal quantities are to be printed: incremental displacements total displacements velocities accelerations reaction forces generalized stresses 2. Different quantities can be printed for different nodal points. 3. The output can be placed in a file other than the standard output file. The PRINT CONTACT and the NO PRINT CONTACT options control the output of the summary of the loads on the contact bodies and their positions. Note:

All quantities are saved on the restart file, and you can obtain them at a later time by using the RESTART option. Quantities that were not printed out are available for later use.

The SUMMARY option allows you to get a quick summary of the results obtained in the analysis. This option prints the maximum and minimum quantities in tabular form. The is designed for direct placement into reports. You control the increment frequency of summary information and the file unit to which the information is written. The SUMMARY option reports on the physical components and the Tresca, von Mises, and mean values of stress, plastic strain, and creep strain. It also reports on such nodal quantities as displacements, velocities, accelerations, and reaction forces. The sort options (ELEM SORT and NODE SORT) allow you to sort calculated quantities in either ascending or descending order. These quantities may either be sorted by their real magnitude or their absolute magnitude. The sort options also allow you to control the type of quantity to be sorted, for example, equivalent stress and the number of items to be sorted. The sort options print the sorted values in tabular form. The is designed for direct placement into reports. You may control the increment frequency of sorted values and the file unit to which these values are written. The PRINT VMASS option allows you to selectively choose which elements and associated volumes, masses, first and second moment of inertia, and strain energy are to be printed. In order to have correct mass computations, mass density for each element must be given. The volumes, masses, and energies can be written on either standard output file unit 6, or user specified unit. The center of mass is also calculated and output.

Grid Force Balance The GRID FORCE option allows the user to output the different contributions to the total force applied on an element or a node.

Main Index

CHAPTER 12 723 Output Results

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

User Subroutines User subroutines can be used to obtain additional output, which can be accessed at each time/load increment. The available subroutines are the following: • IMPD – obtains nodal quantities, such as displacements, coordinates, reaction forces, velocities, and accelerations • ELEVAR – obtains element quantities such as strains, stresses, state variables, and cracking information • ELEVEC – outputs element quantities during harmonic subincrements • INTCRD – obtains the integration point coordinates used for forming the stiffness matrix

Restart One capability of the RESTART option allows you to recover the output at increments where printout was suppressed in previous runs. This option can be used to print time/load increments for a number of consecutive increments. Under this option, Marc does not do any analysis. In conjunction with the RESTART option, you can use either the PRINT CHOICE or PRINT ELEMENT, or PRINT NODE option to select a region of the model for which you want to obtain results.

Element Information The main output from an increment includes element information followed by nodal information. The system provides the element data at each integration point. If you use the CENTROID parameter, the system provides the element data at the centroidal point. You can control the amount of printed output by using either the PRINT CHOICE or PRINT ELEMENT option. All quantities are total values at the

Main Index

724 Marc Volume A: Theory and User Information

current state (at the end of the current increment), and the physical components are printed for each tensor quantity (stress, strain, and generalized stress and strain). The orientation of these physical components is generally in the global coordinate system; however, their orientation depends on the element type. (Marc Volume B: Element Library explains the output for each particular element type.) Also, the physical components may be printed with respect to a user defined preferred system. In addition to the physical components, certain invariants are given, as follows: 1. Tresca intensity - the maximum difference of the principal values, and the measure of intensity usually required for ASME code analysis von Mises intensity - defined for stress as σ =

3 --- S i j S i j 2

1 S i j = σ – --- δ i j σ k k 3

(12-1)

where σ is a stress tensor and S is the deviatoric stress tensor. For beam and truss elements, σ 22 = σ 33 = 0 , and additional shears are zero; for plane stress elements, including plates and shells, σ 33 = 0 . 2. von Mises intensity - calculated for strain type quantities as ε =

2 --- ε i j ε i j 3

(12-2)

Marc uses these measures in the plasticity and creep constitutive theories. For example, incompressible metal creep and plasticity are based on the equivalent von Mises stress. For beam, truss, and plane stress elements, an incompressibility assumption is made regarding the noncalculated strain components. a. For beam and truss elements, this results in 1 ε 22 = ε 33 = – --- ε 11 2

(12-3)

b. For plane stress elements ε 33 = – ( ε 11 + ε 22 )

(12-4)

c. For beam and plane stress elements taken as a whole εk k = 0

(12-5)

3. Mean normal intensity - calculated as ( σ 11 + σ 22 + σ 33 ) ⁄ 3 or ( ε 11 + ε 22 + ε 33 ) ⁄ 3

Main Index

(12-6)

CHAPTER 12 725 Output Results

Equation (12-6) represents the negative hydrostatic pressure for stress quantities. For strain quantities, the equation gives the dilatational magnitude. This measurement is important in hydrostatically dependent theories (Mohr-Coulomb or extended von Mises materials), and for materials susceptible to void growth. 4. The principal values are calculated from the physical components. Marc solves the eigenvalue problem for the principal values using the Jacobi transformation method. Note that this is an iterative procedure and may give slightly different results from those obtained by solving the cubic equation exactly. 5. State variables are given at any point where they are nonzero.

Mentat Computed Element Results These element results are computed based on the Marc output. By default, Marc always outputs the elemental results at the integration points. In Marc Mentat, by default, these data are extrapolated linearly to the nodal positions. The data are then averaged with the contributions from the neighboring elements. Principle values and equivalent values are computed based on these nodal data in Marc Mentat. If a stress or strain tensor is output in the post file, Marc Mentat will compute their principal values and the equivalent items (such as, equivalent stress and strain). Note that the equivalent items may be different from ones directly output by Marc because of the way they are computed in Marc Mentat. For example, the equivalent stress computed in Marc Mentat may show a slightly different result compared to the equivalent von Mises stress from Marc output. It is also possible to turn off the extrapolation procedure in Marc Mentat. This is recommended in problems of high gradients. It can be done through the RESULTS>scalar plot SETTING>EXTRAPOLATION menu by picking TRANSLATE.

Solid (Continuum) Elements For solid (continuum) elements, stress, strain, and state variables are the only element quantities given. Marc prints out stresses and total strain for each integration point. In addition, it prints out thermal, plastic, creep, and cracking strains, if they are applicable. Note that the total strains include the thermal contribution.

Shell Elements Marc prints generalized stresses and generalized total strains for each integration point. For thick shell (Type 22, 72, 75) elements interlaminar shear stresses are printed at the interface of two laminated layers if the TSHEAR parameter is included. The generalized stresses printed out for shell elements are 1 --t

+t⁄2

∫ –t ⁄ 2

σ i j dy

( Section Force per Unit Thickness )

Main Index

(12-7)

726 Marc Volume A: Theory and User Information

1 --t

+t⁄2

∫

yσ i j dy

(12-8)

–t ⁄ 2

( Section moment per Unit Thickness ) The generalized strains printed are Eα β ;

α, β = 1, 2

κα β ;

α, β = 1, 2

( Stretch ) ( Curvature )

(12-9) (12-10)

Physical stress values are output only for the extreme layers unless you invoke either PRINT CHOICE or PRINT ELEMENT. In addition, thermal, plastic, creep, and cracking strains are printed for values at the layers, if applicable. Although the total strains are not output for the layers, you can calculate them using the following equations. ε 11 = E 11 + hκ 11

(12-11)

ε 22 = E 22 + hκ 22

(12-12)

γ 12 = E 12 + hκ 12

(12-13)

where h is the directed distance from the midsurface to the layer; E i j are the stretches; and κ i j are the curvatures as printed. You can obtain these quantities by using the ELEVAR subroutine.

Beam Elements The printout for beam elements is similar to shell elements, except that the section values are force, bending and torsion moment, and bimoment for open section beams. For beam element type 45, interlaminar shear stresses are printed at the interface of laminated layers if the TSHEAR parameter is used. These values are given relative to the section axes (X, Y, Z) which are defined in the COORDINATES or the GEOMETRY option. Before a beam member can be designed, it is necessary to understand the section forces distribution along the axial direction of the beam. For example, if variations of shear force and moment along axial direction are plotted, the graphs are termed shear diagram and moment diagram, respectively. To postprocess these diagrams, post code 261 needs to be specified along with the post codes (shown in Table 12-1) which define the corresponding section forces of the beam element.

Main Index

CHAPTER 12 727 Output Results

Table 12-1

Post Codes for Beam Section Forces

Post Code 265 266 267 268 264 (Moment xx (Moment yy (Shear (Shear yz xz or or Shear Element 269 270 (Axial or Moment or Moment ip) op) Shear ip) op) Type 2-D/3-D Force) (Torque) (Bimoment) 5

2-D

X

X

16

2-D

X

X

45

2-D

X

X

13

3-D

X

X

X

X

14

3-D

X

X

X

X

25

3-D

X

X

X

X

31

3-D

X

X

X

52

3-D

X

X

X

X

76

3-D

X

X

X

X

77

3-D

X

X

X

X

78

3-D

X

X

X

X

79

3-D

X

X

X

X

98

3-D

X

X

X

X

X

X

X

X

X

X

X

The stresses at the section points in the cross section are only output if the PRINT CHOICE or PRINT ELEMENT option are included. If any nonlinearity exists at the section points, they will be provided in the output file.

Gap Elements Marc prints the gap contact force, friction forces, and the amount of slip.

Linear and Nonlinear Springs Marc prints the spring forces.

Heat Transfer Analysis The element temperatures are provided at the integration points. When requested, the temperature gradient and the flux is also provided.

Main Index

728 Marc Volume A: Theory and User Information

Joule Heating Analysis In addition to the temperatures, the voltage, current, and the heat generated at the integration points is output.

Hydrodynamic Bearing Analysis The lubricant thickness, pressure, and pressure gradient are provided.

Electrostatic Analysis The electrical potential ( V ), electric field intensity vector ( E ), and electrical displacement vector/flux ( D ) are provided.

Piezoelectric or Electrostatic-Structural Analysis In addition to the mechanical stresses and strains, the electrical field intensity vector ( E ) and electrical displacement/flux ( D ) are provided.

Magnetostatic Analysis The magnetic potential ( A ), the magnetic field density ( B ), and the magnetic flux density ( H ) are provided. For two-dimensional problems, only the A z component is given.

Electromagnetics Analysis The electric field intensity vector ( E ), the electrical displacement vector/flux ( D ), the magnetic flux density ( H ), and the current density ( J ) are provided.

Acoustic Analysis The pressure and the gradient of the pressure is provided. Note in an Acoustic-Structural analysis, the pressure is only provided as a nodal variable.

Nodal Information Marc also prints out the following quantities at each nodal point.

Stress Analysis • Incremental displacements - the amount of deformation that occurred in the last increment • Total displacements - the summation of the incremental displacements • Total equivalent nodal forces (distributed plus point loads) - the total force applied to the model through distributed loads (pressures) and point loads

Main Index

CHAPTER 12 729 Output Results

• Reaction forces at fixed boundary conditions • Residual loads at nodal points that are not fixed by boundary conditions Note:

Each value listed above is given at each nodal point, unless you invoke the PRINT CHOICE or PRINT NODE option. If you invoke the TRANSFORMATION option, Marc prints the nodal information relative to the user-defined system, rather than the global coordinate system.

Reaction Forces Marc computes reaction forces based on the integration of element stresses. This is the only way to compute total reaction forces in a nonlinear analysis. Since such integration is only exact if the stresses are known at each integration point, the reaction forces are not printed if you use the CENTROID parameter. In a nonlinear analysis, you should check that the reaction forces are in equilibrium with the external forces. If they are not in equilibrium, the analysis will be inaccurate, usually due to excessively large incremental steps. In most cases, the equilibrium is automatically ensured due to the convergence testing in Marc.

Residual Loads The residual loads are a measure of the accuracy of the equilibrium in the system during analysis. This measure is very important in a nonlinear analysis and should be several orders of magnitude smaller than the reaction forces.

Dynamic Analysis In a dynamic analysis, Marc prints out the total displacement, velocity, and acceleration at each time increment.

Heat Transfer Analysis In a heat transfer analysis, Marc prints out nodal temperatures, externally applied fluxes, and calculated nodal heat fluxes.

Joule Heating Analysis In Joule heating analysis, in addition to the thermal vectors, the nodal voltage and the applied and calculated currents are provided.

Rigid-Plastic Analysis In steady-state rigid-plastic analysis, Marc prints nodal velocities.

Main Index

730 Marc Volume A: Theory and User Information

Hydrodynamic Bearing Analysis In a hydrodynamic bearing analysis, Marc gives the mass flux at the nodal points.

Electrostatic Analysis In an electrostatic analysis, Marc prints the scalar potential and the applied and calculated charge.

Magnetostatic Analysis In a magnetostatic analysis, Marc prints the vector potential and the applied and calculated current.

Electromagnetic Analysis In an electromagnetic analysis, Marc prints out the vector and scalar potential, the applied and calculated current and charge.

Piezoelectric or Electrostatic-Structural Analysis In a piezoelectric or electrostatic-structural analysis, in addition to the structural quantities, such as displacement and reaction force, the electric potential, and reaction charges.

Acoustic Analysis In an acoustic analysis, Marc prints the pressure and the source.

Supplementary Information Contact Analysis The standard output includes, at the end of each increment, a summary of information regarding each body. This information reports the increment’s rigid body velocity, the position of the center of rotation, and the total loads on the body. These last values are obtained by adding the contact forces of all nodes in contact with the rigid body. Deformable bodies being in equilibrium have no load reported. Additional information can be obtained by means of the PRINT,5 parameter. In such cases, all the contact activity is reported. Namely, every time a new node touches a surface, or separates from a surface, a corresponding message is issued. Contact with rigid surfaces entails an automatic transformation. Displacement increments and reactions in the transformed coordinates - tangent and normal to the contact interface - are also reported for every node that is in contact in the usual Marc manner.

Electromagnetic Analysis If the EMRESIS or EMCAPAC options are invoked, a summary is output providing the electrical resistance or capacitance for the conducting body.

Main Index

CHAPTER 12 731 Output Results

Post File The post file contains results of the analysis performed. This information can be viewed using Marc Mentat or MD Patran to observe the displaced mesh, contours of element quantities, principal quantities, time history behavior, response gradients, design variables, etc. The post file contains the finite element mesh and any changes to the finite element mesh due to either rezoning or adaptive mesh refinement. Basic nodal quantities (such as displacements, velocities, acceleration, applied loads, and reaction forces) are automatically placed on the post file. It is also possible to include user-defined nodal vectors by use of the UPOSTV user subroutine. Element quantities, such as stress, strain, plastic strain) must be explicitly requested by using the POST model definition option. It is possible to have user-defined element quantities placed on the post file for subsequent display by using the PLOTV user subroutine.

Forming Limit Parameter (FLP) For continuum or shell elements, the Principal Engineering Strains can be calculated based on the true strain values. Correspondingly, the Forming Limit Parameter can be obtained for shell/membranes according to the data of the Forming Limit Diagram (FLD). The principal engineering strains are calculated based on the true strain according to following relation: e i = exp ( ε i ) – 1

(12-14)

where e i are the principal engineering strain components and ε i are the principal true strain components. The principal engineering strain values can be selected for postprocessing. In addition, if shell/membrane elements are used, the Forming Limit Parameters (FLP) can also be selected. The FLP is defined as the ratio of the major principal engineering strain to the maximum allowable major principal engineering strain given by the Forming Limit Diagram. Based on this definition, it is calculated by FLP = e 1 ⁄ FLD ( e 2 )

(12-15)

where e 1 means the major principal engineering strain, e 2 is the minor principal engineering strain. FLD ( e 2 ) is the forming limit corresponding to e 2 . FLD is defined by input data in model definition through material properties. By plotting the major principal engineering strain of each integration point of an element as point ( e 2 , e 1 ) on the chart, as shown in Figure 12-1, it is easy to find that for points below the FLD line is safe. Strain rates above the FLD line imply failure. To consider the FLP value of these fields, one can find that in the field which is above FLD line, the value of FLP is larger than 1. On the FLD line, FLP equals 1, and FLP is less than 1 if a point located in the field below the FLD line. Therefore, by plotting the FLP value in Marc Mentat, it can be seen if the sheet metal forming process is successful.

Main Index

732 Marc Volume A: Theory and User Information

Major Principal Engineering Strain (e1)

FLD(e2) Fail

Safe

Fail FLP>1

FLD(e2) Safe

FLP<1

Minor Principal Engineering Strain (e2) Figure 12-1 The Definition of Forming Limit Parameter (FLP)

The methods employed in Marc to define the Forming Limit Diagram are: 1. Fitted function definition 2. Predicted function definition 3. Table definition (accepts piecewise linear FLD curves) The details of the above methods are described below: 1. Fitted function: By this method, the polynomial functions are utilized to fit the FLD curve. The functions are shown in Equations 12-16a and 12-17b: FLD ( e 2 ) = C 0 + D 1 e 2 + D 2 e 22 + D 3 e 23 + D 4 e 24

( e2 ≤ 0 )

(12-16)

FLD ( e 2 ) = C 0 + C 1 e 2 + C 2 e 22 + C 3 e 23 + C 4 e 24

( e2 ≥ 0 )

(12-17)

2. Predicted function: The predicted functions are generated based on the theories of local necking and diffuse necking. Both theories assume that the material obeys the power-law strain hardening, σ = Kε n . Local necking: The critical strain for the onset of local necking is influenced by strain ratio ρ , where ρ = ε 2 ⁄ ε 1 , ρ ≤ 0 . Equation shows the relationship of critical strain versus strain ratio (by Hill). n ε* = -----------------(1 + ρ)

ρ≤0

For uniaxial tension, ρ = – 0.5 . For plane strain, ρ = 0 .

Main Index

(12-18)

CHAPTER 12 733 Output Results

Diffuse necking: Diffuse necking is the phenomenon that while necking happens, deformation continues. The critical strain for the diffuse necking to happen is determined by Equation 12-19 (by Swift): 2n ( 1 + ρ + ρ 2 ) ε* = -----------------------------------------------------( 1 + ρ ) ( 2ρ 2 – ρ + 2 ) Note:

ρ≤0

(12-19)

For the case of ρ < 0 , the predicted critical strain by Equation 12-19 is well below the experiment data. Therefore, for the purpose of prediction, the diffuse necking theory and the local necking theory are chosen for cases of ρ > 0 and ρ ≤ 0 , respectively.

Experiments (mainly with low carbon steels) showed that the predicted FLD usually is at a level below the experimental FLD curve. The experimental forming limit diagram is characterized by the value of ε* corresponding to plane strain. This value is referred at FLD 0 as shown in Figure 12-2. This value increases with the strain-hardening exponent, n , and the strain-rate exponent, m . The value of ε* is observed to rise as the thickness increases. This phenomenon is referred as thickness effect and it is characterized as thickness coefficient t c . Experiments by Keeler tended to express this relationship as shown in Equation (12-20). FLD 0 = Q ⋅ ( 0.233 + t c ⋅ t )

(12-20)

where Q = n ⁄ 0.21 if n is less than 0.21. Otherwise, Q = 1.0 . T is the thickness of the sheet metal. The thickness coefficient t c is set as 3.59 if the unit used to define the thickness is “Inch”. If the unit used is “mm”, t c is set as 0.141. Similarly, if the unit “cm” is used, t c is then set as 1.41, etc. It should be emphasized that, in most cases, friction is also a very important parameter that will affect the occurrence of necking. On the other hand, Equation (12-20) is mainly from data on lowcarbon steels that have relatively high strain-rate dependence. In materials with low strain-rate dependence (for example, aluminum alloys), the thickness effect should be much less. Finally, it is suggested that for safety purposes, a safety zone, as shown as the shadow area in Figure 12-2, must be set. For points above the safety zone, material is considered as failure. For points below the safety zone, material is considered as safe. If a point locates in the safety zone, the material is in the marginal status. Usually, the thickness of the safety zone is set as 0.1 or 10%. 3. Table definition: The table function in Marc allows users to define any curves through the TABLE model definition option. For example, if the user has FLD point of material, it is possible to define the FLD as piecewise linear curve. For details, refer the Marc Volume C: Program Input, Chapter 3 Model Definition Options, TABLE.

Main Index

734 Marc Volume A: Theory and User Information

Major Principal Engineering Strain e1

Experimental forming limit FLD0

Local necking

Diffuse necking

0 Minor Principal Engineering Strain e2 Figure 12-2 Predicted FLD and Experimental FLD Curves

Program Messages The messages provided by Marc at various points in the output show the current status of the problem solution. Several of these messages are listed below. • START OF INCREMENT x indicates the start of increment number x. • START OF ASSEMBLY indicates Marc is about to enter the stiffness matrix assembly. • START OF MATRIX SOLUTION indicates the start of the solution of the linear system. • SINGULARITY RATIO prints yyy, where yyy is an indication of the conditioning of the matrix. This value is typically in the range 10-6 to 1. If yyy is of the order of machine accuracy (10-6 for most machines), the equations might be considered singular and the solution unreliable. • END OF MATRIX SOLUTION indicates the end of matrix decomposition. • END OF INCREMENT x indicates the completion of increment number x. • RESTART DATA at INCREMENT x ON UNIT 8 indicates that the restart data for increment number x has been written (saved) on Unit 8. • POST DATA at INCREMENT x on UNIT y indicates that the post data for increment number x has been written (saved) on Unit y. In addition to these Marc messages, exit messages indicate normal and abnormal exists from Marc. Table 12-2 shows the most common exit messages.

Main Index

CHAPTER 12 735 Output Results

Table 12-2

Marc Exit Messages

Message

Meaning

MARC EXIT 3001

Normal exit.

MARC EXIT 3004

Normal exit.

MARC EXIT 13

Input data errors were detected by the program.

MARC EXIT 2004

Operator matrix (for example, stiffness matrix in stress analysis) has become non-positive definite and the analysis terminated.

MARC EXIT 3002

Convergence has not occurred within the allowable number of recycles.

Marc HyperMesh Results Interface Marc now outputs results for postprocessing with HyperMesh. The writing of the HyperMesh results file is invoked by the HYPERMESH model definition option described in detail in Marc Volume C: Program Input. Marc Mentat can also be used to write the necessary commands into the Marc data file. The related button can be found one level below each of the ANALYSIS CLASS buttons within the JOBS menu.The binary file created as a result has the title jobid.hmr where jobid is the name of the data file for the job. The geometry data may be imported into HyperMesh from a Marc data file. Alternatively, it can be created by HyperMesh or read in from other formats via the HyperMesh import capability. The types of data that may be selected for writing into the HyperMesh results file are listed in Marc Volume C: Program Input under the HYPERMESH model definition option. It is important to note that, in case eigenvectors for buckling or eigenfrequency analysis are to be written into the results file, the corresponding Marc file should have the BUCKLE INCREMENT or MODAL INCREMENT model definition option, as appropriate. The BUCKLE, MODAL SHAPE, and RECOVER history definition options are not to be used in these cases. Since HyperMesh allows only one deformed shape plot per simulation, each eigenvector of an eigenvalue analysis is saved as a separate simulation. Thus, when using HyperMesh, these eigenvectors can be plotted by skipping to the next simulation rather than skipping to the next data type of a simulation. The contour plots can be obtained for all data types including eigenvectors. In case the number of requested eigenvalues is more than the number extracted, the data type in the HyperMesh “deformed” screen will inform you for those modes that are not extracted. The “next” button may need to be clicked to see the data type in the “deformed” mode of plotting.

Marc SDRC I-DEAS Results Interface A facility exists in Marc to write out an SDRC I-DEAS universal file of the analysis results, in order for postprocessing by the I-DEAS program. The writing of the universal file is invoked by the SDRC model definition option described in detail in Marc Volume C: Program Input. Marc Mentat can also be used to write the necessary commands into the Marc data file. The related button can be found one level below each of the ANALYSIS CLASS buttons within the JOBS menu. The formatted ASCII file created as a result has the title jobid.unv, where jobid is the name of the data file for the job.

Main Index

736 Marc Volume A: Theory and User Information

The model data is imported into I-DEAS by way of the universal file as well. The types of data that may be selected for writing into the I-DEAS universal file are listed in Marc Volume C: Program Input under the SDRC model definition option.

Marc - ADAMS Results Interface ADAMS/Flex allows flexible components to be included into ADAMS models to achieve more realistic simulation results. Marc is capable of generating a Modal Neutral File (MNF) representing the flexible component to be integrated into the ADAMS model. The flexible component can undergo linear or nonlinear loading in Marc up to the point where the MNF is requested to be generated. No more analysis takes place in Marc after generating the MNF. Generating an MNF from Marc is based on performing the most general method of Component Mode Synthesis (CMS) techniques, namely the Craig-Bampton method. Using the Craig-Bampton method, the degrees of freedom, u , of the flexible component are partitioned into two sets of DOFs: • Boundary or Interface DOFs, u B : These DOFs can be used to apply loads in ADAMS or to connect the flexible component to other rigid bodies. • Interior DOFs, u I : These internal DOFs of the flexible component can be condensed out using the superelement technique. Two sets of modes shapes arranged in matrices, Φ I C and Φ I N , and their corresponding modal coordinates vectors, q C and q N , are also defined: • Constraint Modes, Φ I C : These modes are the static shapes obtained by giving each boundary degree of freedom a unit displacement while holding all other boundary DOFs fixed. Corresponding to the constraint modes is the set of modal coordinates q C . The basis of constraint modes completely spans all possible motions of the boundary DOFs, with a one-to-one correspondence between the modal coordinates of the constraint modes and the displacement in the corresponding boundary DOFs, u B = q C . • Fixed-Boundary Normal Modes, Φ I N : These modes are obtained by fixing the boundary DOFs and computing an eigensolution. There are as many fixed-boundary normal modes as the user desires. These modes define the modal expansion of the interior DOFs. The quality of this modal expansion is proportional to the number of modes retained by the user. Corresponding to the fixed-boundary normal modes is the set of modal coordinates q N . The Craig-Bampton modes consist of both the constraint modes and the fixed-boundary normal modes. The relationship between the physical DOFs and the Craig-Bampton modes and their modal coordinates is given by

Main Index

CHAPTER 12 737 Output Results

⎧ ⎪ uB ⎨ ⎪ uI ⎩

⎫ ⎪ ⎬ = ⎪ ⎭

⎧ IB C OB N ⎪ qC ⎨ ΦI C ΦI N ⎪ qN ⎩

⎫ ⎪ ⎬ ⎪ ⎭

(12-21)

where the subscripts B, I, C, and N denote Boundary DOF, Interior DOF, Constraint Mode and Normal Mode, respectively. The above equation indicates that the Craig-Bampton analysis can be considered as a transformation from the physical DOFs to the Craig-Bampton modal basis q in the form u = Φq where Φ is the modal matrix or transformation matrix. The finite element equation of motion is given by Mu·· + Ku = f in which M is the mass matrix, K is the stiffness matrix and f is the load vector. Substituting by the T

transformation relation into the equation of motion and premultiplying by Φ gives T T T ·· Φ MΦq + Φ KΦq = Φ f

The above equation defines the generalized mass and stiffness matrices as: ˆ : Projection of the mass matrix onto the modal space given by • Generalized Mass Matrix, M ˆ = Φ T MΦ M ˆ : Projection of the stiffness matrix onto the modal space given by • Generalized Stiffness Matrix, K ˆ = Φ T KΦ K Note that the ADAMS MNF interface expects lumped mass matrices to be used. Thus, the LUMP parameter must be included in the Marc input. The MNF interface distinguishes between two types of loads: • Modal Preload, ˆf P L : A projection onto the modal space of the internal load vector corresponding to the loads that have already been applied in the finite element analysis up to the point when the MNF is generated. • Modal Loads, fˆ L : A projection onto the modal space of the loads that may be defined in the Marc input using the ASSEM LOAD history definition option but not applied in the finite element analysis. They may be scaled and introduced in the ADAMS simulation. ASSEM LOAD loadcases, if exist, should precede any actual preloading to be applied to the component in Marc. Both types of loads can be computed using the relation ˆf = Φ T f

Main Index

738 Marc Volume A: Theory and User Information

Corresponding to each Craig-Bampton mode, a stress and a strain mode can be computed. These are the incremental nodal stresses and strains found by considering each mode at a time to be the incremental displacement solution and performing a stress recovery. To request the computation and export of stress and/or strain modes, the MNF parameter must be used. The Craig-Bampton analysis is triggered when the SUPERELEM model or history definition option is reached in the input. The SUPERELEM option allows direct definition of the boundary or interface DOFs, u B . The option also allows automatic definition of interface DOFs 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 DOFs are not known a priori. It also allows the specification of interface DOFs 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. A MODAL SHAPE loadcase using the Lanczos method must be present in the input immediately following the SUPERELEM loadcase. No more analysis can be performed afterwards. The units used in the Marc model are specified using the MNF UNITS model definition option. Successful MNF generation produces Marc Exit 3018. The MNF generated will have the same filename as the input file and the extension .mnf. Assuming the input file is jobname.dat, the MNF will have the name jobname.mnf.

Status File The status file contains summarized information of the analysis. Each line within this file includes the load case number, the associated increment number, and the number of cycles, contact separations, and cutbacks associated with that increment; the accumulated total cycles, increment splittings, separations, cutbacks, and remeshing times numbers in the analysis as well as the time step size of each increment and the overall time achieved by the analysis. Marc reports all this information on one line upon completion of each increment. If the increment is partially completed (for example, the completion of one part of a split increment or one part of the whole increment due to cutback), Marc also reports one line for each part of the increment.

References 1. R. R. Craig and M. C. C. Bampton. Coupling of substructures for dynamics analyses. AIAA Journal, 6(7): 1313-1319. 1968. 2. R.R. Craig. Structural Dynamics: An Introduction to Computer Methods. John Wiley & Sons. 1981. 3. ADAMS User Guide: Using ADAMS/Flex. 2002.

Main Index

Chapter 13 Parallel Processing

13

Main Index

Parallel Processing

J

Different Types of Machines

J

Supported and Unsupported Features

J

Matrix Solvers

J

Contact

J

Domain Decomposition

742

742 743

740 740

740 Marc Volume A: Theory and User Information

Marc can make use of multiple processors when performing an analysis. Most, but not all, features of Marc are supported in parallel mode. The type of parallelism used is based upon domain decomposition. A commonly used name for this is the Domain Decomposition Method (DDM). The model is decomposed into domains of elements, where each element is part of one and only one domain. The nodes which are located on domain boundaries are duplicated in all domains at the boundary. These nodes are referred to as inter-domain nodes below. The total number of elements is thus the same as in a serial (nonparallel) run but the total number of nodes can be larger. The computations in each domain are done by separate processes on the machine used. At various stages of the analysis, the processes need to communicate data between each other. This is handled by means of a communication protocol called MPI (Message Passing Interface). MPI is a standard for how this communication is to be done and Marc makes use of different implementations of MPI on different platforms. Marc uses MPI regardless of the type of machine used. The types of machines supported are shared memory machines, which are single machines with multiple processors and a memory which is shared between the processors, and cluster of separate workstations connected with some network. Each machine (node) of a cluster can also be a multiprocessor machine.

Different Types of Machines As mentioned above, Marc can run on a shared memory machine and on a cluster of workstations. The main reason for running a job in parallel on a shared memory machine is speed. Since all processes run on the same machine sharing the same memory, the processes all compete for the same memory. There is an overhead in memory usage so some parts of the analysis need more memory for a parallel run than a serial job. The matrix solver, on the other hand, needs less memory in a parallel job. Less memory is usually needed to store and solve several smaller systems than one large. In the case of a cluster, the picture is somewhat different. Suppose a number of workstations are used in a run and one process is running on each workstation. The process then has full access to the memory of the workstation. If a job does not fit into the memory of one workstation, the job could be run on, say, two workstations and the combined memory of the machines may be sufficient. The amount of speed-up that can be achieved depends on a number of factors including the type of analysis, the type of machine used, the size of the problem, and the performance of communications. For instance, a shared memory machine usually has faster communication than a cluster (for example, communicating over a standard Ethernet). On the other hand, a shared memory machine may run slower if it is used near its memory capacity due to memory access conflicts and cache misses etc.

Supported and Unsupported Features Most of the main features of Marc are supported in parallel mode. For instance, a fully coupled thermomechanical contact analysis can be performed in parallel. A notable feature which is not yet supported is global adaptive remeshing. Local adaptivity is fully supported. New elements and nodes that are created remain in the same domain as the parent element. The list of unsupported features is: • Acoustics • Auto therm creep

Main Index

CHAPTER 13 741 Parallel Processing

• • • • • • • • • • • • • • • • • •

Beam-to-beam contact Bearing Buckling Convective terms in heat transfer Design sensitivity and optimization Eigenvalue extraction Electromagnetics Explicit dynamics Fluids and its coupled analysis Gap elements (but the normal contact is supported) Harmonics Hydrodynamics Insert Radiation Remeshing and rezoning Response spectrum Steady state rolling analysis Superelements

The DDM single input file capability will not support any analyses types and input options that are not currently supported by the traditional multiple input files DDM. Moreover, some additional model and history definition options and command line arguments will not be supported in the Marc 2008 release. These are: • ACTIVATE and DEACTIVATE • ACTUATOR

• BEGIN SEQUENCE and END SEQUENCE • • • • •

• • • • • • •

• • • • • •

CHANNEL CFAST CONRAD GAP CWELD DAMPING DISP CHANGE if not FIXED DISP format. The DISP CHANGE option is supported only if the 1st entry of the data block following DISP CHANGE is equal to 0. EXCLUDE FXORD GLOBALLOCAL GRID FORCE INSERT NEW POINT LOADS with follower forces SUPERPLASTIC QVECT TIME-TEMP TYING CHANGE UDUMP

• def command line option • Auxiliary input files

Main Index

742 Marc Volume A: Theory and User Information

The following additional capabilities are now available: • Ability to generate a single post file from a DDM run • Ability to use nonconsecutive element and node numbering The following notes apply to the use of the single post file option: • Although general DDM jobs support post revisions 7 and higher, the ability to generate a single post file from a DDM job is restricted to post revisions 9 and higher. • Reading a single post file back into a Marc DDM job using the -pid command line option is only available for the AXITO3D and PRE STATE options in this release. • In the case of single input file jobs with continuous post files where the POST option follows the RESTART option, both jobs should either use multiple post files or single post files. If multiple post files are used, then the number of domains should be the same in both jobs.

Matrix Solvers All matrix solvers in Marc are supported in parallel mode with the exception of the unsymmetric solver and the CASI iterative solver (solver type 9). Only the multifrontal solver (solver type 8) supports outof-core solution in parallel. The matrix solvers work somewhat different in parallel mode as compared to serial mode. For the direct solvers, a two-stage approach is used. In a mechanical analysis, all inter-domain nodes are first given fixed displacements and each domain solves the resulting equation system independently. The second stage operates on the interdomain nodes to relax the extra imposed fixed displacements. This stage is not necessarily if there are no connections between the meshes in the different domains. An iterative procedure based upon the conjugate gradient method is performed for this stage. This procedure operates as mentioned on the inter-domain nodes. The number of conjugate gradient iterations needed to converge to the final solution is reported in the Marc output file as “nn inter-domain iterations”. The conjugate gradient iterative solver (solver type 2) operates simultaneously on the whole model. It works to a large extent like in a serial run. For each iteration cycle, there is a need to synchronize the residuals from the different domains. The third type of solver supported is the hardware solver (HP). These solvers are parallelized themselves using multithreading. They do not support runs over a network so they are only available on shared memory machines. For this case, the global stiffness matrix (or the corresponding matrix for nonstructural analysis) is gathered to the parent process (where the job was started). The original child processes are put to sleep and the solver creates new processes (multiple threads) to solve the equation system in parallel. When the solution is finished, the child processes are awakened and the data related to each domain are distributed.

Contact Contact analysis poses a special challenge for parallelization due to its global nature. The current version of Marc fully supports contact analysis including thermal and electrical contact but excluding beam-tobeam contact.

Main Index

CHAPTER 13 743 Parallel Processing

In order to enable a fast contact search procedure, some contact data are duplicated across all domains. A node in one domain must be able to find contact with a segment in a different domain. The duplicated data includes nodes on the exterior boundary of deformable contact bodies. This data duplication is not necessary in a pure rigid contact job, so it is important to define a contact table to indicate that no deformable contact can take place in this case. The default, if no contact table is used, is that all deformable bodies check for contact with all other bodies including itself. If a node touches a segment which is located in a different domain, the nodes making up the segment are imported into the domain of the touching node. If the node separates, the nodes are deleted from the domain. This means that the number of nodes in a domain can dynamically change. This procedure allows the creation of tyings spanning domains. This also has implications on how the domains should be created. One should avoid having contact bodies with a large number of nodes coming into contact across different domains. An extreme case would be two sheets of equal number of shell elements coming into contact on top of each other. If two domains are used and each sheet is in a separate domain, the number of nodes in one domain would double.

Domain Decomposition The way the model is decomposed into domains, in general, affects the performance of the parallel run. Traditionally, domain decomposition had to be performed in the preprocessor stage using Mentat or MD Patran. Both Mentat and MD Patran use Metis to perform the domain decomposition using the multiple file option. For a single input file case, the domain decomposition can also be performed in Marc. The general goal for a good decomposition is to minimize the number of interdomain nodes. Keeping this number low minimizes the overhead in having duplicate nodes and also minimizes the size of the system solved in the interdomain part of the direct solver. It is important to get a good balance between the workload in the different domains if, for instance, different types of elements are used or if the nodes of a cluster have different performance. Another aspect of deformable contact as mentioned above is to avoid having a large number of nodes touching segments of a different domain. Several different methods for creating the decomposition are available in Mentat and MD Patran. One should note that some of them are based on element connectivity so they tend to put separate contact bodies in separate domains which is not always optimal. The optimal number of domains to use for a given job is pretty hard to estimate. It obviously depends on the number of processors available. There is, in general, an optimal number of processors to use for a given job and a given machine or cluster of machines. A general rule is that the larger the model is, the more it pays off to use more processors.

Running a Parallel Job Running a Marc parallel job is not much different from running a serial job. The model can be decomposed into domains by the preprocessor (Mentat or MD Patran) and a separate input file is created for each domain. From a user’s perspective, the extra steps consist of activating the procedure for decomposing the model and activating the parallel run.

Main Index

744 Marc Volume A: Theory and User Information

Marc can also be used to create the domains in case a single input file containing the whole model is used. Two methods can be used to trigger the single input file option; the first is through the command line option as explained below and the second is through the use of the PROCESSOR parameter. If the command line option is used and the PROCESSOR parameter is not defined, the default domain decomposition method, Metis Best, is used. Currently, the single input file option does not support any additional features that are not supported by the traditional multiple input file option as described by the list of unsupported features above. In addition, the single input file option does not support auxiliary input files and the new table input format. For the case of a run on a cluster, one would additionally have to define which machines make up the cluster (unless an automatic cluster tool is used). The run is started as usual and, by default, separate results files are created for each domain. The postprocessor automatically picks up the results from the different domains and combines them into a single model which looks the same as in a serial run. One can also choose to look at the results of each domain separately, which is particularly useful for large jobs. As opposed to the default multiple post file option, in this release, the user also has the option to request a single post file for the whole model. For details on how to use this functionality, refer to Marc Volume C: Program Input for the POST model definition option. When running a parallel job from Marc Mentat or MD Patran, one has to activate the button for parallel and start the job as for a serial job. From the command line, one needs to use an extra argument to specify the number of domains: run_marc -v n -b n -j jobname -np 5 for running a job with five domains using multiple input files generated by a preprocessor. To indicate that a single input file will be used, the -np option is replaced with -nps and the command line in this case becomes: run_marc -v n -b n -j jobname -nps 5 User subroutines are handled in the same way as in a serial run. See Marc Volume D: User Subroutines and Special Routines for a description on special considerations for user subroutines in a parallel run. Running on a cluster (a set of connected computers) requires that the machines communicate properly. The actual connection could be anything from a telephone modem up to a high speed direct connected cluster. A standard 100 Mbit Ethernet network is usually sufficient for reasonable performance, although it can become bottlenecked with fast processors. Faster connections give better performance on the communication part. In order to perform an analysis over a network, one needs to specify which machines are to be part of the analysis. This is done through a so-called host file, which is generic for a Marc run. The Marc startup script converts it into a format that the current MPI implementation expects. The host file is a simple text file that lists the computers that are to be used in the run and some info about the run. The host file typically looks something like (using a Unix system) host1 2 host2 1 /users/joe/run /programs/marc2003 host3 2 /usr/people/joe /programs/marc/marc2003 Here host1, host2, and host3 are the host names of the respective machines. It specifies a job with five domains where two processes are run on host1 and host3 and one on host2. /users/joe/run is the directory where the job is run on host2. This is where the input files should

Main Index

CHAPTER 13 745 Parallel Processing

be and where the results files are created. This directory could be a local directory on a hard drive on host2 or it could be a shared directory (via NFS for example). This directory must be accessible from host2 (but not necessarily from the other hosts). The fourth entry of the host file specifies where the Marc installation directory is located. This can also be a local directory (if Marc is installed on the local machine) or it can point to a shared directory. It is, in general, recommended that the run directory is a local directory to avoid I/O traffic over the network. Not all MPI implementations currently supported uses the fourth entry. This is for instance true for MP-MPICH that is used on Windows systems. Here the Marc installation directory must be shared. If local run directories are used, one must make sure that the input files are available in the run directory of each host. This can be done by means of a built-in file copy program that is automatically launched when the Marc job is started. Before the analysis starts, the necessary input files are copied over to the respective host. The file copy program uses the same MPI communication as the main Marc program. When the analysis is finished, the file copy program copies the post files back to the directory on host1 where the job was started. Please note that only the input files and the post files (not output files, etc.) are copied. This copying can be suppressed by buttons in Mentat and MD Patran or by a command line option if Marc is manually started. If a user subroutine is used together with local run directories, the new executable automatically transfers to all hosts before the Marc job starts. One can also set up Marc to run via external cluster tools. A useful run time option in this context is the command line option -dir. It specifies the run directory for the job and is where the scratch files and results files are created. Suppose Marc is set up to run on a cluster using some kind of cluster tool to distribute the processes and each machine in the cluster has a local disk called /scratch. By using the -dir /scratch option from the command line, the run uses the local directory during the run. The input files are still read from where the job is started (which could be a shared directory on a control workstation which is not even part of the run). The following command line options related to parallel processing are available for the Marc run_marc start-up script: -np nn

specify nn number of processes.

-nps nn

specify nn number of processes if using a single input file.

-ci y|n

if y, copy input files to local run directories; if n, do not copy.

-cr y|n

if y, copy post files from local run directories; if n, do not copy.

-ho hostfile

specify the host file that describes the hosts to use in a network run.

-dir rundir

specify that the run directory of the run is rundir.

Domain Decomposition Methods Metis Best - method performs Metis element based, Metis node based, and Vector decomposition and picks the best decomposition with respect to the number of interdomain nodes as well as the domains balance. (Figure 13-1) Metis_element_based - performs decomposition of graph constructed from element connectivity. Metis_node_based - performs decomposition of graph constructed from nodal connectivity.

Main Index

746 Marc Volume A: Theory and User Information

Figure 13-1 Metis Best Decomposition

Vector - performs decomposition based on IDs of elements. The element ids are sorted by coordinates of the element centroids. The default direction of sorting is in the maximal dimension of the model bounding box in x-, y-, and z-directions respectively. User may also specify direction of sorting by supplying the direction vector. See Marc Volume C: Program Input, Chapter 2, Parameters – PROCESSOR. (Figure 13-2) Radial - performs decomposition based on IDs of elements. The element ids are sorted by distance between the element centroids and axis of rotation. The default (axis of rotation) is specified by default direction and default point on the axis of rotation. Default point for axis of rotation is defined as the centroid of the model bounding box. User may also specify the axis of rotation by point and direction. See Marc Volume C: Program Input, Chapter 2, Parameters – PROCESSOR. (Figure 13-3) Angular - performs decomposition based on ids of elements. The element ids are sorted by angle between the element centroids, axis of rotation and selected start vector. The default (axis of rotation) is specified by default direction and default point on the axis of rotation. User may also specify the axis of rotation by point and direction. See Marc Volume C: Program Input, Chapter 2, Parameters – PROCESSOR. (Figure 13-4) The Fine Graph flag in the 2nd data block on the PROCESSOR parameter tells Metis to use a fine graph for decomposition. This results in higher memory requirements and lower speed for the decomposition. In some cases, it produces better decomposition than the default (Coarse Graph). The Coarse Graph choice might produce more islands. It is recommended to use the default unless there is a need for better quality of domain decomposition. Sometimes the domain decomposition produces disconnected domains resembling islands (Figure 13-5). The best performance usually is obtained when the domains are contiguous. Islands can be added to neighboring domains by turning on the Island Remove flag in the 2nd data block on the PROCESSOR parameter. This might result in worse balance of domains as shown in Figure 13-6.

Main Index

CHAPTER 13 747 Parallel Processing

Figure 13-2 Vector Decomposition with Specified User Direction (1,1,0)

Figure 13-3 Radial Decomposition with User Direction(.5,.5,.707) and Point on Axis (2,2,2.141)

Main Index

748 Marc Volume A: Theory and User Information

Figure 13-4 Angular Decomposition with User Direction(.5,.5,.707) and Point on Axis (2,2,2.141)

Figure 13-5 Metis Node Based Decomposition without Island Removal

Main Index

CHAPTER 13 749 Parallel Processing

Figure 13-6 Metis Node Based Decomposition with Island Removal

Main Index

750 Marc Volume A: Theory and User Information

Main Index

Chapter 14 Code Coupling Interfaces

14

Main Index

Code Coupling Interfaces

J

Code Coupling

J

Coupling Regions

J

References

752

757

754

752 Marc Volume A: Theory and User Information

This chapter describes the coupling interface to external solvers available through the user subroutine programming. The interface allows code coupling libraries such as MpCCI (see [Ref. 1]) to couple Marc with commercial CFD codes, such as STAR-CD and Fluent. The interface may also be used for developing dedicated interfaces to external solvers, for applying complex boundaries to certain regions of the model, or for dedicated postprocessing.

Code Coupling Analyzing fluid-structure interaction problems has become increasingly important in industrial applications. Effects of the deforming structure on the fluid flow and, vice versa, of the fluid pressure on the structure, as well as heat transfer between fluid and structure can be of critical importance for a design, especially if the deformations of the structure are large. The fluid-structure capabilities of Marc (see Chapter 6 Nonstructural Procedure Library in this manual) are limited to nonreactive, incompressible, single phase, laminar flows. This implies that interaction problems such as combustion reactions in airbag gas generators, involving complex turbulent flows with large deformations of the structure cannot be solved. An additional drawback is that, at the fluid-structure interface, the fluid and structural meshes must share the same nodes. This may be inconvenient, as the fluid analysis tends to require a denser mesh than the structural analysis. Code coupling software, such as the MpCCI (Mesh-based parallel Code Coupling Interface) software from Fraunhofer SCAI (see [Ref. 1]), allows structural codes such as Marc to be coupled with commercial CFD codes such as STAR-CD or Fluent. Fluid-structure interaction problems can then be solved using the capabilities of both solvers in their respective domains. The two solvers run simultaneously and exchange data regularly during the analysis on the common boundary between the fluid and the structure. Figure 14-1 shows a flow chart of such a coupled analysis, in which the CFD solver and the structural solver alternately solve their respective parts of the coupled problem. The CFD solver solves the fluid flow problem for a given period of time (the coupling time step) to provide the pressure that the fluid exerts on the structure, the temperature of the fluid at the common boundary with the structure and the film coefficient to the structural solver. The structural solver applies the fluid pressure and the film boundary condition to the structure and computes the deformations and temperatures of the structure for the same period of time. Then it sends the current coordinates of the nodes and the temperature at the fluid-structure interface to the CFD code. The CFD code uses these coordinates to update the flow domain and continues with the next coupling time step. Note that the coupling time step may consist of multiple time steps in each of the solvers.

Main Index

CHAPTER 14 753 Code Coupling Interfaces

Code Coupling Software CFD Analysis

Structural Analysis

CFD Mesh

Structural Mesh

Initialization

Initialization

CFD Time Step(s) Fluid Pressure, Fluid Temperature, Film Coefficient

Coupling Time Step

Structural Time Step(s) Current Coordinates, Structural Temperature

CFD Time Step(s) Fluid Pressure, Fluid Temperature, Film Coefficient

Coupling Time Step Structural Time Step(s)

Current Coordinates, Structural Temperature

Figure 14-1 Flow Chart of a Coupled Fluid-Structure Analysis Using Code Coupling Software

Main Index

754 Marc Volume A: Theory and User Information

The code coupling software serves as a communication layer between the two codes. It handles the data transfer between the solvers and interpolates the data from the CFD mesh to the structural mesh and vice versa, in case the meshes do not match at the common boundary (Figure 14-2). To be able to interpolate the data from one mesh to the other, the code coupling software determines the geometrical relationship between the meshes, using information (connectivity and coordinates) provided by the two solvers at the start of the analysis. CFD Mesh

Structural Mesh

Figure 14-2 Non-Matching Meshes at the Common Boundary Between Fluid and Structure

The basic stages, from a code coupling point of view, in a coupled analysis are: 1. Initialization. The relationship between the CFD mesh and the structural mesh is established. Both the CFD solver and the structural solver must provide the code coupling software with the connectivity and the coordinates of the patches on the common surface between the fluid and the structure. 2. Data exchange. Physical quantities such as the fluid pressure and the temperature of the fluid at the common surface with the structure, are extracted from the CFD code, interpolated to the structural mesh, transferred to the structural code and applied through appropriate boundary conditions to the structural mesh. Likewise, current coordinates and temperature of the structure at the common surface with the fluid are extracted from the structural code, interpolated to the CFD mesh and transferred to the CFD code. The CFD code uses the new coordinates to update the flow domain. 3. Finalization.

Coupling Regions Coupling regions are the basic concept to couple Marc with external solvers via code coupling software such as MpCCI. A coupling region is that part of the surface or volume of the structural 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. Coupling regions are defined by the COUPLING REGION model definition option and are accompanied by an extensive application programming interface (API). The basic

Main Index

CHAPTER 14 755 Code Coupling Interfaces

mechanical and thermal quantities (current coordinates, displacement, force, pressure, temperature, heat flux, film coefficient) can be exchanged with an external solver on coupling regions via API calls. Quantities that are received from the external solver are applied to the coupling region via boundary conditions. The coupling region API consists of three user subroutines and a set of utility routines that can be called from these user subroutines (see Chapter 9 Special Routines - Marc Post File Processor, Marc Volume D: User Subroutines and Special Routines). The three user subroutines correspond to the basic three stages of a coupled analysis, as outlined in the previous section: 1. Initialization: CPLREG_INIT. This subroutine is called once at the start of the analysis and can be used to extract the connectivity and coordinates of the coupling region and pass it to the code coupling software to determine the geometric relationship between the coupling region mesh and the mesh of the external solver. 2. Data exchange: CPLREG_EXCHANGE. This subroutine is called twice per coupling time step, once at the start and once at the end. The call at the start can be used to set the new values of physical quantities that have been received from the external solver for the next coupling time step. The call at the end can be used to extract the new values of physical quantities that must be sent to the external solver. 3. Finalization: CPLREG_FINALIZE. This subroutine is called once at the end of the analysis and can be used to inform the external solver that the Marc analysis has ended. The utility routines can be called from the user subroutines to obtain the connectivity and coordinates of the coupling region, to obtain the current values of physical quantities on coupling regions, to set the new values of physical quantities for the next coupling time step and even to specify the next coupling time step. The available utility routines are listed in Table 14-1. Table 14-1

Available Utility Subroutines for Coupling Regions

Utility Subroutine

Main Index

Available in User Subroutines

Purpose

CPLREG_FIND_NAME

CPLREG_INIT CPLREG_EXCHANGE

Find coupling regions by name.

CPLREG_GET_INFO

CPLREG_INIT CPLREG_EXCHANGE

Get general information about a coupling region.

CPLREG_GET_QUANTS

CPLREG_INIT CPLREG_EXCHANGE

Get the prescribed physical quantities on a coupling region.

CPLREG_GET_MESH

CPLREG_INIT CPLREG_EXCHANGE

Get the mesh of a coupling region.

CPLREG_GET_GLOBAL_VALUES

CPLREG_EXCHANGE

Get the values of a global quantity.

CPLREG_GET_NODE_VALUES CPLREG_GET_ALL_NODE_VALUES

CPLREG_EXCHANGE

Get the values of a node-based quantity at a coupling region.

756 Marc Volume A: Theory and User Information

Table 14-1

Available Utility Subroutines for Coupling Regions (continued)

Utility Subroutine

Available in User Subroutines

Purpose

CPLREG_PUT_GLOBAL_VALUES

CPLREG_EXCHANGE

Put the values of a global quantity.

CPLREG_PUT_NODE_VALUES CPLREG_PUT_ALL_NODE_VALUES

CPLREG_EXCHANGE

Put the values of a node-based quantity at a coupling region.

CPLREG_PUT_EDGE_VALUES CPLREG_PUT_ALL_EDGE_VALUES

CPLREG_EXCHANGE

Put the values of an edge-based quantity at a coupling region.

CPLREG_PUT_FACE_VALUES CPLREG_PUT_ALL_FACE_VALUES

CPLREG_EXCHANGE

Put the values of a face-based quantity at a coupling region.

CPLREG_PUT_ELEM_VALUES CPLREG_PUT_ALL_ELEM_VALUES

CPLREG_EXCHANGE

Put the values of an element-based quantity at a coupling region.

Time Step Control The default coupling time step is equal to the Marc time step, so that the CPLREG_EXCHANGE user subroutine is called at the start and at the end of each increment. If the AUTO STEP time stepping scheme is used, the coupling time step may be prescribed by calling the CPLREG_PUT_GLOBAL_VALUES utility routine from the CPLREG_EXCHANGE user subroutine. In that case, the AUTO STEP algorithm matches the next coupling time, but multiple increments may be needed to reach this coupling time. If multiple increments are performed within a given coupling time step, then the CPLREG_EXCHANGE user subroutine is called at the start of the first increment and at the end of the last increment of the coupling step.

Shell Elements The top and bottom faces of a shell element are independent surface entities, as far as coupling regions are concerned. They can both be part of the same coupling region or they can be part of two different coupling regions. The faces share the same nodes, but the connectivity of the bottom face, as returned by the CPLREG_GET_MESH utility routine, is exactly the opposite of that of the top face (which is the connectivity of the element). In heat transfer and coupled thermo-mechanical analyses, the temperatures (and nodal heat fluxes) at the top and bottom of a shell element are distinct. If a coupling region contains only top faces of shell elements, the CPLREG_GET_NODE_VALUES utility routine returns the top temperatures (and heat fluxes) at the nodes of the region. Similarly, the CPLREG_PUT_NODE_VALUES utility routine prescribes the top temperatures (and heat fluxes) at the nodes of the region. If the coupling region contains only bottom faces of shell elements, these routines return and prescribe the bottom temperatures (and heat fluxes) at the nodes. If both the top and the bottom faces of shell elements interact with the mesh

Main Index

CHAPTER 14 757 Code Coupling Interfaces

of an external solver, two coupling regions must be defined to properly access the temperatures and nodal heat fluxes on both sides of the shell elements: one containing the top faces and the other the bottom faces of the shells.

Parallel Processing In a parallel run with Marc, the finite element mesh is subdivided into domains where each element is part of one domain. Nodes at the boundary between domains are present in all domains sharing that boundary. Coupling regions are allowed to span multiple domains. If a physical quantity is prescribed on a such a coupling region, using the CPLREG_PUT_NODE_VALUES utility routine, the value of the quantity for a given node must be the same in all domains in which the node appears. Similarly, if the coupling time step is prescribed via CPLREG_PUT_GLOBAL_VALUES, the value must be the same in all domains.

References 1. Fraunhofer Institute for Algorithms and Scientific Computing SCAI. MpCCI 3.0.4: Manuals and Tutorials. April 25, 2005, http://www.scai.fraunhofer.de/mpcci.

Main Index

758 Marc Volume A: Theory and User Information

Main Index

Appendix A Finite Element Technology in Marc

A

Main Index

Finite Element Technology in Marc J

Governing Equations of Various Structural Procedures

J

System and Element Stiffness Matrices

J

Load Vectors

J

References

763 764

762

760

760 Marc Volume A: Theory and User Information

Governing Equations of Various Structural Procedures This section describes the basic concepts of finite element technology. For more information, you are urged to refer to the finite element text [Ref. 5]. Marc was developed on the basis of the displacement method. The stiffness methodology used in Marc addresses force-displacement relations through the stiffness of the system. The force-displacement relation for a linear static problem can be expressed as Ku = f

(A-1)

where K is the system stiffness matrix, u is the nodal displacement, and f is the force vector. Assuming that the structure has prescribed boundary conditions both in displacements and forces, the governing Equation (A-1) can be written as K 11 K 12 ⎧ u 1 ⎫ ⎧ f1 ⎫ ⎨ ⎬ = ⎨ ⎬ K 21 K 22 ⎩ u 2 ⎭ ⎩ f2 ⎭

(A-2)

u 1 is the unknown displacement vector, f 1 is the prescribed force vector, u 2 is the prescribed displacement vector, and f 2 is the reaction force. After solving for the displacement vector u , the strains in each element can be calculated from the strain-displacement relation in terms of element nodal displacement as ε e l = βu e l

(A-3)

The stresses in the element are obtained from the stress-strain relations as σ e l = Lε e l

(A-4)

where σ e l and ε e l are stresses and strains in the elements, and u e l is the displacement vector associated with the element nodal points; β and L are strain-displacement and stress-strain relations, respectively. In a dynamic problem, the effects of mass and damping must be included in the system. The equation governing a linear dynamic system is Mu·· + Du· + Ku = f

(A-5)

where M is the system mass matrix, D is the damping matrix, Equation (A-6) is the acceleration vector, and u is the velocity vector. The equation governing an undamped dynamic system is Mu·· + Ku = f

(A-6)

The equation governing undamped free vibration is Mu·· + Ku = 0

Main Index

(A-7)

APPENDIX A 761 Finite Element Technology in Marc

Natural frequencies and modal shapes of the structural system are calculated using this equation. 2

Kφ – ω Mφ = 0

(A-8)

The equations governing some other procedures are similar. For example, the governing equation of transient heat transfer analysis is · CT T + KT T = Q

(A-9)

where C T is the heat capacity matrix, K T is the thermal conductivity matrix, Q is the thermal load vector (flux), T is the nodal temperature vector, and t is the time derivative of the temperature. Equation (A-9) reduces to KT T = Q

(A-10)

for the steady-state problem. Note that the equation governing steady-state heat transfer (Equation (A-10)) and the equation of static stress analysis (Equation (A-1)) take the same form. Similarly, the hydrodynamic bearing problem is analogous to a steady-state heat transfer problem. This problem is governed by an equation similar to Equation (A-10). The matrix equation of the electrical problem in coupled thermo-electrical analysis is K E ( T )V = I

(A-11)

The equation governing the thermal problem is: · E C T ( T )T + K T ( T )T = Q + Q

(A-12)

in both Equation (A-11) and Equation (A-12), v is the voltage, K E ( T ) is the temperature-dependent electrical-conductivity matrix, I is the nodal-current vector, C T ( T ) is the temperature-dependent, heatcapacity matrix, and K T ( T ) is the thermal-conductivity matrix. T is the nodal temperature vector, Q E

is the heat-flux vector, and Q is the internal heat-generation vector that results from the electrical E

current. Electrical and thermal problems are coupled through K E ( T ) and Q . The matrix equations for the thermal-mechanical problem are as follows:

Main Index

Mu·· + Du· + K ( T ,u ,t )u = F

(A-13)

· I C T ( T )T + K T ( T )T = Q + Q + Q F

(A-14)

762 Marc Volume A: Theory and User Information

In Equations (A-13) and (A-14) the damping matrix D , stiffness matrix K , heat-capacity matrix C T and I

thermal-conductivity matrix K T are all dependent on temperature. Q is the internal heat generated due to inelastic deformation. The coupling between the heat transfer problem and the mechanical problem is due to the temperature-dependent mechanical properties and the internal heat generated. If an updated Lagrangian analysis is performed, K and K T are dependent upon prior displacement. The governing equations described above are either sets of algebraic equations (Equations (A-1), (A-10), and (A-11)), or sets of ordinary differential equations (Equations (A-5) through (A-8) and all equations through Equation (A-4)). The time variable is a continuous variable for the ordinary differential equations. Select an integration operator (for example, Newmark-beta, Houbolt, or central difference for dynamic problems, and backward difference for heat transfer) to reduce the set of differential equations to a set of algebraic equations. The final form of governing equations of all analysis procedures is, therefore, a set of algebraic equations.

System and Element Stiffness Matrices The previous section presented system matrices assembled from element matrices in the system. For el

example, the system stiffness matrix K is expressed in terms of the element stiffness matrix K i as N el

∑

K =

(A-15)

Ki

i = 1

where N is the number of elements in the system. The system stiffness matrix is a symmetric-banded matrix. See Figure A-1 for a schematic of the assemblage of element matrices. When the element-byelement iterative solver is used, the total stiffness matrix is never assembled. The element stiffness matrix can be expressed as K

el

v

where v relation.

T

∫

=

β Lβdv

el

(A-16)

el

el

is the volume of the element, β is the strain-displacement relation, and L is the stress-strain

ε = βu

(A-17)

σ = Lε

(A-18)

The mass matrix can be expressed as M

el

=

∫ v

Main Index

el

T

N ρNdv

(A-19)

APPENDIX A 763 Finite Element Technology in Marc

1

2 2

3

1 (a)

3

5

4 5

4 6

8 7 1

2

3

4

5

δ

(b)

[K]

(c)

{F}

δ

Band

Figure A-1

Schematic of Matrix Assemblage

The integration in (A-16) is carried out numerically in Marc, and is dependent on the selection of integration points. The element stiffness matrix can be fully or under integrated. The mass matrix is always fully integrated. Note:

The β matrix is directly associated with the shape functions and geometry of each element. Shape functions associated with different element types are explained in Marc Volume B: Element Library. Stress-strain relations L are discussed in Chapter 7 of this volume.

Load Vectors The nodal force vector f in (A-1) includes the contributions of various types of loading. f = f p o i n t + f s u r f a c e + f b o d y + f∗

(A-20)

where f point is the point load vector, f surface is the surface load vector, f body is the body (volumetric) load vector, and f* represents all other types of load vectors (for example, thermal and creep strains, and initial stress).

Main Index

764 Marc Volume A: Theory and User Information

The point load is associated with nodal degrees-of-freedom and can be added to the nodal force vector directly. Equivalent nodal force vectors f surface , f body y must be calculated from the distributed (surface/volumetric) load first and then added to the nodal force vector. In Marc, the computation of equivalent nodal forces is carried out through numerical integration of the distributed load over the surface area of volume to which the load is applied. This can be expressed as f s u rf a c e =

∫N

T

pdA

(A-21)

A

fb o d y =

∫N

T

pdV

(A-22)

V

where p is the pressure. Figure A-1 shows the assemblage of the nodal force vector.

References 1. Zienkiewicz, O. C. and R. L. Taylor. The Finite Element Method (4th ed.) Vol. 1. Basic Formulation and Linear Problems (1989),) Vol. 2. Solid and Fluid Mechanics, Dynamics, and Nonlinearity (1991) McGraw-Hill Book Co., London, U. K. 2. Bathe, K. J. Finite Element Procedures, Prentice-Hall, Englewood Cliffs, NJ, 1995. 3. Hughes, T. J. R. The Finite Element Method–Linear Static and Dynamic Finite Element Analysis, Prentice-Hall, Englewood Cliffs, NJ. 1987. 4. Ogden, R. W. “Large Deformation Isotropic Elasticity: On The Correlation of Theory and Experiment for Incompressible Rubberlike Solids,” Proceedings of the Royal Society, Vol. A (326), pp. 565-584, 1972. 5. Cook, R. D., D. S. Malkus, and M. E. Plesha, Concepts and Applications of Finite Element Analysis (3rd ed.), John Wiley & Sons, New York, NY, 1989.

Main Index

Appendix B Finite Element Analysis of NC Machining Processes

B

Main Index

Finite Element Analysis of NC Machining Processes J

General Description

J

NC Files (Cutter Shape and Cutter Path Definition)

J

Intersection Between Finite Element Mesh and Cutter

J

Deactivation of Elements

J

Adaptive Remeshing

J

Input of Initial Stresses

766

768

768 769

766 768

766 Marc Volume A: Theory and User Information

General Description Machining (or Metal Cutting) is a type of material removal processes widely used to produce a part with the desired geometry. After removal of the machined material, re-establishment of equilibrium within the remaining part of the structure causes some distortion due to the relief of the residual stresses in the machined materials. Depending on the stress level and geometry of the part, the severe distortion due to machining can result in high scrap rates and increased manufacturing costs, especially for structures with thin wall or large thin plates. A numerical analysis procedure has been developed in Marc to predict the distortion during the 3-D bulk machining so that engineers can optimize their structure design and machining processes. This procedure is based on the assumption that effects introduced by the cutting process are local and small compared to those due to pre-existing residual stresses. The simulation procedure uses the cutter shape and path information obtained from NC machining data. Cutter motion information is used to predict the material to be removed by automatically deleting finite elements that are located within the cutter path. The distortion of the remaining part can be predicted by re-calculating the equilibrium. An interface has been developed in Marc to convert cutter path data into the finite elements to be removed. The cutter path data is stored in either the Automatically Programmed Tools (APT) source or the Cutter Location (CL) data format. The APT source is the NC data output by CAD software CATIA. The CL data is the cutter location data provided by APT compilers. For details on how to use this functionality, refer to Marc Volume C: Program Input for the MACHINING parameter and the DEACTIVATE model definition option and the DEACTIVATE history definition option.

NC Files (Cutter Shape and Cutter Path Definition) The cutter shape and the cutter path are the key parameters to determining the volume of the material to be cut. The cutter shape is defined by the CUTTER statement in the APT source or CL files. The expanded form of the CUTTER statement is as follows: CUTTER ⁄ d ,r ,e ,f ,α ,β ,h where the parameters

Main Index

d

The tool diameter.

r

The radius of the corner circle; it can be zero or larger than d ⁄ 2 .

e

The radial distance from the tool axis to the center of the corner circle.

f

The distance from the tool endpoint to the center of the corner circle measured parallel with the tool axis.

α

The angle from a radial line through the tool endpoint to the lower line segment; it is in range of zero to 90°, and positive.

β

The angle between the upper segment and the tool axis; it is in the ranges of -90° to 90°.

h

The cutter height measured from the tool endpoint along the tool axis.

APPENDIX B 767 Finite Element Analysis of NC Machining Processes

have the following meaning as shown in Figure B-1. Tool axis

Upper Line segment

β

h

Envelope e Lower line segment

r f

α Endpoint d

Figure B-1

Definition of Cutter Geometry

The cutter path is calculated based on the motion of the cutter and cutter shape. The motion is defined by cutter motion statements like GOTO/, GODLTA/, CYCLE/, and DRILL/, etc. In Marc, these motion types are translated into point-to-point, circular, or drilling motion modes, respectively. For details, refer to references by Irvin H. Kral and Dassault Systems. Notes:

1. Marc accepts APT data files written by CATIA V4 and the corresponding CL data files by APT compilers. 2. The cutter can be of either multi-axis or fixed axis. 3. Two cutter motion types: Point-To-Point (for example, GOTO/ and GODLTA/ statements) and Cycle (DRILL/…) are directly supported. Circular motions (either in-plane or out-ofplane) can be interpolated into Point-To-Point motions. The interpolation can be done inside CATIA by choosing the proper option when writing out APT source file. 4. In addition, some statements in the APT/CL files are skipped. If the user chooses statements like TRACUT/, COPY/, /MACRO, or /CALL to define cutter motions, they must be converted into explicit motion statements like Point-to-Point or Cycle (DRILL/) motions before writing out the APT data file. The cutting process is stopped if statements, such as /FINI, /STOP, or /END, or the end of APT/CL file is reached. 5. It is assumed that the part and cutter are defined in the same coordinate system. So, if a part needs to be flipped over between two machining stages, the user can rotate the cutter but keep the part unchanged in space.

Main Index

768 Marc Volume A: Theory and User Information

6. If the user wants to change the boundary conditions for some nodes during the cutting process defined by one APT/CL file, time synchronization should be turned on when defining the machining load case. 7. For visualization purpose, the user can specify a contact surface as cutter surface. During postprocessing, user will be able to visualize the cutter motion along the cutting process. In order to do this, you MUST exclude this cutter surface ID from all kinds of contact checking during analysis. The user can do this by creating CONTACT TABLE and turn off the contact body ID of the cutter surface. In addition, it is also necessary to make sure that the cutter surface is initially set at the location of the origin of the coordinate system and the orientation is initially set to be in the direction of Z-axis.

Intersection Between Finite Element Mesh and Cutter When the cutter moves, its path forms the volume of the material to be cut. This volume is calculated based on the cutter geometry and its path in space. The finite element mesh is checked against this volume to decide the intersection between the volume and the finite element nodes and elements.

Deactivation of Elements The automatic deactivation of finite elements depends on the intersection status between the cutter path and the mesh. The approach is designed for elements that are fully or partially located inside the cut volume. Elements that are fully located inside the cut volume are automatically deactivated and the stress that existed before deactivation is released. For elements that are partially intersected by the cut volume, integration points are checked. In the current version, the check of integration points is limited to the element centroid only. If element centroid is found inside the cut volume, the associated element is deactivated. For deactivated elements, the stresses/strains are set to zero permanently. After the deactivation of elements along the motion of cutter, the part will distort progressively. The updated geometry of the part is used for the next cutting step. Using this method, the whole machining process is simulated with Marc. After the machining is finished, the final distortion of the work piece can be calculated by spring back analysis. The spring back analysis is conducted by removing all fixturing restraints except for those needed to remove rigid body motion.

Adaptive Remeshing Generally speaking, the accuracy of the finite element analysis of machining processes depends on, plays a key role to get the accuracy of initial (residual) stresses. Accurate initial stress the correct deformation of the part. From the view point of FE analysis, the initial FE mesh may affect the accuracy significantly. Finer mesh is needed for accuracy but it results in higher analysis cost due to the increased number of finite elements and increased total number of analysis increments. Also, for most machining processes, the cutter path is complicated enough that it is not possible to properly define the best suited fine mesh at the beginning of the analysis. The adaptive remeshing technology has been enhanced in Marc to obtain accurate results for the FE mesh located inside the cutter path.

Main Index

APPENDIX B 769 Finite Element Analysis of NC Machining Processes

An element is subdivided if the cutter only cuts part of the element in the current cutting step. For example, one 3-D brick element generates 8 new elements after first level subdivision and 64 new elements after the second level subdivision. Therefore, users need to be aware of the potentially large number of new elements with increased levels of subdivision.

Typical Features for Machining 1. Multiple level subdivision of element in one incremental step: Typically, Marc subdivides only once per load step. If the 17th criterion of ADAPTIVE model definition option is used (for NC machining), Marc automatically subdivides the element until the maximum specified level has been reached. This process may generate a huge number of new elements and nodes. Consequently, these newly created elements and nodes may result in excessive memory usage and CPU time, though most of them are immediately cut off. For some problems, it is possible to cut the part with a few large elements but without sacrifice of accuracy if only allowing remeshing to be conducted at some specific locations of the part where finer meshing is required. In such circumstances, it might be reasonable to conduct one round of rough cutting followed by fine cutting based on finer mesh after adaptive remeshing. Details are described in Item 3. 2. ADAPTIVE REMSHING at EACH increment: At the load case of machining, Marc does adaptive remeshing at each increment based on the intersection of the cuter path and the FE mesh. 3. ADAPTIVE REMSHING at LAST increment: A cutting analysis in Marc is not done without adaptive remeshing until the cutting process is completed. However, the cutting process may not be completely finished yet because some elements that are partially cut by cutter are still retained. In order to cut those elements off, the cutter path is re-calculated and those elements that are partially cut are subdivided in order to improve the accuracy of the cutting. In this case, extra incremental steps are added into this machining load case. The added number of extra load steps equal the maximum subdivision level that is defined by the ADAPTIVE option.

Input of Initial Stresses There are various approaches to input the initial stresses into the FE model for machining analysis. Generally speaking, Marc allows user to input the initial stress through the INIT STRESS model definition option. It also allows user to import the data through the PRE STATE option. With the PRE STATE option, the user can transfer information, including strain, stress etc., from previous analysis into the model for new analysis. By using option of INIT STRESS, user may define the stress based on the input values or tables (if the stresses are defined as function of, say, coordinates). Marc also allows the user to define the initial stresses with an ASCII format text file. The text file contains the raw initial stress data of points randomly located in a space field. In Marc, the given initial stress data is processed and interpolated into the finite element mesh according to the location of each element. For details about this data structure and format, see INIT STRESS model definition option in Marc Volume C: Program Input.

Main Index

770 Marc Volume A: Theory and User Information

References 1. Irvin H. Kral, Numerical Control Programming in APT, Prentice-Hall, 1986. 2. Dassault Systems, CATIA Training Guide, Version 4, Release 1.6, April, 1996. 3. Houtzeel Manufacturing systems, Inc., APT Language Reference Manual, March, 1997.

Main Index

MSC.Fatigue Quick Start Guide

Index Marc Volume A: Theory and User Information ABCDEFGHIJKLMNOPQRSTUVWXYZ Index I

N

D

E

X

A ablation 255 ABLATION (parameter) 255, 256 acoustic analysis 312, 513, 597, 669, 728, 730 element types 313, 331 input options 597 ACOUSTIC (parameter) 314 ACTIVATE (history definition option) 59 ADAMS 736 ADAPT GLOBAL (model definition option) 256 ADAPTIVE (model definition option) 82, 101, 102, 675 ADAPTIVE (parameter) 675 adaptive mesh contact 554 global 85 local 82 refinement 675 adaptive time control 141 ALL POINTS (parameter) 287, 664 ALLOCATE (parameter) 32 analysis 337, 512 acoustic 312, 513, 597, 669, 728, 730 contact 730 coupled 323, 545 coupled acoustic-structural 328 coupled contact 545 coupled electromagnetic-thermal 341 coupled electrostatic-structural 669 coupled thermo-electrical (Joule heating) 335 coupled thermo-mechanical 326 crack 147 creep 680 design sensitivity 200 dynamic 729 eigenvalue 166 electrical 596

Main Index

electristatic-structural 513 electromagnetic 304, 513, 598, 670, 730 electromagnetics 728 electrostatic 513, 597, 669, 728, 730 electrostatic-structural 730 electro-structural 728 error 79 fluid 314, 514, 670 fluid/solid interaction 331, 513, 669 Fourier 102 harmonic 308 heat transfer 226, 512, 595, 727, 729 hydrodynamic bearing 292, 513, 596, 670, 730 Joule heating 729 large strain 672, 673 linear 100 magnetostatic 300, 513, 670, 728, 730 nonlinear 105 perturbation 123 piezoelectric 309, 512, 598, 670, 728, 730 post buckling 680 rigid cavity acoustic 312 rigid-plastic 188, 673, 729 snap-through 680 soil 193, 487, 670 steady state rolling 211 stress 728 structural zooming 214 thermal contact 548 thermo-electrical 512 analytical contact 561 ANELAS (user subroutine) 101, 347, 350 ANEXP (user subroutine) 101, 350, 482 ANISOTROPIC (model definition option) 101, 289, 310, 347, 349, 353, 374, 434, 446, 480 anisotropic viscoelastic material 470 ANKOND (user subroutine) 227, 512 ANPLAS (user subroutine) 350, 434 application phase 164

772 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ APPROACH (history definition option) 526 Arbitrary Eularian-Lagrangian (AEL) formulation 119 arc-length methods 695 ASSEM LOAD (model definition option) 737 ASSUMED STRAIN (parameter) 675 assumed strain formulation 675 ATTACH EDGE (model definition option) 81, 584 ATTACH FACE (model definition option) 584 AUTO CREEP (history definition option) 141, 143, 146, 147, 466, 679, 680 AUTO INCREMENT (history definition option) 72, 122, 487, 587, 679, 680, 682, 698 AUTO LOAD (history definition option) 72, 335, 475, 587, 679 AUTO STEP (history definition option) 146, 171, 228, 232, 335, 342, 470, 475, 487, 560, 567, 593, 679, 680, 681, 683, 684, 685, 686, 688, 689, 690 AUTO THERM (history definition option) 593, 679, 680, 681 AUTO THERM CREEP (history definition option) 145, 679, 680 automatic global remeshing 85 Automatic Thermally Loaded Elastic-Creep/ElasticPlastic-Creep Stress Analysis (AUTO THERM CREEP) 145 Automatically Programmed Tools (APT) 766 AUTOMSET (parameter) 621 AUTOSPC (parameter) 545 AXITO3D (model definition option) 210

B bandwidth optimization 70 Barlat’s (1991) yield function 435 beam elements 667, 726 pin code 636 BEAM SECT (parameter) 74, 651, 652, 667 beam-shell offsets 632 adaptive meshing 635 contact 635 dynamics 636 field analysis 635 offset vector specification 634 post file 635 supported elements 635

Main Index

beam-to-beam intersection tying constraints 608 BEARING (parameter) 292 BEGIN SEQUENCE (history definition option) 593 behavior incompressible 125 nearly incompressible 127 nonlinear 679 Bergan and Mollestad 689 B-H RELATION (electromagnetic, model definition option) 309, 513 B-H RELATION (magnetostatic, model definition option) 301, 302, 513 Bingham fluid 316 block definition 60 body motion 524 boundary conditions input options 600 loading types 571 time-dependent 178 treatment of 128 breaking glue 544 BUCKLE (history definition option) 122, 123 BUCKLE (parameter) 105, 122 BUCKLE INCREMENT (model definition option) 105, 122, 123 buckling analysis 122 bushing coordinate system 623 bushings 622 nodal offsets for elements 623 properties 624

C Cam-Clay model 488 capacitor 298 Carreau model 317 CASE COMBIN (model definition option) 101, 103, 691 CASI iterative solver 188, 707, 708, 709, 710 cavity pressure loading 588 radiating 279 rigid, acoustic analysis 312 surface elements 592, 674

773 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ

Main Index

CAVITY DEFINITION (model definition option) 272,

CONSTRAINT (model definition option) 63

282, 284, 596 central difference operator 172, 175, 176, 177 CENTROID (parameter) 112, 115, 121, 287, 593, 664, 691, 702, 723, 729 CFAST (model definition option) 622, 639, 656, 657, 658, 659, 660, 661 Chaboche 449, 464 CHANGE PORE (model definition option) 197 CHANGE STATE (history definition option) 145, 681 CHANGE STATE (model definition option) 34, 227, 287, 593 CHANNEL (model definition option) 227, 325 classical lamination theory, multi-Layered shells 352 closest point projection procedure 136 code coupling basic stages 754 software 752 COEFFICIENT (model definition option) 625 COHESIVE (model definition option) 672 cohesive zone 504 coking 249 linear model 251 water drying model 251 combined hardening 444 common material characteristics 123 COMPOSITE (model definition option) 207, 348, 349 composite continuum elements 349 composite material 348 conditioning number 708 CONN FILL (model definition option) 70 CONN GENER (model definition option) 70 CONNECT (model definition option) 64 connection methods 637 CONNECTIVITY (model definition option) 59, 69, 326, 338, 342, 622, 639, 646, 652, 653, 656 Conrad Gap 285 CONRAD GAP (model definition option) 227 constant dilatation elements 673 constitutive relations 447 constraint rigid link 613

contact adaptive meshing 554 analysis 730 analytical 561 beams 551 bodies 518 constraint implementation 530 coupled 545 deformable 564 detection 526 dynamic 553 friction modeling 532 mathematical aspects 557 neighbor relations 529 optimize ordering 521 quadratic 551 release 545 separation 544 shell 528, 553 thermal 548 tolerance values 556 CONTACT (model definition option) 119, 120, 128, 172, 227, 271, 335, 518, 520, 551, 553, 558, 571, 620, 626, 684 CONTACT CHANGE (rezoning option) 554 CONTACT NODE (model definition option) 519 contact penetration criteria, remeshing 91 CONTACT TABLE (history definition option) 526, 545 CONTACT TABLE (model definition option) 532, 542, 543, 544, 547, 548, 553, 566 CONTINUE (history definition option) 44, 50, 51 continuum composite elements 674 interlaminar stresses 371 continuum elements 666 CONTROL (electromagnetic, model definition option) 305 CONTROL (heat transfer, model definition option) 326 CONTROL (history definition option) 145, 229, 629, 634, 679 CONTROL (magnetostatic, model definition option) 301

774 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ CONTROL (model definition option) 112, 123, 228,

280, 557, 629, 634, 679, 684, 721 control algorithm 72 convergence controls 168 CONVERT (model definition option) 327, 339, 342 COORD SYSTEM (model definition option) 356, 525, 623 COORDINATES (model definition option) 59, 69, 652, 726 Coulomb friction model 533 arctangent model 534 bilinear model 539 stick-slip (modified step function) model 536 COUPLE (parameter) 326, 338 coupled acoustic-structural analysis 328 acoustic medium 330 divergence theorem of Green 329 fluid pressure 330 harmonic analyses 328 coupled analysis 323, 545 coupled contact analysis 545 coupled electrical-thermal-mechanical 337 coupled electrical-thermal-mechanical analysis 337 coupled electrostatic-structural analysis 513 coupled emectromagnetic-thermal analysis 341 coupled thermo-electrical analysis (Joule heating) 335 coupled thermo-mechanical analysis 326 coupling interface 752 coupling region parallel processing 757 shell elements 756 time step 756 coupling regions 754 crack analysis 147 CRACK DATA (model definition option) 485 cracking closure 487 low tension 486 uniaxial 485 Craig-Bampton 736 creep 140 buckling 144 control tolerances 142

Main Index

implicit formulation 462 Maxwell model 456 CREEP (model definition option) 146, 457, 458, 463, 466, 481 CREEP (parameter) 144, 146, 147, 456, 462, 463, 465 creep analysis 680 CREEP INCREMENT (history definition option) 679 Crisfield 698, 699 criteria equivalent values 84 mean strain energy 82 node within a box 84 nodes in contact 84 previously refined mesh 85 remeshing 90 temperature gradient 84 user-defined 85 Zienkiewicz-Zhu 83 Zienkiewicz-Zhu creep strain 84 CRPLAW (user subroutine) 141, 142, 143, 147, 457, 458, 461, 463, 466, 482 CRPVIS (user subroutine) 146, 456, 465, 466 crushing 487 cure kinetics 217 CURE SHRINKAGE (model definition option) 217 CURVES (model definition option) 81 Cutter Location (CL) 766 CWELD (model definition option) 639, 644, 645, 646, 647, 648, 649, 650, 651, 652, 653, 655, 656, 657, 658, 659, 660, 661 CWELD patch-to-patch connections 639 direct 640 indirect 641 cyclic Loading 593 cyclic symmetry tying constraints 625 CYCLIC SYMMETRY (model definition option) 626, 627 CYLINDRICAL (model definition option) 59, 635

D DAMAGE (model definition option) 376, 504

775 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ damage models cohesive zone 504 ductile metals 499 elastomers 501 damping 180 DAMPING (model definition option) 169, 180, 182 DAMPING COMPONENTS (history definition option) 293 deact glue 544 DEACT GLUE (model definition option) 157, 161, 544 deactivate 59 element method 269 DEFINE (model definition option) 43, 44, 45 deformable contact, solution strategy 566 deformable-deformable contact 564 degree of freedom transformation 600 DELAMINATION (model definition option) 165 DENSITY EFFECTS (model definition option) 440 DESIGN DISPLACEMENT CONSTRAINTS (model definition option) 208 DESIGN FREQUENCY CONSTRAINTS (model definition option) 208 DESIGN OBJECTIVE (model definition option) 207 design optimization 202 DESIGN OPTIMIZATION (parameter) 207, 347 DESIGN SENSITIVITY (parameter) 207, 347 design sensitivity analysis 200 design space 204 DESIGN STRAIN CONSTRAINTS (model definition option) 208 DESIGN STRESS CONSTRAINTS (model definition option) 208 DESIGN VARIABLES (model definition option) 207 diffusion 289 DIFFUSION (parameter) 289 dilatational creep 462 direct constraints 558 integration 171 mesh definition input 54 methods 707 DISP CHANGE (history definition option) 145, 327, 339, 618

Main Index

DIST CHARGE (electromangetic, model definition

option) 305 DIST CHARGE (model definition option) 310, 335 DIST CHARGES (electrostatic, model definition

option) 296, 335, 342 DIST CURRENT (electromagnetic, model definition

option) 305 DIST CURRENT (history definition option) 339 DIST CURRENT (Joule, history definition option)

335, 336, 342 DIST CURRENT (magnetostatic, model definition

option) 301 DIST CURRENT (model definition option) 339 DIST FLUXES (history definition option) 336, 339,

342 DIST FLUXES (model definition option) 193, 226,

232, 293, 336, 339 DIST LOADS (history definition option) 145, 339 DIST LOADS (model definition option) 194, 310,

335, 339, 585, 587 DIST LOADS (parameter) 207 DIST MASS (model definition option) 289 DIST SOURCE (model definition option) 314

Domain Decomposition Method (DDM) 740, 745 ductile metals 499 dynamic analysis 729 crack propagation 159, 164 fracture methodology 163 impact 553 DYNAMIC (parameter) 105, 164, 166, 169, 171 DYNAMIC CHANGE (electromagnetic, history definition option) 305, 308 DYNAMIC CHANGE (history definition option) 169, 171, 177, 314, 332, 679

E Edge I-J orientation 354 effects of temperature and strain rates on yield stress 441 eigenvalue analysis 166 ELASTIC (parameter) 79, 100, 101 elastic models 488 ELASTICITY (parameter) 101 elastomeric material 419

776 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ elastomers 501 electrical analysis 596 input options 597 ELECTRO (parameter) 296, 334 electromagnetic analysis 304, 513, 598, 670, 730 element types 305 input options 305, 598 electromagnetics analysis 728 electrostatic analysis 513, 597, 669, 728, 730 Coulomb force 333 coupled electrostatic-structural 333, 513, 598, 669 element types 296 input options 597 electrostatic-structural analysis 728, 730 ELEM SORT (model definition option) 722 element distortion criteria, remeshing 90 elements acoustic analysis 313, 331 beam 667, 726 beams, contact 551 cavity surface 674 classes of stress-strain relations 350 composite continuum 349 connectivity data 55 constant dilatation 673 contact 550 continuum 666 continuum composite 674 deactivate 269 electromagnetic 305 electrostatic 296 fluid 322 Fourier analysis 104 gap-and-friction 671, 727 heat transfer 668 heat transfer convection 288 hydrodynamic bearing 292 incompressible 672 magnetostatic 300 membrane 666 Main Index

piezoelectric 309 plate 668 quarter point 164 rebar 672 reduced integration 673 semi-infinite 674 shell 553, 668 special 671 truss 666 ELEMENTS (parameter) 165, 639, 653, 656, 664 ELEVAR (user subroutine) 723, 726 ELEVEC (user subroutine) 723 EL-MA (parameter) 305, 342 ELSTO (parameter) 31, 32, 33, 34, 716 EMCAPAC (history definition option) 298 EMISSIVITY (model definition option) 282 EMRESIS (history definition option) 340 END (parameter) 50 END OPTION (model definition option) 42, 50, 51, 207, 314 END REZONE (rezoning option) 51 END SEQUENCE (history definition option) 593 Equivalent Values Criterion 84 error analysis 79 ERROR ESTIMATE (model definition option) 79, 102, 128 Eulerian formulation 118 examples of lists input 45 EXCLUDE (history definition option) 528 EXTENDED (parameter) 43

F FAIL DATA (model definition option) 357, 372, 373,

374, 486 FEATURE (parameter) 629, 634

file units 33 FILM (user subroutine) 227, 232, 233, 234, 336, 339, 342, 595, 596 FILMS (model definition option) 226, 232, 244, 271, 336, 339, 342, 595 FILMS (with TABLE input, model definition option) 596 finite element technology basic concepts 760

777 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ

Main Index

FIXED DISP (model definition option) 59, 63, 194,

FORCEM (user subroutine) 81, 178, 305, 310, 335,

310, 327, 332, 335, 339, 618 FIXED POTENTIAL (electromagnetic, model definition option) 305 FIXED POTENTIAL (electrostatic, model definition option) 296, 342 FIXED POTENTIAL (magnetostatic, model definition option) 301 FIXED PRESSURE (model definition option) 193, 289, 292, 314 FIXED TEMPERATURE (model definition option) 226, 231, 282, 323, 327, 336, 339, 342 FIXED VELOCITY (model definition option) 323 FIXED VOLTAGE (model definition option) 335, 339 FLD (Forming Limit Diagram) 731 flow diagram 711 rule 446 FLP (Forming Limit Parameter) 731 fluid analysis 314, 514, 670 elements 322 FLUID (parameter) 670 FLUID DRAG (model definition option) 587 fluid drag and wave input options 587 loads 587 fluid mechanics 314 Bingham fluid 316 Carreau model 317 element types 322 piecewise non-Newtonian flow 316 power law fluid 316 FLUID SOLID (model definition option) 331 fluid/solid interaction analysis 331, 513, 669 FLUX (user subroutine) 227, 232, 234, 293, 296, 301, 310, 314, 335, 336, 339, 342, 595, 596 FOAM (model definition option) 475 FOLLOW FOR (parameter) 112, 121, 585, 586, 603, 675 follow force stiffness contribution 675 FORCDF (user subroutine) 342 FORCDT (user subroutine) 178, 231, 234, 293, 296, 301, 310, 323, 335 force components 572

342 Forming Limit Diagram (FLD) 731 Forming Limit Parameter (FLP) 731 FOUNDATION (model definition option) 101, 121 FOURIER (model definition option) 101, 102, 105 FOURIER (parameter) 102, 105 Fourier analysis 102 coefficients 103 elements used 104 fractal dimension 707 fracture mechanics 147 friction modeling 532 FXORD (model definition option) 65, 69, 668

G gap-and-friction element 671, 727 gasket 378 GASKET (model definition option) 381 generalized alpha operator 172, 175 HHT 176 spectral radius 176 generation phase 163 GENT (parameter) 115 geometric domains 665 GEOMETRY (model definition option) 74, 207, 292, 633, 636, 649, 650, 651, 652, 668, 673, 675, 726 global meshing 554 ZX plane orientation 355 GLOBALLOCAL (model definition option) 34, 214 glue model, friction 543 gradient objective or response function 200 pressure 194 Gurson model, modified 499

H harmonic analysis 308 response 181 HARMONIC (electromagnetic, history definition option) 309

778 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ HARMONIC (electromagnetic, history definition)

342 HARMONIC (parameter) 182, 183 Hashin fabric failure criterion 364 failure criterion 363 tape failure criterion 365 HEAT (parameter) 287, 288, 342, 669 heat fluxes 546, 594 (special) conditions 595 input options 595 heat transfer analysis 226, 512, 595, 727, 729 convection 287 convection elements 288 elements 668 temperature effects 230 hereditary integral model 466 Hill failure criterion 359 yield function 433 history definition options 50 Hoffman failure criterion 360 HOOKLW (user subroutine) 101, 347, 350 HOOKVI (user subroutine) 470 Houbolt operator 172 hydrodoynamic bearinh 728 hydrodynamic bearing analysis 513, 596, 670, 728, 730 elements 292 mass fluxes 596 pump pressures 596 restrictors 596 HYPELA2 (user subroutine) 112, 383, 384, 488 HYPOELASTIC (model definition option) 383

I IBOOC (parameter) 31, 32, 34 IMPD (user subroutine) 723

incompressible Herrmann elastic formulation 126 material behavior 125 material modeled 126 incompressible elements 672 rigid-plastic flow 673

Main Index

incremental mesh generators 69, 70 induction heating 342 inertia relief 185 loads evaluation 186 Support method 185 initial conditions 178 previous analysis result data 209 INITIAL DISP (model definition option) 178 INITIAL PC (model definition option) 197 initial plastic strain 594 INITIAL PORE (model definition option) 197 INITIAL POROSITY (model definition option) 193, 194, 289 initial stress and initial plastic strain input options 594 INITIAL TEMP (model definition option) 226, 231, 336, 339, 342 INITIAL VEL (model definition option) 178 INITIAL VOID RATIO (model definition option) 193, 194 input conventions 42 input options acoustic analysis sources 597 boundary conditions 600 electrical 597 electromagnetic 305, 598 electrostatic 597 fluid drag and wave loads 587 heat fluxes 595 initial stress and initial plastic strain 594 magnetostatic currents 598 mass fluxes and restrictors 596 mechanical loads 585 thermal loads 593 INSERT (model definition option) 621 INTCRD (user subroutine) 723 interface ADAMS 736 hyperMesh results 735 SDRC I-DEAS results 735 interference fit 617 interpolation (shape) functions, type of 665 inverse power sweep 166 ISOTROPIC (acoustic, model definition option) 314, 513

779 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ ISOTROPIC (electromagnetic, model definition

option) 305, 513 ISOTROPIC (electrostatic, model definition option) 296, 513 ISOTROPIC (fluid, model definition option) 332, 513, 514 ISOTROPIC (heat transfer, model definition option) 335, 342, 512, 594 ISOTROPIC (hydrodynamic, model definition option) 513 ISOTROPIC (magnetostatic, model definition option) 300, 302, 513 ISOTROPIC (model definition option) 43, 207, 226, 230, 248, 282, 283, 289, 292, 310, 323, 347, 349, 374, 381, 433, 434, 438, 440, 441, 442, 444, 445, 446, 458, 461, 463, 464, 468, 470, 480, 485, 585 ISOTROPIC (with TABLE input - Stress) 441 isotropic hardening 443

J J-INTEGRAL (model definition option) 101

Joule analysis 729 heating 335 structural 337 JOULE (model definition option) 336, 339 JOULE (parameter) 335, 338

K Kachanov factor 503 Kelvin-Voigt model 465 kinematic constraints 599 hardening 444

L Lagrange multipliers 557 Lagrangian formulation 110 Lanczos method 167 large deformations 125 LARGE DISP (parameter) 111, 112, 116, 121, 122, 127, 383, 441, 615

Main Index

large strain analysis 672, 673 elasticity 124 plasticity 127 LARGE STRAIN (parameter) 111, 112, 115, 138, 172, 283, 327, 383, 441, 490, 603, 615 linear analysis 100 linear elastic material 346 linear fracture mechanics 148 linear springs and elastic foundations input options 622 linked/unlinked 208 list of items, input 43 load AUTO STEP scheme 683 automatic incrementation 682 cavity pressure 588 fixed 681 fluid drag and wave 587 history definition options 679 increment size 681 mass fuxes 596 mechanical 584 mechanical and thermal increments 679 piezoelectric 598 pump pressures 596 recycling criterion 683 residual 729 residual load correction 690 restrictors 596 surface/volumetric 572 thermal 593 types 571 user-defined physical criteria 685 vectors 763 LOAD COR (parameter) 585 load incrementation adaptive scheme 680 fixed scheme 679 LORENZI (model definition option) 151, 153, 164

M machining (or metal cutting) 766 MAGNETO (parameter) 300

780 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ magnetostatic analysis 513, 598, 670, 728, 730 current input options 598 elements types 300 MANY TYPES (model definition option) 64 Marc host systems 30 overview 24 mass fluxes and restrictors 596 MASSES (model definition option) 182 material instabilities 128 low tension 485 mechanical shape memory 413 powder 439 preferred direction 353 material dependent failure criteria 357 Hashin 363 Hashin Fabric 364 Hashin Tape 365 Hill 359 Hoffman 360 maximum strain 358 maximum stress 357 Puck 366 strain failure 358 Tsai-Wu 362 user-defined 363 material model composite 348 elastomers 419 gasket 378 linear elastic 346 Mohr-Coulomb (hydrostatic yield dependence) 437 nonlinear hypoelastic 383 time-independent inelastic 429 Mean Strain Energy Criterion 82 mean-normal method 137 mechanical erosion 244 erosion by other actions 245 loads 584 loads input options 585

Main Index

mechanical shape memory model conversation thermo-mechanical to mechanical SMA 418 experimental data fitting 417 membrane elements 666 MERGE (model definition option) 60 mesh definition 54 refinement tying constraints 606 severe distortion 128 mesh generation, remeshing techniques 92 advancing front meshing 92 Delaunay Triangulation 93 overlay meshing 92 mesh splitting 165 MESH2D 59 MESH2D (model definition option) 64 mixture model 374 MNF (parameter) 738 MNF UNITS (model definition option) 738 modal stresses and reactions 168 superposition 168 MODAL INCREMENT (model definition option) 105 MODAL SHAPE (history definition option) 167, 168, 314, 332 mode separation 153 model connections CWELD patch-to-patch 639 model definition options 50 Mohr-Coulomb linear material 437 parabolic material 438 MOONEY (model definition option) 374, 423, 426, 480 MOONEY (parameter) 115 Mooney-Rivlin 422, 427 MOTION (2-D, user subroutine) 524 MOTION CHANGE (history definition option) 526, 545 MPC-CHECK (parameter) 621 MPI (Message Passing Interface) 740 Mullin’s effect 501 multiplicative decomposition 132, 429 multistage return mapping 138

781 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ analysis 105 N fracture mechanics 150 Narayanaswamy model 146, 476 NASSOC (user subroutine) 147, 463 Nastran RBE2 and RBE3 628 Navier-Stokes 314, 317, 323, 325 NC machining data 766 cutter path 767 cutter shape 766 element deactivation 768 intersection 768 nearly incompressible behavior 127 neighbor relations 529 Neo-Hookean 422 Newmark-beta operator 171, 173 Newton Cooling 484 Newton-Raphson method full 692 modified 693 NiTi alloys 404 NLELAST 383 (bimodulus) elasticity model 396 (bimodulus) elasticity model with either no tension, limited tension, no compression, or limited compression enhancements 396 basic assumptions and definitions 384 converting engineering strain/stress to true strain/stress 385 input of uniaxial stress-strain data 384 Nastran like nonlinear elasticity model 386 nonlinear orthotropic elasticity model 398 principal strain space model 394 small strain nonlinear elasticity model 398 strain invariant model 390 NLELAST (model definition option) 112, 349, 383, 386, 387 nodal degrees of freedom tying constraints 613 NODE CIRCLE (model definition option) 70 NODE FILL (model definition option) 70 NODE GENER (model definition option) 70 NODE MERGE (model definition option) 70 NODE SORT (model definition option) 722 Node Within A Box Criterion 84 Nodes In Contact Criterion 84 nodes, merging of 60 nonlinear

Main Index

nonlinear hypoelastic material 383 HYPELA2 user subroutine 383 NLELAST model definition 383 nonlinearities, three types 109 non-Newtonian 316 nonstructural materials 512 NURBS 519, 520, 531, 561, 562 trimmed 519, 556

O Oak Ridge National Laboratory (ORNL) 141, 440, 461 objective function 200, 201, 206, 207, 208, 209 objective stress rates 130 OGDEN (model definition option) 423, 475, 480, 504 OGDEN (parameter) 115 operator central difference 172 generalized alpha operator 172 Houbolt 172 Newmark-beta 171 single step Houbolt 172 OPTHOTROPIC (model definition option) 445 optimization algorithm 206 OPTIMIZE (model definition option) 70 Option ACTIVATE (history definition) 59 ADAPT GLOBAL (model definition) 256 ADAPTIVE (model definition) 82, 101, 102, 675 ANISOTROPIC (model definition) 101, 289, 310, 347, 349, 353, 374, 434, 446, 480 APPROACH (history definition) 526 ASSEM LOAD (model definition) 737 ATTACH EDGE (model definition) 81, 584 ATTACH FACE (model definition) 584 AUTO CREEP (history definition) 141, 143, 146, 147, 466, 679, 680 AUTO INCREMENT (history definition) 72, 122, 487, 587, 679, 680, 682, 698 AUTO LOAD (history definition) 72, 335, 475, 587, 679

782 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ AUTO STEP (history definition) 146, 171, 228,

232, 335, 342, 470, 475, 487, 560, 567, 593, 679, 680, 681, 683, 684, 685, 686, 688, 689, 690 AUTO THERM (history definition) 593, 679, 680, 681 AUTO THERM CREEP (history definition) 145, 679, 680 AXITO3D (model definition) 210 BEGIN SEQUENCE (history definition) 593 B-H RELATION (electromagnetic, model definition) 309, 513 B-H RELATION (magnetostatic, model definition) 301, 302, 513 BUCKLE (history definition) 122, 123 BUCKLE INCREMENT (model definition) 105, 122, 123 CASE COMBIN (model definition) 101, 103, 691 CAVITY DEFINITION (model definition) 272, 282, 284, 596 CFAST (model definition) 622, 639, 656, 657, 658, 659, 660, 661 CHANGE PORE (model definition) 197 CHANGE STATE (history definition) 145, 681 CHANGE STATE (model definition) 34, 227, 287, 593 CHANNEL (model definition) 227, 325 COEFFICIENT (model definition) 625 COHESIVE (model definition) 672 COMPOSITE (model definition) 207, 348, 349 CONN FILL (model definition) 70 CONN GENER (model definition) 70 CONNECT (model definition) 64 CONNECTIVITY (model definition) 59, 69, 326, 338, 342, 622, 639, 646, 652, 653, 656 CONRAD GAP (model definition) 227 CONSTRAINT (model definition) 63 CONTACT (model definition) 119, 120, 128, 172, 227, 271, 335, 518, 520, 551, 553, 558, 571, 620, 626, 684 CONTACT CHANGE (rezoning) 554 CONTACT NODE (model definition) 519 CONTACT TABLE (history definition) 526, 545 CONTACT TABLE (model definition) 532, 542, 543, 544, 547, 548, 553, 566 Main Index

CONTINUE (history definition) 44, 50, 51 CONTROL (electromagnetic, model definition)

305 CONTROL (heat transfer, model definition) 326 CONTROL (history definition) 145, 229, 629,

634, 679 CONTROL (magnetostatic, model definition)

301 CONTROL (model definition) 112, 123, 228,

280, 557, 629, 634, 679, 684, 721 CONVERT (model definition) 327, 339, 342 COORD SYSTEM (model definition) 356, 525,

623 COORDINATES (model definition) 59, 69, 652,

726 CRACK DATA (model definition) 485 CREEP (model definition) 146, 457, 458, 463,

466, 481 CREEP INCREMENT (history definition) 679 CURE SHRINKAGE (model definition) 217 CURVES (model definition) 81 CWELD (model definition) 639, 644, 645, 646,

647, 648, 649, 650, 651, 652, 653, 655, 656, 657, 658, 659, 660, 661 CYCLIC SYMMETRY (model definition) 626, 627 CYLINDRICAL (model definition) 59, 635 DAMAGE (model definition) 376, 504 DAMPING (model definition) 169, 180, 182 DAMPING COMPONENTS (history definition) 293 DEACT GLUE (model definition) 157, 161 DEFINE (model definition) 43, 44, 45 DELAMINATION (model definition) 165 DENSITY EFFECTS (model definition) 440 DESIGN DISPLACEMENT CONSTRAINTS

(model definition) 208 DESIGN FREQUENCY CONSTRAINTS (model

definition) 208 DESIGN OBJECTIVE (model definition) 207 DESIGN STRAIN CONSTRAINTS (model

definition) 208 DESIGN STRESS CONSTRAINTS (model

definition) 208 DESIGN VARIABLES (model definition) 207

783 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ DISP CHANGE (history definition) 145, 327,

339, 618, 620 DIST CHARGE (electromangetic, model

definition) 305

Main Index

FIXED DISP (model definition) 59, 63, 194,

310, 327, 332, 335, 339, 618 FIXED POTENTIAL (electromagnetic, model

definition) 305

DIST CHARGE (model definition) 310, 335 DIST CHARGES (electrostatic, model

FIXED POTENTIAL (electrostatic, model

definition) 296, 335, 342 DIST CURRENT (electromagnetic, model definition) 305 DIST CURRENT (history definition) 339 DIST CURRENT (Joule, history definition) 335, 336, 342 DIST CURRENT (magnetostatic, model definition) 301 DIST CURRENT (model definition) 339 DIST FLUXES (history definition) 336, 339, 342 DIST FLUXES (model definition) 193, 226, 232, 293, 336, 339 DIST LOADS (history definition) 145, 339 DIST LOADS (model definition) 194, 310, 335, 339, 585, 587 DIST MASS (model definition) 289 DIST SOURCE (model definition) 314 DYNAMIC CHANGE (history definition) 169, 171, 177, 314, 332, 679 DYNAMIC CHANGE (history definition, electromagnetic) 305, 308 ELEM SORT (model definition) 722 EMCAPAC (history definition) 298 EMISSIVITY (model definition) 282 EMRESIS (history definition) 340 END OPTION (model definition) 42, 50, 51, 207, 314 END REZONE (rezoning) 51 END SEQUENCE (history definition) 593 ERROR ESTIMATE (model definition) 79, 102, 128 EXCLUDE (history definition) 528 FAIL DATA (model definition) 357, 372, 373, 374, 486 FILMS (model definition) 226, 232, 244, 271, 336, 339, 342, 595 FILMS (with TABLE input, model definition) 596

FIXED POTENTIAL (magnetostatic, model

definition) 296, 342 definition) 301 FIXED PRESSURE (model definition) 193,

289, 292, 314 FIXED TEMPERATURE (model definition) 226,

231, 282, 323, 327, 336, 339, 342 FIXED VELOCITY (model definition) 323 FIXED VOLTAGE (model definition) 335, 339 FLUID DRAG (model definition) 587 FLUID SOLID (model definition) 331 FOAM (model definition) 475 FOUNDATION (model definition) 101, 121 FOURIER (model definition) 101, 102, 105 FXORD (model definition) 65, 69, 668 GASKET (model definition) 381 GEOMETRY (model definition) 74, 207, 292,

633, 636, 649, 650, 651, 652, 668, 673, 675, 726 GLOBALLOCAL (model definition) 34, 214 HARMONIC (electromagnetic, history definition) 309, 342 HYPOELASTIC (model definition) 383 INITIAL DISP (model definition) 178 INITIAL PC (model definition) 197 INITIAL PORE (model definition) 197 INITIAL POROSITY (model definition) 193, 194, 289 INITIAL TEMP (model definition) 226, 231, 336, 339, 342 INITIAL VEL (model definition) 178 INITIAL VOID RATIO (model definition) 193, 194 INSERT (model definition) 621 ISOTROPIC (acoustic, model definition) 314, 513 ISOTROPIC (electromagnetic, model definition) 305, 513 ISOTROPIC (electrostatic, model definition) 296, 513

784 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ ISOTROPIC (fluid, model definition) 332, 513,

514 ISOTROPIC (heat transfer, model definition)

335, 342, 512, 594 ISOTROPIC (hydrodynamic, model definition)

513 ISOTROPIC (magnetostatic, model definition)

300, 302, 513 ISOTROPIC (model definition) 43, 207, 226,

230, 248, 282, 283, 289, 292, 310, 323, 347, 349, 374, 381, 433, 434, 438, 440, 441, 442, 444, 445, 446, 458, 461, 463, 464, 468, 470, 480, 485, 585 ISOTROPIC (with TABLE input - Stress) 441 J-INTEGRAL (model definition) 101 JOULE (model definition) 336, 339 LORENZI (model definition) 151, 153, 164 MANY TYPES (model definition) 64 MASSES (model definition) 182 MERGE (model definition) 60 MESH2D (model definition) 64 MNF UNITS (model definition) 738 MODAL INCREMENT (model definition) 105 MODAL SHAPE (history definition) 167, 168, 314, 332 MOONEY (model definition) 374, 423, 426, 480 MOTION CHANGE (history definition) 526, 545 NLELAST (model definition) 112, 349, 383, 386, 387 NODE CIRCLE (model definition) 70 NODE FILL (model definition) 70 NODE GENER (model definition) 70 NODE MERGE (model definition) 70 NODE SORT (model definition) 722 OGDEN (model definition) 423, 475, 480, 504 OPTIMIZE (model definition) 70 ORIENTATION (model definition) 347, 349, 353, 434, 470, 664 ORTHO TEMP (model definition) 226, 335, 349, 441, 480 ORTHOTROPIC (electrical, model definition) 513 ORTHOTROPIC (electromagnetic, model definition) 305, 513 ORTHOTROPIC (electrostatic, model definition) 296, 335 Main Index

ORTHOTROPIC (magnetostatic, model

definition) 301, 302, 513 ORTHOTROPIC (model definition) 101, 207,

226, 248, 282, 283, 289, 310, 347, 349, 374, 433, 434, 440, 441, 442, 444, 445, 446, 463, 464, 468, 470, 480, 482, 585 ORTHOTROPIC (thermal, model definition) 335, 342, 512, 513, 594 ORTHOTROPIC (with TABLE input - Stress) 441 PARAMETERS (history definition) 173 PARAMETERS (model definition) 189, 190, 283, 323, 532, 547 PBUSH (model definition) 622, 624, 625 PERMANENT (magnetostatic, model definition) 301, 302 PFAST (model definition) 622, 624, 639, 656 PIEZOELECTRIC (model definition) 310 PIN CODE (model definition) 636 POINT CHARGE (electrostatic, model definition) 305, 335 POINT CHARGE (model definition) 296, 310 POINT CHARGE (with TABLE Input, model definition option) 342 POINT CURRENT (electromagnetic, history definition) 305 POINT CURRENT (history definition) 339 POINT CURRENT (Joule, history definition) 336 POINT CURRENT (Joule, model definition) 335 POINT CURRENT (magnetostatic, model definition) 301 POINT CURRENT (model definition) 339 POINT CURRENT (with TABLE Input Magnetostatic, history definition) 342 POINT FLUX (history definition) 336, 339 POINT FLUX (model definition) 193, 226, 231, 293, 336, 339, 342 POINT LOAD (electrostatic, model definition) 335 POINT LOAD (history definition) 145, 339 POINT LOAD (model definition) 43, 194, 310, 339, 524 POINT MASS (model definition) 289 POINT SOURCE (model definition) 314 POINTS (model definition) 81

785 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ POROSITY CHANGE (model definition) 378 POST (model definition) 145, 227, 287, 371,

681, 731 POTENTIAL CHANGE (history definition) 342 POWDER (model definition) 440 PRE STATE (model definition) 34, 210 PRINT CHOICE (model definition) 184, 369,

721, 722, 723, 726, 729 PRINT ELEMENT (model definition) 369, 721,

723, 726 PRINT NODE (model definition) 721, 722, 723,

729 PRINT VMASS (model definition) 722 PROPORTIONAL INCREMENT (history

definition) 72, 145, 147, 587 PSHELL (model definition) 353, 378 PWELD (model definition) 639, 641, 643, 649,

650, 651, 652 RAD-CAVITY (model definition) 244, 282, 283,

596 RADIATING CAVITY (model definition) 273 RBE2 (model definition) 157, 161, 629, 630,

637, 645, 646 RBE3 (model definition) 630, 631, 637, 638,

641, 645, 646, 656, 661 REAUTO (model definition) 141, 691 REBAR (model definition) 485 RECEDING SURFACE (model definition) 255 RECOVER (history definition) 168 RELATIVE DENSITY (model definition) 440 RELEASE (history definition) 545 RESTART (model definition) 33, 101, 141, 691,

722, 723 RESTART INCREMENT (history definition) 691 RESTART LAST (model definition) 691 RESTRICTOR (model definition) 292 REZONE (rezoning) 51 ROTATION A (model definition) 585 RROD (model definition) 157, 161 SERVO LINK (model definition) 571, 605 SHELL TRANSFORMATION (model definition)

601, 603 SHIFT FUNCTION (model definition) 146, 473 SOIL (model definition) 193, 194, 197, 488 SOLVER (model definition) 675, 706, 707, 708

Main Index

SPECIFIED NODES (model definition) 64 SPLINE (model definition) 257, 519, 565 SPRINGS (model definition) 101, 121, 182 START NUMBER (model definition) 64 STEADY STATE (electrostatic, history

definition) 296 STEADY STATE (history definition) 228, 320,

336, 342 STEADY STATE (magnetostatic, history

definition) 301 STIFFNS COMPONENTS (history definition)

293 STIFFSCALE (model definition) 74 STRAIN RATE (model definition) 190, 323,

349, 441 STRAIN RATE (model definition, fluid) 514 SUMMARY (model definition) 722 SUPERELEM (history definition) 738 SURFACE ENERGY (model definition) 236,

255 SURFACES (model definition) 81 SWLDPRM (model definition) 639, 652, 655,

657 SYNCHRONIZED (history definition) 526 TABLE (model definition) 282, 283, 380, 441,

444, 445, 468, 480, 482 TEMP CHANGE (history definition) 226, 231,

323, 327, 336, 339, 342 TEMPERATURE EFFECTS (coupled thermal-

stress, model definition) 512 TEMPERATURE EFFECTS (heat transfer,

model definition) 335, 512 TEMPERATURE EFFECTS (hydrodynamic,

model definition) 513 TEMPERATURE EFFECTS (model definition)

226, 230, 283, 292, 349, 423, 440, 441, 468, 473, 480, 482, 514 THERMAL CONTACT (model definition) 227, 271, 298, 340 THICKNESS (model definition) 292 THICKNS CHANGE (history definition) 293 TIME STEP (history definition) 441, 470, 475 TIME-TEMP (model definition) 483, 484 TRANSFORMATION (model definition) 525, 600, 608, 620, 635, 729

786 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ TRANSIENT (history definition) 227, 228, 229,

232, 336, 342, 679, 680 TYING (model definition) 227, 331, 571, 605 TYING CHANGE (history definition) 605 UFCONN (model definition) 59 UFXORD (model definition) 59 UTRANFORM (model definition) 600 VCCT (model definition) 147, 153, 159 VELOCITY (model definition) 227, 288, 292 VELOCITY CHANGE (history definition) 227, 288, 323 VIEW FACTOR (model definition) 276, 596 VISCEL EXP (model definition) 146, 479 VISCELFOAM (model definition) 146, 475 VISCELMOON (model definition) 146, 423, 475 VISCELOGDEN (model definition) 146, 423, 475, 504 VISCELORTH (model definition) 470 VISCELPROP (model definition) 470 VOID CHANGE (model definition) 378 VOLTAGE CHANGE (history definition) 336, 339 WELD FILL (model definition) 265, 268, 269 WELD FLUX (model definition) 265, 269, 271 WELD PATH (model definition) 265, 267 WORK HARD (model definition) 190, 349, 441, 444, 445 ORIENT (user subroutine) 101, 348, 353, 354, 356, 434, 470 ORIENTATION (model definition option) 347, 349, 353, 434, 470, 664 ORTHO TEMP (model definition option) 226, 335, 349, 441, 480 ORTHOTROPIC (electrical, model definition option) 513 ORTHOTROPIC (electromagnetic, model definition option) 305, 513 ORTHOTROPIC (electrostatic, model definition option) 296, 335 ORTHOTROPIC (magnetostatic, model definition option) 301, 302, 513 ORTHOTROPIC (model definition option) 101, 207, 226, 248, 282, 283, 289, 347, 349, 374, 433, 434, 440, 441, 442, 444, 446, 463, 464, 468, 470, 480, 482, 585 ORTHOTROPIC (model definition) 310 Main Index

ORTHOTROPIC (thermal, model definition option)

335, 342, 512, 513, 594 ORTHOTROPIC (with TABLE input - Stress) 441

out-of-core storage options 32 output results workspace information 716, 752 overclosure 617 tying 617

P parallel processing contact analysis 742 domain decomposition 743 solvers 742 types of machines 740 unsupported features 740 Parameter ABLATION 255, 256 ACOUSTIC 314 ADAPTIVE 675 ALL POINTS 287, 664 ALLOCATE 32 ASSUMED STRAIN 675 AUTOMSET 621 AUTOSPC 545 BEAM SECT 74, 651, 652, 667 BEARING 292 BUCKLE 105, 122 CENTROID 112, 115, 121, 287, 593, 664, 691, 702, 723, 729 COUPLE 326, 338 CREEP 144, 146, 147, 456, 462, 463, 465 DESIGN OPTIMIZATION 207, 347 DESIGN SENSITIVITY 207, 347 DIFFUSION 289 DIST LOADS 207 DYNAMIC 105, 164, 166, 169, 171 ELASTIC 79, 100, 101 ELASTICITY 101 ELECTRO 296, 334 ELEMENTS 165, 639, 653, 656, 664 EL-MA 305, 342 ELSTO 31, 32, 33, 34, 716 END 50 EXTENDED 43

787 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ FEATURE 629, 634 FLUID 670 FOLLOW FOR 112, 121, 585, 586, 603, 675 FOURIER 102, 105 GENT 115 HARMONIC 182, 183 HEAT 287, 288, 342, 669 IBOOC 31, 32, 34 JOULE 335, 338 LARGE DISP 111, 112, 116, 121, 122, 127, 383,

441, 615 LARGE STRAIN 111, 112, 115, 138, 172, 283,

327, 383, 441, 490, 603, 615 LOAD COR 585 MAGNETO 300 MNF 738 MOONEY 115 MPC-CHECK 621 OGDEN 115 PIEZO 310 PORE 289 PRINT 123, 236, 282, 538, 730 RADIATION 272, 276, 512, 596 RBE 646 RESTRICTOR 292 REZONING 71 R-P FLOW 189, 695 SCALE 679 SHELL SECT 668 SIZING 664, 719 STATE VARS 292 STOP 32 STRUCTURAL 335 TSHEAR 369, 726 T-T-T 483 UFLUXMEC 236 UPDATE 172 VISCO ELAS 146

parameters 50 PARAMETERS (history definition option) 173 PARAMETERS (model definition option) 189, 190,

283, 323, 532, 547 PBUSH (model definition option) 622, 624, 625

penalty 189, 319 methods 557

Main Index

PERMANENT (magnetostatic, model definition

option) 301, 302 perturbation analysis 123 PFAST (model definition option) 622, 624, 639, 656 piecewise linear representation 480 PIEZO (parameter) 310 piezoelectric analysis 309, 512, 598, 670, 728, 730 coupling 312 element types 309 loads 598 PIEZOELECTRIC (model definition option) 310 pin code 636 PIN CODE (model definition option) 636 pipe bend element tying constraints 612 plate elements 668 PLOTV (user subroutine) 731 POINT CHARGE (electrostatic, model definition option) 305, 335 POINT CHARGE (model definition option) 296, 310 POINT CHARGE (with TABLE Input - Electrostatic, model definition option) 342 POINT CURRENT (electromagnetic, history definition option) 305 POINT CURRENT (history definition option) 339 POINT CURRENT (Joule, history definition option) 336 POINT CURRENT (Joule, model definition option) 335 POINT CURRENT (magnetostatic, model definition option) 301 POINT CURRENT (model definition option) 339 POINT CURRENT (with TABLE Input Magnetostatic, history definition option) 342 POINT FLUX (history definition option) 336, 339 POINT FLUX (model definition option) 193, 226, 231, 293, 336, 339, 342 POINT LOAD (electrostatic, model definition option) 335 POINT LOAD (history definition option) 145, 339 POINT LOAD (model definition option) 43, 194, 310, 339, 524 POINT MASS (model definition option) 289 POINT SOURCE (model definition option) 314 POINTS (model definition option) 81

788 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ Poisson’s 100, 346, 347, 348, 349, 440, 480, 483, R 485, 488, 490

PORE (parameter) 289 POROSITY CHANGE (model definition option) 378 POST (model definition option) 145, 227, 287, 371,

681, 731 post buckling analysis 680 post file 731 POTENTIAL CHANGE (history definition) 342 POWDER (model definition option) 440 powder material 439 Power Law Fluid 316 PRE STATE (model definition option) 34, 210 preconditioners, iterative solvers 708 presentation of the energy equation 253 Previously Refined Mesh Criterion 85 Principal Engineering Strains 731 PRINT (parameter) 123, 236, 282, 538, 730 PRINT CHOICE (model definition option) 184, 369, 721, 722, 723, 726, 729 PRINT ELEMENT (model definition option) 369, 721, 723, 726 PRINT NODE (model definition option) 721, 722, 723, 729 PRINT VMASS (model definition option) 722 program initiation 36 messages 734 progressive composite failure 372 PROPORTIONAL INCREMENT (history definition option) 72, 145, 147, 587 PSHELL (model definition option) 353, 378 PSPG 317 Puck failure criterion 366 PWELD (model definition option) 639, 641, 643, 649, 650, 651, 652 PWL (piece-wise linear) 519 pyrolysis 245 alternative formulation 249 presentation of the mass equation 246 principle of 247

Q quadratic contact 551 quarter point elements 164

Main Index

RAD-CAVITY (model definition option) 244, 282,

283, 596 radial return 135 RADIATING CAVITY (model definition option) 273 radiation 271 computational approaches 272 direct adaptive integration 279 Monte Carlo method 276 pixel based modified Hemi-Cube method 273 viewfactors 273 RADIATION (parameter) 272, 276, 512, 596 radiation viewfactors 273 RBE (parameter) 646 RBE2 (model definition option) 157, 161, 629, 630, 637, 645, 646 RBE2 and RBE3 628 RBE3 (model definition option) 630, 631, 637, 638, 641, 645, 646, 656, 661 reaction forces 729 REAUTO (model definition option) 141, 691 REBAR (model definition option) 485 REBAR (user subroutine) 485 rebar elements 672 RECEDING SURFACE (model definition option) 255 RECOVER (history definition option) 168 reduced integration elements 673 RELATIVE DENSITY (model definition option) 440 RELEASE (history definition option) 545 remeshing automatic global 85 criteria 90 remeshing techniques 91 adaptive 768 mesh generation 92 outline extraction and repair 94 target number of elements 96 residual load correction 690 resistor 340 RESTART (model definition option) 33, 101, 141, 691, 722, 723 restart analysis 691 RESTART INCREMENT (history definition option) 691

789 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ RESTART LAST (model definition option) 691 RESTRICTOR (model definition option) 292 RESTRICTOR (parameter) 292

result evaluation, contact 555 REZONE (rezoning option) 51 rezoning 71, 554 REZONING (parameter) 71 rigid contact, solution strategy 562 rigid link constraint 614, 620 rigid-plastic analysis 188, 673, 729 Riks-Ramm 699, 700 ROTATION A (model definition option) 585 R-P FLOW (parameter) 189, 695 RROD (model definition option) 157, 161 rubber foam model 426 RVCNST 535

S SCALE (parameter) 679

scaling, linear-elastic solution 679 selective printout 721 grid force balance 722 options 721 semi-infinite elements 674 sensitivity 200 separation, contact 544 SEPFOR (user subroutine) 563 SEPSTR (user subroutine) 563 Sequential Quadratic Programming 206 SERVO LINK (model definition option) 571, 605 shape memory mechanical 413 thermo-mechanical material 404 shell contact 528 elements 553, 668 stiffener tying constraints 612 transformation 601 SHELL SECT (parameter) 668 shell stiffener tying constraints 612 SHELL TRANSFORMATION (model definition option) 601, 603 shell-to-shell intersection tying constraints 607 shell-to-solid intersections tying constraints 608

Main Index

SHIFT FUNCTION (model definition option) 146,

473 single input DDM 37, 741, 743, 744, 745 single step Houbolt operator 172 singularity ratio 705 SIZING (parameter) 664, 719 snap-through analysis 680 SOIL (model definition option) 193, 194, 197, 488 soil analysis 193, 487, 670 solver conjugate gradient iterative 742 direct 742 hardware 742 matrix 742 multifrontal 742 SOLVER (model definition option) 675, 706, 707, 708 special elements 671 cable 671 curved-pipe 671 Gap-and-Friction 671 interface 672 pipe-bend 671 rebar 672 shear panel 671 SPECIFIED NODES (model definition option) 64 spectrum response 184 SPLINE (model definition option) 257, 519, 565 SPRINGS (model definition option) 101, 121, 182 springs, linear and nonlinear 727 START NUMBER (model definition option) 64 STATE VARS (parameter) 292 status file 738 STEADY STATE (electrostatic, history definition option) 296 STEADY STATE (history definition option) 228, 320, 336, 342 STEADY STATE (magnetostatic, history definition option) 301 steady state rolling analysis 211 Stefan-Boltzmann 596 stick-slip model, friction 538 STIFFNS COMPONENTS (history definition option) 293

790 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ STIFFSCALE (model definition option) 74 STOP (parameter) 32

storage methods 709 strain correction method 694 STRAIN RATE (model definition option) 190, 323, 349, 441 STRAIN RATE (model definition, fluid option) 514 strain rate effects on elastic-plastic constitutive relation 449 stress analysis 728 intensity factor defined 148 intensity factors 149 STRUCTURAL (parameter) 335 structural zooming analysis 214 substructuring 71 SUMMARY (model definition option) 722 SUPERELEM (history definition option) 738 SUPG 318 surface energy 236 SURFACE ENERGY (model definition option) 236, 255 SURFACES (model definition option) 81 SWLDPRM (model definition option) 639, 652, 655, 657 symmetries 63 SYNCHRONIZED (history definition option) 526 system and element stiffness matrices 762

T TABLE (model definition option) 282, 283, 380, 441, 444, 445, 468, 480, 482 TEMP CHANGE (history definition option) 226, 231, 323, 327, 336, 339, 342 TEMPERATURE EFFECTS (coupled thermal-stress, model definition option) 512 TEMPERATURE EFFECTS (heat transfer, model definition option) 335, 512 TEMPERATURE EFFECTS (hydrodynamic, model definition option) 513 TEMPERATURE EFFECTS (model definition option) 226, 230, 283, 292, 349, 423, 440, 441, 468, 473, 480, 482, 514 Temperature Gradient Criterion 84

Main Index

temperature-dependent creep 481 material properties 480 tension softening 486 thermal loads 593 loads input options 593 THERMAL CONTACT (model definition option) 227, 271 thermal contact analysis 548 THERMAL CONTACT(model definition option) 298, 340 thermal expansion coefficient 482 thermochemical ablation and surface wnergy balance 237 thermo-electrical 512 thermo-mechanical shape memory model 404 constitutive theory 407 phase transformation strains 407 transformation induced deformation 406 Thermo-Rheologically Simple material 471 THICKNESS (model definition option) 292 THICKNS CHANGE (history definition option) 293 TIME STEP (history definition option) 441, 470, 475 time step definition 177 time-dependent boundary conditions 178 inelastic behavior 453 time-independent, inelastic behavior 429 TIME-TEMP (model definition option) 483, 484 Time-Temperature-Transformation (T-T-T) 482 tolerance values, contact 556 total Lagrangian procedure 112 TRANSFORMATION (history definition option) 620 TRANSFORMATION (model definition option) 525, 600, 608, 620, 635, 729 TRANSIENT (history definition option) 227, 228, 229, 232, 336, 342, 679, 680 TRSFAC (user subroutine) 473 truss elements 666 Tsai-Wu failure criterion 362 TSHEAR (parameter) 369, 726 T-T-T (parameter) 483 tying overclosure 617 shell-to-solid 614

791 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ TYING (model definition option) 227, 331, 571, 605 TYING CHANGE (history definition option) 605

tying constraints beam-to-beam intersection 608 cyclic symmetry 625 mesh refinement 606 nodal degrees of freedom 613 pipe bend element 612 rigid link 614 shell stiffener 612 shell-to-shell intersection 607 shell-to-solid intersections 608

U UADAP (user subroutine) 85 UADAPBOX (user subroutine) 271 UBEAR (user subroutine) 293 UCOHESIVE (user subroutine) 508 UCOMPL (user subroutine) 182 UCOORD (user subroutine) 81 UCRACK (user subroutine) 485 UCRACKGROW (user subroutine) 158, 160 UCRPLW (user subroutine) 141, 144, 463, 482 UELASTOMER (user subroutine) 426 UELDAM (user subroutine) 504 UENERG (user subroutine) 426 UEPS (user subroutine) 296, 301, 305, 513 UFAH (user subroutine) 239 UFAIL (user subroutine) 357, 363 UFCONN (model definition option) 59 UFCONN (user subroutine) 59 UFINITE (user subroutine) 433 UFLUXMEC (parameter 236 UFLUXMEC (user subroutine) 245 UFMEC (user subroutine) 245 UFORMSN (user subroutine) 605, 613 UFOUR (user subroutine) 102 UFRIC (user subroutine) 542, 543 UFTHP (user subroutine) 243 UFXORD (model definition optiion) 59 UFXORD (user subroutine) 59, 65 UGLAW (user subroutine) 242 UGMEC (user subroutine) 245 UGROOV (user subroutine) 292 UHTCOE (user subroutine) 548, 549

Main Index

UHTCON (user subroutine) 547, 548, 549 UHTNRC (user subroutine) 548, 549 UMOONY (user subroutine) 423 UMU (user subroutine) 305, 513 UNEWTN (user subroutine) 190

uniaxial cracking data 485 UOGDEN (user subroutine) 423 UPDATE (parameter) 172

updated Lagrange Formulation, nonlinear elasticity 428 updated Lagrangian Procedure 115 UPNOD (user subroutine) 189 UPOSTV (user subroutine) 731 URESTR (user subroutine) 292 URPFLO (user subroutine) 190 User subroutine ANELAS 101, 347, 350 ANEXP 101, 350, 482 ANKOND 227, 512 ANPLAS 350, 434 CRPLAW 141, 142, 143, 147, 457, 458, 461, 463, 466, 482 CRPVIS 146, 456, 465, 466 ELEVAR 723, 726 ELEVEC 723 FILM 227, 232, 233, 234, 336, 339, 342, 595, 596 FLUX 227, 232, 234, 293, 296, 301, 310, 314, 335, 336, 339, 342, 595, 596 FORCDF 342 FORCDT 178, 231, 234, 293, 296, 301, 310, 323, 335 FORCEM 81, 178, 305, 310, 335, 342 HOOKLW 101, 347, 350 HOOKVI 470 HYPELA2 112, 383, 384, 488 IMPD 723 INTCRD 723 MOTION (2-D) 524 NASSOC 147, 463 ORIENT 101, 348, 353, 354, 356, 434, 470 PLOTV 731 REBAR 485 SEPFOR 563 SEPSTR 563

792 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ TRSFAC 473 UADAP 85 UADAPTBOX 271 UBEAR 293 UCOHESIVE 508 UCOMPL 182 UCOORD 81 UCRACK 485 UCRACKGROW 158, 160 UCRPLW 141, 144, 463, 482 UELASTOMER 426 UELDAM 504 UENERG 426 UEPS 296, 301, 305, 513 UFAH 239 UFAIL 357, 363 UFCONN 59 UFINITE 433 UFLUXMEC 245 UFMEC 245 UFORMSN 605, 613 UFOUR 102 UFRIC 542, 543 UFTHP 243 UFXORD 59, 65 UGLAW 242 UGMEC 245 UGROOV 292 UHTCOE 548, 549 UHTCON 547, 548, 549 UHTNRC 548, 549 UMOONY 423 UMU 305, 513 UNEWTN 190 UOGDEN 423 UPNOD 189 UPOSTV 731 URESTR 292 URPFLO 190 USIGMA 305, 513 USINC 178, 231 USPLIT_MESH 165 USPRNG 121, 622 USSD 184 UTHICK 292, 293 UTIMESTEP 686

Main Index

UTIMP 245 UTRANS 600 UVELOC 227, 288, 292 UVSCPL 142, 143, 147, 464 UWATERSL 252 UWELDFLUX 265, 266 VSWELL 142, 143, 462, 466 WKSLP 441, 444, 445 YIEL 147, 463 ZERO 147, 463

user subroutine input 59 user-defined Criterion 85 user-defined failure criteria 363 USIGMA (user subroutine) 305, 513 USINC (user subroutine) 178, 231 USPLIT_MESH (user subroutine) 165 USPRNG (user subroutine) 121, 622 USSD (user subroutine) 184 UTHICK (user subroutine) 292, 293 UTIMESTEP (user subroutine) 686 UTIMP (user subroutine) 245 UTRANFORM (model definition option) 600 UTRANS (user subroutine) 600 UVELOC (user subroutine) 227, 288, 292 UVSCPL (user subroutine) 142, 143, 147, 464 UWATERSL (user subroutine) 252 UWELDFLUX (user subroutine) 265, 266

V VCCT (model definition option) 147, 153, 159 VELOCITY (model definition option) 227, 288, 292 VELOCITY CHANGE (history definition option)

227, 288, 323 VIEW FACTOR (model definition option) 276, 596

virtual crack closure technique (VCCT) 147 VISCEL EXP (model definition option) 146, 479 VISCELFOAM (model definition option) 146, 475 VISCELMOON (model definition option) 146, 423,

475 VISCELOGDEN (model definition option) 146, 423,

475, 504 VISCELORTH (model definition option) 470 VISCELPROP (model definition option) 470 VISCO ELAS (parameter) 146

viscoelastic material

793 Index

ABCDEFGHIJKLMNOPQRSTUVWXYZ incompressible isotropic 470 Z isotropic 468 Thermo-Rheologically Simple 471 viscoelasticity 145 viscoplasticity explicit formulation 463, 464 explicit method 146 implicit method 147 VOID CHANGE (model definition option) 378 VOLTAGE CHANGE (history definition option) 336, 339 von Mises 135, 136, 143, 203, 432, 435, 440, 443, 444, 446, 447, 448, 449, 458, 722, 724, 725 VSWELL (user subroutine) 142, 143, 462, 466

W wear 197 weighted mesh 63 WELD FILL (model definition option) 265, 268, 269 WELD FLUX (model definition option) 265, 269, 271 WELD PATH (model definition option) 265, 267 welding 265 weld path 267 weld wlux 265 Williams-Landel-Ferry (WLF) 146, 472 WKSLP (user subroutine) 441, 444, 445 WORK HARD (model definition option) 190, 349, 441, 444, 445 workhardening isotropic 443 rules 443 slope 430 workspace allocation 31

Y YIEL (user subroutine) 147, 463 Young’s 349 Young’s modulus 346, 349, 428, 431, 443, 480, 483, 485, 486, 488

Main Index

ZERO (user subroutine) 147, 463 Zienkiewicz-Zhu Creep Strain Criterion 84 Zienkiewicz-Zhu Criterion 83 zooming 214

794 Marc Volume A: Theory and User Information

ABCDEFGHIJKLMNOPQRSTUVWXYZ

Main Index